Advanced Manufacturing

Solder Paste and Stencils

Solder Paste Stencils

Hand-soldering surface-mount components one pad at a time works, but it is slow and joint quality depends heavily on technique. For boards with many SMT parts, or when assembling more than a couple of boards, a solder paste stencil is the right approach. It is the same process used in industry.

A stencil is a thin sheet of laser-cut stainless steel with apertures punched at the position and size of every SMD pad on the board. When the stencil is aligned over the bare PCB and solder paste is squeegeed across it, paste is deposited through the apertures onto the pads only. Lift the stencil, place the components, and reflow. The paste wicks to the pads and solidifies into joints.

KiCad generates the paste layer data automatically. Every SMT pad in a footprint has a paste aperture defined by the F.Paste (front paste) or B.Paste (back paste) layer. When you export Gerbers, include these layers in the package. Stencil manufacturers accept the paste Gerber directly and use it to cut the apertures. Most PCB fabrication houses that also offer stencils (JLCPCB, PCBgogo, OSH Stencils) accept the paste layer from your standard Gerber export.

For footprints with exposed thermal pads (a power regulator with a large ground tab, for instance), the paste aperture is typically sized to around 50-70% of the pad area, divided into a grid of smaller squares. This prevents outgassing from causing bridging or voids during reflow. KiCad footprints from reputable libraries will have this configured correctly. Check any custom footprints you create.

The Reflow Process

Reflow soldering with a stencil follows a fixed sequence. Each step matters:

• Align and jig the board. Tape the bare PCB to a flat surface and align the stencil over it until the pad copper is visible through the apertures. For batches of more than one board, build a simple jig from spare unpopulated boards to hold each board in exactly the same position under the stencil.
• Apply paste. Deposit a small bead of solder paste along one edge of the stencil and squeegee it across with a flat metal scraper (a paint scraper works well, provided it has no sharp corners that could catch the stencil). Keep firm, even pressure. One or two passes is enough. Overworking the paste degrades it.
• Lift the stencil. Peel the stencil back without sliding it laterally. The paste should sit in clean deposits on each pad. Paste that smears between pads or bridges across fine-pitch pins indicates misalignment or too much paste pressure.
• Place components. Set each SMT component into the paste with tweezers. The paste is tacky enough to hold parts in position. If you are populating several components, orient the board so you work from one end to the other without reaching over already-placed parts.
• Reflow. Apply heat with a hot plate, reflow oven, or hot air station. The paste activates flux, melts, and wets to the pad. Components will self-align slightly as the solder reflows due to surface tension. Allow the board to cool before handling.

Design boards with components on one side only if you intend to use paste and stencil. Two-sided SMT assembly requires reflowing one side and then the other, which means the first-side joints re-melt when the second side is processed. This adds complexity to bench assembly that is difficult to manage without proper fixturing.

If you are using leaded solder paste, wear gloves and wash your hands after handling it. The paste form makes lead significantly more bioavailable than solid solder wire.

Automated Assembly (PCB-A)

Automated PCB Assembly (PCBA)

Most low-cost PCB fabrication houses now offer assembly alongside bare board fabrication. You submit Gerbers as normal, plus a bill of materials and a component placement file, and receive fully assembled boards. For designs with fine-pitch ICs or large component counts, this is often faster and more reliable than hand assembly. At quantities of five or more boards, the cost per board is often comparable to buying the parts separately.

PCBA requires two additional output files from KiCad:

• Bill of materials (BOM). The BOM lists every component on the board: reference designator, value, footprint, and a manufacturer part number (MPN) or supplier part number. Export it via File > Fabrication Outputs > BOM, or via scripted plugins such as the JLC/LCSC BOM plugin which formats the output for JLCPCB's upload tool. The more specific your part numbers, the less back-and-forth with the manufacturer. Add a LCSC field (or equivalent) to schematic symbols for parts you have already sourced. Avoid supplier order codes specific to a single distributor's catalogue. An MPN is portable across suppliers.
• Component placement file (centroid / pick-and-place). This file tells the pick-and-place machine the X/Y position, layer, and rotation of every component. Generate it from File > Fabrication Outputs > Component Placement. KiCad outputs a CSV with columns for reference, value, package, X position, Y position, rotation, and layer. Some manufacturers require a specific column order or header format. Download their template and compare. You can usually reformat by copying columns from the KiCad CSV into the manufacturer's template.

When reviewing the assembled BOM on the manufacturer's portal, check that each component has been matched to the correct part. Manufacturers will attempt to match generic descriptions (e.g. "100nF 0402 10V") from their parts library, but they may select an alternative that differs in a way that matters: voltage rating, tolerance, or case size. For critical components such as crystals, ICs, precision resistors, and current-sense resistors, specify the exact MPN and confirm it in the portal before approving the order.

Parts not in the manufacturer's library, or parts they do not stock, must be handled separately. Either order them yourself and ship them to the manufacturer as customer-supplied parts (this adds cost and lead time), or find an equivalent in their catalogue. Flag any such parts early in the design process so the sourcing decision does not block the order.

Once you have submitted a successful order and confirmed the BOM, reordering is straightforward. The order history preserves your exact part selections, so you can reorder without reworking the BOM from scratch.