A solder mask opening is the window in the solder mask that leaves a pad exposed for soldering. It is normally drawn slightly larger than the copper pad, the difference being the mask expansion (or clearance), so that mask registration error never covers the pad. Component makers often specify a few hundredths of a millimeter: TI’s land pattern for one QFN-style module calls for openings no more than 0.05 mm larger than the pad all around for non-solder-mask-defined (NSMD) pads, and mask overlapping the pad by at least 0.05 mm for solder-mask-defined (SMD) pads. The PCB solder mask opening requirements on the drawing should state NSMD or SMD per package, the expansion, the minimum mask web (dam) between pads, and the mask material and class.
| Item | Typical choice | Why |
|---|---|---|
| Pad definition | NSMD for most SMT pads and BGAs | Copper defines the pad; mask stays clear |
| Expansion | Small, from the part’s land pattern or fabricator’s rule | Absorbs registration error |
| SMD pads | Where the package maker asks for them | Mask defines the solderable area |
| Mask web between pads | Fabricator’s minimum dam, or gang opening if too thin | Prevents bridging; slivers peel off |
| Vias | Tented, plugged or open, stated per via type | Avoids accidental exposure |
| Mask material | IPC-SM-840 qualified | Sets the mask’s performance class |
What Is a Solder Mask Opening?
The area of a pad left uncovered by the solder mask. Solder mask is the polymer coating, usually green, that covers copper everywhere solder should not go; it prevents bridges, protects traces and insulates. Each pad that will be soldered needs an opening, and the shape and size of that opening relative to the copper decides how much of the pad the solder actually wets.
The opening lives in its own Gerber layer (top and bottom solder mask) and is drawn as positive shapes where mask is removed. It is a different layer from the paste mask, which defines the stencil apertures for solder paste; the two are often confused because both look like copies of the pads.
What Is the Difference Between NSMD and SMD Pads?
On an NSMD pad the copper defines the solderable area and the mask opening is larger than the pad; on an SMD pad the mask opening is smaller than the copper and the mask edge defines the solderable area.
| NSMD | SMD | |
|---|---|---|
| Opening vs pad | Larger | Smaller |
| What defines the solder area | Copper edge | Mask edge |
| Solder joint | Wraps the pad sides, strong | Sits on the pad top only |
| Pad size accuracy | Set by etching, accurate | Set by mask registration |
| Pad lifting resistance | Lower | Higher, mask holds the pad edge |
| Typical use | Most SMT pads, most BGAs | Some BGAs, large pads, thermal pads |
NSMD is the common default. AMD, for instance, suggests NSMD board pads for its BGA packages (AMD Versal PCB design rules for BGA). Follow the package datasheet when it says otherwise. TI’s land pattern for its TPSM82850x-Q1 module shows both: NSMD (preferred) with the opening at most 0.05 mm beyond the pad, and SMD with mask at least 0.05 mm over the pad edge, and it notes that mask tolerances vary by fabricator (TI TPSM82850x-Q1 datasheet, page 32).
How Much Solder Mask Expansion Should You Use?
Enough to cover the fabricator’s registration tolerance, and no more. Too little expansion lets misregistered mask creep onto NSMD pads; too much leaves no mask between closely spaced pads. Start from the component’s land pattern when it gives a value, as many fine-pitch packages do, and otherwise from the fabricator’s design rules.
The trade-off shows up between fine-pitch pads. With the expansion added on both sides, the mask web left between two pads is the pad gap minus twice the expansion. If that web is below the fabricator’s minimum dam, it will not hold; it lifts, flakes off or is removed in CAM. In that case either reduce the expansion, accept a gang opening across the row of pads, or check with the assembler whether bridging risk is acceptable. IPC-2221C includes a table of typical minimum mask clearances and dams (IPC-2221C contents, Table 4-15), and IPC-7352 notes that land patterns must account for mask clearance and registration (IPC-7352 contents).
What Is the IPC Standard for Solder Mask?
