Continue to Site

Welcome to

Welcome to our site! is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

Do vias have solder mask over them?

Not open for further replies.
Taking the question literally, you'll find both variants in commercial PCBs, and I'm sure you already know about. Thus I assume, you actually meaned to ask a slightly different question.

IPC-2221A mentions tenting of vias as a way to protect them against process solutions during soldering and cleaning. It also specifies maximum finished hole diameters of 1.0 respectively 0.65 mm for tented vias.

Halfside or incompletely tented vias are inacceptable, because they can't be suffciently cleaned during PCB processing and are vulnerable to corrosion.

I usually opt for open vias with a reduced soldermask opening. They are available as test points and for prototype hardware fixes.
Unmasked vias are used for in-circuit testing. As mentioned, they are also good for probing during debug/trouble-shooting and for making circuit modifications (cut and jump from a via rather than the component).

Either way, had countless number of boards made with both covered and uncovered vias, dosn't make a difference IMO.

If board have power tracks in which solder finish is required, pehaps a mask over vias may be not a good proceeeding, due solder blob could overflow across neighbor vias, short-circuiting them.


Many PCB Manufacturers recommend open vias (non tented) since tenting may leave some chemicals trapped inside the via and cause some long term reliability issues.
I typically leave a slightly negative solder mask expansion so they can be used as test points. See attached image:


I typically leave a slightly negative solder mask expansion so they can be used as test points. See attached image:
That's the same thing I addressed with "reduced soldermask opening". It e.g. allows a via to touch a same net pad and still have sufficient soldermask feature between pad and via opening.

*unmasked vias can be used for ICT ( probing) purposes.
*masked vias can be placed very near to component pad with out causing solder oozing through via
* if no probinng requirement I prefer masked via

Not open for further replies.

Part and Inventory Search

Welcome to