Different BOM structures in one assembly.

[malcolm_smith]

I have a longstanding issue in Inventor with not being able to assign different BOM structures in one assembly. This is an issue if you have a large assembly of a plant and you add new equipment. Specifically, if you have more than one draftsman working on a project what is 'reference' material to one may be 'normal' to another, for the purpose of showing interfaces between bits of equipment. In inventor, it becomes necessary to have different top level assemblies to be able to show this in drawings. Ideally however, you would want one source of truth for the master assembly, rather than multiple copies which need to be managed to maintain consistency.

This issue could be solved simply by allowing different BOM structures to be assigned to view representations or LOD representations. I tried to raise this as an IDEA on the Inventor Ideas forum, but so far I have had no support. I see this as a glaring fault in Inventor. I'm surprised that no-one else seems to see it as an issue, so I though I would raise it here for discussion. Maybe others have workarounds or workflow suggestions which could help?

[Xun.Zhang]

Hi Malcolm,

You are right, LODs are primarily a memory management tool, BOM is the structure holder for entire assembly.

If you suppose to view the structure in Drawing for partlist, here is an example to laverage DV along with iLogic code, hope it can ease your pain a little bit.

create parts lists out of View Representations

Thanks!

[malcolm_smith]

Hi Xun,

I had a quick look at the iLogic code, but I don't think that solves the problem. The issue is that on one drawing I want to show e.g. part (or assembly) A as 'normal' and part (or assembly) B as 'reference'. On a second drawing I want to show A as 'reference' and B as 'normal' This is required for both the linework displayed on the drawing and for the parts list on each drawing.

What I want to be able to do is to is to set the BOM structure for the parts within the assembly and save that in a view representation or LOD (I don't care which). Then you could create another BOM structure and save it in another view representation or LOD, so that you could call up whichever was required for the drawing you are doing.

[Xun.Zhang]

Hi Malcolm,

I know the 'workaround' is not satisfy you perfect, I will try to contact project team to understand more and keep you update.

Sorry for that.

[MechMachineMan]

Design View Reps. PartsList filtering (by assembly views or ballooned parts). Making rows invisible. Changes in line types. 

[torbjorn_heglum1]

Malcolm,

I don't fully understand your workflow here, as it looks like you are sort of mixing the concept of assembly BOM and drawing views.

As I understand the concept, the assembly BOM is absolute. This is all the components you need to build your equipment. For the 3D model there are some brilliant settings to control how each individual component shall be handled in the BOM. If you set one component to be Reference, it is support geometry only and will not be included in the BOM (or in weight & CoG calculations).

One specific component cannot be both a BOM member and not a BOM member. Therefore my humble opinion is that different BOM structures should not be a possibility for one assembly (unless we are talking about configurations).

To show what is 'reference material' in a drawing view, you could base your drawing on the main assembly and change the layer for the 'reference material' to a suitable reference style.

Or you can duplicate the components you need as reference in the assembly, so you have both a 'real' and a 'reference' version. Then you can make view representations for the drawing views you need, showing real or reference versions as required.

Or you could do as we do here. To avoid spending too much time in the huge and slow main assembly, we make sub-assemblies with individual equipments (or groups of equipments), where we also place necessary 'reference material' and set this to BOM Reference. Each subassembly have a view representation called 'Reference Hidden', that we use associatively in the top assembly.

Ok, this was a lot of text, but I hope it makes sense anyway.

(By the way, don't mix up the use of LOD and view representations. Autodesk isn't making it easy for us, making this functionality that looks and feels so similar. My opinion in short: stay away from LOD's, except simplified LOD's for the real large assemblies)

Torbjørn

[malcolm_smith]

Perhaps I need to be a bit more specific. I work in the cement manufacturing business and we have used Inventor for over 15 years for designing the installation of new or modified equipment, which may be anything from patching a hole in a bin to a complete new building and associated equipment and even a new greenfields site on occasion. We do often have very large assemblies (e.g. a complete mill building) that have evolved over many years. They are not always structured in the most efficient way, but a structure which works in one instance may not work so well for another, so they are what they are. The assemblies we work with are often too complex to be spending time trying to make up smaller assemblies for referencing purposes (although we do have to do this on occasion). It's easier to set up an LOD or view rep within the master assembly.

We often have the issue that several new pieces of equipment, and/or platforms etc. are being installed simultaneously. Each piece of equipment will have its own assembly and those assemblies will be contained in a master assembly of the building and existing equipment. When doing a GA for one equipment assembly, you want to show it in situ with the existing and other new equipment shown as reference. To do this in Inventor, I have to make a copy of the master assembly and toggle the BOM structure within the copy to get the desired result for that drawing. It's possible to end up with multiple copies of the master assembly, and as things evolve, no one copy can be relied on as being the absolute source of truth. It's a management issue which can easily get out of hand it there is a lot going on. It would be much better to be able work from one master model and be able to save multiple BOM states.

Regarding LOD's, we use them a lot because we are working with large assemblies. Often at concept stage we will have multiple options for equipment arrangements and we find it useful to use a LOD for each option.

[malcolm_smith]

I forgot to mention that using the BOM structure has major advantages over simply changing the linestyle of parts or assemblies within the drawing, like the fact that you can alter the way that hidden line calculations are done. It is also quick and easy to do and, of course, it aligns automatically with what shows up in the parts list.

