Avoiding solder mask relief issues

October 6, 2016 , in Blog

What’s the problem?

solder mask relief
Solder mask relief (.004″ per side)

Solder mask relief is an area on the surface of the PCB that does not have solder mask — these locations typically surround SMT pads, through hole pads, test points and vias as a margin of error during fabrication. The default design rules in many CADs check for a minimum opening .008″ larger than the pad it is relieving — this comes out to .004″ of relief per side. In some cases, .008″ is fine; for example, when there is a large distance between SMT pads and/or other copper features, that default is sufficient. (see image below).

The solder masked distance between two nearby reliefs is the solder mask web (also known as the solder mask dam). There is a minimum manufacturable solder mask web measurement, and it depends on the solder mask color. Each color has a unique chemical composition that affects its ability to adhere to the board below a particular area size. Certain non-standard solder mask colors can affect the solder mask web minimum, price and lead time.

Solder mask web relief and web

Why and when is it a problem?

In many designs, large solder mask reliefs end up creating a solder mask web smaller than permitted. In more extreme cases, this can expose copper that shouldn’t be exposed. This happens often with traces, ground copper or SMT pads that have the minimum copper-to-copper spacing from other SMT pads.

exposed trace
Exposed trace

Solder mask web violations often delay entire board fabs due to poor solder mask adherence and, if not caught during a DFM (design for manufacturing) check, can lead to a number of issues. With too little relief, solder mask can contaminate SMT pads, making the board surface uneven and difficult to solder on. With too much relief, fine-pitched pads or tight components can suffer solder bridging during assembly.

If there are test point vias or electrical connection vias too close to the SMT pads, this eliminates the solder mask web entirely and gives liquid solder an opportunity to seep through the via during assembly, which can cause shorting or tombstoning on the opposite side of the board.

How can you fix it?

The best solution is to change your design rules file and decrease the solder mask reliefs to only .004″ larger than the pads they are relieving, leaving .002″ of solder mask relief per side.

large solder mask relief with no solder mask web inbetween

Design with one large solder mask relief and no solder mask web in between — because there is no solder mask between pads, there is high chance there will be a short between them 

Corrected design with with sufficient solder mask web in between solder mask reliefs

In addition to this, it is important to understand the implications of a specific solder mask color. See the chart below for what minimum web each color requires. 

Minimum solder mask relief chart

 

The latest PCB news delivered to your inbox.

Search Sign In
[[]
[[]
[").replace(/[]]
[").replace(/[]]
[?&]
[?&]
[^&#]
[^&#]
[name="email"]
[name="email"]
[w-.]
[w-.]
[w-]
[w-]