[{"data":1,"prerenderedAt":67},["ShallowReactive",2],{"blog-solder-mask-design-errors-en":3},{"title":4,"description":5,"date":6,"lastUpdated":6,"category":7,"image":8,"imageAlt":9,"readingTime":10,"wordCount":11,"timeRequired":12,"htmlContent":13,"faq":14,"tags":30,"slug":36,"sourceLocale":37,"availableLocales":38,"jsonld":43},"Solder Mask Design Errors: Expansion, Web Width, Vias and Pad Definition","Review solder mask openings, nominal web widths, via protection and pad definition against package guidance and the fabricator's project-specific process.","2026-11-05","design","/assets/img/blogs/2026/11/solder-mask-design-errors.svg","Conceptual top view of PCB pads in mask openings, separated by solder mask webs.",11,2136,"PT11M","\u003Cp>Solder mask openings and the webs between them must suit both the component design and the fabrication process. Define the intended geometry in the artwork, then agree on finished-board requirements with the selected fabricator. Via coverage and the choice of copper- or mask-defined pads also need explicit review.\u003C/p>\n\u003Cp>The process side of mask application, exposure and curing is covered in our \u003Ca href=\"/en/blog/pcb-soldermask-exposure/\">soldermask exposure and process control article\u003C/a>. This page stays on the design decisions that feed it.\u003C/p>\n\u003Ch2>1. Mask Opening and Registration\u003C/h2>\n\u003Cp>Mask expansion is the nominal opening beyond the copper edge per side. For a non-solder-mask-defined (NSMD) land, positive expansion provides nominal clearance around the copper. For a solder-mask-defined (SMD) land, mask overlap is intentional and should follow the exact package guidance.\u003C/p>\n\u003Cp>A 1:1 opening in supplied artwork is not automatically an error or a finished-board result. Some fabricators request 1:1 input artwork and calculate production compensation themselves; the convention does not establish zero registration error or automatically qualify the design.\u003C/p>\n\u003Cp>Apparent mask-to-pad offset can reflect both fabrication variation and the measurement method. Compare the released artwork and board revision using an agreed datum, sampling plan and measurement rule, then assess the result against the applicable drawing or standard. A single image or pad does not establish a universal tolerance, solderability result or supplier capability.\u003C/p>\n\u003Cp>Agree with the fabricator on production compensation, registration relative to copper, opening variation and acceptable pad encroachment for the actual design. Larger openings reduce nominal webs and can expose adjacent copper.\u003C/p>\n\u003Ch2>2. Mask Web (Dam) Width: The Budget Between Two Openings\u003C/h2>\n\u003Cp>The web is the strip of mask left between two adjacent openings. For equal adjacent lands with equal, symmetric NSMD expansion, the nominal artwork calculation is \u003Cstrong>W = S_copper - 2E\u003C/strong>, where W is nominal web width, S_copper is the copper edge-to-edge spacing, and E is expansion per side.\u003C/p>\n\u003Ch3>Worked budget by pitch\u003C/h3>\n\u003Ctable>\n\u003Cthead>\n\u003Ctr>\n\u003Cth>Package pitch\u003C/th>\n\u003Cth align=\"right\">Land width\u003C/th>\n\u003Cth align=\"right\">Copper gap\u003C/th>\n\u003Cth align=\"right\">Expansion per side\u003C/th>\n\u003Cth align=\"right\">Nominal web\u003C/th>\n\u003C/tr>\n\u003C/thead>\n\u003Ctbody>\u003Ctr>\n\u003Ctd>0.65 mm\u003C/td>\n\u003Ctd align=\"right\">0.35 mm\u003C/td>\n\u003Ctd align=\"right\">0.30 mm\u003C/td>\n\u003Ctd align=\"right\">0.05 mm\u003C/td>\n\u003Ctd align=\"right\">0.20 mm\u003C/td>\n\u003C/tr>\n\u003Ctr>\n\u003Ctd>0.50 mm\u003C/td>\n\u003Ctd align=\"right\">0.25 mm\u003C/td>\n\u003Ctd align=\"right\">0.25 mm\u003C/td>\n\u003Ctd align=\"right\">0.05 mm\u003C/td>\n\u003Ctd