topic Re: Different Assembly Configurations for the Same Part in the Same Drawing File in Inventor Forum

Different Assembly Configurations for the Same Part in the Same Drawing File

Anonymous — Thu, 26 Jan 2017 17:34:52 GMT

Another thing that isn't intuitive or easy, what a surprise here!

I have an assembly file (.iam) that is within its drawing file (.idw) and I need to show the part in two configurations, on two separate sheets. However, every time I try to show the part in one configuration, the drawing views update to that mate configuration on the other sheet as well.

What I've Done:

1. Tried to make new views for both View and Level of Detail here:

2. While messing with the Representations, I've also tried messing with the Associative Option while in the .idw file when editing the drawing views. See what I mean here:

I was surprised (not) to find, that didn't work either! On top of that none of these options actually change anything like most common users think it would. These options, from what I can gather from other community posts, are only there to allow certain parts of the Representaions that a user creates in an assembly to be able to show in a drawing file when the user selects that particular View Representation is activated for example. The Associative Option or the Representation Options DO NOT care about mates for example. In other words, activating the 60 Degree Position Representation will not activate the 60 degree mate, even if that mate was made active in the representation, and then later suppressed in the Master View.

So, is there a normal, feasible way to accomplish this need, or, do I need to add another duplicate part (lower part is what swings out to the left and up) in to my assembly file, constrain that one how I want it and add those parts to the 60 Degree Position Representation and activate that view once it's set up correctly in the .idw file?

Re: Different Assembly Configurations for the Same Part in the Same Drawing File

Curtis_W — Thu, 26 Jan 2017 17:56:28 GMT

Hi Michael,

I think you wan to use a Positional Representation, rather than a View Representation.

And then set each view to use the different Positional Representation.

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

Re: Different Assembly Configurations for the Same Part in the Same Drawing File

MechMachineMan — Thu, 26 Jan 2017 17:56:29 GMT

Uh. You can just use position reps.

Have one position rep for your hinge being fully opened, and one for it being at 60 degrees.

On your first page, have the First position rep active, on your 2nd, have the 2nd one.

View Reps are for if the visibility of parts changes (ie; you don't want to show 1 of the 3 parts in the assembly).

View reps can be used in conjunction with Filters in PartsLists in drawings to make the BOM for that drawing appear as you want.

Level of Detail is for reducing the detail in the part document to make loading quicker, and shouldn't be used for BOM operations.

Positional reps are used for changing the position of parts in an assembly, while retaining all of the same parts.

It seems the way inventor ideally wants to work is that if you have a model that has any number of different parts used than another, it should have it's own assembly file, (and different part numbers) because it IS a different assembly.

Re: Different Assembly Configurations for the Same Part in the Same Drawing File

jtylerbc — Thu, 26 Jan 2017 17:56:37 GMT

Maybe I'm missing something in your explanation, but why are you using View Representations to try to control component positions, instead of Positional Representations?

View Representations save Visibility and Appearance (color) settings. They have nothing to do with constraints.

Level of Detail saves component Suppression status. This also affects component visibility but is primarily intended as a memory management tool to unload portions of the model you aren't working on from the computer's memory. This also has nothing to do with constraints.

Positional Representations save override or Suppression status for constraints. Your screenshots indicate that you don't have any of these created in your assembly.

Your problem isn't that the drawing views are updating to show the wrong configuration. It's that you never had two configurations in the first place. You're just changing the suppression of constraints in the Master Positional Representation (which is the only Positional Representation that exists if you haven't created any). This changes the position of your component everywhere. Anything you do with View Representations or Levels of Detail will have no affect on this situation, because these tools have no connection to constraints.

Yes, you are correct that having two copies of the part in the assembly is the only way to do this using View Representations, and that it is silly and unnecessarily difficult. That's because View Representations aren't the correct tool for this situation in the first place - Positional Representations are.

Re: Different Assembly Configurations for the Same Part in the Same Drawing File

mcgyvr — Thu, 26 Jan 2017 18:01:25 GMT

What a surprise indeed...

Re: Different Assembly Configurations for the Same Part in the Same Drawing File

Anonymous — Thu, 26 Jan 2017 18:09:43 GMT

Ok that makes sense. It looked grayed-out to me almost and doesn't have the Master or Default underneath it so I didn't consider it. Additionally, I come from SolidWorks where things are just more integrated/common sense, although it still has it's quirks from time to time.

Re: Different Assembly Configurations for the Same Part in the Same Drawing File

Anonymous — Thu, 26 Jan 2017 18:12:27 GMT

Thank you for a more detailed synopsis on the similarities and differences between the features. I knew what I was thinking about didn't seem easy or convenient at all. I just need more experience and training with this software (Inventor) because it has more nuances than other modeling software I've used in years past.

Re: Different Assembly Configurations for the Same Part in the Same Drawing File

Anonymous — Thu, 26 Jan 2017 18:17:37 GMT

As I said to the other user who has provided me with more info, thank you for this as it is helping me understand the software more. I have not had formal training with the nuances of this software and it's not as logical or common sense orientated as SolidWorks in every aspect to me at least. At least I can confirm that the way I was going to do it was in fact asinine; I knew there had to be a correct way.

Re: Different Assembly Configurations for the Same Part in the Same Drawing File

mcgyvr — Thu, 26 Jan 2017 18:34:12 GMT

@Anonymous wrote:

I have not had formal training with the nuances of this software and it's not as logical or common sense orientated as SolidWorks in every aspect to me at least.

Funny.. I said the same thing when I tried Solidworks coming from being a long time Inventor user..

Glad you got it sorted out though..

A few days training in any professional software can save hours and hours of headaches/mistakes/fumbling,etc..

They ALL have their own way of accomplishing a goal.. Usually both work well.. Just different..