Silkscreen clipped by solder mask

Diagnostic signature

Silkscreen clipped by solder mask

KiCad emits this DRC warning when a silkscreen object intersects with a solder mask opening for a pad or via, which can lead to illegible markings or defective solder joints during manufacturing.

What it means

In KiCad's Design Rule Check (DRC) system, this diagnostic indicates that a silkscreen element—such as a line, polygon, or text item—physically overlaps with a solder mask opening. During printed circuit board manufacturing, solder mask openings dictate where bare copper is exposed for components to be soldered. If silkscreen ink prints directly over these exposed copper areas, it can contaminate the pad and cause poor or rejected solder joints. To prevent assembly defects, many PCB fabrication houses automatically clip (remove) any silkscreen ink that falls within a solder mask aperture, or discard silkscreen layers entirely if they are unsupported by solder mask. Consequently, the final manufactured board may suffer from truncated, broken, or completely illegible reference designators and symbols.

Why it happens

The PCB Editor emits this warning when a footprint's reference designator, value, or a custom silkscreen graphic is positioned too closely to a surface mount (SMD) or through-hole (PTH) pad, causing its bounding box or stroke width to enter the pad's solder mask clearance. This frequently occurs immediately after importing components from a schematic, as parts may be placed in a tight default grid, forcing one footprint's text over an adjacent footprint's pads. It also commonly happens when users manually move text to make room on a dense board without respecting the clearance boundaries. Furthermore, poorly authored custom footprint libraries—where the courtyard or silkscreen geometry fails to leave adequate margins around the solder mask expansions—will persistently trigger this diagnostic when placed on the board. The internal KiCad engine evaluates this using the `silk_over_copper` rule.

Minimal reproduction

(kicad_pcb (version 20240108) (generator pcbnew)
  (footprint "Resistor_SMD:R_0805_2012Metric"
    (layer "F.Cu") (attr smd)
    (fp_text reference "R1" (at 0 0) (layer "F.SilkS")
      (effects (font (size 1 1) (thickness 0.15)))
    )
    (pad "1" smd roundrect (at -0.9375 0) (size 0.975 1.4) (layers "F.Cu" "F.Paste" "F.Mask"))
    (pad "2" smd roundrect (at 0.9375 0) (size 0.975 1.4) (layers "F.Cu" "F.Paste" "F.Mask"))
  )
)

How to fix it

Reposition the silkscreen item to clear the solder mask opening, or edit the footprint to permanently correct the silkscreen layout.

```KiCad PCB
(kicad_pcb (version 20240108) (generator pcbnew)
  (footprint "Resistor_SMD:R_0805_2012Metric"
    (layer "F.Cu") (attr smd)
    (fp_text reference "R1" (at 0 -1.5) (layer "F.SilkS")
      (effects (font (size 1 1) (thickness 0.15)))
    )
    (pad "1" smd roundrect (at -0.9375 0) (size 0.975 1.4) (layers "F.Cu" "F.Paste" "F.Mask"))
    (pad "2" smd roundrect (at 0.9375 0) (size 0.975 1.4) (layers "F.Cu" "F.Paste" "F.Mask"))
  )
)
```

Step 1

• Run the DRC tool in the PCB Editor and select the 'Silkscreen clipped by solder mask' warning to highlight the offending item.

Step 2

• Click the highlighted silkscreen text or graphic on the PCB.

Step 3

• Press 'M' to move the object, positioning it completely outside the perimeter of the pad's solder mask clearance.

Step 4

• If the text is too large to fit in the available space, edit its properties (press 'E') and reduce the text width, height, and thickness.

Step 5

• If the violation is built into a library footprint, open the footprint in the Footprint Editor, modify the silkscreen lines to ensure adequate clearance, and update the footprint on the board.

Upstream references

PCB Editor | 8.0 | English | Documentation - KiCad Docs

KiCad PCB EDA Suite: drc_item.cpp Source File

No control over packing of footprints on initial import from Update PCB from Schematic (#22302)