Haas 96-8000 - G93 Inverse Time Feed Mode (Group 05); G94 Feed Per Minute Mode (Group 05); G95 Feed Per Revolution (Group 05); G98 Canned Cycle Initial Point Return (Group 10)

175
96-8000 Rev AC
May 2010
G & M Codes
Settings
A G92 command cancels any G52 in effect for the commanded axes. Example:
G92 X1.4 cancels the G52 for the X-axis. The other axes are not affected.
The G92 shift value is displayed at the bottom of the Work Offsets page and
may be cleared there if necessary. It is also cleared automatically after power-
up, and any time ZERO RET and AUTO ALL AXES or ZERO SINGLE AXIS are
used.
YASNAC
If setting 33 is set to Yasnac, a G92 command sets the G52 work coordinate
system so that the commanded position becomes the current position in the
active work system. The G52 work system then automatically becomes active
until another work system is selected.
G93 Inverse Time Feed Mode (Group 05)
F Feed Rate (strokes per minute)
This G code species that all F (feedrate) values are interpreted as strokes
per minute. In other words the F code value, when divided into 60, is the num-
ber 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.
When G93 is active, the feedrate specication is mandatory for all interpolated
motion blocks; i.e., each non-rapid motion block must have its own feedrate
specication.
* Pressing RESET will reset the machine to G94 (Feed per Minute) mode.
* Settings 34 and 79 (4th & 5th axis diameter) are 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 specied
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