What via sizes for cheap PCB Fab houses


Noob here…

On a 2-sided board 3"x4" (2oz copper BTW cuz of some heavy currents / MOSFETS) to be produced by one of the fab houses recommended by pcbshopper.com

For my signal traces (500Khz highest, most in < 1 Khz) I would like the thinnest reasonable traces. I’m trying 6 mil (.153) and am trying to understand the appropriate drill hole and via sizes. Please help.

1. Are there “standard” drill sizes I should be aware of? Or, are these laser cut so that I can put in any size within a range and it will be done that size?

2. What are some recommendations for these track widths, clearances, and via sizes?

  1. Do some fab houses do better than others with certain combinations of clearance+track_width+via_size? How would I know?


I’m pretty sure that is all going to vary from fab to fab. The only way to know for sure is to check with whatever fab you are planing to use. Is this a prototype board or a production run with large numbers?


The KiCad default is safe. Push further to the claimed fab limits and you can expect problems


Beware that with thicker copper the fab min width/cleareances will change. At 2 Oz some fabs derate their specs to 10mils/10mils. At 3Oz they derate more.
You should ask the factory about these things.


Over the last 15 years or so I have dealt with at least a dozen different board fabricators. Every one of them supplied a board that met their advertised specification. Some were well within their specification, while others were near the limits of their specification. Around two years ago I believe there was a thread on this Forum where members commented on the performance and quality of various vendors’ products. (Or maybe it was on the “DIYAudio” forum?)



I have only had to use thinner than the default 10 mil on boards using BGA packages. As you push fabs to 6 mil and fine vias, the fab is going to get yield problems, which you are going to pay for, either in higher prices or by getting some bad boards


The board I most recently finished was done primarily with 20-mil traces and 15-mil spacings. In a few places I had to step down to 15- or 10-mil traces and 10-mil spacing. This board was about 100 SMT components (1206, SOT-23, and SOIC; plus a few through-hole connectors) and will be hand-soldered.



There is a PCB calculator which calculates temperature rise for trace width & thickness.

For vias bigger is better for current handling.
Alternative is to remove the solder mask (un tented vias?) and fill the vias with solder.
You should also consider multiple vias to divide the current.

If your application permits it:
Putting the wires through a hole in the pcb (for mechanical stability) and then soldering them directly to the copper a few cm further is very good for current handling. You should put some vias through the PCB on the place were the wire is soldered for mechanical strength. This way the copper wil not be ripped of the PCB when the wires are pulled. (This also works good for SMD connectors)


I have included drill sets within KiPadCheck, but I have not yet included a variety of algorithms that manufacturers might use to select the specific drill size from their set. Obviously, the manufacturer may specify something different, but the drill sets in KiPadCheck are:


I wouldn’t lose any sleep over trying to cover all possibilities. In the first place, if the PC board is fabricated by anybody living in the 21st century, you are buying the FINISHED hole size, which is a few mils smaller than the drill size that started the process. There are fairly accurate guidelines for how much smaller the finished hole will be, but it will vary from one vendor to another and depends on the details of their fabrication process.

As for the size mapping process, there seems to be two main algorithms. Some vendors fabricate the hole to the standard size that is nearest to your drawing’s requirement, while others sell you the next largest hole (if your requirement doesn’t match a standard size). About a dozen years ago I had a vendor who wouldn’t build my board until the hole sizes on my drawing matched his standard sizes - letting me decide whether a particular hole should be enlarged or reduced, if it wasn’t one of the standard sizes.