G31 Feed Until Skip (Group 00)

Classic Control - Mill Operator's Manual

The Online Interactive Operator's Manual is currently available in English only.

A PDF version of the Operator's Manual is available for download in multiple languages. Click the link below to view the Operator's Manual in your language. Click "Continue" to view the online version in English.

Get a translated PDF Download Continue

(This G-code is optional and requires a probe)

This G-code is used to record a probed location to a macro variable.

F - Feedrate
*X - X-Axis absolute motion command
*Y - Y-Axis absolute motion command
*Z - Z-Axis absolute motion command
*A - A-Axis absolute motion command
*B - B-Axis absolute motion command
*C - C-axis absolute motion command (UMC)

*indicates optional

This G-code moves the programmed axes while looking for a signal from the probe (skip signal). The specified move is started and continues until the position is reached or the probe receives a skip signal. If the probe receives a skip signal during the G31 move, the control will beep and the skip signal position will be recorded to macro variables. The program will then execute the next line of code. If the probe does not receive a skip signal during the G31 move, the control will not beep and the skip signal position will be recorded at the end of the programmed move. The program will continue.

Macro variables #5061 through #5066 are designated to store skip signal positions for each axis. For more information about these skip signal variables see the macro section of this manual.

Notes:

This code is non-modal and only applies to the block of code in which G31 is specified.

Do not use Cutter Compensation (G41, G42) with a G31.

The G31 line must have a Feed command. To avoid damaging the probe, use a feed rate below F100. (inch) or F2500. (metric).

Turn on the probe before using G31.

If your mill has the standard Renishaw probing system, use the following commands to turn on the probe.

Use the following code to turn on the spindle probe.

M59 P1134 ;

Use the following code to turn on the tool-setting probe.

% M59 P1133 ; G04 P1.0 ; M59 P1134 ; %

Use the following code to turn off either probe.

M69 P1134 ;

Also see M75, M78 and M79 ;

Sample program:

This sample program measures the top surface of a part with the spindle probe traveling in the Z negative direction. To use this program, the G54 part location must be set at, or close to the surface to be measured.

% O60311 (G31 SPINDLE PROBE) ; (G54 X0. Y0. is at the center of the part) ; (Z0. is at, or close to the surface) ; (T1 is a Spindle probe) ; (PREPARATION) ; T1 M06 (Select Tool 1) ; G00 G90 G54 X0 Y0 (Rapid to X0. Y0.) ; M59 P1134 (Spindle probe on) ; G43 H1 Z1. (Activate tool offset 1) ; (PROBING) ; G31 Z-0.25 F50. (Measure top surface) ; Z1. (Retract to Z1.) ; M69 P1134 (Spindle probe off) ; (COMPLETION) ; G00 G53 Z0. (Rapid retract to Z home) ; M30 (End program) ; %

Be aware: Many service and repair procedures should be done only by authorized personnel. The service technicians at your Haas Factory Outlet (HFO) have the training, experience, and are certified to do these tasks safely and correctly. You should not do machine repair or service procedures unless you are qualified and knowledgeable about the processes.

Danger: Some service procedures can be dangerous or life-threatening. DO NOT attempt a procedure that you do not completely understand. Contact your Haas Factory Outlet (HFO) and schedule a service technician visit if you have any doubts about doing a procedure.

Feedback