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Simplified Representation Style not available in Drawing

RS_9088995
2-Guest

Simplified Representation Style not available in Drawing

I am using Creo Parametric Release 9.0 and Datecode9.0.0.0

I created a Simplified Representation of an Assembly. I created a Style for the Simplified Representation. I have a drawing, I added the model to the drawing (Simplified Representation chosen). The Style grouped with the Simplified Representation does not come through.

My goal is to have some parts transparent and other parts not -- this is the Style I created. The view is an Isometric view, with shading turned on.

I moved on to re-creating the Style I already made in the assembly, in the drawing, using Component Display. Component Display isn't working. I select my components, select PhantomOpque, won't save.

6 REPLIES 6

Is your simplified rep one of the drawing models? The rep needs to be available as one of the drawing models, then set the rep model to be active before you create the view. Try this and report back.

 

In drawing mode:

Right click/ Properties/ drawing models/ set/add rep and select your Simp rep

 

This should add it to the drawing.

========================================
Involute Development, LLC
Consulting Engineers
Specialists in Creo Parametric

It is indeed. I don't know of another way to get a model into a drawing than having it set/active in the drawing. Model tree shows the part number, Representation shows the Simp. Rep. Another check, from the Drawing View combo box, View States, the correct representation shows up in Simplified Representation. I feel like I've exhausted all options, it just doesn't seem like the Style you create, save, and group with a Simplified Representation ports over to the drawing from the assembly model. 

 

Regarding this, "I moved on to re-creating the Style I already made in the assembly, in the drawing, using Component Display. Component Display isn't working. I select my components, select PhantomOpque, won't save"

Turns out this works, but only when you don't have shaded/shading with edges selected as the Display Style.

 

Creo seems to have a lot of restrictions when it comes to wanting to display things in 3D/shaded when in drawing mode. Not an issue for a lot of work, but when you're doing design intent reports, instruction manuals, diagrams, etc., it certainly does come up. 

Hello,

This is working as designed behavior.

 

Display Style included in a combined state is not applied in a drawing view.

When a Combined State is used in a drawing view it sets only the Orientation Simplified Representation Cross Section and Explode states.

In drawing the display style is controlled by Layout > Edit > Component Display

 

Refer to To Show Models in Various View States

hadardor
17-Peridot
(To:hadardor)

Hello,

This is working as designed behavior.

 

Display Style included in a combined state is not applied in a drawing view.

When a Combined State is used in a drawing view it sets only the Orientation Simplified Representation Cross Section and Explode states.

In drawing the display style is controlled by Layout > Edit > Component Display

 

Refer to To Show Models in Various View States

Certainly, the way it is working for me is exactly like it is stated in the support document. I'm not convinced it's so much "working as designed" or "intended", as much as there should be some coding done here to streamline and consolidate the feature.

 

It's intuitive to assume, especially with the big push for Model Based Definitions, if I create a Style and pair it with a Simplified Representation, I ought to be able to simply display that in a drawing. "Cannot" or "does not" is simply because it's not coded to do so. In this case, that missing code means users have to do the same thing twice, once in the model and then again in the drawing -- not intuitive or efficient.  

When critically comparing with what other CAD vendors are offering, the conclusion to be made is that in the aspect of publishing the MBD information, Creo was designed to be lacking...

I suggest you file a product enhancement idea or vote on one already submitted.  Though I had a quick look, and didn't come across one that would address exactly what you are describing.  This one - CREO-3D-PDF-Export-Template-for-MBD - if implemented, seems it could do the trick.

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