LOD, error " Cannot change the suppression state of component..."

[rchiccarine]

I have an assembly that uses iLogic to supress/unsupress various parts and their associated contraints.  Everything was working fine.  However, when I added a .idw of the assembly, I started getting a level of detail error:

Error in rule: Pistons & Rings [iLogic rule], in document: Head Assembly Master BP120 1L 1U.iam

Component.IsActive: Cannot change the suppression state of component piston:1.
The active Level of Detail in Head Assembly Master BP120 1L 1U.iam is not a custom Level of Detail.

The problem is that the current level of detail is a custom level of detail.  Also, I checked, the .idw views are set to the same level of detail.  I attached a picture of the error, you can see the LOD in the backround

[innovatenate]

There's a discussion, link below, where this same error is discussed. Have you reviewed this discussion?

http://forums.autodesk.com/t5/inventor-general-discussion/suppressed-components-in-bom/td-p/3407931

Just skimming the conversation, some key suggestions are not to have the drawing open simultaneously and not to have the Master LOD active. I hope that helps.

Thanks,

[rchiccarine]

I reviewed it and didn't find it helpful.  The assembly and drawing are both set to the same custom LOD.  Also, I get the error even when only one document is open.

[johnsonshiue]

Hi! I believe you might be hitting a limitation in LOD Drawing workflow. I guess you have an assembly referenced by a drawing view in one LOD state, while it is also opened in a different LOD. I need to take a look at the actual files in order to say the behavior is indeed a limitation. If possible, could you share the files with me? I can set up a secure account for you to upload. Please send me an email (johnson.shiue@autodesk.com).

Thanks!

[bgarden]

I can confirm another case of this exact thing happening.   The assembly and drawing file are looking to the exact same custom level of detail.  It appears fine until you try to access BOM either from assembly or by adding a parts list.  Then the error message stated above kicks in.  

[bgarden]

I can now confirm the drawing is a red herring.   I have removed all drawings linking to this assembly or any part in the assembly.  Everything seems fine until I try to access the Bill of Materials.  Then the error message appears.

[bgarden]

Ok, could never get this to work succesfully using suppression.

Instead, resolved the problem by using iLogic to control the Visibility of components.

At the drawing level, edited the Parts List so it was filtered to look to the active View Representation.

Created a second Parts List and modified its columns to group a custom property named Total Mass.  This Parts List was also filtered to the active View Representation.

If anyone needs further explanation of any of these steps just let me know.

[rchiccarine]

Johnson has solved my problem!!!!!

In his words: "Basically, the Constraint error is triggered due to the fact that iLogic code is trying to modify the assembly in a different LOD state.  The issue is caused by the two iLogic rules set to be run After Open Document. When you tried to create PartsList, Inventor load the assembly in LOD:Master behind the scene. Then the rules are run and they try to modify the assembly in LOD:Master."

Basically, I had some iLogic rules which changed the active state of parts.  These rules were triggered to run After Open Document"  I changed the trigger and haven't gotten the error since

Thanks Johnson!!!

[mrattray]

I recommend avoiding suppression altogether, for this reason as well as others. I've taken to using .isvisible. The BOM can then be controlled either by filter by view rep or by toggling the BOM structure of the components in your iLogic code.

[johnsonshiue · Accepted solution]

Bob,

You are very welcome! There is room for improvement in this particular workflow. I don't think users have to go through several steps to find out where the problem is. It was not apparent to me where went wrong either. I am sorry that it took a while to find a good solution.

Many thanks!

[cadcamm99]

The problem that I have with turning visibility off is when I show a different View Representation in a drawing,  all my invisible components are now visible in the drawing.