Manual
Table Of Contents
- Controls of the 3500i
- Manual Information
- Introduction
- Machining Fundamentals
- Manual Data Input
- Tool Management
- 4.1 Tool Table
- 4.2 Tool Data
- Program Management
- Conversational Editing
- Programming: Canned Cycles, sub-programs
- 7.1 Explaining Basic Cycles
- Round/Chamfer
- Rapid
- Line
- Arc
- Dwell:
- Plane Selection
- Reference Point Return:
- Fixture Offset (Work Coordinate System Select):
- Unit (Inch/MM)
- Dimension (Abs/Inc)
- Absolute Zero Set
- Block Form
- Temporary Path Tolerance
- System Data
- FeedRate
- FeedRate (4th-Axis)
- Spindle RPM
- M - Functions
- Tool Definition and Activation
- Repeat Blocks
- 7.2 Canned Cycles
- 7.3 Probing Cycles
- 7.4 Sub-programs
- 7.1 Explaining Basic Cycles
- Drawing Programs
- Running a Program on the Machine
- CAM: Programming
- 10.1 CAM Programming
- CAM Mode
- Recommended CAM Programming Sequence
- CAM Mode Mouse Operations
- CAM Mode Screen
- Activating CAM Mode
- Creating a New Program
- Tool Path Data Input
- Quick Coordinate Entry
- Job Setup: Basic tab
- Job Setup: Advanced tab
- Comment Tab
- Block Form: Basic tab
- Comment Tab
- Drilling Cycle:
- Drilling dialogue:
- Mill Cycle
- Pocket Cycle
- Pocket Finish Cycles
- Engraving Cycle
- Program Directive
- Modifying Toolbar
- Viewing Tools
- CAM Mode buttons
- CAM Setup
- Geometry
- DXF Import Feature
- Modifying Tools
- Shapes
- Tool Table
- Tool Paths
- CAM Example 1
- CAM Example 2
- 10.1 CAM Programming
- G-Code Edit, Help, & Advanced Features
- 11.1 G-Code Program Editing
- 11.2 G-Code and M-Code Definitions
- 11.3 Edit Help
- 11.4 Advanced Programming
- SPEED
- M - Functions
- Order of Execution
- Programming Non-modal Exact Stop:
- In-Position Mode (Exact Stop Check):
- Contouring Mode (Cutting Mode) :
- Setting Stroke Limit:
- Return from Reference Point:
- Move Reference from Machine Datum:
- Modifiers
- Block Separators
- Tool Offset Modification
- Expressions and Functions
- System Variables
- User Variables
- Variable Programming (Parametric Programming)
- Probe Move (G31)
- Conditional Statements
- Short Form Addressing
- Logical and Comparative Terms
- File Inclusion
- 11.5 Four Axis Programming
- Software Update
- Off-Line Software

436 11 G-Code Edit, Help, & Advanced Features
11.5 Four Axis Programming
Example 3: Mill
Mount a fourth axis as described above. Mount a part 4” in diameter
and 8” long on the face of the rotary table. Support the part on the
X+ end by a live center. The part has a 0.25”, 45° chamfer on one
end. Shortest Distance is set to on. This prevents the need to
unwind the U-axis, saving operation time.
Table 15-3 shows a thread-milling example. Assume that a 4-8 UN
2A thread must be milled from the right end, 6” long. The tool is
tapered to conform to the thread. Set X0 at the right end, Y0 at the
cylinder's center line, U0 at a pre-milled keyway on the cylinder.
Measure the tool offset from the top of the part (with Y axis at 0).
The X start position is one pitch (0.125 in.) to the right of X0, so that
the tool enters the work smoothly.
* 4-AX-THD
* SET Shortest Distance TO "on"
G90 G70 G0 M5
G28 Z0
G53 O1
G0 X0 Y0 U0
T1 * SPECIAL THD-TOOLS3500
S3500
M3
G0 X.125 Y0 U0
Z.1
G1 Z-.075 F20
* SET Shortest Distance TO "on"
* THIS IS TO PREVENT THE NEED TO UNWIND U
* U AXIS MOVE IS
* (360 X 8 PITCH X 6" LONG)
* + 360 FOR 1 TURN X.125 LEAD-IN
* U MOVE WILL BE 17,640.00 DEGREES
* OR 49 TURNS
G91 G1 X-6.125 U((360*8*6)+360)
G90 G0 M5
G28 Z0
X0 Y0 U0
M2