Purchased and Machined part in BOM

[SPerman]

We have a few parts where I buy an off the shelf part from a vendor, and then have the machine shop make modifications to it. I need both parts to appear in the BOM, but I do not want the purchased part to be visible in the assembly or the drawing, only the machined part.

I will say that I am terrible with SW BOM's, most likely because I haven't taken the time to properly understand how they work. For now I've been dumping the BOM results into excel and fixing any issues there, but I would like to eliminate that step, if possible.

[mattpeneguy]

1. Create 2 configurations.
2. Name second config, "Machined".
3. Add part on top of existing part in ASM.
4. Both the purchased part and the "machined" part will now appear in the BOM.
5. ???????
6. Profit.

[SPerman]

Can the BOM and the View the BOM is based on use different configurations?

[CarrieIves]

The way I would generally approach a part that is purchased and then modified is to make an assembly of the part and make the modifications on the purchased part in the assembly. If I make a drawing of it, I am likely to call out the purchased part as the material. (Cutting certain lengths of gasket, adding holes to a piano hinge are examples of things I have done in the past.) This assembly would be a sub-assy of your top level. When you make your BOM, you can expand out the sub-assy to also show the purchased part. I was going to try to take a couple of screen shots, but SolidWorks isn't cooperating this morning.

[Glenn Schroeder]

I don't work with BOM's often, but can you insert the purchased Part in the Assembly and then hide it? I think it would still show up on the BOM.

[SPerman]

The way I would generally approach a part that is purchased and then modified is to make an assembly of the part and make the modifications on the purchased part in the assembly.

That's a thought. The purchased part doesn't have to actually represent the part in a solid model, it just has to appear in the BOM.

[SPerman]

I don't work with BOM's often, but can you insert the purchased Part in the Assembly and then hide it? I think it would still show up on the BOM.

Yes, that works, until you do a "show with dependents" which I do quite regularly. Display states probably have a use case here, but that's another feature I haven't adopted.

[josh]

It sort of depends on where your BOM data goes next... but I have done this by having two different custom properties for the part number - One called "Dwg number" and the other "Purchase Number" (or something like that). Of course, there's a Vendor property as well. For most fab parts (parts that I make a drawing for) the Purchase Number and Vendor are blank (and the Dwg Number is blank for unmodified purchased parts). For modified purchased, I enter the Purchase Number and Vendor as well as the Dwg Number.

[JSculley]

The way I would generally approach a part that is purchased and then modified is to make an assembly of the part and make the modifications on the purchased part in the assembly. If I make a drawing of it, I am likely to call out the purchased part as the material. (Cutting certain lengths of gasket, adding holes to a piano hinge are examples of things I have done in the past.) This assembly would be a sub-assy of your top level. When you make your BOM, you can expand out the sub-assy to also show the purchased part. I was going to try to take a couple of screen shots, but SolidWorks isn't cooperating this morning.

This is exactly how I have been doing it for 20 years. I also typically create 2 configurations in the assembly, one of which is named 'UNMODIFIED' where all the assembly features are suppressed. Then you can have an alternate position view in the drawing which helps the machinist see the before and after:

[josh]

Then you can have an alternate position view in the drawing which helps the machinist see the before and after:

Now available for parts as well as assemblies!

[jcapriotti]

@SPerman

Insert the base vendor part into a new part model to make your modifications. In the dialogue select "Custom Properties" then "Cut list properties". This will insert the base vendor part custom properties into a new weldment cut list in your modified part. Insert into an assembly and drawing and make your BOM and select "Indented" as the type so you can see the insert part.