Mask Clearance on Vias

[Marty L]

Saw something today I couldn't explain, one of the guys here using Pads 7.2 (I use an older version) had zero soldermask clearance around the StandardVia. Pad stack looked normal - i.e. the same as for pad stacks on through hole parts - and the through hole parts had mask clearance. Any suggestions on how to fix this?

[JimR-OCDS]

By zero solder mask clearance I take it to mean that soldermask will flood over the vias?

This because in the CAM output for solder mask, vias are not selected.


Jim

[Marty L]

Hi Jim,

The vias were there in the mask, just zero clearance - same size as the pad. The board shop likes at least .006 clearance, which there was on all other pads, just not the vias.

[Skip Yutkus]

A lot of designers use zero clearance on all pads, and instead specify the maximum a board shop can use when sizing the mask, (board shops all pretty much use what they need for their process), that way each board shop can use what they deem necessary. On vias I almost always cover the vias and allow tent busters, unless they will be used for test points. This minimizes chances for shorts or solder starvation when placed close to an SMT pad.

Skip

[JimR-OCDS]

Hi Jim,

The vias were there in the mask, just zero clearance - same size as the pad. The board shop likes at least .006 clearance, which there was on all other pads, just not the vias.

Marty,
you need to go into CAM in the soldermask set up.

Go into Options, and where it says, "Oversize(Undersize) Pads By," insert the number you want to oversize the pads by.

I use to just use zero clearance, but the vendors were increasing by 4 or sometimes 6mils.

I always want a 5mil min. solder dam between SMT pads and the vias they are
conenected to, so I add 4 mils so that I can see it.

However, I rarely have exposed vias anymore, so I just leave the vias unselected in the CAM setup.

Jim

[Marty L]

Thanks Jim, that's a CAM feature I haven't used before, sounds handy.