[johnsonshiue]

Hi Malcolm,

At the moment, there is no workflow allowing you to have multiple BOM table representations in a given assembly. For your case, there are two workflows you can consider.

Option 1: Copy the given LOD to Design View Rep. So a suppressed component will become an invisible component. Then create a drawing view based on the Design View Rep. When you create a PartsList, make sure add Assembly View Representation Filter to deduct the invisible components.

Option 2: Save copy as another assembly. Configure each assembly accordingly.

Many thanks!

[malcolm_smith]

After discussing this further with my work colleagues, we are going to try the following workflow:

1) Maintain a master assembly, which has a BOM structure in which all components are set to 'normal'.

2) When creating an arrangement drawing, create a new assembly which contains both the part or assembly which is the subject of the drawing and the master model. The BOM structure of the master model will be set to 'reference' in the new assembly and visibility of the subject component withinin the master model will be switched off.

[johnsonshiue]

Hi! The issue with your proposed workflow is that you can only document the assembly in one state (normal or reference). You still cannot create two different PartsList of the same assembly in different states.

I think you will want to explore the Design View Rep workflow.

Many thanks!

[torbjorn_heglum1]

Malcolm,

then I understand your challenge a bit more. We have similar challenges here from time to time; as a crane manufacturer we also make upgrades of already delivered machines. 

We usually end up doing approximately as you. The existing crane model is placed in an assembly as reference, and we cut and chop as required to prepare for new equipment. New equipment are modeled as separate assemblies and placed as Normal BOM components. Then we can make drawings with focus on new stuff, a BOM and total weight of new equipment only.

This think could have been handled as configurations. So I guess we just have to cross fingers and wait til we get the functionality in Inventor

About LOD's again:

If you are limited by RAM you should absolutely use LOD. If not I definitely would prefer view reps. I find view reps more responsive + the drawing handle different view reps without performance issues. The 'edit include components' is great for small and medium assemblies, lock/unlock is very valuable. And for some reason, view reps is the only rep that can be rearranged in the browser.

But the most annoying problem with LOD's is when you have an open drawing with one LOD and the model open in another LOD. If you try to do something in the assembly you usually are stuck with this error message about editing different LOD. The only way to get rid of it is to close the drawing, do your change and open the drawing again. And with a large assembly drawing, this close and open if often a 5-10 min waiting.

(sorry for the rant - just had to explain my earlier statement)

Torbjørn

[catot]

@malcolm_smith @torbjorn_heglum1

I think I have a solution which will help you achieve what you want. See picture below.

If this is of interest, please let me know, and I'll post the workflow required. This is quite easy to set up and maintain.

[catot · Accepted solution]

Here's the workflow.

Create View Representations in the GA-Assembly (top-level). For every layout, create 1 view where only the parts/assemblies you want to show as active are visible, and another view where only the parts/assemblies you want to have as reference are visible. If your assembly doesn't have a Positional Representation, just create one and switch back to master. (explained why later)

On the Drawing, the main view for your layout, should have the "active-view" enabled.

Then create an Overlay View on top of it (that command is only available if there are minimum 2 Positions in the assembly, hence why creating it earlier). Use the "reference-view", and layer as Overlay. (you can even leave the Position at Master)

Filter your drawing partlist using the "active-view" you created.

Repeat as many times as required.

[malcolm_smith]

Torbjørn

Thanks for the info about LOD's. I do get drawing/model with different representations issue a lot, but I didn't reaslise it was specifically to do with LOD's. I can't remember exactly why we ended up preferring LOD's to view reps and I may have to review that for future work.

Mal.

[malcolm_smith]

catot,

I think I understand what you are doing there and it looks like an interesting solution. I will give it a try.

Mal.

[Anonymous]

Catot,

This was a great post showing the work flow and helped me with what I needed to show.

I do have one problem on my end. I use a 3rd party software called "cad-link" by Qbuild to push the Inventor Bom to my company ERP system (Epicor). Cad-link pushes the assembly BOM and not the drawing BOM so this work around doesn't help me with pushing the correct materiel to the ERP system.

Any thoughts?

[johnsonshiue]

Hi! Are you asking how to alter BOM table in assembly using LOD? If yes, you could leverage iLogic to do that. Please keep in mind, the solution does not enable you to have one assembly having multiple BOM representation at the same time. You can export BOM but the exported BOM will not be in sync with assembly, when there is another change in the assembly. If it is Ok to you, please read on.

I am not sure how much you know about iLogic. Here is what you can do.

1) Create a new LOD called iLogic in the top-level assembly.

2) Create a new rule. Find the components you want to removed from the BOM table. Simply write the statement for any part you want to suppress ("Part1:1" as an example).

Component.IsActive("Part1:1") = False

3) Then run the rule and open the BOM. Export the BOM table. You can automate this step in the iLogic rule also.

What Step2 does is simply set the component occurrence to Reference and then suppress the occurrence. This will remove the occurrence from the BOM table.

Many thanks!

[malcolm_smith]

Hi Johnson,

Unfortunately the iLogic solution doesn't help with having several drawings concurrently accessing one assembly, each requiring a different BOM structure. It may allow you to quickly toggle the BOM structure to produce the required drawing views, as long as no-one else was accessing the assembly at the same time. The BOM table is a minor issue. The main issue is the drawing view linework.

[johnsonshiue]

Hi! In that case, you need to save the assembly as multiple assembly files. Inventor currently does not have a good workflow to show different BOM or PartsList of states in one assembly concurrently.

Many thanks!