Cannot open BOM after a save in alternate LOD

[Anonymous]

I am having continuous problems with the bill of materials not updating properly and I have further pin pointed a reason but cannot find a solution other than a work-around that is susceptible to being missed by the drawing office.

The problem

I have an Ilogic model that supresses and un-supresses parts. I have a Level of Detail called ILOGIC that the model works on to allow any suppression. Once the model is configured and updated I then perform a save (still on ILOGIC LOD). I then open a drawing that contains a parts list and sometimes the parts list is incorrect.

The work-Around

I have to make sure that the designers completely close down the updated saved model and re-open it before opening the drawing that contains the parts list or opening the parts list drawing with the model closed.

Further Details

It seems that although we are performing a complete save of the model in an alternative LOD it still requires a save in Master LOD. If the rules are run to supress/un-supress parts and then the model is saved it will not allow me to open the Bill of Materials unless I change the Level of Detail to Master and perform the save again.

This has been a continuous problem for a few years but I never twigged that it needs to be saved on Master LOD, I have just simply closed and re-opened the model.

Surely this cannot be correct? And if so how do I overcome this when we are working with Ilogic in an alternative LOD?

Inventor 2014

[CCarreiras]

Hi!

For iLogic models, it's a good practice to update and save the 3D model. Close it and open the drawings, update and save.

Don't maintain the 3D model and drawings open at the same time.

[Anonymous]

Hi Carlos,

As the writer of the Ilogic within our company I have come to realise this....although no-one can tell me why.

The problem I have is we have 2 seperate methods of updating Inventor models; Spread sheet driven and Ilogic. For complex models the drawing office updates models using spread sheets which then allows  them to manually customise and delete parts as they deem fit. Doing this breaks no rules.

For simpler models we use Ilogic. When using Iogic there is no manual customisation allowed as this breaks the model as rules cannot be re-run.

Because we are constantly swapping between 2 different methods it is impossible to get the rest of the drawing office (and our china office) into a habit of updating, saving, closing, opening, updating, saving, opening drawing, saving.....etc. They just want to save the model and open a drawing with a parts list in and it be correct....as do I.

We are constantly having incorrect parts drawings because the designer forgot to close and re-open the model to re-set whatever it is that needs re-setting.

Cheers anyway.

Gareth

[mcgyvr · Accepted solution]

No idea here but what if you do a rebuild all then save?

[Anonymous]

I have all the same problems without iLogic involved at all.  It seems to be just a LOD problem.  It's a very serious issue for us and we've found no solution.  Not having an drawing and assembly open at the same time is just painful.  Having to open and close constantly is just rediculous.  This is a serious Inventor problem that have yet to see any solution for.  Not much help I know 😞

[Anonymous]

Hi Ikrenler,

Can you try Rebuild All before you save the model as McGyvr suggested? Initial testing for me having possitive results.

If you agree then we can accept Rebuild All as the solution.

[Anonymous]

I can try it maybe on a simple assembly.  However, on my larger ones it took so long (20 minutes +) I gave up and killed the task so I don't really see it as a solution unfortunately.  

[johnsonshiue]

Hi! There is a little bit confusion about how iLogic "IsActive" and LOD work for BOM. I have to reiterate that LOD is a memory management tool, which is not supposed to alter design intent or assembly definition. What iLogic "IsActive" is to provide a way hooking up component suppression status and the component's BOM Structure attribute. When "IsActive" = False, the component occurrece will be suppressed and its BOM Structure attribute is set to "Reference." Then, the occurrence will be removed from the BOM table because the occurence is a reference component (you can do it manually also). This behavior gives false impression that Inventor assembly can be configured to multiple variations using custom LODs and iLogic "IsActive" statements and have them documented in drawing with PartsLists accordingly.

However, at the moment, there is only one BOM table in a given assembly, which all PartsLists of the assembly views point to. So, LOD1 PartsList in drawing will be the same as LOD2 PartsList, depending on which LOD is active in the assembly. There is no way to create LOD1 PartsList based on LOD1's component suppression status and  LOD2 PartsList based on LOD2' status respectively. It will require multiple BOM tables in an assembly, which is not available right now.

If you need to document variations of assembly, particularly different BOM, you will need to create multiple assemblies or convert it to an iAssembly.

Many thanks!

[Anonymous]

Absolutely agree Johnsonshiue. When not working with Ilogic I link the parts lists up by Design view rep filter with the LOD in Master.