Haas Mill User Manual

130
G Codes
96-8000 rev R June 2007
G52 Set Work Coordinate System YASNAC (Group 00 or 12)
The G52 command works differently depending on the value of setting 33. Setting 33 selects the Fanuc, Haas, or
Yasnac style of coordinates.
If Yasnac is selected, G52 is a group 12 G-code. G52 works the same as G54, G55, etc. All of the G52 values will
not be set to zero (0) when powered on, reset is pressed, at the end of the program, or by an M30. When using a
G92 (Set Work Coordinate Systems Shift Value), in Yasnac format, the X, Y, Z, A, and B values are subtracted from
the current work position, and automatically entered into the G52 work offset.
If Fanuc is selected, G52 is a group 00 G-code. This is a global work coordinate shift. The values entered into the
G52 line of the work offset page are added to all work offsets. All of the G52 values in the work offset page will be
set to zero (0) when powered on, reset is pressed, changing modes, at the end of the program, by an M30, G92 or
a G52 X0 Y0 Z0 A0 B0. When using a G92 (Set Work Coordinate Systems Shift Value), in Fanuc format, the
current position in the current work coordinate system is shifted by the values of G92 (X, Y, Z, A, and B). The
values of the G92 work offset are the difference between the current work offset and the shifted amount commanded
by G92.
If Haas is selected, G52 is a group 00 G-code. This is a global work coordinate shift. The values entered into the
G52 line of the work offset page are added to all work offsets. All of the G52 values will be set to zero (0) by a G92.
When using a G92 (Set Work Coordinate Systems Shift Value), in Haas format, the current position in the current
work coordinate system is shifted by the values of G92 (X, Y, Z, A, and B). The values of the G92 work offset are
the difference between the current work offset and the shifted amount commanded by G92 (Set Work Coordinate
Systems Shift Value).
G53 Non-Modal Machine Coordinate Selection (Group 00)
This code temporarily cancels work coordinate offsets and uses the machine coordinate system. In the machine
coordinate system, the zero point for each axis is the position where the machine goes when a Zero Return is
performed. G53 will revert to this system for the block it is commanded in.
G54-59 Select Work Coordinate System #1 - #6 (Group 12)
These codes select one of the six user coordinate system. All future references to axes positions will be interpreted
using the new (G54 G59) coordinate system.
G60 Uni-Directional Positioning (Group 00)
This G code is used to provide positioning only from the positive direction. It is not recommended for use with this
control. It is provided only for compatibility with older systems. It is non-modal, so does not affect the blocks that
follow it. Also see Setting 35.
G61 Exact Stop Mode (Group 15)
The G61 code is used to specify an exact stop. It is modal; therefore, it affects the blocks that follow it. The
machine axes will come to an exact stop at the end of each commanded move.
G64 G61 Cancel (Group 15)
The G64 code is used to cancel exact stop (G61).
G68 Rotation (Group 16)
(This G-code is optional and requires Rotation and Scaling.)
G17, G18, G19 optional plane of rotation, default is current
A optional center of rotation for the first axis of the selected plane
B optional center of rotation for the second axis of the selected plane
R optional angle of rotation specified in degrees
Three-place decimal -360.000 to 360.000.
A G17, 18 or 19 must be used before the G68 command to establish the axis plane being rotated. For example:
G17 G68 Annn Bnnn Rnnn;
A and B correspond to the axes of the current plane; for the G17 example A is the X-axis and B is the Y-axis.

Haas Mill Specifications

General

Travels X Axis	Varies by model
Travels Y Axis	Varies by model
Travels Z Axis	Varies by model
Spindle Speed	Varies by model
Spindle Motor	Varies by model
Table Size	Varies by model
Rapid Traverse Rates	Varies by model
Tool Capacity	Varies by model
Max Cutting Rate	Varies by model
Spindle Taper	Varies by model