Choose the PCB pad definition specified for the actual component package, then check that its copper, mask and stencil dimensions can be built together. An SMD pad is defined by a solder mask opening smaller than its copper land; an NSMD pad is defined by copper, with a larger mask opening around it. Many BGA suppliers recommend NSMD, but other packages specify SMD or a deliberate mix. Pitch alone does not settle the choice.
The IPC-7351 land-pattern article covers footprint standards and density choices; this page focuses on the pad-to-mask tolerance budget and the handoff between layout, fabrication and assembly. Board-wide solder mask expansion and web checks are a separate task from choosing the definition for an individual pad.
1. What Changes Between SMD and NSMD?
For a round pad, call the finished copper diameter D and the mask opening diameter M. SMD means M is smaller than D: mask overlaps the perimeter and the opening defines the nominal exposed top area. NSMD means M is larger than D: the copper perimeter defines the land and there is a clearance ring between copper and mask.
| Design question | SMD: mask-defined | NSMD: copper-defined |
|---|---|---|
| What defines the exposed top boundary? | Mask opening | Copper edge |
| What happens at the pad edge? | Mask overlaps the copper | Clearance exposes the perimeter; solder can wet the sidewall |
| Primary geometry check | Minimum overlap after registration and size variation | Minimum clearance after registration and size variation |
| Routing consequence | Larger copper may reduce the gap for a given opening | Smaller copper may leave more routing room for a comparable exposed diameter |
| Assembly concern | Opening location shifts with mask registration; solder joint geometry changes at the mask edge | Adjacent trace or via may be exposed by the opening; pad edge must remain clear |
SMD here means solder-mask-defined, not surface-mount device. Pad definition on the PCB also need not match the definition on the package substrate. Use the board-side land pattern in the component documentation rather than copying a package-side dimension.
2. Which Pad Type Should You Use?
Start with the exact part number, package drawing and revision. Read the recommended PCB land, mask opening and stencil notes together. A data sheet may give different guidance for a power pad and a signal pad, or identify specific locations that require a different treatment. If the supplier provides a recommended footprint, verify that it matches the package actually ordered and the intended assembly process.
| Situation | Layout decision | Evidence to obtain before release |
|---|---|---|
| Package guide specifies NSMD | Use its land and opening as the starting point | Fabricator's registration, copper and mask-opening tolerances; assembler's stencil review |
| Package guide specifies SMD | Preserve the specified overlap and opening | Minimum overlap across process variation; assembly and inspection plan |
| Guide specifies mixed pad types | Follow the identified locations, not a global rule | Pad-by-pad drawing or library notes; assembler approval of the mixed footprint |
| No package guidance, or a conflict with DFM | Do not silently substitute one type | Component supplier clarification and written fabricator/assembler disposition |
| Tight pitch leaves little or no mask web | Calculate the opening and web budget first | Fabricator's minimum web for the chosen process and assembler's paste/bridging plan |
| Drop, bending or thermal cycling drives the decision | Treat pad type as one variable in the joint system | Qualification plan with representative board, package, process and loading |
For example, AMD's UG1099 recommends NSMD for the BGA devices it covers, while the MPS surface-mount guidance recommends SMD for its BGA power modules and describes a mixed arrangement for certain LGA modules. These are examples of package-specific instructions, not a ranking of manufacturers or a transferable design rule. A switch based only on a generic pitch threshold can invalidate the supplier's intended joint geometry.
3. How Much Clearance or Overlap Remains After Registration?
A nominal ring is not the same as its smallest manufactured value. For concentric circular features, the nominal radial clearance for NSMD is (M-D)/2; the nominal radial overlap for SMD is (D-M)/2. Mask-to-copper registration shift reduces the ring on one side and increases it on the opposite side.
