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:

Home / Ref. Points Not consistently posting


N.Skinner
 Share

Recommended Posts

I have seen this happen in most toolpaths I use. Mainly Contour toolpaths because that's what I mainly use. Put simply, Lets say I turn on Z home ref points for both approach and retract. I input 6.0 inches. When I post, depending on the day or hour of the day, the 6.0 will show up or won't show up. It's a roll of the dice.

Link to comment
Share on other sites

I have seen this happen in most toolpaths I use. Mainly Contour toolpaths because that's what I mainly use. Put simply, Lets say I turn on Z home ref points for both approach and retract. I input 6.0 inches. When I post, depending on the day or hour of the day, the 6.0 will show up or won't show up. It's a roll of the dice.

 

Okay are the incremental or absolute? Are you a WCS or not? Many factors go into the output of code and just putting a 6.0 in the box may or may not give you a 6.0. There are many things that control the output not just checking a box.

  • Like 1
Link to comment
Share on other sites

Using a G54 WCS. Using Absolute. Like I said-- Same file, same parameters, different times posting = different results within the program. I know it sounds like I'm missing something simple, but trust me, I have looked at all angles. I have used MasterCam since X6 and now on 2017. I saw this problem at X9 and it is still there on 2017.

Link to comment
Share on other sites

Unfortunately, due to the nature of what I manufacture, I cannot share a file. And unfortunately it sounds like I'm the only one with this problem.

 

I believe it must be a post error so I am contacting MasterCam now. 

 

The fact that I can post and It will show up correct - close file - next day open file - and the ref points will be missing from the program next time I post. Its sporadic and can't be trusted...

Link to comment
Share on other sites

Unfortunately, due to the nature of what I manufacture, I cannot share a file. And unfortunately it sounds like I'm the only one with this problem.

 

I believe it must be a post error so I am contacting MasterCam now. 

 

The fact that I can post and It will show up correct - close file - next day open file - and the ref points will be missing from the program next time I post. Its sporadic and can't be trusted...

Is your workstation/windowze configuration set so you're the administrator?

Post/machine/control defs properly upgraded from the previous release?

Something's not right that's for sure.

 

Create a simple rectangle or whatever shape, throw on a toolpath and set the parameters as you would and trial it.

If this simple file causes you issues, post it here but also create a zip2go and mail it to your reseller and [email protected] so they can see it.

Link to comment
Share on other sites

Well I program some very involved and complex projects and it is something I have not had an issue with. If I had I would confirm your findings, but I have not so I have to start doing some detective work from who know how many thousands of miles away. Make some sample files and try it out. Easy to reproduce on your end with something you can share. Then post is up and we will see if we see the same thing you are seeing. If we are more support to get a bug fix if we don't then we help you track it down and figure out why you are seeing it.

  • Like 1
Link to comment
Share on other sites

I've had issues with Reference Points not sticking sometimes. I found another one that bit me the other day.

 

  • Enable "Incremental" Approach and Retract of some value. Say "3.0" inches. That should be 3" above whatever geometry you are driving, or the Top of Stock value, depending on how you setup your Linking Parameters.
  • I use them, they post, everything looks good.
  • Move the Origin of your Tool Plane to some new point. I moved mine from the bottom of my part, to Z 3.5". (Now all the depths are "negative" in Z, but all my Linking are still "incremental" from the geometry, and the paths look good, except...
  • The Reference Points have now changed to "-.5" Incremental.
  • When moving the Origin of your Plane, the Reference Points should only be changed in the height of the approach/retract, if the move was specified in Absolute coordinates. When set to "Incremental", that value should remain the same. "3.0" above your geometry is still "3.0" above your geometry, no matter where the Origin of the Plane is located. Yes, the Z values in the NC code change, but the actual height of the move should not.

 

The way I got around this, and this will apply to N.Skinner as well, was to use the "Point" operation.

 

Now, what is a Point Operation you ask? Many people don't know about Point Operations, and have never had the need to use them.