align=\"right\">0.15 mm\u003C/td>\n\u003C/tr>\n\u003Ctr>\n\u003Ctd>0.40 mm\u003C/td>\n\u003Ctd align=\"right\">0.20 mm\u003C/td>\n\u003Ctd align=\"right\">0.20 mm\u003C/td>\n\u003Ctd align=\"right\">0.05 mm\u003C/td>\n\u003Ctd align=\"right\">0.10 mm\u003C/td>\n\u003C/tr>\n\u003Ctr>\n\u003Ctd>0.40 mm\u003C/td>\n\u003Ctd align=\"right\">0.20 mm\u003C/td>\n\u003Ctd align=\"right\">0.20 mm\u003C/td>\n\u003Ctd align=\"right\">0.035 mm\u003C/td>\n\u003Ctd align=\"right\">0.13 mm\u003C/td>\n\u003C/tr>\n\u003C/tbody>\u003C/table>\n\u003Cp>These are not finished-web guarantees. The smaller expansion increases the nominal web but leaves less nominal pad clearance. Uniform translation of the entire mask image does not itself change spacing between its openings, although it changes their alignment to copper. Actual results also depend on opening variation, local distortion, copper geometry, material, coating, imaging, development and the CAM design.\u003C/p>\n\u003Cp>Minimum-web figures are specific to the supplier and production route, not universal acceptance values. Color and finish can matter alongside formulation, copper thickness and process; direct imaging alone does not establish that a particular design is feasible.\u003C/p>\n\u003Cp>Verify finished geometry, acceptable encroachment, minimum retained web, inspection and acceptance with the selected fabricator. If a web is problematic, options include adjusting the land or opening, changing the manufacturing approach, or considering a gang opening with assembly review.\u003C/p>\n\u003Ch2>3. SMD vs NSMD Pads: Review the Exact Package\u003C/h2>\n\u003Cp>An NSMD opening extends beyond the copper land; an SMD opening overlaps the land and defines the exposed boundary. Choose the geometry using the \u003Cstrong>exact part and package land-pattern guidance\u003C/strong>, then check clearance or overlap after fabrication tolerances, including the effect of connected traces and pours. The \u003Ca href=\"/en/blog/smd-vs-nsmd-pads/\">SMD vs NSMD pad guide\u003C/a> covers the tolerance budget and assembly tradeoffs in detail.\u003C/p>\n\u003Cp>For example, TI&#39;s \u003Cem>Manufacturing and Rework Design Guide for MicroSiP Power Modules\u003C/em>, SLIB006A Rev. A, recommends NSMD for the described MicroSiP BGA-pin modules and generally SMD for the described MicroSiL LGA pins, with power-plane geometry considerations. Those recommendations apply to the packages covered by that guide, not all BGA or LGA packages.\u003C/p>\n\u003Cp>Investigate unintentional differences in land definition or geometry, especially across the terminals of a component. Deliberate mixed geometry can be valid when it is supported for the specific design and reviewed with manufacturing and assembly; documenting the choice alone does not qualify it.\u003C/p>\n\u003Cp>Murata&#39;s ceramic capacitor FAQ on tombstoning describes a tension imbalance affected by land area, solder, temperature, and placement. It does not test mixed SMD/NSMD lands, and pad labels alone do not establish measured forces. See also \u003Ca href=\"/en/blog/pcb-tombstoning-causes-prevention/\">PCB tombstoning causes and prevention\u003C/a>.\u003C/p>\n\u003Ch2>4. Via Coverage: Specify the Construction and Acceptance\u003C/h2>\n\u003Cp>&quot;Tent vias&quot; alone leaves too much open to interpretation. In the fabrication files or drawing, identify the affected vias, the side or sides, the desired protection process and construction, and the acceptance criteria. Agree with the fabricator on how coverage will be inspected and what, if any, exposed areas or other imperfections are acceptable.