Can’t seem to find a good answer to this…
2 layer board limits are 8/8/20…but…
On what size grid can traces/parts/etc be placed?
A person can design a PCB with traces/parts/etc placed on a 1mil grid. Doesn’t mean they’re going to end up on that 1mil grid every time.
So I guess the real question is…what is the repeatable positional accuracy?
I would assume that since the limits are 8/8/20, a 10mil grid is ok, even an 8mil grid would be good. What about a 5mil grid? What about that 1mil grid?
Keep in mind the dimension of 1mil - 0.0254mm. The P&P machinery probably has a tolerance a bit larger than that (“Pick and place equipment with a standard tolerance of +/-. 0.05 mm” - random pdf somewhere). Even if it didn’t, by the time the solder paste melts, the component is likely to shift around by more than 1 mil due to the forces acting on it. For reference, the finest pitch you’ll start to see becoming more common is an 0.3mm BGA. That’s just under 12mil. Positioning on a 1mil grid just doesn’t make particular sense 
The dimensions for traces and spacing (say the 8/8) are mostly there for the fab to give yields that work. If you go finer than those, you might get (more) broken traces or traces shorted to each other that shouldn’t be as a result of deficiencies in the etching process. That etching process isn’t strictly grid-bound, though. An arc trace on a board will still be extremely smooth even under a magnifying glass, but if that arc trace is too narrow it might have gaps same as would a straight line.
I don’t know what the tolerances are, but I suspect they’re well under 1 mil for relative positions (i.e. if a pad on one corner of your board is 100 mil from a pad on the other corner, that 100mil would vary negligibly - but relative to the panel it’s on they both might shift around by more than that, and once you start cutting the boards there’s an additional tolerance you’d have to deal with).
I know it doesn’t give you a satisfactory answer (and it would be interesting to know, if BatchPCB happened to be able to give this information - I suspect Laen (OSH Park) might be able to get more details, though), but in terms of designing run-of-the-mill PCBs, the question doesn’t typically arise.
Granted, I don’t do superfine pitch work or anything where I would need to move a component around by just a few mil for some reason, but 0.025" as the finest grid and 0.1" as main grid has served me very well. Most of the SFE boards I’ve loaded are on an 0.05" grid.
If you really wanted to set a lower limit in your app of choice, I suspect you would have to go with traceWidth+traceSpacing. That way you can draw parallel traces that don’t exceed the minimums and have plenty fine control over component positioning.
I hope it's ok for me to speak up on this forum, because I haven't used Batch PCB, but I've laid out dozens of very dense boards for our company with up to 500 parts and 12 layers and the boards were made by many different board houses.skimask:
Can’t seem to find a good answer to this…2 layer board limits are 8/8/20…but…
On what size grid can traces/parts/etc be placed?
A person can design a PCB with traces/parts/etc placed on a 1mil grid. Doesn’t mean they’re going to end up on that 1mil grid every time.
So I guess the real question is…what is the repeatable positional accuracy?
I don’t think the grid matters one bit. I never use one at all, except that my CAD has 1-mil resolution and no finer. Most board houses won’t charge extra until you get below 6-mil trace and space, so I usually stop at 6 or 7. Visiting one of the board houses we’ve used however, even 20 years ago, I saw a sample they did showing they could even do 2-mil trace and space! Under the microscope, you could see that the trace height (from the copper thickness) was almost as much as the width, and it was quite square, with the sides being vertical and the corners sharp! Just incredible. I have no idea how they could do such a thing. Although they would use less care in etching our boards with wider traces and more separation, they still started with the same photoplotter with the same accuracy. I can lay down two traces of 7/7, and the dimensions appear perfect on the finished product, not having a 7-mil slop or even a 2-mil slop just because we didn’t pay for the finer service. And to get maximum density, I also do not limit myself to 0°, 45°, and 90° either, but use any angle I need, and the finished boards do not show any staircasing. The traces are perfectly smooth. I think the pixel size on the photoplotter is 0.1 mil (0.0001"), which is less than a tenth of the thickness of 1-ounce copper. As you might have already figured out, I do not use autorouters, because they cannot get nearly the density I can get doing it by hand and routing while I’m placing parts.
Drilling is not as accurate though. Drilled holes have to start out bigger than the finished size, and the thru-plating and subsequent tinning reduces them to the finished size. So with the bigger drill bit and the fact that it can wander a bit before getting started and perhaps not go through the board perfectly straight to come out the other side centered on its pad, I always make the pads at least .020" bigger than the finished hole size. Also, I never go below approximately 1/4 of the thickness of the board for the diameter of the finished hole. So for example a .062"-thick board gets vias no smaller than .015", and their pads are no smaller than .035" diameter. A breakout on the side of a hole would be extra bad for reliability if it happens where a trace comes to the pad. You can do teardropping to help prevent this, but I think it’s better to just make the pad big enough to prevent breakouts from happening at all. Again, no grid.
If you’re doing SMT for automated assembly, the alignment of the solderpaste screen may not be perfect, but with the LPI soldermask being reasonably accurate and the fact that the surface tension of the melting solder has a strong tendency to pull things in to the center of the pad, parts don’t have to be placed so super accurately. There are some YouTube videos showing how after placement, parts get pulled in to perfect alignment when the solder is melted.
Ok, works for me…Working on a rather large project with a lot of SMT pieces/parts. Using 8/8/20 w/10mil traces, I just can’t get everything places and routed nicely on a 10mil grid. 5mils or less ends up being no problem, and it’s all about getting that last trace in between two parts and still keeping the PCB small enough to fit the case.
On a side note, using Eagle, I’m letting the autoroute cook on the PCB at 5mils. I don’t use the autoroute for the finished product of course, but if the autoroute can do 100% without any input from me, then I can be relatively sure I can get the job done manually…which is the way it should be done anyways…