Model States, BOM and Phantom Sub-Assemblies

[dlongley]

Sorry for wordiness of this question, but background is needed.

I have an Inventor 2024 main assembly (a crane) which contains at least two subassemblies:

- Mounting Kit, and

- Platform Kit.

The Mounting Kit contains just parts, including content centre fasteners.

The Platform Kit contains subassemblies as well as parts (fasteners).  Some of these subassemblies have further subassemblies, etc.

Now in the main assembly there are model states, to reflect different stages of installations (such as driveline mods, platform installation, etc) and various parts and assemblies at the top level are set to BOM Structure "Reference" or suppressed as required.  

However, our two Kit subassemblies are both set to Phantom, so that their child parts/subassemblies show up at the top level, and can be detailed in position on drawing views for particular model states.

Now the PROBLEM...

When I have a Parts List on drawing for Primary model state, using Parts Only BOM, it behaves as expected, all child components down to the lowest level show up as parts.  Useful for letting fabricators know exactly how many of each individual part to make.

But when I use the Model State (say Platform Install) for these Parts Only parts lists, the children of Mounting Kit show up OK - all good.  But the Platform Kit only shows it's subassemblies and any parts at it's "top" level.  It is not exploding through all the levels of all the nested subassemblies to the individual parts, just stopping at the first subassembly.

WHY?  Yet when I RMB on the Parts List to go to the BOM, and look at the Parts Only tab, it all shows exploded through to the individual parts.

It seems to be something to do with the Model State.

If I change the Default BOM of the Platform Kit to Normal, it then shows up in the Parts Only Parts List, not it's subassemblies!  Primary model state still behaves correctly.

So, what am I doing wrong?  I have not seen this behaviour in any previous versions (been using Inventor since second release, so definitely not a newbie), only noticed with this assembly and use of  Model States.

And don't get me started on the lack of BOM structure possibilities and Item numbering within Model States (Autodesk, please take note, lots of people are asking/begging for it to be fixed!)

Over to you all.  As always, thank you kindly in advance for any help you can provide.

Derek

[kacper.suchomski]

Hi

Open the BOM, right click on the Structural tab, Properties and check if it is set to display one or all levels.

[dlongley]

Thanks for the prompt reply.  Problem is not with the Structured BOM, but the Parts Only BOM when used in Parts List on a Drawing.  When displaying the Parts Only BOM for the particular Model State (either from the Assembly or Drawing), it appears correctly, with all subassemblies being "exploded" down to part levels.  But the Parts List using the Parts Only BOM stops at the first level.

I did as you suggested anyway, no change to Parts List behaviour. 

[kacper.suchomski]

Take a screenshot of the parts list and the parts list edit window.

[dlongley]

Here's an excerpt from the Parts Only parts list from the drawing.  The components with Drawing Ref (first column) ending in 23.1 to 31.1 are all subassemblies of the Platform Kit assembly.

Here's the Parts List Edit window:

Here's screenshot from the Parts Only BOM from the model.  You can see lines with DRAWING REF ending with 28.2 down to 44.2 (there's more, just not in the screenshot) are some of the parts that make up the various subassemblies of the Beam Weldments, Platform Assemblies, etc.

Hope that helps.

[kacper.suchomski]

What happens if you create a list of the structural parts of all levels?

[dlongley]

OK, big progress when trying to get some answers for Kacper.

You know how once you have a parts list of a model in the drawing file (say Structured) you cannot create one using Parts Only?  The workaround is to create the Parts Only parts list in separate file, then paste it into the original file.

Well what I have just tried to do is as follows:

Using model state Primary, create Structured parts list - OK.

Using model state Primary, attempt to create Parts Only parts list, but BOM type is greyed out on Structured because already have that BOM in a parts list.

Deleted all parts lists, the tried those same steps, but with another Model State "Platform Install".

In all these instances, the subassembly that was causing the problems, Platform Kit was set to BOM Structure Normal.

Created the Structured parts list first.

Then when go through same steps, it allows me to select Parts Only for the BOM View (not greyed out), even though we already have a Structured parts list on the drawing.

But then the resulting parts list is EXACTLY the same. i.e. even though it looked like I was selecting the Parts Only BOM View, it still gave me the Structured view because that had already been created.

I tried the same again, but this time chose Parts Only first.  And sure enough, the second one was also Parts Only, even though it allowed me to select Structured in the dialog box.

Tried again, but this time I first placed a Structured parts list using Primary model state on the page first.  Then tried steps again with Platform Install model state.  This time, it would only allow Structured BOM View (greyed out).

Once a parts list has been created, you cannot tell whether it is Structured or Parts Only except for looking at the data generated.  Hence why I thought that parts list was acting up.  

