You program G15 Hx where 'x' is the coordinate system that you want to use.
You need to have a look on the Zeroset page to see how many coordinate systems you have available to you, but could be between 50 and 200 depending on your options.
Therefore G15 H1 will select coordinate system 1
G15 H2 is coordinate system 2 ect...
You can manually set the values for each system, or you can store the values in each program. That way, when you setup your fixture again, providing it is in the same position, the coordinate system is automatically loaded and used.
To program a coordinate system use the following codes:
Where the 'x' in the brackets is the coordinate system number that you want to set.
Note that you are setting the coordinate for X Y & Z but on B axis you are setting an "Offset" value.
This means that B axis is offset by whatever degrees you program.
i.e. if you have a part on the pallet that is pointing towards B90 and you want this to be B0 you would program VZOFB[x]=90
This will bring B0 to the B90 position.
Hope that makes sense to you.
The easiest way to find out the values to program is to "CAL" the required position on the ZEROSET page and then copy the values from there into your program.
You do need to make sure you reset your "B" axis offset value at the end of your program, because if you forget it will be still effective for the next job, and that can ruin your whole day! Especially if you have clocked up a job, done it, forgot to reset and machine the next job only to realise that 0.5 degree offset you needed on the last job was still active and the current job is now a bucket of scrap metal. (trust me on that one! I know! )
Hope this helps.
Good luck with the new machine.
We have written our own software to do this on the machine.
I would think I would be hung if I gave you a copy! Sorry.
A bit of a PITA to work out, but the maths is not that hard to work out.
Hope you have the Okuma software, sounds interesting.
While this type of offset has some advantages, there is a downside. The function assumes the machine has perfect geometry. While I have a lot of respect for Okuma as one of the few builders that actually checks machine geometry and delivers a report (cutting tests also), there is always some error in the machine. If you are machining anything down to a few thousandths tolerance from one B position to another there is really no substitute for picking up individual offsets for each index position.
Here is an example: I was setting up a gear housing on an Okuma MH400, and trammed the same locator pin at B0 and B90 for the Y offsets. There was a difference of .0015 in Y. The other programmer at the shop said "what are you doing" and when I explained his response was "that's bull, it should be perfect." Well that error would have put the part out of tolerance and he would have been chasing his tail to find the problem, whereas my first piece was good (at least on that feature ;-).
BTW I worked for a major machine tool builder and quantifying machine geometrical error was a big part of my job. I used ANSI B5.54 tests extensively and without getting into a long thread on the different static and dynamic error you might find, please be aware that your machine is not perfect (niether is your CMM; next time they reject your parts ask to see the R&R report).
Last edited by mfgbydesign; 06-27-2011 at 11:30 AM.
You could get around machine error/variation to some extent if Okuma has the equivalent of the EXT Offset on the Fanuc.
Alternatively, if you create your own macro to automatically calculate the new work offset position, you can designate a particular work offset as your EXT offset and incorporate it into your macro. The EXT offset has been essential to help get my bores in line...my machine sways and swells like a ship on the high seas...
This is a macro b version of the offset calculating trig, should anyone need it: -
(get offset values)
#710=(original X offset)
#711=(original Z offset)
#712=1049.97 (pallet centreline in X)
#713=-250.04 (pallet centreline in Z)