PCB Drawing Parameters, Metric Or Imperial?

[The Doktor]

I'm designing my 1st board in KiCad, and wondering what measurement system to use? I had assumed metric, as most component spec sheets don't even show temperatures in °F anymore, and manufacturing is much less centered on the USA than it used to be. But now I'm not sure. Seems many PCB houses list design rules for track width/spacing in mils only. And most components I'm planning to use have their lead pitch in "Imperial Metric" units (2.54mm, 1.27mm, .635mm).

I'm a hobbyist with no professional future in PCB design. Will mostly be designing fairly simple things like nixie/numitron clocks and various small AVR/ESP8266/ESP32 based gadgets. Both through-hole and SMD will be used. What is your suggestion on which system to use? Also, any suggestions on design rules that will work at the majority of the cheap PCB houses?


Thanks
Ed

[asmi]

AFAIK Chinese fabs use metric drills, so if you specify imperial hole sizes they will pick the closest metric.

[electrolust]

Which doesn't matter. If you use standard hole sizes, drill sizes are wire gauges, and again they will pick the closest.

And holes cannot be drilled to within even the tolerance of conversion error, neither location nor diameter.

I use standard dimensions because it's easier for me to reference the components with the standard footprints.

[chris_leyson]

Either metric or imperial doesn't matter. I prefer metric because I've been using it for so long. Use the the units you find easiest, mm or mils, 1mil=25um or 1mm=40mil near enough.

[oldnewb]

There are no strict conventions when it comes to PCB design and units.  Draw your footprints using whichever units the manufacturer used in the part's data sheet.  Draw your board using whichever units you're most comfortable with, unless there's a good reason to pick one over the other (e.g., enclosure or mechanical assembly considerations).

You're likely to end up using both imperial and metric units together in nearly every design, which leads to minor conflicts like unaligned snap grids (ugly trace routes), etc.  It can be irritating, but not a show-stopper.

[David Hess]

I prefer mils and therefor inches simply because I find mils to be more convenient for typical printed circuit board track widths and clearances.  I would rather write 4 mils than 0.1 mm everywhere.  And most components are centered on mils in one way or another.

Plus, I get to taunt the metric zealots.

[nctnico]

I'm a hobbyist with no professional future in PCB design. Will mostly be designing fairly simple things like nixie/numitron clocks and various small AVR/ESP8266/ESP32 based gadgets. Both through-hole and SMD will be used. What is your suggestion on which system to use? Also, any suggestions on design rules that will work at the majority of the cheap PCB houses?

Use what measurement system you are using. However for most datasheets use the metric system nowadays. What will work for most PCB houses without extra cost is 0.15mm wide traces, 0.15mm clearance and circular pads which are 0.25mm larger than the hole. For most of my boards I use 0.25mm traces.

[Mattylad]

It doesnt really mater which you use when designing your board, the distances are almost the same
However, I'd reccomend setting all your drill sizes in 0.05 increments and not using thou.

Why? Because as far as I am aware the fab houses all use metric drill bits now.

[montemcguire]

One good way to think about this is that your final Gerber data will be rounded with relatively high resolution to either an inches or mm measurement system, but your CAD system can use whatever dimensional system to define the elements you're placing on your PCBs. So, you can specify components and traces using whatever system you choose, and at the end of the day, it will all get rendered and rounded to some number of digits of accuracy to the final Gerber representation units chosen by your rendering software.

It's important to keep in mind that Gerber RS274X provides a _lot_ of resolution, far greater than any real PCB manufacturing process can live up to. So, starting with Imperial measurements and rendering metric will not result in any precision loss at all.

I use Eagle, and by switching the grid, I can use both systems on the same project at different times with full accuracy, since the internal representation of all dimensions is accurate enough to store far more precision than one could ever expect from any manufacturing system. And, that ultra-accurate floating point representation is then rendered down to a Gerber of even less resolution, which is still far more precise than the PCB that I expect to be returned to me by manufacturing.

These days, the controlling dimension for most components is Metric, and the design rule parameters for more than a few PCB fabricators are Imperial (mil) units. I recommend using Metric units when these are the controlling dimensions, and then designing the actual layout using whatever system you're most comfortable with. If you're trying to go right up to a PCB house's fab limits, and they specify these limits using mils, then lay your board out using a mil grid. If your board house uses design limits in metric units, use a metric grid or metric specified drills and traces so you can get right up to the limits of their process. If you're not interested in running right up to the process limits, choose some other grid, perhaps Imperial or metric, but scaled so that you accomplish the circuit design goals that you need to make your PCBs work the best.

I used to think that the choice of units was a critical problem, but the sane answer is to define library parts using the system that the datasheet uses, and lay out your board according to units compatible with the PCB process limits you need to work within.