Model states

[cfairfowl]

When you derive an *.ipt file (for example master geometry) the Model States in that geometry file is not available in the current part. Is there a good reason for this?. I want to use different parameters for the part using model states because I can't change the part within the part file, I need to change it's shape (a bend) using different values in the master geometry's parameters. This is because I haven't figured out how to bend a curved plate using the bend tool. It doesn't seam to work if

 

I try bending the curved plate around the Y axis if it is already formed (curved/bent) around the Z axis. Any ideas?

[BDCollett]

It will not work with model states. Is there a reason you need it to use the different model states?

[SBix26]

Attach your part file and tell us what version of Inventor you're using.

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Sam B

Inventor Pro 2025.2 | Windows 11 Home 23H2

[James_Willo · Accepted solution]

Hi, it doesn't work because that's not how model states work. Model states can only control the current document (or link to one below in the case of assembly).

Model states in the derived document control features and values in the derived document. The geometry you are seeing is derived geometry and so has no history or parameters, it is just an associative blob. Therefore you can only suppress features added afterwards or parameters that concern those new features with Model States. 

You need to edit the derive feature and change the model state in there to change it. 

[cfairfowl]

Hi, and thanks for the reply. Yes, I guessed this is the case the derived *.ipt is Higher Archy.

This means though, I have to copy the *.ipt file with the geometry in it, re-name it then in that copied file create my solids. If the master geometry changes I have two files to edit.

Thank for the reply.

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[James_Willo]

Not really, as long as you don't break the link in the derived file, the geometry will always update to match the master (original document). 

[cfairfowl]

Hi,
I have a curved plate (rolled steel - like part of a pipe with a 10 degree arc), this is then bent, the radius of the curve is constant but the bend varies using different displacements in the parameters with different model states.
The curved plate/section is made from a sketch in the X Y plane, The bent plate is formed using a sweep along a sweep line in a sketch drawn in the X Z plane.
By changing the displacement value at the top of the plate - the opposite side of a triangle and (not the bend angle) in the parameters, changes the amount bend (and displacement) in the plate.
By assigning a different displacement value (in mm) to a different Model State, allows me the change the displacement (and bend angle) simply by changing the Model State.
The reason I used the sweep is because Inventor (2024 - and previous releases) wouldn't bend a curved plate - or at least not for me...
Cheers.
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[James_Willo]

Maybe this is another issue not detailed here. Are you wanting to be able to display all model states by changing the model in the derived file?

You will need to create a new part for each model state and select the correct model state for each when you do the derive. 

[cfairfowl]

I have copied the geometry file and produced the strut feature in that file, this allows different model states to be selected in that part and in any assembly it is in but it means having two files with the same geometry in them.

Cheers

[andrewiv]

I'm guessing you have this set up as a sheet metal part and are using the fold command?  Have you tried using the bend part command instead?  I can bend a piece in two directions using this method and use model states to show it in different stages.  I have attached a file using 2024.

[kacper.suchomski]

It is possible to model a double-bent sheet metal part.

1. Create model with target geometry
    
2. Parameterize the model (depending on your expectations, these may be specific variables or mathematical equations)
3. Create variants using Model States or the iLogic configurator

[kacper.suchomski]

Here's another example.

The first 3 minutes show working with sheet metal; then adapting to production methods.

https://youtu.be/8KxzbaklktM?feature=shared

[James_Willo]

Yes, this is correct, the MS file is the master geometry and then you can insert the derived files into an assembly. 
Unfortunately, part files don't support substitutes so you can't use the more desired workflow.