Please Note While Programming - HEIDENHAIN TNC 620 User Manual

5
Fixed cycles: Pocket milling / stud milling / slot milling
5.2 RECTANGULAR POCKET (Cycle 251, DIN/ISO: G251, software
option 19)

Please note while programming:

With an inactive tool table you must always plunge
vertically (Q366=0) because you cannot define a
plunging angle.
Pre-position the tool in the machining plane to the
starting position with radius compensation R0. Note
parameter Q367 (position).
The TNC automatically pre-positions the tool in the
tool axis. Note the 2nd set-up clearance Q204.
The algebraic sign for the cycle parameter DEPTH
determines the working direction. If you program
DEPTH=0, the cycle will not be executed.
At the end of the cycle, the TNC returns the tool to
the starting position.
At the end of a roughing operation, the TNC
positions the tool back to the pocket center at rapid
traverse. The tool is above the current pecking depth
by the set-up clearance. Enter the set-up clearance
so that the tool cannot jam because of chips.
The TNC outputs an error message during helical
plunging if the internally calculated diameter of the
helix is smaller than twice the tool diameter. If you
are using a center-cut tool, you can switch off this
monitoring function via the suppressPlungeErr
machine parameter.
The TNC reduces the infeed depth to the LCUTS tool
length defined in the tool table if the tool length is
shorter than the Q202 infeed depth programmed in
the cycle.
Danger of collision!
Use the machine parameter displayDepthErr to
define whether, if a positive depth is entered, the
TNC should output an error message (on) or not (off).
Keep in mind that the TNC reverses the calculation
for pre-positioning when a
entered. This means that the tool moves at rapid
traverse in the tool axis to set-up clearance
the workpiece surface!
If you call the cycle with machining operation 2 (only
finishing), then the TNC positions the tool in the
center of the pocket at rapid traverse to the first
plunging depth.
134
positive depth is
below
TNC 620 | User's Manual Cycle Programming | 3/2014