So the problem is not the parts list per se, but the fact that it lets me think that I can create both Structured and Parts Only parts lists on the same drawing file using any model state other than Primary, as long as here is no parts list using the Primary model state.

So, that sounds like an Autodesk problem.  Autodesk, over to you!

Derek

Rep

[johnsonshiue]

Hi Derek,

I vaguely remember seeing a similar issue. This could be a limitation or a bug in Model States. If possible, please share the files in zip with me directly ([email protected]). I would like to understand the behavior better.

Many thanks!

[dlongley]

Hi Johnson,

I've simplified the assembly to make it smaller, and behaviour exists.  It seems to depend on how the Parts List is defined.  If the Parts List is defined by selecting the view, then it will only let you use the Structured or Parts Only BOM View, and it is greyed out when attempting to create parts list using the other.

If you create a parts list by specifying the file (say from the drop down box on dialog), and it is a model state other than Primary, then it will allow you to create both parts lists.  However, the second one will use the same BOM view as the first one, even though you specified the other BOM View.  So for example, if I create a Parts List for Model State 1, by selecting the file from the drop down box (because I've got the assembly open in the background), and select Structured BOM view, i get that parts list OK.  But if I attempt the same thing again, it allows me to select Parts Only BOM View, but I still get the Structured BOM View.

In my files attached, I have 2 model states (1 & 2).  For Model State 1, I created two parts lists like above steps.  I then did the same for Model State 2, but selected Parts Only BOM View first.  So the second Parts List for Model State 2, which is supposed to be a Structured BOM View is actually Parts Only, since there is already one on the page.  

Once a parts list has been created for the Primary model state, then you cannot attempt to create both types of parts lists, it won't let you by greying out the BOM View in the dialog.  

Result:

So in summary, the fault appears to only to be valid if a parts list is created by selecting a file using the drop down box on dialog, AND it is NOT Primary Model State AND Primary Model State is NOT already being used in a parts list (either explicitly or because there are item balloons on a view).  

If it allows me to select a both BOM Views, then it should display the correct BOM View.

If the view is selected instead, behaviour is not evident.

Once a Parts List has been created, it doesn't look like we can see which BOM View it is using, except by looking at the data.  I can assure you that I made the Parts Lists shown on the drawing, multiple times, using the steps above.

The ZIP file for the drawing and model is over 470MB in size.  How do you want me to send that to you?

Thanks,

Derek

[johnsonshiue]

Hi Derek,

Many thanks for sharing the detail! Please share the files on a cloud drive of your choice and grant me the access ([email protected]). I would like to understand the PartsList issue better.

Thanks again!

[dlongley]

Hi Johnson,

Lookout for an invitation from a Onedrive location, there is a ZIP file there for you to investigate.  Main assembly and drawing file have same name as the ZIP file.

Thanks for any help,

Derek

[johnsonshiue]

Hi Derek,

Unfortunately, I have not received any One Drive invite from you. If possible, please resend it to [email protected].

Many thanks!

[tims79]

I have also noticed some buggy behavior regarding sub assemblies, parts lists, and phantom vs normal sub assemblies in IV2025.  I have an idw of one main assembly with a couple of sub assemblies.  Both sub assemblies are set to be phantom in the document settings.  But in the idw part list, only one of the two behaves correctly (shows all the individual parts instead of just the top level subassembly).  In fact, the first subassembly isn't showing up at all in the part list - not even the top level of the subassembly.

I found that if I started a brand new idw, and place a view of the same exact main assembly, then place a part list, suddenly both phantom subassemblies behaved correctly on this new idw.  So it seems to be something wrong with that particular idw file.

[johnsonshiue · Accepted solution]

Hi Folks,

Derek did send me the files to review. Without disclosing the detail, here is what I can share. The PartsList behavior is a limitation unfortunately. Before Inventor 2022 (no Model States), Inventor assembly can only have one BOM. And, once a PartsList is placed in a drawing, the BOM structure will be fixed within the drawing (across multiple sheets). Essentially, Model States inherits the same behavior. Allowing the user to choose BOM structure after a PartsList is placed is actually a bug. This behavior is meant to ensure the item numbers are consistent since the item numbers are BOM structure specific. If two set of item numbers are presented, the ballooning would be very confusing.

However, there is a back door access to allow two BOM structures of the same assembly (or Model State) to present in the same drawing. Basically, you need to create the other BOM structure PartLists in a new drawing. Then copy the sheet and paste it to the old drawing. Though this back door access seems to work, it is not thoroughly tested. There could be potential problems. You want to experiment it before you leverage the technique.

Many thanks!