Allen-Bradley 9/Series CNC Mill Operation and Programming Manual
Important User Information Because of the variety of uses for the products described in this publication, those responsible for the application and use of this control equipment must satisfy themselves that all necessary steps have been taken to assure that each application and use meets all performance and safety requirements, including any applicable laws, regulations, codes and standards.
9/Series Mill Operation and Programming Manual October 2000 Summary of Changes New Information The following is a list of the larger changes made to this manual since its last printing. Other less significant changes were also made throughout. Error Message Log Paramacro Parameters Softkey Tree Error Messages Revision Bars We use revision bars to call your attention to new or revised information. A revision bar appears as a thick black line on the outside edge of the page as indicated here.
Chapter 1-2
Table of Contents Index (General) 9/Series Mill 9/Series PAL Reference Manual Operation and Programming Manual Chapter 1 Using This Manual 1.0 Chapter Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 1.1 Audience . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 1.2 Manual Design . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
TableIndex of Contents (General) 9/SeriesManual Mill 9/Series PAL Reference Operation and Programming Manual 3.1.2 Setting Tool Offset Tables . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 3.1.3 Setting Offset Data Using {MEASURE} . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 3.1.4 Tool Offset Range Verification . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 3.
Table of Contents Index (General) 9/Series Mill 9/Series PAL Reference Manual Operation and Programming Manual 5.4 Digitizing a Program (Teach) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 5.4.1 Linear Digitizing . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 5.4.2 Digitizing an Arc (3 Points) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
TableIndex of Contents (General) 9/SeriesManual Mill 9/Series PAL Reference Operation and Programming Manual Chapter 8 Display and Graphics 8.0 Chapter Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 8.1 Selection of Axis Position Data Display . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 8.2 PAL Display Page . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Table of Contents Index (General) 9/Series Mill 9/Series PAL Reference Manual Operation and Programming Manual 10.4.1 Minimum and Maximum Axis Motion (Programming Resolution) . . . . . . . . . . . . . . . . . . . . . 10.5 Word Descriptions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 10.5.1 A_ L_ ,R_ ,C_ (Quick Plus and Radius-Chamfer Words) . . . . . . . . . . . . . . . . . . . . . . . . . . 10.5.2 Axis Names . . . . . . . . . . . . . .
TableIndex of Contents (General) 9/SeriesManual Mill 9/Series PAL Reference Operation and Programming Manual Chapter 13 Coordinate Control 13.0 Chapter Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 13.1 Rotating the Coordinate Systems . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 13.1.1 Rotating the Current Work Coordinate System (G68, G69) . . . . . . . . . . . . . . . . . . . . .
Table of Contents Index (General) 9/Series Mill 9/Series PAL Reference Manual Operation and Programming Manual Chapter 15 Using QuickPath Plust 15.0 15.1 15.2 15.3 Chapter Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Using QuickPath Plus . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Linear QuickPath Plus . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
TableIndex of Contents (General) 9/SeriesManual Mill 9/Series PAL Reference Operation and Programming Manual 18.4.7 Short Block Acc/Dec G36, G36.1 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 18-22 Chapter 19 Dual--- axis Operation 19.0 Chapter Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 19.1 Dual--axis Operation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Table of Contents Index (General) 9/Series Mill 9/Series PAL Reference Manual Operation and Programming Manual 21.6.6 Moving To/From Machine Home . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 21.6.7 Changing or Offsetting Work Coordinate System . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 21.6.8 Block Look-Ahead . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 21.
TableIndex of Contents (General) 9/SeriesManual Mill 9/Series PAL Reference Operation and Programming Manual 25.1.2 Irregular Pocket Finishing (G89.2) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 25-10 Chapter 26 Milling Fixed Cycles 26.0 Chapter Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 26.1 Milling Fixed Cycles . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Table of Contents Index (General) 9/Series Mill 9/Series PAL Reference Manual Operation and Programming Manual Chapter 28 Paramacros 28.0 Chapter Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 28.1 Paramacros . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 28.2 Parametric Expressions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
TableIndex of Contents (General) 9/SeriesManual Mill 9/Series PAL Reference Operation and Programming Manual 30.5 Using Interference Checking with a Dual-process Mill . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 30.5.1 Measuring Interference Boundaries . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 30.5.2 Entering Interference Values Manually . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 30.5.
Table of Contents Index (General) 9/Series Mill 9/Series PAL Reference Manual Operation and Programming Manual Appendix D Allen-Bradley 7300 Series CNC Tape Compatibility Appendix Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . G-code Compatibility Considerations . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . M-code Compatibility Considerations . . . . . . . . . . . . . . . . .
TableIndex of Contents (General) 9/SeriesManual Mill 9/Series PAL Reference Operation and Programming Manual xiv
Chapter 1 Using This Manual 1.0 Chapter Overview This chapter describes how to use this manual. Major topics include: how the manual is organized and what information can be found in it. how this manual is written and what fundamentals are presumed to be understood by reader. definitions for certain key terms. 1.1 Audience We intend this manual for use by those who program and/or operate any one of the family Allen-Bradley 9/Series CNCs.
Chapter 1 Using This Manual Table 1.A Manual Organization Chapter 1-2 Title Summary 1 Manual Overview Manual overview, intended audience, definition of key terms, how to proceed. 2 Basic Control Operation A brief description of the control’s basic operation including power up, MTB panel, operator panel, access control, and E-STOP. 3 Offset Tables and Setup Basic setup of the offset table, other initial operating parameters.
Chapter 1 Using This Manual Table 1.A (cont.) Manual Organization Appendix Title Summary Appendix A Softkeys Describes softkeys and their functions for softkey levels 1 and 2. Also the softkey tree displaying all levels of softkeys and their location is shown. Appendix B Error and Operator Messages An alphabetical listing of 9/Series system messages with brief descriptions. Appendix C G and M Code Tables Lists the G-codes used to program the control.
Chapter 1 Using This Manual The term PAL is an abbreviation for Programmable Application Logic. This is a ladder logic program that processes signals between the CNC and the machine. It is usually programmed by the system installer. System Characteristics: Metric Absolute IPM 1.4 Terms and Conventions To make this manual easier to read and understand, we shortened the full product names and features.
Chapter 1 Using This Manual 1.5 Warnings, Cautions, and Important Information We indicate information that is especially important by the following: WARNING: indicates circumstances or practices that can lead to personal injury as well as to damage to the control, the machine, or other equipment. CAUTION: indicates circumstances or practices that can lead to damage to the control or other equipment. Important: indicates information that is necessary for successful application of the control. 1.
Chapter 1 Using This Manual 1-6
Chapter 2 Basic Control Operation 2.0 Chapter Overview This chapter describes how to operate the Allen-Bradley 9/Series control, including: Topic: On page: MTB panel 2-12 {FRONT PANEL} 2-15 Power-up 2-23 Emergency stops 2-24 Access control 2-25 Changing modes 2-33 Display system and messages 2-37 Input cursor 2-41 {REFORM MEMORY} 2-41 Removing an axis 2-43 Time part count 2-43 We also tell you about the control conditions automatically assumed at power up. 2.
Chapter 2 Basic Control Operation Figure 2.1 shows the different operator panels available. The color operator panel has identical keys and softkeys in a slightly different configuration. The portable operator panel has the same key locations as the monochrome operator panel but can be removed from the 9/Series I/O ring. Figure 2.1 Operator Panels 9/SERIES 8 9 4 5 6 1 2 3 .
Chapter 2 Basic Control Operation 2.1.1 Keyboard Table 2.A explains the functions of keys on the operator panel keyboard. In this manual, the names of operator panel keys appear between [ ] symbols. Table 2.A Key Functions Key Name Function Address and Numeric Keys Use these keys to enter alphabetic and numeric characters. If a key has two characters printed on it, pressing it normally enters the upper left character. Holding down the [SHIFT] key while pressing it enters the lower right character.
Chapter 2 Basic Control Operation Reset Operations Block Reset Use the block reset feature to force the control to skip the block execution. To use the block reset function, program execution must be stopped. If program execution stops before the control has completely finished the block execution, a block reset aborts any portion of that block that has not been executed. If program execution stops after the complete block execution (as in the case of single block execution or a M00 etc.
Chapter 2 Basic Control Operation Expressions entered on the input line cannot exceed a total of 25 characters. Only numeric or special mathematical operation characters as described below can be entered next to the “CALC:” prompt. Any character that is not numeric or an operation character you enter on the input line generates the error message “INVALID CHARACTER.” The largest number you can enter for a calculate function is 214748367. You cannot enter a number larger than 10 digits.
Chapter 2 Basic Control Operation Example 2.1 Mathematic Expressions Expression Entered Result Displayed 12/4*3 9 12/[4*3] 1 12+2/2 13 [12+2]/2 7 12-4+3 11 12-[4+3] 5 Table 2.C lists the function commands available with the [CALC] key. Table 2.
Chapter 2 Basic Control Operation Example 2.2 Format for [CALC] Functions SIN[2] This evaluates the sine of 2 degrees. SQRT[14+2] This evaluates the square root of 16. SIN[SQRT[14+2]] This evaluates the sine of the square root of 16. Example 2.3 Mathematical Function Examples Expression Entered Result SIN[90] 1.0 SQRT[16] 4.0 ABS[-4] 4.0 BIN[855] 357.0 BCD[357] 855.0 ROUND[12.5] 13.0 ROUND[12.4] 12.0 FIX[12.7] 12.0 FUP[12.2] 13.0 FUP[12.0] 12.0 LN[9] 2.197225 EXP[2] 7.
Chapter 2 Basic Control Operation Example 2.4 Calling Paramacro Variables with the CALC Function Expression Entered 2.1.3 Softkeys Result Displayed #100 Display current value of variable #100 12/#100*3 Divide 12 by the current value of #100 and multiply by 3 SIN[#31*3] Multiply the value of #31 (for the current local parameter nesting level) by 3 and take the sine of that result We use the term softkey to describe the row of 7 keys at the bottom of the CRT.
Chapter 2 Basic Control Operation Softkey level 1 is the initial softkey level the control displays at power-up. Softkey level 1 always remains the same and all other levels are referenced from softkey level 1. The softkeys on opposite ends of the softkey row have a specific use that remains standard throughout the different softkey levels.
Chapter 2 Basic Control Operation To use a softkey function, press the plain, unmarked button directly below the description of the softkey function. Important: Some of the softkey functions are purchased as optional features. This manual assumes that all available optional features have been purchased for the machine. If an option is not purchased, the softkey is blank. 2.1.4 CRT The control can be purchased with a 9-inch monochrome monitor or a 12-inch color monitor.
Chapter 2 Basic Control Operation 2.1.5 Portable Operator Panel The control can be purchased with a 9-inch monochrome portable operator panel. This panel can be attached or detached to the 9/Series I/O ring operator panel interface assembly at any time without disrupting control operation. The portable operator panel is attached through a 10 ft portable operator panel interface cable with a 3--pin D--shell connector at each end. One end of the cable attaches to the front of the portable operator panel.
Chapter 2 Basic Control Operation 2.2 The MTB Panel Figure 2.3 shows the push-button MTB panel. Table 2.D explains the functions of the switches and buttons on the MTB panel. Other optional or custom MTB panels may be used. Refer to the documentation prepared by your system installer for details. We show button names found on the push--button MTB panel between the < > symbols throughout this manual. The push-button MTB panel uses defaults when you turn on power to the control. Table 2.
Chapter 2 Basic Control Operation Table 2.
Chapter 2 Basic Control Operation Table 2.D Functions of the Buttons on the Push-Button MTB Panel Switch or Button Name How It Works = Default for Push-Button MTB Panel SPINDLE SPEED OVERRIDE Selects the override for programmed spindle speeds in 5% increments within a range of 50% to 120%. SPINDLE or SPINDLE DIRECTION Selects spindle rotation, clockwise (CW), spindle stop (OFF), counterclockwise (CCW). Can be overridden by any programmed spindle direction command.
Chapter 2 Basic Control Operation 2.3 Software MTB Panel {FRONT PANEL} The 9/Series control offers a software MTB panel that performs many of the functions of an MTB panel. This feature uses softkeys instead of the normal switches and buttons of a panel. If the control uses a standard MTB panel (described on page 2-12), or some other custom panel, the requests for operations from the panel takes priority.
Chapter 2 Basic Control Operation The software MTB panel can control these features: Feature 2-16 Description Mode Select Select either Automatic, MDI, or Manual modes as the current operating mode of the control. Rapid Traverse This feature replaces the feedrate when executing a continuous jog move with the rapid feedrate. Feedrate Override Selects a feedrate override percentage for feedrates programmed with an F-word, in 10% increments within a range of 0% to 150%.
Chapter 2 Basic Control Operation Software MTB Panel Screen To use the software MTB panel feature, follow these steps: 1. From the main menu screen, press the {FRONT PANEL} softkey. (softkey level 1) PRGRAM OFFSET MACRO MANAGE PARAM PRGRAM SYSTEM CHECK SUPORT FRONT PANEL SWITCH LANG ERROR PASSMESAGE WORD The Software MTB Panel screen displays the current status of the alterable features.
Chapter 2 Basic Control Operation Jog Screen We assume that you have performed the steps to display the Software Front Panel screen. Make sure that the function selected on the Software Front Panel screen is not the Mirror Image or the Axis Inhibit features. 1. Press the {JOG AXIS} softkey. (softkey level 2) JOG AXIS PRGRAM EXEC This screen appears: E-STOP PROGRAM [mm] F 0.000 MMPM 0.0 Z 0.000 S R X 0.000 T 0 C 359.
Chapter 2 Basic Control Operation Program Execute Screen The following assumes that the steps have been performed to display the Software Front Panel screen (see page 2-17). Make sure that the function selected on the Software Front Panel screen is not the Mirror Image nor the Axis Inhibit feature. 1. Press the {PRGRAM EXEC} softkey. (softkey level 2) JOG AXIS PRGRAM EXEC This screen appears.
Chapter 2 Basic Control Operation 2. Select one of these softkey options: block retrace jog retract cycle start cycle stop 3. To Perform a: Press: Cycle Start the softkey that corresponds to the desired feature. Details on these features are described in chapter 7. Cycle Stop the softkey that corresponds to the desired feature. Details on these features are described in chapter 7. Block Retrace the {BLOCK RETRCE} softkey.
Chapter 2 Basic Control Operation Figure 2.4 Jog Retract Software MTB Panel Screen E-STOP PROGRAM[ MM ] F Z 00000.000 S R X 00000.000 T C 359.99 00000.000 MMPM 0 12 FILENAME SUB NAME MEMORY JOG AXES+ MAN STOP JOG AXES- 2.4 Power Procedures The basic procedure for turning power on and off is described in this section. Refer to the documentation prepared by your system installer for more specific procedures. 2.4.
Chapter 2 Basic Control Operation You see the main menu screen: E-STOP PROGRAM[ MM ] F Z 00000.000 S R X 00000.000 T C 359.99 00000.000 MMPM 12345 FILENAME SUB NAME 9999 MEMORY 30000 MDI STOP (PAL messages) PRGRAM OFFSET MACRO MANAGE PARAM PRGRAM SYSTEM CHECK SUPORT The softkeys available on the main menu screen are referred to as “level 1” softkey functions. Some of the softkey functions are purchased as optional and may not appear exactly as shown. 2.4.
Chapter 2 Basic Control Operation 2.5 Control Conditions at Power-Up After powering up the control or performing a control reset operation (see page 2-4), the control assumes a number of initial operating conditions. These are listed below: Initial Password Access is assigned to the level that was active when power was turned off (provided that level is a power-up level selected in access control).
Chapter 2 Basic Control Operation 2.6 Emergency Stop Operations Press the red button on the MTB panel (or any other E-Stop switches installed on the machine) to stop operations regardless of the condition of the control and the machine. WARNING: To avoid damage to equipment or hazard to personnel, the system installer should connect the button, so that pressing the button opens the circuit connected to the E-STOP STATUS terminal on the control.
Chapter 2 Basic Control Operation If the E-Stop occurred during program execution, the control may reset the program when E-Stop reset is performed provided AMP is configured to do so. Assuming that a control reset is performed, program execution begins from the first block of the program when is pressed. If the current axis position prohibits this, the operator can manually jog the axes clear, or consider executing a Mid-Program Start. See chapter 7.
Chapter 2 Basic Control Operation 2.7.1 Assigning Access Levels and Passwords This section describes setting or changing the functions assigned to a particular access level, and changing the password used to activate that access level.
Chapter 2 Basic Control Operation 2. Press the {ACCESS CONTRL} softkey. If the {ACCESS CONTRL} softkey does not appear on the screen, the currently active access level is not allowed to use the {ACCESS CONTRL} function. Enter a password that has access to {ACCESS CONTRL}. (softkey level 2) ACCESS CONTRL This screen appears.
Chapter 2 Basic Control Operation 3. Press the softkey that corresponds to the access level that you want to change. The pressed softkey appears in reverse video, and the password name assigned to that access level is moved to the “PASSWORD NAME.” Important: If you attempt to change the functions available to an access level that is equal to or higher than your the current access level, the error message “ACCESS TO THIS LEVEL IS NOT ALLOWED.
Chapter 2 Basic Control Operation 2.7.2 Password Protectable Functions The following section describes the functions on the 9/Series control that can be protected from an operator by the use of a password. If a user has access to a function, the parameter associated with that function is shown in reverse video on the access control screen. Access to these functions can be controlled by passwords. Table 2.
Chapter 2 Basic Control Operation Table 2.E Password Protectable Functions 2-30 Parameter Name: Function becomes accessible when parameter name is in reverse video: 8) OFFSETS • {WORK CO-ORD} — Display and alter the preset work coordinate system zero locations and the fixture offset value. • {TOOL WEAR} Display and alter the tool wear amount tables for the different tools. • {TOOL GEOMET} — Display and alter the tool geometry tables.
Chapter 2 Basic Control Operation Parameter Name: Function becomes accessible when parameter name is in reverse video: 23) SCALING When SCALING is not in reverse video, the operator still has access to the {SCALNG} softkey; however values on the screen may not be modified. 24) CHANGE DIRECTORY Allows access to the protectable directory for file edit, direct execution selection, and encrypted output.
Chapter 2 Basic Control Operation E-STOP ENTER PASSWORD: PROGRAM [INCH] F 0.000 MMPM 0 Z 00000.000 S R X 00000.000 T C 359.99 MEMORY MAN 1 STOP ACCESS CONTRL 2-32 2. Enter the password you want to activate by typing it in on the input line with the keys on the operator panel. The control displays * for the characters you entered. If you make an error entering the password, edit the input line as described on page 2-41. 3. When the password is correct, press the [TRANSMIT] key.
Chapter 2 Basic Control Operation 2.8 Changing Operating Modes The control provides 3 basic operation modes: manual (MAN or MANUAL) manual data input (MDI) automatic (AUTO) You can select a mode by using on the MTB panel, or using the {FRONT PANEL} softkey. This is configurable by your system installer. Both means of selection cannot be available. Details on using the {FRONT PANEL} softkey are given on page 2-15.
Chapter 2 Basic Control Operation Manual mode To operate the machine manually, select MAN or MANUAL under or press the {FRONT PANEL} softkey. Use the left/right arrow keys to change the mode select options if using {FRONT PANEL}. For details on Manual Mode operation, see chapter 4. Figure 2.5 Manual Mode Screen E-STOP PROGRAM[ MM ] F 00000.000 Z 00000.000 S R X 00000.000 T C 359.
Chapter 2 Basic Control Operation MDI mode To operate the machine in MDI mode, select MDI under or press the {FRONT PANEL} softkey Use left/right arrow keys to change mode select options if using {FRONT PANEL}. For details on MDI operation, see page 4-11. Figure 2.6 MDI Mode Screen MDI: E-STOP PROGRAM[ MM ] F Z 00000.000 S R X 00000.000 T C 359.
Chapter 2 Basic Control Operation Automatic mode To operate the machine automatically, select AUTO under or press the {FRONT PANEL} softkey Use left/right arrow keys to select mode options if using {FRONT PANEL}. For details on automatic operation, see chapter 7. Figure 2.7 Automatic Operation Screen E-STOP PROGRAM[ MM ] F Z 00000.000 S R X 00000.000 T C 359.
Chapter 2 Basic Control Operation 2.9 Displaying System and Machine Messages The control has two screens dedicated to displaying messages. The MESSAGE ACTIVE screen displays up to nine of the most current system messages and ten of the most current machine (logic generated) messages at a time. The MESSAGE LOG screen displays a log of up to 99 system messages and a separate log of up to 99 machine messages that occurred since the last time memory was cleared.
Chapter 2 Basic Control Operation Figure 2.8 Message Active Display Screen MESSAGE ACTIVE SYSTEM MESSAGE (The system error messages are displayed in this area) MACHINE MESSAGE (The logic messages are displayed in this area) ERROR LOG CLEAR ACTIVE This is the information displayed on the MESSAGE ACTIVE screen. The control displays up to 9 active system messages and up to 10 machine messages.
Chapter 2 Basic Control Operation Figure 2.9 Message Log Display Screen MESSAGE LOG PAGE 1 of 9 SYSTEM MESSAGE (The logged system error messages are displayed in this area) MACHINE MESSAGE (The logged logic messages are displayed in this area) ACTIVE TIME ERRORS STAMPS This is the information displayed on the MESSAGE LOG screen. The control displays up to 99 system messages and up to 99 machine messages.
Chapter 2 Basic Control Operation 2.9.1 Clearing Active Messages {CLEAR ACTIVE} After the cause of a machine or system message has been resolved, some messages remain displayed on all screens until you clear them. CAUTION: Not clearing the old messages from the screen can prevent messages that are generated later from being displayed. This occurs when the old resolved message has a higher priority than the newly generated message.
Chapter 2 Basic Control Operation 2.10 The Input Cursor 2.11 {REFORM MEMORY} The input cursor is the cursor located on lines 2 and 3 of the screen. It is available when you need to input data by using the operator panel (as needed in MDI mode, for example). The following section is a description of how to move the cursor and edit data on the input line by using the keys on the operator panel.
Chapter 2 Basic Control Operation CAUTION: The {REFORM MEMORY} function erases all part programs that are stored in control memory. To reformat control memory and delete all programs stored in memory, follow these steps: 1. Press the {PRGRAM MANAGE} softkey. (softkey level 1) 2. PRGRAM OFFSET MACRO MANAGE PARAM PRGRAM SYSTEM CHECK SUPORT FRONT PANEL SWITCH LANG ERROR PASSMESAGE WORD Press the {REFORM MEMORY} softkey.
Chapter 2 Basic Control Operation 2.12 Removing an Axis (Axis Detach) This feature allows the removal of a rotary table or other axis attachment from a machine. When activated, the control ignores messages that may occur resulting from the loss of feedback from a removed axis such as servo errors, etc. Important: This feature removes the selected axis from the control as an active axis. Any attempt to move the removed axis results in an error.
Chapter 2 Basic Control Operation 2. Press the {ACTIVE PRGRAM} softkey. (softkey level 2) ACTIVE EDIT RESTRT DISPLY COPY PRGRAM PRGRAM PRGRAM PRGRAM PRGRAM DELETE VERFY PRGRAM RENAME INPUT PRGRAM PRGRAM COMENT PRGRAM DEVICE REFORM CHANGE MEMORY DIR 3. Press the {TIME PARTS} softkey. This generates the screen shown in Figure 2.10.
Chapter 2 Basic Control Operation You see the Time Parts screen: Figure 2.
Chapter 2 Basic Control Operation Time Part Screen Field Definitions Program -- is the currently active part program, displayed automatically by the control. Date -- is the current date setting. To change this setting: 1. Press the {SET DATE} softkey, provided that you have supervisor-level access. You are prompted for a new date with a line that displays the current date setting. 2. Press the [DEL] key to erase the characters displayed. 3. Type in the new date.
Chapter 2 Basic Control Operation Workpieces Cut/Overall -- indicates the total number of part programs executed to completion by the control. Use this field to determine the need for periodic checkups or as a statement of warranty. This counter is incremented by one each time the control encounters an M02, M30, or an M99 in a main part program (M99 in a subprogram does not increment this counter, though M02 or M30 does). To clear this field to zero: 1.
Chapter 2 Basic Control Operation Cycle Time -- indicates the elapsed execution time for each individual part program. Cycle time begins counting when the cycle-start button is pressed and ends when an M02 reset or M30 is encountered. To reset this field to zero, use one of three methods: press the cycle-start button to initiate program execution turn off the control power follow these steps: 1. Press the {ED PRT INFO} softkey if you have either operator-level or supervisor-level access. 2.
Chapter 2 Basic Control Operation Remaining Workpieces -- indicates the number of workpieces that still need to be cut in the lot. The value for this field is automatically set equal to the lot size each time the “Lot Size” value is changed. When the control encounters an M02, M30, or M99 in a main part program, the remaining workpieces field is decremented by one. The control tells the system installers PAL program when the lot remaining size is zero.
Chapter 2 Basic Control Operation 2-50
Chapter 3 Offset Tables and Setup 3.0 Chapter Overview In this chapter we describe the basics of job setup. Major topics include how to: use the offset table set and display offset data set and display work coordinate systems set and display communication parameters 3.1 Tool Offset Table {TOOL GEOMET} and {TOOL WEAR} The offset tables are broken in to two major tables: the tool geometry offset table and the wear offset table.
Chapter 3 Offset Tables and Setup Figure 3.1 Offset Table Screen for Wear TOOL OFFSET NUMBER: TOOL NO. 1 2 3 4 5 6 7 8 9 10 11 12 13 WEAR TABLE LENGTH .5321 .4421 .0243 .0156 .0265 .081 .032 .0000 .0000 .0000 .0000 .0000 .0000 X PAGE (DIAMETER) .0234 .0142 .0888 .0791 .0532 .043 .022 .0000 .0000 .0000 .0000 .0000 .0000 1 OF 4 [INCH] [INCH] [INCH] [INCH] [INCH] [ MM ] [ MM ] [INCH] [INCH] [INCH] [INCH] [INCH] [INCH] SEARCH REPLCE ADD TO ACTIVE MORE NUMBER VALUE VALUE OFFSET OFFSET 3.1.
Chapter 3 Offset Table and Setup The system installer determines in AMP which axis (or axes) are used by the control as the tool length axis. Refer to documentation prepared by the system installer for details on what axes have been selected for the tool length axis. This manual assumes that the Z axis is used as the tool length axis. Figure 3.
Chapter 3 Offset Tables and Setup Tool Diameter Compensation Data (Geometry Table) To cut a workpiece using the side face of the cutting tool, it is more convenient to write the part program so that the center of the tool moves along the shape of the workpiece. Since all cutting tools have a diameter, a program written for moving the center of the tool must somehow “compensate” for the tool’s radius. The system installer determines if radius or diameter values are entered in the offset table.
Chapter 3 Offset Table and Setup Tool Diameter Wear Compensation Data (Wear Table) The tool diameter wear compensation feature takes into account the wear that a tool diameter will incur from normal usage. Enter a value in the wear table that is equal to the difference in tool diameter as entered in the geometry table and the actual tool diameter.
Chapter 3 Offset Tables and Setup Important: In order for newly modified tool offsets to become immediately active, cutter compensation must be off (G40 mode). If it is on (G41/G42 mode), the control generates the error message “CHANGE NOT MADE IN BUFFERED BLOCKS”. This indicates that the control is still using the old offset values and must first run several program blocks before using the new offsets values. The new offsets may then be activated too late for your particular application.
Chapter 3 Offset Table and Setup Figure 3.3 Tool Offset (Geometry) Screen TOOL OFFSET NUMBER: TOOL GEOMETRY TABLE NO. 1 2 3 4 5 6 7 8 9 10 11 12 13 LENGTH 1.6396 1.4537 .6312 5.7931 7.8432 0.000 0.000 0.0000 0.0000 0.0000 0.0000 0.0000 0.0000 X PAGE 1 (DIAMETER) 1.6000 .8000 .9000 .5000 .6000 .000 .000 .0000 .0000 .0000 .0000 .0000 .
Chapter 3 Offset Tables and Setup Figure 3.4 Tool Offset (TOOL WEAR) Screen TOOL OFFSET NUMBER: TOOL WEAR TABLE NO. 1 2 3 4 5 6 7 8 9 10 11 12 13 X LENGTH .5321 .4421 .0243 .0156 .0265 .081 .032 .0000 .0000 .0000 .0000 .0000 .0000 PAGE (DIAMETER) .0234 .0142 .0888 .0791 .0532 .043 .022 .0000 .0000 .0000 .0000 .0000 .0000 1 OF 4 [INCH] [INCH] [INCH] [INCH] [INCH] [ MM ] [ MM ] [INCH] [INCH] [INCH] [INCH] [INCH] [INCH] SEARCH REPLCE ADD TO ACTIVE MORE NUMBER VALUE VALUE OFFSET OFFSET 5.
Chapter 3 Offset Table and Setup 3.1.3 Setting Offset Data Using {MEASURE} The measure feature offers an easier method of establishing tool offsets. The control, not the user, computes the tool length offsets and enters the value into the tool offset table. Note the measure feature is used to measure tool length offset values for the wear or geometry tables. It is typically not very effective at measuring tool diameters unless special attention is paid to tool orientation.
Chapter 3 Offset Tables and Setup 3.1.4 Tool Offset Range Verification Tool offset range verification checks: the maximum values entering the tool offset tables the maximum change that can occur in either table To use tool offset range verification, follow this softkey sequence: 9. Press the {SYSTEM SUPORT} softkey. (softkey level 1) PRGRAM OFFSET MACRO MANAGE PARAM PRGRAM SYSTEM CHECK SUPORT FRONT PANEL SWITCH LANG ERROR PASSMESAGE WORD 10. Press the {AMP} softkey.
Chapter 3 Offset Table and Setup Your system installer initially sets these values in AMP. You can modify them with online AMP by using this screen: OFFSET RANGE VERIFICATION [inch] .12345 10.12345 MAXIMUM +/-- WEAR RADIUS MAXIMUM +/-- GEOM RADIUS Per table values [inch] .01000 1.00000 .10000 10.
Chapter 3 Offset Tables and Setup Verify for Maximum Value This value represents the absolute maximum value per table for all tool offsets in that table. If you enter: Then: a positive number greater than the maximum value the control generates the error message: “OFFSET EXCEEDS MAX VALUE” a negative number less than the negative of the maximum value The control does not modify the value in the table.
Chapter 3 Offset Table and Setup 2. Press the {TOOL GEOMET} or the {TOOL WEAR} softkey. It does not matter which softkey is pressed. Any changes made to the active offset number on the tool geometry screen also activates the same offset number on the tool wear screen as well and vice versa. (softkey level 2) WORK TOOL CO-ORD WEAR TOOL TOOL GEOMET MANGE RANDOM TOOL COORD BACKUP SCALNG ROTATE OFFSET The tool offset table is displayed.
Chapter 3 Offset Tables and Setup 3.3 Work Coordinate System Offset Tables {WORK CO-ORD} There are two types of data that are entered in the work coordinate system table. One is the initial work coordinate system zero point locations that are called when programming G54-G59.3. The other is the external offset, used to offset all of the G54-G59.3 zero points to make the same set of work coordinate systems fit a variety of applications.
Chapter 3 Offset Table and Setup 3.3.1 Setting Work Coordinate System Tables There are four methods for modifying work coordinate values. Three methods are discussed in the following chapters: Programming G10s (chapter 11) Setting paramacro system parameters (chapter 28) Modify offsets through PAL (see the system installer’s documentation) The fourth method, and the one discussed in this section, lets you modify the work coordinate values immediately by using the keyboard.
Chapter 3 Offset Tables and Setup Figure 3.5 Work Coordinate System Setting WORK COORDINATE TABLES G54 [INCH] X -9999.9999 Y -9999.9999 Z -9999.9999 U -9999.9999 G55 [ MM ] X -9999.9999 Y -9999.9999 Z -9999.9999 U -9999.9999 G56 [ MM ] X -9999.9999 Y -9999.9999 Z -9999.9999 U -9999.9999 G57 [INCH] X -9999.9999 Y -9999.9999 Z -9999.9999 U -9999.9999 G58 [ MM ] X -9999.9999 Y -9999.9999 Z -9999.9999 U -9999.9999 G59 [ MM ] X -9999.9999 Y -9999.9999 Z -9999.9999 U -9999.
Chapter 3 Offset Table and Setup Data can be replaced or added to as follows: To replace stored data with new data, key-in the new data and press the {REPLCE VALUE} softkey. To add to previously stored data, key-in the amount to be added and press the {ADD TO VALUE} softkey. (softkey level 3) REPLCE ADD TO INCH/ VALUE VALUE METRIC 5. 3.4 Backing Up Offset Tables MORE OFFSET Replace or add data.
Chapter 3 Offset Tables and Setup Important: Once the control begins executing a G10 program that has been previously generated, it will clear any data that already exists in the offset table being updated by that G10 command. This makes it impossible for a G10 block to simply add a few offset values. A G10 program must load the entire offset table each time it is run. Note that tool geometry and tool wear tables are separate offset tables. Loading data into one does not clear the other.
Chapter 3 Offset Table and Setup Figure 3.6 Backup Offset Screen BACKUP OFFSETS TOOL WEAR TOOL GEOMETRY WORK COORDINATE ALL SELECT OPTION USING THE UP/DOWN ARROW TO TO TO PORT A PORT B FILE 3. Select the offsets to be backed up by moving the cursor to the desired offset using the up and down cursor keys. The selected offset will be shown in reverse video. There are four options here: TOOL WEAR ---- When wear is selected all data from the tool offset wear tables is stored as a G10 program.
Chapter 3 Offset Tables and Setup 4. Once the data to save has been selected, determine the destination for the G10 program from these three options: Press the {TO PORT A} softkey to send the G10 program to a peripheral attached to port A. Press the {TO PORT B} softkey to send the G10 program to a peripheral attached to port B. Press the {TO FILE} softkey to send the G10 program to control memory. 5.
Chapter 3 Offset Table and Setup 3.5 Programmable Zone Table The programmable zone feature provides a means to prevent tool motion from entering or exiting a designated area. For details on programmable zones see chapter 12. This table contains the values for programmable zones 2 and 3. These values define the boundaries for the programmable zones and are referenced from the machine coordinate system. Important: These values may also be entered in AMP by the system installer.
Chapter 3 Offset Tables and Setup Figure 3.7 Programmable Zone Table ENTER VALUE: PROGRAMMABLE ZONE LOWER LIMIT UPPER LIMIT LIMIT 2 X Y Z U AXIS AXIS AXIS AXIS 0.0000 0.0000 0.0000 0.0000 0.0000 0.0000 0.0000 0.0000 [ [ [ [ MM MM MM MM ] ] ] ] REPLCE ADD TO MORE UPDATE QUIT VALUE VALUE LIMITS & EXIT Important: Programmable zone coordinates are displayed in inch or metric units for a liner axis, depending on which is the currently active program mode. Rotary axes are shown in units of degrees. 4.
Chapter 3 Offset Table and Setup 5. Data can be replaced or added to as follows: To replace stored travel data with new data, key-in the new data and press the {REPLCE VALUE} softkey. To add to previously stored travel data, key-in the amount to be added and press the {ADD TO VALUE} softkey. (softkey level 4) REPLCE ADD TO VALUE VALUE 6. UPDATE QUIT & EXIT To end editing the programmable zone parameters there are two choices.
Chapter 3 Offset Tables and Setup 2. Press the {PROGRAM PARAM} softkey. (softkey level 2) PRGRAM PARAM AMP DEVICE MONISETUP TOR TIME PARTS PTOM SI/OEM 3. Press the {F1 - F9} softkey to display the single digit feedrate table as shown in Figure 3.8. (softkey level 3) ZONE F1-F9 LIMITS MILCYC PROBE PARAM PARAM Figure 3.8 Single Digit Feedrate Table ENTER VALUE: 1-DIGIT F-WORD F1 F2 F3 F4 F5 F6 F7 F8 F9 REPLCE ADD TO VALUE VALUE FEEDRATE [MMPM] .01000 .02000 .03000 .04000 .05000 .06000 .07000 .
Chapter 3 Offset Table and Setup 4. Use the up, or down cursor keys to move the block cursor to the feedrate parameter to be changed. The selected feedrate will be shown in reverse video. 5. There are two choices for changing feedrate values. Type in a new value for the selected feedrate by using the keys on the operator panel. Then press the {REPLCE VALUE} softkey. The value typed in will replace the old value for that feedrate.
Chapter 3 Offset Tables and Setup 3-26
Chapter 4 Manual/MDI Operation Modes 4.0 Chapter Overview This chapter describes the manual and MDI operating modes. Major topics include: Topic: On page: Mechanical handle feed 4-8 Removing an axis 4-8 Manual machine homing 4-8 MDI mode 4-11 Important: This manual assumes that the standard MTB is being used and standard PAL to run that MTB panel has been installed.
Chapter 4 Manual/MDI Operation Modes Figure 4.1 Data Display in MANUAL Mode E-STOP PROGRAM[ MM ] F X 00000.000 S Z 00000.000 T U 00000.000 W 00000.000 MEMORY 30000 MDI 00000.000 MMPM 0.0 1 STOP N 99999 (First 4 blocks of program shown here) (PAL messages) PRGRAM OFFSET MACRO MANAGE PARAM 4.1.1 Jogging an Axis PRGRAM SYSTEM CHECK SUPORT In the jog modes, the motion of the cutting tool is controlled by the use of pushbuttons, switches, or hand pulse generators (HPGs).
Chapter 4 Manual/MDI Operation Modes The control can be equipped with an optional offset jogging feature, activated by a switch installed by the system installer. When this feature is active, all jog moves are used to offset the current work coordinate system and no position registers are changed. Refer to page 4-6 for details. Only normal single-axis jogs (one axis at a time in the continuous, incremental, or HPG modes) are permitted during a jog retract operation.
Chapter 4 Manual/MDI Operation Modes 3. Press the button for the axis and direction to jog. The control makes one incremental move each time the button is recognized. Until the control completes the execution of the incremental move, no other jog moves are recognized on that axis. This includes attempts to perform other incremental moves on that axis.
Chapter 4 Manual/MDI Operation Modes Figure 4.2 HPG Feed – 4.1.5 Arbitrary Angle Jog + If desired, the system installer can enable a feature that allows control over the angle in which a multiaxis jog move will take through the installation of some optional switches. When this feature is activated, the operator selects two different axes to define a plane for the arbitrary angle jog to take place. Then, an angle is selected (between 0• and 360• ) to define a vector for the jog to take place.
Chapter 4 Manual/MDI Operation Modes 4.1.6 Jog Offset The control may be equipped with an optional jog offset feature, activated by a switch installed by the system installer. When this function is active, all jog moves made are added as offsets to the current work coordinate system. Normally, jogging occurs in the manual mode. The system installer has the option to enable a “Jog on the Fly” feature that will allow jogging in automatic or MDI mode for the purpose of jogging an offset.
Chapter 4 Manual/MDI Operation Modes Programmable Zone Overtravel ---- the axes reach a travel limit established by independent programmable areas. Programmable Zones are activated through programming the appropriate G-code. These 3 causes of overtravel are described in detail in chapter 12. When an overtravel condition occurs, all axis motion stops, the control is placed in cycle stop, and one of the following error messages is displayed.
Chapter 4 Manual/MDI Operation Modes 4.2 Mechanical Handle Feed (Servo Off) This feature lets you disable the servo drives, and allows the axes to be moved by external means (such as a hand crank attached to the ball screw) without requiring the control to be in E-Stop. When this feature is enabled, all position displays get updated as the axes are moved. Use this feature in conjunction with the digitize feature described in chapter 5.
Chapter 4 Manual/MDI Operation Modes Figure 4.3 Machine Home +X Machine home point A AMP-defined home coordinates X=A Z=B +Z B Machine coordinate system zero point The following procedure describes how the control is homed manually by using the pushbuttons on the standard MTB panel. Manual homing may be different for some machines depending on the PAL program written by your system installer.
Chapter 4 Manual/MDI Operation Modes 2. Place the control in manual mode. Refer to page 4-1. 3. Determine the direction that each axis must travel to reach the home limit switch. Refer to your system installer on the location of the home limit switch on a specific machine. 4. Press the button for the axis and direction to home. You can select more than one axis at one time. The axis selected moves at the feedrate under .
Chapter 4 Manual/MDI Operation Modes 4.5 MDI Mode In manual data input (MDI) mode, machine operations can be controlled by entering program blocks directly by using the keys on the operator panel. To begin MDI operations, select MDI under or press the softkey followed by the left and right cursor keys to select the mode if not equipped with a mode select switch or button.
Chapter 4 Manual/MDI Operation Modes Figure 4.5 Program Display Screen in MDI Mode E-STOP PROGRAM[ MM ] F X 00000.000 S Z 00000.000 T U 00000.000 W 00000.000 MEMORY 30000 MDI 00000.000 MMPM 0 1 STOP N 99999 (First 4 blocks of MDI shown here) (PAL messages) PRGRAM OFFSET MACRO MANAGE PARAM 4.5.1 MDI Basic Operation PRGRAM SYSTEM CHECK SUPORT Operating procedures in the MDI mode include: 1. When it is in MDI mode, the control accepts standard programming blocks. 2.
Chapter 4 Manual/MDI Operation Modes 3. Pressing the [TRANSMIT] key transmits the blocks to control memory. Once the blocks have been sent to control memory, you cannot send any more MDI blocks until all of the previous set has been executed. The control displays the first 4 blocks of the MDI program entered on lines 17-20 with an ! (exclamation point) just to the left of the blocks.
Chapter 4 Manual/MDI Operation Modes Figure 4.6 MDI Mode Program Screen E-STOP PROGRAM[ MM ] F Z 00000.000 S R X 00000.000 T C 359.99 MEMORY 30000 MDI 00000.000 MMPM 0 1 STOP N 99999 (First 4 blocks of MDI shown here) (PAL messages) PRGRAM OFFSET MACRO MANAGE PARAM PRGRAM SYSTEM CHECK SUPORT Important: Performing a block reset operation causes the control to abort the current MDI program block or skip the following MDI program block. Refer to page 2-4 for details.
Chapter 5 Editing Programs Online 5.0 Chapter Overview This chapter describes the basics of editing programs on line (at the keyboard) including: Selecting the program to edit Editing programs Programming aids {QUICKVIEW} Digitizing a program (Teach) Deleting program {DELETE} Renaming programs {RENAME} Displaying a program {DISPLAY} Comment display {COMENT} Copying programs {COPY PRGRAM} Programs may also be edited off line (at a personal computer).
Chapter 5 Editing Programs Online 5.1 Selecting the Program To Edit This section discusses how to select a part program for editing. Note that only part programs that are stored in control memory may be edited online. If a part program is on tape or other storage device and must be edited online, copy this program to memory as described in chapter 9. Important: You can edit both active and inactive programs.
Chapter 5 Editing Programs Online 2. The part program to be edited can be selected using two methods: Keying-in the program name of the part program to edit or create. or Moving the cursor to the program name on the program directory screen by using the up or down cursor keys. Important: If you are creating a new program and using it as a subprogram, see chapter 10 and its section on program names.
Chapter 5 Editing Programs Online Figure 5.2 Program Edit Screen INSERT : EDIT FILE : 000001 N00020 N00025 N00030 N00035 N00040 N00050 POS 1*1 MODE : CHAR WHILE [#1LT 10] DO 1; G01 F1000 X#1; G04 P1 #1 = [#1 + 1]; END 1; M99; MODIFY BLOCK BLOCK INSERT DELETE TRUNC DELETE EXIT CH/WRD EDITOR The maximum number of programs that you can have is 328. To store a program, it needs to occupy at least 1.3 meters of memory.
Chapter 5 Editing Programs Online 5.2.1 Moving the Cursor {STRING SEARCH} and Cursor Size {CHAR/WORD} The following section discusses moving the cursor in the program display area (lines 7-20 of the CRT). It assumes that a program has already been selected to edit as discussed in section 5.1. Important: The input cursor is the cursor shown on the input lines (2 and 3 on the screen). Details on the input cursor are given in chapter 2.
Chapter 5 Editing Programs Online 3. Key in the character or character string to search for, and press either the: {FORWRD} softkey -- to search in the forward direction in the part program {REVRSE} softkey -- to search in the reverse direction in the part program (softkey level 4) FORWRD REVRSE TOP OF BOT OF PRGRAM PRGRAM If the control cannot find the character or character string, it issues the error message “SEARCH STRING NOT FOUND” 4. To end the search operation press the exit [• ] softkey.
Chapter 5 Editing Programs Online 5.2.2 Entering Characters and Blocks After selecting a part program to be edited, use the following method to add lines, blocks, or characters to the part program. The control should be in the edit mode at this point with EDIT: displayed in the input area of the screen (lines 2-3 ). To enter blocks in a program: 1. Move the block cursor to the location in which program blocks or characters are to be added using the up, down, left and right cursor keys. 2.
Chapter 5 Editing Programs Online 2. Locate the block cursor in the program display area at the character(s) that need to be changed by pressing the up, down, left, and right cursor keys. Characters shown in reverse video on the screen will be the characters changed. 3. Key in a new character or word to replace data located by the cursor in the input area, then press the [TRANSMIT] key. Important: Only the data that is within the cursor will be changed.
