Batch Part Selection

[Anonymous]

Yet another frustrating day for me in the world of autodesk after loosing my work to yet another episode of software failure during a mundane task. In the many versions of autodesk that I have worked with it blows my mind how crashes like these continue to go unresolved. Or is it just me and everybody I know? End rant.

On to my question...

Is there any way in an Inventor Presentation file to select all identical parts of an assembly other than the obvious and  grueling process of manualing selecting each part in the model navigation panel?

I am looking for a more effective way to color code for a set of assemblies that I have to produce. If the ability to use a mass selection process for individual parts exists it could save me a tremendous amount of time and energy. Alternative suggestions are welcome and encouraged. Thanks.

KevinM.

[JDMather]

Can you post a sample dataset here?

[Anonymous]

Not sure what exactly you mean by dataset but here is an example of several parts that I have manually selected in my presentation to change the material properties.

Notice they are identical parts but included in seperate assemblies. I am wondering is there is a more effiecient way to do this.

[JDMather]

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@Anonymous wrote:

Not sure what exactly you mean by dataset  .....

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Pack and go an assembly and attach it here.  I suspect there are additional problems since you are loosing work. 

[Anonymous]

Unfortunately my company contract restricts me from sharing assembly files without appropriate consent but the error happened when I was bringing a different level of detail into my presentation. It said that the presentation failed to accress the already open assembly model. Is there something else I could provide?

[Curtis_Waguespack · Accepted solution]

Hi KevinM,

I'd suggest that you create View Representations to control the colors at the assembly level. Then simply reference these when you place the assembly into the IPN file. The tricky part of this is that you can not change the explosion  to another View Representation after it's created, but if you set the view to be associative you can simply adjust your view rep in the assembly file and have it update in the IPN.

Here's an example:

In the assembly I create a new View Rep. called Green Tires

Then I set the selection filter to Part and select on of the tires

Then I right-click and choose Selection > Select All Occurences

Then I change the color of all of the tires (in the top level assembly)

When prompted I choose to Modify the View Rep (and maintain associtivity)

Then when I create a view in the IPN I select the Options button and specify the Green Tires view rep to be used in the explosion view, and I set it to be associative, so that changes to the assembly view rep are reflected in the IPN

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

[PaulMunford]

I'm not sure why you are colour coding parts inside a presentation file. Couldn't you do this inside your assembly, save it as alocked view rep and then bring the view rep into the presentation file?

[Anonymous]

Paul, looks like Curtis just beat you to the punch but thank you to you both. This is exactly what I was looking for.

I originally wanted to avoid working with material properties of individual parts in the assembly as this would affect all other assemblies linked to these parts but it sounds like the view representation keeps this from happening.

[PaulMunford]

Ha! And a far more comprehensive answer too - nice one Curtis 😉

Kevin - View reps only change the part's colour, not material, so you shouldn't have any problem here.

Happy cadding!

[pdhn8580]

So I do the design view representations in the assembly as described here, then I make the .ipn file and select the view rep and mark it as associative so that i can change the view in the assembly to update it.

Weeks or days later I may go to open up that .ipn and notice that my view representation in the .ipn no longer looks like the view in the .iam anymore even though it is associative. If i go to turn off visibility of items I don't want shown i get the message box that asks: "Unassociate design view representation?". How can i get the view representation back in sync? I dont want to unassociate, but i want the view to be the same as the assembly view.

Thanks,