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
422 11 G-Code Edit, Help, & Advanced Features
11.4 Advanced Programming
Probe Move (G31)
G31 is to be issued with an associated axis move (i.e. G31 X10). When
the G31 is executed, it moves at current feedrate selected for G1 until
the touch probe selected is deflected. At this point, the move is
stopped, and the position where the probe touched the part is read
and passed to system variables (#1060 to #1063 for X to U).
G31 is aborted if any of the following events occur:
The primitive is issued while the probe is still deflected (touching
the part).
The ready signal is not present.
Hardware malfunction: Trigger signal engaged, but no position is
latched.
Start pulse is issued, but probe is not ready after 2 seconds. (Only
cordless probes).
Cordless probe still in "sleeping mode”.
Low battery signal becomes active (Only cordless probes).
Canned cycles are available for the most common probe functions.
Using the G31 primitive, parametric programming, and the M-Code
described here, it is possible to write additional cycles to perform
custom probing functions.
M9387X0 Selects the Tool touch probe (X13)
M9387X1 Selects the 3-D touch probe (X12) (default)
M9387Y0 Copies Tool touch probe state (deflected or not) into
a system variable (#1066)
M9387Y1 Copies 3-D touch probe state (deflected or not) into
a system variable (#1066)
M9387Z0 Turns off cordless probe
M9387Z1 Turns on cordless probe