6
\$\begingroup\$

Why is the tstop aperture around a pad larger than the pad itself? I would have imagined that it would be exactly the same size, or slightly smaller, so that the solder stays only on the defined pad. Would there be any reason to make it larger, or smaller?

enter image description here

\$\endgroup\$
9
\$\begingroup\$

The TStop layer is for solder mask, the thin coating that prevents copper on the board from being exposed except for the areas where desired.

The TStop layer leaves apertures slightly larger than the pads so that the copper is still exposed in case of misalignment when producing the PCB.

However, extreme misalignment can cause copper to be exposed by the wrong aperture and you wind up with a situation where two nets are both easily shorted by solder in the same aperture.

Misaligned solder mask

From Printed Circuit Design & Fab

Some PCB software will let you change the amount of pullback of the TStop layer, but ideally you should have some so that minor misalignment doesn't hide some of the pad, especially with fine pitch pads.

\$\endgroup\$
4
\$\begingroup\$

For additional details on this, Google for the terms "SMD vs NSMD".

In this case, the acronyms stand for "Solder Mask Defined" and "Non-Solder Mask Defined" pads.

In SMD, the mask opening is smaller than the actual copper pad, so the solderable area is defined by the mask. This is used on some BGAs for increased bond strength between the copper and the substrate.

In NSMD, the mask opening is larger than the copper pad, so it is the copper pad itself that defines the solderable area. This is used nearly everywhere else (and it is the default in Eagle), because it makes it easier to get a flat finished surface. Also, the copper area is slightly smaller, making it easer to route traces between pads.

\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.