Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

G49 Without Movement


Recommended Posts

I'm sure this has been covered, but the search function around here ain't what she used to be...

We had a scary situation that we need to find a fix for. We were running a program with a short tool and at the end we had a G49. When it read the G49, the machine was going to move Z-7.5”. This is probably the difference between our dummy tool we pick up with and the actual tool we were cutting with. We were running in single block and noticed the distance to go, so nothing bad happened. 

I know G49 cancels height offset, and I know it’s needed before a G05.1 Q# R# can be called. I vaguely remember a parameter or something that makes the G49 happen without commanding movement. Our control is a Fanuc 31i and my last Fanuc experience was way back in 16m days.
 

Link to comment
Share on other sites

We don't use it on any of our other Fanuc based machines. But it is necessary on machines with any flavor of Fanuc's high speed mode.

Pretty sure it's parameter 5006 and bit# 6 that controls whether the G49 causes movement or not. Waiting on our operator to test it.

Link to comment
Share on other sites

What happens might also depend on how your offsets are set up. If you run +ve (positive )value tool offsets then watch out, as cancelling will cause you to head for the table. You will also head for the table if you forget to enter a +ve offset.  I always prefer -ve offset values as the worst that can happen is a Z positive over travel.

Having said that many if not most shops are set up for +ve tool offsets (and I understand why this is so), and its difficult to change this once you are "baked in" on your existing process......

Let us know how the parameter fix works out as this would be an excellent safety.....

Link to comment
Share on other sites
18 minutes ago, Newbeeee™ said:

G49 after high speed has been cancelled.

Here's the code which ran on our robos (31i), and Chevalier 0imC, 0imD, 0imF controls

Capture.JPG

Yes. You can turn it off whenever, but you need the G49 before you turn it back on.

Link to comment
Share on other sites
Just now, Tim Johnson said:

Here's a Postler reply from the same situation.

 


Tim,

Thanks here are two parameters to try.    

5006.6  Be sure it is set to 1
11260.0 Be sure it is set to 1

Try those and test carefully.    I will get on the machine if I get a chance today and check myself


Dave Postler

Min'e working so one or both did it.

Poor Dave must be getting sick of me. I still haven't heard back from him today.

We changed 5006.6 to one this AM. Operator still hasn't gotten around to testing it.:rolleyes:

Link to comment
Share on other sites
5 minutes ago, Tim Johnson said:

I've just checked a GE480H and both are turned on.

Awesome. Thanks.

I had no idea about the 11260. Have no idea what it is, but I set it to 1.:thumbup:

Speak of the :devil:...

Quote

 

Dear Greg,

There are a few parameters that control this try setting the following parameters.

5006 bit 6             Change from 0 to 1
11260 bit 0           Change from 0 to 1

If those 2 parameters do not work try these as well.

5002 bit 2             Change from 0 to 1
5002 bit 4             Change from 1 to 0

Also be careful when checking this out.  Use dry run keep near estop etc. 

Dave Postler

 

Good thing we were near the e-stop when we ran it how it came from the factory.:ermm:

Link to comment
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

 Share

  • 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

×
×
  • Create New...