BOM quantity custom property

[the_h4mmer]

Using Solidworks 2021 SP5, I'm trying to use the custom property as the BOM quantity, and yet the value doesn't seem to update in the BOM table.

Here's what I'm doing (sorry for the lack of screenshots):

1. Create model of standard length item, 1ft
2. Use Design table to make configurations where only the "cable length" custom property (for configurations only) changes based on the configuration name (n*1ft)
3. Make a second custom property "Length" and set this to reference the "cable length" conflagration custom property, this does update when switching configurations
4. Choose the "Length" as BOM quantity in custom property window
5. Add model to assembly, choose a configuration for the model, but only use the "Default" configuration for the assembly
6. Create a drawing from the assembly
7. Add BOM table
8. BOM table quantity for model = 1 and not "n" like it should

I looked around online and don't see anything else that I should have to do to make this work. Anyone else figure out how to get this to operate correctly?

I did find a small work around, but I don't like it. I can delete the Quantity value from the BOM table, then just reference the model custom property "Length" but if someone else needed to reuse this model, they would need to know to do this and the promise of using a custom property as BOM quantity would mean that it would just work without having to relay additional instructions.

[JSculley]

It's a little hard to follow, but it sounds like you want to have a model where the length is always a base unit (e.g. 1 foot), and a custom property (e.g. LENGTH) is driven by the base unit multiplied by the configuration name. And then this custom property is used as the BOM quantity. If that's correct, I think you may be making it harder than it needs to be. Just create a design table, with some $USER_NOTES rows and columns to hold your base unit. Then use an absolute reference to this base unit cell in the formula to drive the length property in the design table:

Switching configurations changes the LENGTH property (which I've linked to a note, so you can see that it changes):

Then, as you know, set the BOM quantity to the LENGTH property in the Custom Properties for the configurations:

If I make an assembly, and drop three instances of the part, each with a different configuration, the BOM looks like this:

[the_h4mmer]

Seems like there was something going on with my instance of Excel. Yesterday I was running into this issue and today the Design Table wouldn't even load. I closed out Solidworks, closed out Excel, and restarted Solidworks, then inserted a Design Table. After that, it worked as expected.

Now I just need to figure out a way to have the Configuration to default select the Document Name for Part Number in the BOM instead of the configuration name...

[JSculley]

Now I just need to figure out a way to have the Configuration to default select the Document Name for Part Number in the BOM instead of the configuration name...

That is controlled by your part template.

[the_h4mmer]

That is controlled by your part template.

Could you point me to where that setting is? I couldn't find anything obvious in the Document Settings that would control this behavior.

In Configuration Prosperities, the label is for "Bill of Materials Options" but I can't seem to find anything similar to control the default setting

The BOM options look like it's only controlling the BOM table headers

The Configuration options seem to be primarily to do with data marks and saving

[JSculley]

If you open your document template (.prtdot) and change the setting in the Configuration Properties (your first image above) and then save the template, any future parts made with that template will default to that setting.

[the_h4mmer]

Perhaps the Part template needs to have more than the Default configuration because I opened the template, set the Configuration BOM Options to use Document Name for Part number (for Default config), and saved the template file. When making a new part with the Design Table, it's still using the Configuration Name for the generated configurations in the BOM Options and I have change each one manually to Document Name. I'll do more testing later, but this has gotten me 97% of where I need to be, so thank you @JSculley.

FYI, for anyone coming across this later. If you set LENGTH as your BOM Quantity for the configurations before you make the Design Table, that setting will carry thru to all the generated configurations. If you do this after, you will need to do it for each configuration manually.

[JSculley]

When making a new part with the Design Table, it's still using the Configuration Name for the generated configurations in the BOM Options and I have change each one manually to Document Name.

Yep. I see that behavior too. A quick search of the Knowledge Base turns up this:

=================================

Solution Id: S-026841
Product: SolidWorks Office 2008
Created: 8/28/2008
Reviewed Date: 1/20/2021
Area: Configuration
Sub-Area: Part

Question: When creating configurations using the design table, how is it ensured that the 'part number displayed when used in a bill of materials' = document name?

Answer: Add a column called $Partnumber, and in the cells for each configuration, type “$D”.
==================================

Seems to work.

Talk about some secret hidden knowledge......