Creating G code program
6.7 Machining plane, milling direction, retraction plane, safe clearance and feedrate (PL, RP, SC, F)
Milling
Operating Manual, 03/2010, 6FC5398-7CP20-1BA0
205
6.7 Machining plane, milling direction, retraction plane, safe clearance
and feedrate (PL, RP, SC, F)
In the program header, cycle input screens have general parameters that are always
repeated. You will find the following parameters in every input screen for a cycle in a G code
program.
Parameter Description Unit
PL
Each input screen has a selection box for the planes, if the planes have not been
specified by NC machine data.
Machining plane:
G17 (XY)
G18 (ZX)
G19 (YZ)
Milling direction
When milling, the machining direction of rotation (climbing or conventional) and the
spindle direction of rotation in the tool list are taken into consideration. The pocket is
then machined in a clockwise or counterclockwise direction.
During path milling, the programmed contour direction determines the machining
direction.
RP Retraction plane (abs)
During machining the tool travels in rapid traverse from the tool change point to the
return plane and then to the safety clearance. The machining feedrate is activated at
this level. When the machining operation is finished, the tool travels at the machining
feedrate away from the workpiece to the safety clearance level. It travels from the safety
clearance to the retraction plane and then to the tool change point in rapid traverse.
The retraction plane is entered as an absolute value.
Normally, reference point Z0 and retraction plane RP have different values. The cycle
assumes that the retraction plane is in front of the reference point.
mm
SC
Safety clearance (inc)
Acts in relation to the reference point. The direction in which the safety clearance is
effective is automatically determined by the cycle.
The safety clearance must be entered as an incremental value (without sign).
mm
F Feedrate
The feedrate F (also referred to as the machining feedrate) specifies the speed at which
the axes move during machining of the workpiece. The machining feedrate is entered in
mm/min, mm/rev or in mm/tooth before programming a cycle.
The maximum feedrate is determined via machine data.
mm/min
mm/rev
mm/tooth
To Next Page
Loading...
Need help?
General