\u003C/p>\n\u003Cp>Coverage can vary with via geometry, materials and application process. An adjacent pad opening may merge with a via opening or leave too little mask between them, so check the resulting openings rather than relying on the intended tent alone. In its \u003Cem>PCB Design Guidelines for 0.5mm Package-on-Package Applications Processor, Part I\u003C/em>, SPRABB3, section 20.5.1, TI notes that a single-pass LPI mask cannot guarantee complete via coverage and discusses hole size, surface tension and board thickness for screen printing. It does not establish a universal hole-size limit or acceptance criterion.\u003C/p>\n\u003Cp>Distinguish vias \u003Cstrong>in pads\u003C/strong> from vias \u003Cstrong>adjacent to pads\u003C/strong>. An open via in a pad may draw solder away from a joint; an adjacent via may also interact with the pad opening or soldering process. Consider the intended soldering and cleaning processes when choosing protection: cleaning chemistry may enter or be difficult to remove from some constructions, but single-sided coverage does not automatically trap it. See \u003Ca href=\"/en/blog/via-in-pad-vippo/\">via-in-pad\u003C/a> and the \u003Ca href=\"/en/blog/via-filling-material-guide-pcb-stackup-materials/\">via filling material guide\u003C/a>.\u003C/p>\n\u003Cp>Plugging or filling may be options where tenting is unsuitable; neither is a mandatory fix or a guarantee of performance. The Peters PP 2795 technical report describes a specific via-filler product and dependencies on aspect ratio and production parameters. It is not an LPI tenting specification.\u003C/p>\n\u003Cp>The 2006 IPC-4761 table of contents lists these type names: I tented, II tented and covered, III plugged, IV plugged and covered, V filled, VI filled and covered, and VII filled and capped. This public table of contents is not the complete standard and does not establish the detailed construction or acceptance requirements. Use the applicable controlled edition and agree the specific construction and acceptance with the fabricator.\u003C/p>\n\u003Ch2>5. Mask Over Controlled-Impedance Traces\u003C/h2>\n\u003Cp>Solder mask is a dielectric. For an otherwise unchanged outer-layer microstrip geometry, adding mask over the line typically raises effective permittivity and lowers calculated characteristic impedance. The magnitude depends on the geometry and material. A fabricator may compensate by adjusting trace dimensions, so final measured impedance is not necessarily lower (see our \u003Ca href=\"/en/blog/microstrip-vs-stripline/\">microstrip vs stripline comparison\u003C/a>).\u003C/p>\n\u003Cp>Mask cross-section can vary with copper topography, application and cure. Confirm actual coverage, stackup and trace geometry, and the mask material parameters at the relevant frequency or the fabricator&#39;s calibrated model. Review the target and tolerance, fabrication adjustments, representative coupon construction and measurement method with the fabricator.\u003C/p>\n\u003Cp>A local mask opening may change the transmission-line structure. Its significance depends on geometry, transition and frequency and can be evaluated with the connector launch.\u003C/p>\n\u003Ch2>6. Silkscreen and Mask Openings\u003C/h2>\n\u003Cp>Keep legend off solderable surfaces. Agree the target fabricator&#39;s legend-to-opening clearance, registration and CAM clipping policy, and review legend placement against the local mask geometry. Our \u003Ca href=\"/en/blog/pcb-silkscreen/\">PCB silkscreen guide\u003C/a> covers line width, text height and placement.