How to Make a Solder Paste Stencil in Protoboard Designer

Estimated reading time: 9 minutes

A stencil is a thin sheet with a hole over every pad you want to solder. You lay it on the bare board, wipe solder paste across it, lift it off, and the paste is left exactly on the pads, ready for the parts and the oven. It is what makes small surface-mount (SMD) parts practical.

Protoboard Designer works out the holes for you. You never draw them: each pad's opening comes from the pad itself, and you only change it where the default is wrong. Then you either order the stencil from a factory or cut one at home.

How the openings are decided

Only SMD pads get paste. Through-hole pads, vias, tracks and copper pours never do, and neither does a pad that is covered by the solder mask. For the rest, each pad has a Solder paste setting:

Setting	What it does
Auto (the default)	Decides from the part. A fiducial gets no paste. A large exposed pad in the middle of a chip (the QFN's heat pad) and a large tab (a DPAK's) get windows. Everything else is opened in full.
Full	The opening is the pad.
Off	No paste on this pad.
Windows	Splits the opening into a grid of smaller ones, Across by Down, that together cover the Coverage percentage of the pad.

Why windows? A big pad with paste over all of it floats the part on a pool of molten solder and squeezes it sideways. Several smaller openings (about 65 % of the pad is what KiCad's own libraries use) keep the part where you put it. Parts from the library already carry the numbers from KiCad.

Paste never covers a via or a drilled hole. If a pad has vias in it, the openings are laid in the spaces between them, at least 0.1 mm away. This is stricter than KiCad's own thermal-via footprints; open vias draw paste away from the pad and leave voids under it.

Change one pad

1. Select an SMD pad, or open a part's pad list.
2. In the side panel, open Solder paste and choose Auto, Full, Off or Windows.
3. For Windows, set Across, Down and Coverage (%). A small drawing shows the openings that will be cut, over the pad's outline.

Changing several pads at once is one step in the undo history.

Auto already knows the common cases

Check the preview on your QFNs, DPAKs and chips with a big pad before you change anything. Most boards need no changes at all.

Change the whole board

Select the board and open Solder paste in the board panel:

• Paste margin makes every opening bigger (positive) or smaller (negative) on every side. Many boards use a little negative margin to keep paste off the edges of the pads. Leave it at 0 if your fab applies its own.
• Stencil thickness is the foil's thickness, 0.12 mm by default. It does not change the openings. It is only used to check that the paste will release (below).

Order a stencil from JLCPCB

1. Open the Export tool from the left toolbar and choose Export Gerber Files. The two paste layers, Solder Paste Top and Solder Paste Bottom, are ticked by default.
2. Look at the Stencil section that appears while a paste layer is ticked. It checks the board (see the checks). It never stops you from exporting.
3. Export the zip. The paste files are .gtp (top) and .gbp (bottom), or F_Paste and B_Paste with KiCad naming. A side with no SMD pads gets an empty file while Generate empty layers is on, which it is by default.
4. On JLCPCB, start a stencil order (not a PCB order) and upload the zip when it asks for your Gerber files. Choose the options it offers, such as the foil thickness and the frame, and look at the paste layer in the preview before you pay: you should see an opening over every pad you want soldered, windows over the big pads, and nothing over fiducials and vias. 0.12 mm is the stencil thickness this app assumes; if you order a different foil, set the same value under Stencil thickness (above) so the checks match.

Paste files are never mirrored: they are seen from the top like every other fabrication layer, and the factory takes care of the side. The factory also takes care of its own laser's beam width, so the Gerber is always the true size. The laser setting below does not touch it.

If you also want the factory to assemble the board, the parts list is a separate export: see How to make a parts list.

Cut a stencil at home with a laser

A hobby laser cutter can cut a stencil from a thin sheet of Kapton or Mylar. Protoboard Designer exports the cut file as a PDF, or as an image if your software prefers to trace one.

