Reference Parts in a Drawing are shown as Transparent

[cwilliamson232RQ]

I want the Reference Parts in my drawing to show up normal. Not as Transparent. This top picture are the components that i have selected to be REFERENCE and it shows them as transparent in my drawing. I dont want them to be transparent but still want them to be Reference so they do not show up in my BOM.

[mcgyvr]

Edit the base view and in that dialog go to the Model state tab and change reference line style to "as parts" and any other changes as necessary in that section..

Edit: Sorry.. I misread your post initially..

Reference data will always show like that in iso views.. There is no setting to change that sadly..

Vote here to show your support for fixing that..

https://forums.autodesk.com/t5/inventor-ideas/reference-parts-and-shaded-drawing-views/idi-p/5613392

[cwilliamson232RQ]

I have done that already and it is still transparent......

[cwilliamson232RQ]

What! That is terrible! 

[Jon.Dean]

Hi @cwilliamson232RQ,

I don't see an issue viewing the parts correctly in the drawing views.

Check out my screencast. 

Cheers

Jon.

[Mark.Lancaster]

@Jon.Dean 

OP is talking about ISO views on their drawings.

You are only showing it as a normal views...

[cwilliamson232RQ]

Thanks for screencast but i am having the problems in my ISO Views. Try it again and see if you get the same issues. 

[brad]

My workaround for this is to simply not make them "reference" parts.

Instead, I tag those parts as "Phantom" in each part file's document setting.

This keeps them out of the Parts List, yet lets them display normally.

If that "phantom" part is used elsewhere in an actual Parts List, I'll use a copy or derived version of that part and add "phantom" to the filename.  It's not ideal since it's an extra file to deal with, but it allows me full control over the Parts List and the ISO views. 

[cwilliamson232RQ]

That is a good idea. 

What about if you have the same part and just have 2 Levels of Details. One called Phantom and One called Default? 

Can you toggle it this way in your Assemblies? 

[johnsonshiue]

Hi! This is a known limitation at the moment. We have heard this request before (see the idea below). It has been marked as Accepted, which means it is in a queue to be implemented.

https://forums.autodesk.com/t5/inventor-ideas/reference-parts-and-shaded-drawing-views/idi-p/5613392

Many thanks!

[Subtel · Accepted solution]

HI All,

You need set "Display Style" to "Edges as Part, Shaded" and all will work fine 😉