I learned about electronics and through-hole PCB layout in the 1980s, which I never actually put to use at the time. Back then, the design rules as best I can recall allowed for .010" clearance between traces/pads and if I recall correctly, typical trace width was .014"; when combined with pad geometry, this allowed for one trace between pads of a standard DIP package (.100" pin pitch). I am now working on a project, for which I am ordering bare through-hole PCBs I will assemble/solder by hand. I have just completed my design in KiCAD using the default rules. The traces look much finer than I have been used to for through-hole designs, more in line with surface-mount. The design is basically integrating an Arduino with some hall sensors, so no significant currents/voltages. Do I need to be concerned with trace widths? Should I have used different rules given that I will be hand-soldering the boards? If so, where would I find specific guidance on this?
Except for controlled-impedance nets, traces should generally be as wide as practical.
This will improve manufacturing yield on the board, and will make the board easier to repair.
It will also reduce voltage drop, and increase current handling, although those are rarely a consideration on DIY boards.
The default KiCad design rules are needlessly tight, IMHO.
Well, of course you should pay a bit of attention to all aspects of your PCB design, and that includes track width.
PCB’s mostly have digital signals these days, and for digital signals a narrow track width is better (contrary to 3Dog’s statement). Digital signals need a GND plane for EMC concerns and signal integrity, and a thinner track reduces capacitance. But there are limits, as with anything in life. One limit is current handling capability. A 0.25mm wide track can already handle 850mA (Based on 10 degree celcius temperature rise.) That’s much more then for any normal digital track, so that is not an issue in this case. A track of 0.25mm wide and 100mm length (35um copper thickness) has a DC resistance of 0.18 Ohm (Use KiCad’s built in calculator) This resistance is not a concern for digital signals, but it may be important for analog signals or for power distribution. For analog signals and power distribution, capacitance is also less of an issue. (distributed capacitance is even a positive side effect for power distribution).
Very narrow tracks do become more difficult to repair, but when they are covered by soldermask, they are quite robust and not easily damaged in the first place.
Then there is manufacturablility. A lot has changed in the last 20 to 30 years. I think KiCad’s default is 0.2mm. This is just fine for (most) multi layer PCB’s, but it’s nearing the limit of the cheap PCB pooling services for dual layer PCB’s.
Design rules from 3 big KiCad Sponsors:
- Aisler has 0.2mm as it’s minimum
- PCBWay quotes a minimum of 6/6mil ( 153um)
- NextPCB also has default 6/6mil rules for their pooling service.
- OurPcb is also a KiCad sponsor, but I get lost on their website and can’t find their rules for dual layer PCB’s. Apparently they do have other rules for single layer PCB’s, and that is becoming a bit unusual these days.
I like to be on the safe side and 0.25mm wide tracks are likely easily compatible with nearly any PCB manufacturer.
Multi layer PCB’s, are generally made on a more precise process. sometimes there are different rules for inner and outer layers. and when you do other things such as HDI, flex or IMS or other, then you should certainly check with your PCB manufacturer first. It’s also common to have different prices for different rules. (I.e, as a dual layer PCB has fine tracks, it must be made with the same (more accurate / expensive) process as the multi layer PCB’s.
The existing IPC (standard) rules and guidelines of the factory are determined by their technological capabilities and they adhere to IPC to a greater extent