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MichalLukac8-Gravel
8-Gravel
November 11, 2016
Question

Mixed shaded and wireframe assembly components in drawing view

  • November 11, 2016
  • 8 replies
  • 9331 views

Hello,

is it possible to set some components shaded and some wireframe in drawing view? Like in assembly mode by creating style in view manager?

In creo 3

Thanks.

Best regards

Michal

8 replies

D
dschenken1-Visitor
1-Visitor
November 11, 2016

I think so. Look at Component Display under the Layout tab.

A
AmitDeshpande18-Opal
18-Opal
November 14, 2016

Hi Michal,

The only changes to the component display, which are possible, can be found under Layout > Edit > Component Display.

HLR Display

     Hidden

     No Hidden

     Default

Style

     Standard

     Phantom Opaque

     Phantom Transparent

     User Color

Blank

Unblank

Thanks,

Amit

M
MichalLukac8-GravelAuthor
8-Gravel
November 15, 2016

Hello, thanks for reply, but nothing from component display helps..

M
MartinHanak24-Ruby III
24-Ruby III
November 15, 2016

Hi,

Amit told you what is possible. Setting some components shaded and some wireframe in drawing view is not possible.

MH

M
MasterDrew1-Visitor
1-Visitor
April 10, 2019

This isn't directly possible, but I found a work around... Overlay two identical views.

 

Start by creating a view with the desired view style, (say no-hidden). Then duplicate your sheets. On the duplicated sheet with the duplicated view, change the view settings to the other desired style (say shaded).

 

Then use the component display command to blank any components as needed. (typically you'd only need to blank components on the shaded view that you want to show as wire-frame).

 

Then move the duplicated view back to the original sheet where it should exactly overlay the original view. Attached is a zoomed in sample of such a drawing.


A shaded View overlaid on a view a no hidden view with the phantomOpque styleA shaded View overlaid on a view a no hidden view with the phantomOpque style

 

    Patriot_1776
    Patriot_177622-Sapphire II
    22-Sapphire II
    May 3, 2019

    Interesting.  Never tried to play with it before.  When you show the view in anything other than shaded, you can set the "Component Display" to show certain parts in a "Style" of "Phantom Trnsp" and a few other options, but what you CAN'T do, is set up a "Style" in an "All" state in the model where some parts are transparent etc. and use that under the "Combined state" option of the "View States" option in the view.  Sure, it'll let you select it, but it does nothing and you do not get the same visual you get in modeling mode.  You should be able to set your view display to "Shading" or "Shading With Edges" and set your combined state to get the same visual you get in the model, but you can't.  I was easily able to do this in NX 8.5 and it was REALLY nice, it's a HUGE omission not to be able to do it in Creo.  A bug perhaps?

    M
    MasterDrew1-Visitor
    1-Visitor
    May 3, 2019

    @Patriot_1776 I agree that it would be a great feature to have to be able to use the component display tool with shaded views... I wanted that feature so much I spent half a day working out the stupid work around I described above. That said I think this is a classic example of PTC calling things "Not part of Creo Parametric functionality".

     

    This is the most relevant PTC support page I could find : https://www.ptc.com/en/support/article?n=CS259603

     

    Article - CS259603

    Is it possible to have in an assembly one component displayed as shaded and the other as shaded with edges in Creo Parametric

    Created: 29-Mar-2017   |   Modified: 30-Mar-2017   
     

    Applies To

    • Creo Parametric 2.0 to 4.0

    Description

    • Is it possible to have in an assembly one component displayed as shaded and the other as shaded with edges ?
    • Is there a way to apply shaded and shaded with display component display styles to different components of the same assembly ?

    Resolution

     

    Patriot_1776
    Patriot_177622-Sapphire II
    22-Sapphire II
    May 3, 2019

    Hmmmmm, not a perfect solution, but create a quick assembly as a copy of the real one where you define colors where some are more transparent than others.  In your dwg, add it as another model, then add a shaded view of it.  Not perfect, but...

     

    Or, probably a better solution, is you could create materials that are transparent, make the assy a family table, for dwg views have an instance that is with different transparent materials for your dwg.  This is the method I'd use to keep it all in one assy.

     

    Here's a pic from a PDF of a dwg I made to test.

    Tranparent view.jpg

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