Chapter 5 Editing Programs Online Example 5.3 Changing Words To change X97 to X42 in the following block first select the word cursor size (see section 5.2.1): Program Block (Program Display Area) Enter (Input Area) G01X97Z93; Notes Move the block cursor to the word X97 in the program display area and toggle the {MODIFY/INSERT} softkey to “MODIFY:”.
Chapter 5 Editing Programs Online Example 5.4 Inserting Characters To change G01X97Z93; to two separate blocks: Program Block (Program Display Area) Enter (Input Area) G01X97Z93; Notes Move the block cursor to the Z in the program display area and toggle the {MODIFY/INSERT} softkey to “INSERT:”. G01X97Z93; ; Type this data into the input area,then press the [TRANSMIT] key. Note: Entering the EOB in the step above is not necessary. G01X97; Z93; Result Example 5.
Chapter 5 Editing Programs Online 5.2.4 Erasing Characters and Blocks The control can erase part program data in 3 ways: Erase a character or a word Erase all the characters from the current location of the cursor to the EOB code (;). Erase an entire block. Erasing a Character or Word 1. First choose whether to erase a character or a word by pressing the {CHAR/WORD} softkey. 2. From the edit menu move the cursor until the character or word to be erased is in reverse video. 3.
Chapter 5 Editing Programs Online (softkey level 3) MODIFY BLOCK BLOCK INSERT DELETE TRUNC DELETE EXIT CH/WRD EDITOR STRING RENUM MERGE QUICK SEARCH PRGRAM PRGRAM VIEW CHAR/ WORD DIGITZ E Example 5.7 Erasing to the End of the Block Character To erase Z20. from the block below: Program Block (Program Display Area) Enter (Input Area) Notes X93Z20; move the cursor to the Z X93Z20; Press the {BLOCK TRUNC} softkey. X93; Result Erasing An Entire Block: 1.
Chapter 5 Editing Programs Online Example 5.8 Erasing An Entire Block Program Block (Program Display Area) Enter (Input Area) Notes X93M01Z10; Position the cursor any where in the block X93M01Z10; Press the {BLOCK DELETE} softkey. Result -- the block will be completely deleted Important: If the block consist of more than one line on the CRT the entire block is deleted, not just the line that contains the cursor.
Chapter 5 Editing Programs Online Follow these steps to assign or renumber sequence numbers: 1. From the edit menu, press the continue softkey {• } to change the softkey functions. 2. Press the {RENUM PRGRAM} softkey (softkey level 3) MODIFY BLOCK BLOCK INSERT DELETE TRUNC DELETE EXIT CH/WRD EDITOR STRING RENUM MERGE QUICK SEARCH PRGRAM PRGRAM VIEW CHAR/ WORD DIGITZ E 3.
Chapter 5 Editing Programs Online 4. Here are two choices: To assign sequence numbers or to resign sequence numbers to all blocks from the beginning of the part program, press the {ALL} softkey. To assign new sequence numbers to only the blocks that already have sequence numbers, press the {ONLY N} softkey. (softkey level 4) A L L ONLY N Important: Any sequence numbers in a block that are referenced in the current program by a paramacro “GOTO” or “WHILE” will also be renumbered.
Chapter 5 Editing Programs Online 4. Key-in the program name of the part program to insert, then press either the [TRANSMIT] key or the {EXEC} softkey. (softkey level 1) EXEC 5.2.7 Exiting Edit Mode {EXIT EDITOR} When you edit a program, all changes and additions that you make are saved immediately in the control’s memory. No formal “save” command is executed. You cannot quit, abandon or abort an edit session and restore the original version of the program you have been editing.
Chapter 5 Editing Programs Online 5.3 Programming Aids {QUICK VIEW} The QuickView features display sample patterns or the G--code prompts to help in writing part programs. By keying in data corresponding to prompted messages, the control will automatically generate the required block(s) to insert into an existing part program.
Chapter 5 Editing Programs Online Axis Selection The selection of the axes that can be programmed using QuickView is determined by the type of QuickView prompt you are using. The two factors the control uses to determine the axes for QuickView are based on if the QuickView prompt is for a planer G--code or a non-planer G--code. Planar G--codes -- Planar G--codes are any feature that is plane dependant (such as G02, G41, Cycles, etc...).
Chapter 5 Editing Programs Online 5.3.1 Selecting a QuickView Plane This feature is used to select the plane that is used to program the different QuickView features in. This will determine what plane is displayed for the prompting and their axis names displayed for the prompts. It is not possible to select any parallel planes with the QuickView feature, only primary planes may be used. The system installer determines the primary planes established by G17, G18, and G19 in AMP.
Chapter 5 Editing Programs Online 5.3.2 Using {QPATH+ PROMPT} Sample Patterns 5-20 With the QuickView functions and the QuickPath Plus section, dimensions from part drawings can be used directly to create a part program. The sample patterns available with the QuickPath Plus prompts are summarized below. {CIR ANG PT} The arc radius and the taper angle of a line are known for the geometry from an arc to the line.
Chapter 5 Editing Programs Online Angle of a line, corner radius, and chamfer size is often necessary for a sample pattern in QuickPath Plus prompting. The following prompts in QuickPath Plus prompting refer to the following drawing dimensions: ,A ..... Angle ,R ..... Corner radius ,C ..... Chamfer size L ..... Length of line For more information regarding these designations see chapter 15 on programming QuickPath Plus or chapter 16 on programming chamfers and corner radius.
Chapter 5 Editing Programs Online Figure 5.3 QuickPath Plus Menu Screen CIRCLE, ANGLE, POINT ANGLE, CIRCLE, POINT CIRCLE , CIRCLE ANGLE, POINT QUICKPATH PLUS MENU 1 CIR ANG PT 3. CIR CIR ANG CIR PT ANG PT After selecting the desired sample pattern enter values for the parameters in the following way. Use the up and down cursor keys to select the parameter to change or enter. The selected item will be shown in reverse video.
Chapter 5 Editing Programs Online 5. To enter the blocks in the program being edited, move the block cursor in the program display area just past the location in the program where it is desired to insert the new blocks. Then press the [TRANSMIT] key. The generated blocks will be entered to the left of the cursor. 6. Press the exit {• } softkey to return to the main edit menu or press a different QuickView key for more prompting.
Chapter 5 Editing Programs Online 5.3.3 G- code Format Prompting {GCODE PROMPT} G-code format prompting aids the operator in programming different G--codes by prompting the programmer for the necessary parameters. A graphical representation is usually provided also to show the programmer a sample of what the G-code parameters are used for. Milling fixed-cycle G--codes are available under fixed-cycle prompting, section 5.3.4. The following is a description of how to use the G--code prompting menus. 1.
Chapter 5 Editing Programs Online 2. Position the cursor at the desired G--code to prompt by using the up and down cursor keys. The selected G--code is shown in reverse video. 3. Once the correct G--code is selected, press the {SELECT} softkey. A screen with prompts for that G--code is displayed. 4. Use the up and down cursor keys to select the parameters to be changed or entered. The selected item will be shown in reverse video.
Chapter 5 Editing Programs Online 5.3.4 Mill Cycle Format Prompting Milling fixed cycle format prompting aids the programmer by prompting for the necessary parameters for the milling cycle. A graphical representation illustrating the fixed cycles operation and use of the parameters is also displayed. For G--code prompts see section 5.3.3. To use the MILL fixed cycle prompting function follow the steps below. 1. From the QuickView menu press the {MILL PROMPT} softkey.
Chapter 5 Editing Programs Online 4. Use the up and down cursor keys to select the parameters to be changed or entered. The selected parameter will be shown in reverse video. Axis words followed by a (1), (2), or (3) are prompting for the first, second, or third coordinate position respectively. The location of the first, second, or third axis word is shown on the drawing accompanying the prompt screen.
Chapter 5 Editing Programs Online 5.4 Digitizing a Program (Teach) The digitize feature allows the programmer to generate blocks in a program based on the actual position of the cutting tool rather than typing in positions manually. The control records actual tool locations and uses them to generate program blocks. The digitize feature can be used in any operating mode (auto, manual, or MDI).
Chapter 5 Editing Programs Online 4. Press the {MODE SELECT} softkey if it is necessary to change any of the following programming modes while digitizing a program: Inch/metric Absolute programming/incremental programming. Change planes G17, G18, or G19. Press any of the softkeys corresponding to the desired mode to change. The control will display the mode that the next block will be programmed, in the upper right hand corner of the screen. The modes are abbreviated as discussed in Table 5.A.
Chapter 5 Editing Programs Online 5. Determine if the next move will be linear or circular. If the next move is to be linear press the {LINEAR} softkey (section 5.4.1). If the next move is to be circular press either the: {CIRCLE 3 PNT} softkey if 3 points on the arc are known. (section 5.4.2) {CIRCLE TANGNT} softkeys if the endpoint of the arc and the line that is tangent to the start point of the arc is known.(section 5.4.
Chapter 5 Editing Programs Online Figure 5.7 Linear Digitize Screen DIGITIZE: METRIC, ABS, G17 ABSOLUTE [ MM F ] GOO X 0.000 Y 0.000 Z 0.000 0.000 MMPM S STORE END PT 00 EDIT & STORE Reposition the tool at the desired end point of the linear move using any of the following methods. Jog the Axes in manual mode. Automatically move the axes by executing a part program or MDI program.
Chapter 5 Editing Programs Online After the axes have been positioned at the end point of the linear move press either the {STORE END PT} or the {EDIT & STORE} softkeys. This will record the current tool location as the final position for this digitize operation. The {STORE END PT} softkey does not return the control to the program display screen.
Chapter 5 Editing Programs Online Figure 5.8 CIRCLE 3 PNT Digitize Screen DIGITIZE: ABSOLUTE [ MM ] METRIC, ABS, G17 GOO X Y Z F 0.000 0.000 0.000 0.000 MMPM S RECORD MID PT 00 STORE END PT EDIT & STORE Reposition the tool at any point on the arc between the start and the end point using any of the following methods. Jog the Axes in manual mode. Automatically move the axes by executing a part program or MDI program.
Chapter 5 Editing Programs Online After the second point on the arc has been stored reposition the axes at the end point of the arc. Store this block as a circular block by pressing either the {STORE END PT} or the {EDIT & STORE} softkeys. This will record the current tool location as the final position for this digitize operation. The {STORE END PT} softkey does not return the control to the program display screen.
Chapter 5 Editing Programs Online Figure 5.9 CIRCLE TANGNT Digitize Screen DIGITIZE: ABSOLUTE [ MM ] METRIC, ABS, G17 GOO X 0.000 Y 0.000 Z 0.000 F 0.000 MMPM S 00 STORE END PT EDIT & STORE Reposition the tool at the end point of the arc using any of the following methods. Jog the Axes in manual mode. Automatically move the axes by executing a part program or MDI program.
Chapter 5 Editing Programs Online After the axes have been positioned at the end point of the arc press either the {STORE END PT} or the {EDIT & STORE} softkeys. The control will store the current tool position as the end point of the arc. The {STORE END PT} softkey does not return the control to the program display screen.
Chapter 5 Editing Programs Online 5.5 Deleting Program {DELETE PRGRAM} To delete part programs stored in memory: 1. Press the {PRGRAM MANAGE} softkey. (softkey level 1) 2. PRGRAM OFFSET MACRO MANAGE PARAM QUICK CHECK FRONT PANEL SWITCH LANG ERROR PASSMESAGE WORD SYSTEM SUPORT Press the {DELETE} softkey.
Chapter 5 Editing Programs Online 5.6 Renaming Programs {RENAME PRGRAM} To change the program names assigned to the part programs stored in memory: 1. Press the {PRGRAM MANAGE} softkey. (softkey level 1) 2. PRGRAM OFFSET MACRO MANAGE PARAM QUICK CHECK FRONT PANEL SWITCH LANG ERROR PASSMESAGE WORD SYSTEM SUPORT Press the {RENAME PRGRAM} softkey.
Chapter 5 Editing Programs Online 5.7 Displaying a Program {DISPLY PRGRAM} The control has a part program display feature that allows viewing (but not editing) of any part program. Follow these steps to display a part program stored in the control’s memory. 1. Press the {PRGRAM MANAGE} softkey. (softkey level 1) PRGRAM OFFSET MACRO MANAGE PARAM QUICK CHECK FRONT PANEL SWITCH LANG ERROR PASSMESAGE WORD SYSTEM SUPORT 2.
Chapter 5 Editing Programs Online 5.8 Comment Display {PRGRAM COMENT} It is possible to assign a short comment on the program directory screens to each individual program. These comments are used to help identify a program when it is selected for automatic operation or to be edited. Important: These are not normally the same as a comment block made within a part program. Comment blocks are discussed in section 10.2.3.
Chapter 5 Editing Programs Online If a comment has previously been entered it will be displayed to the right of the “COMMENT” prompt. This comment may be edited using the input cursor as discussed in chapter 2, or the old comment may be deleted by pressing the [DEL] key while holding down the [SHIFT] key. 4. 5. 5.9 Copying Programs {COPY PRGRAM} Type in the new comment or edit the old comment by keying it in using the keyboard.
Chapter 5 Editing Programs Online 2. Press the {COPY PRGRAM} softkey. (softkey level 2) ACTIVE EDIT RESTRT DISPLY COPY PRGRAM PRGRAM PRGRAM PRGRAM PRGRAM VERIFY PRGRAM DELETE RENAME INPUT PRGRAM COMENT PRGRAM PRGRAM DEVICE REFORM MEMORY 3. Cursor down to or enter the program name of the program to be copied, followed by a comma and a name for the duplicate program. COPY: FROM_NAME,TO_NAME 4. Press the {MEM TO MEM} softkey.
Chapter 5 Editing Programs Online 5.10 Selecting the Protectable Part Program Directory This section contains information on how to select the protectable part program directory. Use this directory to store part programs that you wish to control access to. When part programs that have previously been protected through encryption are downloaded to the control from ODS or the Mini DNC package, they are automatically stored in the protectable part program directory.
Chapter 5 Editing Programs Online The control displays the main program directory screen: SELECTED PROGRAM: MAIN DIRECTORY NAME MAIN O12345 RRR TEST SIZE 1 OF 1 COMMENT 2.3 14.3 9.3 3.9 4 FILES PAGE THIS IS A TEST PROG 120.2 METERS FREE ACTIVE EDIT RESTRT DISPLY COPY PRGRAM PRGRAM PRGRAM PRGRAM PRGRAM 2. Press the {CHANGE DIR} softkey.
Chapter 5 Editing Programs Online The control displays the protectable directory screen: SELECTED PROGRAM: PROTECTABLE NAME DIRECTORY SIZE PROTECT1 PROTECT2 PROTECT3 PROG PROTECT4 4 FILES 2.3 14.3 9.3 PAGE 1 OF 1 COMMENT THIS IS A PROTECTED 3.9 120.2 METERS FREE REFORM CHANGE NCRYPT SET-UP MEMORY DIR MODE NCRYPT The programs in this directory are protected.
Chapter 5 Editing Programs Online 5.10.1 Protected Program Encryption and Decryption Protected program encryption and decryption allow you to encrypt a protected program so that it is unreadable when it is uploaded. Protected programs in encrypted form can only be uploaded or downloaded by using the Upload and Download utilities of ODS or the Mini DNC package. Use the {NCRYPT MODE} softkey to enable the protected program encryption option.
Chapter 5 Editing Programs Online The control displays the set-up encryption screen: ENTER A CHARACTER: ” # % & ( ) * + ’ - = = = = = = = = = = = . / 0 1 2 3 4 5 6 7 8 = = = = = = = = = = = 9 : ; < = > ? @ A B C = = = = = = = = = = = D E F G H I J K L M N = = = = = = = = = = = O P Q R S T U V W X Y = = = = = = = = = = = Z = [ = ] = UPDATE STORE REVRSE & EXIT BACKUP FILL You must fill in the encryption/decryption table.
Chapter 5 Editing Programs Online To fill in the encryption/decryption table by using the {REVRSE FILL} softkey, press the {REVRSE FILL} softkey. Pressing this softkey automatically fills the spaces of the encryption/decryption table in a reverse order as shown below: ENTER A CHARACTER: ” # % & ( ) * + ’ - = = = = = = = = = = = ] [ Z Y X W V U T S R .
Chapter 5 Editing Programs Online Once the encryption/decryption table is created and you press the {NCRYPT MODE} softkey, protected programs are encrypted when they are uploaded to ODS or the Mini DNC package. When downloading encrypted protected programs to the control, they are decrypted and loaded into the protected program directory. 5.10.
Chapter 5 Editing Programs Online 5-50
Chapter 6 Editing Part Programs Offline (ODS) 6.0 Chapter Overview You can use the offline development system (ODS) to write or edit part programs. Once completed these part programs may be downloaded from the workstation to the control. Programs that already exist on the control may be uploaded to the workstation for editing or backup. Programs on ODS may be edited using the screen or text editor that is configured in ODS.
Chapter 6 Editing Part Programs Offline 6.1 Selecting the Part Program Application Selecting the Part Program application provides access to the part program utilities of ODS. To select the Part Program application: 1. Return to the main menu line of ODS. 2. Press [F3] to pull down the Application menu: The workstation displays this screen: Proj: PALTEST F1 - File Appl: Upload F2 - Project F3 - Application AMP PAL I/O Assignments Part Program Upload Download 3.
Chapter 6 Editing Part Programs Offline 2. Press [F4] to pull down the Utility menu: The workstation displays this screen: Proj: PALTEST Appl: Upload F1 - File F2 - Project F3 - Application Util: Get PAL I/O F5 - Configuration F4 - Utility Edit Part Program File Management 3. Press [E] (E) (F) to select the Part Program option.
Chapter 6 Editing Part Programs Offline 4. Select a new or existing file. To create a new file, type in the new file name. To open an existing file use the arrow keys to select a file or type in a file name. Press [ENTER] when done, or [ESC] to cancel.
Chapter 6 Editing Part Programs Offline 6.3 Interfacing the Workstation with the Control The following sections require the workstation to be interfaced with the control or storage device. Interface the workstation with the control or storage device using the RS-232 serial interface cable. This cable is used to connect the RS-232 interface port on the rear of the workstation to Port B on the control or the RS-232 port on the storage device. Refer to your integration manual for more information.
Chapter 6 Editing Part Programs Offline To download a part program from ODS to the control’s memory, follow these steps: 1. Interface the workstation with the control (see section 6.3) 2. Return to the main menu line of ODS 3. Press [F3] to pull down the Application menu. The workstation displays this screen: Proj: PALTEST F1 - File Appl: Upload F2 - Project F3 - Application AMP PAL I/O Assignments Part Program Upload Download 4.
Chapter 6 Editing Part Programs Offline 5. Press [F4] to pull down the Utility menu. Proj: Demo F1 - File Appl: Download F2 - Project F3 - Application Util: File Management F5 - Configuration F4 - Utility Send AMP params Send PAL and I/O Send Part Program 6. (A) (P) (R) Use the arrow keys to highlight the Send Part Program option then press[ENTER], or press [R].
Chapter 6 Editing Part Programs Offline 7. Use the arrow keys to highlight the download destination or press the letter that corresponds to the download destination. When selected press [ENTER]. The workstation displays the part program files that are stored in the active project directory of the workstation: Proj: Demo Appl: Download F1 - File F2 - Project F3 - Application Util: File Management F4 - Utility F5 - Configuration Downloading Use ARROW keys or Type in name.
Chapter 6 Editing Part Programs Offline If the selected part program file name already exists on the control, the workstation displays this screen: Proj: Demo F1 - File Appl: Download F2 - Project F3 - Application Util: Get Part Program F4 - Utility F5 - Configuration File Already Exits Enter Option Rename existing file Overwrite existing file Abort current file (R) (O) (A) Important: The currently active or open part program on the control can not be renamed or overwritten during a download proc
Chapter 6 Editing Part Programs Offline After selecting the Rename or Overwrite option, or if the file being downloaded did not already exist on the control, the workstation displays this screen: Proj: Demo F1 - File Appl: Download F2 - Project F3 - Application Util: Send Part Program F4 - Utility F5 - Configuration Download In Progress Percent completed 50% The percentage of the download process that has currently been completed is displayed on the screen.
Chapter 6 Editing Part Programs Offline When the download process is complete, you see this screen: Proj: Demo F1 - File Appl: Download F2 - Project F3 - Application Util: Send Part Program F4 - Utility F5 - Configuration Download Complete Download Another File? Yes No 9. (Y) (N) Select “Yes” or “No.” If “Yes” is selected, the programmer will be prompted through the download procedure again. If “No” is selected, the workstation returns to the main menu line of ODS.
Chapter 6 Editing Part Programs Offline 6.5 Upload Part Programs to ODS The programmer can upload a part program from the control’s memory to the workstation using the Upload application of ODS. This allows the part program to be edited or stored on the workstation. 1. Interface the workstation with the control (see section 6.3) 2. Return to the main menu line of ODS 3. Press [F3] to pull down the Application menu.
Chapter 6 Editing Part Programs Offline Proj: Demo F1 - File Appl: Part Program F2 - Project F3 - Application Util: none F5 - Configuration F4 - Utility Get AMP params Get PAL and I/O Get Part Program 6. (A) (P) (R) Use the arrow keys to highlight the Get Part Program option then press[ENTER], or press [R].
Chapter 6 Editing Part Programs Offline The workstation displays the part program files that are stored on the control or storage device: Proj: Demo Appl: Part Program F1 - File F2 - Project F3 - Application Util: Get Part Program F4 - Utility F5 - Configuration Upload From... Use ARROW keys or Type in name. Press ENTER when done, or ESC to cancel. FILE1 FILE2 FILE3 8.
Chapter 6 Editing Part Programs Offline If the selected part program already exists on the workstation, the workstation displays this screen: Proj: Demo Appl: Upload F1 - File F2 - Project F3 - Application Util: Get Part Program F5 - Configuration F4 - Utility File Already Exits Enter Option Rename existing file Overwrite existing file Abort current file (R) (O) (A) If the Rename option is selected, the workstation renames the existing file, which has the same name as the file being uploaded, on
Chapter 6 Editing Part Programs Offline If the Overwrite option is selected, the part program file being uploaded overwrites the file having the same name on the workstation. If the Abort option is selected, the upload process is discontinued and the workstation prompts the programmer for additional files to upload. Important: If a wildcard was entered in place of a file name, the Abort option is repeated for each file that matches the wildcard. Pressing the [ESC] key quits the abort wildcard process.
Chapter 6 Editing Part Programs Offline After the part program has been uploaded to the workstation, the workstation displays this screen: Proj: Demo F1 - File Appl: Upload F2 - Project F3 - Application Util: Get Part Program F4 - Utility F5 - Configuration Upload Complete Upload Another File? Yes No (Y) (N) Select “Yes” or “No.” If “Yes” is selected, the programmer will be prompted through the upload procedure again. If “No” is selected, the workstation returns to the main menu line.
Chapter 6 Editing Part Programs Offline 6-18
Chapter 7 Running a Program 7.0 Chapter Overview This chapter describes how to test a part program and execute it in automatic mode. Major topics include: selecting special running conditions program selection options starting and stopping test and automatic operation program checking modes automatic operation mode interrupted program recover {RESTRT PRGRAM} jog retract block retrace 7.
Chapter 7 Running a Program 7.1.2 Miscellaneous Function Lock When the MISCELLANEOUS FUNCTION LOCK is made active, the control displays M--, second auxiliary functions (B--codes), S--, and T--codes in the part program, except for M00, M01, M02, M30, M98, and M99.
Chapter 7 Running a Program To enter a sequence number to stop execution: 1. Press the {PRGRAM MANAGE} softkey. Note that a program must have already been selected for automatic execution as discussed in section 7.3. (softkey level 1) 2. PRGRAM OFFSET MACRO MANAGE PARAM QUICK CHECK FRONT PANEL SWITCH LANG ERROR PASSMESAGE WORD SYSTEM SUPORT Press the {ACTIVE PRGRAM}.
Chapter 7 Running a Program 7.1.4 Single Block In single block mode, the control executes the part program block by block. Each time the button is pressed, the control executes one block of commands in the part program when in single block mode. Figure 7.1 Single Block SINGLE BLOCK CYCLE START When is pressed, one block of commands is executed Cutting tool Workpiece To activate the single block function, press the button.
Chapter 7 Running a Program 7.2 Selecting a Part Program Input Device Before selecting a part program it is necessary to tell the control where this part program is currently residing.
Chapter 7 Running a Program 3. Press the softkey corresponding to the location the part program is to be read from, {FROM PORT A} , {FROM PORT B}, or {FROM MEMORY}. (softkey level 3) FROM FROM FROM PORT A PORT B MEMORY To activate a part program, it must be selected as discussed in section 7.3. 7.3 Selecting a Program To select a program for automatic execution, follow the steps below.
Chapter 7 Running a Program To select a program for automatic execution: 1. Press the {PRGRAM MANAGE} softkey. The control displays the program directory screen as shown in Figure 7.2. (softkey level 1) PRGRAM OFFSET MACRO MANAGE PARAM QUICK CHECK FRONT PANEL SWITCH LANG ERROR PASSMESAGE WORD SYSTEM SUPORT Figure 7.2 Part Program Directory SELECTED PROGRAM: DIRECTORY NAME TEST O12345 MAIN SHAFT2 XXX PAGE SIZE AE 3.9 1.3 1.3 1.3 1.
Chapter 7 Running a Program 2. Key in the name of the part program to activate. Not that if the program is being selected from control memory the • or • cursor keys may be used to select the program to activate from the directory screen. If the part program is being selected from a peripheral device (attached to port A or port B) the part program name must be manually keyed in. Also make sure the peripheral device is on and ready to output the part program.
Chapter 7 Running a Program 7.4 Deselecting a Part Program It is sometimes necessary to deactivate a part program that has been selected for automatic execution. This is necessary when selecting a different part program for automatic execution. To do this follow these steps: 1. Press the {PRGRAM MANAGE} softkey. The control displays the program directory screen as shown in Figure 7.2.
Chapter 7 Running a Program 7.5 Program Search {SEARCH} Use the Program Search feature to begin program execution from some block other than at the beginning of the program. This feature requires the operator to establish the necessary G, M, S, F, and T words, work coordinate offsets, etc., that should be active for that block’s execution. The control is capable of starting a program at a chosen block and establishing any previous G, M, S, F, and T words work coordinate offsets, etc.
Chapter 7 Running a Program 3. Press the {SEARCH} softkey. (softkey level 3) DE-ACT SEARCH MID ST T PATH SEQ PRGRAM PRGRAM GRAPH STOP TIME PARTS 4.
Chapter 7 Running a Program When using the N search, O search, or STRING search features, first key in the desired N number, O number, or character string to search for. After it has been keyed in, press the [TRANSMIT] key to start the search. Press the {FORWRD} or {REVRSE} softkeys to search for the entered value in the forward or reverse direction. Press the {TOP OF PRGRAM} softkey to return to the top of the program (the beginning of the first block).
Chapter 7 Running a Program 7.6 Search With Recall {MID ST PRGRAM} Use the Mid-Start Program feature to begin program execution from some block other than the first block of the program. This feature will scan the program as it searches and from within the search area: send to PAL the last programmed modal G--codes from each modal group.
Chapter 7 Running a Program Important: The search with recall feature will not: send PAL nonmodal M--codes including user--defined groups 0 -- 3, group 4, group 5, and group 6 M--codes. on dual process systems, halt execution for synchronization codes. read from or write paramacro variables to PAL on dual process systems, shared paramacro variables between processes may not be evaluated as desired depending on the status of the other process.
Chapter 7 Running a Program 3. Press the {MID ST PRGRAM} softkey. (softkey level 3) DE-ACT SEARCH MID ST T PATH SEQ PRGRAM PRGRAM GRAPH STOP TIME PARTS 4. To search for a sequence number press the {SEQ # SEARCH} softkey. To search for a character string press the {STRING SEARCH} softkey. (softkey level 4) SEQ # STRING SEARCH SEARCH 5. Key in the desired character string or sequence number to search for and press the [TRANSMIT] key.
Chapter 7 Running a Program 6. Press the {EXIT} or the {EXIT & MOVE} softkey once the program is at the desired location. {EXIT} - Use this softkey if the tool is at the exact location for execution of the searched program block. While the control searches for your starting block it performs calculations to determine what the absolute position of the axes should be before your selected block is executed.
Chapter 7 Running a Program Program interrupts that are enabled in blocks prior to the searched block (M96L__P__), are active and available for execution once the active program begins execution. Interrupts can not be executed while the mid-program search operation is taking place. 7.7 Basic Program Execution After a program is written or loaded into the control, it should be thoroughly tested before a part is mounted and cut.
Chapter 7 Running a Program Axis Inhibit, Dry Run, and Automatic operation can be interrupted using any of the operations listed below. Execution may be resumed at the interrupted location by pressing the button: (1) Pressing When the button is pressed, motion of the cutting tool decelerates and stops, and the control stops automatic operation.
Chapter 7 Running a Program 7.7.1 {QUICK CHECK} Quick Check is a basic syntax checker for a part program. It checks that proper format and syntax has been followed during programming . No actual axis motion is produced in Quick Check mode however offsets and coordinate system shifts are performed. The Quick Check feature is also available with an optional graphics feature. If the graphics feature is to be used refer to chapter 8 for Quick Check with graphics.
Chapter 7 Running a Program If the control finds no errors during Quick Check the program screen displays the message “COMPLETED WITH NO ERRORS”. The control then automatically resets the program to the first block. To disable Quick Check without the graphics options, simply press the {QUICK CHECK} button again. To disable Quick Check with the graphics options, press the {Quick Check} softkey followed by the {STOP CHECK} softkey.
Chapter 7 Running a Program AXIS INHIBIT can be activated to inhibit motion of any or all of the axes depending on the configuration determined by the system installer. This includes jogging moves. When axis motion has been inhibited for a single axis the remaining axes still execute as normal and the axis location display is updated as if axis motion was occurring on all axes. WARNING: Axes not selected for axis inhibit move as they would if the program were executed in automatic mode.
Chapter 7 Running a Program The switch may be used to modify the cutting feedrate. The system installer determines in AMP if rapid feedrates are overrides by or the switch during Dry Run. CAUTION: When testing a program using Dry Run the control still recognizes and executes M, B, S, and T--codes. To ignore M, B, S, and T--codes execute Dry Run in conjunction with miscellaneous function lock (section 7.1.2).
Chapter 7 Running a Program 7.7.4 Part Production/Automatic Mode Automatic mode is the normal operating mode of the control. A program that is run in the automatic mode is executed with all of the axes active and all of the programmed feedrates active. Graphics is also available as discussed in chapter 8. To select the automatic mode, place (on the MTB panel) in the AUTO position. If not equipped with a mode select switch, use the {FRONT PANEL} softkey.
Chapter 7 Running a Program In automatic mode, the control manages machine operations according to the commands in a part program. CYCLE START ---- begins part program execution CYCLE STOP ---- stops part program execution WARNING: Always test a program prior to automatic operation. Always verify that the workspace is clear and all safety features are intact before pressing CYCLE START. Figure 7.5 Automatic Mode 9/Series 0 12345 . S ____ M ____ . G92 X ____Y ____ . A D _______ . G00 ______ .
Chapter 7 Running a Program 7.8 Interrupted Program Recover {RESTRT PRGRAM} Use the program recover feature to resume a program that was executing and was interrupted by some means such as a control reset, E-STOP, or even power failure in some cases. This feature will scan the program as it searches for the interrupted block and from within the search area: send to PAL the last programmed modal G--codes from each modal group.
Chapter 7 Running a Program CAUTION: When a program recover is performed, the control automatically returns the program to the beginning of the block that was originally interrupted. The beginning of the block is probably not the point that axis motion was interrupted. For absolute linear moves this causes no problem if the tool is still somewhere along the path of the block that program execution was interrupted while cutting.
Chapter 7 Running a Program To perform a program restore operation after automatic program execution has been interrupted follow these steps: 1. Press the {PRGRAM MANAGE} softkey. (softkey level 1) PRGRAM OFFSET MACRO MANAGE PARAM QUICK CHECK FRONT PANEL SWITCH LANG ERROR PASSMESAGE WORD SYSTEM SUPORT Important: DO NOT SELECT A PROGRAM AS AN ACTIVE PROGRAM. Do not disable the currently active program (if any).
Chapter 7 Running a Program CAUTION: When you exit a program restart operation (search with memory), M- and S-codes are sent to PAL. If, during normal execution, that program activated a spindle, mid-program start may also start it. 4. Press the {EXIT} softkey if the block selected is the block to begin program execution from. If it not the desired block, it will be necessary to disable the program or perform a search with memory operation to locate the desired block manually.
Chapter 7 Running a Program CAUTION: If the Jog Retract function is deactivated during its execution (performing a control reset, E-STOP, etc.), attempting to return the tool by pressing cycle start may cause the Jog Retract funtion to abort. The tool will return to the start point of jog retract along a linear path. This is most likely not the retracted path.
Chapter 7 Running a Program Figure 7.6 Jog Retract Operation Jog retract exit moves Jog retract return moves In Figure 7.6 notice that the control only recognized 6 jog moves upon returning instead of the actual 11 moves that were made to retract the tool. This is because the jog retract feature records consecutive jog moves on the same axis as one move.
Chapter 7 Running a Program Figure 7.7 Jog Retract Moves that Exceed the Maximum Allowed in AMP Return path 4 2 3 7 5 1 6 Figure 7.7 emphasizes the possible problems that may result from exceeding the maximum allowed jog retract moves. In this example the number of allowed moves set in AMP is four. When the cycle start button is pressed at the end of the 7th jog move the control ignores moves 5, 6, and 7 and takes the shortest path to the endpoint of exit move 4.
Chapter 7 Running a Program To perform a block retrace operation: 1. Press the or activate the feature button to stop program execution. 2. Press the button. After the button is pressed the control will retrace the block that was being executed when the cycle stop occurred or retrace the block just completed if the single block button was pressed, provided that the block is a legal block for retrace.
Chapter 7 Running a Program The block retrace function is unable to retrace any of the following blocks and an attempt to do so will result in an error message. Threading Tapping Boring Inch/Metric changes (unit conversion) A block that commands a tool change operation. A block that commands a change in the coordinate system. Any block that is followed by a Manual Jog Move except a Jog Retract. The number of blocks retraced is already equal to the maximum number of re-traceable blocks as determined in AMP.
Chapter 7 Running a Program 7-34
Chapter 8 Display and Graphics 8.0 Chapter Overview The first part of this chapter gives a description of the different data displays available on the control. The second part gives a description of the control’s graphics capabilities. 8.1 Selection of Axis Position Data Display Pressing the [DISP SELECT] key displays the softkeys for selecting the axis position data screens. The control provides 8 different axes position data screens as described in Table 8.A.
Chapter 8 Displays and Graphics The screens described above may also show in addition to axis position: The current unit system being used (millimeters or inches) E-STOP The current feedrate The current spindle speed of the controlling spindle The current tool and tool offset numbers The active program name (if any) The active subprogram name (if any) The current amount of usable memory remaining The current operating mode (MDI, manual or automatic) The current operating status (cycle stop, suspend, start,
Chapter 8 Displays and Graphics 3. To return to softkey level 1, press the [DISP SELECT] key again. The most recently selected data position screen will remain in effect for softkey level 1 until either power is turned off or a different position display screen is selected. The default screen selected at power up is the regular size program display. The following figures show the axis position data display that will result when the corresponding softkey is pressed.
Chapter 8 Displays and Graphics (2) {PRGRAM} (Large Display) Axis position in the current work coordinate system displayed in large characters. Figure 8.2 Results After Pressing {PRGRAM} (Large Display) Softkey PROGRAM[ MM E-STOP (ACTIVE PROGRAM NAME) ] X - 7483 .647 Z - 7483 .647 U - 7483 .647 F 0.
Chapter 8 Displays and Graphics {PRGRAM} (Small Display) Axis position in the current work coordinate system displayed for all system axes in the active process (only available when more than 9 axes are AMPed in the system, or more than 8 axes in the process for dual process systems). Figure 8.3 Results After Pressing {PRGRAM} (Small Display) Softkey PROGRAM[ MM X Y Z U V W A B C $X $Y $Z F ] -9999.647 -3333.647 -1111.647 -2222.647 -2222.647 -2222.647 -2222.647 -2222.647 -2222.647 -2222.647 -2222.
Chapter 8 Displays and Graphics (3) {ABS} The axis position data in the machine coordinate system. Figure 8.4 Results After Pressing {ABS} Softkey E-STOP ABSOLUTE[ MM ] 0.000 MMPM 00 X 0.000 S Z 0.000 T 0 U -0.
Chapter 8 Displays and Graphics (4) {ABS} (Large Display) Axis position in the machine coordinate system displayed in large characters. Figure 8.5 Results After Pressing {ABS} (Large Display) Softkey E-STOP ABSOLUTE[ MM ] (ACTIVE PROGRAM NAME) X 0.000 Z 0.000 U -0.035 F 0.
Chapter 8 Displays and Graphics {ABS} (Small Display) The axis position data in the machine coordinate system displayed for all system axes in the active process (only available when more than 9 axes are AMPed in the system, or more than 8 axes in the process for dual process systems). Figure 8.6 Results After Pressing {ABS} (Small Display) Softkey ABSOLUTE X Y Z U V W A B C $X $Y $Z F [ MM ] -9999.647 -3333.647 -1111.647 -2222.647 -2222.647 -2222.647 -2222.647 -2222.647 -2222.647 -2222.647 -2222.
Chapter 8 Displays and Graphics (5) {TARGET} The coordinate values of the end point of the currently executing axis move is displayed at a position in the current work coordinate system. Figure 8.7 Results After Pressing {TARGET} Softkey E-STOP TARGET[ MM ] F X -7483.647 S Z -7483.647 T 0 U -7483.647 MEMORY MAN PRGRAM A B S 0.
Chapter 8 Displays and Graphics (6) {TARGET} (Large Display) The coordinate values in the current work coordinate system, of the end point of commanded axis moves in normal size characters. Figure 8.8 Results after Pressing {TARGET} Softkey TARGET [ MM F E-STOP (ACTIVE PROGRAM NAME) ] X - 7483 . 647 Z - 7483 . 647 U - 7483 . 647 0.
Chapter 8 Displays and Graphics {TARGET} (Small Display) The coordinate values of the end point of the currently executing axis move is displayed at a position in the current work coordinate system for all system axes in the active process (only available when more than 9 axes are AMPed in the system, or more than 8 axes in the process for dual process systems). Figure 8.9 Results After Pressing {TARGET} (Small Display) Softkey TARGET X Y Z U V W A B C $X $Y $Z F [ MM ] -9999.647 -3333.647 -1111.
Chapter 8 Displays and Graphics (7) {DTG} The distance from the current position to the command end point, of the commanded axis in normal size characters. Figure 8.10 Results After Pressing {DTG} Softkey E-STOP DISTANCE TO GO[ MM F X 0.021 S Z 0.000 T 0 U 0.000 MEMORY MAN PRGRAM A B S 8-12 ] 0.
Chapter 8 Displays and Graphics (8) {DTG} (Large Display) The distance from current position to the command end point of the commanded axis move in large characters. Figure 8.11 Results After Pressing {DTG} (Large Display) Softkey E-STOP DISTANCE TO GO[ MM F ] (ACTIVE PROGRAM NAME) X 0.021 Z 0.000 U 0.000 0.
Chapter 8 Displays and Graphics {DTG} (Small Display) The distance from the current position to the command end point, of the commanded axis in normal size characters is displayed for all system axes in the active process (only available when more than 9 axes are AMPed in the system, or more than 8 axes in the process for dual process systems). Figure 8.12 Results After Pressing {DTG} (Small Display) Softkey Distance to Go X Y Z U V W A B C $X $Y $Z F ] 0000.000 0000.000 0000.000 0000.000 0000.
Chapter 8 Displays and Graphics (9) {AXIS SELECT} Important: {AXIS SELECT} is available only during a large character display or when more than 9 axes are displayed on a normal size display. When you press {AXIS SELECT}, the control displays the axis names in the softkey area. Press a specific axis letter softkey to toggle the position display of that axis on and off.
Chapter 8 Displays and Graphics (10) {M CODE STATUS} The currently active M codes are displayed. This screen indicates only the last programmed M code in the modal group. It is the PAL programmer’s responsibility to make sure proper machine action takes place when the M code is programmed. Figure 8.
Chapter 8 Displays and Graphics (11) {PRGRAM DTG} This screen provides a multiple display of position information from the program screen and the distance to go screen. Figure 8.15 Program, Distance to Go Screen E-STOP PROGRAM DISTANCE TO GO X - 7483.647 X 0.031 Y - 7483.647 Y 0.000 Z - 7483.647 Z 0.000 F 0.
Chapter 8 Displays and Graphics {PRGRAM DTG} (Small Display) This screen provides a multiple display of position information from the program screen and the distance to go screen. It displays all system axes in the active process (only available when more than 9 axis are AMPed in the system, or more than 8 axis in the process for dual process systems). Figure 8.16 Program, Distance to Go Screen (Small Display) Distance to Go PROGRAM X Y Z U V W A B C $X $Y $Z F 0.
Chapter 8 Displays and Graphics (12) {ALL} This screen provides a multiple display of position information from the program, distance to go, absolute, and target screen. The all display is only available on systems with 6 or less axes. On systems with more than 6 axes, other combination screens are available which display a subset of the data available on the ALL display. Figure 8.17 Result After Pressing {ALL} Softkey E-STOP PROGRAM DISTANCE TO GO X Y Z X Y Z - 7483.647 - 7483.647 - 7483.647 0.
Chapter 8 Displays and Graphics (13) {G CODE STATUS} The currently active G-codes are displayed. Figure 8.18 Results After Pressing {G CODE} Softkey PROGRAM STATUS PAGE 2 OF 2 G50.1 MIRROR IMAGE CONTROL G64 G67 CUTTING MODE MACRO CALL CANCEL G70 G80 G90 G94 G97 G98 INCH PROGRAMMING CANCEL OR END FIXED CYCLE ABSOLUTE FEED/MIN CSS PROGRAMMING OFF FIXED CYCLE INITIAL LEVEL RETURN PROGRAM STATUS G01 G07 G12.
Chapter 8 Displays and Graphics (14) {SPLIT ON/OFF} The split screen softkey is only available if your system installer has purchased the dual-process option. When you press the {SPLIT ON/OFF} softkey, you can view information for both processes. The screen displays two 40-column screens on one 80-column screen. Process 1 is displayed on the left, and process 2 is displayed on the right. The active process appears in reverse video.
Chapter 8 Displays and Graphics A large screen display makes it easier for you to see the axes. E-STOP PROGRAM [MM] PROGRAM [MM] R R F X 0.000 Z 0.000 0.000 IPM S O R F X 0.000 0.000 PRGRAM 8.2 PAL Display Page ABS IPM S O TARGET DTG AXIS SELECT If desired the system installer has the option of configuring custom screens that will show up on the CRT.
Chapter 8 Displays and Graphics When changing the value of some parameter on the PAL display page, part program execution is not typically interrupted. If some data that is used in a currently executing part program is changed the control will handle that data in the following manner: If the parameter altered is used in the currently executing program block, that value will not be activated until the following block (unless a cutter compensation value is being altered).
Chapter 8 Displays and Graphics 9/240 CNCs The 9/240 control is equipped to display four languages. The languages available and the order they are displayed are fixed in this order: English Italian Japanese German 8.4 Graphics QuickCheck and active program graphics function similarly. They both plot tool paths. The following section describes how to use both types of graphics and distinguishes how they differ.
Chapter 8 Displays and Graphics 2. Select a program. Press {SELECT PRGRAM}. (softkey level 2) SELECT QUICK PRGRAM CHECK STOP CHECK T PATH T PATH GRAPH DISABL 3. Use the up and down cursors to select a program. 4. Press {ACTIVE PRGRAM} to return to level 2 and activate the program. Follow these steps to run graphics: 8.4.2 Running Graphics 1. Press the {PRGRAM CHECK} softkey. (softkey level 1) 2.
Chapter 8 Displays and Graphics The control for both QuickCheck and active graphics continues to plot tool paths, even if the graphics screen is not displayed. Actual display of the tool paths is only possible on the graphics screen. When the graphics screen is displayed again, any new tool motions appear on the screen. While on the graphics screen only the currently executing block is displayed. The currently executing block is displayed on line 22 of the CRT, and it is limited to 80 characters.
Chapter 8 Displays and Graphics In some cases, you may want to operate without graphics. For example, you cannot edit a part program using QuickView while in graphics, or you may want to speed up processing by disabling graphics. 8.4.
Chapter 8 Displays and Graphics You may want to change the parameters to alter your graphics. If you want to view a different graphics screen, you must change the default values for the parameters.
Chapter 8 Displays and Graphics 2. Set Select Graph. Use the up and down cursor keys to select the axes. Then set them by pressing the left or right cursor keys. The data for the selected axes change each time you press the left or right cursor key. A pictorial representation of the selected graph, which is determined by the selected axes, is displayed on the screen. You have three fields that you can adjust. The axes are shown as horizontal and vertical axes.
