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ptc-31164191-Visitor
1-Visitor
August 8, 2014
Question

Need help with drawings in Creo 2

  • August 8, 2014
  • 4 replies
  • 14298 views

Okay I'm in Pro E Creo 2.0 and working on a drawing. I normally work on NX and these two do not work the same. The original assembly I set the drawing to was named incorrectly so I did a save as on the assembly. I am trying to replace the old assembly in the drawing with the new one that has the correct name and it's a big fail. I am able to "set" the new model in the drawing but cannot get the views to update to the new model. Now this drawing pulls in both models if I close and re-open it. I am unable to delete the old model from the drawing without getting the error "Cannot delete model with views using it" How do I get rid of the old model and update the views to display the new one?


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4 replies

J
JamesBurcham1-Visitor
1-Visitor
August 8, 2014

If the model are not part of the same family table or interchange they will not directly replace. If you are replacing a model in a drawing with a completely unrelated model you are almost better off just starting a new drawing. To remove a model from a drawing you need to remove everything related to it. That means all views that contain that model, and any notes or tables linked to that model.

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ptc-31164191-VisitorAuthor
1-Visitor
August 8, 2014

I've been on several different CAD systems over the last 20 years and ProE has impressed me the least. User unfriendly and remedial. What takes 4-5 pokes in NX or Catia takes at least twice that in ProE or the task can't even be done at all. As simple a thing as replace a model in a view cannot be done. Shame on PTC.

    R
    ReinhardN1-Visitor
    1-Visitor
    August 8, 2014

    Why dont you

    - rename the assembly to the old name

    - open the drawing

    - rename the assembly to the new name

    - save drawing and assembly

    For renaming you must have all dependent objects in session. ProE will correct all dependencies for you.

    And dont forget to save.

      D
      dgschaefer21-Topaz II
      21-Topaz II
      August 8, 2014

      Assuming that you are not using Windchill or another PDM, an easier approach would have been to open the drawing and any assemblies that contain that assy and use the rename command in Creo. Then all objects that refer to [old].asm will now refer to [new].asm.

      If you've already replaced the old assy with the new everywhere but the drawing, you can trick Creo into using the new assy using the method Reinhard suggested. To clarify, you open the newly named assy, use the Creo rename in session function to rename it back to the old name, open the drawing, go back to the assy and use the Creo rename in session function to rename it back to the new name, save all.

      You shouldn't loose anything with either method.

      R
      ReinhardN1-Visitor
      1-Visitor
      August 9, 2014

      As you can do much damage with renaming I usually work with copies in a separate folder after I have erased all objects from memory. If everything was successful I copy them back to my working dir.

      Reinhard

      D
      dschenken1-Visitor
      1-Visitor
      August 9, 2014

      If it worked just like NX it would be NX.

      The reason for Creo not to replace models in views with unrelated models is that the view structure begins with the model - orientation, scaling, sections - and without those things the view no longer exists. There are special cases where a model can have variations, such as family tables, that have suitably identical structures and can be easily replaced.

      You could have created a temporary family table in the original item, replaced the model in the drawing from the family table, then deleted the table and, in saving the drawing, saved the new model with the new name. I have to assume that you wanted to keep the wrong name model and the right name model, otherwise you would have just renamed the model.

      Still waiting for the software endpoints analysis so that users can see what they know and don't know and can search them for results they want so they can backtrack on how to get them. Someone should have written them down before developing the software; they don't just pick a bunch of steps and then say to themselves, 'what should happen now?'

      T
      TomD.inPDX17-Peridot
      17-Peridot
      August 9, 2014

      So here's a question... how do templates deal with predefined views when the model changes on creating a new drawing?

      D
      dschenken1-Visitor
      1-Visitor
      August 9, 2014

      Here's a better one. I searched for NX views to see just how easy things are over there and found

      "As Cowski mentioned projected views are not associative with their base views once that they have been added to the sheet. Section views are dependant upon how the section cut is defined as to some extent are the detail views upon boundary definitions. I think that the sheer complexity involved in re-orienting views as you appear to suggest invites a number of problems that may challenge the drafter's ability to confidently control the results, which is why I don't find myself warming to the idea."

      The rest is at http://www.eng-tips.com/viewthread.cfm?qid=271309

      D
      dhermosillo15-Moonstone
      15-Moonstone
      October 3, 2014

      @Jeff, are you using Creo stand alone or in a linked session with Windchill?

      If it is the former, then any of the aforementioned methods will work.

      If you are using Windchill, select both the drawing and the model in your workspace and do a save as. This will copy the drawing and the model to a new drawing and model. The last step is to go into Windchill and rename the the files to what you want them to be. If you aren't going to use the original anymore, we usually just append it with _obsolete.

      Keep in mind that Creo/Windchill currently has a limitation that will not let modified items be copied. I know it's stupid and I've filed a ticket with PTC, but they refuse to acknowledge that it's a bug. It is particularly annoying since that is how a lot of new iterations happen; you start to modify a model and then realize it should be another part entirely. PTC has no easy way to accomplish this right now.

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