1. Open the Export tool and choose PDF export.
2. Pick the preset Solder Paste Stencil. It selects Solder Paste Top, turns on the board outline and the 1:1 scale lock, and turns off everything that would add marks you do not want. For the bottom side, open Special layers and tick Solder Paste Bottom instead.
3. Fill in the Laser kerf in the Laser cutting section (below), then export. The file is named with the kerf (for example my-board_kerf0.04.pdf), so a compensated file is never mistaken for a true-size one.
4. Import the PDF into your laser software at 100 %. Check the board outline against the real board before you cut.

An image export does the same for software that traces a picture: in the image exporter choose black-and-white and tick the paste layer.

Black cuts and blue guides

The openings are black: those are the cuts. Everything else on the page is pure blue (#0000FF): the board outline, the registration marks, the ruler and the footer. In your laser software, put blue on its own layer and set it to skip, or to score lightly, so the outline helps you line the sheet up without being cut out.

The page is never inverted: even if you ticked Inverted, a stencil has black openings. The bottom page is the board as seen from the top; turn the sheet over, or tick Mirror, if your software wants the view from below.

Laser kerf

A laser burns away a strip as wide as its beam, the kerf, along the line it follows. A hole cut along a pad's outline therefore comes out one kerf too big: with a 0.1 mm kerf, a 0.5 mm opening comes out 0.6 mm wide. The Laser kerf (beam width), mm field fixes that: every opening is drawn half a kerf smaller on each side, so it comes out at its true size.

Set the kerf once, in one place

If your laser software also has a kerf or offset compensation, leave it at zero, or leave the field in Protoboard Designer at 0. Do not set both: the correction would be applied twice and every opening would come out too small.

A line of text under the field says what it does to your board, for example Each opening is cut 0.05 mm smaller on every side: the narrowest, 0.30 mm, is cut at 0.20 mm.

Measure your kerf with the test strip

You do not need to know the beam width in advance.

1. Set the kerf to 0 and turn on Add a kerf test strip. The strip is a 10 mm square and four slots 0.2, 0.3, 0.4 and 0.5 mm wide, printed below the board at full size.
2. Cut the sheet with your usual settings.
3. Measure the 10 mm square with calipers, in a few places, and take the average. Your kerf is the measured size minus 10 mm: a hole that measures 10.06 mm means a kerf of 0.06 mm.
4. Type that into Laser kerf, export again with the strip still on, and cut a second time. The square should now measure 10.00 mm. If it is still off, add the difference to the kerf.

Once the kerf is set, a slot narrower than the beam is cut as a single line, which is the smallest hole your laser makes. The checks below name any real opening in that position.

If there is no room for the strip on the paper, it is left out, and the dialog says so.

The checks

Two sections list what is worth knowing before you order or cut. The Stencil section of the Gerber export covers the first two checks; the Laser cutting section of the PDF and image exports covers the rest. None of it blocks an export.

• Paste may not release from these pads. The openings' area ratio (the opening's area divided by the area of its walls at your stencil thickness) is below 0.66, the usual limit. A thinner foil or a bigger opening helps. Pads are named by part and pin, like R7 2.
• Open solder mask but no paste. These pads have no paste, but their solder mask is open. A factory may ask about them. Fiducials normally appear here, and that is fine.
• Narrower than the beam (laser only). These openings are smaller than the kerf and are cut as a single line, which is the smallest hole your laser can make.
• Strips of foil between openings under 0.15 mm (laser only). A web of foil that thin tears when you lift the stencil or wipe the paste. The check counts the pairs and tells you the narrowest.
• The correction is smaller than one pixel (image export only). Use the PDF export, or a higher resolution.

Good to know

• The test strip is not mirrored on a mirrored page, and the kerf is always in millimetres, even if you work in inches.
• The strip's label is in Latin letters only, whatever your language: the PDF's built-in font has no others.
• A board imported from KiCad or Eagle keeps the paste data of its source where it has any, and Eagle pads marked "no cream" get no paste. A footprint imported on its own can be off by the board's paste margin.
• Boards saved before this feature have no paste settings, and the Auto rules apply.

Related guides

• How to Export Gerber Files
• How to Export a PDF
• How to Order a PCB
• How to Make a Parts List