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AJ_TROGLIO14-Alexandrite
14-Alexandrite
January 18, 2024
Solved

Sheet metal flat pattern simplified rep / Multi-user use with Windchill

  • January 18, 2024
  • 2 replies
  • 2237 views

We are in the process of testing Creo 8.0.0.0 and Windchill 12.  My question is regarding sheet metal flat pattern representations and multi-user use thru Windchill.

 

Our design team would like to design the formed configuration and put in the flat pattern rep.  They check this into Windchill.  Our drafting group would check out this model, do the detail drawing of the formed view, and then check these both back in. Modified parameters in the model used in the title block causes a change to the model and we're OK w/ this. 

 

At this point the Adv Mfg Eng team would like to pull out the formed design model and create a new drawing showing the flat pattern rep with the overall dimensions and the dimensions to the bend lines.  These are created dimensions in the drawing only.  Sheet 2 would be a 1:1 view for DXF output.

 

In our testing, the act of creating a new drawing and creating dimensions in the drawing has caused a 'change' to the design model such that Windchill sees it as being changed.  The AME group does not have permissions to check in design models. 

 

Why would the addition of creating dimensions in a new drawing kick all the way back to the model?  Definitely did not expect this behavior. 

 

Thanks...

Best answer by BenLoosli

Because of the parametric properties of the design files, the creation of the dimensions on the flat pattern are referencing model entities. Even though they are drawn dimensions, the system still treats them as being parametric and thus they could change the model.

They manufacturing team should still be able to check in the flat pattern drawing.

2 replies

B
BenLoosli23-Emerald IIIAnswer
23-Emerald III
January 18, 2024

Because of the parametric properties of the design files, the creation of the dimensions on the flat pattern are referencing model entities. Even though they are drawn dimensions, the system still treats them as being parametric and thus they could change the model.

They manufacturing team should still be able to check in the flat pattern drawing.

    A
    AJ_TROGLIO14-AlexandriteAuthor
    14-Alexandrite
    January 18, 2024

    Hi Ben

    Well I accepted the solution too soon w/o a follow up question.

     

    If I double click the created dimension in the drawing it's not giving me the option of changing the number, only reporting on what the dimension is.  I don't see how this should mark the model as changed.  I can't see the dimension in the model.   How is it actually 'changing' the design model behind the scenes?   This goes against my 30 years of Pro/E driving, but, I was never much on creating drawing dimensions so maybe it's always been this way.

     

    The user cannot check in the new drawing as it wants to drag along the changed model. 

     

    Thanks..

     

    A
    AJ_TROGLIO14-AlexandriteAuthor
    14-Alexandrite
    January 18, 2024

    I think I found the answer.  Once again, it's a config option.

     

    https://www.ptc.com/en/support/article/CS32596

     

    Option to avoid models being modified, when creating dimensions in a drawing:

    • create_drawing_dims_only yes  (default is no)
    mkajdan
    mkajdan14-Alexandrite
    14-Alexandrite
    January 18, 2024

    Maybe this is causing the issue?

     

    create_drawing_dims_only

    If this config setting is set to yes, the dimensions created in a drawing are saved in the drawing.

    If this config setting is set to no, the dimension created in a drawing are saved in the part or assembly and will show those parts or assemblies as modified.

     

    https://support.ptc.com/help/creo/creo_pma/r8.0/usascii/#page/detail/dims_saving.html

     

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