I am working on a prototype of a project and it involves an antenna. This means that I will probably have to tune this first version a little bit once I get it assembled. To do this, I wanted to place into my circuit a "dummy" capacitor. I realize that I could make a pads in the CAD with the right dimensions, but this wouldn't show up in the schematic. Also, I have seen in schematics capacitors with DNP values. This is what I am essentially looking for. Is there an easy way to do this/best practice? I am a student trying to learn the right way to accomplish these tasks..

  • 3
    \$\begingroup\$ Look in the Altium documentation for the term "variants". \$\endgroup\$ – The Photon Aug 5 '14 at 18:54
  • \$\begingroup\$ Ahh much better googling that. I'll answer this later, thanks \$\endgroup\$ – mtleising Aug 5 '14 at 18:57
  • 1
    \$\begingroup\$ For a one-off, I wouldn't usually mess with variants, though. Just put "DNP" in the comment field. \$\endgroup\$ – The Photon Aug 5 '14 at 19:05
  • \$\begingroup\$ Ok, would I have to do anything extra for the manufacturer or do they usually look for and see that stuff? Or does that actually show up in the BOM as DNP? \$\endgroup\$ – mtleising Aug 6 '14 at 1:01

The correct way to do this is with variants, as others have pointed out. Do not use the 'Type' property. For every project I have a variant named "Only Populated Components" which makes it super easy to DNP components. Not populated components should NOT appear on the BOM, as this will indubitably lead to questions from the CM. They should also not appear on the PCBA assembly drawing.

A good sanity check to see what is populated and what is not is to view the PCBA in 3D; you can tell at a glance which components are missing.


The preferred method for this functionality seems to be the component's Type property. Specifically, I think you would use the Standard (No BOM) part type for the capacitor in question. This means the part has electrical information and is synchronized between the schematic document and the PCB document, but it will be ignored by any BOM generation.

See Altium's documentation page on it.

  • 2
    \$\begingroup\$ is there a way to show this on the schematic? So people see that without looking at the BOM. \$\endgroup\$ – Brian Carlton May 29 '17 at 0:01
  • \$\begingroup\$ If you use Variants, rather than Type, you can select the variant in the Project tree, then compile, then you get a little tab on the bottom of the screen. When you click on the tab, the menus change around a little, and the non-populated components get marked with a big red X, or whatever option it is you have set for how to show these things. From that view you can also click on the X icon and click individual components that will be "not fitted", which is Altium's terminology for non-populated/non-stuffed, whatever. \$\endgroup\$ – Sonicsmooth Nov 2 '18 at 19:33

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.