 

  1. A 'Point' Operation is simply Point-to-Point motion that you specify in a Tool Path.
  2. It is about the most simple Operation you can create in Mastercam.
  3. Start by creating some Point Geometry. If you are using "Approach" and "Retract" moves at the start op, and end op of a sequence, then add a "Point" Operation in front of the ops, and one after the ops. So create a Point or an Arc
  4. With Toolpaths > Point, you simply select "Rapid" or "Feed" mode, and then pick the points that you want to move to. You could actually create simple toolpath cutting motion if you desire, but most of the time I use "Point" as an Approach or Retract move.
  5. That's pretty much it. Pick the Point you want to move to (the motion "to" the point is from the machine Tool Change Position), and then pick the tool. Give it an RPM if you want the tool to turn on.
  6. You can then copy/paste the point move after the group of Ops, or single Op, that you want a Retract move afterwards.

The nice thing about the Point Ops is that they will Post 100% of the time, and you can see them as Operations in the Ops Manager. Now you don't have to go through and check out the Reference Points options on a bunch of paths. Just use "Edit Common Parameters", and disable the Ref Points, and let the Point Toolpaths take care of it...

  • Like 1
Link to comment
Share on other sites

I have seen this happen in most toolpaths I use. Mainly Contour toolpaths because that's what I mainly use. Put simply, Lets say I turn on Z home ref points for both approach and retract. I input 6.0 inches. When I post, depending on the day or hour of the day, the 6.0 will show up or won't show up. It's a roll of the dice.

 

I have seen that happens to me few times. Most of the time I see this problem with approach. Its checked and value is there, But approach moves wouldn't post and doesn't show up in back plot. I usually have to end up re-doing that tool path from scratch as work around. 

Link to comment
Share on other sites

I have seen that happens to me few times. Most of the time I see this problem with approach. Its checked and value is there, But approach moves wouldn't post and doesn't show up in back plot. I usually have to end up re-doing that tool path from scratch as work around. 

Try to force regenerate (Select all toolpaths and push the regenerate with the green sideways triangle). I'm just doing it to the whole file now everytime before i post. It is working and i'm so glad i'm able to trust it again

  • Like 1
Link to comment
Share on other sites
  • 1 month later...

Try this

Save and close your file

Saving a back up copy can't hurt

open a fresh empty session

Open System Configuration/Files

Uncheck "Restore entire toolpath data in File Open"

now open your file

Every single toolpath will be dirty

Regen and check your Reference Points.

This has worked for me several times

 

next time I run into this, I will try N Skinner's "Force Regen" suggestion

Its a whole lot simpler than mine

Link to comment
Share on other sites

Ok I have my answer!!!

 

In order to ensure the approach and retract values posted I was told to "Force" regenerate and it works!!!

 

 

Now that you mention it I have this issue as well.  In fact it's such a habit that any time I change anything I force regenerate.  Period.

Link to comment
Share on other sites

Try this

Save and close your file

Saving a back up copy can't hurt

open a fresh empty session

Open System Configuration/Files

Uncheck "Restore entire toolpath data in File Open"

now open your file

Every single toolpath will be dirty

Regen and check your Reference Points.

This has worked for me several times

 

next time I run into this, I will try N Skinner's "Force Regen" suggestion

Its a whole lot simpler than mine

 

 

Worked!  Pain in the butt, however, since this has cost me a spindle before, not terribly worried about the extra effort.

  • Like 1
Link to comment
Share on other sites
  • 2 years later...
On 12/12/2016 at 1:05 PM, N.Skinner said:

Unfortunately, due to the nature of what I manufacture, I cannot share a file. And unfortunately it sounds like I'm the only one with this problem.

 

I believe it must be a post error so I am contacting MasterCam now. 

 

The fact that I can post and It will show up correct - close file - next day open file - and the ref points will be missing from the program next time I post. Its sporadic and can't be trusted...

 

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

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

 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

×