Handling DNP parts in ActiveBom in Altium Designer 19

Question

I have another issue with ActiveBOM in Altium Designer 19, this time related to DNP ("do not populate") parts. For example, I have a bunch of 1k resistors in my design, some of which are not populated: I have a field in the resistor library part called "Populate" and it's empty for parts to be used and set to "DNP" for parts to not be populated. So far, so good.

The exported base-view BOM has DNP has "[No Value], DNP" as the values and my vendor needs the DNPs removed from the BOM. So, I have to manually go through the schematic and find the designators for the DNPs and delete that designator from the BOM. This process has to be repeated for every BOM export.

This is silly, manual and time consuming. Is there a better way?

A flat-view BOM export (with Populate column showing) addresses these issues, but is not in a consolidated view.

Another, loosely related SO question about BOMs and DNPs.

Answer 1

You can use the Standard (No BOM) part type which will work better than using a custom parameter

Answer 2

An alternative solution to @Oscillonoscope's suggestion of using the "Standard (No BOM)" part type, is to use the Variants feature (Project -> Variants).

One would define a new variant of the base project. Open the variant manager and specify which parts are DNP.

You could then produce a BOM based on the Variant. This BOM would indicate the DNP parts along with all of the other parts.

You can also see the DNP parts by clicking on the schematic tab with new variant's name.

In addition, you can print SCH's with the DNP parts properly identified on the printout by specifying the Variant's name in the 'Variant' column of the OutJob setup window.

Good luck!