I've ran into quite a few engineers from unrelated backgrounds that put unpopulated components on the BOM. Some will do a section clearly labelled DNP at the bottom, others will leave them dispersed throughout the BOM, but highlight the rows.

Having a DNP section seems like the way to go if you must do this, the only downside I can think of being that there will have to be more manual editing of the CAD package output. (Have personally witnessed this, the DNPs were changed at the last minute, the DNP section didn't get editted properly, and parts that shouldn't have been on the board were placed.) Leaving them throughout and highlighting the rows seems suboptimal because there could easily be duplicate rows for populated and not populated, and again, more manual editing.

I don't see why this practice is necessary. A BOM by definition is a list of things required to build something. If a component is not on the BOM and assembly drawing, it should not be on the board. Adding components that aren't actually there just seems like a source of confusion further down the line for whoever enters the BOM into the ERP and purchasing. What does putting unpopulated parts on the BOM achieve that leaving them off the BOM and assembly drawing doesn't?


If you don't explicitly document that these components are not to be placed, you will inevitably have your manufacturing team notice that there is a location on the board with no corresponding line in the BOM, and delay the build to send an engineering query asking what is supposed to be placed there.

Explicitly documenting not-placed components avoids these queries, much like "this page intentionally left blank" in the manual avoids people asking what was supposed to be printed on the pages that were blank in their copy.

  • \$\begingroup\$ I would buy that explanation if the assembly drawing was non-existent, but if the assembly drawing says nothing goes there, and the BOM says nothing goes there, nothing goes there. \$\endgroup\$ – Matt Young Jul 1 '17 at 3:32
  • 19
    \$\begingroup\$ @MattYoung, the documentation shouldn't be written to please your aesthetic sense, or to make your life easier. It should be written to minimize the chance of mistakes in manufacturing. \$\endgroup\$ – The Photon Jul 1 '17 at 3:46
  • 3
    \$\begingroup\$ For me "manufacturer asked to do so" is always a good reason. \$\endgroup\$ – Gregory Kornblum Jul 1 '17 at 4:16
  • 1
    \$\begingroup\$ @MattYoung, a screw-up that can be caught in review (same designator listed under both DNI and with a PN) is better than a screw-up that can't be caught (accidentally dropped a line from the BOM so the assembly guys just assume all those locations are DNI). Also I doubt anybody ever reviews the assembly drawing in detail --- a manual operation --- when a pick & place file is available and can be automatically compared to whatever their machine's internal programming format is. \$\endgroup\$ – The Photon Jul 1 '17 at 18:55
  • 1
    \$\begingroup\$ @MattYoung many of our designs have several variants, different options such as output voltage or fitted interface, and I don't want to maintain say 16 Assembly drawings so we have a location drawing instead that shows where a component goes if it is fitted, though it may not be or a different value. Specifically listing not fitted components saves confusion as its clear for example R27 is not fitted otherwise the technician spends ages searching the BOM to make sure it is really not there rather than have they missed it. \$\endgroup\$ – Warren Hill Jul 7 '17 at 8:41

This practice is not necessary. But when there is a QC worker checking the board assembly, and she finds an unpopulated component, she will wonder, is it a mistake or not. So she will go to BOM and chem with the DNP section.

It's true that this method can be messed up, just like any other method.


There are several reasons why we might have a board with positions for components, where none are fitted in the final product.

a) These components control options, so a single bare PCB might be populated differently go into products with different capabilities.

b) It's expensive to make a batch of PCBs. The design might have changed to fix an error, or enhance a feature, but there are 10,000 boards to be used up.

c) These are test points, or needed to set up some test mode, and are only used in the lab, and should not be fitted in the production unit.

For whatever reason, boards may require component footprints that are empty. Of the three options for an 'infinite value' resistor ...

1) fit a very large resistor, so large it has no effect
2) don't fit the resistor and keep quiet about it in the BOM and
3) don't fit the resistor and mention that fact in the BOM

1) is slightly more expensive

2) troubles engineers who read the documentation in PCB manufacturers, test houses, repair houses, because they are checking against human error, and want to be happy that the board in their hand is really described by the document in front of them (has the component fallen off? was missed by the assembly machine? removed in error?)

3) only confuses people who don't know yet why it's done that way

  • \$\begingroup\$ Your first 4 paragraphs aren't related to the question. The question pre-supposes that not-installed components are part of a design and asks about the best way to document them. \$\endgroup\$ – The Photon Jul 1 '17 at 15:52

There are a lot of reasons for "Do Not Place" parts, and for that reason I maintain two different BoMs:

The procurement BoM. This does not include parts that are not fitted; from this perspective, it meets the requirement that there can be no confusion in kitting the assembly.

The engineering (design) BoM, where not fitted parts are clearly called out. If someone wants to know why, it should be clearly stated on the schematic.

The master print for production is the assembly drawing, and not fitted parts as well as unused reference designators have a table for each.

Note that pick and place files may have not fitted parts, which is why they are called up in the assembly drawing.

This does require proper procedures and some discipline, but it works.


These are good reasons but we have one more reason.

We use the same board for five different components (unique boards are expensive). What the component is depends on what parts are placed on it. This varies from four parts not placed to two-thirds of the board not placed depending on what part the board is to be used for.

A couple of placements take different parts depending on what component is being assembled, and one placement is a tuning resistor that actually does get swapped out with a soldering iron from time to time.


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.