Phantom parts in a drawing

[Anonymous]

Hello,

I am trying to figure out how to show only a single part, in one view, as a phantom wireframe in an .idw and have the rest of the parts shaded.  I can't seem to find any method of doing this without causing the other views to do the same thing.

Is this possible to do?

[Curtis_W]

Hi jbupp,

What version of Inventor do you have?

Inventor 2016 and 2017 have the ability to have transparent parts in a drawing view:

http://www.inventortales.com/2015/04/transparent-parts-in-autodesk-inventor.html

But there is also this method (see tip #1):

http://inventortrenches.blogspot.com/2011/06/autodesk-inventor-tips-from-around-web.html

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[Anonymous]

I'm currently on Inventor 2015 so I don't have that option in the popup menu when selecting the part.

I did find the second option online, but the "As Material" button in the view menu was removed, I believe they did this when they switched to a separate appearance library.

So unfortunately neither of those options work for me at this time.

[Curtis_W]

Hi jbupp,

I messed around with this a bit, and could not get it to work in 2015 either. I might have overlooked a setting in the appearance style, but I suspect that the setting put in 2016 was put in to address this issue, and that there is not a solution in 2015.

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[Curtis_W]

@Anonymous,

Wait wait wait!

I just remembered another way to do this using positional representations and overlay views.

• Create one new Positional Representation ( no need to do anything else with it, other than creating it).
• Create 2 View Representations
• In View Representation 1, turn off the visibility of the part you want to show wireframe
• In View Representation 2, turn off the visibility of everything else
• Create a drawing Base View and set it to use View Representation 2
• Create an Overlay View, and set it to use the Positional Representation and View Representation 1
• In the Overlay View dialog box set the style to be not shaded & hidden lines removed
• And also in the Overlay View dialog box set the Layer dropdown to be 'As Parts'.

Note you can right click on the Overlay View in the browser and edit it, if you missed something when creating it.

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[brad · Accepted solution]

Jbupp,

1. Start a new part file

2. Derive the part you want to show as phantom  (you could also just copy the original file, but deriving will keep them both always the same)

3. Save

4. Place this "phantom" part in your assembly 

5. Right click on the "phantom" part: BOM structure: Reference

6. Either manually in the IDW or using view reps in the .iam. :  hide the "phantom" part in the other views, and hide the original part in your "phantom view".