HOW TO USE CALL OO88?

[lowcountrycamo 35]

I want to use CALL OO88 on a MU 4000 and MU 6300 okuma.   Do you post out CALL OO88 with every rotation move? Or just at the start of the program and the control keeps up with the zero from there on.  Also, do I need to cancel?  

Thanks,

Steve Austin

[Greg Williams 105]

Yes correct with every rotation move, attached is a sample, Basically it runs a macro in the control and recalculates a new work offset based on the PP and PH numbers, the control then uses the new work offset. Selecting the original work offset will turn it off

 

5-AXIS-TEST.MIN

[huskermcdoogle 350]

CALL OO88 is just an offset calculator for 3+2 (5ax config) or 3+1(4th planar) work work only. Takes your starting offset and calculates the needed offset based on the angle inputs.  It's main advantage is that it uses the kinematic offsets in the control instead of them being hard coded in the program.  Generally speaking the macro also has framework for many different types of machines built into it.  When initially setup you have to configure the macro for you machine, but if the kinematic offsets get updated down the road you shouldn't have to do anything to the CALL OO88 program.

[Brad Lisle 71]

You can have it at the header for each offset you want to use or at each rotation output. Either way works fine as long as you call up the correct work offset numbers. I personally like them at the header. The CALL OO88 is just a calculation tool, therefore there is no mode that needs to be cancel ed. When you change work offsets it will effectively cancel the previous offset. 

As you can see in Greg's sample code the post is setup to always use the same temporary offset #51 and always references offset #1. Using this format you must have it at every rotation to recalculate every time and it also calls up the temp offset #51 to be active. I have my post setup to program using different work offset numbers for various tool planes. Similar to other posts that do not use "CALL OO88" and outputs a different offset for each rotation. Using this method you only need the CALL OO88 statement only once and it can be anywhere before the offset is called, IE... beginning of program. Just make sure you always call up the active work offsets.

[lowcountrycamo 35]

I have a postability post and it is only posting at header.  Not for every rotation. I need to figure that one out.  

[Greg Williams 105]

If you are resetting the WCS this may be the issue

[Jwfich 0]

So the CALL OO88 can not be used with live 5-axis machining

[lowcountrycamo 35]

No only 3+2