\u003C/p>\n\u003Ch2>7. Error-to-Symptom Matrix\u003C/h2>\n\u003Ctable>\n\u003Cthead>\n\u003Ctr>\n\u003Cth>Design error\u003C/th>\n\u003Cth>What shows up\u003C/th>\n\u003Cth>Where it is caught\u003C/th>\n\u003Cth>Fix in layout\u003C/th>\n\u003C/tr>\n\u003C/thead>\n\u003Ctbody>\u003Ctr>\n\u003Ctd>Unagreed opening convention or compensation\u003C/td>\n\u003Ctd>Unintended clearance or pad encroachment\u003C/td>\n\u003Ctd>Artwork and fabrication review\u003C/td>\n\u003Ctd>Define intended openings; agree compensation, registration, opening variation and acceptable encroachment with the fabricator\u003C/td>\n\u003C/tr>\n\u003Ctr>\n\u003Ctd>Web not retained as intended\u003C/td>\n\u003Ctd>Missing or incomplete mask between openings\u003C/td>\n\u003Ctd>CAM and finished-board inspection\u003C/td>\n\u003Ctd>Calculate nominal web; agree finished geometry, minimum retained web, inspection and acceptance; review alternatives if needed\u003C/td>\n\u003C/tr>\n\u003Ctr>\n\u003Ctd>&quot;Tent all vias&quot; without a coverage requirement\u003C/td>\n\u003Ctd>Coverage may be incomplete, depending on the process and geometry\u003C/td>\n\u003Ctd>CAM review or fabrication inspection\u003C/td>\n\u003Ctd>Identify affected vias and sides; agree the protection process and coverage acceptance with the fabricator\u003C/td>\n\u003C/tr>\n\u003Ctr>\n\u003Ctd>One-sided tent on open via\u003C/td>\n\u003Ctd>Solder or cleaning chemistry may enter; removal or inspection may be difficult depending on the construction and process\u003C/td>\n\u003Ctd>Design, assembly or cleaning review\u003C/td>\n\u003Ctd>Specify the intended sides and protection; agree construction and acceptance for the soldering and cleaning processes\u003C/td>\n\u003C/tr>\n\u003Ctr>\n\u003Ctd>Via land inside pad expansion zone\u003C/td>\n\u003Ctd>The pad and via openings may merge, leaving the via exposed or changing local mask coverage\u003C/td>\n\u003Ctd>Solder-mask opening or CAM review\u003C/td>\n\u003Ctd>Check the opening geometry and distinguish adjacent vias from vias in pads; agree the required protection and acceptance\u003C/td>\n\u003C/tr>\n\u003Ctr>\n\u003Ctd>Accidental SMD/NSMD mix\u003C/td>\n\u003Ctd>Possible variation in exposed geometry and soldering behavior; the effect depends on the design and process\u003C/td>\n\u003Ctd>Compare intended and actual copper and mask geometry at the component terminals\u003C/td>\n\u003Ctd>Investigate unintended differences; review any deliberate mix for the specific design with manufacturing and assembly\u003C/td>\n\u003C/tr>\n\u003Ctr>\n\u003Ctd>Mask coverage or transmission-line geometry differs from the impedance model\u003C/td>\n\u003Ctd>Calculated or measured impedance may differ from target, depending on the structure and fabrication adjustments\u003C/td>\n\u003Ctd>Model and coupon review\u003C/td>\n\u003Ctd>Agree coverage, stackup, model and representative coupon with the fabricator\u003C/td>\n\u003C/tr>\n\u003Ctr>\n\u003Ctd>Legend inside mask opening\u003C/td>\n\u003Ctd>Legend may be clipped or contaminate solderable surfaces\u003C/td>\n\u003Ctd>CAM and fabrication review\u003C/td>\n\u003Ctd>Follow the agreed legend clearance and clipping policy\u003C/td>\n\u003C/tr>\n\u003C/tbody>\u003C/table>\n\u003Ch2>8. Pre-Release Mask Checklist\u003C/h2>\n\u003Cp>\u003Cimg src=\"/assets/img/blogs/2026/11/solder-mask-design-errors-release-checks.svg\" alt=\"Three release checks: compare copper and mask files from the same revision; review openings, gaps and intended via coverage; agree material, process, inspection and acceptance with the fabricator.\">\u003C/p>\n\u003Col>\n\u003Cli>Define each opening convention and expansion per side; follow exact package guidance for intentional SMD overlap.\u003C/li>\n\u003Cli>Calculate nominal webs where applicable, and check the effect of expansion on both web width and pad clearance.\u003C/li>\n\u003Cli>Agree with the fabricator on production compensation, registration, opening variation, acceptable encroachment, finished geometry, minimum retained web, inspection and acceptance.\u003C/li>\n\u003Cli>Identify affected vias and sides, and specify the protection process, construction and acceptance criteria agreed with the fabricator.