Tapping - Siemens SINUMERIK 840D sl Operation/Programming Manual

08/2005
5

5.2.5 Tapping

1 cut
Stock removal
Chipbreaking
♥ Siemens AG, 2005. All rights reserved
SINUMERIK 840D sl Operation/Programming ShopTurn (BAT) – 08/2005 Edition
The "Tapping" function is used when you want to tap an internal
thread on the end face or peripheral surface.
The spindle speed can be changed with the spindle override during
tapping. The feed override is inoperative during this process.
You can select drilling in one cut, chipbreaking or retraction from the
workpiece for stock removal.
The tool is moved at rapid traverse to the programmed position,
allowing for the retraction plane and safety clearance.
With the spindle stationary, the tool moves at rapid traverse to the
retraction plane and then to the safety clearance.
Here the spindle begins to rotate and the spindle speed and feedrate
are synchronized.
The tool continues to move at rapid traverse towards the programmed
position.
1. The tool drills at the programmed spindle speed S or cut rate V as
far as the tapping depth X1 or Z1.
2. The direction of rotation of the spindle reverses and the tool
retracts to the safety clearance at the programmed spindle speed
SR or cut rate VR.
1. The tool drills at the programmed spindle speed S or feedrate V
as far as the first infeed depth (maximum infeed depth D).
2. The tool retracts from the workpiece to the safety clearance at
spindle speed SR or cut rate VR for stock removal.
3. Then the tool is inserted again as far as the 1st infeed depth at
spindle speed S or feedrate V and drills to the next infeed depth.
4. Steps 2 and 3 are repeated until the programmed final drilling
depth X1 or Z1 is reached.
5. The direction of rotation of the spindle reverses and the tool
retracts to the safety clearance at spindle speed SR or cut rate
VR.
1. The tool drills at the programmed spindle speed S or feedrate V
as far as the first infeed depth (maximum infeed depth D).
2. The tool retracts by the retraction amount V2 for chipbreaking.
3. The tool then drills to the next infeed depth at spindle speed S or
feedrate V.
4. Steps 2 and 3 are repeated until the programmed final drilling
depth X1 or Z1 is reached.
ShopTurn Functions
5
5.2 Drilling
5-175