IPC-SM-840 qualifies the mask material, and IPC-6012 sets how the mask is accepted on the finished board. IPC-SM-840E covers permanent solder masks and flexible cover materials and assigns them to performance classes, T and H (IPC-SM-840E contents). IPC-6012F covers mask coverage, cure, adhesion and thickness in section 3.7 (IPC-6012F contents). Mask thickness is checked against the drawing when you specify it; if you do not, the fabricator’s process thickness applies.
A qualified material does not make the opening geometry correct; that still comes from your design data and the fabricator’s DFM review.
How Should Vias and Special Pads Be Treated?
State them separately, because a blanket expansion rule treats them wrongly:
- Vias: decide whether each via type is tented (mask over), plugged, filled or left open, and make sure the mask layer agrees. A via accidentally given a pad-sized opening next to a fine-pitch pad can steal solder.
- Thermal pads: large exposed pads under QFNs are often given segmented or SMD-style openings so the mask holds the copper and the solder does not float the part.
- Test points: give probe points a clear opening; mask on a test point causes false opens.
- Edge connectors and contacts: no mask over fingers or contact pads.
Our guide to tenting, plugging and filling vias covers the via options.
What Should the Mask Notes Say?
| Item | Example |
|---|---|
| Mask layer | “Openings per top/bottom solder mask Gerbers; do not modify without approval” |
| Pad definition | “NSMD unless noted; SMD on U5 thermal pad” |
| Expansion | Value used in design, or “per fabricator standard” |
| Dams | “Maintain mask web between fine-pitch pads where ≥ fabricator minimum; gang openings allowed on U1” |
| Vias | “Vias tented both sides except test vias” |
| Material and class | “LPI mask, IPC-SM-840 Class H, green” |
The fabricator will adjust openings in CAM to fit its registration and dam limits. Say which changes it may make without asking, such as uniform expansion changes, and which need approval, such as removing dams on a fine-pitch part. A free DFM check shows those changes before production.
How Can We Help?
QueenEMS holds a minimum solder mask bridge of 3 mil, so fine-pitch rows that need a dam between pads can usually keep one. Our DFM review lists every opening CAM would change, with the reason, before production. Send the Gerber files with the mask layers and any package-specific NSMD or SMD requirements; we price bare boards within 2 hours.
Conclusion
| Pad | Opening |
|---|---|
| Standard SMT pad | NSMD, small expansion per land pattern |
| BGA | NSMD unless the package maker specifies SMD |
| QFN thermal pad | Per datasheet, often SMD or segmented |
| Fine-pitch row with thin web | Reduce expansion or allow gang opening |
| Via | Tented, plugged or open, stated separately |
Take openings from the part’s land pattern, check that the dams survive, and tell the fabricator which changes need approval. Contact us with the Gerber files, mask requirements and quantities.
FAQ
What is a solder mask opening in a PCB? The window in the solder mask that leaves a pad exposed for soldering.
What should solder mask expansion be? Enough to cover registration error, usually a few hundredths of a millimeter; take the value from the part’s land pattern or the fabricator’s rules.
What is the IPC standard for solder masks? IPC-SM-840 qualifies the mask material; IPC-6012 sets acceptance of the mask on the finished board.
What is the difference between a solder mask and a paste mask? The solder mask is a permanent coating on the board; the paste mask defines the stencil openings for solder paste during assembly.
What is a solder mask dam? The strip of mask left between two adjacent openings; it keeps solder from bridging between pads.
Upload your files today · Free DFM check before production · Ship worldwide
Get your PCB prototypes in as fast as 24 hours. We handle FR4, Rogers, and hybrid boards, with standard builds up to 24 layers and higher layer counts subject to engineering review — free prototypes for 2–4 layer FR-4 boards, no minimum order.
Just upload your Gerber + BOM — we source every part, assemble, and inspect (AOI + X‑Ray) so you don't have to chase suppliers. PCB assembly typically takes 5–8 working days once all components are in stock. The confirmed delivery schedule is subject to your quotation.