Pardon some noob confusion. Seed studio has the following spec selection for PCBs:
Min Tracking/Spacing: 4/4mil 5/5mil 6/6mil
How does that translate into pcbnew design rules? First of all, a “mil” in common parlance is 1/1000 of an inch - why specify this in mils and everything else in mm? Do they really mean “mm” here, or 1/1000 inch (.0254mm)?
Also, even 4mm min track seems huge - the tracks on my PCB are 0.25mm. There is a major cost difference between these 3 options.
I must be missing something… what would the design rules look like for (say) the “6/6mil” option?
I sent a board just recently to Seeed’s Fusion service. It really is 6mil. No idea why it’s specified in mils. I used .306mm for most tracks, .55mm for power, and 0.153 only where I needed to. I think I still have 0.153 for all spacings, though.
Those mm values are rounded up to the nearest micron. Most people seemed to say 0.152mm = 6mil, but it’s actually 0.1524mm, and I was afraid of being flagged for below minimum if I had set track width or spacing for 0.152.
Here’s what I used in Global Design Rules. I didn’t really use net classes, but I probably should have. I could have specified clearance values that were suitable for each net class.
The PCB industry, and PCB layout tools, evolved and matured in places where the so-called “imperial measurement system” predominated. (Where I live, we usually shift the blame by calling it the “English system”.) The term “mils”, meaning 1/1000 inch, is deeply embedded in our minds, documentation, and software. Some of us gray-haired old men (GHOM) occasionally still use the term “thou”, for “one-thousandth of an inch”. The industry is moving at nearly a glacial velocity toward using millimeters as the default unit for all distances, but even where this has been proclaimed as the “official” standard the working folks still hang onto inches, mils, and thou.
So yes, when Seeed Studio says “mils”, they mean 1/1000 inch.
@Rene_Poschl gave you the pragmatic answer to setting the KiCAD global design rules: Set Preferences to “Inches” (there’s a handy button for this on the left-hand toolbar), enter the values for your global design rules, close “Design Rules” and switch back to millimeters. KiCAD’s internal calculations are done in nanometers(!) as I recall so the length conversions are carried out to about a dozen decimal places beyond what is significant.
At this time I estimate that the plurality of PCB fabricators provide boards meeting “6/6” rules (6 mil minimum trace width and 6 mil minimum copper-to-copper spacing) as their standard product. However, it may not be wise to design your board right at the edge of their capabilities. (That’s a GHOM speaking.) At the very least you should allow for the folks in purchasing who will locate a lower-cost provider who can’t consistently produce boards at the limits of your preferred supplier’s capability. I routinely set my global rules to 10/10 (mils), and deal with situations where that is not practical on a case-by-case basis. If your board will be manually assembled, hand soldered, or possibly subject to component removal and replacement due to experiments in the development effort, wider traces and more spacing is beneficial.
I have had some boards come back from the cheapo PCB fabs with 6 mil tracks nearly etched through, as well as deep scratches on the board (they claim to do 100% e-test, but that is clearly fake!). So 8/8 is probably a better rule if 6/6 is the claimed ability.
Fun fact: “mil” comes from the French “mille” meaning thousand. The French have the best words.
The board I just did was 14/11.5. Why? Because that is the largest I could go and still sneak traces through 100 mill spaced dip pads. The board designer also mislead me a little on future current needs. I felt with that much cushion the board could be made anywhere, even home brew in a pinch. In reality I had no need to go smaller so why do so?
A few fabs state their tolerances for over- and under-etching of traces but in general you don’t REALLY know what it means when they claim that 6/6 rules (or ANY minimum for trace/space distances) is within their capability. It could mean, “We won’t over-etch by more than 2.9995 mils.”, leaving just 0.001 mil of conductor from the trace that displays as “6.00 mil” in your layout software. Or it might mean that over-etching will be 1.5 mil or less - leaving at least 50% of a 6-mil trace intact.
But suppose you want to sneak TWO traces between the pads?
It sounds like a silly game but I also set the trace/space rules based on the geometric properties of components: what trace widths will pass between the pads of a passive SMT resistor or capacitor; how many traces can I run under the body of an SO integrated circuit, etc. And the game plays out in the other direction when I create a footprint: how large can I make the pads and still get a trace between them under a particular set of trace/space rules?
. Funny that every unit on the seed studio is mm except for this one.