A conservative first-pass budget, with all tolerances expressed as positive diameter limits, is:
Here R is the maximum radial relative offset between mask and copper, C\min is the smallest NSMD clearance and O\min the smallest SMD overlap. Use the applicable fabrication tolerances for the actual mask material, imaging route, panel and drawing. Include any other specified allowance in the budget; do not count the same allowance twice. The simple model assumes round features and a bounded relative offset. It is a screening calculation, not an acceptance standard.
Worked example: one hypothetical NSMD BGA land
Suppose the design calls for a 0.30 mm copper pad and a 0.40 mm mask opening. Assume, for illustration only, copper diameter 0.29–0.31 mm, opening diameter 0.39–0.41 mm and a 0.03 mm maximum relative offset. The nominal clearance is (0.40-0.30)/2 = 0.05 mm per side. The worst-case minimum is (0.39-0.31)/2-0.03 = 0.01 mm. Only 10 µm remains on the narrow side under those combined assumptions.
That result does not establish that the board is manufacturable. Compare it with the fabricator's required clearance and inspection criteria. If it is inadequate, discuss a larger opening, a different process or another component-approved design. A larger opening consumes mask web and can uncover a nearby trace, so rerun those checks before accepting the change.
For the corresponding SMD check, imagine a 0.40 mm nominal copper land and 0.30 mm opening with the same ±0.01 mm diameter limits and 0.03 mm offset. The minimum overlap is (0.39-0.31)/2-0.03 = 0.01 mm. This is an arithmetic comparison only: these two hypothetical lands are not automatically interchangeable for a real package. Obtain the manufacturer's required minimum overlap and the supplier's process capability.
4. Will the Mask Web and Escape Routing Fit?
For equal round openings in a row, nominal mask web is the center-to-center pitch minus the opening diameter. At 0.50 mm pitch with a 0.25 mm NSMD copper land and 0.05 mm radial mask expansion, the opening is 0.35 mm and the nominal web is 0.15 mm. This is a layout result, not a guaranteed finished web. Opening size, registration, artwork and process variation matter; the fabricator must confirm the usable minimum for the selected mask and color.
The nominal copper gap between the same adjacent pads is 0.50-0.25=0.25 mm. A centered 0.10 mm trace leaves (0.25-0.10)/2=0.075 mm copper clearance on each side in a simplified two-pad cross-section. Confirm trace-to-pad clearance, via features and actual shape in the DRC; the mask opening may also uncover the trace. A valid copper DRC does not prove that the mask protects that trace.
If an individual mask dam cannot be built, the fabricator and assembler may consider a common opening across a row or array. That decision changes solder exposure and bridging risk. Check the device supplier's requirements and have the assembler review stencil apertures, paste printing and inspection before changing the artwork. A missing dam should never be assumed harmless just because the copper spacing passes.
5. Does NSMD Always Produce a Stronger Joint?
No single pad type guarantees joint life. NSMD exposes the pad perimeter, so solder can wet the copper sidewall as well as the top. SMD overlaps the pad edge, and the larger copper land used in some designs may help with pad attachment. Neither observation alone predicts the failure mode of an assembled product.
For scale, an ideal circular pad 0.30 mm in diameter and 0.030 mm thick has a top area of about 0.0707 mm² and a cylindrical side area of about 0.0283 mm², or 40% of the top. This is geometric area, not measured wetted area, added joint strength or a fatigue-life prediction. A real pad has a trace connection, a surface finish and a three-dimensional solder fillet; actual wetting depends on the process.
Failure may occur in the solder, at an interface, in the copper attachment or in the laminate beneath the pad. Package size and stiffness, board thickness, laminate, solder alloy, pad geometry, board support and the thermal or mechanical load all matter. When reliability is critical, compare representative assemblies using the test conditions and acceptance criteria for the product. Record the failure location as well as pass/fail results.
