G01 Linear Interpolation Motion (Group 01)

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
F - Feedrate
* X - X-Axis motion command
* Y - Y-Axis motion command
* Z - Z-Axis motion command
* A - A-Axis motion command
* B - B-Axis motion command
* C - C-axis motion command
* ,R - Radius of the arc
* ,C - Chamfer distance

*indicates optional

G01 moves the axes at a commanded feed rate. It is primarily used to cut the workpiece. A G01 feed can be a single axis move or a combination of the axes. The rate of axes movement is controlled by feedrate ( F) value. This F value can be in units (inch or metric) per minute ( G94) or per spindle revolution ( G95), or time to complete the motion ( G93). The feedrate value ( F) can be on the current program line, or a previous line. The control will always use the most recent F value until another F value is commanded. If in G93, an F value is used on each line. Refer also to  G93.

G01 is a modal command, which means that it will stay in effect until canceled by a rapid command such as G00 or a circular motion command like G02 or  G03.

Once a G01 is started all programmed axes move and reach the destination at the same time. If an axis is not capable of the programmed feedrate the control will not proceed with the G01 command and an alarm (max feedrate exceeded) will be generated.

Corner Rounding and Chamfering Example

Corner Rounding and Chamfering Example #1

% O60011 (G01 CORNER ROUNDING & CHAMFER) ; (G54 X0 Y0 is at the top-right of part) ; (Z0 is on top of the part) ; (T1 is an end mill) ; (BEGIN PREPARATION BLOCKS) ; T1 M06 (Select tool 1) ; G00 G90 G40 G49 G54 (Safe startup) ; G00 G54 X0 Y0 (Rapid to 1st position) ; S1000 M03 (Spindle on CW) ; G43 H01 Z0.1 (Activate tool offset 1) ; M08 (Coolant on) ; (BEGIN CUTTING BLOCKS) ; G01 Z-0.5 F20. (Feed to cutting depth) ; Y-5. ,C1. (Chamfer) ; X-5. ,R1. (Corner-round) ; Y0 (Feed to Y0.) ; (BEGIN COMPLETION BLOCKS) ; G00 Z0.1 M09 (Rapid retract, Coolant off) ; G53 G49 Z0 M05 (Z home, Spindle off) ; G53 Y0 (Y home) ; M30 (End program) ; %

A chamfer block or a corner-rounding block can be automatically inserted between two linear interpolation blocks by specifying ,C (chamfering) or ,R (corner rounding). There must be a terminating linear interpolation block after the beginning block (a G04 pause may intervene).

These two linear interpolation blocks specify a corner of intersection. If the beginning block specifies a ,C, the value after the ,C is the distance from the intersection to where the chamfer begins, and also the distance from the intersection to where the chamfer ends. If the beginning block specifies an ,R, the value after the ,R is the radius of a circle tangent to the corner at two points: the beginning of the corner-rounding arc and the endpoint of that arc. There can be consecutive blocks with chamfering or corner rounding specified. There must be movement on the two axes specified by the selected plane, whether the active plane is XY ( G17), XZ ( G18) or YZ ( G19).

F - Feed rate
* B - B-axis motion command
* C - C-Axis motion command
* U - X-axis incremental motion command
* W - Z-axis incremental motion command
* X - X-axis absolute motion command
* Y - Y-axis absolute motion command
* Z - Z-axis absolute motion command
* A - Optional angle of movement (used with only one of X, Z, U, W)
* ,C - Distance from center of intersection where the chamfer begins
* ,R - Radius of the fillet or arc

This G code provides for straight line (linear) motion from point to point. Motion can occur in 1 or more axes. You can command a G01 with 3 or more axes All axes will start and finish motion at the same time. The speed of all axes is controlled so that the feed rate specified is achieved along the actual path. The C-Axis may also be commanded and this will provide a helical (spiral) motion. A C-Axis feed rate is dependent on the C-Axis diameter setting (Setting 102) to create a helical motion. The F address (feedrate) command is modal and may be specified in a previous block. Only the axes specified are moved.

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.