Level of detail and Parts List

[Anonymous]

After cussing LODs for months I have decided to give in and see if I can make them work for me. I have an assembly that I am designing that has 3 possible options for manufacturing. Looks like a good place to use LODs to suppress items from the other options. Now I am attempting to make a drawing with a Parts List for one of the options but even with the components selected as referance and suppressed in the LOD shown in the drawing , all the components are showing in the Parts List. Short of setting the parts to suppressed or referance in the default or master LOD, what do I need to do to remove these parts from the parts list?

Thank you

[jtylerbc]

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@jaskiratVPK8U wrote:

I am also looking for the solution to get right BOM/parts list in the drawing by using different level of details. I have used solidworks for 7 years and it has configurations (same as level of details)

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This statement (bolded above) is not correct.  Inventor's LOD's are not equivalent to the Configurations in Solidworks.  As was mentioned a couple of times earlier in this thread, LOD's are not really intended to be a configuration tool.  They are intended for memory management to improve computer performance while working in the model.  

The closest equivalent to what you want in Inventor is probably iAssemblies, not LOD's.  There's a good chance you are still correct about Solidworks having the advantage in this area.  But currently, I don't think you are comparing the correct features in the two programs.  Inventor LOD's and Solidworks Configurations were designed for completely different purposes. 

[RNDinov8r]

So, this thread has been somewhat eye opening for me. I have always assumed that you control the BOM with LOD's not DVR....and I've been using this software for nigh 13 years. I decided to run an experiment yesterday using iLogic and LOD's. 

I created a parameter called "Style" and made it multivalue text. I then created three variables for the parameter. "Type 1", "Type 2", and "Type 3". 

I then created a form and dragged the paramter into the form...iLogic creates all the buttons and pull downs automatically.

Then I wrote some super quick iLogic code to suppress objects. (I created an LOD called iLogic - since you can't run iLogic code that suppresses/activates objects in the Master LOD). You can see how easy it is to write code to suppress or turn on...I copied 2 of the 3 if statements and just changed some True to False ....

'Controls ObjectSuppression
If Style = "Type 1" Then
	Component.IsActive("Assembly1:2") = False
	Component.IsActive("AS1211F-M5-06A:1") = False
	Component.IsActive("AS1211F-M5-06A:2") = False
	Component.IsActive("Festo Adapter:2") = False
    Component.IsActive("Festo Adapter:3") = False
Else If Style = "Type 2" Then
	Component.IsActive("Assembly1:2") = False
	Component.IsActive("AS1211F-M5-06A:1") = False
	Component.IsActive("AS1211F-M5-06A:2") = False
	Component.IsActive("Festo Adapter:2") = True
    Component.IsActive("Festo Adapter:3") = True	
Else If Style = "Type 3" Then
	Component.IsActive("Assembly1:2") = True
	Component.IsActive("AS1211F-M5-06A:1") = True
	Component.IsActive("AS1211F-M5-06A:2") = True
	Component.IsActive("Festo Adapter:2") = True
    Component.IsActive("Festo Adapter:3") = True
End If	


 

I then dropped the assembly into a drawing, selecting the iLogic LOD for the view. I was able to quickly go back into the model, open the form, and change the style, and the parts list updated flawlessley when I went back to the drawing. 

This may be a good method, if you make a master model that is your template assembly with all parts, pick the right configuration, save as a new p/n, and then delete out all the suppressed items. Honestly, I haven't worked on it, but you could probably write a quick iLogic code that would delete all suppressed content...therefore making your model truly accurate.

That said, you if there was a way to control the BOM style (Normal/Purchased/Inseperable/Reference) with iLogic easily, you wouldn't need a special level of detail...as you would not need to suppress anything...basically anything set to reference wouldn't be counted. How do you alter this thru the API?

[BP-OZ]

I know this is a very old thread, but 'set your hidden parts to reference' is very good advice. 

That is the simplest solution. 

[Anonymous]

This helped me, but overcomplicated... here the short version:

Before suppressing a part, just define it's BOM as "reference", then suppress it in the level of detail.

Then in the drawing, you'll have the correct BOM structure for that particular level of detail you are referring to.

Enjoy.

[ps-kirk]

I know this is an old thread but it seems to be the most searched when investigating LOD and parts lists/BOMs. We developed a simple workaround for this about 5 years ago and just recently I had to rediscover this myself. I'll try to add more details later, but here is the short of it.

1. We start with a main level assembly. In our case we define it as 000.
2. Within the main assembly there are various 1st, 2nd and 3rd tier subassemblies.
3. Establish a LOD that identifies the subassembly you want to annotate in the Inventor drawing. In my example I use 310 for a 2nd tier subassmebly.
4. While the 310 LOD is active, supress all parts and assmblies that don't belong in the main assembly as part of the 310 assembly that you want in the drawing.
5. Create a new Inventor drawing as normal and insert the main assmbly as the view you want to annotate using the 310 LOD . Associative does not need to be checked.
6. Create a parts list. Make sure that the BOM view is set to "Structured".
7. Balloon the LOD view. These initial balloons will show the item # of the items normally found in the main assembly. In my case they were all item #4.
8. Open the parts list. Between the balloon icon and the assembly icon in the parts list you will see a + sign. Click on the + to expand to the next tier (unsuppressed parts/assemblies within the main assembly).
9. In my 310 case I am dealing with a 2nd tier subassembly so I need to click the + sign one more time. As per the above screen capture I had two 300 level 1st tier subassemblies in the main assembly. If I would have done this Parts List BOM View as parts only I would have end up with double the amount of item qty as shown in the LOD (which would have reflected the actual parts qty in the main assembly.    
10. Now you have a LOD view defined in the main assembly that shows the correct BOM item qty for the subassembly you wanted.

Hope this solves your LOD BOM problem.

[SER4]

Here's something to vote for:

https://forums.autodesk.com/t5/inventor-ideas/level-of-detail-filter-for-parts-list/idi-p/7255784

but it's probably all irrelevant with the new Model States coming:

https://knowledge.autodesk.com/support/inventor/learn-explore/caas/CloudHelp/cloudhelp/2022/ENU/Inve...

[85180200]

the filter:"balloned items only "can help you?

[ggreene_64]

The best solution I have found (now using Inventor Pro 2021) is to use the filter in the Parts List editor, and use the 'Ballooned Items Only' filter. The only parts that show up in the parts list are those that have a balloon attached. You just have to make sure you attach balloons to all parts.

Sorry, I just now saw the previous message that says the same thing.