166
G Codes
96-8000 rev R June 2007
A specific X, Y, Z, A, B position must be programmed before the canned cycle is commanded. This position is used
as the “Initial Start position”.
G174 CCW Non-Vertical Rigid Tap (Group 00)
G184 CW Non-Vertical Rigid Tap (Group 00)
F Feedrate in inches per minute
X X position at bottom of hole
Y Y position at bottom of hole
Z Z position at bottom of hole
S Spindle Speed
A specific X, Y, Z, A, B position must be programmed before the canned cycle is commanded. This position is used
as the “Start position”.
This G code is used to perform rigid tapping for non-vertical holes. It may be used with a right-angle head to perform
rigid tapping in the X or Y axis on a three-axis mill, or to perform rigid tapping along an arbitrary angle with a five-
axis mill. The ratio between the feedrate and spindle speed must be precisely the thread pitch being cut.
You do not need to start the spindle before this canned cycle; the control does this automatically.
G187 Setting the Smoothness Level (Group 00)
G-187 is an accuraccy command that can set and control both the smoothness and max corner rounding value
when cutting a part. The format for using G187 is G187 Pn Ennnn.
P Controls the smoothness level, P1(rough), P2(medium), or P3(finish).
E Sets the max corner rounding value, temporarily overriding Setting 85 "Max Corner Rounding".
Setting 191 sets the default smoothness to the user specified "rough," "medium," or "finish" when G187 is not
active. The "medium" setting is the factory default setting. NOTE: Changing setting 191 to "Finish" will take longer
to machine a part. Use this setting only when needed for the best finish.
G187 Pm Ennnn sets both the smoothness and max corner rounding value. G187 Pm sets the smoothness but
leaves max corner rounding value at its current value. G187 Ennnn sets the max corner rounding but leaves
smoothness at its current value. G187 by itself cancles the E value and sets smoothness to the default smooth-
ness specified by Setting 191. G187 will be cancelled whenever "Reset" is pressed, M30 or M02 is executed, the
end of program is reached, or E-stop is pressed.
G188 Get Program From PST (Group 00)
Calls the parts program for the loaded pallet based on the Pallet Schedule Table entry for the pallet.
To Next Page
Loading...
Need help?
General