\u003C/li>\n\u003Cli>Check pad definition against the exact part and package guidance and the intended copper and mask geometry. Investigate unintended differences; confirm that any deliberate differences are supported for the specific design and reviewed with manufacturing and assembly.\u003C/li>\n\u003Cli>Check covered outer-layer controlled-impedance structures using the agreed stackup, model and representative coupon assumptions.\u003C/li>\n\u003Cli>Check legend placement against the selected fabricator&#39;s clearance, registration and CAM clipping rules.\u003C/li>\n\u003Cli>Record mask color and finish. When needed, agree mask material, thickness, tolerance, measurement method and permitted substitutions with the fabricator.\u003C/li>\n\u003C/ol>\n\u003Cp>For assembly considerations such as land patterns, solder-mask clearance and via-in-pad conditions, see \u003Ca href=\"/en/products/smt-assembly/\">HILPCB SMT assembly\u003C/a>. For a project-specific quote, submit your fabrication data through the \u003Ca href=\"/en/quote/\">HILPCB quote page\u003C/a> and confirm the required review and inspection scope.\u003C/p>\n\u003Cdiv data-component=\"BlogQuickQuoteInline\">\u003C/div>\n\n\u003C!-- faq:start -->\n\u003Ch2>FAQ\u003C/h2>\n\u003Ch3>How much solder mask expansion should I use?\u003C/h3>\n\u003Cp>Use the expansion appropriate to the land design and agree on the artwork convention and production compensation with the fabricator. Expansion is nominal opening beyond copper per side; a 1:1 input may be appropriate for some supplier workflows. For SMD lands, follow the exact package guidance for intentional overlap.\u003C/p>\n\u003Ch3>What is the minimum solder mask web between pads?\u003C/h3>\n\u003Cp>There is no universal minimum for every design and process. Calculate the nominal artwork web, then agree on the minimum retained web and its inspection and acceptance with the selected fabricator. If needed, review land or opening changes, the manufacturing approach, or a gang opening with assembly review.\u003C/p>\n\u003Ch3>Should I tent vias or plug them?\u003C/h3>\n\u003Cp>Tenting, plugging and filling are options, not interchangeable guarantees. Choose based on the via location, required protection, soldering and cleaning processes, and the fabricator&#39;s proposed construction. Identify the affected vias and sides, then agree the process and acceptance criteria with the fabricator using the applicable controlled standard edition.\u003C/p>\n\u003Ch3>When should I use solder-mask-defined pads?\u003C/h3>\n\u003Cp>Use solder-mask-defined pads when the exact part and package guidance and the specific design support them. Review the copper and mask geometry, routing and pours, fabrication tolerances, paste and assembly process, and expected thermal and mechanical loading with manufacturing and assembly. There is no universal SMD recommendation based on package type alone.\u003C/p>\n\u003Ch3>Does solder mask affect trace impedance?\u003C/h3>\n\u003Cp>Yes. For an otherwise unchanged outer-layer microstrip, mask typically lowers calculated impedance, but the effect depends on the material and geometry. Fabrication adjustments can change the result, so measured impedance is not necessarily lower. Confirm the coverage and model assumptions with the fabricator.\u003C/p>\n\u003C!