Chapter 8 Displays and Graphics 4. Set Auto Size. Use the up and down cursor keys to select the parameter. Set auto size by pressing the left or right cursor keys. The value for the selected parameter changes each time you press the left or right cursor key. If you turn this parameter “ON”, the control re-sizes the graphics screen to the size of the programmed part. To use this feature, turn this parameter “ON”, then run the part program.
Chapter 8 Displays and Graphics 7. Set the Main Program Sequence Starting #: parameter. It is only available with QuickCheck. Use the up and down cursors to select this parameter. Set it by typing in the new value for that parameter using the keys on the operator panel. Press the [TRANSMIT] key when the new value has been typed in. The old value for the sequence number is replaced with the new value.
Chapter 8 Displays and Graphics 9. Set the Process Speed parameter. It is only available with QuickCheck. Use the up and down cursors to select this parameter. Set it by pressing the left or right cursor keys. The data for the selected parameter changes each time you press the left or right cursor key. Use this parameter to select the speed for the control to draw graphics.
Chapter 8 Displays and Graphics 8.4.5 Graphics in Single-Block 8.4.6 Clearing Graphics Screen The active and QuickCheck graphics features can run in single-block or continuous mode as described in chapter 8. In: This happens: Single block one block of a part program executes each time you press the . Continuous mode the control continues to execute blocks sequentially as they are read.
Chapter 8 Displays and Graphics Figure 8.19 Zoom Window Graphic Display Screen 20.0 15.6 11.1 6.7 2.2 -2.2 -6.7 X -11.1 -15.6 -20.0 -20.0 -10.3 Z -0.5 9.2 INCR DECR WINDOW WINDOW 18.9 27.7 ZOOM ABORT 38.4 48.1 57.9 ZOOM This screen resembles the regular QuickCheck graphics screen with the exception that it includes a window and different softkeys. Use the window to define a new size and location for the tool path graphic display. The area within the window will become your next screen.
Chapter 8 Displays and Graphics To use the zoom window feature: 1. Press the {ZOOM WINDOW} softkey. This changes the display to the zoom window display. (softkey level 3) CLEAR MACHNE ZOOM GRAPHS INFO WINDOW 2. ZOOM BACK GRAPH SETUP Use the cursor keys on the operator panel to move the center of the window around the screen. To move the window center at a faster rate, press and hold the [SHIFT] key while pressing the cursor keys.
Chapter 8 Displays and Graphics 3. 4. To change the size of the window, use the {INCR WINDOW} or {DECR WINDOW} softkeys. To change the window size at a faster rate, press and hold the [SHIFT] key while pressing the {INCR WINDOW} or {DECR WINDOW} softkeys. Each time you press: The Zoom Window : {INCR WINDOW} increases in size. {DECR WINDOW} decreases in size. Once the size and the location of the window are correct, press the {ZOOM} softkey to return to the regular QuickCheck graphics screen.
Chapter 8 Displays and Graphics 8.6 Power Turn-on Screen When power is turned on, the control displays the power turn-on screen. The following section discusses how to modify information displayed on this screen at power up. Editing the System Integrator Message Lines To edit the system integrator message lines of the power turn-on screen, do the following: 1. Press the [SYSTEM SUPORT] softkey.
Chapter 8 Displays and Graphics 4. Press the {ENTER MESAGE} softkey. This highlights the softkey, and the control displays the input prompt “PTO MESSAGE:” at the top of the screen. Also, the current text, if any, of the selected message line is shown on the input line next to the prompt. (The text may be edited like any other input string.) (softkey level 3) ENTER MESAGE 5. STORE BACKUP Once the line has been edited, press the key. This transfers the edited line to the PTO screen.
Chapter 8 Displays and Graphics 8.7 Screen Saver The 9/Series screen saver utility is designed to reduce the damage done to the CRT from “burn in”. Burn in is the result of the same lines or characters being displayed at the same location on the screen for a such a long period of time that they leave a permanent imprint on the CRT.
Chapter 8 Displays and Graphics 2. Press the [SCREEN SAVER] softkey. (softkey level 2) PRGRAM PARAM AMP PTOM SI/OEM DEVICE MONI- TIME SETUP TOR PARTS SYSTEM SCREEN TIMING SAVER The screen saver setup screen appears. SCREEN SAVER ACTIVATION TIMER : 05 MINUTES SAVER ON/OFF INCR TIMER DECR TIMER Press This Softkey To: SAVER ON/OFF toggle between enabling and disabling the screen saver. When the softkey name is shown in reverse video, the screen saver is enabled.
Chapter 9 Communications 9.0 Chapter Overview This chapter covers: 9.1 Setting Communications This section covers the communication port parameters that are available with the control. You use communication parameters to let the control communicate with peripheral devices.
Chapter 9 Communications 2. Press the {DEVICE SETUP} softkey to display the device setup screen as shown in Figure 9.1. (softkey level 2) PRGRAM PARAM AMP DEVICE MONISETUP TOR TIME PARTS PTOM SI/OEM The 9/230 CNC does not support port A. It uses only port B. Figure 9.
Chapter 9 Communications 3. Use the up or down cursor keys to move the cursor to the parameter to be changed. The current value for each parameter will be shown in reverse video. Important: Select both the SERIAL PORT (A or B) and the DEVICE being set first (see Figure 9.1) since all other parameters are device dependent. 4. To change a value after a parameter has been selected, press the left or right cursor keys.
Chapter 9 Communications DEVICE (setting type of peripheral) Select your peripheral device immediately after selecting your serial port. The devices with default communication parameters stored in the control are listed in Table 9.A. If the device that you are using is not listed, select either USER PUNCH, USER PRINTER, or USER READER. Important: You cannot select the same device for both peripheral ports.
Chapter 9 Communications PORT TYPE Port type options differ depending on the port you select.
Chapter 9 Communications PROTOCOL Select the protocol for communications from the following options. LEVEL_1 LEVEL_2* DF1 RAW PARITY (parity check) Select the parity from the following parity check schemes: Parity Parity Check NONE No parity check EVEN Even parity ODD Odd parity STOP BIT (number of stop bits) Select the number of stop bits with this parameter. You can select: 1, 1.5, or 2 bits DATA LENGTH Select the number of bits that constitute one character with this parameter.
Chapter 9 Communications OUTPUT CODE Select either EIA (RS-244A) or ASCII (RS-358-B) as output codes for 8 bit data lengths. Selecting 7 bit data length sets this output code to “N/A” since EIA and ASCII do not apply to this type. AUTO FILENAME This parameter is valid only if you are inputting part programs to the control from a tape reader (refer to DEVICE for details). This parameter is used only if your tape contains more than one part program.
Chapter 9 Communications STOP PRG END This parameter is available only if you are reading a tape and have selected a tape reader as your device (refer to DEVICE for details). It determines if the tape reader is to stop at the end of each program or continue reading until the end-of-tape code is reached. Refer to the PROGRAM END section to determine what defines the end-of-program for your system. Setting Result Yes the tape reader stops every time it encounters a program end code.
Chapter 9 Communications If “%” is set to “yes”, making it a valid program end-code, no program end-code other than PRGRM NAME can be set to “yes”. If another program end-code is set to “yes”, the “%” option is automatically set to “no”. Refer to the descriptions for M-codes in chapter 10 for details. M02, M30 -- refer to the descriptions for M-codes in chapter 10 for details M99 -- refer to the descriptions for M-codes in chapter 10 for details % -- also used as end-of-tape code.
Chapter 9 Communications Figure 9.2 Program Directory Screen SELECTED PROGRAM: DIRECTORY NAME O12345 TEST MAIN TTTE XXX PAGE SIZE 1.3 3.9 1.3 1.3 1.3 5 FILES 1 OF 1 COMMENT SUB TEST 1 NEW THIS IS A TEST PROGRAM 120.7 METERS FREE ACTIVE EDIT RESTRT DISPLY COPY PRGRAM PRGRAM PRGRAM PRGRAM PRGRAM 3. Press the {COPY PRGRAM} softkey.
Chapter 9 Communications 5. Select the device to copy from by using this table. If the peripheral device is connected to: Press this softkey: Port A {FROM A TO MEM} Port B {FROM B TO MEM} The screen is changes to the “COPY PARAMETERS” screen (Figure 9.3) and displays the current device and setup parameters for that communication port. If the device displayed on the screen is not correct, select the correct device using the procedure described in section 9.1.1 Figure 9.
Chapter 9 Communications 6. Specify if you want to copy one program or multiple programs. Input Single Program Press {SINGLE PRGRAM} to copy one program from tape. Input terminates when the first program end or tape end code is encountered. Input Multiple Programs Press {MULTI PRGRAM} to copy multiple programs from the tape into memory. If STOP PRG END was set to the tape reader “yes” stops each time it encounters a program end or tape end code.
Chapter 9 Communications 9.3 Outputting Part Programs to a Tape Punch If a program is in control memory and you want to send a copy of that program to a peripheral device, follow these steps: 1. Verify that the peripheral device is connected to the correct serial port and that the port is configured for that device (see section 9.1.1). 2. Press the {PRGRAM MANAGE} softkey. The control displays the screen shown in Figure 9.4.
Chapter 9 Communications 3. Press the {COPY PRGRAM} softkey. (softkey level 2) ACTIVE EDIT RESTRT DISPLY COPY PRGRAM PRGRAM PRGRAM PRGRAM PRGRAM VERIFY PRGRAM DELETE RENAME INPUT PRGRAM COMENT PRGRAM PRGRAM DEVICE REFORM MEMORY 4. Enter the program name to output from memory. There are two ways to do this: Type in the program name using the alphanumeric keys on the key board. The control displays program name on the input line (line 2 of the screen) next to the prompt “FILENAME”.
Chapter 9 Communications 6. Specify if you want to output one, multiple, or all programs onto tape. Output Single Program Press {SINGLE PRGRAM} to output the program selected in step 4. Output Multiple Programs Press {MULTI PRGRAM} to output more than one program. After you pressed the {MULTI PRGRAM} key, the program selected in step 4 is output. The Program Directory Screen (refer to Figure 9.
Chapter 9 Communications Output All Programs Press {OUTPUT ALL} to copy all programs in memory to tape at one time. {OUTPUT ALL} works like {MULTI PRGRAM} except that you cannot select the programs you want to output. {OUTPUT ALL} selects all programs automatically and outputs them to the peripheral device. All programs are copied to the peripheral device and stored using the same program name as the original, in the order that they appear on the Program Directory Screen.
Chapter 9 Communications 9.4 Verifying Part Programs Against Source Programs To verify that a part program stored in memory matches a source program stored in memory or on a peripheral device: 1. If one of the programs to either verify or verify against is on a peripheral device, make sure that the peripheral device is connected to the correct serial port and that the port is configured for that device (see section 9.1.1). 2. Press the {PRGRAM MANAGE} softkey. (softkey level 1) 3.
Chapter 9 Communications 5. To verify a part program in memory against a part program stored on a peripheral device, press the {VERIFY PORT A} or {VERIFY PORT B} softkey depending on where the peripheral device is connected. To verify a part program in memory against another part program in memory, press the {VERIFY MEMORY} softkey. (softkey level 3) VERIFY VERIFY VERIFY PROT A PORT B MEMORY 6. Press the {VERIFY YES} softkey. To abort the verify operation press the {VERIFY NO} softkey.
Chapter 10 Introduction to Programming 10.0 Chapter Overview The control performs machining operations by executing a series of commands that make up a part program. These commands are interpreted by the control which then directs axis motion, spindle rotation, tool selection, and other CNC functions. Part programs can be executed from the control’s memory or from a CNC tape. Programs on tape can be executed directly from the tape, or can be loaded into the control and executed from memory.
Chapter 10 Introduction to Programming Tape with Program End = M02, M30, M99 This particular tape format allows single- or multi-program format on a tape. It also allows you to enter either M02, M30 or M99 as a program end code (refer to chapter 9 for details on legal program end codes). Figure 10.1 shows a typical configuration for a multiple program tape with M30 and M99 as program end codes.
Chapter 10 Introduction to Programming Figure 10.
Chapter 10 Introduction to Programming (3) Program Start Code The first end-of-block code (EOB code) after the leader section indicates the beginning of the part program. The EOB code is designated with: line feed (LF) ---- ASCII format carriage return (CR) ---- EIA format Important: When performing an EOB search, the search is executed from the beginning of the part program, NOT from the point of display. (4) O--word Program Name The program name, if on the tape, must follow the program start code.
Chapter 10 Introduction to Programming (6) Comment Information punched between the control out code “(” and the control in code “)” within the program section is considered a comment and is not handled as significant information (even though it is copied to and from control memory or tape). Any number of comments can be included in a part program interspersed with program blocks or words. Example 10.1 Comments in Part Programs X1.Z1.
Chapter 10 Introduction to Programming 10.2 Program Configuration Each machining operation performed by the control is determined by the control’s interpretation of a group of words (commands) called a “block.” Individual blocks in a part program define each machining process. Part programs consist of a number of blocks that together define a complete operation on a part.
Chapter 10 Introduction to Programming The control sequentially executes blocks in a part program to conduct the required machining operation. Important: To make jumps, loops, or calculations within an executing program or subprogram use the paramacro features as discussed in chapter 28. A part program has a: beginning ---- setting up the control and the machine to perform the operations wanted.
Chapter 10 Introduction to Programming 10.2.1 Program Names Enter up to 8 alphanumeric characters for program names, which the control uses to call up programs for editing or automatic operations. Subprograms are designated with the letter O followed by 5 numbers. If a new program name is entered with 5 numeric characters, the control assumes that it is a subprogram and automatically inserts the letter O as the first character in the name.
Chapter 10 Introduction to Programming 10.2.2 Sequence Numbers Each block in a part program can be assigned a sequence number to distinguish one block from another. Sequence numbers begin with an N address followed by a one to five digit numeric value. Sequence numbers can be assigned at random to specific blocks or to all blocks if desired. Blocks assigned sequence numbers can be called later by designating their sequence number.
Chapter 10 Introduction to Programming 10.2.3 Comment Blocks Information between the control out code “(” and the control in code “)” within a part program is regarded as a comment and not handled as significant information. The comment can be described in up to 128 characters (including the control out/in codes) consisting of alphanumeric characters and special symbols. Example 10.6 Program Block With A Comment N00010G91X5.(CHANGE TO INC. 10.2.
Chapter 10 Introduction to Programming The control considers a “/” without a number to mean “/1”. However, “/1” must be programmed if more than one block delete number is to be used in a block. The block delete is active for sequence number search and dry run operations. The control ignores the block delete when loading a part program from tape or other device into control memory. The control also ignores the block delete when a part program is saved on punched tape or other device from control memory.
Chapter 10 Introduction to Programming 10.3 Using Subprograms When the same series of blocks are repeated more than once it is usually easier to program them using a subprogram. The key difference between a subprogram and a G65 paramacro is that a paramacro always gets a new set of local parameters, a subprogram uses the same set of local parameters that the main program used. See chapter 28 for details on paramacros and local parameters.
Chapter 10 Introduction to Programming 10.3.1 Subprogram Call (M98) Generally, programs are executed sequentially. When an M98Pnnnnn (“nnnnn” representing a subprogram number) command is entered in a program, the control will merge the subprogram, designated by the address P, before the block that immediately follows the M98 command. Note that the control will issue the error message “CANNOT OPEN SUBPROGRAM” if it can not find the subprogram designated by the M98 command.
Chapter 10 Introduction to Programming 10.3.2 Main and Subprogram Return (M99) M99 code acts as a return command in both sub- and main programs. There are specific differences, however, when the code is used in a sub program and when it is used in a main program.
Chapter 10 Introduction to Programming Example 10.8 Subprogram Calls and Returns MAIN PROGRAM SUBPROGRAM 1 SUBPROGRAM 2 (MAIN PROGRAM); (SUBPROGRAM 1); (SUBPROGRAM 2); N00010...; N00110; N00210; N00020...; N00120...; N00220...M99; N00030M98P1; N00130M99; N00040...; N00140...; N00050...; N00150M30; N00060M98P2L2; N00070M30; The following path of execution will result when the main program above is selected as the active program. (MAIN PROGRAM); N00010...; N00020...
Chapter 10 Introduction to Programming Nesting is the term used to describe one program calling another. The program called is said to be a nested program. When a subprogram is called from the main program it is said to be on the first nesting level or nesting level 1. If that subprogram in turn calls another subprogram the called subprogram is said to be in nesting level 2. Subprograms may be nested up to a maximum of 4 levels. 10.3.3 Subprogram Nesting Figure 10.
Chapter 10 Introduction to Programming 10.4 Word Formats and Functions Words in a part program consist of addresses and numeric values. Address ---- A character to designate the assigned word function. Numeric value ---- A numeral to express the event called out by the word. Figure 10.4 Word Configuration Word G 0 Address Word 1 X 1 .3 1 Numeric value For each word used in a part program, there is a format that designates the number of digits allowable as a numeric value for that word.
Chapter 10 Introduction to Programming Table 10.A shows the effects of leading zero suppression (LZS) and trailing zero suppression (TZS). It presumes that the system installer has set a format of X5.2 (integer 5 digits, decimal 2 digits) in AMP. Different formats would result in different decimal point placement compared to those shown on the following page, but the end result would be comparable. Table 10.
Chapter 10 Introduction to Programming Important: If backing up a table using a G10 program (such as the offset tables or coordinate system tables), keep in mind the G10 program output is generated in the current format of the control (LZS or TZS). If you intend to transport this table to a different machine it must also be using the same format.
Chapter 10 Introduction to Programming Table 10.B Word Formats and Descriptions Address A Valid Range Inch Valid Range Metric Function 8.6 8.5 Rotary axis about X (AMP assigned) 3.3 3.3 Angle in QuickPath Plus programming 8.6 8.5 Rotary axis about Y (AMP assigned) 3.0 3.0 Second miscellaneous function (AMP assigned) 8.6 8.5 Rotary axis about Z (AMP assigned) 8.6 8.5 Chamfer length in QuickPath Plus programming 3.0 3.0 Tool radius compensation number 8.6 8.5 Fixed cycle parameter.
Chapter 10 Introduction to Programming Table 10.B Word Formats and Descriptions Address S Valid Range Inch Valid Range Metric Function 5.3 5.3 Spindle rpm function 5.3 5.3 Spindle Orient 4.3 3.3 CSS T 6.0 6.0 Tool selection function U 8.6 8.5 Incremental axis name (Lathe A only) 5.3 5.3 Length of dwell in G04 and fixed cycles. V 8.6 8.5 Incremental axis name (Lathe A only) W 8.6 8.5 Incremental axis name (Lathe A only) X 8.6 8.5 Main axis (AMP assigned) 5.3 5.
Chapter 10 Introduction to Programming 10.5 Word Descriptions This section describes general features of the words used in programming. Later chapters in this manual describe, in detail, how to use these words. 10.5.1 A_ L_ ,R_ ,C_ (Quick Plus and Radius-Chamfer Words) To simplify programming an angle, corner radius, or chamfer between two lines, all that is necessary is the angle between the lines and the radius or chamfer size connecting them.
Chapter 10 Introduction to Programming 10.5.4 F- words (Feedrate) An F--word with numeric values specifies feedrates for the cutting tool in linear interpolation (G01), and circular interpolation (G02/G03) modes. The feedrate is the speed along a vector of the commanded axes, as shown in the following figure. Figure 10.
Chapter 10 Introduction to Programming In a metric part program for a linear axis, a feedrate of 100 millimeters per minute (mmpm) typically would be written as F100.; (depending on the active word format). For details on programming feedrates using the different feedrate modes, see chapter 18. Important: Feedrates programmed in any of the feedrate modes (G93, G94, or G95) can be overridden by use of the switch. 10.5.
Chapter 10 Introduction to Programming How the modal G-codes are executed is shown below, taking G00 and G01, both classified into the same G--code group. Example 10.9 Modal G- code Execution G00 X1. Y2.; G00 mode is effective Y3. ; G00 mode is in effect G01 X2. Y1. F1; G01 mode is made effective X3. Y3. ; G01 mode is in effect G00 X1.Y2.
Chapter 10 Introduction to Programming Table 10.E G-codes G- Code G00 Modal Group 01 Rapid Positioning G01 Linear Interpolation G02 Circular/Helical Interpolation (Clockwise) G03 Circular/Helical Interpolation (Counterclockwise) G04 00 Dwell G05 Send Command and Wait for Return Status (for 9/Series Data Highway Communication Module) G05.1-G05.
Chapter 10 Introduction to Programming G- Code G22 Modal Group 04 Function Programmable Zone 2 and 3, ON G22.1 Programmable Zone 3, ON G23 Programmable Zone 2 and 3, OFF G23.1 G24 Feed to Hard Stop Adaptive Feedrate (torque mode) G26 Adaptive Depth G27 Machine Home Return Check G28 Automatic Machine Home G29 Automatic Return From Machine Home G30 Return to Secondary Home G31 External Skip Function 1 G31.1 External Skip Function 1 G31.2 External Skip Function 2 G31.
Chapter 10 Introduction to Programming G- Code G48 Modal Group 00 Reset Acc/Dec to Default AMPed Values G48.1 Acceleration Ramp for Linear Acc/Dec Mode G48.2 Deceleration Ramp for Linear Acc/Dec Mode G48.3 Acceleration Ramp for S-- Curve Acc/Dec Mode G48.4 Deceleration Ramp for S-- Curve Acc/Dec Mode G48.5 Type Non-- Modal Programmable Jerk Value G49 08 Tool Length Offset Cancel) Modal G50.1 11 Programmable Mirror Image (Cancel) Modal G51.
Chapter 10 Introduction to Programming G- Code Modal Group Function G86 Boring Cycle (Spindle Stop, Rapid Out) G87 Back Boring Cycle G88 Boring Cycle (Spindle Stop, Manual Out) G88.1 00 Pocket Milling Roughing Cycle G88.2 Pocket Milling Finishing Cycle G88.3 Pocket Milling Roughing Cycle G88.4 Pocket Milling Finishing Cycle G88.5 Hemispherical Milling (Roughing Cycle) G88.6 Hemispherical Milling (Finishing Cycle) G89 09 Boring Cycle (With Dwell, Feed Out) G89.
Chapter 10 Introduction to Programming 10.5.6 I ,J, and K Integrand Words Integrand words are typically used to define parameters that relate to a specific axis for a canned cycle, probing cycle, or circular motion block; though not limited to use only in these operations. For example, in circular motion blocks the axis integrands are used to define the center point of the arc being cut.
Chapter 10 Introduction to Programming The basic M--codes for the control are shown in Table 10.F. A part program block may contain as many basic M--codes as desired. If more than one M--code from any modal group is programmed in the same block, the rightmost M--code in that block for that modal group is the active M--code for the block. The system installer may have defined additional M--codes in PAL. Up to four of these PAL M--codes may be activated in any one block.
Chapter 10 Introduction to Programming Table 10.F M- codes M-code Number Modal or Non-modal Group Number Function M00 NM 4 Program stop M01 NM 4 Optional program stop M02 NM 4 Program end M06 NM 4 Tool change M30 NM 4 Program end and reset (tape rewind) PRIMARY SPINDLE M03 M 7 Spindle positive rotation (cw) M04 M 7 Spindle negative rotation (ccw) M05 M 7 Spindle stop M19 M 7 Spindle orient AUXILIARY SPINDLE 2 M03.2 M 11 Spindle positive rotation (cw) M04.
Chapter 10 Introduction to Programming The following is a description of some of the basic M--codes provided with the control. (Program Stop (M00) When M00 is executed, program execution is stopped after the block containing the M00 is completed. At this time, the CRT displays the “PROG STOP” message. To restart the operation, press the {CYCLE START} button.
Chapter 10 Introduction to Programming End of Program, Tape Rewind (M30) If executing a program from control memory the M30 code acts the same as an M02, program execution is stopped and the control enters the cycle stop state. The program is reset to the first block and a will begin part program execution over again (see M99 for auto cycle start).
Chapter 10 Introduction to Programming End of Subprogram or Main Program Auto Start (M99) M99 End of Subprogram or Paramacro program When M99 is executed, subprogram execution is completed and program execution returns to the calling program. This word is not valid in an MDI command though it may be contained in a subprogram called by an MDI command. For details on programming an M99, refer to section 10.3.
Chapter 10 Introduction to Programming Synchronization with Setup (M150-M199) M150 - M199 — Synchronization with Setup (dual-process system only) This set of M-codes cancels any information already in block look ahead and re-setup the blocks before process execution is resumed. This re-setup is only essential when shared information is being changed from one process to another, as in the case of the dual processing paramacro parameters. See page 30-7.
Chapter 10 Introduction to Programming 10.5.7.1 Auxiliary Miscellaneous Function (B- word) The B--word is commonly used when the number of M--codes is not sufficient for the available number of miscellaneous functions. Any alphabetic character which is not used for other functions may be used instead of B by setting the proper AMP parameter. For details, refer to the documentation prepared by your system installer, or your AMP reference manual.
Chapter 10 Introduction to Programming L--words in a subprogram call (M98) are used to designate a repeat count for a subprogram. The number following the L--address designates the number of times a subprogram will be executed consecutively before execution is returned to the main program. 10.5.11 S- word (Spindle Speed) Program spindle speeds (in RPM) using an S--word with up to five integer digits and three decimal digits. The actual legal format is defined in AMP by the system installer.
Chapter 10 Introduction to Programming Cutting Speed The term “cutting speed” refers to the velocity of the surface of the revolving cutting tool relative to the workpiece. Cutting speeds are determined by the spindle speed in revolutions per minute (rpm) and the diameter of the cutting tool in the following equation: Metric Units English Units 3.14159 x D x N V = --------------1000 3.
Chapter 10 Introduction to Programming Figure 10.6 Cutting Speed N Cutting Speed, speed of tool surface relative to workpiece D WORKPIECE TABLE 10.5.12 T- words (Tool Selection) A workpiece usually requires different kinds of cutting processes, and usually there are cutting tools that correspond to each process. The cutting tools are typically stored in a tool magazine and are assigned tool numbers (see Figure 10.7). Figure 10.
Chapter 10 Introduction to Programming A T--address followed by a numeric value programs a tool selection. When the control executes the T--word, it outputs a tool selection signal to a tool changer. The tool changer should perform a sequence of operations to deliver the proper tool in response to the tool selection signal. For example, to select a cutting tool that is assigned tool number “03”, write “T03” in the part program. The system installer may require a M06 in the program to cause a tool change.
Chapter 10 Introduction to Programming 10-42
Chapter 11 Coordinate Systems Offsets 11.0 Chapter Overview 11.1 Machine Coordinate System (Absolute) This chapter covers the control of the coordinate systems. G-words in this chapter will be among the first programmed because they define the coordinate systems of the machine in which axis motion is programmed in. This chapter describes: Information about: On page: Machine (absolute) coordinate system 11-1 Preset work coordinate systems; G54 - G59.
Chapter 11 Coordinate System Offsets Figure 11.1 Machine Coordinate System, Home Coordinate Assignment +Y 10 Mechanically fixed Machine Home point 15 +X Machine Coordinate System zero point In Figure 11.1 the system installer has defined the zero point of the machine coordinate system by assigning the machine home point to have the coordinates Y=10 and X=15 in the machine coordinate system. Note that the coordinate values assigned to the machine home point do not affect the position of machine home.
Chapter 11 Coordinate System Offsets Important: The control must be in absolute mode (G90) when the G53 command is executed. If a G53 is executed while in incremental mode (G91), the G53 code and any axis words in the G53 block will be ignored by the control. Example 11.1 Motion in the Machine Coordinate System Program Block Comment N1G54G00X30.Y30.; axis motion in work coordinate system. N2 G53X10.Y25.; axis motion in machine coordinate system. N3 X50.Y20.; axis motion in work coordinate system.
Chapter 11 Coordinate System Offsets When cutting a workpiece using a part program made from a part drawing, it is desirable to match the zero point on the coordinate system of the part drawing with the zero point of the work coordinate system. 11.2 Preset Work Coordinate Systems (G54-59.3) As shown in the illustrations in Figure 11.
Chapter 11 Coordinate System Offsets The machine coordinate system is established by the control immediately after the machine home operation is completed. The default work coordinate system, determined in AMP by the system installer, is activated simultaneously. The default work coordinate system is established upon execution of a control reset operation, E-STOP, G92.1, or power up.
Chapter 11 Coordinate System Offsets Figure 11.5 Examples of Work Coordinate System Definition Y Y Y Y G55 G58 G56 G57 X X X X Y+3.3 X-3.1 Y+3.3 X-7.2 Y G54 Y+2.9 X+.4 Y+3.5 X+5.5 G59 Y-1.0 X-6.1 X Y Machine coordinate system zero point Y-1.0 X+4.8 X To change work coordinate systems simply specify the G--code corresponding to the desired work coordinate system in a program block.
Chapter 11 Coordinate System Offsets Figure 11.6 Results of Example 11.2 Y Y 20 10 2 X G54 Work Coordinate System X 3 10 G55 Work Coordinate System 20 11.2.1 Altering Work Coordinate Systems (G10L2) There are 4 methods to change the value of a work coordinate system zero point in the work coordinate system table. Three methods can be found in the following sections: Manually alter the work coordinate system table as described in section 3.3.
Chapter 11 Coordinate System Offsets Where : Is : L2 tells the control that you want to alter the coordinate system tables. P specifies which coordinate system (G54 through G59.3) you want to work on. P1 through P9 correspond to the work coordinate systems G54 through G59.3. P1 = G54 work coord. system P2 = G55 work coord. system P3 = G56 work coord. system P4 = G57 work coord. system P5 = G58 work coord. system X_Y_Z_ P6 = G59 work coord. system P7 = G59.1 work coord. system P8 = G59.2 work coord.
Chapter 11 Coordinate System Offsets Figure 11.7 Results of Example 11.3 Y Y Y Tool position 50 25 15 40 G54 Work coordinate system after changing table value 30 15 20 25 X X G54 Work coordinate system 20 30 40 50 X Machine coordinate system zero point 11.3 Work Coordinate System External Offset The external offset allows all work coordinate system zero points to be shifted simultaneously, relative to the machine coordinate system.
Chapter 11 Coordinate System Offsets Figure 11.8 External Offsets Y Y Y Y G56 G54 X G54 X X X Y+4.0 X-6.5 Y+3.3 X-3.1 G56 Y+4.1 X+1.1 Y+3.4 X+4.5 Work coordinate systems prior to external offset Machine coordinate system zero point Work coordinate systems after to external offset of Y.7 X-3.4 Important: Once an external offset is entered into the coordinate offset table it cannot be canceled. This offset remains active even after power has been turned off.
Chapter 11 Coordinate System Offsets 11.3.1 Altering External Offset (G10L2) There are 4 methods used to change the value of an external offset in the work coordinate system table. Three methods can be found in the following sections: Manually alter the external offset value in the work coordinate system table as described in section 3.3.1. Alter the paramacro system parameter values 5201 - 5206 as discussed in chapter 28.
Chapter 11 Coordinate System Offsets Example 11.4 Changing the External Offset Through G10 Programming Program Block Comments G10L2P1X-15.Y-10.; defines work coordinate system zero point to be at X-15, Y-10 from the machine coordinate system zero point G90; sets external offset of X-15, Y-20 moving work coordinate system zero point to be at X-30, Y-30 from the machine coordinate system zero point G10L2P0X-15.Y-20.
Chapter 11 Coordinate System Offsets 11.4 Offsetting the Work Coordinate Systems This section discusses the more temporary ways of offsetting the work coordinate systems. These offsets are activated through programming and are cancelled when an M02 or M30 is executed, a control reset is performed, or power to the control is turned off. Important: All of these offsets are global in nature. This means that they will apply to all of the work coordinate systems.
Chapter 11 Coordinate System Offsets Once the work coordinate system is offset, all absolute positioning commands in the program are executed as coordinate values in the offset coordinate system. Example 11.5 Work Coordinate System Offset (G92) Program Block Comment X25.Y35.; rapid move to X25, Y35 in the G54 work coordinate system. G92X10.Y10.
Chapter 11 Coordinate System Offsets CAUTION: G92 offsets are global. This means that changing from one coordinate system to another does not cancel the offset. Do not specify a change in coordinate systems (G54-G59.3) unless the effects of the offset have been considered. Example 11.6 shows the effect of changing work coordinate systems while the G92 offset is active. Example 11.
Chapter 11 Coordinate System Offsets Figure 11.11 Results of Example 11.6 Y Final move to Y10, X5 after G92 offset was activated in previous work coordinate system Y 30 N6 New zero point established by the G92 block Y X N7 30 N4 20 X 10 N3 10 20 30 Zero point for the G54 work coordinate system X 10 20 30 Zero point for the G55 work coordinate system In Example 11.6 and Figure 11.11, the offset entered for the G54 work coordinate system has also shifted the G55 coordinate system.
Chapter 11 Coordinate System Offsets Example 11.7 Work Coordinate System Offset By G52 Program Block Machine Coordinate Position Work Coordinate Position G01F55X25.Z25.; X25 Y25 X25 Y25 G52X10.Y10.; X25 Y25 X15 Y15 Figure 11.12 Results of Example 11.
Chapter 11 Coordinate System Offsets 11.4.3 {SET ZERO} Offset When a Set Zero operation is performed the control shifts the current work coordinate system so that the current tools position is the zero point of the coordinate system. The axis that set zero is effective in is selected through PAL (refer to system installers Documentation) or by the current jog axis if using the {FRONT PANEL} option. The Set Zero offset is similar to the execution of a G92 X0 Y0 Z0 block, with one exception.
Chapter 11 Coordinate System Offsets 11.4.4 Jogging an Offset The jog offset feature allows the operator to manually create a desired offset by jogging the axes during an automatic or MDI operation. Important: This feature will function only if the system installer has supplied a special switch and the appropriate PAL programming. See the “Jog Offsets” and “Jog-on-the-fly” PAL flags in your PAL reference manual or else refer to the documentation supplied by the system installer.
Chapter 11 Coordinate System Offsets 5. Return to Automatic or MDI mode. When the button is pressed, execution will continue from the new tool location, at the jogged offset. Important: When the jog offset move is made the axis position displays do not change on the screen (unless the currently active screen is displaying absolute position coordinates as described in section 8.1).
Chapter 11 Coordinate System Offsets Figure 11.13 Results of Example 11.9 Y Y N3 25 25 N1 15 Work coordinate system zero point after G52 offset X 10 15 25 X 10 25 Original work coordinate system zero point, and work coordinate system after G92.1 11.4.6 Canceling Selected Coordinate System Offsets (G92.2) The G92.2 command cancels the following offsets: G92 work coordinate system offset {SET ZERO} offset Jog offset It will not cancel an external offset (see section 11.
Chapter 11 Coordinate System Offsets 11.5 PAL Offsets The system installer has the option of activating, deactivating, or altering the value of the following offsets through PAL: Work coordinate systems External offset Tool length offsets (geometry and wear) Tool diameter offsets (geometry and wear) These offsets may be modified through a PAL display page created by the system installer or through some other input to PAL.
Chapter 12 Overtravels and Programmable Zones 12.0 Chapter Overview This chapter discusses overtravels and programmable zones. 12.1 Overtravels and Programmable Zones Overtravels and programmable zones define areas that restrict the movable range of the cutting tool. The control is equipped to establish two overtravel areas and two programmable zones as illustrated in Figure 12.1. Figure 12.
Chapter 12 Overtravels and Programmable Zones There are two types of overtravels. Hardware overtravels -- Established by the system installer by mounting mechanical limit switches on the movable range of the axes. Software overtravels -- Established in AMP by the system installer designating coordinate values in the machine coordinate system. There are two types of Programmable Zones. Programmable Zone 2 -- Established by the operator, or person in charge of job setup.
Chapter 12 Overtravels and Programmable Zones The coordinate values of the points defining the software overtravels are set in AMP by the system installer. This overtravel may only be disabled by the system installer in AMP. If the system installer has enabled the software overtravels the control will not be allowed to exit the area defined by the software overtravels. 12.2 Software Overtravels Figure 12.
Chapter 12 Overtravels and Programmable Zones Figure 12.3 Area Defining Software Overtravel Z Max Y value Software overtravel area as defined in AMP by min. and max.
Chapter 12 Overtravels and Programmable Zones 12.3 Programmable Zone 2 (G22, G23) Programmable zone 2 defines an area which the tool axes may not enter. Generally, zones are used to protect some vital area of the machine or part located within the software overtravels. Important: Programmable zones are defined using coordinates in the machine coordinate system. They are not affected by any changes in the work coordinate system, including external offsets.
Chapter 12 Overtravels and Programmable Zones Important: When made active the current tool location must be outside of the area defined by programmable zone 2. G22 programmable zone 2 and 3 active G23 programmable zone 2 and 3 inactive G23 is normally automatically made active at power up though this is determined by the system installer in AMP. Any zone that is activated in a program or MDI block, remains active even after a control reset, E- STOP reset, or end of program block (M02 or M30).
Chapter 12 Overtravels and Programmable Zones Programming this G-code: turns Zone 2: turns Zone 3: G22 On On G22.1 Off On G23 Off Off G23.1 No Change* Off * A G23.1 turns on programmable zone 2 if it is the default power up condition configured in AMP (also activated at a control reset). G23.1 does not turn on programmable zone 2 when it is activated in a part program. Your system installer can also turn zones on and off with PAL.
Chapter 12 Overtravels and Programmable Zones Figure 12.
Chapter 12 Overtravels and Programmable Zones Figure 12.7 Programmable Zone 3 Zero Point (Machine Coordinate System) Software overtravel Programmable Zone 3 if enabled when tool is inside of this area Programmable Zone 3 if enabled when tool is outside of this area Programmable zone 3 becomes active when either the G22 or G22.1 code is executed. It is made inactive when the G23 or G23.1 code is executed. Important: You must home your axes first before the control will enable the programmable zones.
Chapter 12 Overtravels and Programmable Zones Programming zone 3 values (3 or less axes) You can reassign values for the parameters that establish programmable zone 3 by programming axis words in a G22 program block. Two methods are available. This section discusses programming values for zone 3 when 3 or less axes have been configured on the system (this does not include any spindle).
Chapter 12 Overtravels and Programmable Zones Programming zone 3 values (4 or more axes) You can reassign values for the parameters that establish programmable zone 3 by programming axis words in a G22 program block. Two methods are available. This section discusses programming values for zone 3 when 4 or more axes have been configured on the system (this does not include any spindle).
Chapter 12 Overtravels and Programmable Zones These blocks: Results in: G22 X10 I-- 10 Y14 J-- 14 Z1 K-- 1; G22 U5 I-- 5 V13 J-- 2 W11 K10; G22 A3 I2 B7 J-- 7 C12 K11; upper and lower zone 3 limits for all 9 axes are changed. Zones 2 and 3 are both activated when the first block in this series of blocks is executed. G22 X1 Y2 Z3 U4 V5 W6 A7 B8 C9; upper zone 3 limits are changed for all 9 axes. Zones 2 and 3 are both activated.
Chapter 12 Overtravels and Programmable Zones 12.5 Resetting Overtravels The control stops tool motion during overtravel conditions. Overtravel conditions may occur from 3 causes: hardware overtravel -- the axes reach a travel limit, usually set by a limit switch or sensor mounted on the axis. Hardware overtravels are always active. software overtravel -- commands cause the axis to pass a software travel limit.
Chapter 12 Overtravels and Programmable Zones To reset a software or programmable zone overtravel condition: 1. Determine whether the control is in E-STOP. If it is not, go to step 4. 2. Look for and eliminate any other possible conditions that may have caused emergency stop, then make sure that it is safe to reset the emergency stop condition. 3. Press the button to reset the emergency stop condition. If the E-STOP does not reset it is a result of some cause other then overtravel causing E-STOP. 4.
Chapter 13 Coordinate Control This chapter describes: 13.0 Chapter Overview 13.1 Rotating the Coordinate Systems How to: On page: rotate a coordinate system 13-1 select a plane 13-11 use absolute and incremental modes 13-12 apply inch and metric measures 13-13 use scaling 13-14 The control has a feature (G68) that can rotate the work coordinate system.
Chapter 13 Coordinate Control 13.1.1 Rotating the Current Work Coordinate System (G68, G69) To rotate the current work coordinate system, program the following command. G68 X__ Y__ Z__ R__; Where : Is : X, Y, Z Specify the center of rotation using only the two axis words that are in the current active plane (G17, G18, or G19). The value entered with these axis words represent a position in the current work coordinate system.
Chapter 13 Coordinate Control Example 13.1 Rotating the Active Work Coordinate System (G68) These program blocks cause the rotation of the active work coordinate system as shown in Figure 13.2. ABSOLUTE PROGRAM INCREMENTAL PROGRAM N1 G54 G17 G00; N1 G54 G17 G90; N2 G90 X0. Y0. F500; N2 G00 X0. Y0.; /N3 G68 X10 Y10 R45; /N3 G68 X10 Y10 R45; N4 G90 G00 X5. Y5.; N4 G91 G00 X5. Y5.; N5 G01 X15. F100; N5 G01 X10 F100; N6 Y15.; N6 Y10; N7 X5.; N7 X-10; N8 Y5.
Chapter 13 Coordinate Control Note that in the preceding figure the center of rotation programmed in the G68 block is ignored when the block immediately following the G68 is an incremental motion block. Angles and centers of rotation for G68 blocks are modal and remain in effect for following G68 blocks until a new center of rotation or angle is specified with a G68 command. Important: It is possible to rotate all of the work coordinate systems at once by using the external part rotation.
Chapter 13 Coordinate Control Figure 13.3 Results of Example 13.2 Y Y X Center point for rotation in block N03 Y After executing block N03 X 30• After executing block N02 10• X After executing block N04 Rotating the work coordinate system can be helpful anytime a part has a repetitive shape. This feature combined with the G52 work coordinate system shift can reduce the size of a part program appreciably. The following program is an example of this. Example 13.
Chapter 13 Coordinate Control Figure 13.4 Results of Example 13.3 Cut during third execution of subprogram Cut during fourth execution of subprogram Center of rotation after G52 Initial center of rotation + (55, 60) + (55, 60) Cut during second execution of subprogram (40, 45) Cut during first execution of subprogram (45, 15) 13.1.2 External Part Rotation (70, 45) (65, 15) The external part rotation feature simulates a rotation of the machine coordinate system.
Chapter 13 Coordinate Control Any work coordinate system rotation that is to be done using the external rotation feature must be performed before program execution begins. Program execution may not be interrupted to perform a external part rotation. If an attempt is made to interrupt a program to perform an external part rotation the rotation will not become effective until the end of program (M02 or M30) command is read, a control reset, or E-STOP reset is performed. Figure 13.
Chapter 13 Coordinate Control Activating the External Part Rotation Feature To activate the External Part Rotation feature, follow these steps: 1. Place the control in E-STOP and press the {OFFSET} softkey. (softkey level 1) 2. PRGRAM OFFSET MACRO MANAGE PARAM QUICK CHECK FRONT PANEL SWITCH LANG ERROR PASSMESAGE WORD SYSTEM SUPORT Press the {COORD ROTATE} softkey. This will display the external part rotation parameters screen as shown below.
Chapter 13 Coordinate Control Figure 13.6 Typical External Part Rotation Parameter Screen ENTER VALUE: E-STOP MODE = [ MM ] EXTERNAL PART ROTATION PLANE [ OFF ] X Z CENTER -2.440 -2.600 VECTOR 0.000 0.000 ANGLE PROGRAMMABLE ANGLE 15.000 PART ROTATION 0.000 EXTERN ON/OFF 3. Move the cursor to the desired parameter to be changed by pressing the up, down, left, right cursor keys. The selected parameter will be shown in reverse video. 4.
Chapter 13 Coordinate Control The work coordinate systems are all rotated as soon as the external rotation feature is activated. The current work coordinate system can be changed while an External Part Rotation is active. If changed, the new work coordinate system will be rotated as described by the External Part Rotation parameters. The “PROGRAM” and “TARGET” position displays (as discussed in section 8.
Chapter 13 Coordinate Control 13.2 Plane Selection (G17, G18, G19) The control has a number of features that operate in specific planes. For that reason it is frequently necessary to change the active plane using a G17, G18, or G19. Some of the features that are plane dependant are: Circular interpolation Cutter compensation Work Coordinate system rotation Many fixed cycle operations Important: The system installer determines the planes defined by G17, G18, and G19 in AMP.
Chapter 13 Coordinate Control Important: Any axis word in a block with plane select G-codes (G17, G18, G19) causes axis motion on that axis. If no value is specified with that axis word, the control assumes a value of zero or generates an error depending on how your system is AMPed. 13.3 Absolute/Incremental Modes (G90, G91) There are two methods for programming axis positioning commands, absolute positioning and incremental positioning.
Chapter 13 Coordinate Control Figure 13.7 Incremental and Absolute Commands. Absolute command G90X10.Y20.; Incremental command G91X-25.Y10.; Y End point 20 Start point 10 X 10 13.4 Inch/Metric Modes (G20, G21) 35 The selection of a unit system (inch or metric) can be done by programming either G20 for the inch system or G21 for the metric system. These unit system G codes should be among the first blocks written in a program. Both G20 and G21 are modal, and cancel each other.
