Level of detail and Parts List
Accepted solution
Hi JimSteinmeyer,
As mentioned above, the iAssembly tools are the correct choice for creating configurations. LOD's are intended for memory manangment.
With that in mind, try this:
- Set your LOD active and then right-click on it and choose "Copy to View Rep"
- Then set the newly created View Representation active.
- Then use these steps to create a rule in iLogic:
- On the ribbon, click Manage tab > iLogic panel > Add Rule button.
- Name the new rule.
- In the rule text area of the Edit Rule dialog box, simply paste in the code below.
- Click OK to save and run this new rule.
' set a reference to the assembly component definintion. ' This assumes an assembly document is open. Dim oAsmCompDef As AssemblyComponentDefinition oAsmCompDef = ThisApplication.ActiveDocument.ComponentDefinition 'Iterate through all of the occurrences Dim oOccurrence As ComponentOccurrence For Each oOccurrence In oAsmCompDef.Occurrences 'check for and skip virtual components If Not TypeOf oOccurrence.Definition Is VirtualComponentDefinition Then 'set BOM as default if the component is visible If Component.Visible(oOccurrence.Name) = True Then Component.InventorComponent(oOccurrence.Name).BOMStructure = _ BOMStructureEnum.kDefaultBOMStructure 'set BOM as reference if the component is not visible ElseIf Component.Visible(oOccurrence.Name) = False Then Component.InventorComponent(oOccurrence.Name).BOMStructure = _ BOMStructureEnum.kReferenceBOMStructure End If Else End If Next
This will set the BOM structure so that the visible component occurences won't list in the BOM.
I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com
As you have discovered, Inventor does not handle this workflow well.
LODs are memory management tools, not configuration management tools. You are finding the reasons that make using LODs to define assembly steps hard.
I haven't tested any of this, but if I had to make assembly steps I would use the iAssembly workflow.
Configuration management in Inventor is handled by iAssemblies. As I understand it, Inventor will give you a correct Parts List for each iAssembly member on a print. I think that workflow will have fewer issues for you.
See http://help.autodesk.com/view/INVNTOR/2014/ENU/?guid=GUID-6E529299-CAB9-4F5C-B100-7901D877B83F
Convert your design to an iAssembly and make a new member for each assembly step, plus a member for the finished assembly.
When you go to make your print, place the place the finished assembly member on the first page and add your parts list. Then add a page for each assembly step and place the proper iAssembly member on that page. Add a parts list pointing to that iAssembly member too.
You might try building a quick test assembly with a few components to see if the iAssembly method will come closer to your needs.
If you have an existing drawing that you want to keep, try this:
Keep the LODs that you have now and add the iAssembly members as above. Generate all the member assemblies and save them to disk. Go to your drawing and place new Parts Lists. When you do, don't pick the view in the page to define the Parts List. Instead, use the file open button to navigate to the correct factory member on disk. That should get you a Parts List that matches the LOD as long as the LOD from the iAssembly factory and the factory member assembly have the same components.
Steve Walton
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Inventor 2025
Vault Professional 2025
Hi! This is an old thread. Without getting into detail of the implementation, I would like to bring up some basics about LOD and PartsList. Inventor LOD was designed to be a memory management tool to overcome memory usage limit in 32-bit Windows. It unloads files to reduce memory footprint. However, the BOM table remains unchanged in any LOD, even if you unload a given component, it will remain on the BOM and show up in the PartsList.
There is a way to deduct the component from the BOM and the PartsList by making the component "Reference." You can manually do it or programmatically do it. iLogic IsActive() command automates the process. But, it does not change the fact that LOD does not alter BOM data. This approach only works if you export BOM table or PartsList as static data. If you have two LODs: Master vs Non-Master. You cannot have two BOM states or two different PartsLists at the same time. It is not supported yet.
The better approach here is to use Design View Rep. You can simply copy LOD to Design View Rep. Then activate LOD Master and activate the LOD converted Design View Rep. BOM data is still unaffected. But, in the PartsList, you can turn on Design View Rep Filter to deduct the invisible components from the PartsList. You can have as many Design View Reps as you want and each has a different PartsList.
Many thanks!
Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer
Hi! You are using the right workflow. It should work. Try this. Make sure the assembly has been saved. Close the assembly and the drawing. Open the drawing by itself -> edit the drawing view -> select the desirable DVR, check the associative box, and set LOD to Master. Now edit the partslist and enable the filter.
I guess the drawing view was still referencing the custom LOD.
Many thanks!
Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer
Deleting the View Did the Trick, very odd that thats what stops the process.
Thanks for the Help 
