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Repeat Region: Shown in Drawing? (Creo 2.0)

wjamieson
4-Participant

Repeat Region: Shown in Drawing? (Creo 2.0)

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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1 ACCEPTED SOLUTION

Accepted Solutions

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


Martin Hanák

View solution in original post

12 REPLIES 12

William,

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

Martin Hanak


Martin Hanák

Shown or not shown in what way?

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

wjamieson
4-Participant
(To:dschenken)

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.

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.ht...

wjamieson
4-Participant
(To:wjamieson)

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

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


Martin Hanák

View solution in original post

William,

There is no direct option for Yes/No for Included components in repeat region. If I need to accomplish this in my drawings I will add component parameter in assembly components and will call component parameter in repeat region.

1. In assembly > Parameters set Look in for Component > Select included component > Add String parameter and add Value as No, (Add same parameter for all components with value as Yes)

2. In repeat region call report parameter asm>mbr>cparam> User defined> Enter added parameter> Done.


This will display the value of parameter added at component level.

Where do I find assembly> parameters? Thanks for your help.

William,

in Creo Parametric 2.0

  1. open an assembly
  2. activate Tools tab
  3. use Parameters button

Martin Hanak


Martin Hanák

param.jpg

William,

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

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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