G35 Automatic Tool Diameter Measurement (Group 00)

Next Generation 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 set a tool diameter offset.

F - Feedrate
*D - Tool diameter offset number
*X - X-Axis command
*Y - Y-Axis command

*indicates optional

Automatic Tool Diameter Offset Measurement function (G35) is used to set the tool diameter (or radius) using two touches of the probe; one on each side of the tool. The first point is set with a G31 block using an M75, and the second point is set with the G35 block. The distance between these two points is set into the selected (non-zero) Dnnn offset.

Setting 63 Tool Probe Width is used to reduce the measurement of the tool by the width of the tool probe. See the settings section of this manual for more information about Setting 63.

This G-code moves the axes to the programmed position. The specified move is started and continues until the position is reached or the probe sends a signal (skip signal).


This code is non-modal and only applies to the block of code in which G35 is specified.

Do not use Cutter Compensation (G41, G42) with a G35.

To avoid damaging the probe, use a feed rate below F100. (inch) or F2500. (metric).

Turn on the tool-setting probe before using G35.

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

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

Use the following commands to turn off the tool-setting probe.

M69 P1134 ;

Turn on the spindle in reverse (M04), for a right handed cutter.

Also see M75, M78, and M79.

Also see G31.

Sample program:

This sample program measures the diameter of a tool and records the measured value to the tool offset page. To use this program, the G59 Work Offset location must be set to the tool-setting probe location.

% O60351 (G35 MEASURE AND RECORD TOOL DIA OFFSET) ; (G59 X0 Y0 is the tool setting probe location) ; (Z0 is at the surface of tool-setting probe) ; (T1 is a spindle probe) ; (BEGIN PREPARATION BLOCKS) ; T1 M06 (Select tool 1) ; G00 G90 G59 X0 Y-1. (Rapid tool next to probe) ; M59 P1133 (Select tool-setting probe) ; G04 P1. (Dwell for 1 second) ; M59 P1134 (Probe on) ; G43 H01 Z1. (Activate tool offset 1) ; S200 M04 (Spindle on CCW) ; (BEGIN PROBING BLOCKS) ; G01 Z-0.25 F50. (Feed tool below surface of probe) ; G31 Y-0.25 F10. M75 (Set reference point) ; G01 Y-1. F25. (Feed away from the probe) ; Z0.5 (Retract above the probe) ; Y1. (Move over the probe in Y-axis) ; Z-0.25 (Move tool below surface of the probe) ; G35 Y0.205 D01 F10. ; (Measure & record tool diameter) ; (Records to tool offset 1); G01 Y1. F25. (Feed away from the probe) ; Z1. (Retract above the probe) ; M69 P1134 (Probe off) ; (BEGIN COMPLETION BLOCKS) ; 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.