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Parts only for visualisation

AlexK
14-Alexandrite

Parts only for visualisation

Dear Community

 

I would like to show this "shelf" in a "Down" and "Up" position on the drawing. (See Image below)

 

What is the best way to add these parts to the assembly without having them on the BOM?

 

We could delete them from the BOM on the drawing, but that brings the risk of someone forgetting to delete it from the BOM. So ideally the parts would be marked as non BOM parts when placing them in the assy.

AlexK_0-1694085830713.png

Thanks for your suggestions!

 

Best wishes

 

Alex

 

 

 

1 ACCEPTED SOLUTION

Accepted Solutions
AlexK
14-Alexandrite
(To:AlexK)

Thanks for all the suggestions!

finally i've made a shrinkwrap of the dummy parts in the assy. if it is set to manual update, the dummy part can be suppressed or deleted.

View solution in original post

4 REPLIES 4
Dale_Rosema
23-Emerald III
(To:AlexK)

You can have multiple models in a drawing. The model that you either first bring in or is active when you set up the BOM should be the one with the parts that you want. You can then add additional models for other views to show what you are looking to show.

 

If it is two positions of the same model others may have better ideas, but I usually have a family table with one instance in the open (in use) position and another instance in the closed (storage) position.

I recommend taking a look at snapshots or simplified reps. These options allow you to create display states assemblies and mechanisms. They also allow you to avoid the issues related to adding multiple models to a drawing. That said, those "risks" really only apply if you're using Windchill as drawings associate to the models that are shown on them. 

 

If your shelf is constrained with a mechanism constraint, I would create two snapshots for the open and closed positions. These can then be shown on the drawing in separate views. There's a link below but also great content on YouTube related to setting these up.

 

If you do need to assemble another copy of the part, you could nest it inside an assembly that is set to be filtered from your BOM. 

 

 

 

https://support.ptc.com/help/creo/creo_pma/r9.0/usascii/index.html#page/assembly/asm/About_Dragging_and_taking_Snapshots.html# 

 

https://support.ptc.com/help/creo/creo_pma/r9.0/usascii/index.html#page/assembly/asm/About_Simplified_Representations.html# 

KenFarley
21-Topaz I
(To:AlexK)

If you're just looking to make a nice "picture" and aren't worried about the view being driven by an assembly configuration in the future, there is a somewhat "dirty" trick that could be used.

(1) Modify (temporarily) the assembly or build a new temporary assembly to show the configuration you want.

(2) Bring that temporary assembly into the drawing.

(3) Use that assembly to create the view you wish to have.

(4) Select that view and execute the command Edit->Convert to Draft Entities.

 

You'll now have a view with just drafting entities, a snapshot of the configuration you wanted. Once this view is converted, you no longer have any association with the temporary assembly, so it can be removed via Drawing Models -> Del Model.

 

Of course, now the view is just a big bunch of "dumb" geometry, but if things are in the final state, it is a way to get around having multiple models in a drawing.

 

AlexK
14-Alexandrite
(To:AlexK)

Thanks for all the suggestions!

finally i've made a shrinkwrap of the dummy parts in the assy. if it is set to manual update, the dummy part can be suppressed or deleted.

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