Pad size for 0.05" pitch connector?

Community PCB Design
1

Hi there,

I’m trying to build a library part for a Samtec SMS connector which has 0.05" pitch leads on it. The connector is the SMS-106-01-G-S. It is a single row micro socket strip which you can see here:

http://www.samtec.com/technical_specifi … series=SMS

Samtec recommends a drill size of 0.031" but when I place the pads for my package with the default “Auto” diameter, the pads end up touching.

My question is what is the minimum pad diameter that is supported by BatchPCB? Is there a minimum copper spacing between pads? Is there a minimum copper width for the pad?

Thanks, Shareef.

2

8mil spacing and 8mil width is the minimum. This includes pads and spacing between the pads.

http://www.batchpcb.com/index.php/Faq#W … d%20limits

3

If you use a 28 mil (0.028") drill vs 31 mil (0.031"), then the distance from one hole’s edge to the next hole’s edge is 22 mils (50mil - 28mil). Because an 8 mil gap is required by BatchPCB, that means that the width of the pad’s ring is 7 mils. In other words the pad’s diameter is 42 mils (28 + 2*7). You will have to change EAGLE’s restring minimum from 10 mils to 7 mils. This may or may not work with BatchPCB. An alternative is to use an SMD part instead of through-hole.

4

That was a much better answer than mine, but I’ll add… I don’t think the width of copper around the hole is limited in size. The gerber treats the pad as a full copper spot and then drops the hole on top of it.

One of the gerber experts can really answer this, but I don’t think the line around the hole is considered an individual line, rather than a larger copper blob with a hole dropped on it.

amirite?

5

If you look at the gerber output, you will see a “flash” that is the diameter of the pad. In the drill file, there will be a corresponding “hit” for a drill bit in the center of that pad. During manufacturing, the board is etched with a full circle of copper, and later the hole is drilled, and then plated through.

The minimum trace/space requirements do not apply to this situation. They indicate tolerances in the etching process. Instead, manufacturers normally provide an “annular ring” requirement, which is the minimum copper width around the hole. This requirement accounts for x-y alignment issues, drill wander, and drill bit size tolerances.

Now, I have no idea how BatchPCB validates this parameter, as they don’t indicate an annular ring requirement.

6

Thanks a lot for the info guys, I’ll email BatchPCB and post the result here.

7

I couldn’t find out from Gold Phoenix’s web site (they actually make the boards for BatchPCB) what the rules are for annulus.

Another PCB board house, Advanced Circuits (www.4pcb.com) says:

–

Pad Size/Annular Ring

Pad size should be at least + 0.010" [10mil] over finished hole size for vias and + 0.014" [14mil] over finished hole size for component holes. This means the annular ring (radius of the pad) should be at least .005" [5mil] for vias and a minimum of 0.007" [7mil] for component holes.

–

So what I suggested before - using a 42mil pad with a 28mil drill would probably work (42-28=14). Using teardrops will help connect the trace to the pad if the drilling is a little off center. I think that there is a teardrop ULP.

8

Right, I’ve created a small breakout board with 42mil pads and 28mil drill size. It passes BatchPCB’s DRC checks so I’ll get it fabbed in my next run and report back the results.

Thanks for all the help.