topic Re: Exploded view transparency in drawing environment in Inventor Forum

Exploded view transparency in drawing environment

imbik — Sat, 22 Apr 2023 11:35:48 GMT

Hi, it is me again. I do know that part transparency in drawings has been discussed and even partially solved in this forum but is there really a satisfactory solution for how to get exact same result (or reasonably acceptable) both in assembly and drawing files with exploded view?

I have attached pictures of the same assembly in both environment and whatever I do/try ( adding transparency, changing BOM from normal to reference, selecting part priority, changing colour (component properties), contacting to Nasa, tweeting to Alon Musk, etc. none of them actually gives you the same result 🙂

I have been fighting with Inventor for hours and it seems it is winning. Can anyone advise or enlighten me on this matter please?

Thanks

Re: Exploded view transparency in drawing environment

kacper.suchomski — Sat, 22 Apr 2023 21:17:09 GMT

Try this::

Indicate the components (parts) in the drawing
Right click and select Select as Edges
Right click and turn off edge visibility.

Regardless of the color of the object and the display style of the model, the drawing environment always shows the edges of the model by default.

Just hide them.

P.S. You can indicate them manually and turn them off one by one.

Re: Exploded view transparency in drawing environment

SBix26 — Mon, 24 Apr 2023 19:41:19 GMT

What is happening in your image from the assembly model? It appears that most of the parts are disabled, or that you are actually editing the opaque part in the assembly context, which has the same visual effect. In either case, the assembly model shows most parts as transparent not because they are a transparent material, but because they are not fully participating in the modeling operation. There is no equivalent in a drawing view, plain and simple-- a shaded drawing view shows all edges as solid lines or, for reference parts, as phantom lines. Setting components to Transparent in a drawing view is mainly useful for materials that are transparent, so that you can see through windows, for example, in a non-shaded view.

If you are hoping for something similar to your assembly model with disabled parts, then I think you will continue to be disappointed.

Update: I just did some experimenting in Inventor 2024 (you haven't told us what version you're using), and found that the following may work for you:

In the assembly model, create a View Representation in which all of the faces of the transparent parts are set to a transparent appearance
In the drawing view, select the new View Rep as the Design View
In the drawing browser select the transparent components and choose Select as Edges; right click in the view and choose Visibility (making the edges invisible)

This is the result-- look useable for you?

Sam B

Inventor Pro 2024 | Windows 10 Home 22H2

Re: Exploded view transparency in drawing environment

imbik — Mon, 24 Apr 2023 21:23:15 GMT

OMG! that definitely has worked 🙂 The parts I wanted to make transparent were actually extruded aluminium profiles so I had edges all over it. The only thing I needed to do (addition to what you suggested) was to choose the material for the actual parts as "clear glass", then when I applied your solution the whole aluminium frame nearly disappeared in drawing.

Thanks again.

Re: Exploded view transparency in drawing environment

imbik — Mon, 24 Apr 2023 21:31:46 GMT

Hi, thanks for your suggestion. I have just applied that and got the same result as yours. By the way sorry for not mentioning about the version, I am currently using Inventor pro 2017.

Thanks for the support.