"Make Part" and "Make Components" buttons becoming grayed out on complicated multi body parts — cannot turn them into assembly.

[mailswamp]

I designed a large multi-body part, in which three parts are a table-driven version of one of the bodies. I am trying to turn this multi-body part into an assembly, so I can use all three instances of this one table-driven body with one changing variable (jaw), animate it in 3D.

This part is a 3D printed educational model for children to play with.

Unfortunately, the "Make Part" and "Make Components" buttons do not work.

For some reason, "the edit factory scope" is highlighted yet neither of the two options that it offers open a menu that would allow me to turn this multi-body part into an assembly.

I used Inventor 2024 instead of Inventor 2022 to open the files and experienced a similar problem.
Yet when I designed a simple test part by extruding two boxes from the same sketch that were not connected, the problem of extracting one of those boxes as a separate part from the simple 'multi-body part' was not a problem.

Why is this happening?

Thank you for reading my question.

[JoshuaNAM]

Hi,

I have worked for companies that have exceeded the multibody workflow by far. They had many thousands of parts that needed to be generated from a multibody design. I found it to be a very complicated and time consuming process to make changes to the design. But nevertheless they were able to export it to parts and assemblies. Your explanation sounds quite complex. Have you tried some test files including table driven options as you describe but then for a much smaller multibody design? Perhaps what you are trying to do isn't possible? Or have you done it before with success?

Kind regards,

Joshua

[johnsonshiue]

Hi! I suspect you have converted the part to an iPart. In an iPart factory, Make Part and Make Components are disabled.

You may want to use Model States instead. Make Part and Make Components should be allowed.

Many thanks!

[mailswamp]

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@johnsonshiue wrote:

Hi! I suspect you have converted the part to an iPart. In an iPart factory, Make Part and Make Components are disabled.

You may want to use Model States instead. Make Part and Make Components should be allowed.

Many thanks!

---

I think that you are right about iPart Factory.

Thank you.

I did convert it into i Part. I deleted the i Part table variations and Make Part and Make Component reappeared.
There was a part that was controlled by the table with 3 different values for one of the dimensions.
Is it possible to make a part that has more than one variation without using i Parts?
Where would I enter a list of different values for the changing dimension?

How would I add a dimension to this Excel spreadsheet?
If so, this almost doubles the function of i Part, yet it offers no way to edit the variables from within Inventor.

[johnsonshiue]

Hi! You may want to look at Model States. The workflow is similar to iPart/iAssembly but with fewer limitations and all the members are saved in the same iam/ipt file (factory).

And Make Part and Make Components are allowed.

Many thanks!

[mailswamp]

I found many tutorials on I parts and I part factory, yet I found no model states tutorials other than on how to create new "model states" in the menu, with no explanation of how to save differences between models into them.

I do not see any way I can make model states different from one another.

Why hasn't in been combined with the ipart functionality?

[johnsonshiue]

Hi! You will need to enable the "Member Edit Scope" (one pencil, not all pencils). When "Member Edit Scope" is enabled, any design change (parameters and properties) will be captured on the Model State table. Please share an example that you are having some trouble with.

Many thanks!

[mailswamp]

Thank you.
I like how model states open an excel spread sheet with a changing dimension instead of some clumsy Inventor table.
Is there a convenient way to export all three model states of the jaw part at once?
Or do I have to load each state individually and click "make part" and save it as a new file every time?

[johnsonshiue]

Hi! No, unfortunately there is no out-of-the-box solution to do that. You may write an iLogic rule to automate the process.

Many thanks!

[mailswamp]

Is there an example code that I can use to create such an iLogic rule?

Otherwise, I can do everything by hand. I am just curious.

It would be easier for me to write code if I saw a similar code that is known to work.

How are the names of model states to be written in the code?

I put " ' " to comment out code and commented code still gives me errors. Why?

If Component.ActiveModelState("ThisDoc.ActiveModelState = ThisServer.LanguageTools.CurrentPrimaryModelStateString") Then
Component.Replace("' ThisDoc.ActiveModelState = "Jaw 02", "OtherAssembly.iam<Model State1>", True)
'Component.Replace("SubAssembly:1", "OtherAssembly.iam<Model State1>", True)
End If

 

[mailswamp]

I want to explore the functionality of Inventor with this 3D printable 3 jaw chuck.
I want to make a tutorial about this model myself and start a challenge for the users of all 3D CAD modeling software to design a similar model and to show the process.