Until the past year, the tightest PCB trace separation I have had to use is 5 mils [0.13mm]. Typically I try to use 8 mils [0.20mm] or 10 mils [0.25mm] if possible to reduce PCB costs.
I recently did a board that required 4-mil [0.10mm] minimum trace separation. Many PCB fab houses consider 4 mil traces with 4 mil gaps between them (i.e. 4/4) to be a standard technology.
Pad-to-Trace separation needs to take into account mask registration. Everyone who creates an SMT padstack thinks about mask registration when they make the soldermask openings extend 3 mils [0.08] mils beyond the copper on pads. This way if there is 3 mils of registration error between the mask and the copper, we can still be confident we will not have soldermask on the pad. This is important because mask on the pad can cause assembly defects. The pad-to-trace separation needs to be at least the mask opening on the pad (x) plus the mask registration tolerance, usually 3 mils. 3-mil mask openings (x) and 3-mil tolerance means minimum pad-to-trace gap must be 6 mils.
This registration issue is worse when a diagonal traces passes by the corner of a rectangular pad. The separation between the copper pad and the edge of the soldermask opening here is the hypotenuse (d) of the lateral opening (x). If we are using 3 mils of opening, that’s sqrt (3^2 + 3^2) = sqrt (18) = 3*sqrt(2) = 4.24 mils. This means if the pad-to-trace spacing constraint is set to 4 mils, a trace passing by the corner can be partially exposed without any registration error.
Minimum mask width becomes an issue in pad-to-pad spacing. There must be at least 4 mils of mask (m) between two mask openings to guarantee mask is deposited properly. If the mask is open 3 mils (x) beyond copper pads, this means pads connected with a trace must be 3 + 3 + 4 mils = 10 mils apart to guarantee mask deposition between them. If no mask is deposited, solder paste could flow onto the trace resulting in insufficient paste on the pad.
I am interested to hear if any CAD software packages support DRCs based on mask-to-copper separation. This would be especially useful for the hypotenuse problem. If you set the copper spacing based on the worst case of a trace passing by a rectanuglar pad’s corner, the separation needs to be sqrt (2) times what it needs to be for lateral spacing. Without a mask-based DRC rule we have set the separation to the hypotenuse value, clean up DRCs at pad corners ignoring other DRCs, and then set the contraints back to the lateral value.
To allow closer copper-to-copper spacing of pads, you can order PCBs with 2-mil soldermask registration tolerance. It’s more expensive, but this extra 1 mil of accuracy buys 2 mils of decreased separation because it allows 1 mil less of mask opening on each side of the pad plus one mil less tolerance to account for. You have to take care, though, not to use the padstacks with 2-mils of mask opening on boards fabricated with standard 3-mils of mask registration tolerance.
Contract manufacturers (CMs) typically have DFM software that checks for soldermask clearance and width issues. A DFM report from a CM is a good final check.