lowcountrycamo

HOW TO USE CALL OO88?

Recommended Posts

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

Share this post


Link to post
Share on other sites

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

  • Like 1

Share this post


Link to post
Share on other sites

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.

Share this post


Link to post
Share on other sites

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.

Share this post


Link to post
Share on other sites

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

Share this post


Link to post
Share on other sites

Create an account or sign in to comment

You need to be a member in order to leave a comment

Create an account

Sign up for a new account in our community. It's easy!

Register a new account

Sign in

Already have an account? Sign in here.

Sign In Now

  • Recently Browsing   0 members

    No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us