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YJ_145925906-Contributor
6-Contributor
June 23, 2026
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Multibody drawing, separate body for each view, for a mould

  • June 23, 2026
  • 5 replies
  • 127 views

Hey

I have a Mould that has 3 Bodies

When I make a drawing I want to show only one of each bodies.

 

My goal is 

in the 1st sheet I will show the views of  top part of the mould

in the 2nd sheet I will show the views of middle part of the mould

in the 3rd sheet I will show the views bottom part of the mould

and in the 4th sheet I will show 1 view top part and another view middle part and so on..

 

each sheet will have top view, bottom view and side views of the body

 

 

Please let me know how I can do it

Best answer by tbraxton

I would propose an alternate that I think would be faster than creating combination states and simplified reps in the multibody model. You may not be aware that in a drawing you can reference more than one model such that you can place views from multiple models on sheets within the drawing. You could use this functionality as well by saving each body as a part in your design model. You would then add each of these three part models to the drawing and then create views on each sheet as desired for each mold component. You can do this by setting the active model in the drawing to then place the views as needed on each sheet.

 

In general, I would not use a design model (your multibody model for the mold) to create 2D drawings or even for MBD definitions. I would save each body as part and add the inspection data etc. at the part level. This is a choice and you should consider how your workflow including 2D drawing creation is impacted by either approach.

 

5 replies

Michael_Bourque
Michael_Bourque12-Amethyst
12-Amethyst
June 23, 2026

Yes you can do this, but do not try to hide/show bodies manually on each drawing sheet. The better workflow is to create body specific display states as simplified representations in the part, then assign the correct state to each drawing view.

Michael Bourque
    Y
    YJ_145925906-ContributorAuthor
    6-Contributor
    June 23, 2026

    But I’m not able to change the simplified representation.
    How do I activate it?

    Michael_Bourque
    Michael_Bourque12-Amethyst
    12-Amethyst
    June 23, 2026

    Create a combination state that represents each body and rep so that it hides the other bodies. Then when you create a sheet, choose the drawing models ui to select that combine state. Then you can edit the view and choose which combination state would be shown. Which version of Creo are you on and maybe I can send you an example. I tested this in Creo 13.

    Michael Bourque
    Y
    YJ_145925906-ContributorAuthor
    6-Contributor
    June 23, 2026

    I’m using creo 11.0.1.0 academic edition
    Will try doing it again.


    And yes, an example would be helpful

    Michael_Bourque
    Michael_Bourque12-Amethyst
    12-Amethyst
    June 23, 2026

    I could send example, but I doubt you would be able to open in academic version. Will try to recreate in V11

    Michael Bourque
    tbraxton
    tbraxton22-Sapphire IIAnswer
    22-Sapphire II
    June 23, 2026

    I would propose an alternate that I think would be faster than creating combination states and simplified reps in the multibody model. You may not be aware that in a drawing you can reference more than one model such that you can place views from multiple models on sheets within the drawing. You could use this functionality as well by saving each body as a part in your design model. You would then add each of these three part models to the drawing and then create views on each sheet as desired for each mold component. You can do this by setting the active model in the drawing to then place the views as needed on each sheet.

     

    In general, I would not use a design model (your multibody model for the mold) to create 2D drawings or even for MBD definitions. I would save each body as part and add the inspection data etc. at the part level. This is a choice and you should consider how your workflow including 2D drawing creation is impacted by either approach.

     

      Michael_Bourque
      Michael_Bourque12-Amethyst
      12-Amethyst
      June 23, 2026

      Great point!

      Michael Bourque
      tbraxton
      tbraxton22-Sapphire II
      22-Sapphire II
      June 24, 2026

      I would ask why you state: “I want each feature that belong to the particular body also to be saved along with the body.” The save body as part is intended to be used as a top-down design tool and in that context, it makes no sense to provide access to the features used in the master model (your multi body model). If the features came when across and you could edit them in a derivative model that causes problems with circular references within the Creo environment (you have two models that can drive each other, so no master->slave paradigm).

       

      When using this method, Creo creates a new part file where the only feature is an Extern Copy Geom feature. You will not have access to the full feature tree used in the parent multibody model used to create the geometry of the body with this strategy. When using master models in a top-down design paradigm it is good to plan on how the derivative models will be used in your workflow so that you can exploit the tools in Creo to maximize efficiency across the product development process.

      With this in mind if your reason for using multibody was to split out the mold blocks (cavity, core, etc.) from the tool steel then you can split the mold steel into the required blocks and then save the bodies as parts. You can then add the features required to the split out blocks in the derivative part models such that most of the features would be in the part model derived from the master model. If you are in need of something different in terms of managing design intent, if you provide details of what you are trying to accomplish then you will get some suggestions.

        S
        S_Edgenear15-Moonstone
        15-Moonstone
        June 25, 2026

        There are workarounds as mentioned, but it would be very useful to have this capability in a future Creo version. There have been no Drawing module improvements at all in the last few Creo versions.

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