Solder mask is the permanent polymer coating that covers most of a printed circuit board while leaving pads and other selected features exposed. A good solder mask specification does more than choose green or black. It defines which copper must remain accessible, how registration tolerance is handled, where mask dams are required, how vias are treated and which performance standard applies.
This guide turns those requirements into practical design rules and fabrication notes. The exact minimums still depend on your board manufacturer's material, imaging equipment, copper thickness and registration capability, so use the values below as a framework for a fabrication-approved rule set rather than a universal capability table.
What Solder Mask Does#
Solder mask limits where solder can wet during assembly, protects conductors from handling and contamination, and provides electrical insulation between exposed features. IPC's Solder Mask Handbook also describes protection of laminate, holes and traces during fabrication, assembly and service.
It is not the same as conformal coating. Solder mask is applied during bare-board fabrication and remains part of the PCB. Conformal coating is normally applied after assembly to protect components and exposed conductors. Neither should be treated as a substitute for required creepage, clearance or environmental sealing.
Solder Mask Types Used on PCBs#
| Type | Typical use | Design implication |
|---|---|---|
| Liquid photoimageable (LPI) | Most rigid and multilayer PCBs | Supports fine openings and accurate imaging when the process is controlled |
| Dry-film photoimageable | Selected fine-feature or specialized processes | Film thickness and lamination affect coverage around copper topography |
| Flexible solder mask | Dynamic or flexing areas of flex circuits | Material must be qualified for bending; rigid-board mask can crack |
| Coverlay | Traditional flexible circuits | Mechanically formed openings need larger tolerances than photoimaged mask |
| Specialty mask | High temperature, high voltage, optical or chemical environments | Qualification and application-specific tests must be agreed before release |
For ordinary rigid boards, LPI is the default assumption, but drawings should still name the required qualification, color and finish. Flex and rigid-flex designs must distinguish flexible solder mask from coverlay and identify the bend zones.
IPC-SM-840 and Board Acceptance#
IPC-SM-840 is the qualification and performance specification for permanent solder mask and flexible cover materials. IPC's current standardization status lists Revision F. It addresses the material and its performance system; it does not automatically define every pad opening or artwork tolerance for your board.
Finished-board acceptance also depends on the applicable printed-board performance specification, fabrication drawing and agreed class. A useful note identifies the required solder mask material qualification and then separately defines artwork, registration, coverage and visual acceptance. Avoid writing “IPC Class 2 solder mask” as if one phrase completely specifies the coating.
For high-reliability, high-voltage, medical, automotive or harsh-environment products, ask whether additional adhesion, insulation resistance, chemical resistance, thermal cycling or electrochemical migration testing is required. IPC-HDBK-840 explains why not every application-specific property belongs in general material qualification.
Solder Mask Expansion#
Solder mask expansion is the offset between the copper pad boundary and the mask-opening boundary. Positive expansion makes the opening larger than the pad. Negative expansion lets mask overlap the copper and is used only for controlled mask-defined lands or special features.
A positive expansion compensates for registration error so the mask does not encroach onto a solderable pad. The correct value must cover the fabricator's imaging and layer-to-layer registration tolerance while preserving enough mask between adjacent pads.
Set expansion in the CAD rules by pad class or component type. Do not apply one inherited default blindly to BGAs, connectors, test points and large mechanical pads. Altium, for example, exposes expansion as a manufacturing design rule that can be scoped to selected pads or component classes.
Solder Mask Defined vs. Non-Solder Mask Defined Pads#
Non-solder mask defined pads
With a non-solder mask defined (NSMD) pad, the mask opening is larger than the copper land. The copper edge controls the solderable area. NSMD pads are widely used for BGAs because solder can wet the top and side of the pad, while copper dimensions remain controlled by the etching process.
Solder mask defined pads
With a solder mask defined (SMD) pad, the mask overlaps the copper, so the mask opening controls the exposed area. This can help retain mechanically vulnerable pads or fit a particular package recommendation, but it makes mask registration and adhesion more critical.
Follow the component manufacturer's land-pattern guidance and the assembler's process recommendation. Mixing SMD and NSMD lands within one BGA without a documented reason can create inconsistent solder volumes and joint geometry.
