How do I make parts list show all parts in a drawing?

[sschulteH6WZ3]

Hi all, I am trying to make a parts list that will show all the parts in an assembly drawing that is generated from a assembly that consist of two weldments. The weldments have many parts with many shared. It was modeled by some one who recently quit. All inventor will show is just the two weldments and not all the parts inside of them. As soon as I select the view the ability to select levels grays out and reverts to first level. Any one have a idea or is this not available in Inventor? 

[MechMachineMan · Accepted solution]

1. Go into the Bill of Materials and ENABLE the Structured BOM view.

2. Go into the View Properties and Select all levels.

3. In a drawing that has no other PartsLists placed (new idw file), place the all levels structured BOM.

4. Edit the PartsList and click the arrows to expand the rows.

4a. If it still does not show the sub levels, go into the sub-assemblies and ensure the BOM Structure is NOT set to Inseparable or Reference.

Good luck.

[mcgyvr]

Don't forget...stand on one leg, hold your left ear and pat your tummy with your right arm while you are doing that..

[jtylerbc]

If these are modeled as Weldments, the problem is most likely that they are set as Inseparable in the BOM.  This happens by default when Weldments are created, so if that isn't what you want, you will need to change that setting.

The "Inseparable" BOM Structure setting causes the weldment subassemblies to act like a single part in the Parts List.  To change that, go into the Bill of Materials and set the BOM Structure for those subassemblies to Normal.

[Borsht]

I cant seem to make it work.  I've gone to the sub assembly, clicked Bill of Materials, Structured tab, then pulled down the icon to get to the Structured properties to select the Level, but First level is shown, grayed out and not  changeable.  .  In doing this I noticed that some of the parts in the list have their Part Numbers listed in grey instead of black. May that be the problem, and do you have a fix for that?

[johnsonshiue]

Hi! I believe you are looking at an iAssembly BOM table, right? iAssembly BOM does not support PartsOnly. You need to place the iAssembly member in another assembly and then look at the BOM table there.

iPart/iAssembly were designed to be library components for reusing purpose. The BOM table for iAssembly has limited usage. It is usually part of a bigger assembly.

Many thanks!

[Anonymous · Accepted solution]

I believe I found the solution for this, at least in Autodesk Inventor Professional 2024.

You have to go to the assembly file, and then click on Bill of Materials. It should bring up the Bill of Materials window and have 3 tabs listed: Model Data, Structured, Parts Only (Disabled)

If you click on the Structured, which is what the Parts List on the drawing is going to pull information from, it will initially only have item A listed, with a total quantity of parts on the assembly. However, if you click on the Model Data tab, you will notice that all the parts have A listed by it. You can manipulate the Part Number by clicking on each item and entering in a new one. It could be difficult to know what each part is since there is no width or length column available, but it does give a part view.

I hope this helps. It took me a while to find this. I was struggling with the same problem I believe you were experiencing.