[Claude Boudreau]

Can you specify a value for work offset in bobcad or is it only determined in the controller like Mach 3 ?

[BurrMan]

Work Offsets are something set on the controller, to be able to "fake" that the geometry at "world 0" can be at many different area's. In BobCad, you can give your feature a work offset to use, 54, 55, 56....Then on your controller, you program where those offsets are located.

The way it would look to do it with BobCad, is to not use work offsets and just copy the geometry to the location where it will sit on the table and then set features to those. But this would be more difficult, unless you have a fixture that places everything on the table "exactly" where the coords should be. Work offsets allow you to zero out those areas if the fixture placement changes at all.

[Claude Boudreau]

Work Offsets are something set on the controller, to be able to "fake" that the geometry at "world 0" can be at many different area's. In BobCad, you can give your feature a work offset to use, 54, 55, 56....Then on your controller, you program where those offsets are located.

The way it would look to do it with BobCad, is to not use work offsets and just copy the geometry to the location where it will sit on the table and then set features to those. But this would be more difficult, unless you have a fixture that places everything on the table "exactly" where the coords should be. Work offsets allow you to zero out those areas if the fixture placement changes at all.

So the value you put for Work coordinate offset (1 to 26) in the Stock window when you select edit from Milling stock, has to be define in Mach 3?
And what if you dont want a work offset ? Do you input 0?

[BurrMan]

Hi Claude,
THe workoffset in the milling stock edit is global. Just leave that one at 1.

THen in BobCad, say you have 1 circle centered at zero.

Make a pocket feature and set it up the way you want. Then make a second pocket feature and set it up the same way (Or save and reload the first feature) then on the "posting tab" of the feature edit, select the next work offset ( say 2...Or that would be 55 in a default setting) Repeat this for as many pieces you will cut with work offsets.

Now in Mach3 Zero out your "machine coords" up and out of the way, then reference all home and re-zero. THis sets the machine coords to this place as zero. Now move to the first place on the table that you will be calling work offset "54" or "1" and zero out the machine (but dont reference all home...Just zero there) Now you have setup work coord offset 1. On your table, you will have your fixture with say 4 pieces, you just set one, now in Mach, on the work offsets page, you will see that G54 is set to the coords you just did. Choose the G55 field, then move your machine to the next piece on your fixture and zero that out for the G55 field and save. repeat for more offsets.

Now when BobCad outputs code, each feature will have the offset set in it, output in the code with the appropriate G54, 55, 56 etc... and when the code for pocket number 3, set at work offset G56 is read by the controller, the table will move to that area and cut the circle there.

If this is confusing to you, The machsupport website has a great tutorial on how to setup work offsets in Mach. I think it's called homing and limits.

If you want me to do some screen caps to illustrate better, I could probably put something easier to understand than this explanation together.

Let me know if this doesnt make sense.
Burr