skimask wrote: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 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.
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.
