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
The only changes to the component display, which are possible, can be found under Layout > Edit > Component Display.
Amit told you what is possible. Setting some components shaded and some wireframe in drawing view is not possible.
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.
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?
@FrankSSchiavone 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 ParametricCreated: 29-Mar-2017 | Modified: 30-Mar-2017
- Creo Parametric 2.0 to 4.0
- 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 ?
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.