PCB Solder Mask vs Solder Paste Layers: Key Differences and Common Gerber Mistakes

Introduction

Solder mask and solder paste layers can look similar in a Gerber viewer: both often contain shapes around component pads. They describe different manufacturing instructions, however. Solder mask data defines where the board's protective coating is opened; solder paste data defines where paste is intended to be printed for assembly. Substituting one for the other can leave solderable pads covered or create an unsuitable stencil.

This guide explains the distinction, shows why copper, mask, and paste geometry must be reviewed separately, and provides a release checklist for PCB designers and PCBA buyers. The goal is a clear manufacturing handoff, not a universal set of footprint dimensions.

Solder Mask vs Solder Paste: The Essential Difference

Solder Mask Belongs to Bare-Board Fabrication

Solder mask is the permanent protective coating over selected board surfaces. Pads and other features that need exposed metal require openings. In the usual CAD mask-layer representation, a pad-shaped feature indicates an opening, not a patch of coating to add. Always confirm the interpretation in the exported file and CAM viewer rather than judging it by the display color.

Solder Paste Data Belongs to Assembly Preparation

The paste layer describes intended printing apertures. A stencil uses these openings to deposit solder paste before component placement and reflow. The paste artwork is not an extra copper layer or a coating that the bare-board fabricator applies. The assembler may propose changes to the supplied paste geometry; the approved production stencil should remain traceable to the board revision.

A useful release question is: Does this feature need exposed metal, printed paste, or both? That question is more reliable than assuming that every exposed pad needs an identical paste opening.

Compare Three Geometries, Not Just Two Files

Copper Defines the Conductive Land

The copper layer establishes the physical pad. A mask edit does not enlarge its conductor, and a paste edit does not repair an incorrect land pattern. Start with the component manufacturer's recommended footprint and the exact package variant.

Mask Defines the Exposed Region

For a non-solder-mask-defined pad, the opening extends beyond the copper boundary. For a solder-mask-defined pad, the mask overlaps the copper and defines the exposed area. These are intentional design choices, not interchangeable export settings. Follow the package guidance rather than applying one choice to every component. Texas Instruments discusses both styles in its QFN and SON PCB attachment guide.

Paste Defines the Printing Pattern

The paste aperture may differ from both the copper and mask opening. Consider an illustrative rectangular copper pad measuring 1.00 mm by 0.60 mm. A mask expansion of 0.05 mm on each edge produces a 1.10 mm by 0.70 mm opening. A separate paste inset of 0.03 mm per edge produces a 0.94 mm by 0.54 mm aperture.

Those dimensions demonstrate the geometry only; they are not recommended production settings. The resulting paste area is 0.5076 mm squared, approximately 84.6% of the original 0.60 mm squared pad area. Reducing both dimensions by a percentage therefore does not reduce area by that same percentage. Distinguish linear reduction, area coverage, and paste volume when reviewing a stencil proposal.

Why One Global Clearance Can Be Misleading

CAD tools can combine board defaults with footprint or pad overrides. KiCad, for example, provides separate mask expansion and absolute or relative paste clearances. Review the settings at the level where they actually apply, then inspect the generated result. The KiCad PCB Editor manual documents these controls and manufacturing outputs.

Check the Remaining Mask Bridge

As a simple geometric example, two copper edges separated by 0.20 mm with 0.05 mm outward mask expansion on each facing edge leave a nominal 0.10 mm mask bridge. This calculation is a screening tool, not proof that a supplier can reproduce the bridge. Registration tolerance and the agreed fabrication process still matter.

Keep Exceptions Visible in the Release Review

If one fine-pitch footprint requires different settings, record the exception and inspect its exported openings. Otherwise, a later library replacement or default-setting change can silently alter the production artwork even when the schematic remains unchanged.

QFN Thermal Pads and Vias Need Separate Decisions

Do Not Copy a Large Mask Opening into the Stencil

For exposed-pad QFN packages, stencil thickness and aperture geometry jointly affect deposited paste volume. Dividing the thermal-pad aperture into smaller windows can help control deposition; excessive paste can lift the package and interfere with peripheral joints. Use the exact package recommendation and the assembler's process review rather than a universal coverage percentage. These considerations are covered in the TI attachment guide.

