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:

Kitamura cutter comp issue


Noise
 Share

Recommended Posts

We have four kitamura mills. One of them needs to have a different value than the tool number. We add 50. Example Tool#1, Diameter Offset #51. I edited the control definition to add 50. This only work when you renumber tools. I would like it to be done automatically when I post.

Thanks for any input.

Link to comment
Share on other sites
On 11/10/2019 at 5:23 PM, Allan said:

overwrite the variable for the tool offset like this:

tldia$ = t$ + 50

Allan

Allan, don't you think a MMD with a specific name used would be a good way to handle this? That way they have can a unique MMD for that machine where it controls this behavior through the post and only have the need for one post for the different machines using the MMD as the control flag in the post to force them to think about that machine they are programming for? We do this with some customers who have several 5 axis machine with the same control, but have different pivot points. We control that difference in the MMD, but they only have one Post to worry about for all their different machines. They want to change the program for a different machine just change the MMD and done. Can't do this with Generic Mastercam 5 Axis posts, but that is the beauty of have a 3rd Party post is you all have taken the effort to use the MMD and CMD correctly for 5 Axis machines. 😉

Link to comment
Share on other sites

Another option could be to solve this on the machine side. In the toolchange macro you could set for example:

#800 = #4120 (H-offset)

#801 = #4120+50(D-offset) (OR +0)

Than you have to change the post to call for H#800 and D#801

One program for all machines, down side is that you can not use multiple tooloffsets.

I have done this for our Matsuura. 

Link to comment
Share on other sites
1 hour ago, Werktuigbouwer said:

Another option could be to solve this on the machine side. In the toolchange macro you could set for example:

#800 = #4120 (H-offset)

#801 = #4120+50(D-offset) (OR +0)

Than you have to change the post to call for H#800 and D#801

One program for all machines, down side is that you can not use multiple tooloffsets.

I have done this for our Matsuura. 

 matsuura uses #518 for height and #517 for d from the factory.   When using redundant tools on a pallet these will update to the duplicate tools

  • Like 1
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...