10.4.5
Thread undercut (CYCLE940)
Function
The "Thread undercut DIN" or "Thread undercut" cycle is used to program thread undercuts
to DIN 76 for workpieces with a metric ISO thread, or freely definable thread undercuts.
Approach/retraction
1. The tool first moves to the starting point calculated internally in the cycle at rapid traverse.
2. The first cut is made at the machining feedrate, starting from the flank and traveling along
the shape of the thread undercut as far as the safety distance.
3. The tool moves to the next starting position at rapid traverse.
4. Steps 2 and 3 are repeated until the thread undercut is finished.
5. The tool moves back to the starting point at rapid traverse.
During finishing, the tool travels as far as cross-feed VX.
Procedure
1.
The part program or ShopMill program to be processed has been created
and you are in the editor.
2.
Press the "Turning" softkey.
3.
Press the "Undercut" softkey.
4.
Press the "Thread undercut DIN" softkey.
The "Thread Undercut (DIN 76)" input window opens.
- OR -
Press the "Thread undercut" softkey.
The "Thread Undercut" input window opens.
G code program (undercut, thread DIN) parameters
ShopMill program parameters
PL
Machining plane
T
SC
Safety clearance
mm
D
Cutting edge number
F
Feedrate
*
F
Feedrate
mm/min
mm/rev
S / V
Spindle speed or
Constant cutting rate
rpm
m/min
Programming technological functions (cycles)
10.4 Turning - milling/turning machine
Milling
Operating Manual, 08/2018, 6FC5398-7CP41-0BA0
529
