Inventor General Discussion

Inventor General Discussion

Distinguished Contributor
Posts: 164
Registered: ‎10-10-2007
Message 21 of 25 (407 Views)

Re: feature suppression in drawing views

06-24-2011 06:44 AM in reply to: elise_moss

You may also have run into another issue, a part so convoluted that it's better to remodel from scratch correctly then to continue trying to use it. Think about how long it would take you to remodel it, vs how long you've been fighting with it.

Distinguished Contributor
Posts: 361
Registered: ‎02-18-2003
Message 22 of 25 (403 Views)

Re: feature suppression in drawing views

06-24-2011 06:52 AM in reply to: donovan.cox

I agree that considering how bloated the part file is and how long it takes to rebuild after any operation, it would be better in the long run to fix the part.  I am also concerned that any cad file (step or stl) that we send out to be fabbed is going to have issues because of the extra/underconstrained/unconstrained/poorly defined geometry.  It's a garbage in - garbage out scenario. 


I'll be using this part in the future as an example of what NOT to do.  LOL



Active Contributor
Posts: 38
Registered: ‎04-01-2008
Message 23 of 25 (322 Views)

Re: feature suppression in drawing views

07-25-2012 06:35 AM in reply to: elise_moss



I realize this is a bit late for Elise, but for everybody else who tries to do this, could this reply perhaps be of help...


From Inv. 2011 you can make a multi solid part. And by changing the visability of the solids you can use the different design states.


Eg. I make one sketch which represents the crosssection of a lip seal. In this sketch you can draw the seal in a mounted state, and in an unmounted state.

Then use revolve to get the seal as part, and select only the unmounted sketch.

Then make another revolve by using the same sketch, but now use the mounted crossection, and select create new solid (under the join, cut, intersect option).

Now you can place this part in an assembly or on a drawing. And by changeing the visability of one of the solids you can use the wanted state viewing of a single part


In Inv. 2012 and 2013 you can use viewrepresentation to save the different settings / states.


When you want to view or suppres specific features, you can possible make two (or more) solids which are the same... and then supply the features to a solid which you can set the visability of when you don't want to display that features.


I hope I explained it clear enough...


Regards, Leander.

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Autodesk Inventor 2013 & 2014 Certified Professional
Active Member
Posts: 6
Registered: ‎11-16-2012
Message 24 of 25 (61 Views)

Re: feature suppression in drawing views

08-13-2014 11:15 AM in reply to: L.van.Gorsel
Thank you!
Posts: 2,219
Registered: ‎04-30-2008
Message 25 of 25 (53 Views)

Re: feature suppression in drawing views

08-13-2014 12:15 PM in reply to: jjenkins87

Or you can make the part an iPart with each member representing each stage (certain features suppressed). Earlier discussion in this thread contains some confusing information. One user claimed that Part Design View can solve the problem. That is not completely true. PDV does not deal with feature hiding or suppression. However, bodies (not features) can be hidden and its visibility can be controlled by PDV.. This workflow will work only if the delta between each stage is a separate body (hiding the additional body would help).

If the delta is features, currently iPart documentation workflow should help achieve the goal.



Johnson Shiue (
Principal SQA Engineer, Inventor
Mechanical Design
Autodesk, Inc.

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