Do Not Treat Via Tenting as Via Filling

A mask instruction alone does not specify a filled and copper-capped via structure. If a via is within an assembly land, identify its required construction in the fabrication notes and review the paste pattern together with that construction. Our via-in-pad design guide explains why this decision belongs in the fabrication and assembly review.

Common Gerber Mistakes and How to Catch Them

Confusing File Names with Verified Layer Functions

Do not release a file merely because its extension looks familiar. Load the complete set, identify each layer's side and function, and compare it against the copper and outline. Gerber attributes can carry layer information; Ucamco maintains the official Gerber format documentation and reference viewer. A clear file manifest is useful alongside the machine-readable data.

Copying Mask Artwork into the Paste File

This loses the distinction between exposed metal and printed paste. During review, inspect representative SMT lands, fiducials, test points, and connector contacts separately. Mark which features intentionally receive paste. Investigate any unexpected agreement between the entire mask and paste files instead of assuming it is correct.

Exporting the Wrong Side or a Different Revision

A visually plausible paste file can still belong to yesterday's layout. Overlay copper, mask, paste, and outline from the actual release archive. Check an asymmetric feature and a known component location on each populated side. Avoid manually mirroring an individual output unless the receiving process explicitly requires it and the transformation is documented.

Leaving Stencil Changes Outside Revision Control

If the assembler adjusts apertures after review, keep the approved stencil data with the manufacturing record. For a repeat order, specify whether that approved stencil remains valid. A board filename alone is insufficient when its associated assembly tooling has changed.

Assuming a Bare-Board File Set Is a Complete PCBA Package

Confirm responsibility for stencil design and include the applicable assembly data: BOM, placement file, population variant, and assembly notes. State whether paste data is a starting point for review or an approved manufacturing output. See the PCB assembly process guide for the broader handoff.

A Practical Pre-Release Checklist

Use these checks on the files that will actually be sent, not only on the open CAD project:

• Verify the board name, revision, outline, units, and common layer alignment.
• Identify top and bottom copper, mask, and paste explicitly.
• Inspect one ordinary SMT footprint and every package with custom mask or paste settings.
• Check intentional mask overlap, narrow bridges, and openings near adjacent copper.
• Review exposed thermal pads and via construction against package and fabrication notes.
• Confirm which test points, fiducials, and connector contacts must remain paste-free.
• Check the BOM and population variant against the intended assembly process.
• Record stencil thickness, aperture changes, revision, and approval responsibility.

For example, if a supplier reports a missing mask bridge, first identify the affected pads and the required exposed geometry. Then evaluate the proposed change with both fabrication and assembly stakeholders. Simply shrinking every mask opening could solve one local issue while changing unrelated footprints.

Conclusion

Solder mask controls exposure on the fabricated board; solder paste artwork controls the intended assembly printing pattern. Neither replaces the copper land pattern. Reviewing all three together makes discrepancies easier to detect before the board or stencil is produced.

The most useful release discipline is to inspect exported files, document package-specific exceptions, and agree on who approves stencil adjustments. A consistent file set and a clear manufacturing record are more valuable than an unverified global clearance rule.

Frequently Asked Questions

Are solder mask and solder paste layers interchangeable?

No. Solder mask data defines openings in the board coating, while paste data describes intended printing apertures for assembly. Review them independently against the copper lands.

Should the paste opening match the copper pad exactly?

Not automatically. Follow the package recommendation and approved stencil design. A different aperture size or segmented pattern may be appropriate for the assembly process.

Does every exposed pad need a paste opening?

No. Exposure and paste deposition serve different purposes. Identify which features are soldered during printing and reflow, and check test points and connector contacts separately.

Can one paste reduction value be used for the entire board?

A global setting can be a starting point, but it does not replace footprint review. Check package-specific overrides and inspect the final exported apertures before release.

Does a tented via count as a filled and capped via?

No. A solder mask instruction does not specify filling and copper capping. State the intended via construction separately in the fabrication requirements.

What should I provide for a PCB and stencil review?

Provide the revision-controlled fabrication files, mask and paste layers, BOM, placement data, assembly notes, and relevant package recommendations. Identify custom apertures and agree on who approves the production stencil.

← Back to Blog