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Drawing View "Associative" Selection

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Message 1 of 11
Cadmanto
6198 Views, 10 Replies

Drawing View "Associative" Selection

In the continuing persuit to learn Inventor, can some one please explain the purpose and usefulness

of this selection in the drawing view editor?

Associative.JPG

 

I have noticed one thing.  When it is checked it turns off the visibility of parts within an assembly view.

Just looking to learn more about this command.

Best Regards,
Scott McFadden
(Colossians 3:23-25)


10 REPLIES 10
Message 2 of 11
Ray_Feiler
in reply to: Cadmanto

That links the visibility back to the IAM's design view parts visibility when it is checked. If a parts visibility is off in the design view used during the placement of the view it will be off in that view.


Product Design & Manufacturing Collection 2024
Sometimes you just need a good old reboot.
Message 3 of 11
Cadmanto
in reply to: Ray_Feiler

Is that the only thing it affects is the ability to turn the visibility on/off of parts in assembly drawings?

This is how I stumbled on it was because I could not toggle the visibility of certain parts in the assembly drawing, but I posed this question wondering if there were other things affected by this selection.

Best Regards,
Scott McFadden
(Colossians 3:23-25)


Message 4 of 11
Ray_Feiler
in reply to: Cadmanto

You are right. With it checked you can not turn off the visibility of parts in the drawing because it is associated with the assembly. When you unchecked it you can turn off the visibility of parts in the drawing independent of the assembly.


Product Design & Manufacturing Collection 2024
Sometimes you just need a good old reboot.
Message 5 of 11
Cadmanto
in reply to: Ray_Feiler

And that is all it does.  In my opinion they should have named it something different that made it sound like it

was associated with the visibility.  Based on the name "Associative" I would have bet that it did more then that.

Best Regards,
Scott McFadden
(Colossians 3:23-25)


Message 6 of 11
Ray_Feiler
in reply to: Cadmanto

As far as I know that is all it does. I'm sure if I'm wrong someone will correct me though. Smiley Happy


Product Design & Manufacturing Collection 2024
Sometimes you just need a good old reboot.
Message 7 of 11
SBix26
in reply to: Cadmanto

This means that the view is controlled by the assembly's view representation.  In any assembly where I have parts that I don't want to show in the drawing, or don't want to show in one particular view, I'll make a view rep in the assembly for that purpose.  The associated view rep can be changed in the Edit View box any time you want-- for instance, right after you've realized the need for one and created it.

Message 8 of 11
jtylerbc
in reply to: Cadmanto


@Cadmanto wrote:

And that is all it does.  In my opinion they should have named it something different that made it sound like it

was associated with the visibility.  Based on the name "Associative" I would have bet that it did more then that.


It associates the drawing view with a particular View Representation in the assembly.  The name is based on the fact that it is part of the View Representation selection.  If "Associative" is turned off, you can turn component visibility off in the drawing view, as you stated.  However, it will ignore any visibility changes you make in the assembly.

 

If it is checked on, you can't make manual visibility changes in the drawing view, but that drawing view will obey the visibility settings in your View Representation.

 

Basically, you're telling the system whether you want to control visibility from the drawing or the assembly.  Associative is particularly useful when you're going to be turning the same components on and off in several views - you can set it up ONCE in a view rep in the assembly, then just set that rep active in the drawing views.

 

Turning associative OFF is useful for that one oddball view where you need to turn a specific part off or on.

Message 9 of 11
Cadmanto
in reply to: SBix26

Thanks Sam.

I appreciate the explanation.

 

 

Best Regards,
Scott McFadden
(Colossians 3:23-25)


Message 10 of 11
Cadmanto
in reply to: jtylerbc

That is a great explanation and what I was looking for.  Thank you for outlining that out.  Nice job.

What you said makes total sense.  I can see that point now.  Prior to what you posted I was really wondering what the point was for this added feature.

 

I can see based on how you said it where this would be needed.  I have already run into this situation in my short dealings with Inventor.

Best Regards,
Scott McFadden
(Colossians 3:23-25)


Message 11 of 11
jtylerbc
in reply to: Cadmanto

You're welcome, glad that helped.

 

Personally, my preference is to favor the Associative views and control the visibility from the assembly.  It cuts out a ton of going around to views suppressing the same things over and over.  I then turn the associativity off only if I have some strange exception I need to deal with - sometimes there's just that one part that's in the way.

 

If you're using shaded views on the drawing, it also works for view reps with color overrides.  Even if I'm not having to hide anything, I almost always have two view reps - one with the "real world" color for use in realistic-appearing higher level assemblies, and one with the components color-coded for identification.  Having the drawing views set to Associative allows it to pick up color changes as well as the visibility changes.

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