8.7 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 spin‐
dle direction of rotation in the tool list are taken into consideration. The pocket is then
machined in a clockwise or counter-clockwise 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)
The safety clearance specifies from which clearance to the material rapid traverse is no
longer used. The direction in which the safety clearance is active is automatically deter‐
mined by the cycle. It is generally effective in several directions.
The safety clearance is entered incrementally (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 unit of the feedrate (mm/min, mm/
rev, mm/tooth etc. ) always refers to the feedrate type programmed before the cycle call.
The maximum feedrate is determined via machine data.
Generating a G code program
8.7 Machining plane, milling direction, retraction plane, safe clearance and feedrate (PL, RP, SC, F)
Milling
306 Operating Manual, 08/2018, 6FC5398-7CP41-0BA0
To Next Page
Loading...
Need help?
General
