Haas Mill User Manual

147
G Codes
96-8000 rev R June 2007
G93 Inverse Time Feed Mode (Group 05)
F Feed Rate (strokes per minute)
This G code specifies that all F (feedrate) values are interpreted as strokes per minute. In other words the F code
value, when divided into 60, is the number of seconds that the motion takes to complete.
G93 is generally used in 4 and 5-axis work. It is a way of translating the linear feedrate (inches/min) into a value
that takes rotary motion into account. In G93 mode, the F value will tell you how many times per minute the tool
move can be repeated.
When G93 is active, the feedrate specification is mandatory for all interpolated motion blocks; i.e., each non-rapid
motion block must have its own feedrate specification.
* Pressing RESET will reset the machine to G94 (Feed per Minute) mode.
* Settings 34 and 79 (4th & 5th axis diameter) not necessary when using 93.
G94 Feed Per Minute Mode (Group 05)
This code deactivates G93 (Inverse Time Feed Mode) and returns the control to Feed Per Minute mode.
G95 Feed per Revolution (Group 05)
When G95 is active; a spindle revolution will result in a travel distance specified by the Feed value. If the Setting 9
Dimensioning 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.
G98 Canned Cycle Initial Point Return (Group 10)
Using G98, the Z-axis returns to its initial starting point (the Z position in the block before the canned cycle was
commanded) between each X and/or Y location. This allows for positioning up and around areas of the part and/or
clamps and fixtures.
G99 Canned Cycle R Plane Return (Group 10)
Using G99, the Z-axis will stay at the R plane between each X and/or Y location. When obstructions are not in the
path of the tool G99 saves machining time.
G100 Cancel Mirror Image (Group 00)
G101 Enable Mirror Image (Group 00)
X X-axis command
Y Y-axis command
Z Z-axis command
A A-axis command
Programmable mirror imaging is used to turn on or off any the axes. When one is ON, axis motion may be mirrored
(or reversed) around the work zero point. These G codes should be used in a command block without any other G
codes. They do not cause any axis motion. The bottom of the screen will indicate when an axis is mirrored. Also
see Settings 45 through 48 for mirror imaging.
The format for turning Mirror Image on and off is:
G101 X0 = Will turn on mirror imaging for the X axis.
G100 X0 = Will turn off mirror imaging for the X 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