Set part list in assembly drawings as per different "Model States" in Autodesk Inventor 2025

[dsakpal]

Hello Team,

Recently I switched to Inventor 2025 version.

Here, my existing assembly drawing is set to the 'XYZ' Model-State. Also the part list or Bill of Material which is in assembly drawing is set to the 'XYZ' Model-State.

Now, I want to change the part list to the another Model-State which namely as 'PQR'.

Please suggest how to change Model-State for part list/Bill of material.

Please refer attached image.

[CGBenner · Accepted solution]

@dsakpal 

Hello.  From what I can see the BOM will reflect whatever the current Model State is in the part or assembly file.  The Parts List on the drawing will initially reflect the Model State that you choose when you place the List into the drawing.  To change that to a different model state, I believe you must change the model state of the drawing views.  You will then be prompted asking if you would like to also change all Parts Lists on the drawing sheet.

@SBix26 @blandb @kacper.suchomski Do any of you have any thoughts, or anything to add?  Did I get this right?

[johnsonshiue · Accepted solution]

Hi! As Chris mentioned, you may edit the drawing view and select a different Model State. Or, you may use Replace Model Reference command (Manage -> Replace Model Reference) to switch to a different Model State.

Many thanks!

[dsakpal]

I have already changed the model state of Drawing Views but even though its not reflecting into part list. I have considered all views which are on the drawing sheet.

[dsakpal]

I have already changed the model state of Drawing Views but even though its not reflecting into part list. I have considered all views which are on the drawing sheet.

Again, I think, it doesn't required which model state is active in .iam file...

We could able to change the model state in .idw file just by switching the model states... but how ? Still, I'm struggling.

[johnsonshiue]

Hi! Then I need to see the files. It should just work. Please share the files in zip here or send it to me directly johnson.shiue@autodesk.com. I would like to understand the PartList behavior better.

Many thanks!

[dsakpal]

after several trials I reached to the solution...

I'm just co-relating words from @CGBenner... "the BOM will reflect whatever the current Model State is in the part or assembly file" & words from @johnsonshiue ... "use Replace Model Reference command (Manage -> Replace Model Reference) to switch to a different Model State"

So, while replacing model reference (through, Manage >  Replace Model Reference), Inventor giving you the option of changing part list according to the current model-state. So, here, user must set the expected model-state in ".iam" file & then replace the file reference in ".idw" document.

What I learn here is, If user just change the model state in drawing file by editing views, it will not reflect in part list. User must set the expected model state in ".aim" file & then need to change reference in ".idw" file (through, Manage >  Replace Model Reference); which is quite cumbersome task.

I think, Autodesk need to improvise this method in next version by just right clicking on part list & choose the expected model-state, so that, BOM/part list could change within  few seconds.

[dsakpal]

you could check attached image here...