Chapter 13 Coordinate Control 13.5 Scaling Use the Scaling feature to reduce or enlarge a programmed shape. Enable this feature by programming a G14.1 block as shown below: G14.1 X__Y__Z__P__; Where : Is : X, Y, Z the axis or axes to be scaled and the center of scaling for those axes P the scaling magnification factor for the specified axes. The axes programmed in the G14.1 block determine which axes will be scaled. The corresponding axis word values specify the center of scaling for each axis.
Chapter 13 Coordinate Control Figure 13.8 Results of Example 13.5 Y 10 9 8 7 Scaled 6 Original 5 4 3 2 1 X 0 1 2 3 4 5 6 7 8 9 10 When incremental mode (G91) is active, the control ignores the programmed centers of scaling. The control performs scaling on the axes programmed in the G14.1 block, but the scaling moves are referenced from their current axis positions not the programmed center of scaling or the active coordinate zero point.
Chapter 13 Coordinate Control Figure 13.9 Results of Example 13.6 Y 10 9 8 7 Scaled 6 Original 5 4 3 2 1 X 0 1 2 3 4 5 6 7 8 9 10 G14 disables scaling on all axes. When scaling is disabled, the center of scaling and any scaling magnification factors are cleared. The next time scaling is enabled these values must be reset. In addition to G14, M99 in the main program, M02, M30, and a control reset operation will disable scaling. The system will power up with scaling disabled.
Chapter 13 Coordinate Control 13.5.1 Scaling and Axis Position Display Screens When scaling is enabled for a particular axis, the letter “P” will be displayed next to the axis name on all axis position display screens. The following screen shows scaling enabled on all axes. Figure 13.10 Axis Position Display Screen Showing Scaling Enabled E-STOP PROGRAM[ MM ] F P X 1234.567 S P Y 9876.000 T P Z 2468.000 MEMORY MAN 00 0 (ACTIVE PROGRAM NAME) STOP PRGRAM OFFSET MACRO MANAGE PARAM 13.5.
Chapter 13 Coordinate Control The scaling magnification data screen is accessed through these steps: 1. Press the {OFFSET} softkey on the main menu screen. (softkey level 1) 2. PRGRAM OFFSET MACRO MANAGE PARAM QUICK CHECK FRONT PANEL SWITCH LANG ERROR PASSMESAGE WORD SYSTEM SUPORT Press the {SCALNG} softkey to display the scaling magnification data screen. (softkey level 2) WORK TOOL CO-ORD WEAR TOOL TOOL RANDOM GEOMET MANAGE TOOL COORD BACKUP SCALNG ROTATE OFFSET Figure 13.
Chapter 13 Coordinate Control Important: If an axis is configured as a rotary axis, the scaling magnification display screen will display dashes instead of numbers for that axis. Rotary axes cannot be scaled. The left column lists the current center of scaling for each axis. When scaling is cancelled, the current center of scaling for each axis is set to zero. The format of this value is determined by the word format of the selected axis.
Chapter 13 Coordinate Control Scaling is applied to G52 and G92 offsets. The center of scaling will be shifted when the work coordinate systems are shifted by a G92 offset or by changing coordinate offset values. When using a G52 offset, the center of scaling will be adjusted to the new local coordinate system Scaling is not applied to external offsets, tool wear, tool geometry, tool radius, or tool length offsets. Scaling will not be applied to blocks containing dwells (G04), data setting codes (G10, G10.
Chapter 13 Coordinate Control Important: R uses the scale factor associated with the axis that is perpendicular to the active plane G38 G38 H__R__D__E__F__ H (scaled) R (scaled) D (scaled) E (not scaled) F (not scaled) Important: The active plane scale factors must be equal. H, R, and D use the scale factor associated with the active plane G38.1 G38.
Chapter 13 Coordinate Control G88.3, G88.4 G88.x X_Y_Z_I_J_Q_(,R or,C)_P_H_D_L_E_F_ X, Y (scaled) Z (scaled) I, J (scaled) Q (scaled) ,R ,C (scaled) P (not scaled) H (not scaled) D (scaled when scale factor is less than 1 ) (not scaled when scale factor is greater than or equal to 1) L (scaled when scale factor is less than 1 ) (not scaled when scale factor is greater than or equal 1) E (not scaled) F (not scaled) Important: The active plane scale factors must be equal.
Chapter 13 Coordinate Control Important: The active plane scale factors must be equal. R uses the scale factor associated with the active plane. L uses the scale factor associated with the axis that is perpendicular to the active plane: G89.1, G89.2 G89.
Chapter 13 Coordinate Control 13-24
Chapter 14 Axis Motion 14.0 Chapter Overview 14.1 Positioning Axes This chapter describes the group of G-words that generates axis motion or dwell data blocks.
Chapter 14 Axis Motion The system installer specifies a rapid feedrate individually for each axis in AMP. The feedrate of a positioning move that drives more than one axis is limited by the rapid rate set for the slower axis. The slower axis is driven at its rapid rate while the feedrate for other axes is reduced to maintain a linear move. This also assures that all axes start and stop at the same time. G00 is a modal command and remains in effect until cancelled by a G--code of the same group.
Chapter 14 Axis Motion 14.1.2 Linear Interpolation Mode (G01) The format for the linear interpolation mode is as follows: G01X__ Y__ Z__ F__ ; G01 establishes the linear interpolation mode. In linear interpolation mode, the cutting tool is fed along a straight line at the currently active or programmed feedrate. The axes to be moved are determined by the axis names in the G01 block. The end point of the move to be generated is determined by the values programmed with the axis names.
Chapter 14 Axis Motion Figure 14.2 Results of Linear Interpolation (G01) Example Y end point 60 Tool follows this path at a feedrate of 200 20 start point X 20 80 Once the feedrate, F, is programmed it remains effective until another feedrate is programmed (F is modal). It is possible to override programmed F--words. For information on overriding feedrates, see chapter 18. Example 14.3 Modal Feedrates Program Block Comment G91G01X10.Y20.
Chapter 14 Axis Motion G02 and G03 establish the circular interpolation mode. In G02 mode, the cutting tool moves along a clockwise arc; in G03 the tool moves along a counterclockwise arc. Figure 14.3 shows clockwise and counterclockwise orientation relative to the positive X, Y, and Z axes. 14.1.3 Circular Interpolation Mode (G02, G03) Figure 14.
Chapter 14 Axis Motion The system installer determines which axes are assigned to each plane in AMP. This manual assumes the axes are assigned to the planes as indicated below: Circular Interpolation in XY plane G17{G02} X__ Y__ {I__ J__} F__ ; G03 R__ Circular Interpolation in ZX plane G18{G02} Z__ X__ {K__ I__} F__ ; G03 R__ Circular Interpolation in YZ plane G19{G02} Y__ Z__ {J__ K__} F__ ; G03 R__ Where : Is : X, Y, Z In absolute (G90) mode, these are the coordinate values of the end-point.
Chapter 14 Axis Motion Example 14.4 Circular Interpolation Absolute Mode Incremental Mode G17; G17; G00X90Y40; G91G02X-20.Y20.J20.F200; G02X70.Y60.J20.F200; G03X-36.Y-36.J-36.; G03X34.Y24.J-36.; M30; M30; or or G17; G17; G00X90Y40; G91G02X-20.Y20.R20.F200; G90G02X70.Y60.R20.F200; G03X-36.Y-36.R36; G03X34.Y24.R36.; M30; M30; Figure 14.4 Results of Circular Interpolation Example Y Tool takes this path at a feedrate of 200. 60 R 20. Start point 40 R 36.
Chapter 14 Axis Motion Example 14.5 Arc Programmed Using + or - Radius Arc 1 center angle less than 180 degrees Arc 2 center angle greater than 180 degrees G00X15Y30; G00X15Y30; G90G02X40.Y25.R18.F200; G90G02X40.Y25.R-18.F200; M30; M30; Figure 14.5 Results of Arc Programmed Using Radius Example Y Arc 2 start point 25 R--18 R18 Arc 1 end point + X 40 If the end point of the arc is not specified, or if the end point is the same as the start point, do not use R.
Chapter 14 Axis Motion Example 14.6 Arc End Points Same As Start Points Arc 1 - Full Circle Arc 2 - No Motion G00X5.Y15; G00X5.Y15; G02X5.Y15.I5.J-5.F100; G02X5.Y15.R7.07.F100; M30; M30; Figure 14.6 Arc with End Point Equal To Start Point Arc 1 Arc 2 Full circle 0 degree center angle arc (no axis motion) Y Y start 15 15 end start end 10 10 Center defined by I and J 5 10 Control cannot determine centerpoint because R was used.
Chapter 14 Axis Motion 14.1.4 Helical Interpolation Mode (G02, G03) G02 or G03 may also be used to perform helical interpolation. Figure 14.7 shows how a part may be cut with helical interpolation. Figure 14.7 Helical Interpolation (G02, G03) (End cam) Use G02 or G03 to add a third axis to the circular interpolation command block. The direction of the helical interpolation that results depends on whether a G02 or G03 was used. Refer to Figure 14.8.
Chapter 14 Axis Motion Figure 14.8 Helical Interpolation Direction Y X G03 Z G03 G02 G02 X G17 G03 G02 Z G18 Y G19 Helical Interpolation in the XY Plane with the Z axis normal. G17{G02} X__ Y__ Z__ {I__ J__} F__ ; G03 R__ Helical Interpolation in the XZ Plane with the Y axis normal. G18{G02} X__ Z__ Y__ {I__ K__} F__ ; G03 R__ Helical Interpolation in the YZ Plane with the X axis normal.
Chapter 14 Axis Motion 14.1.5 Positioning Rotary Axes A rotary axis is a non-linear axis that typically rotates about a fixed point. A rotary axis is not the same as a spindle which uses an M19 to orient to a specific angle. A rotary axis is a fully positionable axis that is capable of interpolated motion when programmed in a block with other axes. The system installer determines which axes are rotary axes in AMP, and determines the address that is used to command those axes.
Chapter 14 Axis Motion In incremental mode (G91) the rotary axis is programmed to move an angular distance (not to a specified angle as in absolute). The maximum incremental departure depends on the programming format selected in AMP by the system installer. The sign of the angle determines the direction the rotary axis will rotate. For example if the current C axis position is 25 degrees and the following block is programmed: G91C50; the C axis would rotate 50 degrees in the positive direction.
Chapter 14 Axis Motion Determining Rotary axis feedrates The feedrate for a rotary axis is determined in much the same way as linear axes. When the control is in rapid mode (G00) the feedrate for the rotary axis is the rapid feedrate for that axis as set in AMP. Remember that if other axes are moving in the same block the feedrate for the block is limited by the axis which will take the longest time to complete its programmed move at its rapid speed (see chapter 18 for details).
Chapter 14 Axis Motion Important: Cylindrical interpolation requires that the cylindrical interpolation rotary axis rollover value be 360 degrees. This discussion assumes the following AMP axis name assignments. Refer to the literature provided by your system installer for the axis names used by your machine. Feed axis is Z Park axis is Y Linear axis is X Rotary axis is A Figure 14.9 shows a typical mill configuration for cylindrical interpolation. Figure 14.
Chapter 14 Axis Motion Cylindrical Interpolation Block Format The block used to activate cylindrical interpolation has the following format: G16.1 R__ X__ Z__ A__ F__ Where : Is : R The radius at which the feed axis (typically the Z axis) will be positioned at the start of cylindrical interpolation. Can be used to alter the feed axis depth if programmed in a G16.1 block during cylindrical interpolation.
Chapter 14 Axis Motion If an A axis position is programmed, the A axis will be rotated to the specified angle. If the A and X axes are programmed together in the same block, then a vector motion will result. around the circumference of the part. If G02 or G03 circular interpolation is made active while in G16.1 cylindrical interpolation mode, a circular cut can be made around the circumference of the part (such as the contour cut in Figure 14.9).
Chapter 14 Axis Motion Cylindrical Interpolation Operation When cylindrical interpolation is activated, the control will position the tool on the cylindrical work surface with two distinct moves. In the first move, all programmed axis moves in the initial G16.1 block (including the A axis) will be executed. At the same time, the park axis (Y) is positioned to the park axis coordinate as specified in AMP (refer to the documentation provided by your system installer).
Chapter 14 Axis Motion The angle for the A move in the G02 block above was determined using the following equation, with L = 20 and R = 100. • 360 ( L ) = ------------2 • ( R ) Where : Is : • The angle to be programmed for the A axis. L The length of the arc along the circumference of the cylinder, as required to define a legal endpoint for the arc programmed in the G02/G03 block. R The radius at which the feed axis is positioned. This is the active R value programmed in the initial G16.
Chapter 14 Axis Motion Cylindrical Interpolation Programming Restrictions When the cylindrical interpolation feature is enabled the following programming restrictions apply: Work coordinate system offsets (G52, G54--G59, and G92) for the park and feed axes (Y and Z) will be temporarily cancelled when in G16.1 mode.
Chapter 14 Axis Motion 14.2 Polar Coordinate Programming (G15, G16) Polar programming allows a programmer to use polar coordinates (using angles and distance specified with a radius) as a means of establishing the end point of a move rather then specifying the normal cartesian coordinates of the end point. G16 and G15 are modal G--codes used to start and stop polar coordinate programming respectively.
Chapter 14 Axis Motion Polar positioning is done by defining a vector using a radius and angle value. The head (or end) of the vector defined by the radius and angle values is used as the end point of a polar move. In both incremental and absolute mode the cutting tool will follow a path starting at the end point of the last move and ending at the head of the vector defined by the radius and angle. How the tool reaches that endpoint is determined by the current positioning mode (G00, G01, G02, or G03).
Chapter 14 Axis Motion If programming in absolute mode (G90): The radius is measured from the zero point of the currently active work coordinate system at the specified angle and defines a vector. This vector is independent of the current tool position. The angle is referenced from the first axis that is used to define the currently active plane and is independent of the previous move. Example 14.
Chapter 14 Axis Motion Angles may be entered in a polar block with positive or negative values. Angles are referenced counter-clockwise if specified as positive and clockwise if negative. Clockwise and counterclockwise orientation for the X, Y, and Z axes is shown in Figure 14.3. Angle values greater than 360 degrees are permitted. Programming 365 degrees or 725 degrees will have the same result as if 5 degrees were programmed. Radius values may be programmed as positive or negative values.
Chapter 14 Axis Motion When programming using polar blocks the values programmed with the axis words are stored much as if they had been position commands. Normally, programming an incremental move of Y1.3 would position the Y axis 1.3 units from its previous position. The X axis position would not change. This also holds true for polar programming. 14.2.1 Polar Programming Special Cases Programming Y20. with polar programming active specifies an angle of 20 degrees.
Chapter 14 Axis Motion It is possible to change from incremental to absolute or absolute to incremental modes during polar programming if desired. The axis word is interpreted by the control in the mode that it was specified in. Mixed combinations such as angles designated in absolute and radii designated in incremental are possible. Example 14.10 is used to illustrate this. Example 14.10 Changing Between Incremental and Absolute During Polar Moves N10G01X0Y0Z0F100; N20G16; G90X10.Y0.; G81G91Y30.Z10.R5.
Chapter 14 Axis Motion It is also possible to use polar programming when the angles are programmed in absolute mode and the radii are in incremental. See Example 14.11 and Figure 14.15. Example 14.11 Polar Programming - Angle in Absolute, Radii in Incremental N10 G00 X0Y0 F500; rapid move to X0 Y0 N20 G90 G81 X3.Y0 R3. Z10.; drilling cycle at X3 Y0 N30 G16; polar programming N40 G91 X4. G90 Y135.; radius of 4 at 135 deg abs N50 Y225.; still radius of 4 at 225 deg abs N60 Y315.
Chapter 14 Axis Motion When programming an arc using I, J, or K words the control does not use these values as polar coordinates. Program the center of the arc in the same manner as normal circular programming described in section 14.1.3 . I, J, and K are always cartesian coordinate values. Example 14.12 Circular Polar Programming G00X0.Y0.; G91G16F100; G02X20.Y20.I9.397J3.42; G15; M30; Figure 14.
Chapter 14 Axis Motion 14.3 Automatic Motion To and From Machine Home Machine tools have a fixed machine home position that is used to establish the coordinate systems. The control offers two different methods for homing a machine after power up. Manual machine home operation that uses switches or buttons on the MTB panel provided solely for this purpose. Manual homing is discussed in detail in section 4.3. Automatic machine home operation that uses a programmed machine home code. 14.3.
Chapter 14 Axis Motion Automatic Machine Homing (G28) with Distance Coded Markers The following outlines automatic machine homing (G28) for an axis with DCM feedback if the axis has not already been homed: 1. The axis moves at a speed and direction defined in AMP by G28 Home Speed and G28 Direction to Home, respectively. The axis will come to a stop once the axis crosses three consecutive markers on the DCM scale.
Chapter 14 Axis Motion Although this command moves the axes at rapid feedrate as if in G00 mode, it is not modal. If G01, G02, or G03 modes are active, they will only be temporarily canceled for the return to home moves. Only the axes specified in the G28 block are moved. For example: N1 G28 X4.0; the X axis is moved to home after moving to 4.0 N2 G28 X4.0 Y2.0; the X and Y axes are moved to home after moving to (4.0 ,2.0) Figure 14.
Chapter 14 Axis Motion Important: When the control executes a G28 or G30 block it temporarily removes any tool offsets and cutter compensation during the axis move to the intermediate point. The offsets and/or cutter compensation are automatically reactivated during the first block containing axis motion following the G28 or G30 unless that block is a G29 block.
Chapter 14 Axis Motion Figure 14.18 Automatic Return From Machine Home, Results of Example 14.13 X Machine home 200 N30 150 N30 N10 N40 N20 100 50 Y 50 100 150 200 Important: When a G29 is executed, tool offsets and/or cutter compensation will be deactivated on the way to the intermediate point and are re-activated when the axis moves from the intermediate point to the point indicated in the G29 block. 14.3.
Chapter 14 Axis Motion If an attempt is made to execute a G27 before the axes have been homed the control will go to cycle stop and the following error message will be displayed: “MACHINE HOME REQUIRED OR G28” 14.3.5 Return to Alternate Home (G30) The G30 command is similar to the G28, with the main difference being that the axis or axes move to an alternate home position instead of machine home. The command format determines whether the axes return to a second, third, or fourth alternate home position.
Chapter 14 Axis Motion If an axis included in the G30 block has not been homed, block execution will stop and the following error message will appear: “MACHINE HOME REQUIRED OR G28” Important: When the control executes a G28 or G30 block it temporarily removes any tool offsets and cutter compensation during the axis move to the intermediate point.
Chapter 14 Axis Motion 14.4.1 Dwell - Seconds In the G93 (inverse time feed) and G94 (feed per minute) modes, G04 suspends execution of the commands in the next block for a programmed length of time in seconds. G94G04 P__; X__; U__; Specify the required dwell time by either a P, X, or U word in units of seconds. It does not matter which of these three words are used, as long as only one appears in the same block. The allowable dwell time is 0.001 99999.999 seconds.
Chapter 14 Axis Motion The axis word programmed with the G51.1 command is used to define the location mirroring will be about. The defined location intercepts the programmed axis at the programmed position. If only one axis is programmed, the mirroring plane is perpendicular to that axis. If more than one axis is programmed, the mirror plane passes through these points. Important: The control only mirrors those axes that are programmed in the G51.1 block. Axes not programmed in the G51.
Chapter 14 Axis Motion Figure 14.19 Results of Programmable Mirror Image Example Y 120 90 Start point 75 End point 60 30 0 X 30 60 75 90 120 When the mirror image function is active on only one of a pair of axes used in circular interpolation or cutter compensation, the control: executes a reverse of programmed G02/G03 arcs. G02 becomes counterclockwise and G03 become clockwise. activates a reverse of programmed G41/G42 cutter compensation. G41 becomes tool right and G42 becomes tool left. 14.
Chapter 14 Axis Motion The mirrored plane is fixed and cannot be moved from the selected axis. This mirrored plane is the equivalent of programming a programmable mirror image and using all zero values for the axis words. The system installer may install a switch for each of the 4 available axes. What axes are mirrored with what switches is dependant on the PAL program in a particular system.
Chapter 14 Axis Motion 14.7 Feed to Hard Stop (G24) The feed to hard stop feature is used to position the axis of a transfer line station or the transfer bar of the station against a mechanical stop and hold it against the stop. This mechanical stop physically halts axis travel. The system installer determines the position of this hard stop based on mechanical consideration of the machine and the process currently being performed by the axis or transfer bar. Program a feed to hard stop using a G24 code.
Chapter 14 Axis Motion Moving to the Hard Stop The G24 code must be in a block that programs a position for one and only one axis. The G24 code is non-modal (G--code group 0). The active cutting mode when the G24 code is executed must be G01 (linear interpolation). Other cutting modes and rapid traverse (modal group 01), are invalid during a G24 block. Once the G24 code is executed the axis moves towards the programmed endpoint at the currently active feedrate.
Chapter 14 Axis Motion Special Considerations Feature: Consideration: Control Reset If a control reset operation is performed while the control is against a hard stop the holding torque is released and the axis is taken out of the hard stop state. Block Reset If a block reset is performed during a G24 block before the hard stop has been reached, the torque limits applied to that axis are removed and the G24 block is aborted.
Chapter 15 Using QuickPath Plus• 15.0 Chapter Overview 15.1 Using QuickPath Plus The QuickPath Plus (QPP) feature is offered as a convenient programming method to simplify programming. This method of programming can prove useful in simplifying the programming of a part directly from a part drawing.
Chapter 15 Using QuickPath Plus The angle word (,A) is always interpreted as an absolute angle regardless of the current mode (G90 or G91). The L-word is always interpreted as an incremental distance from the current position regardless of the current mode (G90 or G91). Radius or diameter mode (G08 - G09) has no effect on the ,A- or L-word.
Chapter 15 Using QuickPath Plus 15.2 Linear QuickPath Plus One- end coordinate Many times part drawings will only give a programmer one--axis dimension for a tool path and require that the other axis dimension be calculated by the angle. The following QPP feature eliminates the need for this calculation. This must be a linear block (see section 15.3 for circular).
Chapter 15 Using QuickPath Plus Figure 15.1 Results of Angle Designation Example 15.1 Y 20 165• 15 10 5 X 5 10 15 20 25 Important: An arc may also use an angle (,A) program block. This is discussed in chapter 16. No end coordinate known (L) This feature of QPP allows the programmer to define a tool path using only the start point angle and length of a tool path. This must be a linear block.
Chapter 15 Using QuickPath Plus The format for this block is as follows: ,A__ L__; Where : Is : ,A Angle - This word is always displayed as by the control even if the angle is named differently in AMP. If you have a 9/240 program that uses a different address than ,A and you want to run the program on a 9/260 or 9/290 control the angles will work but the control names them ,A. L Length - This word determines the length of the tool path.
Chapter 15 Using QuickPath Plus No Intersection Known This feature of QPP allows the programmer to define two intersecting, consecutive, linear tool paths without knowing the point that the actual intersection takes place at. Both of these blocks must be linear blocks and programmed in absolute mode. The angle of both of these lines must be known. This is done with a sequence of two linear blocks (in the current plane) in which QPP is used to calculated the end point of the first block.
Chapter 15 Using QuickPath Plus Figure 15.3 Results of Unknown Intersection From Example 15.3 Y 20 165• 15 10 5 X 5 10 15 20 25 If the control cannot determine an intersection point for the two linear paths (for example if the paths are parallel) an error will occur. 15.3 Circular QuickPath Plus (G13, G13.1) Circular QPP is used to help the programmer when a drawing does not call out the actual intersection of two consecutive tool paths and at least one of the tool paths is circular.
Chapter 15 Using QuickPath Plus Figure 15.4 G13 vs G13.1 Intersections Second block if G13.1 programmed Second block if G13 programmed 1st block 1st block When programming Circular QPP, remember: When there is only one intersection involved with the tool paths, the G13 and G13.1 codes may be programmed interchangeably, however, one must be programmed. The G13 or G13.1 code must be programmed in the first of the two blocks defining the two tool paths.
Chapter 15 Using QuickPath Plus Linear to Circular Blocks When the coordinates of the intersection of a linear path into a circular path are not known, use the following format. Note that G13 or G13.1 must be programmed. These blocks must be programmed in absolute.
Chapter 15 Using QuickPath Plus Circular to Linear Blocks When the coordinates of the intersection of a circular path into a linear path are not known, use the following format. Note that G13 or G13.1 must be programmed in the first of the two blocks. These blocks must be programmed in absolute.
Chapter 15 Using QuickPath Plus Circular to Circular Blocks When the coordinates of the point of intersection of a circular path into a circular path are not known, use the following format. Note that G13 or G13.1 must be programmed. If using this format the R word may not be used to specify the radius of an arc in either of the circular blocks. These blocks must be programmed in absolute.
Chapter 15 Using QuickPath Plus Example 15.6 Arc Into Arc Without Programming Intersection G0X0Y.; G13G03J5F100.; G02Y12X5I2J-2.75; M30; Figure 15.7 Results of Example 15.
Chapter 16 Using Chamfers and Corner Radius 16.0 Chapter Overview This describes how to use chamfer and corner radius to create corners. A chamfer is a linear transition between blocks. A corner radius is an arc transition between blocks. 16.1 Chamfers and Corner Radius For cornering you can use either a chamfer or a corner radius between two motion blocks. Both the chamfer and the corner radius features are generated between two motion blocks which must be programmed in the same plane.
Chapter 16 Using Chamfers and Corner Radius Using Chamfers Program a chamfer size following the address ,C to cut a chamfer between consecutive tool paths. The chamfer word must follow a comma (,) and is programmed in the first of two paths connected by the chamfer. The value following the ,C address is the amount of tool path cut of each programmed tool path by the chamfer. The angle that the chamfer makes with the tool paths is dependant on the size of the chamfer.
Chapter 16 Using Chamfers and Corner Radius Example 16.2 Linear-to-Circular Motions with Chamfer N10 G00 X0 Y0 F100; N20 G01 X10. Y10., C3; N30 G02 X20. Y20. R10; N40 M30; Figure 16.2 Results From Chamfer Example 16.
Chapter 16 Using Chamfers and Corner Radius Example 16.3 Programming a Radius For a Circular Path into a Linear Path N10 G00 X10. Y30; N20 X10. Y30 F100; N30 G02 X10. Y10 R10, R3; N40 G01 X30. Y10; N50 M30; Figure 16.3 Results of Radius Example 16.3 Y 30 25 N20 20 Actual end point of block N20 and start point of corner block Corner block 15 R N30 10 5 Actual start point of block N30 and end point of corner block Programmed end point of block N20 X 5 10 15 20 Example 16.
Chapter 16 Using Chamfers and Corner Radius Figure 16.4 Results of Radius Example 16.4 Y 35 30 5.0 25 180• R 5.0 20 135• 15 10 5 X 5 10 15 20 25 Guidelines for Using Chamfers and Corner Radius If the control is executing in single block mode, the control will enter the cycle stop state after executing the first block and the adjacent chamfer or corner radius.
Chapter 16 Using Chamfers and Corner Radius An error is generated if an attempt is made to change planes between blocks that are chamfer or corner radius blocks. ,C and ,R must be programmed in blocks that contain axis motion in the current plane. If they are programmed in a block that does not contain axis motion in the currently active plane, the control will generate an error.
Chapter 17 Spindles 17.0 Chapter Overview 17.1 Controlling Spindle (G12.1, G12.2, G12.3) This chapter describes how to program spindles: Information about: On page: Controlling Spindle 17-1 Spindle Orientation 17-3 Spindle Direction 17-5 Synchronized Spindles 17-6 The G12 code is used to program the active controlling spindle for features and modes requiring spindle operation. The G12 code is modal. Only one spindle may be the controlling spindle.
Chapter 17 Spindles Important: On the 9/260 and 9/290 controls, if the auxiliary spindles are programmed but have not been configured as active through AMP, these errors are given as decode errors on any blocks that have the G12.2 or G12.3 code: “SPINDLE 2 NOT CONFIGURED” and/or “SPINDLE 3 NOT CONFIGURED” Spindle Speed (S-word) Use the S-word to program the spindle speed for all configured spindles.
Chapter 17 Spindles 17.2 Spindle Orientation (M19) For each spindle configured in a system, the control is equipped to perform a spindle orient operation. This operation is used to rotate the spindle to a given angle. Typically this may be used to orient the spindle for tool positioning for special machining operations, position a mechanical chuck for automatic chuck wrench operations, etc. This orient operation is not the same as using a spindle as an axis for positioning.
Chapter 17 Spindles Refer to the system installers documentation to determine which orient the system is equipped to perform. This manual assumes that a closed loop type orient is available. If an open loop orient is the only spindle orient available on a specific system refer to the system installers documentation for details on its operation as it is highly PAL dependant. Both open- and closed-loop spindle orients can be requested either by programming the appropriate spindle orient code (M19, M19.
Chapter 17 Spindles 17.3 Spindle Direction (M03, M04, M05) Use the spindle directional M-codes to program each configured spindle program controlled spindle rotation. Table 17.B lists the spindle direction codes. Table 17.B Spindle Directional Codes Spindle Type Directional Code This means: Primary M03 M04 M05 Spindle 1 clockwise Spindle 1 counterclockwise Spindle stop Spindle 2 M03.2 M04.2 M05.2 Spindle 2 clockwise Spindle 2 counterclockwise Spindle 2 stop Spindle 3 M03.3 M04.3 M05.
Chapter 17 Spindles 17.4 Synchronized Spindles Use this feature to synchronize the position and/or velocity between two spindles with feedback using your 9/440, 9/260, or 9/290 control. Two types of synchronization are available: Velocity — synchronizes the speed between two spindles only Velocity and Position — synchronizes the speed and angular position between two spindles Prior to activation, you are responsible for selecting the proper gear ranges and ratios.
Chapter 17 Spindles 17.4.1 Using the Spindle Synchronization Feature Use these three G--codes to manipulate the spindle synchronization feature: Set spindle positional synchronization (G46)— sets the follower spindle speed/direction and relative position offset to match the controlling spindle. Set active spindle speed synchronization (G46.1)— sets the follower spindle speed/direction to match the controlling spindle.
Chapter 17 Spindles The following example assumes that the controlling and follower spindles were defined as spindle 2 and spindle 1, respectively, by your system installer. Example 17.2 Spindle Synchronization M03 S200; Spindle 1 clockwise 200 rpm M04.2 S400; Spindle 2 counterclockwise at 400 rpm G12.
Chapter 17 Spindles Deactivate Spindle Synchronization (G45) Use G45 to deactivate the synchronized spindle feature. When synchronization is deactivated, the follower spindle will remain in the same state (M03, M04, M05, or M19) and at the last programmed speed for controlling spindle until you change the program settings or if your system installer writes PAL to recommand the spindle.
Chapter 17 Spindles you are responsible for selecting proper gear ranges prior to activating synchronization. The following features cannot be used while synchronization is active: solid--tapping virtual/cylindrical programming The following features cannot be used while synchronization is ramping: threading deep--hole peck drilling Important: Virtual C and threading are available on synchronized spindles once synchronization is achieved.
Chapter 17 Spindles the example below shows what will happen when: no overlap occurs between the controlling and follower spindles’gear ranges the controlling spindle has a higher gear range than the follower spindle the controlling spindle has a lower gear range than the follower spindle Example 17.
Chapter 17 Spindles 17-12
Chapter 18 Programming Feedrates 18.0 Chapter Overview 18.1 Feedrates This chapter describes how to program feedrates and acceleration/deceleration. Use this table to find the information in this chapter: Information about: On page: Feedrates 18-1 Special AMP Assigned Feedrates 18-12 Automatic Acceleration/Deceleration 18-14 Feedrates are programmed by an F--word followed by a numeric value. Feedrates can be entered in a part program block or through MDI.
Chapter 18 Programming Feedrates Feedrates for linear and circular interpolation are “vector” feedrates. That is, all axes move simultaneously at independent feedrates so that the rate along the effective path is equal to the programmed feedrate (see Figure 18.1). Figure 18.
Chapter 18 Programming Feedrates For inside arc paths, the resulting speed of the outside surface of the tool relative to the part surface would be greater than the programmed feedrate. Since this could cause excessive tool loading and poor cutting performance, the control automatically decreases feedrate.
Chapter 18 Programming Feedrates To avoid this problem, the system installer must set a minimum feed reduction percentage (MFR) in AMP. This will set a minimum feedrate to be used whenever the value of Rc/Rp is very small. If Rc/Rp control will reduce the tool radius center feedrate no more than the MFR percentage. 18.1.2 Inverse Time Feed Mode (G93) In G93 (inverse time feed) mode, the F--word represents the amount of programmed axis or axes motion that will be completed in a minute (moves per minute).
Chapter 18 Programming Feedrates 18.1.3 Feed- Per- Minute Mode (G94) In the G94 mode (feed--per--minute), the numeric value following address F represents the distance the axis or axes move (in inches or millimeters) per minute. If the axis is a rotary axis, the F--word value represents the number of degrees the axis rotates per minute. To request a feedrate of 35.5 mm of tool motion per minute, program: G94 G21 F35.5; Figure 18.
Chapter 18 Programming Feedrates Figure 18.5 Feed Per Revolution Mode (G95) Amount of cutting tool motion per spindle revolution Cutting tool position after one spindle revolution F When changing from G93 or G94 modes to G95 mode, an F--word must be programmed in the initial G95 block. Since the G95 code is modal, it remains active until canceled by the G94 mode. It is also temporarily cancelled during execution of a G93 block.
Chapter 18 Programming Feedrates 18.1.6 Feedrate Overrides Feedrate Override Switch Feedrates programmed in any of the feedrate modes (G93/94/95) can be overridden using the feedrate override switch on the MTB panel. The feedrate override switch has a range of 0-150 percent of the active feedrate, and can alter the active feedrate in 10 percent increments. The feedrate override switch operates on the feedrate that is active.
Chapter 18 Programming Feedrates Feedrate Override Switch Disable An M49 causes the override amounts that are set by the switches on the MTB panel to be ignored by the control. With M49 active, the override switches for feedrate, rapid feedrate, and spindle speed are all set to 100 percent. They can be enabled by programming an M48 (overrides enabled). Feedhold The system installer may have written PAL to allow the activation of a feedhold state through the use of a button or switch.
Chapter 18 Programming Feedrates The maximum cutting feedrate limits the axis feedrate for any move controlled by a F--word. Feedrate override switch settings that cause the feedrate to exceed the maximum cutting feedrate will also be accordingly modified to keep the feedrate below or at the maximum cutting feedrate. When the feedrate is “clamped” to a value below the programmed feedrate the control displays a flashing C next to the current axes feedrate.
Chapter 18 Programming Feedrates Programming G25 Adaptive Feed Program a G25 block as follows: G25 X__ Y__ Z__ Q__ F__ E__; Where: Programs: X, Y, or Z Axis endpoint. Program the endpoint of the axis that is to be positioned using the adaptive feed feature. This endpoint can be programmed as either an absolute or incremental value (G90 or G91 mode). You can only program one axis in an adaptive feed block. You can not program axes that are positioned by more than one servo (dual or deskew axes).
Chapter 18 Programming Feedrates Adaptive Feed Maximum Feedrate When cutting under low to no load the servo may not be able to reach the programmed torque without exceeding your programmed F--word. In these cases, once the maximum servo feedrate is reached, the control allows the torque to drop below your programmed torque so as to not exceed the maximum programmed axis feedrate (F). The error “Adaptive Feed Max Limit” is displayed on the CRT.
Chapter 18 Programming Feedrates 18.3 Special AMP Assigned Feedrates It is possible to select special feedrates that are assigned in AMP. This covers the feedrates assigned by AMP for the single digit F--word and the External feedrate switch. It does cover the feedrate for rapid moves or for dry run. 18.3.1 Single Digit F- words Program a one-digit numeric value (1-9) following the F--code to select various preset feedrates.
Chapter 18 Programming Feedrates 18.3.2 External Feedrate Switch The system installer may install an optional external deceleration switch if desired. Typically, this is a mechanical switch mounted on the machine axes inside the hardware overtravel switches (refer to documentation prepared by the system installer for details on the application and location of this switch). When this feature is active any axis moves that are to take place at a cutting feedrate (e.g.
Chapter 18 Programming Feedrates There are three types of axis acceleration/deceleration available: 18.4 Automatic Acceleration/Deceleration (Acc/Dec) Exponential Acc/Dec Uniform or Linear Acc/Dec S--Curve Acc/Dec These are used to produce smooth starting and stopping of the machine’s axes and prevent damage to the machine resulting from harsh movements. Your system installer determines the acc/dec parameter type (exponential or linear) for some manual motion types.
Chapter 18 Programming Feedrates 18.4.1 Exponential Acc/Dec To begin and complete a smooth axis motion, the control uses an exponential function curve to automatically accelerate/decelerate an axis. The system installer sets the acceleration/deceleration time constant “T” for each axis in AMP. Figure 18.7 shows axis motion using exponential Acc/Dec. Figure 18.
Chapter 18 Programming Feedrates 18.4.2 Linear Acc/Dec Axis motion response lag can be minimized by using Linear Acc/Dec for the commanded feedrates. The system installer sets Linear Acc/Dec values for interpolation for each axis in AMP. Figure 18.8 shows axis motion using Linear Acc/Dec. Velocity Figure 18.
Chapter 18 Programming Feedrates When S--Curve Acc/Dec is enabled, the control changes the velocity profile to have an S--Curve shape during acceleration and deceleration when in Positioning or Exact Stop mode. This feature reduces the machine’s axis shock and vibration for the commanded feedrates. Figure 18.9 shows axis motion using S--Curve Acc/Dec. 18.4.3 S- Curve Acc/Dec Figure 18.
Chapter 18 Programming Feedrates 18.4.4 Programmable Acc/Dec Programmable Acc/Dec allows you to change the Linear Acc/Dec modes and values within an active part program via G47.x and G48.x codes. You cannot retrace through programmable acc/dec blocks (G47.x and G48.x). However, you can retrace through blocks where programmable acc/dec was already active. Selecting Linear Acc/Dec Modes (G47.x - - modal) Programming a G47.x in your part program allows you to switch Linear Acc/Dec modes in nonmotion blocks.
Chapter 18 Programming Feedrates Selecting Linear Acc/Dec Values (G48.n - - nonmodal) Programming a G48.x in your part program allows you to switch Linear Acc/Dec values in nonmotion blocks. Axis values in G48.n blocks will always be treated as absolute, even if the control is in incremental mode. Below is the format for calling G48 commands. Use this format with the axis names assigned by your system installer: G48.
Chapter 18 Programming Feedrates 18.4.5 Precautions on Corner Cutting When Acc/Dec is active, the control automatically performs Acc/Dec to give a smooth acceleration/deceleration for cutting tool motion. However, there are cases in which Acc/Dec can result in rounded corners on a part during cutting. In Figure 18.10 this problem is most obvious when the direction of cutting changes from the X axis to the Y axis. In this case, the X axis decelerates as it completes its move while the Y axis is at rest.
Chapter 18 Programming Feedrates Cutting Mode (G64 -- modal) G64 establishes the cutting mode. This is the normal mode for axis motion and will generally be selected by the system installer as the default mode active on power up. Block completes when the axes reach the interpolated endpoint. Cancel this code by programming G61, G62, or G63. Tapping Mode (G63 -- modal) In the G63 tapping mode, the feedrate override value is fixed at 100 percent, and a cycle stop is ignored.
Chapter 18 Programming Feedrates The system installer sets these values in AMP: angle Ap in AMP in 1 degree increments within a range of 1-90 degrees range in which the automatic corner override function is active -essentially, the values of “a” and “c” in absolute distance measured along the tool path for “b” override value in 1-percent increments within a range of 1-100 percent. To use an exact stop function while the automatic corner override mode (G62) is active, use the G09 instead of the G61.
Chapter 18 Programming Feedrates Figure 18.12 Feedrate Limited Below Programmed Feedrate to Allow Deceleration Time Programmed feedrate F100 Feedrate clamped here to allow time for deceleration F80 LINEAR Deceleration LINEAR Acceleration X5 X5.1 For normal programming, this typically causes no problem. However, in cases where a series of very short blocks exist, the limitation to the feedrate may cause finish problems as well as increased cycle time.
Chapter 18 Programming Feedrates If any of the above considerations are not met during the G36.1 mode, the control will overshoot positions, since the axis will not have time to decelerate. For example, consider the following velocity curve if a drastic change in direction is requested after the move from X5 to X5.1 when in G36.1 mode. Note that the position X5.1 is overshot, and the axis must reverse direction to reach proper position. Figure 18.
Chapter 18 Programming Feedrates G36 is the default mode and is established at power up, E--STOP reset, and end-of-program (M02, M30, or M99). The recommended method of programming G36 and G36.1 is to program a relatively long entry and exit move into/out of the mode. The entry move should be a long move in the general direction of the first short block, and at the same feedrate as the first short block. This entry move should be long enough for the axes to reach programmed speed. Program the G36.
Chapter 18 Programming Feedrates 18-26
Chapter 19 Dual-- axis Operation 19.0 Chapter Overview This chapter describes how to program a dual axis. Use this table to locate specific information about dual axis operation: Information about: On this page parking a dual axis 19-3 homing a dual axis 19-4 programming a dual axis 19-5 setting offsets for a dual axis 19-7 Important: This feature is not available on 9/230 CNCs. 19.
Chapter 19 Dual Axis Operation Figure 19.1 Dual Axis Configuration Lead screw Axis 1 Encoder Servo motor Dual Axes - two completely separate axes responding to the same programming commands. Encoder Servo motor Axis 2 Lead screw The control can support two dual axis groups. A dual axis group consists of two or more axes coupled through AMP and commanded by a master axis name.
Chapter 19 Dual Axis Operation Figure 19.2 shows the position display for a system that contains a dual axis group containing two axes with a master axis name of X. Whether or not all axes of a dual group show up on the position display is determined in PAL by the system installer. Figure 19.2 Axis Position Display for Dual X Axis E-STOP PROGRAM[ MM ] F X1 -7483.647 S Z -1955.051 T Y -5677.040 X2 -7483.647 MEMORY 00 0 (ACTIVE PROGRAM NAME) MAN PRGRAM OFFSET MACRO MANAGE PARAM 19.1.
Chapter 19 Dual Axis Operation CAUTION: Care must be taken when an axis is unparked. When an axis is unparked, any incremental positioning requests made to the dual axis group are referenced from the current location of all axes in the dual group. This includes any manual jogging or any incremental part program moves. When an axis is unparked, we recommend the next command made to the dual axis group is an absolute command to re-align the axes in the dual group to the same position.
Chapter 19 Dual Axis Operation When using automatic homing (G28), the axes must be homed one at a time. This is accomplished by parking all other axes in the dual axis group except the axis that is to be homed and requesting the AMP assigned master axis name be homed in the G28 block. Once homed, that axis should be parked, the next axis to be homed should be unparked, and the homing procedure repeated. Refer to chapter 14 for details on how to request an automatic home operation (G28).
Chapter 19 Dual Axis Operation Special consideration must be given when programming the following features: Feature: Consideration: Mirror Imaging Programmable mirror image is applied to all axes in the dual group. Manual mirror image, however, can be applied to each axis in the dual group individually. When manual mirroring is performed on selected axes in the dual group, positioning commands are in effect reversed from the programmed commands to the master axis.
Chapter 19 Dual Axis Operation 19.1.4 Offset Management for a Dual Axis Consideration should be given to offsets used for a dual axis. In most cases, each axis can have independent offset values assigned to it. This section discusses the difference in operation of a dual axis when it concerns offsets. How to activate/deactivate and enter these offset values is not discussed here unless some change specific to a dual axis occurs.
Chapter 19 Dual Axis Operation Set Zero A set zero operation may be performed on the axes in a dual group on an individual basis. For example, if you have a dual axis named X and it consists of two axes, X1 and X2, when the set zero operation is executed through PAL, you must specify which axis in the dual group to set zero. When the set zero operation is performed on an axis, the current axis location becomes the new zero point of the coordinate system.
Chapter 19 Dual Axis Operation Assigning Tool Length Offsets Manually For dual axes, extra tool length offset tables have been provided, one for each member of the dual axis group. By pressing the {NEXT SELECT} or {PREV SELECT} softkey, you can select which axis you are assigning length offset values in the dual axis group. Each member of the dual axis group is represented by the master axis name followed by a number indicating which axis in the group is active.
Chapter 19 Dual Axis Operation 19-10
Chapter 20 Tool Control Functions 20.0 Chapter Overview Tool control functions can be classified into 3 categories: Tool Selection- Programming a T--word and using random tool and tool life management to help select a tool Tool length offsets-compensate for the difference between the tool length assumed while programming, and the actual length of the tool used for cutting (see chapter 21 for details on tool diameter offsets using cutter compensation).
Chapter 20 Tool Control Functions Figure 20.1 Typical Mill Tool Magazine 06 07 08 05 09 10 04 03 02 01 A T--address followed by a numeric value programs a tool selection (or tool group number - see section 20.5 on tool life management). The system installer determines in AMP how a tool change operation is programmed. There are four different options available. They are: Return tool in M06 - When this method the T--word to activate is programmed in a block that does not contain an M06.