Minimum Solder Mask Dam#
The solder mask dam, web or sliver is the strip of mask left between two adjacent openings. If it is narrower than the manufacturer's process can reproduce, it may peel away or be removed during data preparation. That can merge openings that the designer expected to remain separate.
Ask for two different numbers:
- Minimum producible mask web: the narrowest mask strip that can be imaged and survive processing.
- Minimum guaranteed finished web: the width remaining after registration and process tolerances.
These are not interchangeable. Fine-pitch BGAs may intentionally use a gang opening when individual webs cannot be guaranteed. Decide that before release so paste design, inspection and solder-bridging risk can be reviewed together.
Registration and Mask-to-Copper Clearance#
Solder mask registration is the alignment of the imaged mask to the copper pattern and drilled features. The risk is highest where a small opening surrounds a small pad, or where an opening sits close to an unrelated trace.
Your DFM check should cover both sides of the tolerance stack. The opening must remain large enough not to cover the functional pad after maximum shift, but it must not expose adjacent copper at the opposite shift. For very fine features, provide the actual pad, opening, spacing and registration assumptions rather than only a nominal expansion number.
IPC technical resources on ultra-thin test packages note that registration around 0.4 mm-pitch lands is critical and that mask cannot overlap the intended land surface. This illustrates why fine-pitch acceptance should be tied to the chosen fabricator's verified process.
Vias: Tented, Plugged, Filled or Exposed#
A via called “covered” in casual conversation can mean several different structures. Use precise terminology and drawing notes:
- Tented: solder mask covers the via opening on one or both sides.
- Plugged: the hole is filled or closed with a specified material or process.
- Filled and capped: the via is filled, planarized and plated over for via-in-pad use.
- Exposed: a mask opening leaves the via pad or hole accessible for test, soldering or thermal connection.
Mask tenting alone may not seal a large hole reliably, and trapped process chemistry can be a concern. For via-in-pad, do not rely on solder mask to prevent solder loss; specify a qualified fill-and-cap process. Review the finished data in the online Gerber viewer and compare it with the drill table.
Openings for Test Points, Connectors and Mechanical Features#
Expose test points that require electrical contact and give probes enough flat metal area after registration tolerance. If a test pad is close to a trace, enlarge copper clearance rather than assuming the mask will be the only insulation barrier.
Edge connectors and gold fingers need controlled mask pullback so mask does not contaminate the contact area or interfere with beveling. Mechanical pads, chassis contacts and shield lands also need deliberate openings. Mounting holes should be exposed or covered according to whether they are grounded, soldered, plated or isolated.
For selective soldering or hand-soldered connectors, review mask clearance with the assembly process. A large opening can expose nearby copper and increase bridging risk; an opening that is too tight can reduce wetting or leave cured mask on the pad edge.
Color, Finish and Optical Inspection#
Green is common because many factories have mature processes and inspection settings for it, but other colors can be used when branding or optical behavior matters. Color affects contrast, opacity and sometimes the achievable feature capability. Black and white masks can be harder to inspect, and white may discolor through repeated heat exposure.
Do not assume every color has the same minimum dam, registration capability or lead time. If appearance is important, define a color reference or approved sample and state whether cosmetic variation is acceptable. Our black PCB guide covers the specific inspection and material tradeoffs of black solder mask.
Matte and gloss descriptions can also vary by supplier. Treat finish as an agreed manufacturing attribute rather than a universally standardized visual grade.
Solder Mask Thickness and Copper Topography#
Finished mask thickness is not perfectly uniform. Coating over laminate, trace edges and high copper features can differ because liquid material flows and cures over a three-dimensional surface. Heavy copper makes coverage more difficult at conductor corners and between closely spaced traces.
If minimum insulation thickness matters, identify where it is required and how it will be measured. A blanket nominal thickness without a measurement location is ambiguous. Confirm that the selected mask and coating process are qualified for the released copper weight.
Do not use solder mask thickness as the sole control for safety isolation. Creepage and clearance rules must consider the applicable safety standard, pollution degree, voltage, material group and coating qualification.
