I am unable to show a hidden part.

[cpoirier]

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.

[TomU]

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

[cpoirier]

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.

[TomU]

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.)

[cpoirier]

HI Tom,

Thanks for joining in on the fun, the assembly was left in insert mode, but the sub assembly is above the arrow.

I canceled insert mode. No effect, that part is still hidden. So just to see I selected the part in the tree and rt clicked>

representation>master and an odd thing happened. The entire assembly disappeared. This is while in master rep.

Chris

[TomU]

Nice.  When you selected the part and then clicked representation>master, you created an 'on the fly' simplified rep with just that one component on it.  That fact that you still don't see it confirms that something else is going on.  To get back to the master rep (for everything), open the view manager and double click on Master Rep.  That should remove the on-the-fly rep and remove the plus sign.

I'm wondering if maybe there is a layer issue....  What happens if you go to the assembly layers and hide them all and then unhide them all?

[cpoirier · Accepted solution]

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

[StephenW]

User get inventive sometimes! I know I have when I'm under the gun to get something done. I can hack with the best of them!

[StephenW]

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?

[cpoirier]

Found it, it was an assembly cut.

[kdirth]

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.

[cpoirier]

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

Thank you for the heads up.