Chapter 20 Tool Control Functions M06 Required - This method defines that a tool is only activated in an M06 block. A T--word that is programmed by itself becomes the next tool activated at an M06 block. Programming an M06 by itself activates the next tool. If a T--word is programmed in an M06 block that T--word is used as the active tool and any other unactivated T--word is discarded. Activate Tool in T--word - For this method no M06 needs to be programmed to change tools.
Chapter 20 Tool Control Functions The control offers a function called tool length offset for offsetting tool paths. The tool length offset is usually equal to the difference between the bottom face of the tool and the gauge line. Put the tool length offset into memory in advance. This function lets the control use the same program to produce the same workpiece regardless of the length of the cutting tool. Figure 20.2 illustrates the reference points used for deriving a tool length offset. Figure 20.
Chapter 20 Tool Control Functions G44 If the sum of the tool geometry and the tool wear is a negative offset value, program G44. For example: If the values for tool offset no. 1 are: Tool Geometry -3.0000 Tool Wear +0.1000 The tool offset is: -2.9000 G49 To cancel the tool length offset function, program G49. Figure 20.
Chapter 20 Tool Control Functions Use these formats for programming G43 or G44: G43H__; G44H__; (“H” is the tool offset number.) G43 or G44 does not have to be programmed with an H--word in the same block, or vice versa, in order for a tool offset to be made active. But the tool offset will only be activated at the time both a G--word and H--word are active. Important: If using the tool life management feature, programming a H--word may not be necessary. (See section 20.
Chapter 20 Tool Control Functions Figure 20.4 Results of Example 20.1 Case 2 G43 Positive geometry offset in table Case 3 G44 Negative geometry offset in table Gauge Line Case 1 G49 No offset active Z-100 Offset “H00” in the offset table is always equal to a value of zero, but does not cancel the tool offset mode like G49. HOO cancels H--words. Programming a G49 will not change the current H--word to H00. Example 20.2 illustrates this. Example 20.
Chapter 20 Tool Control Functions 20.2.1 Activating Tool Length Offsets The system installer has the option in AMP to determine exactly when the geometry and wear offsets will take effect and when the tool position will change to the new position. This manual makes the assumption that the system is configured to immediately shift the coordinate system by the geometry and wear amounts, and delay the move that will reposition the tool to the same location in the current work coordinate system.
Chapter 20 Tool Control Functions Important: Any block that activates or deactivates a tool length offset must be programmed in linear mode (G00 or G01) when executed. If a tool change is made in the circular mode, no axis motion may take place in the block changing the tool offset. The offset must be activated in a block with no axis words. 20.2.2 Tool Length Offset (TLO) Axis Selection (G43.1, G44.
Chapter 20 Tool Control Functions To copy the offset values from one axis to another, follow these steps: 1. Press the {OFFSET} softkey. (softkey level 1) 2. PRGRAM OFFSET MACRO MANAGE PARAM PRGRAM SYSTEM CHECK SUPORT FRONT PANEL SWITCH LANG ERROR PASSMESAGE WORD Press the {TOOL WEAR} or {TOOL GEOMET} softkey, choosing the table from which you want to copy. (softkey level 2) WORK TOOL CO-ORD WEAR TOOL TOOL GEOMET MANGE RANDOM TOOL COORD BACKUP SCALNG ROTATE OFFSET 3. 4.
Chapter 20 Tool Control Functions 20.3 Random Tool The random tool feature is typically used to speed up production by saving cycle time when a tool is returned to the tool changing device. This is done by allowing the tool changer to randomly return the cutting tool to the most convenient pocket in the tool changing device. The control will remember what pocket the tool is returned to and be able to call the same tool from the new pocket at any time.
Chapter 20 Tool Control Functions Manually Entering Random Tool Data Data may be entered into the random tool table either manually, as described here, by programming, or by running a backup program of the tool data. These other methods are described later in this section. To manually enter the random tool data, follow the steps described below: 1. Press the {OFFSET} softkey. (softkey level 1) 2.
Chapter 20 Tool Control Functions Figure 20.5 Typical Random Tool Pocket Assignment Screen POCKET ASSIGNMENT TABLE PKT 001 004 007 010 013 016 019 022 025 028 031 034 037 TOOL 0002 0007 0006 PKT 002 005 008 011 014 017 020 023 026 029 032 035 038 TOOL 0003 XXXX XXXX REPLCE CLEAR VALUE VALUE PAGE 1 OF 2 PKT 003 006 009 012 015 018 021 024 027 030 033 036 039 TOOL 0001 XXXX XXXX CUSTOM ACTIVE BACKUP The columns labeled PKT give the pocket numbers of the tool changer.
Chapter 20 Tool Control Functions 4. To modify tool data there are three choices: To remove a tool assigned to a pocket press the {CLEAR VALUE} softkey. The selected tool is deleted from the table. To enter a tool number for the pocket, press the {REPLCE VALUE} softkey, key in the new tool number and press the [TRANSMIT] key. The old tool value will be replaced with the new value just keyed in.
Chapter 20 Tool Control Functions The following block is used to set data for the random tool pocket assignment table: G10.1 L20 P__ Q__ O__ R__; Where : Is : G10.1 L20 This tells the control that the block will be setting data for the random tool pocket table. The G10.1 L20 is not modal, it must be programmed in every block that sets data for the random tool pocket assignment table. P The value following the P-- word determines the pocket number that is being set.
Chapter 20 Tool Control Functions Backup Random Tool Table The control has a feature that will allow the information in the random tool table to be backed up (saved in the form of a program). This is done by the control generating a G10.1 program from the information already in the table. To do this follow these steps: 1. Press the {OFFSET} softkey. (softkey level 1) 2.
Chapter 20 Tool Control Functions Starting a program with a tool already active If desired, a part program may begin execution with a tool already active in the chuck. In order for random tool to be able to properly handle that tool, it is necessary to enter information about that tool in the random tool table. Important: If random tool was used when the tool was loaded into the chuck, it is not necessary to enter any data since random tool will remember what tool is loaded even after power is turned off.
Chapter 20 Tool Control Functions 20.4 Programming Alterations of the Offset Tables (G10L10 G10L13) It is possible to alter or generate values in the tool offset tables (see section 3.1) by using the programming feature discussed in the following section. It is possible to enter data in the offset tables by programming the correct G10 command. The following section describes the use of the G10 commands. Important: Note that G10 blocks may not be programmed when cutter compensation is active.
Chapter 20 Tool Control Functions Value for the L Parameter P Parameter Definition R, X, Y, Z L12 Geometry table Offset Number Tool radius geometry value L13 Wear table Offset Number Tool radius wear value Example 20.4 Replacing the Tool Offset Tables Through Programming (G90) Assume a Z axis geometry value (tool length) of 2 for offset number 4. N00001 G90; N00002 G10 L10 P4 Z3; Offset number 4 has a new value of 3 for tool length.
Chapter 20 Tool Control Functions 20.5.1 Tool Directory Data This section discusses how to set up the tool groups and the information that must be entered for each tool group. Note that this section discusses the manual method of entering this information. Section 20.5.3 discusses a method of entering all information into the tables by programming. Assigning Tool Numbers to Groups Normally tools that are assigned to the same group have similar characteristics (such as a boring tool or a drilling tool).
Chapter 20 Tool Control Functions 2. Distance - This is selected by choosing 2 as the type of tool life measurement. Distance measures tool life as the distance that the tool has been moved using a cutting feedrate. The value for the expected tool life is entered in units of inches or millimeters depending on the mode that the control is operating in at the time. For multi-axis moves, the vectorial distance traveled by the tool is the distance used for tool life measurement.
Chapter 20 Tool Control Functions 2. Press the {TOOL MANAGE} softkey. (softkey level 2) WORK CO-ORD TOOL WEAR TOOL TOOL RANDOM GEOMET MANAGE TOOL COORD BACKUP SCALNG ROTATE OFFSET 3. Press the {TOOL DIR} softkey. The control will display the current tool directory screen showing all of the current tools and the groups that they have been assigned to (see the following figure). The control will display the prompt “EDIT GROUP:”. (softkey level 3) TOOL DIR TOOL DATA BACKUP DATA Figure 20.
Chapter 20 Tool Control Functions At this point if it is desired to delete any or all tool groups that already exist for some reason follow these steps: To delete a select tool group press the {DELETE GROUP} softkey. Key in the desired group number to delete and press the [TRANSMIT] key. This will delete all information in the tool group including the tool offset numbers, threshold rate, tool numbers, etc.... To delete all of the tool groups press the {DELETE ALL} softkey.
Chapter 20 Tool Control Functions 5. From this screen it is possible to perform the following operations. The application of these operations was discussed in detail earlier in this section. Change Tools - Alter one of the tool numbers that has already been entered in the group. Move the cursor to the tool number to be changed by pressing the up or down cursor keys (move the cursor full pages by holding down the shift key while pressing a cursor key). Press the {CHANGE TOOL} softkey.
Chapter 20 Tool Control Functions 20.5.2 Assigning Detailed Tool Data This section assumes that tools have already been assigned to their specific groups as discussed in section 20.5.1. This section discusses specific information that is to be entered into the tool life management tables for the individual tools. This information may also be entered into the tool management tables using the programming method discussed in section 20.5.3.
Chapter 20 Tool Control Functions The following is a discussion of the units that should be entered for the different tool life measurement types: 20-26 0. Time - If tool life is measured in units of time (0 is selected as tool life type), then the units for the expected tool life is minutes. Enter the minutes of operation that the tool is expected to operate and still be within the tolerance required for the part being cut.
Chapter 20 Tool Control Functions Entering Specific Tool Data The following steps describe in detail the method of entering specific tool data for tool management. This includes tool offset numbers, and expected tool life: Important: This section assumes that the steps required to assign tools to specific groups has been performed as described in section 20.5.2. 1. Press the {OFFSET} softkey. (softkey level 1) 2.
Chapter 20 Tool Control Functions Figure 20.8 Typical Tool Data Screen GROUP 1 DATA TYPE=TIME (FILE NAME) PAGE 1 OF 1 THRESHOLD RATE = 80% TOOL T.LEN CUTTER EXPECT ACCUM TOOL NO OFF NO CMP NO LIFE LIFE STATUS 1 12 23 2 20 40 3 57 95 100 100 100 EDT LN EDT CT OFF # OFF # 5. 100 95 0 EDIT LIFE EXPIRED OLD RENEW TOOL SCROL COLOR From this screen it is possible to perform the following operations. The application of these operations was discussed in detail earlier in this section.
Chapter 20 Tool Control Functions Enter or alter the expected life of a tool - To enter or alter a value for the expected life of a tool, move the cursor to the tool number of the tool to alter and press the {EDIT LIFE} softkey. Key in the new expected life of the tool (in units as determined by the tool life type) and press the [TRANSMIT] key. The old value for expected life (if any) is discarded and the new value replaces it.
Chapter 20 Tool Control Functions Any time after the G10L3 command, parameters may be programmed to enter what tool group is being entered, the type of tool life measurement that is being used, and the tool life threshold percentage. Details on these features are discussed in section 20.5.1. The format for this block is: P__I__Q__; Where : Is : P The value entered with the P-- word is used to program what tool group number is being edited. The following blocks will assign tools to that tool group.
Chapter 20 Tool Control Functions When all of the tools for all of the different groups have been entered, end the execution of editing the tool life management table by programming either a M02 or M30 end of program blocks or by entering the following block: G11; This cancels the G10 data setting mode for tool management. Important: Any information that was previously entered for any of the tool groups is lost when the control executes the G10L3 block. Example 20.
Chapter 20 Tool Control Functions Backing up tool management tables This feature causes the control to automatically generate a G10L3 program that will store all of the information that it finds in the current tool management table. Any time that this G10 program is executed it will clear any information that is currently in the management tables and replace it with the information that is in the G10 program. To generate the G10L3 backup program of the tool management tables follow these steps: 1.
Chapter 20 Tool Control Functions 20.5.4 Programming Using Tool Management The following section discusses how to activate a tool using tool life management. Here are some considerations to keep in mind when using tool life management. The system installer sets up a boundary for T--words used with tool life management in AMP. Any T--word that is programmed less than or equal to this number will be used as a normal tool number.
Chapter 20 Tool Control Functions Example 20.7 Programming Tool Changes Using Tool Life Management The following example assumes that the system installer has configured in AMP, both, the boundary for tool life management at 100, and an M06 to perform a tool change. It also is assumed that the tool changer is located at the secondary machine home point called by a G30, this is not necessarily true for different machine applications.
Chapter 21 Cutter Diameter Compensation (G40, G41, G42) 21.0 Chapter Overview To cut a workpiece using the side face of the cutting tool, it is more convenient to write the part program so that the center of the tool moves along the shape of the workpiece. Since all cutting tools have a diameter, a program written for moving the center of the tool will not cut the workpiece to the proper size.
Chapter 21 Cutter Diameter Compensation (G40, G41, G42) We use these terms in this section: inside -- An angle between two intersecting programmed tool paths is referred to as inside if, in the direction of travel, the angle measured clockwise from the second tool path into the first is less than or equal to 180 degrees. If one or both of the moves are circular, the angle is measured from a line tangent to the tool path at their point of intersection.
Chapter 21 Cutter Diameter Compensation (G40, G41, G42) Figure 21.2 Definition of Inside and Outside workpiece Inside angle (less than 180 degrees) Outside angle (greater than 180 degrees) workpiece 21.
Chapter 21 Cutter Diameter Compensation (G40, G41, G42) Program the cutter compensation function with the following format: G41(or G42)X ___ Y ___ Z ___ D ___ ; Where : Is : G41(or G42) cutter compensation direction, G41=left, G42=right X, Y, Z End-point of entry move into cutter compensation. Program an entry move on axes only in the currently active plane. Axis motion must take place in order for cutter compensation to be active on an axis.
Chapter 21 Cutter Diameter Compensation (G40, G41, G42) Example 21.2 Cutter Compensation Sample Paths All of the following blocks result in the same tool path. Assume the selected plane is the XY plane. N1D1X0Y0; N2G41X1Y1; N3X2; M30; or N1X0Y0F500; N2G41X1Y1D1; N3X2; M30; or N1X0Y0F500; N2G41; N3X1Y1D1; N4X2 M30; Important: The cutter compensation feature is not available for any motion blocks that are programmed in MDI mode (see section 21.6.5).
Chapter 21 Cutter Diameter Compensation (G40, G41, G42) Unless Cutter Compensation is active, when a program recover is performed, the control automatically returns the program to the beginning of the block that was interrupted. In the case of power failure, the control will even reselect the program that was active prior to the interruption. Figure 21.
Chapter 21 Cutter Diameter Compensation (G40, G41, G42) N11G00G40X0Y0D00; Rapid to start point and cancel compensation N12M30; End of Program Figure 21.5 Results of Cutter Compensation Program Example Programmed path Cutting tool center path N8 N7 N6 N5 N9 N4 N10 N3 N11 N2 N1 21.2 Cutter Compensation Generated Blocks G39, G39.1 In certain instances, cutter compensation creates a non-programmed move called a generated block. These blocks are improve cycle time and corner-cutting quality.
Chapter 21 Cutter Diameter Compensation (G40, G41, G42) When is active and is cutting: which is: G41 straight line to arc (or arc to straight line) greater than 90 degrees but less than 180 degrees G42 straight line to arc (or arc to straight line) greater than 180 degrees but less than 270 degrees Figure 21.
Chapter 21 Cutter Diameter Compensation (G40, G41, G42) Besides choosing between types A and B (selected in AMP), cutter compensation generated blocks can also be controlled by programming a G39 or G39.1. These G-codes determine whether the generated block will be linear (G39) or circular (G39.1) as shown in Figure 21.7. G39(or G39.1); Where : Causes: G39 linear generated blocks. If neither G39 nor G39.1 is programmed, G39 is the default. This command is modal. G39.1 circular generated blocks.
Chapter 21 Cutter Diameter Compensation (G40, G41, G42) 21.3 Cutter Compensation (Type A) The easiest way to demonstrate the actual tool paths taken by the cutting tool when using cutter compensation type A is by pictorial representation. The following subsections give a brief description of the cutter path, along with a figure to clarify the description. 21.3.
Chapter 21 Cutter Diameter Compensation (G40, G41, G42) Figure 21.9 through Figure 21.11 show examples of typical entry moves using type A cutter compensation: Figure 21.
Chapter 21 Cutter Diameter Compensation (G40, G41, G42) If the next programmed move is circular (an arc), the tool is positioned at right angles to a tangent line drawn from the start-point of that circular move. Figure 21.
Chapter 21 Cutter Diameter Compensation (G40, G41, G42) Example 21.4 Sample Entry Move After Non-Motion Blocks Assume current compensation plane is the XY plane. N1X0Y0F500; N2G41D1; This block commands compensation left. N3Z1; This is not the entry block since no axis motion takes place in the current plane. N4...; No axis motion in current plane. N5...; No axis motion in current plane. N6...; No axis motion in current plane.
Chapter 21 Cutter Diameter Compensation (G40, G41, G42) Figure 21.11 Entry Move Followed by Too Many Non-Motion Blocks Programmed path r r Too many non-motion blocks here Cutter compensation re-initialized here G41 r r r 21.3.2 Cutter Compensation Type A Exit Moves The cutter compensation feature is cancelled by programming G40. The path that is taken when the tool leaves cutter compensation is refereed to as the exit move.
Chapter 21 Cutter Diameter Compensation (G40, G41, G42) Example 21.6 Type A Sample Exit Moves Assume the current plane to be the XY plane and cutter compensation is already active before the execution of block N100 in the following program segments. N100X1Y1; N110X3Y3G40; Exit move. N100X1Y1; N110G40; Exit move. N120X3Y3; N100X1Y1; N110G40; N120Z1; No axis motion in the current plane. N130...; No axis motion in the current plane. N140...; No axis motion in the current plane.
Chapter 21 Cutter Diameter Compensation (G40, G41, G42) Figure 21.12 through Figure 21.16 show examples of typical exit moves using type A cutter compensation. All examples assume that the number of non-motion blocks before the designation of the G40 command have not exceeded the number allowed as determined by the system installer in AMP. Figure 21.
Chapter 21 Cutter Diameter Compensation (G40, G41, G42) If the last programmed move prior to the exit move (which must be linear) is circular (an arc), the tool is positioned at right angles to a tangent line drawn from the end-point of that circular move. Figure 21.
Chapter 21 Cutter Diameter Compensation (G40, G41, G42) The I, J, and K words in the exit move block define a vector that is used by the control to redefine the end-point of the previous compensated move. I, J, and K words are always programmed as incremental values regardless of the current mode (G90 or G91).
Chapter 21 Cutter Diameter Compensation (G40, G41, G42) Figure 21.15 Exit Move Defined By An I, J, K Vector But Limited To Radius Compensated path using I, J vector Compensated path if no I, J in G40 block N11 Compensated path r Programmed path r N10 r I, J Intercept line If the vector defined by I, J, and/or K is parallel to the programmed tool path, the resulting exit move are offset in the opposite direction of the I, J, K vector by one radius of the tool. Figure 21.
Chapter 21 Cutter Diameter Compensation (G40, G41, G42) 21.4 Cutter Compensation (Type B) The easiest way to demonstrate the actual tool paths taken by the cutting tool when using cutter compensation type B is by pictorial representation. The following subsections give a brief description of the cutter path along with a figure to clarify the description. 21.4.
Chapter 21 Cutter Diameter Compensation (G40, G41, G42) Figure 21.18 and Figure 21.19 show examples of typical entry moves using type B cutter compensation: Figure 21.18 Tool Path for Entry Move Straight Line-to-Straight Line G39 (Linear Generated Blocks) 0 • • • 90 D E r D C G41 G41 r C G39.
Chapter 21 Cutter Diameter Compensation (G40, G41, G42) If the next programmed move is circular (an arc), the tool is positioned at right angles to a tangent line drawn from the start-point of that circular move. Figure 21.19 Tool Path For Entry Move Straight Line-to-Arc G39 (Linear Generated Blocks) 0 • • • 90 r r r G39.
Chapter 21 Cutter Diameter Compensation (G40, G41, G42) There is no limit to the number of blocks that may follow the programming of G41 or G42 before an entry move takes place. The entry move are always the same regardless of the number of blocks that do not program motion in the current plane for compensation. Example 21.7 Sample Entry Move After Non-Motion Blocks Assume current compensation plane is the XY plane. N01X0Y0F500; N2G41D1; This block commands compensation left.
Chapter 21 Cutter Diameter Compensation (G40, G41, G42) Figure 21.20 Entry Move Followed By Too Many Non-Motion Blocks Programmed path r r Too many non motion blocks here Cutter compensation re-initialized here G41 r r r 21.4.2 Cutter Compensation Type B Exit Moves The cutter compensation feature is cancelled by programming G40. The path that is taken when the tool leaves cutter compensation is referred to as the exit move.
Chapter 21 Cutter Diameter Compensation (G40, G41, G42) Example 21.9 gives some sample exit move program blocks: Example 21.9 Examples of Exit Move Blocks Assume the current plane to be the XY plane. N100X1Y1; N110X3Y3G40; Exit move. N100X1Y1; N110G40; N120X3Y3; Exit move. N100X1Y1; N110G40; N120Z1; No axis motion in the current plane. N130...; No axis motion in the current plane. N140...; No axis motion in the current plane. ” ” ” ” N200X3Y3; Exit move.
Chapter 21 Cutter Diameter Compensation (G40, G41, G42) Figure 21.21 and Figure 21.22 show examples of typical exit moves using type B cutter compensation. All examples assume that the number of non-motion blocks before the designation of the G40 command has not exceeded the number allowed as determined by the system installer in AMP. Figure 21.21 Tool Path For Exit Move Straight Line-to-Straight Line G39 (Linear Generated Blocks) 0 • • • 90 G39.
Chapter 21 Cutter Diameter Compensation (G40, G41, G42) If the last programmed move is circular (an arc), the tool is positioned at right angles to a tangent line drawn from the end-point of that circular move. Figure 21.22 Tool Path For Exit Move Arc-to-Straight Line G39 (Linear Generated Block) 0 • • • 90 End-point G39.
Chapter 21 Cutter Diameter Compensation (G40, G41, G42) It is possible to modify the path that the tool takes for an exit move by including an I, J, and/or K word in the exit move. Only the I, J, or K words that represent values in the current plane are programmed in the block containing the exit move. I, J, and K correspond to the X, Y, and Z axes respectively.
Chapter 21 Cutter Diameter Compensation (G40, G41, G42) Figure 21.24 Exit Move Defined By An I, J, K Vector But Limited to Tool Radius Compensated path using I, J vector Compensated path if no I, J in G40 block N11 Compensated path Programmed path r N10 r r I, J Intercept line If the vector defined by I, J, and/or K is parallel to the programmed tool path, the resulting exit move are offset in the opposite direction of the I, J, K vector by one radius of the tool. Figure 21.
Chapter 21 Cutter Diameter Compensation (G40, G41, G42) 21.5 Tool Path During Cutter Compensation Except for entry and exit moves, the basic tool paths generated during cutter compensation are the same for types A and B cutter compensation. The paths taken are a function of the angle between tool paths (whether G41 tool-left or G42 tool-right is specified) and the radius of the cutting tool.
Chapter 21 Cutter Diameter Compensation (G40, G41, G42) Figure 21.26 through Figure 21.29 illustrate the basic motion of the cutting tool as it executes program blocks during cutter compensation: Figure 21.26 Cutter Compensation Tool Paths Straight Line-to-Straight Line G39 (Linear Generated Block) r G41 • r Circular generated block G41 r Programmed path G42 G39.
Chapter 21 Cutter Diameter Compensation (G40, G41, G42) Figure 21.27 Cutter Compensation Tool Paths Straight Line-to-Arc G39.1 (Circular Generated Block) 0 • • • 90 G39 (Linear Generated Block) 0 • • • 90 Linear generated blocks r Circular generated block r r r • • r Programmed path Programmed path G41 G41 G42 90 • • • 180 G42 180 • • • 270 G41 Linear generated block r Programmed path r r r G41 G42 • r Programmed path Linear generated block G42 G39.
Chapter 21 Cutter Diameter Compensation (G40, G41, G42) Figure 21.28 Cutter Compensation Tool Paths Arc-to-Straight Line G39.
Chapter 21 Cutter Diameter Compensation (G40, G41, G42) Figure 21.29 Cutter Compensation Tool Paths Arc-to-Arc G39 (Linear Generated Block) 0 • • • 90 G39.1 (Circular Generated Block) 0 • • • 90 r r r • G41 r r r r r • G41 Programmed path Programmed path G42 G42 r r 180 • • • 270 90 • • • 180 • • r G41 Programmed path G41 Programmed path r G42 G42 G39 (Linear Generated Block) 270 • • • 360 G39.
Chapter 21 Cutter Diameter Compensation (G40, G41, G42) 21.
Chapter 21 Cutter Diameter Compensation (G40, G41, G42) Figure 21.30 Linear-to-Linear Change with Block Direction Reversed Point 1 & 2 Compensated N10 Programmed G41 N11 N13 Programmed G42 N12 Figure 21.
Chapter 21 Cutter Diameter Compensation (G40, G41, G42) Figure 21.32 Linear-to-Linear Change with A Generated Block r r r r N11 Compensated path N10 Programmed path N12 G41 G42 r r Point 2 Point 1 Figure 21.
Chapter 21 Cutter Diameter Compensation (G40, G41, G42) For one of the following cases that changes the cutter compensation direction, the control will attempt to find an intersection of the actual compensated tool paths: Linear-to-Circular, Circular-to-Linear, or Circular-to-Circular Tool Paths For the following cases that change the cutter compensation direction, the control attempts to find an intersection of the actual compensated tool paths.
Chapter 21 Cutter Diameter Compensation (G40, G41, G42) Figure 21.35 Change in Compensation with No Possible Tool Path Intersections Compensated path G41 r2 r1 r1 Programmed path G42 Programmed path r1 G41 r2 r1 Compensated path G42 Compensated path G41 r Programmed path G41 G42 r 21.6.2 Too Many Non-Motion Blocks The control is always looking ahead to the next motion block to determine the actual tool path taken for a motion block in cutter compensation.
Chapter 21 Cutter Diameter Compensation (G40, G41, G42) If the control, when scanning ahead, does not find a motion block before the number of non-motion blocks has been exceeded, it will not generate the normal cutter compensation move. Instead the control sets up the compensation move with an end-point one tool radius away from and at right angles to the programmed end-point. In many cases, this may cause unwanted over-cutting of a work piece. Figure 21.36 and Figure 21.
Chapter 21 Cutter Diameter Compensation (G40, G41, G42) Figure 21.37 Too Many Non-Motion Blocks Following a Circular Move Programmed path Programmed path Compensated path G42 Compensated path G42 r + + Too many non-motion blocks here Programmed path Compensated path G42 r r r Too many non-motion blocks here r + + Too many non-motion blocks here 21.6.
Chapter 21 Cutter Diameter Compensation (G40, G41, G42) Figure 21.38 Compensation Corner Movement for Two Generated Blocks This block is eliminated if both • X1-X1 • and • Y1-Y2 • are X1Y1 less than AMP parameter New block if block is eliminated X2Y2 + Compensated Programmed When the control generates three motion blocks, the length of the second generated block is checked against a minimum allowable length as determined in AMP by the system installer.
Chapter 21 Cutter Diameter Compensation (G40, G41, G42) If a tool becomes excessively worn, broken, or if any other reason requires the changing of the programmed tool radius, the cutter compensation should be cancelled and reinitialized after the tool has been changed. The following section describes the resulting tool path if, for some reason, it is desirable to program a change in cutter radius during cutter compensation. 21.6.
Chapter 21 Cutter Diameter Compensation (G40, G41, G42) Figure 21.41 describes the tool path when the programmed moves are linear-to-circular. Figure 21.41 Linear-to-Circular Change in Cutter Radius During Compensation No control-generated motion blocks With control-generated motion blocks Generated blocks Compensated path Compensated path r1 Programmed path r1 Programmed path r1 r2 r2 r2 + Figure 21.42 describes the tool path when the programmed moves are circular-to-circular. Figure 21.
Chapter 21 Cutter Diameter Compensation (G40, G41, G42) Change in Cutter Radius During Jog Retract This section describes a change in the cutter radius during a jog retract operation. This is a typical operation since the jog retract feature is often used when a tool becomes very worn or is broken. It may be necessary to replace the tool with a tool of a slightly different diameter. Cutter compensation is able to adjust to the new tool diameter.
Chapter 21 Cutter Diameter Compensation (G40, G41, G42) Figure 21.43 gives an example of a typical change in tool radius during jog retract with cutter compensation active. Figure 21.43 Change in Cutter Radius During a Jog Retract Programmed path . Compensated path Original tool radius . . . . . Difference in tool radius • R . . . Jog retract return moves . Tool radius changed here 21.6.5 MDI or Manual Motion During Cutter Compensation . 90• . . .
Chapter 21 Cutter Diameter Compensation (G40, G41, G42) Figure 21.44 is an example of the possible tool path that is taken when you interrupt an automatic operation during cutter compensation to execute MDI motion blocks. This same tool path applies also, if you interrupt cutter compensation to perform a manual jog move. Figure 21.
Chapter 21 Cutter Diameter Compensation (G40, G41, G42) Figure 21.45 Cutter Compensation Re-Initialized after a Manual or MDI Operation. Cutter Compensation is re-initialized here. The control assumes that the current position is a programmed position at the point of re-initialization. Consequently, after the initialization, tool compensation is offset by twice the tool radius. Manually jog axes (or any MDI execution) and return to the compensated path.
Chapter 21 Cutter Diameter Compensation (G40, G41, G42) If compensation was not cancelled using a G40 command before returning to machine or secondary home points, the control automatically re-initializes cutter compensation for the return from machine or secondary home points. This is done by using the move to the intermediate point, designated when the operation is performed, as an entry move for compensation. Figure 21.46 gives an example of either a G28 or G30 block followed by a G29 block. Figure 21.
Chapter 21 Cutter Diameter Compensation (G40, G41, G42) If compensation is not cancelled using a G40 command, the control automatically, temporarily cancels compensation for the change in work coordinate system. This is done by using the last compensated move in the current coordinate system as an exit move for compensation. The control then automatically re-initializes cutter compensation after the new work coordinate system is established.
Chapter 21 Cutter Diameter Compensation (G40, G41, G42) At times (especially possible during cutter compensation) the control may not have enough look-ahead blocks to correctly execute the current block. When this happens, the control automatically starts disabling the block retrace feature. The block retrace feature uses one set-up buffer for every retraceable block. The number of re-traceable blocks is set in AMP by the system installer (a maximum of 15 is possible).
Chapter 21 Cutter Diameter Compensation (G40, G41, G42) Figure 21.48 Typical Backwards Motion Error Compensated Path Programmed Path A D’ A’ C’ Compensated path motion opposite of programmed path B D B’ C Circular Departure Too Small This error is generated when the cutter radius is larger than the radius of the programmed arc. Note this form of compensation error cannot be disabled with an M-code. Programming this contour with tool tip radius compensation on always generates an error. Figure 21.
Chapter 21 Cutter Diameter Compensation (G40, G41, G42) Interference This error occurs when compensation vectors intersect. Normally when this intersection occurs, a backwards motion error is generated; however, a few special cases exist that are caught only by interference error detection. Figure 21.
Chapter 21 Cutter Diameter Compensation (G40, G41, G42) Error detection M--codes are only functional when cutter compensation is active. Cutter compensation is active when the control is in G41 or G42 mode and has already made the entry move into compensation. If an M800 or M801 is programmed in G40 mode or before the entry move into cutter compensation takes place, the M code is ignored.
Chapter 22 Using Pocket Milling Cycles 22.0 Chapter Overview Use pocket milling cycles to cut circular, rectangular, hemispherical pockets and posts, or irregular pockets and posts. Pocket milling cycles are cycles that make multiple passes along the X, Y, and Z axes to cut out a pocket in a workpiece. There are 8 pocket milling cycles. These include: five G88.1 Pocket Milling Roughing Cycles three G88.
Chapter 22 Using Pocket Milling Cycles 22.1.1 Rectangular Pocket Roughing Using G88.1 Use the G88.1 pocket milling roughing cycle to rough out a rectangular pocket in a workpiece. This cycle makes multiple rectangular cuts at a programmed width and depth. The G88.1 block used to rough out a rectangular pocket has this format: G88.1 X__Y__Z__I__J__(,R or,C)__P__H__D__L__E__F__; Where : Is : X Y The coordinates that specify the center of the rectangular pocket.
Chapter 22 Using Pocket Milling Cycles Where : Is : E Plunge feedrate. This parameter determines the feedrate of any Z axis moves. If not programmed, the roughing feedrate (F) will be used. F Roughing feedrate. This parameter determines the feedrate of any XY axis moves. If not programmed, the existing (modal) feedrate will be used. Important: The rectangular pocket does not have to be parallel to the axes of the selected plane. It may be rotated by rotating the work coordinate system (G68).
Chapter 22 Using Pocket Milling Cycles If L is programmed, the tool plunges along the Z axis to the incremental depth specified by the L parameter. If L is not programmed, the tool plunges along the Z axis to the pocket depth specified by the Z parameter. This move takes place at the plunge feedrate specified by the E parameter. If E is not programmed, the plunge takes place at the roughing feedrate specified by the F parameter.
Chapter 22 Using Pocket Milling Cycles If ,R or ,C is not programmed in the G88.1 block, each corner of the rectangular pocket is squared off as much as the tool radius will allow. If ,R or ,C is programmed in the G88.1 block, the corners of the rectangular pocket will either be rounded or chamfered. Refer to chapter 16, Using Chamfers and Corner Radius, for additional information on chamfers and corner rounding. 22.1.2 Rectangular Pocket Enlarging Using G88.1 Use the G88.
Chapter 22 Using Pocket Milling Cycles Figure 22.2 Rectangular Pocket Enlarging Using G88.1 Q (X, Y) Plunge Position EXISTING POCKET D D Q D H+TR Important: The tool should be positioned near the center of the original pocket prior to the G88.1 block. The Z coordinate of this position determines the initial Z level or top of the pocket. This is the pre-cycle position of the tool. The pre-cycle position must be at some depth other than the cycles programmed final depth or an error is generated.
Chapter 22 Using Pocket Milling Cycles If L is programmed, the tool plunges along the Z axis to the incremental depth specified by the L parameter. If L is not programmed, the tool plunges along the Z axis to the pocket depth specified by the Z parameter. The plunge takes place at the plunge feedrate specified by the E parameter. If E is not programmed, the plunge takes place at the roughing feedrate specified by the F parameter.
Chapter 22 Using Pocket Milling Cycles 22.1.3 Slot Roughing Using G88.1 Use the G88.1 pocket milling roughing cycle to rough out a slot in a workpiece. This cycle makes multiple cuts at a programmed length and depth. The G88.1 block used to rough out a slot has this format: G88.1 X__Y__Z__I__R__P__H__D__L__E__F__; (X axis slot) or G88.1 X__Y__Z__J__R__P__H__D__L__E__F__; (Y axis slot) Where : Is : X Y The coordinates that specify the center of the slot.
Chapter 22 Using Pocket Milling Cycles Figure 22.3 Slot Roughing Using G88.1 Y X H+TR D (X, Y) Plunge Position D/2 J D/2 R D I Important: The tool should be positioned at the center of the slot prior to the G88.1 block. The Z coordinate of this position determines the initial Z level or top of the pocket. This is the pre-cycle position of the tool. The pre-cycle position must be at some depth other than the cycles programmed final depth or an error is generated.
Chapter 22 Using Pocket Milling Cycles If L is programmed, the tool plunges along the Z axis to the incremental depth specified by the L parameter. If L is not programmed, the tool plunges along the Z axis to the pocket depth specified by the Z parameter. The plunge takes place at the plunge feedrate specified by the E parameter. After the plunge operation a roughing cut is made at the feedrate specified by the F parameter to the arc-center at the +X or +Y end of the slot.
Chapter 22 Using Pocket Milling Cycles Figure 22.4 Circular Pocket Roughing Using G88.1 Y Plunge Position X H+TR D D D/2 (X, Y) R Important: The tool should be positioned near the center of the pocket prior to the G88.1 block. The Z coordinate of this position determines the initial Z level or top of the pocket. This is the pre-cycle position of the tool. The pre-cycle position must be at some depth other than the cycles programmed final depth or an error is generated.
Chapter 22 Using Pocket Milling Cycles After completing the 360 degree circular path, the control makes a single-axis rough cut outwards along the -X axis then cuts another 360 degree circular path. This process is repeated until the sides of the pocket, less the finish allowance H, are reached. The tool is then simultaneously raised by the clearance amount and moved at rapid feedrate back to the plunge-position. This completes machining of one L level.
Chapter 22 Using Pocket Milling Cycles 22.1.5 Circular Pocket Enlarging Using G88.1 Use the G88.1 pocket milling roughing cycle to enlarge an existing circular pocket in a workpiece. This cycle makes multiple circular cuts at a programmed width and depth. The G88.1 block used to enlarge an existing circular pocket has this format: G88.1 X__Y__Z__R__Q__P__H__D__L__E__F__; Where : Is : X Y The coordinates that specify the center of the original circular pocket.
Chapter 22 Using Pocket Milling Cycles Figure 22.5 Circular Pocket Enlarging Using G88.1 Y X D D D (X, Y) R Q Plunge Position EXISTING POCKET Important: The tool should be positioned near the center of the pocket prior to the G88.1 block. The Z coordinate of this position determines the initial Z level or top of the pocket. This is the pre-cycle position of the tool. The pre-cycle position must be at some depth other than the cycles programmed final depth or an error is generated.
Chapter 22 Using Pocket Milling Cycles After completing the 360 degree circular path, the control makes a single-axis rough cut outwards along the -X axis then cuts another 360 degree circular path. This process is repeated until the sides of the pocket, less the finish allowance H, are reached. The tool is then simultaneously raised by the clearance amount and moved at rapid feedrate back to the plunge-position. This completes machining of one L level.
Chapter 22 Using Pocket Milling Cycles These features are prohibited during execution of pocket milling cycles: MDI mode Tool offset changes through the offset softkey The following subsections cover using the G88.2 finishing cycle for each of the possible pockets. 22.2.1 Rectangular Pocket Finishing Using G88.2 Use the G88.2 pocket milling finishing cycle to finish a rectangular pocket in a workpiece.
Chapter 22 Using Pocket Milling Cycles Important: The rectangular pocket does not have to be parallel to the axes of the selected plane. It may be rotated by rotating the work coordinate system (G68). Refer to chapter 13 for additional information on rotating the work coordinate system. In a finishing cycle, a smooth entry to and exit from the finish contour is accomplished by having the tool approach and leave the finish contour along a tangential arc.
Chapter 22 Using Pocket Milling Cycles From the pre-cycle position, the control simultaneously raises the tool by the clearance amount (AMP selectable, refer to the literature provided by your system installer) while moving it to the center of the rectangular pocket specified by the X and Y parameters. This simultaneous move takes place at the rapid feedrate. The control starts the finish pass by moving the tool from the pocket center to the start point of the tangential entry/exit path.
Chapter 22 Using Pocket Milling Cycles 22.2.2 Circular Pocket Finishing Using G88.2 Use the G88.2 pocket milling finishing cycle to finish a circular pocket in a workpiece. This cycle is typically used to remove the finish allowance that was left on the sides of a circular pocket during a G88.1 cycle. The G88.2 block used to finish a circular pocket has this format: G88.2 X__Y__Z__R__P__H__L__F__; Where : Is : X Y The coordinates that specify the center of the circular pocket.
Chapter 22 Using Pocket Milling Cycles Important: The tool should be positioned near the center of the pocket prior to the G88.2 block. The Z coordinate of this position determines the initial Z level or top of the pocket. This is the pre-cycle position of the tool. The pre-cycle position must be at some depth other than the cycles programmed final depth or an error is generated.
Chapter 22 Using Pocket Milling Cycles If the programmed R parameter is greater than the tool radius, this cycle is processed similar to a G88.2 finishing cycle for a rectangular pocket. The difference being that the R parameter programmed in a slot finishing cycle specifies the radius of the arc at the end of the slot verses the radius of the corners in a rectangular finishing cycle.
Chapter 22 Using Pocket Milling Cycles 22-22
Chapter 23 Using Post Milling Cycles 23.0 Chapter Overview 23.1 Post Milling Roughing Cycle (G88.3) This chapter describes how to use G88.3 and G88.4 to program post milling cycles. Use this table to find the information: Information on: On page: Rectangular Post Roughing Using G88.3 23-2 Circular Post Roughing Using G88.3 23-5 Post Milling Finishing Cycle ( G88.4) 23-7 Rectangular Post Roughing Using G88.4 23-8 Circular Post Finishing Using G88.4 23-11 Use the G88.
Chapter 23 Using Post Milling Cycles Use the G88.3 post milling roughing cycle to rough out a rectangular post in a workpiece. This cycle makes multiple cuts at a programmed width and depth. 23.1.1 Rectangular Post Roughing Using G88.3 The G88.3 block used to rough out a rectangular post has this format: G88.3 X__Y__Z__I__J__Q__(,R or,C)__P__H__D__L__E__F__; Where : Is : X Y The coordinates that specify the center of the rectangular post.
Chapter 23 Using Post Milling Cycles Figure 23.1 Rectangular Post Roughing Using G88.3 Q Q I J POST (X, Y) H + Tool Radius D Plunge Position Tool Radius Y X Important: The tool should be positioned near the center of the post prior to the G88.3 block. The Z coordinate of this position determines the initial Z level or top of the pocket. This is the pre-cycle position of the tool. The pre-cycle position must be at some depth other than the cycles programmed final depth or an error is generated.
Chapter 23 Using Post Milling Cycles If L is programmed, the tool plunges along the Z axis to the incremental depth specified by the L parameter. If L is not programmed, the tool plunges along the Z axis to the pocket depth specified by the Z parameter. This move takes place at the plunge feedrate specified by the E parameter. If E is not programmed, the plunge takes place at the roughing feedrate.
Chapter 23 Using Post Milling Cycles 23.1.2 Circular Post Roughing Using G88.3 Use the G88.3 post milling roughing cycle to rough out a circular post in a workpiece. This cycle makes multiple circular cuts at a programmed width and depth. The G88.3 block used to rough out a circular post has this format: G88.3 X__Y__Z__R__Q__P__H__D__L__E__F__; Where : Is : X Y The coordinates that specify the center of the circular post.
Chapter 23 Using Post Milling Cycles Figure 23.2 Circular Post Roughing Using G88.3 Y X R D D H+TR POST (X, Y) R Plunge Position Q Important: The tool should be positioned near the center of the post prior to the G88.3 block. The Z coordinate of this position determines the initial Z level or top of the pocket. This is the pre-cycle position of the tool. The pre-cycle position must be at some depth other than the cycles programmed final depth or an error is generated.
Chapter 23 Using Post Milling Cycles If L is programmed, the tool plunges along the Z axis to the incremental depth specified by the L parameter. If L is not programmed, the tool plunges along the Z axis to the pocket depth specified by the Z parameter. This move takes place at the plunge feedrate specified by the E parameter. If E is not programmed, the plunge takes place at the roughing feedrate.
Chapter 23 Using Post Milling Cycles Important: Tool length, work coordinates, and diameter offsets must be entered and active prior to the G88 block. The radius/diameter of the tool can not exceed the length of the shortest side of the pocket. If it does, the control enters Cycle-Stop mode and displays the error message “TOOL RADIUS TOO LARGE.
Chapter 23 Using Post Milling Cycles Where : Is : L Incremental plunge depth of each cutting pass along the Z axis. If L is programmed, a finish pass is made at each L level. If L is not programmed, only one finishing pass is made at the programmed Z depth. This is an optional parameter. It is typically programmed when a very deep pocket is being finished. F Finishing feedrate. If not programmed the existing (modal) feedrate will be used.
Chapter 23 Using Post Milling Cycles From the pre-cycle position, the control simultaneously raises the tool by the clearance amount (AMP selectable, refer to the literature provided by your system installer) while moving it to the center of the rectangular post specified by the X and Y parameters. This simultaneous move takes place at the rapid feedrate. The control starts the finish pass by moving the tool from the post center to the start point of the tangential entry/exit path.
Chapter 23 Using Post Milling Cycles 23.2.2 Circular Post Finishing Using G88.4 Use the G88.4 post milling finishing cycle to finish a circular post in a workpiece. This cycle is typically used to remove the finish allowance that was left on the sides of a circular post during a G88.3 cycle. The G88.4 block used to finish a circular post has this format: G88.4 X__Y__Z__Q__R__P__H__L__F__; Where : Is : X Y The coordinates that specify the center of the circular post.
Chapter 23 Using Post Milling Cycles Figure 23.4 Circular Post Finishing Using G88.4 Y X Q FINISH CUT POST (X, Y) r R Important: The tool should be positioned near the center of the post prior to the G88.4 block. The Z coordinate of this position determines the initial Z level or top of the pocket. This is the pre-cycle position of the tool. The pre-cycle position must be at some depth other than the cycles programmed final depth or an error is generated.
Chapter 24 Using Hemisphere Milling Cycles 24.0 Chapter Overview 24.1 Hemisphere Milling Roughing Cycle (G88.5) This chapter describes how to use G88.5 and G88.6 to program hemisphere milling cycles. Use this table to find information: Information on: On page: Hemisphere Milling Roughing Cycle (G88.5) 24-1 Concave Hemisphere Roughing Using G88.5 24-2 Convex Hemisphere Roughing Using G88.5 24-5 Hemisphere Milling Finishing Cycle 24-7 Concave Hemisphere Finishing Using G88.
