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wjamieson1-Visitor
1-Visitor
February 11, 2015
Solved

Repeat Region: Shown in Drawing? (Creo 2.0)

  • February 11, 2015
  • 12 replies
  • 6270 views

I am trying to find a repeat region that depends on whether a component in a BOM is shown or not shown in a drawing. The BOM I am using is already populated with items that are included or assembled in the drawing. I would like to add a field that displays a "No" if the item is included in the assembly but not shown in the drawing, and a "Yes" if the item is assembled in the drawing and shown in the drawing. Does anyone know how to do this? I'm using Creo 2.0. Thanks!


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Best answer by MartinHanak

William,

I don't see any quick&simple solution.

You can create string parameter PARYESNO in your models and put Yes/No value in it manually and show the parameter value in the Repeat region.

You can use Search tool in Assembly mode and find Included components using rule Relation is equal to Unplaced. Then you can select all found models, press RMB in Model Tree and use Edit Parameters command. Then you can modify the value of PARYESNO parameters in single window.

You can also create a layer defined by rule Relation is equal to Unplaced.

Martin Hanak

12 replies

MartinHanak24-Ruby III
24-Ruby III
February 12, 2015

William,

can you upload some test data (parts, assembly, drawing) ?

Martin Hanak

dschenken1-Visitor
1-Visitor
February 12, 2015

Shown or not shown in what way?

Hiding components by layer, simplified rep, just not visible?

wjamieson1-VisitorAuthor
1-Visitor
February 12, 2015

What I'm really looking for is a field that displays "No" for components that are included in the assembly, instead of assembled. This is done in assembly mode by clicking the arrow under the "Assemble" button and then clicking "Include." This step is shown in "include.png." Included parts in an assembly do not display their geometry in the assembly, and they show up in the model tree as seen in assembly. In he attached "assembly.png," ASSEMBLE.PRT is the cube with the visible geometry, and INCLUDE.PRT is the part that is in the model tree, but not seen in the drawing. As you can see from the model tree of the assembly, the symbols for an included part and an assembled part are different. However, in a drawing, both included parts and assembled parts will appear in the BOM.

dschenken1-Visitor
1-Visitor
February 12, 2015

There used to be a filter dialog for including/excluding Unplaced and Skeletons from BOMs, but I don't find a repeat region variable associated with the assembly status. If there is a repeat region relation could be written to substitute the word for the status description.

ref http://help.ptc.com/creo_hc/creo30_pma_hc/usascii/index.html#page/pma/detail/About_Adding_Filters.html

wjamieson1-VisitorAuthor
1-Visitor
February 12, 2015

I've also attached a picture of the drawing with a BOM in it, to show how this assembly will appear in a drawing.

MartinHanak24-Ruby IIIAnswer
24-Ruby III
February 13, 2015

William,

I don't see any quick&simple solution.

You can create string parameter PARYESNO in your models and put Yes/No value in it manually and show the parameter value in the Repeat region.

You can use Search tool in Assembly mode and find Included components using rule Relation is equal to Unplaced. Then you can select all found models, press RMB in Model Tree and use Edit Parameters command. Then you can modify the value of PARYESNO parameters in single window.

You can also create a layer defined by rule Relation is equal to Unplaced.

Martin Hanak

    Mahesh_Sharma
    Mahesh_Sharma22-Sapphire I
    22-Sapphire I
    February 19, 2015

    William,

    Are you able to get the desired results by using any of the suggestions?

    wjamieson1-VisitorAuthor
    1-Visitor
    February 20, 2015

    The solutions posted are able to work. Since a lot of our drawings have BOMs that have parts not shown in the assembly, I hope we could see an automatic relation added to a future release of Creo Parametric.

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