Sign in to follow this  
Nightsky84

YCM 4th Axis Post Edit Help!

Recommended Posts

I have a ycm 4th axis post that works perfectly as far as machining. The only thing I want to change is how do I get rid of it going back to A0. at the end of every tool change?? Like I will be machining at a 90degree angle and the next tool will do the same but before it gets to the next tool it wants to home to A0. first then change and go back to A90. or whatever angle I am machining at. I have to manually delete the A0. out of every tool change to make sure it doesn't go back. Thanks!! If you need to see my post I can attach it let me know!

Share this post


Link to post
Share on other sites

There might be a switch in the post to tell it not to go home at each index, but without everything in front of me to see it hard to tell. when you reached out to your Local Mastercam Dealer what did they recommend?

Share this post


Link to post
Share on other sites
3 hours ago, Nightsky84 said:

The only thing I want to change is how do I get rid of it going back to A0.

This could be in pretract, pretract0 or peof depending on your starter post. My bet is its a string literal so look at these postblocks and see if there is a "A0" on an output line.

As Ron said, I have mine set up via Mi 7 and Mr 7 to give me a choice whether I output (Mi 7), and if I want it to go to a specific rotation angle I enter that in Mr 7.

But this is not the default post condition, so you may have to hunt a little, depending if the post editor knew what he / she was doing.

Do you know how to use the debugger?

Share this post


Link to post
Share on other sites

Easy.

Look for this switch in your Post:

frc_cinit : yes$

change to:

frc_cinit  : no$

The variable name is "force 'C' initialize". (In the 4 Axis Posts, 'c$' is the 'Rotary Address Variable', even though it is typically configured to output either 'A' or 'B'.

 

  • Like 1

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
Sign in to follow this  

  • 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