Chapter 24 Using Hemisphere Milling Cycles 24.1.1 Concave Hemisphere Roughing Using G88.5 Use the G88.5 concave milling roughing cycle to rough out a concave pocket in a workpiece. This cycle makes multiple concentric circular cuts at a programmed width and depth. The G88.5 block used to rough out a concave pocket has this format: G88.5 X__Y__Z__R__Q0_P__H__D__L__E__F__; Where : Is : X Y The coordinates that specify the center of the concave hemisphere in the selected plane.
Chapter 24 Using Hemisphere Milling Cycles Figure 24.1 Concave Hemisphere Roughing Using G88.5 Y X Plunge Position D’ D D D (X, Y) R D’ INITIAL Z-LEVEL CUSP HEIGHT (L) L’ Z Important: The tool should be positioned near the center of the concave hemisphere prior to the G88.5 block. The Z coordinate of this position determines the initial Z level or top of the pocket. This is the pre-cycle position of the tool.
Chapter 24 Using Hemisphere Milling Cycles Prior to each plunge, the control computes a delta rough cut thickness, D’, and a delta plunge depth, L’. These computations are based on the cusp height (L parameter) and the hemisphere radius (R parameter) programmed in the G88.5 block, and the tool radius programmed prior to the G88.5 block. With the axis positioned at the plunge-position, a plunge along the Z axis, of depth L’is performed.
Chapter 24 Using Hemisphere Milling Cycles 24.1.2 Convex Hemisphere Roughing Using G88.5 Use the G88.5 convex milling roughing cycle to rough out a convex pocket in a workpiece. This cycle makes multiple concentric circular cuts at a programmed width and depth from the top center of the convex hemisphere to the outermost diameter of the convex hemisphere. The G88.5 block used to rough out a convex pocket has this format: G88.
Chapter 24 Using Hemisphere Milling Cycles Figure 24.2 Convex Hemisphere Roughing Using G88.5 Y X R D’ TR D D D (X, Y) INITIAL Z-LEVEL TOOL DIA D’ Z R From the pre-cycle position, the control simultaneously raises the tool by the clearance amount (AMP selectable, refer to the literature provided by your system installer) while moving it to the center of the convex hemisphere specified by the X and Y parameters. This simultaneous move takes place at the rapid feedrate.
Chapter 24 Using Hemisphere Milling Cycles With a convex hemisphere, the plunge is actually a contour move to the outward along the -X axis. This move cuts along the spherical contour, axes X and Z, at the plunge feedrate specified by the E parameter. This plunge simultaneously moves the X and Z axes by the D’and L’amounts. After the plunge, the control moves the tool in a 360 degree circular path around the plunge-position.
Chapter 24 Using Hemisphere Milling Cycles The following subsections cover using the G88.6 finishing cycle for concave or convex hemispheres. 24.2.1 Concave Hemisphere Finishing Using G88.6 Use the G88.6 concave milling finishing cycle to finish a concave pocket in a workpiece. This cycle is typically used to remove the finish allowance that was left on the sides of the concave hemisphere during the G88.5 roughing cycle. The G88.6 block used to finish a concave pocket has this format: G88.
Chapter 24 Using Hemisphere Milling Cycles Figure 24.3 Concave Hemisphere Finishing Using G88.6 Y X PRE-CYCLE POSITION (X, Y) R TR+D’ D’ L’ INITIAL Z-LEVEL R Z Important: The tool should be positioned near the center of the concave hemisphere prior to the G88.6 block. The Z coordinate of this position determines the initial Z level or top of the pocket. This is the pre-cycle position of the tool.
Chapter 24 Using Hemisphere Milling Cycles If the programmed Z depth of the pocket has not been reached, another plunge takes place simultaneously along the X and Z axes to the next L’ level. Another 360 degree circular path is cut. This process is repeated until the programmed Z depth of the concave hemisphere is reached, at which time the tool is moved at rapid feedrate along the Z axis back to the initial Z level. The tool is then moved at rapid feedrate along the X and Y axes to its pre-cycle position.
Chapter 24 Using Hemisphere Milling Cycles Figure 24.4 Convex Hemisphere Finishing Using G88.6 PLUNGING AXIS D’ L’ TOOL DIA, CUSP CUSP HEIGHT L R Important: The tool should be positioned near the center of the convex hemisphere prior to the G88.6 block. The Z coordinate of this position determines the initial Z level or top of the pocket. This is the pre-cycle position of the tool.
Chapter 24 Using Hemisphere Milling Cycles If the programmed Z depth of the pocket has not been reached, another plunge takes place simultaneously along the X and Z axes to the next L’ level. This plunge simultaneously moves the X and Z axes by the D’and L’amounts. This level is then finished as described in the previous paragraphs.
Chapter 25 Irregular Pocket Milling Cycles 25.0 Chapter Overview Important: The Irregular Pocket Milling Cycles feature (G89.1 and G89.2) is only available prior to release 12.xx. Any attempt to program a G89.1 or G89.2 in release 12.xx or later will result in the error message, “Illegal G--code”. This chapter describes how to use G89.1 and G89.2 to program irregular pocket milling cycles. Use this table to find information: 25.
Chapter 25 Irregular Pocket Milling Cycles 25.1.1 Irregular Pocket Roughing (G89.1) Use the irregular pocket milling roughing cycle (G89.1) to rough out an irregular pocket in a workpiece. This cycle makes multiple cuts at a programmed depth, one cutter radius in width. The G89.1 block used to rough out an irregular pocket has this format: G89.1 X__Y__Z__P__Q__H__E__F__L__; Where : Is : X Y The coordinates that specify the start/end corner of the irregular pocket in the selected plane.
Chapter 25 Irregular Pocket Milling Cycles Prior to the G89.1 block, the tool should be positioned near the start/end corner of the pocket and should be just above but not touching the part. This position is referred to as the start-point of the cycle (A in figure 16.16). From the start-point the cutter must be able to move down into the part and then directly over to the start/end corner of the pocket without cutting into any wall of the pocket.
Chapter 25 Irregular Pocket Milling Cycles Figure 25.1 Irregular Pocket Roughing Cycle Entry Moves TOP VIEW End wall (defined in block called out by Q parameter) Start-point A/B C Start wall (defined in block called out by P parameter) Y H D Start/end corner X H A Initial Z level (top of pocket) L C B D SIDE VIEW Z (incremental) c Z X b d Z (absolute) From the final cutter position of Figure 25.
Chapter 25 Irregular Pocket Milling Cycles These two passes cut a channel around the inside perimeter of the pocket that provides clearance for the cutter to be raised and lowered as necessary at the beginning and end of the rest of the roughing passes. While cutting this channel, the control automatically adjusts the roughing feedrate so that the volume of material being removed per unit time is the same as will be removed later during normal roughing passes. Figure 25.
Chapter 25 Irregular Pocket Milling Cycles Figure 25.3 Roughing-Out Adjacent Areas in an Irregular Pocket Q N TOP VIEW R Y X U/W V O P S Y X Z T H Start/end corner If there is no undone area within one cutter radius of the current cutter position, the control raises the cutter to the initial Z level (point O in figure 16.19).
Chapter 25 Irregular Pocket Milling Cycles Figure 25.4 Roughing-Out Non-Adjacent Areas in an Irregular Pocket S V W N/O TOP VIEW P/Q/R No undone cutting to do in this area X T U Y H Start/end corner X H O P Initial Z level (top of pocket) Q N e SIDE VIEW R L T U X Z (incremental) Y Z (absolute) X Once the current plunge-level has been machined-out , the cutter is moved back to the start-point. The control raises cutter to the initial Z level then moves it to the start-point.
Chapter 25 Irregular Pocket Milling Cycles Once the programmed depth is reached, the control raises the cutter to the initial Z level then moves it to the start-point. This completes the irregular pocket roughing cycle. Example 26.1 shows an irregular pocket roughing cycle. Example 26.1 Irregular Pocket Roughing Cycle Program Block N46 G92 X1 Y-1 Z0; N47 G10 L12 P1 R.125; N48 G90 G42 D1; N49 G89.1 X3 Y-2 Z-1 P50 Q57 H.01 E5 F100 L.
Chapter 25 Irregular Pocket Milling Cycles Figure 25.5 Results of Example 26.1 Y 2 TOP VIEW End wall (defined in block called out by Q parameter) 0 Start-point A/B C Start wall (defined in block called out by P parameter) D 0.01 (H) -2 Start/end corner -6 -3 0 X 3 0.01 (H) A Initial Z level (top of pocket) SIDE VIEW C B D C B D C B D C B D 0.
Chapter 25 Irregular Pocket Milling Cycles 25.1.2 Irregular Pocket Finishing (G89.2) Use the irregular pocket milling finishing cycle (G89.2) to finish an irregular pocket in a workpiece. This cycle is typically used to finish an irregular pocket formed using a G89.1 irregular pocket roughing cycle. A tool change is usually performed between the G89.1 and G89.2 cycles. You can use this cycle to finish a post that was formed by combining two pocket cycles. The G89.2 block has this format: G89.
Chapter 25 Irregular Pocket Milling Cycles Before invoking the G89.2 cycle, the programmer must activate cutter compensation left or right by programming G41 or G42. This allows the control to begin interpreting the blocks that define the contour of the pocket as they are encountered. CAUTION: From the start-point the cutter must be able to move down into the part and then directly over to the start/end corner of the pocket (A through D in Figure 25.6) without cutting into any wall of the pocket.
Chapter 25 Irregular Pocket Milling Cycles Figure 25.6 Irregular Pocket Finishing Cycle Entry Moves TOP VIEW End wall (defined in block called out by Q parameter) Start-point A/B C Start wall (defined in block called out by P parameter Y Will leave H finish allowance if programmed in the G89.2 block D Start/end corner X H A Initial Z level (top of pocket) C B L D e SIDE VIEW Z (incremental) c Z b d Z (absolute) X If H is programmed in the G89.
Chapter 25 Irregular Pocket Milling Cycles The finish pass ends at a point along the start-wall that is determined by the angle formed by the start-wall and a line drawn from the endpoint of the start-wall to the start-point. An example of this is shown in the following figure. From this point the cutter is moved back to the start-point of the cycle. Figure 25.7 Irregular Pocket Finishing Cycle Exit Moves TOP F G VIEW Will leave H finish allowance if programmed in the G89.
Chapter 25 Irregular Pocket Milling Cycles CAUTION: The cutter must be able to move from the end-point of the P block to the start-point (I through K in Figure 25.7) without cutting into any wall of the pocket. If the programmed Z depth of the pocket has not been reached, another plunge along the Z axis to the next L level takes place. This level is then finished as described in the previous paragraphs. This process is repeated until the programmed Z depth is reached.
Chapter 26 Milling Fixed Cycles 26.0 Chapter Overview This chapter covers the G-word data blocks in the milling fixed-cycle group.
Chapter 26 Milling Fixed Cycles Milling fixed cycles (sometimes referred to as canned cycles or autocycles cycles) repeat a series of basic machining operations, such as, boring, drilling or tapping. These operations, designated by a single block command, usually consist of a fixed series of steps that are dependent on the type of machining application. 26.1 Milling Fixed Cycles The control provides the milling fixed cycles shown in Table 26.A. Table 26.
Chapter 26 Milling Fixed Cycles In general, milling fixed cycles consist of the following operations (see Figure 26.1): Figure 26.
Chapter 26 Milling Fixed Cycles 26.2 Positioning and Hole Machining Axes This section assumes that the programmer can determine the hole machining axis using the plane select G--codes (G17, G18, and G19). Refer to the system installer’s documentation to make sure that a specific axis has not been selected in AMP to be the hole machining axis. G--codes, G17, G18 or G19, determine the plane, the positioning axes and the hole machining axis.
Chapter 26 Milling Fixed Cycles The plane selection codes (G17-G19) can be included in the milling fixed cycle block, or can be programmed in a previous block. Figure 26.2 shows typical milling fixed cycle motions in absolute (G90) or incremental (G91) modes. Note the changes in how the R point and Z level are referenced. Figure 26.
Chapter 26 Milling Fixed Cycles Figure 26.3 shows the two different modes available for selecting the return level in the Z axis after the hole has been drilled. These two modes are selected with G98 (which returns to the same level the cycle started at) and G99 (which returns to the level defined by the R point). Figure 26.
Chapter 26 Milling Fixed Cycles The following section provides a detailed explanation of each parameter that can be programmed for the milling fixed cycles. Some of these parameters are not valid with all cycles. Refer to the specific description of each cycle in section 26.4. To alter milling cycle operation parameters, refer to section 26.5. 26.3 Parameters We describe these milling fixed-cycle parameters below.
Chapter 26 Milling Fixed Cycles Important: After programming a milling fixed cycle block, parameters X, Y, Z and R can be programmed in later blocks with different values. This, of course, permits axis motion to be changed. Parameters Q, P, I and K can only be programmed in the calling block for the milling fixed cycle. They cannot be programmed following the calling block. If they are, the control will ignore them. 26.
Chapter 26 Milling Fixed Cycles (G73): Deep Hole Peck Drilling Cycle with Dwell The format for the G73 cycle is as follows: G73X__Y__Z__R__Q__P__F__L__; Where : Is : X,Y specifies the location of the hole position in the selected plane. Z defines the hole bottom. R defines the R point level. Q defines the infeed amount for each step into the hole. P defines the dwell period at hole bottom. F defines the cutting feedrate. L defines the number of times the milling fixed cycle is repeated.
Chapter 26 Milling Fixed Cycles 4. If a value was programmed for the P parameter, the drilling tool will dwell after it reaches the bottom of the hole. 5. It then retracts by an amount d at a rapid feedrate. The amount d is specified by the system installer, or can be set by the operator as described in section 26.5. This intermittent feed simplifies chip disposal and lets a small retraction amount to be set in peck drilling. 6.
Chapter 26 Milling Fixed Cycles Important: When programming a G74 tapping cycle, consider this: The programmer or operator must start spindle rotation. Override usage- the control ignores the feedrate override switch and clamps override at 100 percent. During tapping the feedrate override switch, and the feedhold feature are both disabled. Cycle stop is not acknowledged until the end of the return operation. Figure 26.
Chapter 26 Milling Fixed Cycles 4. If a value was programmed for the P parameter, the threading tool dwells after it reaches the bottom of the hole, and after the spindle has been commanded to reverse. The spindle reverses to the clockwise direction. 5. The threading tool retracts at the cutting feedrate to the R point. 6. If a value was programmed for the P parameter, the threading tool will dwell after it reaches the R point. (Dwells may be ignored if the system installer has chosen to do so in AMP.
Chapter 26 Milling Fixed Cycles Where : Is : X specifies location of the hole. Z defines the hole bottom. R defines the R point level. F represents the thread lead along the drilling axis (Z in this manual). It is mandatory and modal in any subsequent solid tapping cycle blocks until a new F-word is programmed. The control interprets the F-word as the thread lead in inches per revolution or millimeters per revolution, depending on the inch/metric mode active.
Chapter 26 Milling Fixed Cycles to re-tap a hole, a Q-word must have been programmed when the hole was originally tapped block retrace is possible during the tap-in portion of the cycle, but not during the tap-out Figure 26.6 G74.1: Left-Hand Solid-Tapping Cycle Tapping feed 7 Rapid feed initial point level 1 2 6 6 R R point level 3 4 Z Hole bottom 5 5 G98 G99 Spindle rotation direction is reversed at hole bottom In the G74.
Chapter 26 Milling Fixed Cycles 5. Tap-out: The spindle and linear motion reverse to the clockwise direction and retract to the R point. The tap-out speed is determined by F * S unless you programmed D (tap-out rpm), in which case tap-out speed is F * D. At the R point, spindle rotation has ramped to zero. 6. With G98 active, the cutting tool then accelerates to the rapid feedrate and retracts to the initial point level. With G99 active, the cutting tool remains at R point; no movement occurs.
Chapter 26 Milling Fixed Cycles Figure 26.7 G76: Boring Cycle, Spindle Shift Cutting feed Rapid feed 8 Initial point level 7 1 2 R point level 6 3 Hole bottom Shift Spindle orient after dwell at Z point level to position tool for removal Q Q 4 5 Spindle orientation after shift Shift Shift In the G76 boring cycle, the control moves the axes in this manner: 1. The tool rapids to the initial point level above the hole location. 2.
Chapter 26 Milling Fixed Cycles Method I This shift method is a single axis shift. The direction and axis for the shift is set in AMP by the system installer or can be altered using the milling fixed cycle parameter table (see section 26.6). The direction of the axis is specified as + or -. The feedrate using this shift method is always rapid traverse. The Q--word shift amount is always interpreted as a positive value. A negative Q--word is not allowed.
Chapter 26 Milling Fixed Cycles (G80): Cancel or End Fixed Cycles The format for the G80 cancel or end fixed cycles is as follows: G80; Programming a G80 cancels the currently active milling fixed cycle mode. (G00, G01, G02, or G03 will also cancel any active milling fixed cycle.) If milling fixed cycles are canceled with a G80, program execution returns to the mode which was in effect when the cycles were last turned on, for example, G00 - G03.
Chapter 26 Milling Fixed Cycles Figure 26.8 G81: Drilling Cycle without Dwell Cutting feed Rapid feed 1 initial point level 2 R R point level 4 Z 3 Hole bottom In the G81 drilling cycle, the control moves the axes in the following manner: 1. The tool rapids to the initial point level above the hole location. 2. The drilling tool then rapids to the R point level, slows to the programmed cutting feedrate and begins the drilling operation. 3.
Chapter 26 Milling Fixed Cycles (G82): Drill Cycle, Dwell/Rapid Out The format for the G82 cycle is as follows: G82X__Y__Z__R__P__F__L__; Where : Is : X,Y specifies location of the hole. Z defines the hole bottom. R defines the R point level. P defines the dwell period at hole bottom. F defines the cutting feedrate. L defines the number of times the milling fixed cycle is repeated. (See section 26.3 for a detailed explanation of these parameters.
Chapter 26 Milling Fixed Cycles In the G82 drilling cycle, the control moves the axes in the following manner: 1. The tool rapids to initial point level point above the hole location. 2. The drilling tool then rapids to the R point level, slows to the programmed cutting feedrate and begins the drill operation. 3. The cutting tool drills at the programmed feedrate to the pre-programmed depth of the hole (defined by the Z--word in the boring cycle block). 4.
Chapter 26 Milling Fixed Cycles Figure 26.10 G83: Deep Hole Drilling Cycle 1 initial point level 2 R 5 R point level Q 4 d 3 7 Q 6 d Q d Moves to hole bottom when Q is larger than remaining depth Hole bottom In the G83 drilling cycle, the control moves the axes in the following manner: 26-22 1. The tool rapids to initial point level above the hole location. 2.
Chapter 26 Milling Fixed Cycles 7. The cutting tool is then retracted at a rapid feedrate to the initial point level as determined by G98. When the single block function is active, the control stops axis motion after steps 1, 2 and 7. (G84): Right-Hand Tapping Cycle This cycle is used to cut right-handed threads. The format for the G84 cycle is as follows: G84X__Y__Z__R__P__F__L__; Where : Is : X,Y specifies location of the hole. Z defines the hole bottom. R defines the R point level.
Chapter 26 Milling Fixed Cycles Figure 26.11 G84: Right-Hand Tapping Cycle Cutting feed Rapid feed 1 7 initial point level R 2 R point level Spindle rotation in the forward direction 6 3 Z 5 Hole bottom 4 Spindle rotation direction reversed at hole bottom In the G84 right-hand tapping cycle, the control moves the axes in the following manner: 1. The tool rapids to initial point level above the hole location. 2.
Chapter 26 Milling Fixed Cycles When the single block function is active, the control stops axis motion after steps 1, 2 and 6. If the operator activates a feedhold during steps 3, 4 or 5, axis motion stops after step 7. Axis motion will also stop during steps 1, 2, and 7. However, if the operator activates a feedhold during step 7, axis motion will stop immediately. Important: Your system installer can enable a tap retract feature for this cycle through PAL.
Chapter 26 Milling Fixed Cycles the spindle speed that is active at the start of the cycle determines the effective Z feedrate the direction of spindle rotation for tap-in and tap-out phases will be automatically generated by the control spindle speed override has no effect on the solid tapping cycle; you can use feedrate override to adjust the tapping operation D cannot exceed the maximum tapping spindle speed set in AMP you cannot select tools via D-word while in solid tapping mode gear changes are locke
Chapter 26 Milling Fixed Cycles In the G84.1 right-hand solid-tapping cycle, the control moves the axes in this manner: 1. The tool rapids to the tapping position above the hole location. 2. The threading tool then rapids to the R point. 3. The control either orients or stops the spindle. If a Q-word was programmed: the control: yes orients the spindle no stops the spindle 4.
Chapter 26 Milling Fixed Cycles (G85): Boring Cycle, No Dwell/Feed Out The format for the G85 cycle is as follows: G85X__Y__Z__R__F__L__; Where : Is : X,Y specifies location of the hole. Z defines the hole bottom. R defines the R point level. F defines the cutting feedrate. L defines the number of times the milling fixed cycle is repeated. (See section 26.3 for a detailed description of these parameters.) Important: The programmer or operator must start spindle rotation. Figure 26.
Chapter 26 Milling Fixed Cycles 4. The control retracts the boring tool at the cutting feedrate to the R point. 5. The control retracts the drilling tool at a rapid feedrate to the initial point level, as determined by G98. When the single block function is active, the control stops axis motion after steps 1, 2 and 5.
Chapter 26 Milling Fixed Cycles (G86): Boring Cycle, Spindle Stop/Rapid Out The format for the G86 cycle is as follows: G86X__Y__Z__R__P__F__L__; Where : Is : X,Y specifies location of the hole. Z defines the hole bottom. R defines the R point level. P defines the dwell period at hole bottom. F defines the cutting feedrate. L defines the number of times the milling fixed cycle is repeated. (See section 26.3 for a detailed description of these parameters.
Chapter 26 Milling Fixed Cycles In the G86 milling fixed cycle, the control moves the axis in the following manner: 1. The tool rapids to the initial point level above the hole location. 2. The cutting tool then rapids to the R point level, slows to the programmed cutting feedrate and begins the boring operation. 3. The cutting tool bores at the programmed feedrate until it reaches the depth of the hole as programmed with the Z--word. 4.
Chapter 26 Milling Fixed Cycles (G87): Back Boring Cycle The format for the G87 back boring cycle is: G87X__Y__Z__{I__J__K__}R__F__L__; Q__ Where : Is : X,Y specifies location of the hole. Z defines the Z point level. The Z point level in this case is the top of the hole that is being cut by the back boring operation. Q or I, J, K defines the tool shift amount and direction. R defines the position beyond the hole bottom so the tool can safely shift. F defines the cutting feedrate.
Chapter 26 Milling Fixed Cycles In the G87 back boring cycle, the control moves the axes in the following manner: 1. The tool rapids to the initial point level above the hole location. 2. After the back boring tool is positioned, the control orients the tool to a position determined in AMP by the system installer. The control shifts the boring tool by one of two possible methods, as discussed below. The shift method is determined in AMP by the system installer.
Chapter 26 Milling Fixed Cycles When using Method II, remember: If both axes in the current plane are to be shifted, specify both words to move the axes. The move generated will be a single linear move and will execute at rapid traverse. 3. The back boring tool moves at a rapid feedrate through the existing hole to the depth designated by the R--word. 4.
Chapter 26 Milling Fixed Cycles Important: The programmer or operator must start spindle rotation. Figure 26.15 G88: Boring Cycle, Spindle Stop/Manually Out Cutting feed Rapid feed Manual operation Initial point level 1 7 Spindle rotation in the forward direction R 2 6 R point level Cycle start 3 Z 5 Hole bottom 4 Spindle stops at hole bottom after dwell In the G88 boring cycle, the control moves the axis in the following manner: 1.
Chapter 26 Milling Fixed Cycles 7. At this point, the rotation of the spindle changes to the clockwise direction. When the single block function is active, the control stops axis motion after steps 1, 2 and 5. (G89): Boring Cycle, Dwell/Feed Out The operations in G89 are identical to as those of the G85 boring cycle with the exception that the control executes a dwell at hole bottom.
Chapter 26 Milling Fixed Cycles Figure 26.16 G89: Boring Cycle, Dwell/Feed Out Cutting feed Rapid feed Initial point level 1 R 6 2 R point level 3 Z Hole bottom 4 5 Dwell In the G89 boring cycle, the control moves the axes in the following manner: 1. The tool rapids to initial point level above the hole location. 2. The boring tool then rapids to the R point level, slows to the programmed cutting feedrate and begins the boring operation. 3.
Chapter 26 Milling Fixed Cycles 26.5 Altering Milling Fixed Cycle Operating Parameters The system installer determines many parameter for the milling fixed cycles in AMP. The following 3 parameters are set in AMP but may be overridden by the operator using the Milling Cycle Parameter screen. When changed through this screen, the new values remain in effect until they are manually changed or AMP is downloaded with new values.
Chapter 26 Milling Fixed Cycles 3. Press the {MILCYC PARAM} softkey. The Milling Cycle Parameter screen is displayed. Figure 26.17 shows a typical Milling Cycle Parameter screen. (softkey level 3) ZONE F1-F9 LIMITS MILCYC PRBCYC PARAM PARAM Figure 26.17 Milling Cycle Parameter Screen MILLING CYCLE PARAMETERS ENTER VALUE: G73 DEEP HOLE PECK DRILLING CYCLE RETRACT AMOUNT 1.000 [ MM] G83 DEEP HOLE DRILLING CYCLE CLEARANCE AMOUNT 1.
Chapter 26 Milling Fixed Cycles 5. Replace the parameter value or add to it. There are two ways to quit the Milling Cycle Parameter screen: To save the changes just made to the parameters and leave the Milling Cycle Parameter screen, press the {UPDATE & EXIT} softkey. To discard any changes just made to the parameters and leave the Milling Cycle Parameter screen, press the {QUIT} softkey. (softkey level 3) REPLCE ADD TO VALUE VALUE 6. 26.
Chapter 26 Milling Fixed Cycles Figure 26.18 Result of Examples 27.2 and 27.
Chapter 26 Milling Fixed Cycles 26-42
Chapter 27 Skip, Gauge, and Probing Cycles 27.1 Chapter Overview 27.2 External Skip, Gauge, and Probe Functions This chapter describes the external skip, gauge, and probe functions available on the control. Use this table to find information: Information on: On page: External Skip Functions (G31 codes) 27-2 Tool Gauging External Skip functions (G37 codes) 27-4 Hole Probing (G38) 27-8 Parallel Probing Cycle (G38.
Chapter 27 Skip, Gauge, and Probing Cycles The control provides several means of triggering an external skip, gauge, or probing block: Discrete inputs on the I/O ring Any one of the four available “High Speed inputs” (not available on 9/230 CNCs) A “Probe” input that directly latches the feedback counters. These different inputs, each with different degrees of precision, may be used to signal the control to store the current axes positions.
Chapter 27 Skip, Gauge, and Probing Cycles Format for any G31 external skip blocks is as follows: G31 X__ Y__ Z__ F__; Where : Is : G31 Any of the G codes in the G31 series or G04. Use the one that is configured to respond to the current external skip signal device that is being used. X, Y, Z The endpoint of the move if no external skip signal is received. These also determine the direction that the tool will travel in. F The external skip function feedrate.
Chapter 27 Skip, Gauge, and Probing Cycles Skip Function Application Examples One typical application for these G-codes would be moving the part until it contacts a probe and then proceeding with a machining operation from that point. This would provide part feature consistency by insuring that the machining of all parts began from a fixed reference point (probe trigger point).
Chapter 27 Skip, Gauge, and Probing Cycles Format for any G37 skip blocks is as follows: G37 Z__ F__; Where : Is : G37 Corresponds to any of the G-codes in the G37 series. Use the one that is configured to respond to the current skip signal device that is being used. X, Y, Z The axis on which the offset measurement is to be taken is specified here as either X, Y, or Z. Only one axis may be specified in a G37 block.
Chapter 27 Skip, Gauge, and Probing Cycles CAUTION: If modifying a tool length offset, the offset value generated with this gauging operation is immediately loaded into the offset table. Since this offset must be the currently active offset, it becomes effective either immediately when the next block is executed, or delayed until the next block that contains motion on the tool length axis is executed (when an offset is activated is determined in AMP).
Chapter 27 Skip, Gauge, and Probing Cycles Tool Gauging Application Example A typical application for these G-codes in determining tool offsets would execute as follows: 1. When the control executes the G37 block, the triggering device moves towards the tool using the axis specified in the block. 2. When the control receives the appropriate skip signal through PAL, axis motion stops. 3. The control records the position when the skip signal is received.
Chapter 27 Skip, Gauge, and Probing Cycles 27.4 Hole Probing (G38) The purpose of this cycle is to provide a means to measure the actual radius and/or locate the center of a hole in a part or gauge using a touch probe. To use the G38 cycle, the currently active plane when the G38 is programmed must be the same plane that the hole to be measured is in (see chapter 13 for information on plane selection).
Chapter 27 Skip, Gauge, and Probing Cycles They may be programmed directly in the G38 block. Values entered for these parameters in the G38 block supercede both AMP values and probe parameter table values. Figure 27.2 Parameters for G38 Hole Probing Cycle Probe Probe radius (see section 27.
Chapter 27 Skip, Gauge, and Probing Cycles 3. The axis continues towards the estimated diameter (H) until the probe signals that contact has been made. If the probe triggers before reaching the negative tolerance band (D), or does not trigger after passing through the positive tolerance band (D), a PROBE ERROR will occur. This error appears on the screen as a warning but does not place the control in E-STOP. Instead the G38 block is aborted, and program execution proceeds to the next block. 4.
Chapter 27 Skip, Gauge, and Probing Cycles Important: To accurately measure a hole radius and determine its center, the exact probe tip radius must be available to the control. This value is entered either through AMP, through paramacro system parameter #5096, or through the probe parameter table discussed in section 27.5. Table 27.A shows the paramacro system parameters used to relay information from the probing operation to the programmer.
Chapter 27 Skip, Gauge, and Probing Cycles 27.5 Parallel Probing Cycle (G38.1) The purpose of this cycle is to provide a means to measure the amount that a part is out of parallel (or rotated) with a selected axis through the use of a touch probe. Note that the currently active plane (G17, G18, or G19) must be the same plane in which probe motion is to occur in and must be active before the probing cycle block is executed. Format for the G38.1 code is as follows: G38.
Chapter 27 Skip, Gauge, and Probing Cycles Figure 27.4 Parameters and Motion Paths for G38.1 Probing Cycle +Y Work piece or fixture D 2nd hit 1st hit D D D J F feedrate F feedrate X Point where G38.1 block is executed I Y E feedrate R E feedrate E feedrate E feedrate +X Parameters R, D, E, and F can be entered in 3 ways: The system installer may have entered them in AMP, in which case they will always be available and need not be programmed in the G38.1 block.
Chapter 27 Skip, Gauge, and Probing Cycles The control executes the G38.1 cycle in this manner: 1. When the G38.1 block is executed, the control initially moves only the first axis in the G38.1 block to the coordinate position entered with it. The approach feedrate (E) is used for this move. 2. The second axis in the G38.1 block is then moved to the coordinate defined by the approach distance parameter, R. Again, the approach feedrate (E) is used. 3.
Chapter 27 Skip, Gauge, and Probing Cycles Figure 27.5 G38.1 Parallel Probing Cycle Paramacro Parameter Values Work piece or fixture 2nd hit 1st hit (#5091 Rise Distance) (#5090 Run distance) 27.6 Probing Parameters Table Use this feature to access the Probe Parameters table and alter probe parameters affecting the operation of the G31, G37, and G38 codes . For details on the parameters available here, refer to the appropriate section of this chapter. Access to this table may be restricted.
Chapter 27 Skip, Gauge, and Probing Cycles 2. Press the {PROGRAM PARAM} softkey. (softkey level 2) PRGRAM AMP PARAM DEVICE MONSETUP TOR TIME PARTS PTOM SI/OEM 3. Press the {PROBE PARAM} softkey to display the probing cycle parameter table. (softkey level 3) ZONE F1-F9 MILCYC PROBE LIMITS PARAM PARAM Figure 27.6 Probing Parameters Screen PROBING PARAMETERS APPROACH DISTANCE TOLERANCE BAND APPROACH FEEDRATE PROBE FEEDRATE PROBE LENGTH PROBE RADIUS R D E F 0.000 0.000 0.000 0.000 0.000 0.
Chapter 27 Skip, Gauge, and Probing Cycles 5. You can change parameter values two ways: Press the {REPLCE VALUE} softkey then type in a new value for the selected parameter by using the keys on the operator panel. When you press the [TRANSMIT] key, the value typed in will replace the old value for that parameter. Press the {ADD TO VALUE} softkey then type in a value to add to the old value for the selected parameter by using the keys on the operator panel.
Chapter 27 Skip, Gauge, and Probing Cycles 27.7 Adaptive Depth (G26) Use the Adaptive Depth feature to enable an adaptive depth probe that monitors tool depth relative to the actual part surface. This feature is sometimes referred to as “cut to length” or “ cut to depth”.
Chapter 27 Skip, Gauge, and Probing Cycles Format for an adaptive depth block is as follows: G26 X__ Y__ Z__ I__ J__ K__ ; Where: Programs: X, Y, or Z Adaptive Depth Axis word. Use the axis word associated with the adaptive depth (the system installer selects this axis as the controlling axis in AMP). Program an axis destination that is sufficiently beyond where you expect the depth probe to contact the part surface.
Chapter 27 Skip, Gauge, and Probing Cycles The control will perform its normal axis deceleration as it approaches the final depth. When the final depth is reached the axis stops and the part program continues on from that point. Since the actual location of the endpoint of the move is not known until the probe is depressed, the control must re-setup any part program blocks that it previously read into block look ahead.
Chapter 27 Skip, Gauge, and Probing Cycles The system installer determines how many counts of the adaptive depth probe constitutes contact with the part (a probe fired event AMPed as the probe trigger tolerance). Multiple counts are typically required because of the potential for probe deflection from acceleration/deceleration or machine vibration. This number of counts for the probe to fire is added back into the current axis position for an accurate part surface location.
Chapter 27 Skip, Gauge, and Probing Cycles Once the probe is fired you must position the adaptive depth axis (assuming the probe is closing the feedback loop) using the integrand word in a G26 block. You must also still program an adaptive depth axis word (see Example 27.2). If you use a non-G26 block to position the adaptive depth axis, feedback is immediately switched from the adaptive depth probe back to the adaptive depth axis’normal feedback device.
Chapter 27 Skip, Gauge, and Probing Cycles “Probe Trips During Deceleration” Warnings An axis deceleration can occur before the probe trips caused by the programmed endpoint of the G26 block being to close to the position at which the depth probe trips. In this situation, the control having failed to receive a probe fired indication, has begun to decelerate to the G26 programmed endpoint. During this deceleration the probe trips and feedback is switched over to the adaptive depth probe.
Chapter 27 Skip, Gauge, and Probing Cycles The adaptive depth probe position is zeroed automatically at power turn on. In the event that you must re-zero the probe the system installer can write PAL to enable you to zero the probe any time the adaptive depth axis is not in motion. Refer to your system installers documentation on using $ADPCLR. WARNING: We strongly recommend that you require (either through PAL or some other procedure) a manual probe zeroing operation be performed after every power up.
Chapter 27 Skip, Gauge, and Probing Cycles Feature Considerations This feature: Used with G26 adaptive depth: Virtual C Spindle Cylindrical Interpolation Corner Radius and Chamfer Programming All Fixed Cycles (except some transfer line only cycles) QuickPath Plus program blocks Is incompatible with the adaptive depth probe. An error is generated if one of these features is active or activated when a G26 block is executing.
Chapter 27 Skip, Gauge, and Probing Cycles This feature: Used with G26 adaptive depth: Dual and De-skew axes Is incompatible with the adaptive depth probe. An error is generated when you attempt to run an adaptive depth cycle if one of these types of axes are configured as the adaptive depth axis. Mid Start/ Program Restart If motion to the block that is selected for Mid Start/Program Restart generates a move that fires the depth probe, a unexpected depth probe trip will occur.
Chapter 28 Paramacros 28.0 Chapter Overview 28.1 Paramacros This chapter describes paramacros and and how to program them. Use this table to find information: Information on: On page: Paramacros 28-1 Parametric Expressions 28-2 Transfer of Control Commands 28-7 Parameter Assignments 28-12 Assigning Parameter Values 28-37 Macro Call Commands 28-45 Macro Output Commands 28-55 The paramacros feature is similar to a subprogram with many added features.
Chapter 28 Paramacros 28.2 Parametric Expressions It may be necessary for mathematical expressions to be evaluated in a complex paramacro. This requires that some form of mathematical equation be written in a paramacro block. The following is a discussion of the operators and function commands available for use on the control. These operators and function commands are valid in any block within a program, subprogram, paramacro, or MDI program. 28.2.
Chapter 28 Paramacros All logical operators have the format of: A logical operator B where A and B are numerical data or a parameters with a value assigned. If B is negative in the above format, an error will occur. If A is negative, the absolute value of A is used in the operation and the sign is attached to the final result. Before evaluation, A and B are made integers by rounding and truncating. Example 28.2 Logical Operation Examples Expression Entered Result [16.2MOD3] 1.0 [-16.2MOD3] -1.
Chapter 28 Paramacros 28.2.2 Mathematical Function Commands This subsection lists the basic mathematical functions that are available on the control and their use. Use these functions to accomplish mathematical operations that are necessary to evaluate the trigonometric and other complex mathematical equation such as rounding off, square roots, logarithms, exponent, etc. Table 28.B lists the basic functions that are available and their meanings. Table 28.
Chapter 28 Paramacros Example 28.3 Format for Functions SIN[2] This evaluates the sine of 2 degrees. SQRT[14+2] This evaluates the square root of 16. SIN[SQRT[14+2]] This evaluates the sine of the square root of 16. LN[#2+4] This evaluates the logarithm of the value of parameter #2 plus 4. Example 28.4 Mathematical Function Examples Expression Entered Result SIN[90] 1.0 SQRT[16] 4.0 ABS[-4] 4.0 BIN[855] 357 BCD[357] 855 ROUND[12.5] 13.0 ROUND[12.4] 12.0 FIX[12.7] 12.0 FUP[12.
Chapter 28 Paramacros 28.2.3 Parametric Expressions as G- or M- Codes You can use parametric expressions to specify G-codes or M-codes in a program block. For example: G#1 G#100 G#500 M#1 M#100 M#500; G#520 G[#521-1] G[#522+10] M#520 M[#522+1] M[#522+10]; When using a parametric expression to specify a G-- or M-code, remember: When specifying more than one G-- or M-code in a block from the same modal group, the G-- or M-code closest to the End-of-Block of that block is the one activated.
Chapter 28 Paramacros Attempting to use any of the above as MDI commands, 9/PC generates an “ILLEGAL MACRO CMD VIA MDI” error message. 28.3 Transfer of Control Commands Use transfer of control commands to alter the normal flow of program execution. Normally the control executes program blocks sequentially. By using control commands, the programmer can alter this normal flow of execution and transfer execution to a specific block or begin looping (executing the same set of blocks repetitively).
Chapter 28 Paramacros Program a condition between the [ and ] brackets in this format: [A EQ B] where A and B represent some numerical value. The values for A and B can be in the form of some mathematical equation or in the form of a paramacro parameter. Example 28.6 Evaluation of Conditional Expressions Expression Evaluation [6.03 EQ 6.0301] FALSE [6.03 NE 6.0301] TRUE [2.5 GT 2.5] FALSE [2.5 LT 2.51] TRUE [2.51 GE 2.5] TRUE [2.5 LE 2.5] TRUE [[2.
Chapter 28 Paramacros Example 28.7 Unconditional GOTO N1...; N2...; N3GOTO5; N4...; N5...; N6...; /N7GOTO1; In Example 28.7, execution continues sequentially until block N3 is read; then execution transfers to block N5 and again resumes sequential execution to block N6. If optional block skip 1 is off, block N7 will transfer execution back to block N1. Conditional IF-GOTO The conditional IF-GOTO command is dependent on whether a mathematical condition is true.
Chapter 28 Paramacros When block N2 is read, parameter #3 is compared to the value -1.5. If the comparison is true, then blocks N3 and N4 are skipped, and execution continues on from block N5. If the comparison is false, then execution continues to block N3. When block N6 is read, parameter #4 is compared to the value 3. If the comparison is true, then execution is transferred to block N1; if it is false, execution continues to block N7. 28.3.
Chapter 28 Paramacros Use this format for the WHILE-DO-END command: WHILE [ (condition) ] DO m; ; ; ; END m; Where : Is : (condition) some mathematical condition. This condition is tested by the control to determine if it is true or false. m an identifier used by the control to relate a DO block with an END block. The value of m must be the same for the DO as it is for the corresponding END. This value can be either 1, 2, or 3.
Chapter 28 Paramacros Example 28.10 Nested WHILE DO Commands N1#1=1; N2WHILE[#1LT10]DO1; N3#1=[#1+1]; N4WHILE[#1EQ2]DO2; N5...; N6END2; N7END1; N8...; In Example 28.10, blocks N2 through N7 are repeated until the condition in block N2 becomes false. Within DO loop 1, DO loop 2 will be repeated until the condition in block N4 becomes false. 28.4 Parameter Assignments The following subsections describe assigning different paramacro parameter values and how these parameters are used in a paramacro.
Chapter 28 Paramacros Local parameters are used in a specific macro to perform calculations and axis motions. After their initial assignment, these parameters can be modified within any macro at the same nesting level. For example macro O11111 called from a main program has 33 local parameter values to work with (#1 to #33). All macros called from the main program, and nested at the same level, use the same local parameters with the same values unless they are initialized in that macro.
Chapter 28 Paramacros Example 28.11 Assigning Using More Than One I, J, K Set G65P1001K1I2J3J4J5; The above block sets the following parameters: parameter #6 = 1 parameter #7 = 2 parameter #8 = 3 parameter #11 = 4 parameter #14 = 5 If the same parameter is assigned more than one value in an argument, only the right-most value is stored for the parameter. Example 28.12 Assigning the Same Parameter Twice G65P1001R3.1A2R-0.5 The above block sets the following parameters: parameter #1 = 2.
Chapter 28 Paramacros 28.4.2 Common Parameters The common parameters refer to parameter numbers 100 to 199 and 500 to 999 for all 9/Series controls except for the 9/240, which allows 100 to 199 and 500 to 699. The common parameters are assigned through the use of a common parameter table as described on page 28-41. Common parameters are global in nature. This means that the same set of parameters can be called by any program, macro, subprogram, or MDI program.
Chapter 28 Paramacros Table 28.
Chapter 28 Paramacros 5671 to 5682 1 Acceleration Ramps for S-- Curve Acc/Dec Mode 28-32 5691 to 5702 1 Deceleration Ramps for S-- Curve Acc/Dec Mode 28-32 5711 to 5722 1 Jerk 28-33 28-17
Chapter 28 Paramacros Table 28.D System Parameters (continued) Parameter # System Parameter Page 5731 to 5743 Home Marker Distance 28-33 5751 to 5763 Home Marker Tolerance 28-34 1 These parameters may only have their value received (read-only) 2 These parameters may only have their value changed (write-only) #2001 to 2999 Tool Offset Tables These parameters may be changed or simply read through programming.
Chapter 28 Paramacros #3000 Program Stop With Message (PAL) Use this parameter to cause a cycle stop operation and display a message on line 1 of the CRT. Any block that assigns any non-zero value to parameter 3000 will result in a cycle stop. The actual value assigned to parameter 3000 is not used. Parameter 3000 is a write-only parameter. When the control executes this block, a cycle stop is performed and the message “SEE PART PROGRAM FOR MACRO STOP MESSAGE” is displayed on line 1 of the CRT.
Chapter 28 Paramacros #3002 System Clock This parameter is referred to as a clock parameter and references an hour counter. It is a read-write parameter with negative value assignments being illegal. The maximum value for this parameter is 1 year (8760 hours). The parameter value is maintained when power is lost. It is incremented by .000005556 every 20 ms.
Chapter 28 Paramacros #3004 Block Execution Control 2 This parameter determines whether a cycle stop request will be recognized, whether the feedrate override switch is active, and whether exact stop mode is available (G61 mode). The range of this parameter is from 0 to 7 and it is a write-only parameter. Table 28.F shows the results of the different values for parameter number 3004. If they are ignored, the control will not allow the feature to be used.
Chapter 28 Paramacros For example, programming: #3006=.1 (Install Tool Number 6); will cause program execution to stop at the beginning of this block and the message display the message telling the operator to read the comment in the block. #3007 Mirror Image This parameter is a read-only. It generates an integer that represents, in binary, what axes are mirrored. For example, if the value of this parameter was 3, the binary equivalent for this is 00000011.
Chapter 28 Paramacros Table 28.G Modal Data Parameters Parameter Number Modal Data Value #4001 to 4021 These correspond to the different G-code Groups 1-21 (see chapter 10) and show what G-code from group is currently active.
