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cpoirier1-Visitor
1-Visitor
August 25, 2021
Solved

I am unable to show a hidden part.

  • August 25, 2021
  • 3 replies
  • 9210 views

Hello, I am using Creo Parametric 3.0 M150 and having some difficulty with a hidden part.

I have a main assembly where a component in a sub assembly is hidden and I can not find a way to show it. The part is visible when the sub assembly is open. It is not on a layer, it is not hidden, there is no simplified rep substitution hiding it, the master rep is active, there is no family table, the appearance is something I can see. I am at a loss as to why this part is hidden. I have obviously missed a trick somewhere. The user who did this is no longer with the company. I am wondering if there is a tool not on the toolbar he used. I found he never used simplified reps and always chose to hide the component in the drawing.

Best answer by cpoirier

I found it! It is an assembly cut only cutting the component that is hidden. The system says it was made in this assembly and gave me the feature name, I found all this by selecting the feature>rt click> information>references, I'll find the silly thing using the search tool next. Please pardon me but why the expiative, bleep bleep would anyone do this? I used model player and it briefly showed up, this was a hint. Oddly I went to far and canceled out by mistake. After canceling insert mode and slowly using model player it did not show up a second time probably clicking around too fast. That's odd, but par for the course today.

 

Chris

3 replies

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TomU23-Emerald IV
23-Emerald IV
August 25, 2021

What happens if you switch from 'Default Rep' to 'Master Rep'?

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cpoirier1-VisitorAuthor
1-Visitor
August 25, 2021

Stays hidden in either rep. I can not figure out how this items is hidden. Is there a similar tool like: layout tab>component display>blank in drawing mode.... only in an assembly mode? I'm going to search the tools in the customize the ribbon window next and see if I can make something work like component display.

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TomU23-Emerald IV
23-Emerald IV
August 25, 2021

The pictures you took show that you are in insert mode with a simplified rep active.  Are you *positive* that insert mode is not active and you are in the master rep?  (It should show master rep in the text on the screen.)

StephenW
StephenW23-Emerald III
23-Emerald III
August 25, 2021

With respect to the visibility of a part similar to component display/blank, these is the style command in the view manager, but it should also display on the screen that you are in a Style State.

I don't think Creo 3 had layer controls that could vary in top level assemblies.

Does the part  just happen to be a surface model?

StephenWilliams_0-1629919127323.png

 

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cpoirier1-VisitorAuthor
1-Visitor
August 25, 2021

Found it, it was an assembly cut.

kdirth
kdirth21-Topaz I
21-Topaz I
August 25, 2021

Another trick to watch out for is using flexibility to suppress a component, my favorite way to remove an unneeded part (usually only there for shipping) from an assembly.

There is always more to learn.
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cpoirier1-VisitorAuthor
1-Visitor
August 25, 2021

I've never used flexibility before, I'll have to check it out.

Thank you for the heads up.

 

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