I have been using 10 mil trace with 10 mil spacing. The PCB vendors quote that they like traces down to 7 mil. But then I ran across a PDF showing how to fan out a QFP to get all the signals accessible. They use millimeters because the QFPs are packaged with 0.4mm or 0.6mm pitches.
They also make an argument that using a 0.05mm grid approximates mils, but mm allows you to route buses in between the vias and pads.
Should I be using mil or mm when I am routing a PCB?
While the metric system is arguably saner, those that have been doing PCBs for much longer than myself have are pretty adamant about using mils. I think it has something to do with the machines used by manufacturers. That being said, if you have a board house in mind, and they spec their capabilities out mm, then yea you'll probably get a neater routing by picking a grid that is "natural" to your components. Typically though, you're going to have a mix of parts that are mm and mil based, so you'll likely have a "grid mismatch" regardless. I pretty much always use a 25mil grid and things usually turn out "good enough."
I think the system used by the majority of your active parts is the system to choose. Older parts were all 0.1 inch pitch, but at least some newer parts have ball or pin pitches specified in mm. I'd default to metric because it's the world standard, but if you're manufacturing in the US, you might default to inches.
Tom at PCB Matrix advocates using metric exclusively, as the majority of high-tech parts are metric. I actually use both, in the same design sometimes, if I have a mixture of metric and Imperial parts. It doesn't really matter all that much with the software I use, as it can make connections off-grid, but I get neater results.
Use whatever is more convenient for you. It doesn't matter what units packages are defined in because any decent software decouples package definitions from layout and routing dimensions anyway. Use whatever metrics the datasheet uses when defining the package footprint, since that will minimize errors. Even then, I switch back to inches when defining the silkscree and documentation layers because that's what I can relate to more directly.
For layout and routing, use whatever you are comfortable with. I learned this stuff thinking in inches and mils, so that's what I use. I can picture 8 mils in my head, but I'd have to convert the equivalent in mm to get a mental picture. That's what computers are for. They are very good at multiplying or dividing by 25.4, so let them serve you, not the other way around.
When exporting files to a board house, I'd use inches. That seems to be more of the univeral standard, probably due to history. The board house's computers can multiply by 25.4 too, so those board houses that use mm internally won't be bothered. A few years back, some board houses wanted all input in inches, but I suspect that's no longer true today.
This question is a decade old, but still highly trafficked, so I figured it's worth adding my (more recent) insight as a PCB designer by trade (U.S.-based).
At this point, mils/inches are starting to feel somewhat obsolete for a handful of reasons:
If you are looking for your board to be compatible with all output formats, everywhere, then a 0.05 mm grid (or its multiples) is technically the objectively correct answer, as it's been agreed upon by dozens of organizations and will work without rounding for all outputs.
However, we're at a point where you can pretty much throw grids out the window unless you're going for visual appeal. Gerber X2 recommends 10nm or 1nm grids for all outputs, small enough that any routing grid is huge by comparison. When I'm doing HDL I usually place on a 0.05 mm grid (for assembly) then route with grid off since it serves little purpose.
That being said - if your components are aligned on a metric grid than your a routing grid can actually be useful (that is, a 0.1mm placement and routing grid means your tracks will connect perfectly with most newer component footprints, and go exactly between vias for BGAs).
In short, if you're seasoned at designing and used to mils, there's really not much motivation to change (though I was, and I did), especially on the hobby level. And everyone should certainly use what they are comfortable with. However, if you're just starting out, my recommendation at this point would be to learn to route in metric. 10 years ago I would have said it really doesn't matter, but the industry (currently a messy mix of both units) is slowly but surely moving toward metric only, so it's worth at least getting a feel for that.
For completeness, here are few exceptions I can think of:
Typically I place parts on a 25mil grid and route on a 5mil grid. For low density boards I can usually route on a 10-25mil grid.
When I route I have the traces snap to the mid-point of the pad so that traces end in the center of the pad for all components.
Brazil uses metric system but my layouts are in mils because because it is the most widely used.
I use mil, because that's what they use at the company I outsource the PCBs to.
I have the same opinion as Olin, since I'm used to think in metric I choose mm; if I were born in the US I'd probably go for mils. But I keep a conversion table for the most common sizes/distances at hand, so I don't have to make calculations every time. Oddily enough, my PCB fab requires some dimensions in mm, some in mils, so I'd have to convert either way. Even if not for that, you'll from time to time stumble upon values that need to be converted no matter what you choose. Why not pick the choice you're most comfortable with, then?
It depends on the parts you're using and the capabilities of the fabricator. If the fabricator is working with mils, then making the design on an mm grid may cause minor alignment issues. These issues though, are only a problem if you're really testing their clearance specifications. Even then, its unlikely to actually result in a non functioning PCB.
Personally, I use mils. The vast majority of my parts use mils for pin spacing specification. Mils also lets me think in terms of integers for things like wire width, clearance, and so on. And my manufacturer deals with mils anyway.
The PCB vendors quote that they like traces down to 7 mil.
No, it's not that they like it. It's just what they can support. So, for a particular board product, there is a limitation that trace and space must be 7mils or wider. Beyond that it's entirely up to you. So, as long as your spaces and traces are 7mils or more, you can use whatever grid you feel like using.
State of the art PCB software supports multiple grids at different areas in the circuit, with different spacing and different angles, including dynamic grid that follows the last trace endpoint and direction. But in any case grids are only aids for manual routing. Automated or semi-automated routing works at whatever design rule trace and space is set, and it doesn't use a grid at all.