6. What Must the Assembler Check?
Stencil and paste. The paste aperture is a separate design feature from the solder mask opening. Its size and thickness determine the nominal deposit, while release depends on aperture geometry, paste and printing conditions. Do not assume that the aperture must always equal the mask opening. The component supplier's stencil drawing and the assembler's process review are the starting points. Solder paste inspection (SPI) can check the printed deposit when included in the inspection plan.
Vias. An exposed via connected to a pad can draw solder away during reflow soldering. Via-in-pad treatment depends on the package, via location, permitted surface condition and assembly process. An open thermal via may be acceptable in a supplier's documented design; another location may require filling and capping. Specify the actual via construction and surface requirement rather than assuming SMD or NSMD decides it.
Mixed definitions. Some component instructions deliberately use different definitions within a package. Elsewhere, a mix can alter solder geometry and print behavior. Document every intentional exception in the footprint and assembly drawing, and ask for an explicit manufacturing review rather than allowing CAM or a global rule to alter it silently.
Inspection. Mask registration and pad exposure can be reviewed on the bare board; paste deposits can be assessed before placement. AOI inspects visible features, while selected X-ray can examine hidden joints where specified. For joint-specific symptoms and inspection limits, see BGA soldering defects. X-ray does not by itself establish fatigue life or prove every interface sound. Agree on locations, sampling and acceptance criteria before the build, and investigate suspicious joints with additional analysis when appropriate.
7. Release Checklist for Design, Fabrication and Assembly
| Owner | Release question | Deliverable or decision |
|---|---|---|
| Designer | Does the footprint match the exact package and revision? | Copper, mask and paste layers; component drawing; documented exceptions |
| Designer | Do worst-case overlap or clearance, web and copper DRC all fit? | Dimension and tolerance budget; local overrides identified |
| Fabricator | Can the specified mask and copper features be produced together? | DFM disposition, mask process constraints and any proposed artwork changes |
| Assembler | Do stencil, paste, via treatment and board support fit the package? | Stencil and process review; first-article inspection scope |
| Quality / product owner | What must the finished product withstand? | Applicable qualification conditions, acceptance criteria and change-control owner |
| Procurement | What is included in the order? | Agreed quantities, inspection locations, reports and approval route for deviations |
Send Gerber or ODB++ and drill data, the BOM with manufacturer part numbers, placement data, assembly drawing, relevant component land-pattern guidance and any special mask or via requirements. Mark critical footprints and identify whether a proposed artwork change requires customer approval. Include the required reliability and inspection evidence in the quote request rather than assuming it is a standard deliverable.
HILPCB's SMT assembly scope includes review of package land patterns, solder-mask clearance, stencil apertures and via-in-pad conditions. SPI, AOI and selected X-ray are matched to the agreed inspection scope; the actual route and deliverables are confirmed for the submitted design. Include the package and footprint details with a quote request, or contact our team to discuss the required review.
Frequently Asked Questions
What is the difference between an SMD and an NSMD pad?
An SMD pad has a mask opening smaller than the copper land, so the mask defines the exposed top boundary. An NSMD opening is larger than the land, so the copper edge defines the pad. SMD in this context means solder-mask-defined.
Is NSMD always better for a BGA?
No. Many BGA package guides recommend NSMD, while others specify SMD. Follow the exact component manufacturer's PCB land pattern and confirm the design with the fabricator and assembler.
How do I calculate NSMD mask clearance?
For concentric circular features, subtract the copper diameter from the opening diameter and divide by two. To estimate the smallest clearance, use the minimum opening, maximum copper diameter and maximum relative registration offset, then compare the result with the fabricator's process requirements.
Can I mix SMD and NSMD pads under one component?
Some manufacturers specify a deliberate mix for particular packages. Otherwise, get the component supplier and assembler to review the change: different pad definitions can affect solder geometry, printing and bridging. Document any intentional exceptions.
Does pad definition determine the stencil aperture?
No. The copper land, mask opening and stencil aperture are separate features. Use the component's assembly guidance and the assembler's review to select aperture geometry and stencil thickness for the intended paste and process.