I am working on a PCB design. 50k PCBs will be produced.

SMD components: 100

Through-hole components: 25

I need to minimize PCB size. There are no high-speed signals or sensitive signals in the design.

I have two options:

  1. Components on single-side PCB with multilayer (4 or higher) layout

  2. Components on both (double side) sides of PCB with 2 layer layout

I need to clarify which costs less in production.

  • 9
    \$\begingroup\$ You can probably use the online quote systems to get an idea of the cost for both options. Even though they may not provide the most accurate lowest price for larger quantities like this, they should be able to give you a hint. \$\endgroup\$
    – jcaron
    Dec 25, 2019 at 10:51
  • 2
    \$\begingroup\$ You might also want to consider the total costs for assembly. There the single-side PCB has a major advantage, as you can do it in a single SMD and THT process. Also be aware of that (from a technical view), the 4-layer multilayer is the better solution in terms of EMI design (RF emission & immunity). \$\endgroup\$ Dec 25, 2019 at 11:49
  • 3
    \$\begingroup\$ In my experience the premium for double sided mounting of SMT parts is not large. You should also consider 2-sided mounting on multilayer. You have a LOT of through hole parts, if there is a lot of area devoted to them consider a small multi layer board and a larger 1 or 2 layer board for the big parts. \$\endgroup\$ Dec 25, 2019 at 13:05
  • 1
    \$\begingroup\$ Peter has a good anwser regarding production costs. However I am not so sure about your options. A double sided layout may require more layers than a single sided layout. The best way to know would be to design both and get quotes - manufacturers rarely provide "guesses". You need to minimize your PCB size, but costs seems to be a more important target. You can make size smaller by choosing smaller components and you may have smaller SMD alternatives to your SMD components. Sometimes a smarter part can replace a lot of functions that are implemented discretely otherwise. \$\endgroup\$
    – le_top
    Dec 25, 2019 at 19:34
  • \$\begingroup\$ what about through-hole components on top SMD glued on the bottom all soldered in a single pass over the wave-solder machine ? \$\endgroup\$ Dec 25, 2019 at 23:10

1 Answer 1


PCB size is not the only cost consideration and you need to consider recurring costs vs. one time (non-recurring) costs (some of the non-recurring may actually occur more than once for a 50k run).

Note that using double sided techniques rarely (if ever) yield a PCB half the size of a single sided part - in my experience you may get one that is perhaps 40% smaller if it is given lots of attention.

The non-recurring costs associated with PCBs includes the cost of tooling and the cost of solder stencils (which really are not that expensive although with a run of 50k you may need to use new ones after a certain number of runs which is very specific to the actual PCB).

Also in this category is test tooling which does have a certain amount of volume costs (50k boards will require the test tooling to have a certain amount of maintenance).

Another non-recurring cost is the fabrication and assembly documentation; poor documentation will incur recurring costs as you will be constantly fielding calls from the assembler and the specifics of the PCB may not be as controlled as you need. I suggest using the guidelines from IPC-D-326 (which incorporates IPC-D-325).

Recurring costs are:


Number of layers

Size (panelizing can reduce this depending on the specifics of the PCB)

Number of drill holes (often forgotten but can be a major cost driver)

Size of drill holes (to minimise costs keep the aspect ratio - the thickness of the PCB to the diameter of the drill - no higher than 8:1 and no smaller than 0.3mm)

The quality of the material (in particular Tg) as identified from IPC-4101. If you have high via densities you will need a relatively high Tg or you risk breaking the via barrels; this is a very common 'gotcha' that can destroy yields at assembly (the bare PCB test will not pick this up as it will only show up post reflow - the time above Tg is critical).

The PCB class (as identified from IPC-A-600)


The assembly class as identified from IPC-A-610.

The number of passes through reflow and perhaps in your case selective soldering; basically there is a recurring cost for each process step required. You should also keep in mind that if a cleaning process is applied, it will normally be done for each pass through soldering.

The number of boards in a single panel; the more the better, in general (so you get more PCBs through for each process step although pick and place will have a higher cost but that is usually small compared to the gains from fitting more PCBs per panel).

Component density has an impact here as well; there will inevitably be some waste of components (usually the smaller parts) and the higher the density the higher that waste is typically.


An automated test will have a non-recurring cost for the implementation and the lowest possible recurring cost (apart from no test at all). In terms of cost, it increases as you go from automated -> unskilled test labour -> skilled test labour on a per unit time basis.

There are other issues but these are the main ones in my experience and there is no single (or simple) answer; it depends on the specifics of your PCB. In the past where I have had the space for a single sided unit I have had the design done for both single sided and double sided design (incurring another non-recurring cost at the design stage) for high volume applications and sent both for quotations and the result can often be quite surprising.

In one case (where the design was always going to be double sided due to space constraints), the overall cost of fabrication and assembly was lower (by about 20%) when I increased the layer count from 14 to 18.

This significantly reduced the via count and eliminated high aspect ratio drills (the lower layer count had aspect ratios of up to 12 - the higher layer count maxed out at 10) and had the serendipitous effect of enhanced signal integrity (as I was able to use single layer routing for the majority of high speed signals).

[The methods required to run high speed signals across multiple layers while minimising losses is beyond the scope of this answer - suffice to say they are quite involved and use up more space than would otherwise be necessary]

  • \$\begingroup\$ Do you have any examples of "surprising results"? \$\endgroup\$ Dec 26, 2019 at 18:58
  • \$\begingroup\$ updated with an admittedly always double sided board. \$\endgroup\$ Dec 27, 2019 at 10:16

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

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