Potential cost savings from eliminating vias

Design and Layout
1

I’m designing a simple two-layer PCB (35mm x 25mm) and can potentially complete the layout without any vias. I’m curious to know if eliminating vias from my PCB design can potentially provide some cost savings. Is it worth the effort to design the board without vias, or are the potential savings worth it?

1 Like
2

When it comes to drilling vias and other through-holes, here’s a breakdown of how drilling costs are calculated for vias and through-holes:

  1. Initial setup time – Mounting the board onto the drilling machine.
  2. Drilling time –The time the board spends on the machine, which depends on the number and size of vias as well as the frequency of bit changes.
  3. Board Removal – Unmounting the board from the machine, which remains consistent no matter the via quantity.
  4. Post-Drilling Plating – Adding plating to through-holes, also a standard cost.

While setup, removal, and through-hole plating costs are consistent regardless of via count, drill time does increase with the number of vias and the complexity of the drilling. Reducing via count or using larger hole sizes can cut down on wear and bit changes, but for a simple board, this may not significantly affect costs.

Additionally, if your board has unique shapes, “mouse bites,” or other features for panelization, these add routing time on the drilling machine and can be a primary cost factor. Using V-scoring (v-scribe) for singulation can help avoid these extra costs.

1 Like
3

While it is possible to estimate the cost of using vias, it is important to remember that this is only a part of the total cost equation. Suppose that the circuit uses a simple surface mounted MCU with a clock frequency of say 50 MHz, it becomes strongly advisable to use a GND plane on the bottom of the board to keep the EMC issues in check. Since all the components on the top side of the board to avoid too many splits in the GND plane, vias become unavoidable. If the routing is now done using the techniques needed to minimise EMC issues, the cost saving is not from removing the cost of the vias in your PCB, rather it is that it does not cost you a fortune to comply with the EMC regulations.

Routing the board without vias may be possible; but if it compels you to add extra components to keep within the EMC limits the cost saving of no vias is likely to be more than offset by the cost of the extra parts you needed for compliance.

In the end it really comes down to the circuit and what may be required for it to meet your own target performance and also that needed by the regulatory authorities. It is of course possible for single-sided boards to comfortably pass all the requirements expected of them, but there are many circuits for which this is a simple impossibility. If your design falls into the category where you do not need vias, that’s great, just be careful that you don’t compromise your design for the sake of trying to save what is likely to be a small sum of money and end up having to design it twice.

4

In the past, PCB manufacturing costs were often directly tied to the number of vias or hole sizes on a board. However, this pricing model has largely been phased out, and most modern board shops don’t charge per hole for standard designs. That said, there could still be additional charges if your design includes an unusually high number of holes, such as a pattern resembling a plastic breadboard. For typical boards, though, via count alone is unlikely to significantly impact costs. Keep in mind that pricing policies may vary slightly depending on the manufacturer, so it’s worth checking with your specific board shop if you’re concerned about costs.

2 Likes
5

If I am understanding this (and earlier comments on other threads from @steve.carney ) correctly, then the variable cost of drilling – even the wear on the bits themselves – is small enough that it usually doesn’t affect pricing.

But would skipping vias entirely (and therefore the whole process step) be meaningful? Or is that strange enough that the resulting custom handling would offset the savings?

I suppose there is a similar question about layers like silkscreen or solder mask or even etching if you can keep plane layers truly unbroken other than connecting vias.

1 Like
6

If layers 1 & 2 don’t need to be connected it’s really just a single sided board and no reason to even have vias. If the thought is to connect 1 & 2 using some type of edge plating that would be considerably more difficult/expensive than using vias.

1 Like
7

I think some information is missing, technically a 2-Layer PCB needs holes (plated holes if only SMT components, non-plated holes use is possible if SMT+THT components are used). I see 3 different cases :

  1. 1-Layer PCB VS 2-Layer PCB, same dimensions : 2-Layer CCL should be more expensive than 1-Layer CCL, hole drilling, deburring, desmear, copper plating, AOI solder mask processes extra costs. —>
    2-Layer PBC should be more expensive.

  2. 1-Layer PCB VS 2-Layer PCB, 2-Layer PCB smaller : Same assumptions as 1) but the size reduction can make the 2-Layer PCB cost effective. So it also depends on the panelization parameters (% of the panel use) of the two designs.

  3. NPTH 2-Layer PCB VS PTH 2-Layer PCB, same size : PTH vias size smaller, copper plating process extra costs for the PTH PCB —> PTH PCB should be more expensive.

(Assumptions are made without consideration of manufacturing yields nor volume effects)