Common Solder Mask Defects#
| Defect | Likely concern | Prevention or control |
|---|---|---|
| Mask on pad | Reduced solderability or contact area | Correct expansion and verified registration tolerance |
| Exposed adjacent copper | Bridging, corrosion or insulation risk | Increase spacing or reduce opening within process capability |
| Missing mask dam | Merged openings and higher bridging risk | Meet guaranteed web width or approve a gang opening |
| Blistering or lifting | Poor adhesion, contamination or under-cure | Qualified cleaning, imaging and cure process |
| Pinholes and voids | Local copper exposure | Control coating, cleanliness and inspection criteria |
| Cracking at trace edges | Loss of protection, especially over heavy copper | Compatible material, adequate coating and validated cure |
| Via tent rupture | Unexpected exposed hole or trapped residue | Match hole size to tenting capability or specify plugging |
What to Put in the Fabrication Data#
Export separate top and bottom solder mask layers with clear polarity. In standard Gerber workflows, drawn features usually represent openings, but the file naming and job information should remove any doubt. Include mask information in the controlled fabrication drawing and README rather than relying on filenames alone.
A practical fabrication note set should identify:
- required solder mask type, color and finish;
- qualification to the specified revision of IPC-SM-840 or an approved equivalent;
- whether artwork may be modified for manufacturing and when approval is required;
- minimum guaranteed mask dam and registration expectation where critical;
- special SMD or NSMD land requirements;
- via tenting, plugging, filling and capping requirements by via class;
- areas prohibited from receiving mask, including contacts, test points and tooling features;
- additional thickness, insulation, color-match or cosmetic acceptance requirements.
Keep these requirements synchronized with the manufacturing package, assembly drawing and controlled product revision.
PCB Solder Mask DFM Checklist#
- Confirm the manufacturer and assembler agree on mask material and process.
- Set expansion rules by pad or component class instead of using one unreviewed default.
- Verify minimum finished mask dams between fine-pitch pads.
- Check maximum registration shift for pad encroachment and accidental copper exposure.
- Review BGA lands as SMD or NSMD against the component recommendation.
- Specify every via as exposed, tented, plugged, filled or capped where necessary.
- Expose test points, contacts and chassis lands intentionally.
- Review heavy-copper edges and dense traces for coating coverage.
- Confirm non-green colors do not reduce the required feature capability.
- Inspect top and bottom mask files with copper, paste and drill data overlaid.
- State the applicable qualification and finished-board acceptance requirements.
- Approve any proposed mask-artwork edits before production when they affect functional features.
Official Engineering References#
- IPC Status of Standardization
- IPC-HDBK-840 Solder Mask Handbook
- IPC TM-650 Test Methods Manual
- Altium PCB Design Rules Overview
Final Takeaway#
A robust solder mask specification connects CAD rules to a verified fabrication process. It defines openings, expansion, finished mask dams, registration, via treatment, material qualification and special exposed areas without assuming the coating can correct an unsafe copper layout.
Ask the selected fabricator for guaranteed values, apply them by feature class, and inspect the released mask files together with copper and drill data. That prevents small artwork assumptions from becoming soldering, insulation or inspection problems in production.
PCB Solder Mask FAQ#
What is a typical solder mask expansion?
There is no universal value. It must accommodate the fabricator's registration tolerance while preserving adequate mask between pads. Use the manufacturer's approved rule set for the selected technology.
Should BGA pads be solder mask defined or non-solder mask defined?
Many BGA designs use NSMD pads, but some packages or reliability strategies require SMD lands. Follow the component manufacturer's recommendation and confirm the choice with the assembler and fabricator.
Can solder mask cover a via completely?
Small vias can often be tented, but tenting is not the same as plugging or filling and may not seal larger holes. Specify the required via-protection structure explicitly.
Does IPC-SM-840 define my solder mask openings?
No. IPC-SM-840 qualifies permanent solder mask materials and performance. Your design rules, fabrication drawing and board acceptance requirements define the actual openings and tolerances.
Is black solder mask harder to manufacture?
It can reduce inspection contrast and may have different minimum-feature capability or lead time. Confirm the exact process with the manufacturer before applying standard green-mask rules.
Is solder mask an electrical safety coating?
It provides insulation, but it should not be the sole basis for safety creepage and clearance unless the applicable standard and qualified coating system explicitly allow that use.