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 always repeat.
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
- only for milling
When machining a pocket, a longitudinal slot or a spigot, the machining direction (climbing
or conventional) and the spindle direction are taken into account in the tool list. 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 traverses 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 traverses at the machining fee‐
drate away from the workpiece to the safety clearance level. It traverses 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 determined by the
cycle. Generally, it is effective in several directions. 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 when machining 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.
Creating a G code program
8.7 Machining plane, milling direction, retraction plane, safe clearance and feedrate (PL, RP, SC, F)
Turning
272
Operating Manual, 06/2019, A5E44903486B AB
