I have done the following work on Net classes in KiCad, which is derived from what I wrote about IPC 2221 standard trace widths and Creepage and Clearance a while ago.
I have been doing some work on my ROV, where I am trying to make two lights for the front of the vehicle. I want these two lights to be as small as possible while still being fairly bright. I am looking to use a CXA1304-0000-000N00B440F LED in each light; these LEDs are 13.35 mm on a side.
The PCBs I am looking to use with it are designed to be barely larger than the LED itself; I am looking at circles of about 26 mm ⌀. Since space is at a premium, I am looking to reduce the track widths from the KiCad defaults of 0.2 mm track clearance and 0.5 mm track width. I normally use PCBway for my boards.
From the PCBway capabilities page, we get this information for their standard PCB capabilities:
| Feature | 1 Layer PCB | 2 Layer PCB | Multilayer PCB |
|---|---|---|---|
| Copper weights external Layers/ | 1, 2, 2.5, 3.5, 4.5 oz | 1, 2 oz | |
| Copper weights Internal layers | 0.5, 1 2 oz | ||
| Drill Diameter1 | 0.3 – 6.3 mm | 0.15 – 6.3 mm2 | |
| Minimum via hole size3 | 0.15 mm hole, 0.25 mm via | 0.15 mm hole, 0.25 mm via | |
| Via Hole-to-Hole spacing | 0.2 mm | ||
| Pad Hole-to-Hole spacing | 0.45 mm | ||
| Minimum track width and spacing | 1 oz – 0.1 / 0.1 mm (0.09 / 0.09 mm for BGA fan-outs). 2 oz – 0.16 / 0.16 mm | ||
| 2.5 oz – 0.2 / 0.2 mm 3.5 oz – 0.25 / 0.25 mm 4.5 – 0.3 / 0.3 mm | |||
| Minimum text height (silkscreen) | 0.8mm | ||
Information for PCBway PCB capabilities
PCBway KiCad Netclass information
I have taken the above table of information and made a Net Class called ‘PCBway minimum 1 Oz’, which looks like this:
| Name | Clearance | Track Width | Via Size | Via Hole |
|---|---|---|---|---|
| PCBway minimum 1 oz | 0.1 mm | 0.1 mm | 0.4 mm | 0.2 mm |
I don’t normally use copper weights other than 1 ounce (~35 µm thick), or more than 2 layers on a PCB.
Clearance is derived from IPC 2221 Creepage and Clearance using a conductor coading of B24 which allows a minimum spacing between traces of 0.1 mm for DC voltages of 0-16 VDC, and 16-30 VDC. For voltages above 31 VDC, that distance goes up from a minimum of 0.6 mm.
IPC 2221 standard trace KiCad Netclass information
In addition to the PCBway minimum mentioned above tend to use a fairly small selection of other track widths, depending on the maximum current required; these are derived from the IPC 2221 standard trace widths.
| Name | Clearance | Track Width | Via Size | Via Hole |
|---|---|---|---|---|
| Default5 | 0.2 mm | 0.5 mm | 0.6 mm | 0.4 mm |
| 1 oz – 1 A | 0.1 mm | 0.3 mm | 0.4 mm | 0.2 mm |
| 1 oz – 2 A | 0.1 mm | 0.7 mm | 0.8 mm | 0.6 mm |
| 1 oz – 3 A | 0.1 mm | 1.4 mm | 1.4 mm | 1.2 mm |
| 1 oz – 4 A | 0.1 mm | 2 mm | 2 mm | 1.8 mm |
KiCad Netclasses Board Setup
This is the above information in KiCad:
- Holes with a diameter ≥ 6.3 mm are CNC routed from a smaller drilled hole.
Min. drill diameter for 2- or more-layer PCBs is 0.15 mm - Smaller than 0.2 mm may incur extra charges
- Smaller than 0.2 mm may incur extra charges
- External conductors (Uncoated), between sea level and 3050 meters (Solder resist does not count as a coating)
- This is the Default KiCad track
