吃瓜tv

What is solder mask?

Solder mask is a patterned protective coating on a PCB surface. It covers selected copper and dielectric areas while leaving specified pads, contacts, test points and other openings accessible. Its functions include protecting circuitry and helping control where solder can wet during assembly. It is not the copper pattern, the printed legend or the stencil that deposits solder paste. These layers may look similar in a CAD viewer but represent different manufacturing instructions.

The useful design question is not simply which color to choose. You need to know which surfaces must remain exposed, how the openings align with the copper, whether a narrow mask web can survive the process and what cured coating is required. A nominal clearance value without its reference edge can create a misunderstanding that is difficult to see in a rendered image.

This page owns mask materials, openings and fabrication. For paste deposition, use the PCB stencil guide; for identification ink, use silkscreen PCB. The manufacturing process overview places mask within the complete bare-board route.

Start with three different shapes

A non-solder-mask-defined pad normally has an opening larger than the copper pad, exposing the pad boundary. A solder-mask-defined pad intentionally uses the mask opening to define the exposed area. These are functional choices, not two interchangeable export settings. If the design requires mask-defined geometry, identify it explicitly so a routine manufacturing adjustment does not remove the intended condition.

Do not enlarge the paste aperture merely because the mask opening is enlarged. Paste printing is a separate volumetric problem. Likewise, a mask opening over a test point does not create a suitable probe surface by itself: pad shape, finish, clearance and fixture access still matter. Checking the three layers together is more informative than reviewing each as an isolated colored image.

For circular NSMD lands, the solder mask clearance worksheet separates radial expansion, relative registration and the remaining web. Use the exact package and fabrication conditions for release.

How liquid photoimageable mask is formed

A common LPI route begins with a clean and appropriately prepared surface. The coating is applied using a compatible method and dried to the state needed for imaging. Exposure transfers the opening pattern, development removes the intended material, and the coating receives its specified final cure. The chemistry, exposure and cure requirements belong to the selected product and qualified factory route.

Taiyo's distinguishes material systems and technical literature. That is more useful than assuming every green coating has identical processing or properties. Inkjet mask and dry-film systems organize deposition and imaging differently. A process choice should be evaluated with the required topography, openings and final performance, rather than described as inherently best for every board.

The coating must work over the actual copper relief and hole environment. Heavy copper, filled vias and unusual surfaces can complicate coverage or registration. Ask about the complete construction if a design pushes several conditions simultaneously. A color selection in an order form does not establish the achievable web width, local coverage or acceptance requirement.

Check a mask web and an opening margin

For two equal rectangular pads, a simple nominal web is the pad pitch minus pad width minus twice the opening expansion. With a 0.80 mm pitch, 0.40 mm pad width and 0.05 mm expansion on each side, the nominal web is 0.30 mm. If each opening edge can grow another 0.025 mm toward the web, the screened remaining web is 0.25 mm. These dimensions are an arithmetic example, not 吃瓜tv's published minimum capability.

Global translation of the entire mask image does not reduce the web between its own openings, because both openings move together. It does affect exposure relative to the copper. The worksheet therefore handles opening-to-pad registration separately. With 0.05 mm nominal expansion, 0.04 mm relative registration allowance and 0.025 mm inward edge allowance, the worst-side exposure margin is negative 0.015 mm. A generous web can coexist with an exposure problem.

The screen uses independent worst-case allowances supplied by the user. It excludes local distortion, irregular pad shapes, curved edges and process correlations. Negative margin identifies a question to resolve, while positive margin only shows that the entered geometry fits the entered assumptions. The manufacturer must agree the actual design rules, process tolerances and inspection criteria.

Make via protection a separate decision

Tenting, plugging, filling and capping are different via treatments. A mask drawing that covers a small hole does not automatically specify a filled, planar or hermetically sealed structure. If an open via near a solder pad can draw solder away, review the complete via treatment and assembly interface rather than relying on its appearance in the mask layer.

Specify the required condition on both sides and identify any keepout around the via. Filled and capped via-in-pad structures may need an earlier manufacturing route and different verification. The HDI via-in-pad review helps distinguish this construction from ordinary mask coverage. Do not change the treatment late without checking its effect on processing, cost and test access.

Mask should not be assumed to replace the product's required creepage, clearance or insulation system. Voltage, environment, contamination and the applicable product standard influence those requirements. The cured material's qualification and the finished board's electrical design are related but distinct evidence. Keep the required insulation function explicit in the drawing and procurement review.

Choose color and contrast for the actual use

Color affects appearance, contrast and the inspection environment, but it does not establish board quality. Dark legend on a light background and light legend on a dark background can be useful, provided the actual ink and process give readable results. Inspect a representative sample under the lighting and magnification used by operators rather than judging only a bright screen rendering.

For LEDs, sensors or optical systems, reflectance or spectral behavior may matter. In that case, specify the relevant measurement and material instead of treating a color name as an optical specification. Coating thickness, cure and aging conditions can also be relevant. The LED PCB guide connects the board construction to the lighting application without assuming that all white masks behave alike.

Inspect the cured result, not only the artwork

Review registration to pads, contamination of intended openings, coverage over conductors and the condition of webs and edges. Surface appearance can reveal some issues, but adhesion, cure and electrical behavior require their appropriate methods. Define which evidence is included in the order and which is a separate qualification activity. A photograph of a green board cannot establish chemical compatibility or long-term insulation performance.

Relevant standards include IPC-SM-840 for permanent solder-mask qualification and performance, with board acceptance requirements determined by the applicable procurement documents. Use the to identify document scope and version, then use the complete agreed standard. This page does not turn a CAD clearance or a worksheet result into IPC compliance.

A first article should preserve the mask material, artwork revision and any approved opening adjustments. When a later order changes color, supplier material, surface finish or component layout, determine whether the original evidence still applies. A repeat order number alone is not enough if the coating system or process interface has changed.

Export and review the files together

Export top and bottom mask layers with the rest of the fabrication package. Confirm whether the format expresses openings or covered areas and inspect the actual exported result in a suitable viewer. Include the copper and outline so the review has a physical reference. Avoid using a screenshot as the controlling manufacturing definition of the apertures.

Ask for review of intentional mask-defined pads, unusual tenting, mask-free areas, connector contacts and any special color or surface requirement. If the factory proposes a clearance adjustment, examine its effect on both exposure and remaining webs. An automatic clipping or expansion operation may be useful, but it should not silently override a functional requirement.

Use the PCB DFM review for the wider manufacturing release. If a mask issue is discovered during assembly, retain the board revision, photos, affected locations and process conditions. These details help separate artwork, fabrication and assembly causes without assigning a cause from a single symptom.

What adds cost or review time?

Fine webs, unusual colors, special materials, demanding topography and additional qualification records may change the process or inspection effort. These are quotation questions rather than universal surcharges. A design that can accept a slightly larger opening or wider spacing may be easier to manufacture, but a change should follow the component and product requirements.

For a useful enquiry, send the fabrication files, board revision, intended mask system or performance requirement, color, surface finish and the critical geometry. Identify which regions are functional and which are cosmetic. If a minimum opening or web is not yet decided, provide the package or application constraint and ask for a manufacturable proposal.

The mask worksheet can document your geometry assumptions, but it does not transfer them automatically into Contact. Download the brief and attach it manually with the drawing. Customers with completed fabrication data can go directly to the manufacturing service and request review without using the tool.

Solder-mask questions