iParts in assemblies and drawings

[Anonymous]

The attached sketch shows how I originally decided to use iParts in drawings and assemblies.  In assemblies I use the generated iPart, and in drawings I use the "master" iPart file.  I did that because I wanted to keep the drawing linked to the "master" part, to avoid the situation where the drawing would be out of date because I forgot to regenerate the iParts.

The problem is that I don't know how to force the drawing to refer to the correct version of the iPart.  To use the terminology in my sketch, I open X2.idw and get a drawing of X1.ipt, not X2.ipt.  Am I going about this wrong?  Should I use the generated iPart in my drawings?  And, if so, is there a way I can automatically regenerate.  I'm prone to forgetting key steps like that.

[Cadmanto · Accepted solution]

If you RC on the view and select "Edit View" under the "Model State" tab you will see your list of iparts.

If this solved your issue please mark this posting "Accept as Solution".

Or if you like something that was said and it was helpful, Kudos are appreciated. Thanks!!!! 

     

[Curtis_Waguespack · Accepted solution]

Hi tmchenry,

If I understand correctly, what you want to do is edit your drawing view and go to the Model State tab, and use the IPart Member area to select a specific iPart member, rather than just leaving it to use the Active Factory Member option.

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

[Anonymous]

Thanks, guys, that helps a lot.  I have the feeling I once knew that, but since I don't do it very often I had forgotten.

Regarding assemblies, am I correct that the best way is to use the generated iPart, as shown in my sketch (first post)?  Or is there a way to "lock in" the model state in an assembly, too?

I have to admit, I've never really understood why there are generated iParts.  I come from a SolidWorks background and the paradigm there is a bit different.  You create "configurations," but they're always part of the one file.  There are no generated files.  I'm still trying to understand the Inventor paradigm.

[Cadmanto]

No problem.  Glad to help.  Unfortunately generating the files is the only way to go with Inventor ipart/iassemblies.

I came from Solidworks myself (12 years of it) so I know exactly what you are talking about.   That is why if you go to the Inventor IdeaStation a lot of the ideas I have posted are things I used to be able to do in SW.

Including this idea that pertains to removing the need to generate these factory files.

If this solved your issue please mark this posting "Accept as Solution".

Or if you like something that was said and it was helpful, Kudos are appreciated. Thanks!!!! 

     

[Curtis_Waguespack]

Hi tmchenry,

When you attempt to place an iPart factory (parent) file in an assembly, Inventor will actually place the iPart member (child) file based on the choices you make when you place the file. If the file hasn't been generated manually, then this happens automatically at this time. So, it doesn't really matter if you browse for the factory file or the member file when you place it in the assembly, the result will be the same: you will place the iPart member in the assembly.

In fact you can't actually end up with the factory in an assembly, unless you trick Inventor into doing so, by first placing the part file, and then converting it into an iPart factory. This is not the intended use of iParts, but there are some unique workflows where this trick works well.

So it sounds like you're using iParts correct based on what you described.

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

[Cadmanto]

Curtis,

I know you have to be careful with your second point in creating the factory after the file has been inserted, because you end up having to replace the file in the assembly with the updated factory file in order to see all of the iparts created in the factory file table.

If this solved your issue please mark this posting "Accept as Solution".

Or if you like something that was said and it was helpful, Kudos are appreciated. Thanks!!!! 

     

[Curtis_Waguespack]

Hi Cadmanto,

Correct, and there are some other issues that arise as well. Therefore, Autodesk does not recommend/support that workflow. But there are some times when "bending the spoon" in this respect and converting to an iPart after placing it in an assembly is helpful.

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