Solder mask expansion, slivers and dams: real fab numbers

Three numbers that decide what the mask looks like

The solder mask layer in your Gerber set is a negative: it draws the openings, and the fab coats everything else. Three numbers control how that layer behaves at the fab.

• Expansion (also called mask margin, clearance or annular ring): how far the opening extends past the copper pad on each side.
• Dam (also called web, bridge or segment): the strip of mask left between two neighbouring openings. On fine pitch parts it is what stops solder from running from one pad to the next.
• Clearance to other copper: the distance between an opening and a track or plane of a different net. If it is too small, the opening exposes copper that should be covered.

A sliver is a dam, or any other piece of mask, that is narrower than the fab can produce. Fabs do not try to print it. They remove it, and the result is one large opening where you drew several small ones. That is the main reason this topic matters: the board still gets made, but fine pitch pads lose the mask between them and nobody tells you.

How the numbers relate

The geometry is simple. If two pads are separated by a copper gap G and each opening is expanded by E per side, the dam left between them is:

dam = G - 2 x E

Eurocircuits builds its rules exactly this way, and the published values add up. For its DI (direct imaging) mask, the minimum mask annular ring is 0.030 mm and the minimum mask segment is 0.075 mm. Its minimum pad to pad distance is 0.135 mm, which is 0.075 + 2 x 0.030. The minimum track to pad distance, 0.090 mm, is the 0.030 mm ring plus a 0.060 mm mask overlap on the track.

OSH Park writes the same idea as an inequality on its stop mask expansion page:

(mask expansion) < (copper isolation) - (mask tolerance)

Its tolerance figure is 3 mil (0.0762 mm), which it says covers expansion, retraction and shift. With its 6 mil copper clearance on 2 layer boards, that leaves room for a 2 mil expansion and no more. On 4 layer boards the copper clearance is 5 mil, so the recommended expansion drops to 1.5 mil (0.0381 mm). OSH Park adds that you can keep 2 mil on 4 layer boards if you raise the isolation of copper pours and ground planes to 6 mil.

What the fabs publish

The figures below come from each fab's own design rules or capabilities page, checked today.

A few details sit behind the table.

Colour matters. Eurocircuits runs two processes. Green, black, red and blue are direct imaged, and white and transparent are photo imaged with reduced registration accuracy. The minimum pad to pad distance goes from 0.135 mm on DI to 0.330 mm on PI. JLCPCB shows the same effect on a smaller scale: black and white need 0.13 mm between pads instead of 0.10 mm. If you pick white mask for looks, check the fine pitch parts again.

Copper weight matters. At JLCPCB the minimum pad spacing for a mask bridge doubles from 0.10 mm to 0.20 mm when you go from 1 oz to 2 oz copper. Thicker copper means a taller step for the mask to cover.

JLCPCB allows zero expansion. Its capabilities page says the pad to opening ratio can be 1:1 since its June 2025 LDI upgrade. OSH Park also accepts 0 mil, and notes that the only cost is losing up to 3 mil at the edge of the pad when the mask shifts.

Some fabs resize the openings for you. An AISLER staff member explained on the AISLER community forum that larger openings on one customer's board came from AISLER's own opening adjustments, and pointed to a minimum mask width of 100 µm. If your fab does this, drawing a large expansion yourself stacks on top of theirs.

A worked example: 0.5 mm and 0.4 mm pitch

Take a QFN with 0.5 mm pitch and 0.25 mm wide pads. The copper gap is 0.25 mm.

• With a 0.030 mm ring (the Eurocircuits DI minimum), the dam is 0.25 - 0.06 = 0.19 mm. That clears the 0.075 mm minimum easily.
• With a 0.0508 mm expansion (the OSH Park 2 layer value), the dam is about 0.15 mm. Also fine.

Now a 0.4 mm pitch part with 0.20 mm pads, so a 0.20 mm gap.

• Eurocircuits DI, 0.030 mm ring: dam of 0.14 mm. Above 0.075 mm, so the dam stays.
• Eurocircuits PI (white mask), 0.100 mm ring: dam of 0.20 - 0.20 = 0 mm. The pads share one opening.
• JLCPCB, 1 oz, green: the 0.20 mm gap is above the 0.10 mm minimum. In black or white it is above 0.13 mm. With 2 oz copper it is exactly at the 0.20 mm limit.

The same footprint gets a mask dam at one fab and a gang opening at another, depending on colour and copper weight. That is why the fab and the finish should be chosen before the footprints are final, not after.

The matching settings in KiCad

KiCad keeps these values in Board Setup, under Solder Mask/Paste. They are global values, and footprint or pad settings override them. The KiCad 10 manual describes them like this:

The minimum web width setting is the useful one for slivers. If you leave it at 0, KiCad writes every opening as drawn and the fab removes the thin dams on its side. If you set it to the fab's minimum, the merge happens in your own Gerber output, and the DRC tells you which footprints are affected. Our KiCad 10 Gerber export walkthrough covers the rest of the plot settings.

A short check before you upload

1. Find the fab's minimum dam for the mask colour and copper weight you are ordering, not the default green and 1 oz.
2. Find out whether the fab expects openings at pad size or already expanded. Do not add your expansion on top of theirs.
3. For every fine pitch footprint, compute the copper gap minus twice the expansion and compare it with the minimum dam.
4. Look at the mask layer around the fine pitch parts. A row of pads inside one rectangle means the dams are gone.
5. Check vias near pads. If they are untented, their openings can merge with a pad opening and pull solder away from the joint.

Steps 4 and 5 are visual. Drop the ZIP into the PCB Tools Gerber viewer, show the copper and mask layers together and zoom in on the fine pitch parts. Then go through the guide to checking Gerber files before ordering. If the surface finish is still open, our comparison of HASL, ENIG and OSP covers the other side of fine pitch soldering, and common Gerber file errors lists the other problems worth catching before the order.

The online Gerber viewer zooms to pad level, which is enough to see the mask openings and the dams between them. To preview the same board in different mask colours, use the PCB render tool.

Sources

All sources checked on 22 October 2026.

• Eurocircuits, PCB design guidelines: soldermask
• JLCPCB, PCB manufacturing capabilities
• OSH Park, Understanding stop mask expansion
• OSH Park, KiCad design rule setup
• AISLER community, Solder mask expansion settings with Altium
• KiCad, PCB Editor manual (10.0)

Information in this article comes from the public documentation of manufacturers, standards bodies and software vendors as of the publication date and may have changed. Check current conditions with the company concerned before you order. Company and product names are trademarks of their owners; mentions are editorial, with no sponsorship or affiliate relationship. See the terms of use.

Share: LinkedInRedditX