How to convert an iam assembly to and ipt part in Inventor?

[liminma8458]

Hi,

I am doing some cable and harness project. I want to assign pins to some connectors. But these connectors are assembly models, and pins only can be assigned to ipt part. Normally I use shrinkwrap to convert iam model to ipt model. Do you have any other ways to do it?

Thanks

Limin

[kgilham]

There are 3 different ways in Inventor to create an ipt from and iam. The first one you mentioned already which is shrinkwrap. Is there some reason you are not wanting to use that workflow? The second is called Create Simplified Part in the Simplify tab. This is a part of the Revit simplification workflow so is really intended for creating a part for Revit. The third is Derive. This is in the 3D Model tab of an ipt. It has all of the options that shrinkwrap does plus the ability to manually include or exclude parts from the assembly.

Let me know if you would like to know more about any one of those three options.

[Xun.Zhang]

Hi, Have you try Derive in Create panel of a part?

[Yijiang.Cai]

Maybe you have finished creating all the connectors as assembly. If not, please create the connector as part multiple solid body, and use it in C&H as connector. When you want to create the drawing view for this connector, please use make component to generate the assembly using the multi-body first, then create drawing using generated assembly.

Hope it helpful for you!

[mcgyvr]

Any reason you don't just assign the harness pins at the ipt level of the pins used in the connector?

[liminma8458]

That is great!

I do not use Revit at all. So I will choose to use derive.

An extra question: I just go through the "derived assembly" dialog, I can not find something like "de-associate" or "break link with original assembly", so the derived part always dependent. Can we make the part independent?

Thanks

Limin

[Xun.Zhang · Accepted solution]

Yes, exactly, you can break the link with source file once the Derive feature created, please break link in context menu of this feature.

[liminma8458]

Many times, you get the original connector files from supplier or with other format. when you convert it and it is an iam file. Can you force a step file or solidwork assembly to open in Inventor as an ipt part format?

[liminma8458]

Hi, zhang, I just create a derived part from an assembly. But where is "break link" command in the part mode? I don't see it in the right click context menu

[liminma8458]

oh, great!

I see it.

Thank you so much!

[Xun.Zhang]

Hi, Just right click the feature node of Derive, there is one called 'Break Link with base component'. I paste the image in previous thread, please fresh the page to see the image.

[Yijiang.Cai]

Yes, we have.

Please new a part document, and use "Import" command to import the 3rd party dataset, which will be the multiple body.

[liminma8458]

Hi, Cai,

Your way works great! Thank you very much!