[dingo0722]

I was wondering if there is a way to have multiple offsets for the same tools on the 10UL controllers, like a G54/G55

[iMillJoe]

On our Okuma lathes, you can always use multiple offsets for the same tool. say you are finishing two different OD's, one closer to the chuck than the other, and you are having trouble holding the tolerance on the size of them, for one OD you could use the tool offset you would normally use, (say T0101 for tool 1), then when while you are moving to the next one, issue a T0111, (tool 1 using offset 11).

There is nothing I know of that works like G54/G55 on a lathe. There is only one work offset. You can programmatically change the work offset, but that has strong caveats.

[dingo0722]

We make a lot of parts that we chuck up, do some work on one side and flip the part and do some work on the back side. Getting the thicknesses dead-on is a major pain in the ass, since we have to do it through programming, and there is only 1 Z zeroset. We will have to try using the other tool offsets. I thought it might work. Do the lathes recognize tools over T12, EG would
T0125, work for tool 1 offset25.

[iMillJoe]

I that should work. When you come into to do the back side, you can use T0125. We use the same tools with different offsets all the time. The biggest problem is when the operator does not know it about it, and only sets the regular offset, you you need to make sure the set-up/operator is well informed, or you could crash, (and it's no fun lining a turret up).

[Algirdas]

if there is a way to have multiple offsets for the same tools on the 10UL controllers

sure yes. Check the turret has 8 tool stations, and OSP tool data contains 32 tool offset lines

[broby]

They way I have approached this "Multiple Operation Program" in one set of jaws is to program the new Z zeroset value in the program.
VZOFZ=1234.567 will set the Z0 point for you within the program easily, but the downside is that you need to program BOTH Z0 positions, one for the first part of the program and then the second value for the second part of the program.
If the machine is reset, restarted in the wrong way, i.e. a number search restart type of thing, then you could end up with the wrong Z0 position.
The other method, and a far better one in my opinion, is to use the Z Zero Shift function, VZSHZ=-1.25(mm) for example.
Using this method, when the machine is reset or reaches the end of the program, the machine will revert to the original Z0 position every time with out fail.
An example would be thus, You establish your Z0 position as per your normal procedure for the first end of the part.
When you have machined the first end, flip the part over and regrip the part for the second part of the program, Re-Calculate your Z0 position for the second operation and calculate the difference between these two positions, this is the value to use with the VZSHZ system parameter.
N1 (First part of job)
blah
blah
blah
.
.
.
M00 (First side done, remove part and flip over)
NRST2 G0 X400 Z800
NOP2 VZSHZ=-2.3
N0002 Continue program for Second Side...
blah
blah
blah
M2

The line number NRST2 can be used as a restart line if you need to restart at the start of the second operation.
The value on line NOP2 is the amount you will need to "move" the Z axis towards the chuck to be in the correct position for machining the second operation.

Why do it like this you ask?

Well, no more having to establish multiple offsets for any of your tools just to get them in the right position for both operations.
No more weird dimensions in your program to get the tools into the right position for the second operation.

I have found this method works great on all models since the OSP5000 series.
Cheers
Brian.