In an idw, if I select Parts List, the BOM setting of layers can be swithced between First Level and All Levels. Once I select my view, the option grays out and selects First Level. I need my BOM to show All Levels.
What do I do to select All Layers for my drawing?
Solved! Go to Solution.
Solved by Curtis_Waguespack. Go to Solution.
@eveylynne wrote:In an idw, if I select Parts List, the BOM setting of layers can be swithced between First Level and All Levels. Once I select my view, the option grays out and selects First Level. I need my BOM to show All Levels.
What do I do to select All Layers for my drawing?
Once you pick a view, it defaults to the level settings set in the BOM for that assembly. Right click on the view, prior to placing your parts list, and select Bill of Materials. Once in the BOM go to the View Properties:
You can select All Levels under there, and then when you place a Parts List, it will come in structured that way.
Chris Benner
Inventor Tube & Pipe, Vault Professional
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Can you post the files, or a sample drawing (with parts) that shows this behavior? Or at the least some screen shots?
Do you use Vault? What version of Inventor is this?
Chris Benner
Inventor Tube & Pipe, Vault Professional
Cad Tips Tricks & Workarounds | Twitter | LinkedIn
Autodesk University Classes:
Going With The Flow with Inventor Tube and Pipe | Increasing The Volume with Inventor Tube and Pipe | Power of the Autodesk Community | Getting to Know You | Inventor Styles & Standards |Managing Properties with Vault Professional | Vault Configuration | Vault - What is it & Why Do I Need It? | A Little Less Talk - Tube & Pipe Demo | Change Orders & Revisions - Vault, Inventor & AutoCAD | Authoring & Publishing Custom Content
@eveylynne wrote:It is grayed out there as well.
Hi eveylynne,
When you're in the BOM editor as cbenner instructed, ensure that you have the Stuctured tab set active. If the Model Data tab is active, then the button will be grayed out.
Once you have the BOM set to use All Levels, then you can edit the Parts List in the drawing, and should see a + next to the subassemblies that can be clicked to show all levels.
I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com
Thanks Curtis... I missed that little detail!
Chris Benner
Inventor Tube & Pipe, Vault Professional
Cad Tips Tricks & Workarounds | Twitter | LinkedIn
Autodesk University Classes:
Going With The Flow with Inventor Tube and Pipe | Increasing The Volume with Inventor Tube and Pipe | Power of the Autodesk Community | Getting to Know You | Inventor Styles & Standards |Managing Properties with Vault Professional | Vault Configuration | Vault - What is it & Why Do I Need It? | A Little Less Talk - Tube & Pipe Demo | Change Orders & Revisions - Vault, Inventor & AutoCAD | Authoring & Publishing Custom Content
Thanks guys, I'm still stuck though.
I'm working in 2014. We don't use Vault. The assembly is large & proprietary, so I can't really share it. It is also an iassembly.
I shared two pngs to show my menus. Both are greyed out.
I've treid using different idw templates, in case my custom one was somehow doing it. I've tried enabling & disabling the BOM. No luck.
I also tried a smaller assembly that wasn't an iassembly, and that one let me choose All Layers. I can then edit the BOM, and expand the sub assembly parts and they show up as they should.
Any suggestions?
@eveylynne wrote:... It is also an iassembly.
Hi eveylynne ,
There's the issue. iAssemblies simply cannot be expanded in the BOM.
Unfortunately, I don't have any suggestions for getting an expanded BOM from an iAssembly other than the one mentioned here (see the comments area):
http://beinginventive.typepad.com/being-inventive/2011/05/exporting-all-level-bom-from-inventor.html
I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com
Thank you!
That script more or less did what I needed!
All of the parts are in the BOM, and I mean everything, so I still need to edit quantities. However, that is much better than some of my alternatives.
Hi
There is a workaround to your problem.
Create a new assembly and place one of the iAssemblies into the new assembly.
Save this as something like NAME_DETAILING_ASSY.
This will now give you full control over the BOM/Parts list. and will maintain any links to the host assembly.
Just an fyi, the BOM seems to revert in the assembly. You have to run it every time you open it? Anywho, it resets the BOM on the print to one layer.