How does solder mask layer work?

What is soldermask and how does these layers work in KiCad?

Solder mask is physical substance applied to the physical board. There are holes in this mask which expose copper pads.

In KiCad (and other EDA) the graphical layer which represents solder mask is negative. Where there is graphics in this layer, the physical solder mask isn’t applied and there will be a hole in the solder mask.

There are two values for solder mask in Board Setup: clearance and minimum width.


IMPORTANT NOTE: always check your manufacturer’s recommendations. Most manufacturers can modify the mask layer clearance and bridge width to adapt to their processes. Use zeroes unless you need certain values and know the manufacturer can handle them.

The “minimum width” of the solder mask in the board settings means the physical solder mask, not the graphics in the layer. From the standpoint of the layer it means the minimum allowed space between graphic items.

Clearance (sometimes called “solder mask swell”) can be overridden in footprint or pad level. Minimum width is always global. Minimimum width is similar to a zone minimum width, although solder mask layer is negative. This means that if space between two graphic items in the F.Mask or B.Mask layer is smaller than the minimum, those items are fused together when gerbers are generated.

The reason is that manufacturers can’t guarantee that thin strips of physical solder mask substance stay in the board. It may peel off. Therefore that area should rather be left without mask altogether. For KiCad this means that when gerbers are generated the too thin space between graphic items in the layer is removed and the graphic items form a larger blob. Unfortunately we don’t see this when we edit the layout with pcbnew.

The result of “minimum width” setting of 0.15 mm together with < 0.15 actual mask bridge width can be seen here:

You should check your manufacturer’s recommendation for the minimum mask width (or “web” or “dam” or “bridge” as it may be called). 0.15mm or as low as 0.10mm are pretty common nowadays.

If you use the recommended value you normally shouldn’t worry about ICs having no mask between pads. They work well without it.

Footprint pads and solder mask

Normally there should be mask openings in copper pads of footprints. In KiCad each pad has layers enabled or disabled, including the mask layers.

Graphics in each layer has the same shape as the pad. Clearance value is applied to this shape.

Most often pads are Non Solder Mask Defined (NSMD). This means that the mask opening is larger than the pad and the copper shape defines the area where the pin is soldered. Sometimes Solder Mask Defined (SMD) pads are used. Negative clearance can be used for that.

Negative clearance isn’t enough if the mask opening is displaced compared to the copper or has different shape. In that case you can create a new pad and set Pad type to Aperture and set only the Mask layer selected. In the copper pad you should then deselect the Mask layer. Clearance values aren’t applied to aperture pads. These pads don’t have pad number or net, either, because they aren’t connected to anything.

Mask openings outside of footprints

You can draw directly to the mask layer of a board with the graphic tools. You can also write text. These have many uses:

  • Add mask opening to an edge connector.
  • Create uncovered strips on a copper zone which can be plated with tin. This is sometimes used with high currents.
  • A test point without a footprint.
  • Add text, like copyright holder and revision number.
  • Add a logo or other graphics.

On top of board body material this is less attention-getting than silk screen. Text or graphics which uncovers copper looks either cool or cooler, depending on the copper finish. Mask has much better resolution than silk and text can be smaller.

A board manufacturer has some problem with the solder mask

First, you should always plot both mask layers, even if you have one layer board. The physical board always has two sides anyways, even when the back side has no pads or holes in it. And if you leave the gerber out althogether it’s unclear whether you want to have solder mask or not. Then your manufacturer halts the order and will email you. The situation is different with other layers which are automatically interpreted as “doesn’t exist” if there are no gerber files for them.

Additionally, when you have something else than the most common situation - namely that you want to have both sides with mask and both sides have some mask openings for SMD pads and/or THT holes - you should always give a note to your manufacturer telling clearly what you want. That way you can avoid needless email conversations.

Without mask

If you want to have no mask in the back side you should cover the whole board area with graphics in the corresponding design layer. (At least that’s what normal logic says because the layer is negative.) Don’t forget to give a note, too.

A neat trick is to draw a zone (not just a graphic polygon) around the whole board and set the width to 0. When you fill zones, this will be filled, too, so that it covers the whole board area but nothing more, just like with copper zones.

Completely covered with mask

Some people have had problem with some (cheap Chinese) manufacturers when the mask layer gerber file is empty. This is the only logical way to communicate “cover with mask without openings” in Gerber standard, yet the manufacturer may wonder what you wanted. The first thing is to remember to give an extra note to the manufacturer.

If you want to be sure there will be no problems you can add something to the B.Mask layer on the board area. Some options are (see also “Mask openings outside of footprints” above):

  • Graphics or text.
  • Extra THT hole (footprint) for example to work as a stitching via.
  • Extra exposed SMD pad, for example a test point.
  • Select “Do not tent vias” option when generating gerbers (it’s not possible to choose individual vias to be uncovered).

Problem with mask openings fused together

The efffect of minimum width is explained above. It’s important to check the gerbers to see if it happens in wrong places. Removing thin mask strips between e.g. pads of ICs is predictable if the space between pads is very small. However, you should think twice if pads of two different components are too close, whether they belong to the same net or different nets. Obey the manufacturer’s recommendations for mask values and preferably move the problematic components farther from each other if possible to avoid mask openings between pads. The correct minimum clearance is more important if you feel forced to try smaller mask values. In case of doubt always try to communicate with your manufacturer.