Bill of Materials in Drawing Files vs Assembly Files

[leonardheck]

Working on a project (as analyst) for retrieving the Bill of Material using the Inventor API and have a few basic questions for Inventor users. We are trying to determine if it is logical to extract the Bill of Materials based on data in the Drawing file, rather than the Assembly file.

1. Are Drawing files typically linked to Assembly or Part files? If not always linked, for what reasons would they not be linked?

2. Would the Parts List present in a Drawing File hold data that isn’t already present in the Assembly file? If not, for what reasons would the data be different?

3. Is it likely that Drawings would be created without an associated Assembly/Part file? If not, for what reasons would they not be associated?

4. Is there any specific reason to retrieve Bill of Material data from a Drawing file instead of an Assembly file if the files are linked?
   

   Thanks for your responses.
   

[swalton · Accepted solution]

I will answer based on the drafting practice at my office.

First, some definitions:

BOM: A list of components in an assembly file.

Parts List: a child of a BOM, placed in a drawing file.

1. We use drawing files as a way to convey 2d information about the 3d cad model of a part or assembly.  A drawing that is not linked to a part or assembly will be blank.  In my practice, there are times when concept level drawing will show several different assemblies or parts and there will be times that a part or assembly is shown on several different drawing files.  A drawing file can display a parts list for a part or assembly that is not shown in a view on any sheet of the drawing file.

2. Parts lists are children of assembly BOMs.  The user can manually override values in the parts list table and not push those changes back to the source BOM.  We don't do this.  The user can filter the Parts List to only display components that are shown in assembly Design View Representations.  I have done this once or twice.

3. I can't see a reason to do this, but I am sure that someone has.

4. Inventor is set up so that information about parts flows into an Assembly BOM and then into Parts Lists on drawings.  The assembly BOM is the master set of information.  You will need to decide what information you need to pull from your model to decide if you should pull from the assembly BOM or the possibly filtered, manually edited, re-numbered, etc Parts list in the idw file.  If you choose to pull from the Parts List, your users will have to understand what local overrides they can apply to parts lists and still give you the data you need.

[mcgyvr]

I think a BOM should always be extracted from the assembly file.

[CCarreiras]

Hi!

For start:

The part list in Drawings are always associative with the BOM (Bill Of Materials) configured in the 3D Assembly.

Part List: in Drawing

BOM: in Assembly

1 - They are always linked. Any remove or add in the 3D model, will be reflected in the drawing part list.

2 - If there's no extra configuration, the data in the drawing and in the assembly must be equal.

The data can be different in drawing and assembly for many reasons, but this only occur due user edits

Examples:

a) Type of List: you can have a list by "Struture" (where main assembly parts and sub assemblys are considered as 1 member) or Listed by "Parts only" (all the parts are counted, from the main assembly and the all the parts from the subassemblys)

b) In BOM you can configure some assembly elements to be "Invisible" in the lists, they are just like a phantom and they are in the assembly for model/position issues, these phantom parts are supposed not to count in the drawind list.

c) Also in the drawing, you can have filters based in "represention views", "Standard content center components (only, in or out of the list)", "purchase components (only, in or out of the list)", etc etc.

3 - To work all well, the assembly must be placed first in the drawing. Always will be associative.

4 - Like i said in point 2, in drawing you can have several filters to have several part lists, so you can have one for manufacturing, other for content center, another for purchase elements etc, but these "Sub part lists" are always based in the main list, provided by the 3D BOM.

So, in the end, you have to study well how works and how to configure the assembly BOM. When you understand this, it will be easy to have a good data in the drawings.

Also you can extract the data in both enviroments, so you must know the type of info do you need.

Did you find this reply helpful ? If so, use the    Accept as Solution or Kudos - Thank you!

[leonardheck]

Thanks. I appreciate your input. It has been helpful.

[leonardheck]

Thanks for your input. I appreciate it.

[leonardheck]

Thanks of your input. It is appreciated.