Chapter 28 Paramacros #5021 to 5032 Coordinates of Commanded Position These parameters are read-only. They correspond to the current coordinates of the cutting tool. These are the coordinates in the work coordinate system.
Chapter 28 Paramacros #5061 to 5069 or #5541 to 5552 Skip Signal Position Work Coordinate Position These parameters are read-only. They correspond to the coordinates of the cutting tool when a skip signal is received to PAL from a probe or other device such as a switch. These are the coordinates in the work coordinate system.
Chapter 28 Paramacros Or if your system has more than 9 axes: 5561 Axis 1 coordinate position 5567 Axis 7 coordinate position 5562 Axis 2 coordinate position 5568 Axis 8 coordinate position 5563 Axis 3 coordinate position 5569 Axis 9 coordinate position 5564 Axis 4 coordinate position 5570 Axis 10 coordinate position 5565 Axis 5 coordinate position 5571 Axis 11 coordinate position 5566 Axis 6 coordinate position 5572 Axis 12 coordinate position The system installer determines in AMP
Chapter 28 Paramacros #5090 to 5094 Probing Cycle Positions These parameters are read-only. They correspond to values (in the machine coordinate system) generated by the last successful probing cycle. These cycles are programmed using G-codes G38 (circle diameter and center measurement) and G38.1 (parallel probing cycle). 5090 G38.1 rise measurement 5091 G38.
Chapter 28 Paramacros #5095 to 5096 Probe stylus Length and Radius These parameters correspond to the values set in the probing cycle parameter table discussed in chapter 27. When values are assigned to these parameters, the current values in the probe table is replaced. 5095 Probe stylus Length 5096 Probe stylus Radius For details on probe radius and length parameters, see chapter 27 on tool gauging. #5101 to 5112 Current Following Error These parameters are read-only.
Chapter 28 Paramacros #5221 to 5392 Work Coordinate Table Value These parameters are read or write. They correspond to the current value set in the work coordinate table for the G54-G59 work coordinate systems (see chapter 3). You can read data from the tables and set data into the table by assigning values to the parameters. The axis names are set in AMP.
Chapter 28 Paramacros #5221 to 5392 Work Coordinate Table Value (continued) 5261 G56 Axis 1 Coordinate 5361 G59.2 Axis 1 Coordinate 5262 G56 Axis 2 Coordinate 5362 G59.2 Axis 2 Coordinate 5263 G56 Axis 3 Coordinate 5363 G59.2 Axis 3 Coordinate 5264 G56 Axis 4 Coordinate 5364 G59.2 Axis 4 Coordinate 5265 G56 Axis 5 Coordinate 5365 G59.2 Axis 5 Coordinate 5266 G56 Axis 6 Coordinate 5366 G59.2 Axis 6 Coordinate 5267 G56 Axis 7 Coordinate 5367 G59.
Chapter 28 Paramacros #5630 S- Curve Time per Block This parameter is read only. The value represents the amount of time (seconds converted to system scans) for a part program block’s S--Curve filter where S--Curve Acc/Dec is applied during G47.1 mode. When it is multiplied by the scan time, the product equals the amount of time required by the acceleration. This parameter is only calculated for blocks that have programmed motion with S--Curve Acc/Dec.
Chapter 28 Paramacros #5671 to 5682 Acceleration Ramps for S- Curve Acc/Dec Mode These parameters are read only. They correspond to the active acceleration ramps in S--Curve Acc/Dec mode. You can set these parameters by programming a G48.3 in your part program block. Control Reset, Program End (M02/M03), or G48 will reset these values to their default AMP values. For more information about programming G48.x codes, refer to chapter 18 in your 9/Series CNC Operation and Programming Manual.
Chapter 28 Paramacros #5711 to 5722 Jerk These parameters are read only. They are only applicable to the current jerk values when S--Curve Acc/Dec mode is active. You can set these parameters by programming a G48.5 in your part program block. Control Reset, Program End (M02/M03), or G48 will reset these values to their default AMP values. For more information about programming G48.x codes, refer to chapter 18 in your 9/Series CNC Operation and Programming Manual.
Chapter 28 Paramacros #5751 to 5763 Home Marker Tolerance These parameters are read only. They correspond to the current home marker tolerance. These parameters will contain the tolerance value at power turn on and will represent 3/8 of an electrical cycle of the feedback device converted to current axis programming units (inch/metric, degrees or revolutions). 28.4.
Chapter 28 Paramacros The control always interprets parameter #1032, #1033, #1034, and #1035 as integer values regardless of how they are assigned in PAL (as an integer or on a per bit basis). #1032 is the only parameter that may also be interpreted by the control on a per-bit basis using parameters #1000 - #1031. PAL may always interpret these values on either a per-bit basis or as integer values. The second set of parameters, #1072 -- #1075, functions the same way.
Chapter 28 Paramacros #1132 -- #1135 and #1172 -- #1175 The control always interprets these parameters as integer values. #1132 is the only parameter that may also be interpreted by the part program on a per-bit basis using parameters #1100 #1131. The second set of parameters, #1172 -- #1175, functions the same way. See the system installer’s documentation for a detailed description of the use and operation of these input flags. 28.4.
Chapter 28 Paramacros 28.5 Assigning Parameter Values There are 3 methods for assigning parameters. They can be assigned by: using arguments (only available for local parameters) direct assignments using tables (view or set common parameters, view local parameters) Assigning Parameters Using Arguments Arguments may be used only to assign local parameter values. System, Common, and PAL variables may not be assigned using arguments. Usually parameters assigned using an argument are variables for a macro.
Chapter 28 Paramacros Table 28.
Chapter 28 Paramacros To enter a value for a parameter # using an argument, enter the word corresponding to the desired parameter number in a block that calls a paramacro (for legal argument locations, see specific formats for calling the macro) followed by the value to assign that parameter. For example: G65P1001A1.1 B19; assigns the value of: 1.1 to local parameter #1 in paramacro 1001 19 to local parameter #2 in paramacro 1001 You can specify arguments as any valid parametric expression.
Chapter 28 Paramacros Example 28.15 Assigning Parameters: #100=1+1; #100=5-3; #100=#3; #100=#7+1; #100=#100+1; You can also assign multiple paramacro parameters in a single block. In a multiple assignment block, each assignment is separated by a comma. For example: #1=10,#100=ROUND[#2+#3],#500=10.0*5; If you use multiple assignments in the same block, remember: You can enter as many assignments as can be typed into one block (127 characters maximum).
Chapter 28 Paramacros Direct Assignment Through Tables Use this feature to view or set common parameters and view local parameters. Assignment through tables is generally used to edit common parameters. To edit the values of the common parameters or view the local parameters, follow these steps. 1. Press the {MACRO PARAM} softkey. (softkey level 1) 2.
Chapter 28 Paramacros If viewing the local parameter table, do not continue to step 3. If editing one of the common parameter tables, move on to step 3. (softkey level 3) LOCAL PARAM 3. COM-1 PARAM COM-2A COM-2B PARAM PARAM Select a parameter to change by moving the cursor to the desired parameter number. Note that the selected parameter is shown in reverse video. Move the cursor by an entire page by pressing the up or down cursor key while holding down the [SHIFT] key.
Chapter 28 Paramacros Select and complete the appropriate step to alter the common parameter names. The 3 options include: To edit an existing parameter name or enter a parameter name for the first time for a local parameter, press the {REPLCE NAME} softkey. Key in a parameter name for the parameter. A name may be up to 8 characters long and include any alphanumeric character with the exception of a few of the special symbols. After the name is keyed in, press the [TRANSMIT] key.
Chapter 28 Paramacros Addressing Assigned Parameters Once you assign a parameter you can address it in a program: Example 28.16 Addressing Assigned Parameters #100=5; #105=8; G01X#100+5 ; Axis moves to 10. G01x[#100+5] Axis moves to 8 You can also indirectly address parameters with other parameters Example 28.17 Indirectly Addressing Parameters #100=101 #101=2.345 G01 X#[#100]; X axis moves to the contents of #100 which is #101. #101 has the value of 2.345.
Chapter 28 Paramacros 2. Enter a name for the backup file and press [TRANSMIT]. The system verifies the file name and backs up the selected parameters into a part program. You can restore these parameters by selecting and executing that part program. Important: If part program calculations cause an overflow value, then the generated backup file contains an M00 and the parameter number followed by the word “OVERFLOW” as a comment. 28.
Chapter 28 Paramacros CAUTION: Any edits that are made to a subprogram, or to a paramacro program (as discussed in chapter 5) that has already been called for automatic execution, are ignored until the calling program is disabled and reactivated. Subprograms and paramacros are called for automatic execution the instant that the calling program is selected as active (as discussed in chapter 7). 28.6.
Chapter 28 Paramacros 28.6.2 Modal Paramacro Call (G66) Use this format for calling a paramacro using the G66 command: G66 P_ L_ A_ B_; Where : Is : P Indicates the program number of the called macro. P ranges from 1 - 99999. L Programs the number of times the macro will be executed after each motion block that follows the G66. L ranges from 1 - 9999, and may be expressed as any valid parametric expression. If not specified, the control uses a default value of 1. A-Z Optional argument statements.
Chapter 28 Paramacros Unlike non-modal macro calls, the G66 macro call repeats automatically after any axis move until cancelled by a G67 block. This also applies to nested macros. When the control begins execution of the nested macro 1002 in the program below, each axis move in the nested macro also calls for the execution of the macro 1001. Example 28.18 Modal Macro Call N0100G66P1001; N0200G65P1002; In Example 28.18, after the complete execution of the macro 1002, the macro 1001 is called.
Chapter 28 Paramacros Important: When the control executes block N040, the original value as set in block N020 for parameter number 1 is ignored, and the most current value (1.7) is used. The first time macro 1001 is executed, Z moves 1.1 units. The second time macro 1001 is executed, Z moves 1.7 units. 28.6.3 Modal Paramacro Call (G66.1) Use this format for calling a paramacro using the G66.1 command: G66.1 P_ L_ A_ B_; Where : Is : P Indicates the program number of the called macro.
Chapter 28 Paramacros The L--word or any optional argument statements following a G66.1 can contain any valid mathematical expression. For example: G66.1 P1002 L[#1+1] A[12*6] B[SIN[#101]]; Example 28.20 G66.1 Macro Operation N0100G90G17G00; N0110G66.1P9400; Macro 9400 is executed. N0120G91G18G01; G91 and G18 become effective, 01 is assigned to parameter #10, macro 9400 is executed. N0130G03X1.; 03 is assigned to parameter #10, 1. is assigned to parameter #24, macro 9400 is executed.
Chapter 28 Paramacros 28.6.4 AMP-defined G-Code Macro Call Use this format for calling an AMP-defined macro: G_ A_ B_; Where : Is : G_ Programs an AMP-defined G-code command (from G1 to G255.9). A-Z Optional argument statements. May be programmed using any letter from A to Z excluding G, L, N, O, or P. Used to assign numeric values to parameters in the paramacro (see Table 28.H). Arguments may be specified as any valid parametric expression.
Chapter 28 Paramacros 28.6.5 AMP-Defined M-Code Macro Call Use this format for calling an AMP-defined M-code macro: M255 A_B_ Where : Is : M255 Programs an AMP-defined M-code command. A-Z Optional argument statements. May be programmed using any letter from A to Z excluding G, L, N, O, or P. Used to assign numeric values to parameters in the paramacro (see Table 28.H). Arguments may be specified as any valid parametric expression. These macros are executed only as non-modal macro.
Chapter 28 Paramacros These macros are executed only as non-modal macro. The execution of the T--, S--, or B--code macro calls is the same as M-code macro calls with the following exceptions: the parameter # referenced when called the macro program called T calls macro 9000 S calls macro 9029 B calls macro 9028 In order for the T--, S--, or B--words to call up a macro program, these prerequisites must be met: 1. The value following the word must be equal to the value stored for the specified parameter #.
Chapter 28 Paramacros Precautions must be taken when attempting to nest AMP assigned macro calls since many combinations of these calls may not be valid. The system installer determines in AMP the functionality of the AMP-defined macro call when nested.
Chapter 28 Paramacros Table 28.J Works as the System-defined Code TYPE OF MACRO NESTED 1 CALLING PROGRAM G65, G66,or G66.1 AMP-G AMP-M AMP-T S or B G65, G66 or G66.1 Yes Yes Yes Yes AMP G-code Yes No No No AMP M-code Yes No No No AMP-T-- , S-- , or B-- code Yes No No No 1 What Yes/No means: Yes - - the macro type across the top row may be called from the macro type down the left column.
Chapter 28 Paramacros POPEN This command affects a connection to the output device by sending a DC2 control code and a percent character “%” to the RS-232 interface. This command must be specified prior to outputting any data. After this command, the control outputs any following program blocks including the parameter values that are used in them.
Chapter 28 Paramacros Example 28.22 would yield an output equal to the character strings with the * symbols being converted to spaces and the parameter values for parameters #123 and #234. The value of the parameter is output in binary as a 32-bit string with the most significant bit output first. Negative values are output in 2’s complement. Example 28.23 BPRNT Program Example #123=0.40936; #124=-1638.4; #10=12.
Chapter 28 Paramacros There may be as many S and #P in a block as desired provided that the length of the block does not exceed the maximum block size. Example 28.24 Sample of a DPRNT Block DPRNT[INSTALL*TOOL*#123[53]*PRESS*CYCLE*STOP**#234[20]]; Example 28.24 would yield an output equal to the character strings with the * symbols being converted to spaces and the parameter values for parameters #123 and #234. The value of the parameter is output as a string of decimal digits.
Chapter 29 Program Interrupt 29.0 Chapter Overview This chapter describes the program interrupt feature. This feature lets you execute a subprogram or paramacro program while some other program is executing. This subprogram or paramacro is executed when PAL receives an interrupt signal (usually through the use of some switch triggered by the operator or one of the axes). The interrupt program can be executed even mid-block during a programs execution.
Chapter 29 Program Interrupt The format for these M codes is: M96L__P__; M97L__; Where : Selects: L the type of interrupt and the signal that will call the interrupt. L ranges from 0 - 3. P the interrupt program. P is followed by a 5 digit non-decimal program name. An error is generated if anything other than an N word, a P or L word, a block delete /, or a comment character is programmed in the M96 or M97 block. An interrupt M code M96 or M97 may also be programmed within a interrupt program.
Chapter 29 Program Interrupt Selecting an Interrupt Program Any legal subprogram or paramacro may be selected as a interrupt program (refer to the section in chapter 10 on subprograms or chapter 28 for paramacros). For a program to be used as an interrupt program it must have a program name of 5 numeric characters following an O address (see the section on program names in chapter 10). This interrupt program must contain an M99 block as the last block in the interrupt program.
Chapter 29 Program Interrupt 29.2 Interrupt Request Considerations When using system interrupts, take into consideration: The system installer can determine in AMP if a signal to execute an interrupt program is delayed until the end of a currently executing block, or if the interrupt is executed immediately when the signal is received.
Chapter 29 Program Interrupt If an interrupt occurs during a block retrace, the interrupt will be performed. The block retrace however will be aborted at that point and no further retrace will be allowed. Block retrace will, however, still be able to return any moves that have already been retraced before the interrupt occurred.
Chapter 29 Program Interrupt Figure 29.
Chapter 29 Program Interrupt Figure 29.2 Type 2 Interrupt M99 M99 Return path Return path Motions due to Immediate Action interrupt Part program path before interrupt Motions due to Delayed interrupt Interrupt occurs This block is not executed unless there are no motion commands in the interrupt Programmed Path Path of Interrupt It is possible to alter the number of blocks that the control re-executes in reverse when returning to the start position of the interrupt.
Chapter 29 Program Interrupt The number of retrace blocks as set with this M code is the same for all active or inactive interrupts. If an interrupt is enabled after this M code is programmed it will take on the number of retrace blocks as programmed with this M code. When the return from interrupt is executed (M99 in the interrupt) the control will generate a linear move to the end point of the last remembered move for retrace.
Chapter 29 Program Interrupt If using a type 2 interrupt (L1, L2, or L3), remember that the control remembers up to the first 4 blocks in the program and uses these to retrace its moves back to the starting point of the interrupt program. The control remembers up to 4 of the first moves or until a circular block is executed. For details, see section 29.3 on interrupt types. The interrupt program may contain a milling cycle in the interrupt.
Chapter 29 Program Interrupt 29-10
Chapter 30 Using a 9/Series Dual-processing System 30.0 Chapter Overview Read this chapter to learn general information related to programming and operating a dual-processing system. Major topics in this chapter cover: Topic: 30.
Chapter 30 Using a 9/Series Dual--processing System 30.2 Operating a Dual-processing System Dual-process systems operate almost exactly the same as their single-process counterparts. Each process functions as an independent 9/Series control. With the exception of shared dual-processing paramacro parameters and shared axes, there is little shared data between processes. Each process has its own offset tables, programmable zone tables, and paramacro parameters.
Chapter 30 Using a 9/Series Dual--processing System You cannot switch the active process while you use the digitize feature, a tool path or QuickCheck graphic display, or within an active program search operation. If you attempt to switch the active process while using one of these features, the control displays an error message. Select an active process by using one of these methods: Method: Description: [PROC SELECT] key found on the operator panel next to the [TRANSMIT] key.
Chapter 30 Using a 9/Series Dual--processing System Editing a Part Program An “E” next to the program name on the part program directory screen indicates that the program is currently being edited. Only one program can be open for editing at a time. You cannot edit programs in more than one process at the same time. You cannot edit a program that is currently active (selected to run) in a different process.
Chapter 30 Using a 9/Series Dual--processing System Error Messages The control displays error messages on the screen for only the currently active process (except on split-screens). The name of the currently active process flashes in reverse video if an error occurs in another process. Change to the appropriate process to display the current errors for that process. On a split-screen display, the control displays the full error messages for both processes, regardless of which process is currently active.
Chapter 30 Using a 9/Series Dual--processing System Reset Operations Dual-process systems have a process reset operation, in addition to the normal block reset and control reset functions. These reset operations work as follows: If you want to perform a: Press: The control will: Block Reset [RESET] Skip the currently active block in the currently selected process (see chapter 2).
Chapter 30 Using a 9/Series Dual--processing System 30.3 Synchronizing Multiple Part Programs On some machines or systems, it is often necessary to synchronize the operations of 9/Series dual processes. For example, if one process is drilling holes while the second process is tapping the holes, it is extremely important that the drilling process completes before the second process attempts tapping of the hole. Figure 30.
Chapter 30 Using a 9/Series Dual--processing System Synchronization M-codes are ignored during QuickCheck execution and during a Mid-Program Start operation. Example 30.1 Example of Synchronization for Tapping (see Figure 30.1) Process 1 Comment N10 G90 S500 G00 X0 Y0; Start spindle and move to start point N20 G81 X-- 1 Y5.5 R3 Z1; Drilling hole at X5.7 Y0 N40 M100; Release process 2 block N3 N60 M101; Comment N1 G90 G00 X-- 2.
Chapter 30 Using a 9/Series Dual--processing System Example 30.2 Incorrect Use of Simple Synchronization with Shared Paramacro Parameters Process 1 Comment N17 #7100=100; Paramacro parameter 7100 is set to 100 Process 2 Comment N32 M100; Process pauses waiting for M100 in process 1. Block N33 is set up in buffer prepared for execution. N33 X#7100; Destination of this block is dependent on when this block was read into the setup buffer.
Chapter 30 Using a 9/Series Dual--processing System Important: You cannot use these synchronization with setup M--codes when cutter compensation is active. Use one of the simple synchronization M--codes or turn off cutter compensation before programming the synchronization with setup M--code. Coordinating Synchronization Between Processes Remember that both processes are executing coordinated part programs.
Chapter 30 Using a 9/Series Dual--processing System Synchronization in MDI Mode Synchronization M-codes can be programmed in MDI mode. These can prove useful when attempting to manually start multiple programs from some point other than the beginning or when it is necessary to execute MDI programs on both processes simultaneously.
Chapter 30 Using a 9/Series Dual--processing System For example, press to place process 1 in cycle suspend mode, while process 1 is waiting for process 2 to execute an M101. Later, when you request for process 1, the synchronization M-code is re-activated and process 1 is again paused, waiting for process 2 to execute an M101. If, while process 1 is in cycle suspend mode, process 2 executed an M101, process 2 pauses at that synchronization block.
Chapter 30 Using a 9/Series Dual--processing System CAUTION: These interference boundaries only help prevent collision with another interference boundary configured for another process. They do not protect against collisions with other machine fixtures that may or may not be protected by a programmable zone or software overtravel. They do not account for any tool offsets that are active at the time. They are absolute positions. Figure 30.
Chapter 30 Using a 9/Series Dual--processing System Activating Interference Checking The interference boundaries for each process are entered into the interference checking tables. These tables relate the boundaries to specific tool or offset geometries. The system installer selects the number of boundaries that are available (from 1-32) for each process. Each process can have a different interference boundary number active at the same time.
Chapter 30 Using a 9/Series Dual--processing System Using Interference Checking to Prevent Collisions When two protected areas are about to collide, the control suspends motion, stopping one or both of the processes and preventing a collision. In Example 30.6, process 1 collides with process 2. Since process 2 is stationary, the control puts process 1 in cycle suspend to prevent a collision. Once the control detects the collision, it suspends the action. Interference checking operates in real time.
Chapter 30 Using a 9/Series Dual--processing System 30.5.1 Measuring Interference Boundaries The control can store as many as 32 different boundaries for each process. Two separate areas make up each of these boundaries. Both axes are activated when the boundary is activated through PAL. Figure 30.4 illustrates the use of two areas to make up interference boundary 01. Figure 30.4 Using Two Areas to Define an Interference Checking Boundary Area 2 Area 1 These areas define an interference boundary.
Chapter 30 Using a 9/Series Dual--processing System Figure 30.
Chapter 30 Using a 9/Series Dual--processing System CAUTION: The distance between the boundaries before a collision is detected is dependant upon factors such as: speed of the axes direction of axis travel with relationship to one another For example, a programmed collision between two axes traveling at rapid directly towards one another may not be detected in time to fully stop the axes before some overlap of the interference boundary occurs.
Chapter 30 Using a 9/Series Dual--processing System 30.5.2 Entering Interference Values Manually To manually enter values into the interference checking tables, follow this procedure: 1. Press the {SYSTEM SUPORT} softkey. (softkey level 1) PRGRAM FRONT MANAGE PANEL MACRO PARAM OFFSET ERROR PASSMESAGE WORD 2. PRGRAM SYSTEM CHECK SUPORT SWITCH LANG Press the {PROGRAM PARAM} softkey. (softkey level 2) PRGRAM AMP PARAM DEVICE MONISETUP TOR TIME PARTS PTOM SI/OEM 3.
Chapter 30 Using a 9/Series Dual--processing System Figure 30.7 Interference Checking Data Table INTERFERENCE TABLE PAGE TOOL NO *1 X X Z Z PLUS MINUS PLUS MINUS AREA 1 [INCH] 1.5000 -.5000 1.5000 0.0000 1 OF 32 AREA 2 [INCH] 1.5000 -1.0000 6.0000 1.5000 SEARCH REPLCE ADD TO MORE NUMBER VALUE VALUE ZONES BACKUP INTERF 4. Select a process. Refer to the system installer’s documentation for details on selecting a process, or press the [PROC SELECT] key. 5.
Chapter 30 Using a 9/Series Dual--processing System 8. 9. 30.5.3 Entering Interference Values through Programming (G10L5 and G10L6) Enter the boundary area values as determined on page 30-16. Enter values in one of two ways: Press This Softkey: Then: Press: The New Value: {REPLCE VALUE} Type in the new value. [TRANSMIT] replaces the old value for that feedrate. {ADD TO VALUE} Type in the new value. [TRANSMIT] is added to the old value for that area.
Chapter 30 Using a 9/Series Dual--processing System This is a representation of the basic format for modifying the tables. G10 L{ 5 6 } P__ X___ Z___ I___ K___; Where : Is : L(5-6) The definition of which area in the table is being modified. L5 - Modifies the Area 1 values L6 - Modifies the Area 2 values P The boundary number of the interference boundary that is having its values changed is specified following the P address.
Chapter 30 Using a 9/Series Dual--processing System Example 30.7 Using G10 to Change the Interference Boundaries N1 G90 G20; N2 G10 L5 P1 Z20 K13 X19 I15; Boundary number 1 area 1 is defined. N3 G10 L6 P1 Z23 K20 X21 I10; Boundary number 1 area 2 is defined. Figure 30.8 Resulting Boundary from Example 30.7 +X Process 1 23” 20” 13” Area 1 21” Machine Home Process 1 19” Area 2 15” Machine Coordinate System Zero Point (Both Processes) 10” +Z 12608-I 30.5.
Chapter 30 Using a 9/Series Dual--processing System To back up the interference tables, follow these directions: 1. Press the {SYSTEM SUPORT} softkey. (softkey level 1) PRGRAM FRONT MANAGE PANEL MACRO PARAM OFFSET ERROR PASSMESAGE WORD 2. PRGRAM SYSTEM CHECK SUPORT SWITCH LANG Press the {PRGRAM PARAM} softkey. (softkey level 2) PRGRAM AMP PARAM DEVICE MONISETUP TOR TIME PARTS PTOM SI/OEM 3.
Chapter 30 Using a 9/Series Dual--processing System Figure 30.9 Backup Interference Boundary Screen STORE TO BACKUP INTERFERENCE TABLE TO TO TO PORT A PORT B FILE 5. Determine the destination for the G10 program: To Send the G10 Program To: Press This Softkey: Go to Step: peripheral attached to port A {TO PORT A} 7. a peripheral attached to port B {TO PORT B} 7. to control memory {TO FILE} 6. 6. Press the {TO FILE} softkey. The control asks for a program name.
Chapter 30 Using a 9/Series Dual--processing System 30.6 Shared Axes on Dual- processing Systems Your system installer can configure an axis to be shared by different processes. With this feature multiple processes can execute part program commands or perform manual operations on the same shared axis. A shared axis can not be commanded by more than one process simultaneously. Control of the shared axis must be changed from process to process thru the system installer’s PAL program. 30.6.
Chapter 30 Using a 9/Series Dual--processing System Block Retrace Any part program blocks prior to an axis process switch can not be retraced. If you attempt to retrace beyond the point that an axis switch occurred, the control generates an error. Also an axis process switch can not be performed if you are currently performing a block retrace. Scaling Scaling is performed on a per process basis. If you switch processes for a scaled axis, scaling is removed in the new process.
Chapter 30 Using a 9/Series Dual--processing System 30.6.2 Switching a Shared Axis to a Different Process The system installer determines what axes are shared and how a shared axis is changed from process to process. Using AMP and PAL the system installer determines the process for a shared axis at power up, control reset, and E-STOP reset. Refer to your system installer’s documentation for details.
Chapter 30 Using a 9/Series Dual--processing System 30.6.3 Setting up a Shared Axis Your system installer performs the majority of set up operations in PAL and AMP to define a shared axis configuration. This section covers operations you should perform on the control to properly operate the shared axis.
Chapter 30 Using a 9/Series Dual--processing System You can not change the offset for an axis that is not currently assigned to the process through a part program (G52, and G92). You can however change coordinate system tables without the shared axis being in the process using PAL or by manually inputting the data through the {OFFSET} softkey. If the shared axis is not in the process activating the new work coordinate system (G54-G59.
Chapter 30 Using a 9/Series Dual--processing System 30.7 Dual Axes on a Dual- processing System The Dual Axis feature allows the part programmer to simultaneously control multiple axes while programming commands for only one. It differs from the split axis feature of the control in that the split axis feature is used to control a single axis positioned by two servo motors.
Chapter 30 Using a 9/Series Dual--processing System 30.7.1 Decoupling a Dual Axis Group A dual axis group is assigned in AMP to a specific process. All axes in the dual group must be configured to be part of the dual axis group and must be AMPed to be in the same process (called the default process for the group). Dual axes can only exist as a dual group in their respective default process. You can not share a dual group as an axis with another process.
Chapter 30 Using a 9/Series Dual--processing System Other restrictions are as follows: If the dual axis is currently: Then: performing a manual motion (including continuous, incremental, or handwheel jog, homing, jog on the fly, or angled jogs) the request to decouple that axis is ignored until the manual motion is completed being positioned by the PAL axis mover the request to decouple that axis is ignored until the PAL axis mover has completed moving the dual axis in the active plane and cutter c
Chapter 30 Using a 9/Series Dual--processing System An axis that is decoupled from its dual group can have an integrand letter assigned to it in AMP by the system installer. This integrand is used with that axes originally assigned AMP axis name to perform functions such as circular interpolation. Plane dependant operations (such as circular interpolation or cutter compensation) are available to a dual axes while coupled (provided the dual axis is defined in the active plane).
Chapter 31 Using Transfer Line Cycles 31.0 Chapter Overview This chapter details the user-defined cycles that are included with the transfer line option.
Chapter 31 Using Transfer Line Cycles 31.
Chapter 31 Using Transfer Line Cycles 31.1.1 Using Transfer Line Cycles The cycles for the transfer line are user-defined. With the transfer line option, there are 19 templates that perform drilling, boring and transfer line functions. You can customize pre-written templates by using QuickView. In QuickView, there is a screen for each cycle. On each screen there is a graphic representation of each cycle and prompts with which you customize the program.
Chapter 31 Using Transfer Line Cycles N00001(QV09 BORING CYCLE G85) N00002(DRILL SLIDE VARIABLES) N00003IF[#1131EQ0]GOTO26 (INITIALIZES VARIABLES ONE TIME) N00004#500=90 (G90/G91) N00005#501=10 (HOLE POSITION 1ST AXIS) N00006#502=0 (HOLE POSITION 2ND AXIS) N00007#503=15 (DEPTH OF HOLE) N00008#504=12 (CLEAR POSITION) N00009#505=15 (FULL RETURN POSITION 1ST AXIS) N00010#506=0 (FULL RETURN POSITION 2ND AXIS) N00011#507=200 (FEEDRATE) N00012#508=0 (TOOL CHANGE POSITION) N00013#509=.
Chapter 31 Using Transfer Line Cycles Using QuickView to Customize the Cycles Though your transfer line control comes with part program templates, you need to customize that template into a working part program for your application. QuickView prompts that are designed to work with the part program templates let you to modify your program template. In QuickView, the illustrations vary slightly for drilling/boring cycles and transfer cycles.
Chapter 31 Using Transfer Line Cycles 31.1.2 Selecting the Program to Edit or Create Before you begin editing a part program, the control needs to be in E-stop or the bit for Stop Program Cycle for Local Manual Control must be set. 1. Press the {PRGRAM MANAGE} softkey. The program directory screen is displayed. (softkey level 1) PRGRAM OFFSET MACRO MANAGE PARAM QUICK CHECK FRONT PANEL SWITCH LANG ERROR PASSMESAGE WORD SYSTEM SUPORT Figure 31.
Chapter 31 Using Transfer Line Cycles 2. Type 1 for the selected program name and then press {EDIT PRGRAM}. The control names the created part program O00001. (softkey level 2) ACTIVE EDIT RESTRT DISPLY COPY PRGRAM PRGRAM PRGRAM PRGRAM PRGRAM VERIFY PRGRAM DELETE RENAME INPUT PRGRAM COMENT PRGRAM PRGRAM DEVICE REFORM MEMORY Figure 31.
Chapter 31 Using Transfer Line Cycles 3. From the edit menu, press the {QUICK VIEW} softkey. (softkey level 3) MODIFY BLOCK BLOCK DELETE EXIT INSERT DELETE TRUNC CH/WRD EDITOR STRING RENUM MERGE QUICK CHAR/ SEARCH PRGRAM PRGRAM VIEW WORD DIGITZ E 4. The softkey functions will change to those indicated below.
Chapter 31 Using Transfer Line Cycles 31.1.3 Creating a Transfer Line Part Program The control prompts you for information it needs to create part programs. To select the cycle you want to create a part program for, and enter the information for the cycle, follow these steps: 1. From the QuickView menu press the {TRNSFR PROMPT} softkey. The transfer line cycle selection screen appears.
Chapter 31 Using Transfer Line Cycles 3. Once the correct cycle is selected, press the {SELECT} softkey. A screen with prompts for that cycle and a graphical representation of that cycle is displayed. SINGLE AXIS TRANSFER CYCLE F1 X2 I X1 TRANSFER VELOCITY FULL ADVANCE POSITION FULL RETURN POSITION HARD STOP SENSE ZONE F1_____ X1_____ X2_____ I______ F1 STORE 4. Use the up and down cursor keys to select the parameters to be changed or entered. The selected item is shown in reverse video.
Chapter 31 Using Transfer Line Cycles 6. After all data for the cycle has been entered store the data by pressing the {STORE} softkey. (softkey level 6) STORE The control will generate the cycle’s part program. See the section titled Editing Part Programs to adjust your settings. 7. Press the {EXIT EDITOR} softkey to leave the editor and make the program available for execution.
Chapter 31 Using Transfer Line Cycles 31.1.4 Editing Part Programs Once you press the [STORE] softkey, the control generates a part program. Here is an example of a part program that the control generates: INSERT : EDIT FILE : 000001 POS 1*1 MODE : CHAR N00001(QV15 SINGLE AXIS TRANSFER CYCLE) N00002(TRANSFER VARIABLES) N00003IF[#1131EQ0]GOTO29 (INITIALIZES VARIABLES ONE TIME) N00004#500=195 (TRANSFER VELOCITY) N00005#501=1.234 (FULL ADVANCE POS.) N00006#502=5.678 (FULL RETURN POS.) N00007#503=4.
Chapter 31 Using Transfer Line Cycles Changing the Part Program through QuickView If you need to modify the program, you can do so by entering different information at the prompts in QuickView. Since the control generates a new part program after you save the QuickView changes, you need to delete or rename the previous program you made with QuickView before you enter new information.
Chapter 31 Using Transfer Line Cycles Table 31- A Standard T-Line-9 Paramacro Variables 31-14 Paramacro When a 1 is assigned to this value, the control: 1000 raises the transfer bar during a transfer cycle 1001 lowers the transfer bar during a transfer cycle 1002 advances the transfer bar or completes the drill cycle 1003 returns the transfer bar or retracts the tool 1004 stops the part program execution for any manual operations that need to be performed on the station.
Chapter 31 Using Transfer Line Cycles If you want to activate a paramacro through remote I/O or through the fiber optic ring, use this table to determine what remote I/O flag or ring point is assigned to each variable: Paramacro Variables QV# Application 1000 1102 1103 1104 01 Drilling Cycle, No Dwell/Rapid Out H H H H H H H 02 Drilling Cycle, Dwell/Rapid Out H H H H H H H 03 Deep Hole Drill Cycle, Chip Clear H H H H H H H 04 Deep Hole Drill Cycle, Chip Break H H H H
Chapter 31 Using Transfer Line Cycles Changing the Program with the Part Program Editor You can change program generated by QuickView with the part program editor. To learn how to use the part program editor, refer to the appropriate chapter in this manual. The changes you make to to the part program will be specific to that part program and will not change the templates. The templates are kept in the protected directory, and are used by QuickView every time it generates a program.
Chapter 31 Using Transfer Line Cycles 31.1.5 Reloading Part Program Templates Part program templates were loaded on your control when it was shipped from Allen-Bradley. They are however stored in a volatile area of control memory (requires power to be maintained). Common causes for losing the part program templates stored in this area are: Memory Lost Because: Detail: Power Loss The control comes standard with 5 to 7 days of supercap power to maintain volatile memory.
Chapter 31 Using Transfer Line Cycles Important: When a transfer line program template is downloaded from ODS to the control, it must be inserted into the protected program directory on the control. You can do this by selecting the protected directory on the control before beginning the download. The protected directory can be password protect to help prevent unauthorized edits. Refer to your 9/Series operation and programming manual for details.
Chapter 31 Using Transfer Line Cycles 3. Press [F3] to pull down the Application menu. The workstation displays this screen: Proj: TRAN230 F1 - File Appl: Upload F2 - Project Util: Get PAL I/O F3 - Application F4 - Utility AMP PAL I/O Assignments Part Program Upload Download (A) (P) (I) (R) (U) (D) F5 - Configuration 4. Use the arrow keys to highlight the Download application then press [ENTER] or press [D]. 5. Press [F4] to pull down the Utility menu.
Chapter 31 Using Transfer Line Cycles 6. Use the arrow keys to highlight the Send Part Program option then press[ENTER], or press [R].
Chapter 31 Using Transfer Line Cycles 7. Use the arrow keys to highlight the control as the download destination and press [ENTER], or press [C]. The workstation displays the part program files that are stored in the active project directory of the workstation: Proj: TRAN230 Appl: Download F1 - File F2 - Project F3 - Application Util: File Management F5 - Configuration F4 - Utility Downloading Use ARROW keys or Type in name. QVO1 QV11 QV02 QV12 8.
Chapter 31 Using Transfer Line Cycles If some of the program templates still exist in control memory, the workstation displays this screen: Proj: TRAN230 F1 - File Appl: Download F2 - Project F3 - Application Util: Send Part Program F4 - Utility F5 - Configuration File Already Exits Enter Option Rename existing file Overwrite existing file Abort current file (R) (O) (A) Select Overwrite existing file and press [ENTER], or press [O].
Chapter 31 Using Transfer Line Cycles Proj: TRAN230 Appl: Download F1 - File F2 - Project F3 - Application Util: Send Part Program F4 - Utility F5 - Configuration Download In Progress Percent completed 50% The percentage of the download process that has currently been completed is displayed on the screen. This value is updated continually throughout the download process.
Chapter 31 Using Transfer Line Cycles If the workstation is unable to complete the download procedure in the allotted time frame due to communication failure, it displays this screen: Proj: TRAN230 F1 - File Appl: Download F2 - Project F3 - Application Util: Send Part Program F4 - Utility F5 - Configuration A time-out occurred ... Press any key to continue ... Press any key to return to the ODS main menu. If the Download Failed If the download failed and the message “A time--out occurred ...
Chapter 31 Using Transfer Line Cycles 31.1.6 Running the Cycles Once you enter information in the QuickView screens, the cycle acts just like a part program. The program runs within these conditions: G90 -- all the cycles operate in absolute mode. If you enter try to a G91 into the QuickView prompt you’ll get an error message. WARNING: If you enter a G91 into a transfer line part program, the control will run in incremental mode, even though the program was designed for absolute mode.
Chapter 31 Using Transfer Line Cycles Template 1: Drilling Cycle, No Dwell/Rapid Out Letter Paramacro Label Description G 500 G90/91 G-codes G90 or G91 for absolute or incremental modes. At this time only absolute mode, G90, is available. X,Y 501, 502 HOLE POSITION X, Y The location to which the tool moves before it begins a drilling operation. X 503 DEPTH OF HOLE The location to which the tool drills into the part.
Chapter 31 Using Transfer Line Cycles Figure 31.
Chapter 31 Using Transfer Line Cycles Template 2: Drilling Cycle, Dwell/Rapid Out Letter Paramacro Label Description G 500 G90/91 G-codes G90 or G91 for absolute or incremental modes. At this time only absolute mode, G90, is available. X,Y 501, 502 HOLE POSITION X, Y The location to which the tool moves before it begins a drilling operation. X 503 DEPTH OF HOLE The location to which the tool drills into the part.
Chapter 31 Using Transfer Line Cycles Figure 31.
Chapter 31 Using Transfer Line Cycles Template 3: Deep Hole Drill Cycle, Chip Clear Letter Paramacro Label Description G 500 G90/91 G-codes G90 or G91 for absolute or incremental modes. At this time only absolute mode, G90, is available. X,Y 501, 502 HOLE POSITION X, Y The location to which the tool moves before it begins a drilling operation. X 503 DEPTH OF HOLE The location to which the tool drills into the part.
Chapter 31 Using Transfer Line Cycles Figure 31.
Chapter 31 Using Transfer Line Cycles Template 4: Deep Hole Drill Cycle, Chip Break Letter Paramacro Label Description G 500 G90/91 G-codes G90 or G91 for absolute or incremental modes. At this time only absolute mode, G90, is available. X,Y 501, 502 HOLE POSITION X, Y The location to which the tool moves before it begins a drilling operation. X 503 DEPTH OF HOLE The location to which the tool drills into the part.
Chapter 31 Using Transfer Line Cycles Figure 31.
Chapter 31 Using Transfer Line Cycles Template 5: Right- Hand Tapping Cycle Letter Paramacro Label Description G 500 G90/91 G-codes G90 or G91 for absolute or incremental modes. At this time only absolute mode, G90, is available. X,Y 501, 502 HOLE POSITION X, Y The location to which the tool moves before it begins a tapping operation. X 503 DEPTH TO TAP The location to which the tool taps into the part. R 504 CLEAR POSITION The location the tool retracts to after an operation.
Chapter 31 Using Transfer Line Cycles Template 6: Right- Hand Solid-Tapping Cycle Letter Paramacro Label Description G 500 G90/91 G-codes G90 or G91 for absolute or incremental modes. At this time only absolute mode, G90, is available. X,Y 501, 502 HOLE POSITION X, Y The location the tool moves to before it begins a tapping operation. X 503 DEPTH TO TAP The location where the tool completes the tap into the part.
Chapter 31 Using Transfer Line Cycles Template 7: Left-Hand Tapping Cycle Letter Paramacro Label Description G 500 G90/91 G-codes G90 or G91 for absolute or incremental modes. At this time only absolute mode, G90, is available. X,Y 501, 502 HOLE POSITION X, Y The location the tool moves to before it begins a tapping operation. X 503 DEPTH TO TAP The location where the tool completes the tap into the part. R 504 CLEAR POSITION The location that the tool retracts to after an operation.
Chapter 31 Using Transfer Line Cycles Template 8: Left-Hand Solid Tapping Cycle Letter Paramacro Label Description G 500 G90/91 G-codes G90 or G91 for absolute or incremental modes. At this time only absolute mode, G90, is available. X,Y 501, 502 HOLE POSITION X, Y The location the tool moves to before it begins a tapping operation. X 503 DEPTH TO TAP The location where the tool completes the tap into the part.
Chapter 31 Using Transfer Line Cycles Template 9: Boring Cycle, No Dwell/Feed Out Letter Paramacro Label Description G 500 G90/91 G-codes G90 or G91 for absolute or incremental modes. At this time only absolute mode, G90, is available. X,Y 501, 502 HOLE POSITION X, Y The location to which the tool moves before it begins a boring operation. X 503 DEPTH OF HOLE The location to which the tool bores into the part.
Chapter 31 Using Transfer Line Cycles Template 10: Boring Cycle, Spindle Stop/Rapid Out Letter Paramacro Label Description G 500 G90/91 G-codes G90 or G91 for absolute or incremental modes. At this time only absolute mode, G90, is available. X,Y 501, 502 HOLE POSITION X, Y The location to which the tool moves before it begins a boring operation. X 503 DEPTH OF HOLE The location to which the tool bores into the part.
Chapter 31 Using Transfer Line Cycles Figure 31.
Chapter 31 Using Transfer Line Cycles Template 11: Boring Cycle, Spindle Shift Letter Paramacro Label Description G 500 G90/91 G-codes G90 or G91 for absolute or incremental modes. At this time only absolute mode, G90, is available. X,Y 501, 502 HOLE POSITION X, Y The location to which the tool moves before it begins a boring operation. X 503 DEPTH TO TAP OR HOLE The location to which the tool bores into the part.
Chapter 31 Using Transfer Line Cycles Figure 31.
Chapter 31 Using Transfer Line Cycles Template 12: Back Boring Cycle Letter Paramacro Label Description G 500 G90/91 G-codes G90 or G91 for absolute or incremental modes. At this time only absolute mode, G90, is available. X,Y 501, 502 HOLE POSITION X, Y The location to which the tool moves before it begins a boring operation. X 503 DEPTH OF HOLE The location to which the tool bores into the part. R 504 CLEAR POSITION The location that the tool retracts to after an operation.
Chapter 31 Using Transfer Line Cycles Template 13: Boring Cycle, Dwell/Feed Out Letter Paramacro Label Description G 500 G90/91 G-codes G90 or G91 for absolute or incremental modes. At this time only absolute mode, G90, is available. X,Y 501, 502 HOLE POSITION X, Y The location to which the tool moves before it begins a boring operation. X 503 DEPTH OF HOLE The location to which the tool bores into the part. R 504 CLEAR POSITION The location that the tool retracts to after an operation.
Chapter 31 Using Transfer Line Cycles Template 14: Single Axis Lift Cycle Letter Paramacro Label Description F1 500 MAX. LIFT VELOCITY The velocity of the bar goes when it approaches a part before the low soft touch position, and after the soft touch high position. F2 501 SOFT TOUCH VELOCITY The velocity of the bar when it goes between the soft touch low position and soft touch high position.
Chapter 31 Using Transfer Line Cycles Template 15: Single Axis Transfer Cycle Letter Paramacro Label Description F1 500 TRANSFER VELOCITY The velocity of the bar as it transfers the part to the station. X1 501 FULL ADVANCE POSITION The location that indicates that the part has been fully transferred to the station. X2 502 FULL RETURN POSITION The location that indicates that the bar has returned to the station it started at.
