96-8000 161
G CODES
June 1999
Each G code defined in this control is part of a group of G codes. The Group 00 codes are non-modal; that is,
they specify a function applicable to the block they are in and do not affect other blocks. The other groups are
modal and apply to all subsequent blocks until the end of the program or until replaced by a different G code
from the same group. A modal G code means blocks between G code group members do not need to re-
specify the same G code for each block.
There is also one case where the Group 01 G codes will cancel the Group 9 (canned cycles) codes. If a
canned cycle is active (G73 through G89), the use of G00 or G01 will cancel the canned cycle.
RAPID P OSITION C OMMANDS (G00)
G00 Rapid Motion Positioning Group 01
X Optional X-axis motion command
Y Optional Y-axis motion command
Z Optional Z-axis motion command
A Optional A axis motion command
This G code is used to cause a rapid traverse of the three or four axes of the machine. The auxiliary axes B, C,
U, V, and W can also be moved with a G00. This G code is modal so that a previous block with G00 causes all
following blocks to be rapid motions until another Group 01 code is specified. The rapid traverse rate is depen-
dent on the maximum speed possible for each axis independently as modified by the RAPID override keys.
Generally, rapid motions will not be in straight lines. All of the axes specified are moved at the same speed but
will not necessarily complete their motions at the same time. The control will wait until all motions are com-
plete. Only the axes specified are moved and the incremental or absolute modal conditions (G90 or G91) will
change how those values are interpreted. Parameter 57 can change how closely the machine waits for a
precise stop before and after a rapid move.
INTERPOLATION C OMMANDS (G01, G02, G03)
G01 Linear Interpolation Motion Group 01
F Feed rate in inches (mm) per minute
X Optional X-axis motion command
Y Optional Y-axis motion command
Z Optional Z-axis motion command
A Optional A axis motion command
This G code provides for straight line (linear) motion from point to point. Motion can occur in 1, 2 or 3 axes. All
axes will start and finish motion at the same time. The rotary axis may also be commanded and this will
provide a helical motion. The speed of all axes is controlled so that the feed rate specified is achieved along the
actual path. Rotary axis feed rate is dependent on the rotary axis diameter setting (Setting 34) and will provide
a helical motion. The F command is modal and may be specified in a previous block. Only the axes specified
are moved and the incremental or absolute modal commands (G90 or G91) will change how those values are
interpreted. The auxiliary axes B, C, U, V, and W can also be moved with a G01 but only one axis is moved at
a time.
To Next Page
Loading...
Need help?
General
