21
\$\begingroup\$

I'm an experienced board designer, having designed 100+ boards over the past decade, and I have yet to hear a good answer for why the PCB part number is traditionally on an external copper layer, and the PCBA part number is on a silkscreen layer. To me copper is always "sacred" and should not have anything unnecessary on it, as this can screw up voltage isolation, RF performance, etc. But for some reason designs tend to have the bare PCB part number in copper instead of silkscreen. Why?

\$\endgroup\$
8
  • 4
    \$\begingroup\$ I'd guess because it's harder to wear off copper than silkscreen. \$\endgroup\$ – Hearth Jun 8 '20 at 17:15
  • 5
    \$\begingroup\$ For me, the PCBA part number is never on silkscreen but on a sticky label. You need to be able to assemble and label the PCBA variants. \$\endgroup\$ – Stefan Wyss Jun 8 '20 at 17:18
  • 2
    \$\begingroup\$ Who (besides you) says that it is traditionally so?.. The only sensible reason I can think of for doing it the way you describe would be to get different colours (contrast) for the two, but it is just a guess. And I don't agree with you on the "copper is sacred" point, If you're an experienced pcb designer then you should be able to manage keeping your tracks etc. out of the area where you have a part number. \$\endgroup\$ – Vinzent Jun 8 '20 at 17:18
  • 2
    \$\begingroup\$ A lot of PCBs don’t have silk screen. One large multinational I used to work for didn’t have any silk screen on any boards. This was not a cost thing either. We didn’t put any silk screen on 8 layer boards. When you put components as close together as the DRC would allow the designators start overlapping such that it is unclear which capacitor is C73. What we did was make a separate document for assembly where we put all the designators in a clear manner. \$\endgroup\$ – user110971 Jun 8 '20 at 17:21
  • 2
    \$\begingroup\$ Sometimes even if you have silkscreen, you want the prototype ASAP and ask the fab house to omit silkscreen and save a day turnround. \$\endgroup\$ – Brian Drummond Jun 8 '20 at 20:23
41
\$\begingroup\$

Copper etching is a very early step in the PCB manufacturing process. Etching the board number on the copper layer allows identification of the board at all subsequent stages. To omit it would risk confusion due to lack of a board identifier.

\$\endgroup\$
5
  • 2
    \$\begingroup\$ Okay thats an interesting point, didn't think of that, but then again; why would you need to identify the PCB at later stages in production? all the places I've worked the production was so streamlined that different pcb's didn't get mixed in a way so that it would make sense to mark them. \$\endgroup\$ – Vinzent Jun 8 '20 at 17:26
  • 5
    \$\begingroup\$ @Vinzent no quality control between steps? Quality control is, as far as I know, at least partially manual process in many factories, and where are people, there are mix-ups. \$\endgroup\$ – Mołot Jun 9 '20 at 8:39
  • 5
    \$\begingroup\$ @Vinzent I suspect the practice started – and was much more important – when production was nowhere as streamlined as it is now. Think stacks of boards waiting for the next step. \$\endgroup\$ – TripeHound Jun 9 '20 at 10:53
  • 1
    \$\begingroup\$ @TripeHound Absolutely. I've worked briefly in a prototype-house and batches under 50 often weren't automatically tested at all. All manual labour, and manual labour is never as streamlined as you want it to be. Especially back then (roughly a decade ago). The further back you go in time, the more important it was. \$\endgroup\$ – Mast Jun 10 '20 at 11:30
  • 1
    \$\begingroup\$ Rob: "What are you doing up?" Bucky Katt: "I'm on mouse patrol." Rob: "But we don't have mice." Bucky Katt: "We don't have mice, because, I do mouse patrol!" The factories don't have problems like that, possibly because they label the boards first step. \$\endgroup\$ – Harper - Reinstate Monica Jun 10 '20 at 17:46
32
\$\begingroup\$

I do a lot of multi-layer boards and the board reference number plus layer name gets put into the copper on all layers plus, there is a drawing accompanying the job that states the layer stack up to make sure that the bare PCB is made correctly. No chance of screw ups. If there is enough room on the PCB (say with 4 inner layers), there will be 4 distinct places on the board that if you shine a strong light through you will see the internal numbers. You can therefore inspect the layer stack to see it has been built correctly.

I'm not saying that there aren't other reasons but these are mine.

\$\endgroup\$
2
  • 2
    \$\begingroup\$ This is a good response and I totally agree that it is extremely necessary to have both board reference number and the layer stack up number, specially on very complex multi-layer double-reflow boards. In the company were I worked lastly, the board design rules provided to have a lot of drawing templates according board dimensions, scoring and for their panelization; and all these templates had very rigid rules providing the location of board reference number and layer stack up number. Having a set of drawing templates greatly helps the pcb designer. \$\endgroup\$ – barrow Jun 8 '20 at 22:51
  • 3
    \$\begingroup\$ +1 for this. By the same token, you should also have registration targets on all layers too, again as a quick check that the multilayer assembly went together correctly. \$\endgroup\$ – Graham Jun 9 '20 at 12:03
15
\$\begingroup\$

My company started designing PC boards in the early '80s. These were single-sided boards with NO solder mask or silkscreen. The only permanent location for the board number and company information was on the solder-side, in copper.

Even though we now design double-sided boards with solder mask and silkscreen, we still include board number and company info on the copper-side layer. We also include that information on the component-side layer as well, room permitting. And the silkscreen layer, of course.

\$\endgroup\$
12
\$\begingroup\$

I asked this same question years ago earlier in my career. The answer I got was that the copper layer usage for the board number was more permanent than silkscreen. In other words it was harder for someone to scrape off the copper number text than it was for someone to remove the silkscreen.

Some of the intention of more permanent board markings, I was told, was to make it easier to see if some unauthorized person or company was modifying your hardware somehow and selling it as their own product. A scraped off copper area on the board would be much more obvious than a silkscreen that was removed by some solvent.

\$\endgroup\$
1
  • \$\begingroup\$ That was a possible reason. But who would do that nowadays?. Traditions die hard. ;) \$\endgroup\$ – Fredled Jun 8 '20 at 22:58
0
\$\begingroup\$

It's better to have the BOM sticker (with revision) on a sticker, never know if you are going to have two alternatives :)

If you are cheap you might skip the silk and have the PN on copper.

\$\endgroup\$
2
  • 4
    \$\begingroup\$ I can't tell you how many times I've seen stickers just fall off, though. From boards in industrial machines, to computers and home appliances, the stickers just aren't reliable. It can be due to high heat, extreme low temperatures, age, bad stickum, spillage of solvents or lubricants, or placement over components, they really aren't as reliable as other methods. Stickers are useful, but shouldn't be the sole source for identification. \$\endgroup\$ – computercarguy Jun 9 '20 at 19:25
  • \$\begingroup\$ There certainly are sticker materials that would be reliable for applications like computers and home appliances and there are standard tests to verify it. On cheap boards the BOM stickers would be of the cheapest type though and only expected to last through the manufacturing process to not add cent to BOM cost. Sometimes stickers are safety critical and expected to last even in various industrial applications. \$\endgroup\$ – Ralph Jun 10 '20 at 20:08

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.