-- faq:end -->\n\u003Csection class=\"related-links\" aria-label=\"Related\">\u003Ch3>Related links\u003C/h3>\u003Cul>\u003Cli>\u003Ca href=\"/en/blog/pcb-soldermask-exposure/\">PCB Soldermask Exposure and Manufacturing Process Control\u003C/a>\u003C/li>\u003Cli>\u003Ca href=\"/en/blog/smd-vs-nsmd-pads/\">SMD vs NSMD Pads: How to Choose and Check the Mask\u003C/a>\u003C/li>\u003Cli>\u003Ca href=\"/en/blog/pcb-tombstoning-causes-prevention/\">PCB Tombstoning: Causes, Diagnosis and Prevention in SMT Assembly\u003C/a>\u003C/li>\u003Cli>\u003Ca href=\"/en/blog/via-in-pad-vippo/\">Via-in-Pad plated over (VIPPO): The ultimate interconnect technology to solve AI chip packaging bottlenecks\u003C/a>\u003C/li>\u003Cli>\u003Ca href=\"/en/blog/via-filling-material-guide-pcb-stackup-materials/\">Via Filling Material Guide for PCB Stackups\u003C/a>\u003C/li>\u003Cli>\u003Ca href=\"/en/blog/microstrip-vs-stripline/\">Microstrip vs Stripline: Choosing a PCB Routing Structure\u003C/a>\u003C/li>\u003Cli>\u003Ca href=\"/en/blog/pcb-silkscreen/\">PCB Silkscreen Design Guide: Font Sizes, CAM Clipping Rules, and Screen Printing Methods\u003C/a>\u003C/li>\u003C/ul>\u003C/section>",[15,18,21,24,27],{"question":16,"answer":17,"answerText":17},"How much solder mask expansion should I use?","Use the expansion appropriate to the land design and agree on the artwork convention and production compensation with the fabricator. Expansion is nominal opening beyond copper per side; a 1:1 input may be appropriate for some supplier workflows. For SMD lands, follow the exact package guidance for intentional overlap.",{"question":19,"answer":20,"answerText":20},"What is the minimum solder mask web between pads?","There is no universal minimum for every design and process. Calculate the nominal artwork web, then agree on the minimum retained web and its inspection and acceptance with the selected fabricator. If needed, review land or opening changes, the manufacturing approach, or a gang opening with assembly review.",{"question":22,"answer":23,"answerText":23},"Should I tent vias or plug them?","Tenting, plugging and filling are options, not interchangeable guarantees. Choose based on the via location, required protection, soldering and cleaning processes, and the fabricator's proposed construction. Identify the affected vias and sides, then agree the process and acceptance criteria with the fabricator using the applicable controlled standard edition.",{"question":25,"answer":26,"answerText":26},"When should I use solder-mask-defined pads?","Use solder-mask-defined pads when the exact part and package guidance and the specific design support them. Review the copper and mask geometry, routing and pours, fabrication tolerances, paste and assembly process, and expected thermal and mechanical loading with manufacturing and assembly. There is no universal SMD recommendation based on package type alone.",{"question":28,"answer":29,"answerText":29},"Does solder mask affect trace impedance?","Yes. For an otherwise unchanged outer-layer microstrip, mask typically lowers calculated impedance, but the effect depends on the material and geometry. Fabrication adjustments can change the result, so measured impedance is not necessarily lower. Confirm the coverage and model assumptions with the fabricator.",[31,32,33,34,35],"solder mask design","solder mask expansion","solder mask web","via tenting","SMD vs NSMD pads","solder-mask-design-errors","en",[37,39,40,41,42],"de","cn","fr","ru",{"blog":44,"breadcrumb":53},{"@context":45,"@type":46,"headline":4,"description":5,"image":8,"url":47,"datePublished":6,"dateModified":6,"timeRequired":12,"keywords":48,"articleSection":7,"author":49,"publisher":52},"https://schema.org","BlogPosting","https://hilpcb.com/en/blog/solder-mask-design-errors/","solder mask design, solder mask expansion, solder mask web, via tenting, SMD vs NSMD pads",{"@type":50,"name":51},"Organization","HILPCB",{"@type":50,"name":51},{"@context":45,"@type":54,"itemListElement":55},"BreadcrumbList",[56,61,65],{"@type":57,"position":58,"name":59,"item":60},"ListItem",1,"Home","https://hilpcb.com/",{"@type":57,"position":62,"name":63,"item":64},2,"Blog","https://hilpcb.com/en/blog/",{"@type":57,"position":66,"name":36,"item":47},3,1795146063868]