Chapter 31 Using Transfer Line Cycles Template 16: Two-Axis Transfer Bar Cycle Letter Paramacro Label Description F1 500 MAX. LIFT VELOCITY The velocity of the bar goes when it approaches a part before the low soft touch position, and after the soft touch high position. F2 501 SOFT TOUCH VELOCITY The velocity of the bar when it goes between the soft touch low position and soft touch high position.
Chapter 31 Using Transfer Line Cycles Template 17: Single Axis Cross Cycle Letter Paramacro Label Description F1 500 CROSS FEEDRATE The velocity of the tool as it traverses the part. This is the maximum feedrate if the adaptive feed feature is used. X1 501 CROSS FINAL POSITION The final position of the tool after it traverses the part. X2 502 CROSS RETURN POSITION The position of the slide when it started the cycle.
Chapter 31 Using Transfer Line Cycles Figure 31.
Chapter 31 Using Transfer Line Cycles Template 18: Single Axis Feed Cycle Letter Paramacro Label Description F1 500 MAIN RAPID FEEDRATE The velocity of the tool as it approaches the part. X1 501 MAIN FEED START The position of the tool as it drills into the part. F2 502 MAIN FEEDRATE The velocity of the tool as it drills into the part. X2 503 MAIN FINAL POSITION The depth of the tool at its final position in the part.
Chapter 31 Using Transfer Line Cycles Template 19: Two-Axis Cross Feed Cycle Letter Paramacro Label Description F1 500 MAIN RAPID FEEDRATE The velocity of the tool as it approaches the part. X1 501 MAIN FEED START The position of the tool as it drills into the part. F2 502 MAIN FEEDRATE The velocity of the tool as it drills into the part. X2 503 MAIN FINAL POSITION The depth of the tool at its final position in the part.
Chapter 31 Using Transfer Line Cycles Figure 31.
Appendix A Softkey Tree Appendix Overview This appendix explains softkeys and includes maps of the softkey trees. Understanding Softkeys We use the term softkey to describe the row of 7 keys at the bottom of the CRT. The function of each softkey is displayed on the CRT directly above the softkey. Softkey names are shown in this manual between the { } symbols. Softkeys are often described in this manual as being on a certain level, for example, softkey level 3.
Appendix A Softkey Tree For example : (softkey level 1) PRGRAM OFFSET MACRO MANAGE PARAM PRGRAM SYSTEM CHECK SUPORT When softkey level 1 is reached, the previous set of softkeys is displayed. Press the continue softkey {• } to display the remaining softkey functions on softkey level 1. (softkey level 1) FRONT PANEL ERROR PASSMESAGE WORD SWITCH LANG On softkey level 1, the exit softkey is not displayed since the softkeys are already on softkey level 1.
Appendix A Softkey Tree Describing Level 1 Softkeys (softkey level 1) PRGRAM OFFSET MACRO MANAGE PARAM PRGRAM SYSTEM CHECK SUPORT FRONT PANEL SWITCH LANG ERROR PASSMESAGE WORD If you want to: Press: Edit, activate, or copy a program from a peripheral or control memory {PRGRAM MANAGE} Display or enter tool offset data, the work coordinate system offset data, etc.
Appendix A Softkey Tree AXIS POSITION DISPLAY FORMAT SOFTKEYS PRGRAM A B S TARGET D T G AXIS SELECT M CODE STATUS PRGRAM D T G A L L G CODE STATUS SPLIT ON/OFF A-4 NOTE: The first 4 softkeys (from PRGRAM to DTG) toggle between small and large screen display.
Appendix A Softkey Tree THE FUNCTION SELECT SOFTKEYS LEVEL 1 WITH POWER UP (AXIS POSITION) DISPLAY SCREEN Optional PAL flag set to display “front panel” when MTB is not part of the total CNC system PRGRAM MANAGE see page A-6 OFFSET see page A-7 MACRO PARAM see page A-9 PRGRAM CHECK see page A-10 SYSTEM SUPORT see page A--11 FRONT PANEL see page A-13 ERROR MESAGE see page A-13 PASSWORD see page A-14 SWITCH LANG PAL Display Page Option: Five softkeys available on third screen.
Appendix A Softkey Tree PRGRAM MANAGE level 1 level 2 PRGRAM MANAGE ACTIVE PRGRAM EDIT PRGRAM level 3 level 4 see page A-15 see page A-16 EXEC RESTRT PRGRAM QUIT EXIT DISPLY PRGRAM MEM TO PORT A COPY PRGRAM FROM A TO MEM MEM TO PORT B FROM B TO MEM MEM TO MEM DELETE YES DELETE PRGRAM VERIFY PORT A VERIFY PORT B VERIFY MEMORY PRGRAM COMENT RENAME YES RENAME PRGRAM RENAME NO FROM PORT A FROM PORT B FROM MEMORY INPUT.
Appendix A Softkey Tree OFFSET (Lathe & Mill) level 1 level 2 level 3 level 4 level 5 REPLCE VALUE OFFSET WORK CO-ORD ADD TO VALUE INCH/ METRIC RADI/ DIAM (lathe only) MORE OFFSET SEARCH NUMBER REPLCE VALUE ADD TO VALUE ACTIVE OFFSET MORE.
Appendix A Softkey Tree OFFSET (Grinder) level 1 level 2 level 3 level 4 REPLCE VALUE OFFSET WORK CO-ORD ADD TO VALUE INCH/ METRIC RADI/ DIAM (cylindrical only) MORE OFFSET MODIFY LABEL SEARCH NUMBER REPLCE VALUE WHEEL GEOM ADD TO VALUE CHANGE OFFSET MORE.
Appendix A Softkey Tree MACRO PARAM level 1 level 2 level 3 SEARCH NUMBER MACRO PARAM LOCAL PARAM REFRSH SCREEN SEARCH NUMBER COM-1 PARAM REPLCE VALUE ZERO VALUE 0 ALL VALUES REFRSH SCREEN SEARCH NUMBER REPLCE VALUE ZERO VALUE REPLCE NAME COM-2A PARAM CLEAR NAME CLEAR ALL NM COM-2B PARAM SHARED PARAM 0 ALL VALUES REFRSH SCREEN A-9
Appendix A Softkey Tree PRGRAM CHECK level 1 PRGRAM CHECK level 2 level 3 SELECT PRGRAM ACTIVE PRGRAM DE-ACT PRGRAM QUICK CHECK level 4 CLEAR GRAPH MACHIN INFO GRAPH ZOOM WINDOW SYNTAX ONLY ZOOM BACK GRAPH SETUP STOP CHECK T PATH GRAPH T PATH DISABL A-10 level 5 DEFALT PARAM SAVE PARAM
Appendix A Softkey Tree SYSTEM SUPPORT level 1 level 2 level 3 level 4 level 5 REPLCE VALUE SYSTEM SUPORT PRGRAM PARAM (lathe only) DRLCYC PARAM ZONE LIMITS ADD TO VALUE MORE LIMITS F1-F9 UPDATE & EXIT MILCYC PARAM PROBE PARAM QUIT REPLCE VALUE ADD TO VALUE UPDATE & EXIT (mill only) QUIT REVERS ERROR AMP AXIS PARAM HOME CALIB AXIS CALIB SERVO PARAM SPNDL PARAM PATCH AMP REPLCE VALUE SEARCH NUMBER UPDATE & EXIT UPDATE BACKUP TO BACKUP FROM BACKUP REPLCE VALUE INSERT POINT DELETE P
Appendix A Softkey Tree SYSTEM SUPPORT (continued) level 1 level 2 level 3 level 4 level 5 Continued from previous page DISPLY RING I/O SYSTEM SUPORT MONI-TOR REMOTE I/O FAST I/O AXIS MONITOR SERIAL I/O RECOVR ENABLE START RECOVR DISABL STOP @ AXIS RECV PORT A @ = AXIS NAME SINGLE XMIT RECV PORT B START XMIT PORT A STOP XMIT PORT B REPEAT XMIT SINGLE XMIT DATA SCOPE SEARCH MONITR PORT A PORT B 1394 DRIVES FORWD SEARCH REVRSE SEARCH SET TIME ADJUST VIEW SET DATE SYMBOL COMENT ED PR
Appendix A Softkey Tree FRONT PANEL level 1 FRONT PANEL level 2 JOG AXIS level 4 level 3 SET ZERO JOG AXES+ JOG AXES-- PRGRAM EXEC BLOCK RETRCE JOG AXES+ JOG RETRCT JOG AXES-- CYCLE START CYCLE STOP ERROR MESAGE level 1 ERROR MESAGE level 2 ERROR LOG CLEAR ACTIVE level 3 ACTIVE ERRORS FULL MESAGE TIME STAMPS This softkey toggles between [TIME STAMPS] and [FULL MESAGE] A-13
Appendix A Softkey Tree PASSWORD level 1 PASSWORD level 2 ACCESS CONTRL level 3 UPDATE & EXIT 01 (NAME) 02 (NAME) 03 (NAME) 04 (NAME) UPDATE & EXIT 05 (NAME) 06 (NAME) 07 (NAME) 08 (NAME) STORE BACKUP A-14 (NAME) = PASSWORD NAME
Appendix A Softkey Tree ACTIVE PRGRAM level 2 level 3 level 4 level 5 level 6 FORWRD ACTIVE PRGRAM REVRSE DE-ACT PRGRAM TOP OF PRGRAM CANCEL N SEARCH SEARCH EXIT O SEARCH EOB SEARCH FORWRD SLEW REVRSE STRING SEARCH TOP OF PRGRAM CANCEL EXIT CONT MID ST PRGRAM SEQ # SEARCH TOP OF PRGRAM STRING SEARCH QUIT EXIT T PATH GRAPH CLEAR GRAPHS MACHNE INFO ZOOM WINDOW ZOOM BACK T PATH DISABL GRAPH SETUP INCR WINDOW DECR WINDOW ZOOM ABORT ZOOM DEFALT PARAM SEQ STOP TIME PARTS SAVE PARAM
Appendix A Softkey Tree EDIT PRGRAM level 2 EDIT PRGRAM level 3 level 4 level 5 MODIFY INSERT BLOCK DELETE FORWRD BLOCK TRUNC DELETE CH/WRD REVRSE EXIT EDITOR TOP OF PRGRAM BOT OF PRGRAM STRING SEARCH ALL RENUM PRGRAM MERGE PRGRAM QUICK VIEW ONLY N see page A-17 EXEC CHAR/ WORD LINEAR DIGITZ E CIRCLE 3 PNT CIRCLE TANGNT MODE SELECT STORE END PT EDIT & STORE RECORD MID PT STORE END PT EDIT & STORE INCH/ METRIC ABS/ INCR PLANE SELECT DIA/ RADIUS A-16 (lathe only)
Appendix A Softkey Tree QUICK VIEW level 3 MILL QUICK VIEW level 4 QPATH+ PROMPT level 5 level 6 see page A-18 G CODE PROMT SELECT MILL PROMPT SET PLANE SELECT G17 STORE G18 G19 LATHE QUICK VIEW QPATH+ PROMPT G CODE PROMT SELECT DRILL PROMPT SET LATHE PROMPT PLANE SELECT G17 STORE G18 G19 A-17
Appendix A Softkey Tree QPATH+ PROMPT level 4 level 5 level 6 QPATH+ PROMPT CIR ANG PT STORE CIR CIR ANG CIR PT ANG PT 2ANG PT 2ANG PT R 2PT R 2ANG PT C 2PT C 2ANG 2PT 2R 3PT 2R 2ANG 2PT 2C 3PT 2C 2ANG 2PT RC 3PT RC 2ANG 2PT CR 3PT CR END OF APPENDIX A-18
Appendix B Error and System Messages Overview This appendix serves as a guide to error and system messages that can occur during programming and operation of the 9/Series control. We listed the messages in alphabetical order along with a brief description. Important: To display both active and inactive messages, press the {ERROR MESAGE} softkey found on softkey level 1. For details, see chapter 2. Important: This appendix covers only error and system messages.
Appendix B Error and System Messages Message Description 2 2MB RAM IS BAD/MISSING The control has discovered the RAM SIMMs for the two megabyte extended storage option are either damaged or missing. The RAM SIMMs must be installed or replaced. Contact your Allen Bradley sales representative for assistance. 9 9/SERIES LATHE - CANNOT USE MILL AMP The control was powered up with a lathe software option chip installed, when the AMP file that was downloaded was configured for a mill.
Appendix B Error and System Messages Message Description AMP WAS MODIFIED BY PATCH AMP UTILITY This message always appears after changes have been made to AMP using the patch AMP utility. Its purpose is to remind the user that the current AMP has not been verified by a cross-reference check normally performed by ODS. It is meant as a safety warning.
Appendix B Error and System Messages Message Description AXIS INVALID FOR G24/G25 The programmed axis was not AMPed for software velocity loop operation, and can not be used in a G24 or G25 block. To use these features the axis programmed must be configured for tachless operation (or be a digital servo).
Appendix B Error and System Messages Message Description BAD RAM DISC SECTOR CHECKSUM ERROR A RAM disk sector error was detected during the RAM checksum test at power-up. Attempt to power-up again. If the error remains, contact Allen-Bradley customer support services. BAD RECORD IN PROGRAM This indicates a serious problem with the program. Attempt to open the program a second time. If retry doesn’t work, you may have to delete the program.
Appendix B Error and System Messages Message Description CANNOT COPY The requested copying task cannot be performed due to an internal problem in the file or RAM disk. Contact Allen-Bradley customer support service. CANNOT DELETE - OPEN PROGRAM The selected program is either active or open for editing and cannot be deleted.
Appendix B Error and System Messages Message Description CANNOT RENAME When performing a rename of a program name, the new program name has not been correctly entered. The format is OLD PROGRAM NAME,NEW PROGRAM NAME. CANNOT REPLACE START POINT An illegal attempt was made to change the axis calibration start-point using the online AMP feature. CANNOT RESTART G24 HARD STOP An attempt was made to restart a part program on a block which would have an axis at the hard stop.
Appendix B Error and System Messages Message Description CHARACTERS MUST FOLLOW WILDCARD You have used incorrect search string syntax in the PAL search monitor utility. CHECKSUM ERROR IN FILE The file (AMP, PAL) being downloaded from a storage device has a checksum error. The file cannot be used. CIRCLE MID-POINT NOT ENTERED The center-point of an arc is not entered in a circular programming block. Circular blocks require programming either an R or an I, J, K in the block.
Appendix B Error and System Messages Message Description CPU #2 HARDWARE ERROR #4 The 68030 main processor has detected an illegal address. Consult Allen-Bradley customer support services (9/290 only). CPU #2 HARDWARE ERROR #6 The 68030 main processor has detected a privilege violation. Consult Allen-Bradley customer support services (9/290 only). CPU #2 HARDWARE ERROR #8 CPU #2 has detected an unassigned vector interrupt. Consult Allen-Bradley customer support services (9/290 only).
Appendix B Error and System Messages Message CYLIND/VIRTUAL CONFIGURATION ERROR Description An axis configuration error was detected by the control when cylindrical interpolation or end face milling was requested in a program block. Some examples would include: A cylindrical/virtual axis is named same as a real axis or is missing (for example on a lathe A, the cylindrical axis may have been named the same as a incremental axis name).
Appendix B Error and System Messages Message Description DEPTH PROBE TRAVEL LIMIT The adaptive depth probe has moved to its AMPed travel limit. Note the value entered in AMP is the adaptive depth probe deflection from the PAL determined probe zero point. It may not be the actual total probe deflection. DEPTH PROBE NOT SUPPORTED A depth probe axis has been AMPed on an axis located on a servo card or a 9/230 that does not support the adaptive depth feature. (analog servo rev < rev 0.
Appendix B Error and System Messages Message Description DRESSER WARNING LIMIT REACHED The axis specified as the dresser axis has been dressed smaller than the dresser warning limit value as specified on the dresser status page. DRILL AXIS CONFIGURATION ERROR The drilling axis is not a currently configured machine axis. On dual processing controls this message may result when the drilling axis is in another process.
Appendix B Error and System Messages Message Description ENCODER QUADRATURE FAULT An error has been detected in the encoder feedback signals. Likely causes are excessive noise, inadequate shielding, poor grounding, or encoder hardware failure. END OF FILE When transferring a file over the serial port, the control has reached the last block in the program. END OF PROGRAM When displaying a part program on the CRT, the control has reached the last block in the program.
Appendix B Error and System Messages Message EXTRA KEYBOARD OR HPG ON I/O RING Description The control detected a keyboard or HPG on the 9/Series fiber optic ring that was not configured as a ring device. The I/O ring will still function and the control will NOT be held in E-Stop. You may also use the keyboard or HPG by selecting it as the active device via the corresponding PAL flags.
Appendix B Error and System Messages Message Description FLASH SIMMS CONTAIN INVALID DATA Flash SIMMs have become corrupted probably from a communication error during a system update. Retry the system executive update utility. If the situation persists, contact Allen-- Bradley support. FLASH SIMMS U10 AND U14 ARE EMPTY OR MISSING Make sure your flash SIMMs are installed in the correct tracks.
Appendix B Error and System Messages Message GRAPHICS ACTIVE IN ANOTHER PROCESS Description Graphics can only be active in one process at a time. You must turn graphics off in one process before you can activate them in another process. H HARD STOP ACTIVATION ERROR An attempt was made to (G24) hard stop an axis while a different axis was already holding against a hard stop.
Appendix B Error and System Messages Message Description HIPERFACE PASSWORD FAILURE During the SINCOS device’s alignment procedure, the logic used to set the passwords detects an incorrect password. A section of the code will repeatedly attempt various combinations of each of the passwords to correct the error condition. HOME REQUEST ON A PARKED AXIS An attempt was made, while using dual axes, to do a homing operation on a parked axis.
Appendix B Error and System Messages Message Description ILLEGAL DUAL CONFIGURATION Both dual master axes names have the same letter OR when assigning dual groups in AMP, dual groups must be assigned in contiguous order, starting with group 1, 2, 3, 4, and 5. You can not assign axes to dual group 3 without axes having been assigned to dual groups 1 and 2. ILLEGAL DUAL LINEAR/ROTARY CONFIGURATION The dual group cannot contain a mixture of linear and rotary axes.
Appendix B Error and System Messages Message Description INCOMPATIBLE TOOL ACTIVATION MODES This message is displayed and the control is held in E-Stop at power up when the tool geometry offset mode is “Immediate Shift/Immediate Move”and the tool wear offset mode is “Immediate Shift/Delay Move” or when the tool geometry offset mode is “Immediate Shift/Delay Move”and the tool wear offset mode is “Immediate Shift/Immediate Move”. These modes are incompatible.
Appendix B Error and System Messages Message Description INVALID CHECKSUM DETECTED This error is common for several different situations. Most typically it results when writing or restoring invalid data to flash memory. For example if axis calibration data is being restored to flash and there was an error or invalid memory reference in the axis calibration data file. Typically this indicates a corrupt or invalid file. INVALID CNC FILENAME An error occurred in G05 DH+ communications block.
Appendix B Error and System Messages Message Description INVALID FIXED DRILLING AXIS The axis selected as the drilling axis is an invalid axis for a drilling application. INVALID FORMAT SPECIFIED IN B/DPRNT CMD Improper format was used in the paramacro command (BPRNT or DPRNT) that outputs data to a peripheral device. INVALID FUNCTION ARGUMENT An invalid paramacro argument was used in a paramacro function. The argument contains either bad syntax or an illegal value.
Appendix B Error and System Messages Message Description INVALID PROGRAM NUMBER (P) A program number called by a sub-program or paramacro call is invalid. A P-word that calls a sub-program or paramacro can only be an all-numeric program name as many as 5 digits long. The O-word preceding the numeric program number in control memory cannot be entered with the P-word. INVALID REMOTE NODE NAME An error occurred in G05 DH+ communications block.
Appendix B Error and System Messages Message Description INVALID TOOL LENGTH OFFSET NUMBER An attempt was made to enter a tool length offset number in the tool life management table that is larger than the maximum offset number allowed. If the tables are being loaded by a G10 program, the length offset number is entered with a H-word in the block. INVALID TOOL LIFE TYPE An attempt was made to enter an invalid tool life type for a tool group in the tool management tables.
Appendix B Error and System Messages Message Description LARGER MEMORY - REFORMAT This message typically occurs after a new AMP or PAL has just been downloaded to the control. There is now more memory available for the RAM disk, but you need to reformat to use it. If desired, you do not have to reformat RAM and can continue to run the control with the RAM disk at its current size.
Appendix B Error and System Messages Message Description MAXIMUM BLOCK NUMBER REACHED A renumber operation was performed to renumber block sequence numbers (N-words), and the control has exceeded a block number of N99999. Either the program is too large to renumber, or the parameters for the first sequence number, or the sequence number increment, are too large. When this error occurs, the renumber operation stops renumbering at the last block within the legal range of N-words.
Appendix B Error and System Messages Message Description MINIMUM RPM LIMIT AUXILIARY SPINDLE 2 The commanded aux spindle 2 speed requested by the control is less than the AMPed minimum aux spindle 2 speed for the current gear being used. This requires a gear change operation or a change in the programmed aux spindle 2 speed. In some cases, the switch may be sufficient.
Appendix B Error and System Messages Message Description MISSING I/O RING DEVICE The I/O assignment file that was compiled and downloaded with PAL defines an I/O ring device that is not physically present in the I/O ring. Verify that all device address settings are correct. MISSING INTEGRAND/RADIUS WORD A circular or helical block has been programmed with axis data and no radius (R) or integrand (I, J, or K) values.
Appendix B Error and System Messages Message Description MULTIPLE FUNCTIONS NOT ALLOWED Multiple functions are not allowed. MULTIPLE SPINDLE CONFIGURATION ERROR Each multiple spindle must have a servo board identified in AMP to indicate to which board the spindle is connected. The spindle must be included in the number-of-motors AMP parameter for the board the spindle is on. MUST ASSIGN TOOL NUMBER FIRST In random tool, an attempt was made to customize a tool before the tool number was assigned.
Appendix B Error and System Messages Message Description N NEED SHADOW RAM FOR ONLINE SEARCH Your system contains the DH+ module and you have not installed the extra RAM SIMMS that are required to run the PAL online search monitor with the DH+ module installed. You must buy additional RAM for a system equipped with both of these features. Contact your Allen-Bradley Sales representative to purchase these SIMMS. Refer to your 9/Series integration manual for details on installing additional SIMMS.
Appendix B Error and System Messages Message Description NO PROGRAM TO RESTART There is no program to restart. The previous program was either completed or cancelled. NO RECIPROCATION DISTANCE A reciprocation interval of zero (0) was programmed for a grinder reciprocation fixed cycle. NO RECIPROCATION FEEDRATE The reciprocation feedrate, E-word, required during a grinder reciprocation fixed cycle was not programmed.
Appendix B Error and System Messages Message Description O OBJECT NOT FOUND IN PROGRAM The object you are searching for in the search monitor utility does not exist in the current module, or does not exist in the program in the direction you are searching. OCI ETHERNET CARD NOT INSTALLED An OCI dual-- process system has a standard CRT installed. The OCI Ethernet card has not been installed. This may happen if a dual-- process OCI executive is loaded into a non-- OCI system.
Appendix B Error and System Messages Message Description OVER SPEED IN POCKET CYCLE The programmed feedrate for an irregular pocket cycle (G89) was too high for the cycle to keep up. The part program stops at the endpoint of the block in which the error occurred. The cycle must be executed with a lower feedrate. OVERTRAVEL (+) The indicated axis has reached the positive software overtravel limit during an axis jog. This message can appear prior to reaching the overtravel limit in certain instances.
Appendix B Error and System Messages Message Description PAL SOURCE REV. MISMATCH - CAN’T MONITOR PAL source code in the control does not match the revision of the CNC executive. The PAL code may execute if all of the PAL system flags exist but the monitor cannot be used. PAL USING MEMORY - REFORMAT The AMP parameter allowing PAL to be stored in RAM memory has been enabled. This changes the amount of RAM memory available for part program storage, requiring the RAM disk to be reformatted.
Appendix B Error and System Messages Message Description POCKET IS PART OF CUSTOM TOOL An attempt was made to assign a tool to a tool pocket that is already used by a custom tool. Custom tools are assigned to tool pockets that are shown with an XXXX next to the pocket number on the random tool table. POCKET MILLING SHAPE IS INVALID A parameter is missing in the G88 programming block. POINT ALREADY EXISTS The point that you are trying to enter is already in the axis calibration table.
Appendix B Error and System Messages Message Description PROGRAM NOT FOUND The program cannot be located in memory. Check to make sure the program name was correctly entered. PROGRAM OPEN FOR EDIT IN ANOTHER PROCESS On a dual-processing system, you cannot edit a program that is active in another process. You will need to switch processes if you want to edit the other program. PROGRAM REWIND ERROR An attempt to rewind the tape was not successful.
Appendix B Error and System Messages Message Description RECIP AXIS IN WRONG PLANE The reciprocation axis specified in a G81 or a G81.1 programming block is not in the currently selected plane. RECIP AXIS NOT PROGRAMMED No reciprocation axis was specified in a G81 or a G81.1 programming block. RECIPROCATION NOT STOPPED An attempt was made to deactivate the current part program while reciprocation is still active. You must deactivate reciprocation before deactivating the current part program.
Appendix B Error and System Messages Message Description REMOTE I/O USER FAULT OCCURRED The RIO module detected that the user fault bit was set. The interboard communications fault LED is flashing. REMOTE I/O WATCHDOG TIMEOUT The watchdog mechanism on the RIO module timed out, indicating that the RIO module has not operated in an expected manner for possibly 17ms. The processor fault LED is turned ON.
Appendix B Error and System Messages Message Description S-- CURVE OPTION NOT INSTALLED An attempt was made to select S-- Curve Acc/Dec (G47.1) when the S-- Curve option bit was set to false. Make sure your system includes the S-- Curve option. S NOT LEGAL PROGRAMMING AXIS NAME This is displayed at power-up when the letter “S”is assigned to linear or rotary axis. Only the spindle(s) can be AMPed with “S”as the name; it cannot be assigned to a programmable axis.
Appendix B Error and System Messages Message SERVO AMP C LOOP GAIN ERROR Description One of the following AMP parameter errors exist:: Current Prop. Gain + Current Integral Gain < 4096 or Current Prop. Gain - Current Integral Gain > 0. SERVO AMP ERROR There is an error in one or more of the AMP parameters relative to servo control or an absolute feedback encoder failed to initialize.
Appendix B Error and System Messages Message Description SERVO PROCESSOR OVERLAP The analog version of the servo sub-system provides fine iteration overlap detection. This message is displayed if the fine iteration software on the DSP does not execute to completion in one fine iteration. SERVO PROM CHECKSUM ERROR The checksum test on the servo processor software stored in PROM memory has failed. This test is performed on power-up and periodically while the system is running.
Appendix B Error and System Messages Message Description SPINDLE IS CLAMPED An attempt was made to program a block containing a spindle code other than an M05 while the PAL servo clamp request flag for the spindle was set. SPINDLE MODES INCOMPATIBLE An attempt was made to enter virtual mode when the spindle that is used for this mode is synchronized as the follower spindle or an attempt was made to perform end face milling during synchronization.
Appendix B Error and System Messages Message Description SYSTEM MODULE GROUND FAULT The 1394 system module has detected a ground fault. The system generates a ground fault when there is an imbalance in the DC bus of greater than 5A. This drive error can be caused by incorrect wiring (verify motor and ground wiring), motor malfunction, or an axis module IGBT malfunction. SYSTEM MODULE OVER TEMP The 1394 contains a thermal sensor which senses the internal ambient temperature.
Appendix B Error and System Messages Message Description THREAD LEAD IS ZERO No thread lead has been programmed in a block that calls for thread cutting. Thread lead is programmed with either an F- or an E-word. THREAD PULLOUT DISTANCE TOO LARGE The programmed threading pullout distance is larger than the programmed distance of the thread departure.
Appendix B Error and System Messages Message Description TOO MANY NONMOTION CHAMFER/RADIUS BLOCKS Too many non-motion blocks separate the first tool path that determines the chamfer or radius size (programmed with a ,R or ,C) from the second tool path. A maximum number of non-motion blocks is set in AMP by the system installer. A non-motion block is defined as any block that does not generate axis motion in the current plane.
Appendix B Error and System Messages Message Description UNABLE TO SYNCH IN CURRENT MODE The control can not perform the request to synchronize spindles. Possible causes are: synchronization is already active; virtual/cylindrical programming or a threading operation is active on the primary or follower spindle when the synchronization request is made; or on a dual-- process system, one of the requesting processes cannot gain control over both spindles.
Appendix B Error and System Messages Message Description Z Z-WORD CANNOT BE GREATER THAN R-WORD The depth (Z-word) of a pocket formed using a G88.5 and G88.6 hemispherical pocket cycle cannot be greater than the radius (R-word) of that pocket. ZONE 2 PROGRAM ERROR The next block in the program or MDI entry would cause the specified axis to enter the restricted area of programmable zone 2.
Appendix C G-code Tables Appendix Overview This appendix lists the G-codes for 9/Series Mill controls. They are listed numerically along with a brief description of their use. These G-codes are discussed in detail in the sections within this manual that refer to their specific usage. The group numbers given in the table refer to modality. Group 00 are not modal and are independent of other G-codes. The remaining G-code groups are modal with other G-codes with the same group number.
Appendix C G-code Tables A G12.1 Modal Group 21 Primary Spindle Controlling G12.2 Auxiliary Spindle 2 Controlling G12.3 Auxiliary Spindle 3 Controlling G13 QuickPath Plus (Use First Intersect.) G13.1 G14 G15 Polar Coordinate Programming (Cancel) Plane Selection Inch System Selection Modal Metric System Selection 04 Programmable Zone 2 and 3, ON G22.1 Programmable Zone 3, ON G23 Programmable Zone 2 and 3, OFF G23.
Appendix C G-code Tables A G39 Modal Group 20 G39.1 G40 Function Cutter Diameter Comp (Linear Generated Block) 07 Cutter Diameter Compensation (Cancel) Cutter Diameter Compensation (Left) G42 Cutter Diameter Compensation (Right) 08 Tool Length Offset (Plus) G43.1 Tool Length Offset Selection (Plus) G44 Tool Length Offset (Minus) G44.1 G45 Disable Spindle Synchronization Set Spindle Positional Synchronization G46.
Appendix C G-code Tables A Modal Group Function G66.1 Paramacro Modal Call G67 Paramacro Modal Call (Cancel) G68 16 G69 G73 Part Rotation Deep Hole Peck Drilling Cycle (With dwell) Left-Hand Tapping Cycle G74.1 Left-Hand Solid Tapping Cycle G76 Boring Cycle (Spindle Shift) G80 Drilling Cycle (No Dwell, Rapid Out) Drilling Cycle (Dwell, Rapid Out) G83 Deep Hole Peck Drilling Cycle G84 Right-Hand Tapping Cycle G84.
Appendix D Allen-Bradley 7300 Series CNC Tape Compatibility Appendix Overview The 7300 Series CNC tape compatibility feature has been developed for customers with an existing library of standard 7320 and 7360 CNC tapes. This feature allows those 7300 tapes to be read and executed by the control. If desired, these 7300 tapes can be copied into the control’s memory to allow editing and execution, or they can be executed directly from tape, with the exception of 7300 pattern repeat subprograms.
Appendix D Allen-Bradley 7300 Series CNC Tape Compatibility Table D.
Appendix D Allen-Bradley 7300 Series CNC Tape Compatibility M-code Compatibility Considerations Table D.B lists all standard 7300 M-codes that the control can execute in 7300 mode. Important: In order to provide the same functionality as the 7300 PAL, the system installer has to write a specific application in PAL when interfacing with the control. Refer to the System 7320 Programming Manual for details on these M-codes and their operation. Table D.
Appendix D Allen-Bradley 7300 Series CNC Tape Compatibility M06 Tool Transfer Depending upon your 7300 configuration, M06 can be executed in two ways: all tool change operations must be handled by the PAL program. Note: This is the way M06 works on the 9/Series control. or the active tool offset is cancelled and the axes move to a predefined tool change position. In order for your control to do this, you have to reconfigure your AMP.
Appendix D Allen-Bradley 7300 Series CNC Tape Compatibility We recommend that you use this set-up when running your control in 7300 mode: Set This Tool Length Offset Parameter: To: Explanation: Tool Geometry Mode (AMP [202]): immediate shift/immediate move once the offset is programmed, the geometry offset is activated immediately and the coordinate system gets shifted immediately.
Appendix D Allen-Bradley 7300 Series CNC Tape Compatibility Important: The 9/Series control allows the Power-Turn-On (PTO) mode of the control to be specified in AMP with respect to inch/metric (G70/G71) and absolute/incremental (G90/G91) etc. For 7300 tape compatibility, these parameters may need to be modified if a certain PTO mode is expected. Refer to your AMP reference manual for details on these parameters.
Appendix D Allen-Bradley 7300 Series CNC Tape Compatibility At this time, the control creates an internal cross-reference table for all pattern repeat names. The cross-reference table is generated so that any blocks that call pattern repeat do not need to be rewritten using the new program name. Refer to the section on Pattern Repeat for details. You can not copy pattern repeat programs from memory to memory. Doing so does not create the necessary cross-reference table.
Appendix D Allen-Bradley 7300 Series CNC Tape Compatibility Important: The (DP) block is saved in memory as part of the program, and it is treated as a comment block during the execution of the part program. Executing 7300 Part Programs The system installer has to write PAL program for control to execute in 7300 tape compatibility mode. Refer to your PAL reference manual for details.
Appendix D Allen-Bradley 7300 Series CNC Tape Compatibility The main program, which has the pattern repeat call block “(CP, name, r)”, can be executed from tape or from the control’s memory. However, if you want to make minor editing to your main program, you must copy the program into the control’s memory. Refer to Section 9.2, “Inputting Part Programs,” for details on how to copy a program from tape. Important: To execute a program from tape, the tape must be positioned at the start of the main program.
Appendix D Allen-Bradley 7300 Series CNC Tape Compatibility Table D.
Index Index (General) 9/Series Mill 9/Series PAL Reference Manual Operation and Programming Manual Symbols All Position Display, 8-19 Alternate, home return, 14-34 ; As End of Block, 10-11 AMP, Reference Manual, 1-5 / Block Delete, 10-10 AMP Feedrate, 18-12 / Block Delete Character, 7-1 Angles, for polar programming, 14-21 Angular Jogging, 4-5 Numbers 7300 Series CNC Tape Compatibility 9/240 G Codes Applicable, D-9 Features Not Supported on 9/240, D-10 G Code Considerations, D-1 M Code Considerati
Index Index (General) 9/Series Mill 9/Series PAL Reference Manual Operation and Programming Manual Definition, 1-4 Password Protection, 2-30 Setting Power on Time/After Reset, 2-47 Power on Time/Overall, 2-46 Base Coordinate System, 11-1 Basic Control Operation, 2-1 Basic Program Execution, 7-17 Baud Rate, Selecting MAX, 9-5 Baud Rate, Setup, 9-5 Block by Block, 2-14 Block by Block Execution, 7-4 Changing Languages, 8-23 Changing Parameters Auto Erase, 8-32 Auto Size, 8-30 Grid Lines, 8-30 Overtravel Zon
Index Index (General) 9/Series Mill 9/Series PAL Reference Manual Operation and Programming Manual Control Reset, 2-3, 2-4 Cutting Speed, 10-39 Coordinate Offset, on shared axis, 30-29 Cutting Speeds, 10-23 Coordinate System inch/metric, 13-13 Offset Tables, 3-14 Offsetting Work Systems, 11-13 Rotating (G68, G69), 13-2 Rotating External, 13-6 Cutting Torque, G25, 18-9 Coordinate System Offset (G92), 11-13 Cycle Stop for Dual-Processing, 30-11 Coordinate System, Absolute, 13-12 Cycle Time (per pro
Index Index (General) 9/Series Mill 9/Series PAL Reference Manual Operation and Programming Manual Displaying a Program {DISPLAY PRGRAM}, 5-39 Displaying Machine Information, 8-33 Displaying Position ABS, 8-6 ABS (Large Display), 8-7 absolute (Small Display), 8-8 ALL, 8-19 distance to go (Small Display), 8-14 DTG, 8-12 DTG (Large Display), 8-13 G Code Status, 8-20 M Code Status, 8-16 PRGRAM, 8-3 PRGRAM (Large Display), 8-4 PRGRAM (Small Display), 8-5 PRGRAM DTG, 8-17 program/DTG (Small Display), 8-18 Targ
Index Index (General) 9/Series Mill 9/Series PAL Reference Manual Operation and Programming Manual End of Program Rewind M30, 10-34 Feed to Hard Stop (G24), 14-40 End Program on Tape, 10-5 Feedback, as an adaptive depth probe, 27-18 Energizing the Control, 2-21 Feedhold Status, 7-18 English, Language Display, 8-23 Feedrate as torque control (G25), 18-9 dry run, 7-21 English/Metric, 13-13 Enlarging, scaling, 13-14 Entering Characters and Blocks, 5-7 Entering Interference Values Manually, 30-19 Ente
Index Index (General) 9/Series Mill 9/Series PAL Reference Manual Operation and Programming Manual G21, 13-13 G22, 12-5 G22.1, 12-7 G23, 12-5 G23.1, 12-7 G24, 14-40 G25, 18-9 G26, 27-18 G27, 14-33 G28, 14-29, 14-30 G29, 14-32 G30, 14-34 G31, 27-2 G31.1, 27-2 G31.2, 27-2 G31.3, 27-2 G31.4, 27-2 G37, 27-4 G37.1, 27-4 G37.2, 27-4 G37.3, 27-4 G37.4, 27-4 G38, 27-8 G38.1, 27-12 G39, 21-7 G39.1, 21-7 G40, 21-3 G41, 21-3 G42, 21-3 G43, 20-3 G44, 20-3 G47, 18-18 G48, 18-19 G49, 20-3 G50.1, 14-36 G51.
Index Index (General) 9/Series Mill 9/Series PAL Reference Manual Operation and Programming Manual Disabling, 8-27 Grid Lines, 8-30 Machine Information, 8-33 Overtravel Zone Lines, 8-30 Process Speed, 8-32 Rapid Traverse, 8-29 Running Graphics, 8-25 Scale, 8-26 Select Graph, 8-29 Selecting a Program, 8-24 Sequence Starting #:, 8-31 Sequence Stopping #:, 8-31 Single-Block, 8-33 Tool Paths, 8-24 Zooming, 8-33 Graphics for Dual-Processing, 30-4 Machine Home Check (G27), 14-33 HPG jogging, 4-4 I I--word, 10
Index Index (General) 9/Series Mill 9/Series PAL Reference Manual Operation and Programming Manual Japanese, Language Display, 8-23 Limits, Overtravels and Zones, 12-1 Jog Offset Function, 4-6 Limits, Programmable Zones, 12-5 Jog on the Fly, Offsets, 11-19 Limits, Resetting, 12-13 Jog Retract, 2-14, 7-28 Limits, Software Overtravels, 12-3 Jog Select, 2-13 Jog Select Switch, 4-3 Line Numbers, 10-9 Linear Acc/Dec, 18-16 Jogging Arbitrary Angle Jog, 4-5 Continuous Jog, 4-3 HPG Jog, 4-4 In Auto mode
Index Index (General) 9/Series Mill 9/Series PAL Reference Manual Operation and Programming Manual Machine Home, Establishing, 11-2 Message, at PTO, 8-37 Machine Home, Manual, 4-8 Metric Mode, 13-13 Machine Information, 8-33 Mill Cycle Format Prompting, 5-26 Machine Messages, 2-37 Clearing Active Messages, 2-40 Macro Call Commands, 28-44 Nesting, 28-52 Output Commands, 28-54 Millimeters/Inches, 13-13 Magazine, Tool Selection, 10-40 Mirror, 14-36 Magnification, scaling, 13-14 Main Program End M99
Index Index (General) 9/Series Mill 9/Series PAL Reference Manual Operation and Programming Manual O O word, as program name, 10-8 O--words, 10-37 ODS Downloading Part Programs, 6-5 Uploading Part Programs, 6-12 Operator Panel, 2-1 Calculator Function, 2-4 Keyboard, 2-3 monochrome, 2-2 Operators, Valid Mathematical, 2-5 Optional Stop, 7-18 ODS, Using to Edit Part Programs, 6-1 Optional Stop M01, 10-33 Offset, Length Offset, 20-3 Output code, for Communications, 9-7 Offset Data, Measure Feature, 3-9
Index Index (General) 9/Series Mill 9/Series PAL Reference Manual Operation and Programming Manual Input Flags, 28-33 Output Flags, 28-34 Parameter Value Assignment, 28-36 Through Programming, 28-38 Through Tables, 28-40 Using Arguments, 28-36 System Parameters, 28-15 WHILE DO END, 28-10 Paramacro Variables in CALC operation, 2-7 Transfer Line, 31-14 Parameter Table, 10-19 Parameters, Changing, 8-27 Parameters, Definition, 10-6 Parametric Expressions, 28-2 Parity, for communications, 9-6 Parking a Dual Ax
Index Index (General) 9/Series Mill 9/Series PAL Reference Manual Operation and Programming Manual Probing Applications (G31), 27-4 Applications (G37), 27-7 Hole Probing (G38), 27-8, 27-9 Parallel Cycle (G38.
Index Index (General) 9/Series Mill 9/Series PAL Reference Manual Operation and Programming Manual QUICKPATH Plus and Radius Chamfer Words, 10-22 Reflect, mirror, 14-36 QuickPath Plus Prompting Patterns, 5-20 Reformat Memory, 2-41 QUICKVIEW, 5-17 Reloading Part Program Templates, 31-17 QuickView, with Transfer Line Cycles, 31-5 Remaining Workpieces, 2-49 QuickView for Dual-Processing, 30-4 QV01, Drilling Cycle, No Dwell/Rapid Out, 31-2, 31-15, 31-26 Removing an Axis, 4-8 Removing and Axis, 2-43
Index Index (General) 9/Series Mill 9/Series PAL Reference Manual Operation and Programming Manual S--word, Spindle Speed, 10-38 Shifting Work Coordinate Systems, 11-9 Save CRT, 8-39 Saving Offset Tables, to a part program or external device, 3-17 Short Block Acc/Dec Entry and Exit, 18-25 G36 G36.
Index Index (General) 9/Series Mill 9/Series PAL Reference Manual Operation and Programming Manual G CODE, 8-1 G CODE PROMPT, 5-24 G CODE STATUS, 8-20 GRAPH, 8-25 GRAPH SETUP, 8-28 JOG AXIS, 2-18 JOG AXIS +, 2-18 JOG AXIS - , 2-18 JOG RETRCT, 2-19 M CODE, 8-1 M CODE STATUS, 8-16 MACHNE INFO, 8-33 MACRO PARAM, 28-40 MEASURE, 3-9 MERGE PRGRAM, 5-15 MID ST PRGRAM, 7-13, 7-25 MILL PROMPT, 5-26 MODIFY INSERT, 5-7 MORE OFFSET, 3-7 NCRYPT MODE, 5-46 OFFSET, 3-1, 3-12 PASSWORD, 2-26 PLANE SELECT, 5-19, 5-29 PRGRA
Index Index (General) 9/Series Mill 9/Series PAL Reference Manual Operation and Programming Manual Storage Capacity, Memory, 6-4 Subprogram Call M98, 10-34 Subprogram Call, (M98), 10-13 Subprogram End M99, 10-35 Subprogram Names, 10-8 Subprogram Nesting, 10-16 Subprogram Return, (M99), 10-14 Subprogram, Using, 10-12 Suppression, of Zeros, 10-18 surface speed, 10-39 Switching a Shared Axis Process, 30-28 Synchronization Coordinating, 30-10 Cycle Stop, 30-11 M-codes, 30-7 MDI Mode, 30-11 Multiple Part Progr
Index Index (General) 9/Series Mill 9/Series PAL Reference Manual Operation and Programming Manual Tool Data, Assigning Detailed, 20-25 Tool Directory Data, 20-20 Tool Gauging Function (G37), 27-1 Tool Length Axis Selection, 20-9 Tool Length Offset Function (G43, G44, G49), 20-3 Tool Management, 20-19 Tool Offset Dimensional Parameters, 3-2 Tool Offset Table Setup, 3-1 Tool Offset Words, 10-22 Tool Offsets Activating, 20-8 backing up, 3-17 changing active, 3-12 entering diameter values, 3-4 entering diame
Index Index (General) 9/Series Mill 9/Series PAL Reference Manual Operation and Programming Manual Word Descriptions and Ranges, 10-19 Workpieces Cut, 2-47 Word Format, Zero Suppression, 10-18 Word Format and Functions, 10-17 Word, Definition, 10-6 Work Coordinate, Changing or Offsetting, 21-49 Work Coordinate System Defining, 11-5 External Offset, 11-9 Offsetting, 11-13 Work Coordinate System (G54 G59), 11-4 Altering using G10, 11-7 Work Coordinate System Offset Tables, 3-14 External Offsets, 3-14 Sett
Publication 8520-- UM513A-- EN-- P - October 2000 Supersedes Publication 8520--5.1.3 -- August 1998 PN 176957 Copyright 2000 Allen-Bradley Company, Inc.