Siemens SINUMERIK 840D sl Operation/Programming Manual page 317

08/2005
5
Machine counterspindle
Rear side
♥ Siemens AG, 2005. All rights reserved
SINUMERIK 840D sl Operation/Programming ShopTurn (BAT) – 08/2005 Edition
5.9 Machining with the counterspindle
When the rear face is machined, ShopTurn automatically transposes
the coordinate system into a mirror image, i.e. you program the
machining operation for the rear face as for the front face.
Make sure that the Y axis points to the opposite direction during
milling operations. If this is not wanted, then mirroring of the Y axis
must be programmed.
Machine counterspindle (without first transferring workpiece)
The programming might look like this:
1. Rear face
WO: Work offset is only activated
ZV: Parameter is not calculated.
2. Machine counterspindle
Please note the following special features of the "Rear face" program
step when machining on the counterspindle without first transferring
the workpiece.
The work offset that you choose in the parameterization screen form is
only activated and not calculated. This means that the workpiece zero
for counterspindle machining should be stored in the work offset.
In addition, parameter ZV is not calculated.
Machine bars
If you use bars to produce your workpieces, you can machine several
workpieces on the front and rear face by starting the program just
once.
Machining of bars can be programmed as follows, for example:
1. Program header specifying the work offset in which the workpiece
zero is stored
2. Machine main spindle
3. Complete (pull blank: Yes; Parting cycle: yes)
4. Parting
5. Machine counterspindle
6. End of program with number of workpieces to be machined
Alternatively you can program the machining of bars as follows:
1. Start marker
2. Machine main spindle
3. Complete (pull blank: Yes; Parting cycle: yes)
4. Parting
5. Machine counterspindle
6. Front side
7. End marker
8. Repeat from start to end marker
ShopTurn Functions
5
5-317