G95 Feed per Revolution (Group 05)

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

When G95 is active, a spindle revolution will result in a travel distance specified by the Feed value. If Setting 9 is set to INCH, then the feed value F will be taken as inches/rev (set to MM, then the feed will be taken as mm/rev). Feed Override and Spindle Override will affect the behavior of the machine while G95 is active. When a Spindle Override is selected, any change in the spindle speed will result in a corresponding change in feed in order to keep the chip load uniform. However, if a Feed Override is selected, then any change in the Feed Override will only affect the feed rate and not the spindle.

*C - C-Axis absolute motion command (optional)
F - Feed Rate
R - Position of the R plane
S - RPM, called prior to G95
W - Z-axis incremental distance
X - Optional Part Diameter X-axis motion command
*Y - Y-axis motion command
Z - Position of bottom of hole

* indicates optional

G95 Live Tooling Rigid Tapping is an axial tapping cycle similar to G84 Rigid Tapping in that it uses the F, R, X and Z addresses, however, it has the following differences:

  • The control must be in G99 Feed per Revolution mode in order for tapping to work properly.

  • An S (spindle speed) command must have been issued prior to the G95.

  • The X Axis must be positioned between machine zero and the center of the main spindle, do not position beyond spindle center.

% o60951 (G95 LIVE TOOLING RIGID TAP) ; (G54 X0 Y0 is at the center of rotation) ; (Z0 is on the face of the part) ; (T1 is a 1/4-20 tap) ; (BEGIN PREPARATION BLOCKS) ; T101 (Select tool and offset 1) ; G00 G18 G20 G40 G80 G99 (Safe startup) ; M154 (Engage C Axis) ; G00 G54 X1.5 C0. Z0.5 (Rapid to 1st position) ; M08 (Coolant on) ; (BEGIN CUTTING CYCLE) ; S500 (Select tap RPM) ; G95 C45. Z-0.5 R0.5 F0.05 (Tap to Z-0.5) ; C135. (next position) ; C225. (next position) ; C315. (last position) ; (BEGIN COMPLETION BLOCKS) ; M155 (Disengage C Axis) ; G00 G53 X0 M09 (X home, coolant off) ; G53 Z0 (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