Board setup - design rules for Pcbway and other questions


This is my first time manufacturing a PCB, and I’m unsure if I’ve set up my constraints correctly. I’m planning to use PCBWay. Here’s what I’ve done so far:

And here are their capabilities:

Could you please verify if everything is set up correctly? here is also a link to their website: pcbway - capabilities I am not sure if it should be 0.15 or 0.1524? if I choose 0.1524 i get a lot of errors as most of the holes are 0.15…

Additionally, should I adjust any parameters in the “Physical Stackup” section? I’m planning to manufacture my PCB with 2 layers and include some SMD/TH components.

Another question is regarding the designation of F.Cu and B.Cu in the “Board editor layers”. I’m using copper fill on B.Cu for GND and GNDA, and F.Cu for signal and power.

should I change anything here?

Your help would be greatly appreciated.
Thank you!

A min annular ring of 0.15mm (pcbway spec) and min hole dia of 0.3mm (reasonable) means a min via dia of 0.6mm (not 0.5).

I would also recommend min track width of 0.2mm and min clearance also 0.2mm. I often use 0.25mm tracks when a layout is not tight.

You can do finer tracks/vias/holes when needed, but it may cost more.

Copper-to-edge of 0.4 or 0.5mm is reasonable.

Silk (text thickness and lines) should be 0.15mm min (not 0.08). 0.1524mm is 6-mil (0.006 inch) and that is a holdover from US standards being 6-mil min silk width. I have all my libraries set to 0.15mm and have never had a problem with pcbway or jlcpcb making boards. I like my silk text to be 0.64x0.64x0.15mm.

The stackup will affect your 3d renders (total board thickness and soldermask color) but that is not transferred to pcbway as they just get the gerber and excellon fab files.

Not sure what you are asking about the F.Cu/B.Cu. I have called them top/bottom copper for decades, not front/back. Sure, you can do ground planes on the bottom (you need a net-tie to connect GND and AGND) but you can also fill in ground on the top layer open spaces as well to add a bit more ground area for a bit less emi.

My setup:


thank you very much for the answer :slight_smile: it helped me a lot

1 Like

The “minimums” from any PCB mfg are exactly that. They are something you only use if you have no alternative. They should not be used as a “default”. So depending on the density of the copper runs I would use 0.3 mm as my minimum track width and I would double (or more) the minimum annular ring. This last suggestion is more for prototype boards and not production boards. A small annular ring will be difficult to UNsolder if you have to change a component or wire.