Inventor General Discussion

Inventor General Discussion

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Valued Contributor
tmchenry
Posts: 73
Registered: ‎02-14-2011
Message 1 of 7 (416 Views)
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Representations

416 Views, 6 Replies
11-07-2012 01:55 PM

I'm a long-time 3D CAD user, but a relative newcomer to Inventor.  I can't seem to come to grips with Representations.  Specifically, I don't understand why there are three different kinds of representations, what differs between them, and how best to use each one.  Can anyone point to an article or book somewhere that might help me out?

 

On a related note, one of the problems I've found with most Inventor documentation is that it seems to have two premises that don't fit my situation.  All the Inventor documentation I've seen seems to assume that the reader knows something about AutoCAD but nothing about 3D CAD.  That's probably true of many new Inventor users, but I'm the opposite:  I know a fair bit about 3D CAD and have used many different 3D CAD tools, but I know next to nothing about AutoCAD.  Can anybody recommend any material for someone in my situation?

*Expert Elite*
jtylerbc
Posts: 877
Registered: ‎09-01-2010
Message 2 of 7 (408 Views)

Re: Representations

11-07-2012 02:40 PM in reply to: tmchenry

Here's a bit of an introduction:

 

View Representations save sets of Visibility settings and color overrides.  If, for example, you needed to be able to see an enclosed box with the lid removed, you could use a View Rep called "Lid Removed", and turn visibilty off on the lid.  You can also use it to save color overrides in the assembly.  An example I use often is to have a representation where the parts are overridden to various colors to make the parts more distinguishable, and another one where it is more realistically colored.

 

Level of Detail representations save sets of Suppression settings.  The difference between Suppression and Visibility confuses a lot of new users, because they both render the part invisible.  However, Suppression also unloads it from the computer's memory.  It is intended more as a memory management tool for working in large assemblies.  Don't make the common mistake of using it when all you really need is to control visibility of parts - that's not what it's for, and it will cause you grief if you try to use it that way.

 

Positional Representations can suppress or enable different combinations of constraints, to show an assembly in different physical positions.  If a constraint has an offset value, PosReps can also be used to override that value.  For example, if you have a hydraulic cylinder, you could have a PosRep for the cylinder fully retracted, fully extended, and at specific points in the stroke.  Or reusing the example of the box, you could represent the lid being open, instead of just disappearing.

 

Hopefully that helps.  Some searching on this board would also probably turn up some more detailed explanations of the differences specifically between Views and LOD's - it's a common question that confuses new users, and I know I've written about it a few times myself.

John Tyler
Inventor 2015
Windows 7 64 Bit
Valued Contributor
tmchenry
Posts: 73
Registered: ‎02-14-2011
Message 3 of 7 (402 Views)

Re: Representations

11-07-2012 03:45 PM in reply to: jtylerbc

Thanks, that is a big help.

 

When I wrote the post I was in the middle of creating two versions of an assembly, one with some parts suppressed.  It did seem that Level of Detail was the right kind of representation for that, but I had encountered some weird behaviour that was causing me to have doubts.  It appears that the weird behaviour had to do with the need to save the changes to each representation before they "take;" in other words, it seems that if you suppress a part, and then change representations before saving, that act of supression is lost.

Valued Contributor
tmchenry
Posts: 73
Registered: ‎02-14-2011
Message 4 of 7 (278 Views)

Re: Representations

03-07-2013 04:18 PM in reply to: jtylerbc

I'm hoping someone can help me with a related issue -- something I've been trying to figure out how to do properly in Inventor since I started using it, without success.  Perhaps an example will explain it best.

 

At the moment, I'm working on a latch assembly.  The latch assembly includes a barrel lock with a cam, which is a separate sub-assembly.  What I would like to do is have two versions of the barrel lock, Locked and Unlocked, with the barrel rotated to the appropriate position in each version.  Then I want to have the latch assembly (the higher-level assembly) to also have two versions, Locked and Unlocked, which would each use the appropriate version of the barrel lock sub-assembly.

 

I thought I could do this by making two Positional Representations of the barrol lock, and then specify which one I wanted to use in the higher-level assembly.  But it's not possible to select a Positonal Representation in a higher-level assembly.  The menu choice is greyed out.  So that's obviously not how Positional Assemblies were intended to be used.

 

However, from the explanation above it doesn't appear that either View Representations or Level Of Detail representations are an appropriate way to do this, either.  Is this not an appropriate use of Representations?  Should I be using a different approach, such as iAssemblies or a parameter-driven approach?

Valued Contributor
tmchenry
Posts: 73
Registered: ‎02-14-2011
Message 5 of 7 (277 Views)

Re: Representations

03-07-2013 04:27 PM in reply to: tmchenry

Never mind.  (Emily Litella moment.)

 

I'm not sure how I got the idea that the Positional Representation menu choice was greyed out.  It's not now.  So it appears that my instinct about how to do this was right.  Wierd that I had a greyed-out menu before, though.  Perhaps the sub-assemblly has to be set to Flexible?

Valued Contributor
tmchenry
Posts: 73
Registered: ‎02-14-2011
Message 6 of 7 (215 Views)

Re: Representations

05-03-2013 11:27 AM in reply to: tmchenry

Okay, I'm back to being confused again.  I tried the exact same thing on a new assembly (two postional representations in the sub-assembly, referred to by two postional representations in the higher-level assembly);postional representations are greyed out in the higher-level assembly.  I have no idea why.

 

Can someone direct me to some documentation that explains how postional representations work, and how we're meant to use them?  The "how to" help that comes with Inventor isn't helping, because it's telling me to make a menu selection from a greyed-out menu.

*Expert Elite*
blair
Posts: 4,076
Registered: ‎11-13-2006
Message 7 of 7 (211 Views)

Re: Representations

05-03-2013 11:42 AM in reply to: tmchenry

LOD's are a memory tool to unload part of the assembly from memory. Look at the Documents Open in the lower RH corner of the screen. If you suppress or turn visibility off, the item/document is still loaded when you open the IAM.

 

If you create a new LOD and suppress a number of items, you will notice that the Open Documents is reduced. The main goal of LOD's is to reduce the memory foot-print on your IAM when it loads.

 

The easiest is to a new Positional View (RMB on the Position) such as Open or Unlocked, then suppress the constraints and create new constraints to reposition your model or suppress items to allow you to select these views in the IDW. Either Overlays or views with items suppress such a a plumbing view with only the Tube and Pipe items showing.

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