KiCad “Text thickness out of range”: why 0.15 mm becomes 0.125 mm, and how to fix every label at once

The forum report: references 0.5 mm wide and 0.5 mm tall, line width 0.15 mm, a design rule warning below 0.15 mm, and a warning anyway. At 0.6 mm the warning went away. The test board below reproduces it on KiCad 9.0.9 with three library 0603 resistors whose references are 0.5, 0.6 and 1.0 mm tall, all typed with a 0.15 mm line, and the Board Setup minimums set to 0.5 mm height and 0.15 mm thickness:

[text_thickness]: Text thickness out of range (board setup constraints silk text thickness min thickness 0.1500 mm; actual 0.1250 mm)
    Rule: board setup constraints silk text thickness; warning
    @(103.0000 mm, 103.7000 mm): Reference field of R1

Only R1 fails. KiCad keeps your 0.15 mm in the file but draws the strokes at most a quarter of the text’s smaller dimension, and the design rules check reads the drawn width. Measured on the same board for several sizes:

Width counts as much as height: narrow text with full height is capped the same way. The rule of thumb that follows is simple. For a minimum line width T, the text must be at least 4 × T in both directions: 0.6 mm for 0.15 mm, 0.48 mm for 0.12 mm. KiCad’s text dialog has a warning for the same thing, “Text thickness is too large for the text size.”

The minimums live in Board Setup → Design Rules → Constraints, as “Minimum text height” and “Minimum text thickness”. On a new KiCad 9 board they are 0.8 mm and 0.08 mm. With those defaults, the 0.5 and 0.6 mm references fail on height instead:

[text_height]: Text height out of range (board setup constraints silk text height min height 0.8000 mm; actual 0.5000 mm)
    Rule: board setup constraints silk text height; warning
    @(103.0000 mm, 103.7000 mm): Reference field of R1
[text_height]: Text height out of range (board setup constraints silk text height min height 0.8000 mm; actual 0.6000 mm)
    Rule: board setup constraints silk text height; warning
    @(108.0000 mm, 103.7000 mm): Reference field of R2

Both checks apply to silkscreen text only. The same 0.5 mm text with a 0.05 mm line on a copper layer and on the fabrication layer produced no warning; on the silkscreen it produced both. Both are warnings by default: kicad-cli pcb drc lists them unless you pass --severity-error, and a check that only counts errors lets the board through.

For reference, new silkscreen text in KiCad 9 defaults to 1.0 mm with a 0.1 mm line, and the library’s 0603 resistor carries its reference at 1.0 mm with a 0.15 mm line. The fabrication layer copy of the reference is 0.4 mm with a 0.06 mm line, which is fine because nothing prints it.

A design rule should be your fab’s number, not a guess. Two common fabs publish theirs:

The 0.15 mm line in the forum report matches both fabs. At either fab, the 0.5 mm text is also below the minimum height, which KiCad would only report if the height minimum were set to match. A library reference, 1.0 mm with a 0.15 mm line, meets both. A reply in the same thread reports 0.64 mm tall text with 0.13 mm lines coming out readable from three US fabs, though the poster needs a loupe to read it. Smaller is possible, but it is the fab’s promise that matters, so set both minimums from its capabilities page and let DRC hold you to them.

Ticking Bold replaces your line width with one fifth of the text size. Above 0.75 mm that is thicker than 0.15 mm; below it, thinner. A 0.6 mm reference passes at 0.15 mm, but in bold it is drawn 0.12 mm wide:

[text_thickness]: Text thickness out of range (board setup constraints silk text thickness min thickness 0.1500 mm; actual 0.1200 mm)
    Rule: board setup constraints silk text thickness; warning
    @(108.0000 mm, 103.7000 mm): Reference field of R2

Bold 0.5 mm text gets a 0.1 mm line. If you want heavier small labels, make them larger rather than bold.

Edit → Edit Text & Graphics Properties opens a dialog that edits many items in one pass. Tick Reference designators, plus any other footprint fields that print, enter the new size and line width, or use “Set to layer default values” to apply the defaults from Board Setup, then apply. Filters narrow it by layer, net, net class or reference designator, which helps when only the tiny parts need changing.

Outside the editor, the same fix is a few lines of pcbnew Python. This script raises every visible silkscreen field below the smallest size that passes the board’s own minimums, and leaves larger text alone:

import sys, pcbnew
b = pcbnew.LoadBoard(sys.argv[1])
ds = b.GetDesignSettings()
# KiCad draws a line at most 1/4 of the text size, so the smallest size that passes is
# the larger of the minimum height and 4 x the minimum thickness.
low = max(ds.m_MinSilkTextHeight, 4 * ds.m_MinSilkTextThickness)
for fp in b.GetFootprints():
    for f in fp.GetFields():
        if f.IsVisible() and f.GetLayer() in (pcbnew.F_SilkS, pcbnew.B_SilkS):
            s = f.GetTextSize()
            if min(s.x, s.y) < low:
                f.SetTextSize(pcbnew.VECTOR2I(max(s.x, low), max(s.y, low)))
pcbnew.SaveBoard(sys.argv[1], b)

On the forum board it raised R1 to 0.6 mm, and on the defaults board R1 and R2 to 0.8 mm. DRC came back with 0 violations on both. Placement is still yours: larger references need room, so check for the warnings below afterwards.

Resizing labels often causes the other two silkscreen warnings. On the same board, R1’s reference was moved onto its own pad and R3’s onto R2’s:

[silk_over_copper]: Silkscreen clipped by solder mask
    @(102.1750 mm, 105.0000 mm): Reference field of R1
[silk_overlap]: Silkscreen overlap
    Rule: board setup constraints silk; warning
    @(108.0000 mm, 103.7000 mm): Reference field of R2
    @(108.6000 mm, 103.7000 mm): Reference field of R3

“Silkscreen clipped by solder mask” means part of the label sits inside a solder mask opening. Ink cannot go on copper that will be soldered, so that part is cut away and the label prints incomplete. JLCPCB asks for 0.15 mm between pads and silkscreen. “Silkscreen overlap” means two silkscreen items print on top of each other. Move the labels, or put the dense ones on the fabrication layer and keep the silkscreen for what someone holding the board needs to read.

PCBEditor draws every label with KiCad’s stroke font and the same cap, a line no wider than a quarter of the text size, so the line width on screen is the one in the fab files. A label’s line is 15% of its height, raised to the board’s minimum silkscreen width. Its rules check reports a label printed over a pad, using the label’s real strokes and the pad’s real outline. When you export to KiCad, Board Setup carries a 0.8 mm minimum text height and a minimum text thickness equal to the board’s silkscreen minimum, so KiCad checks the same numbers.

It has no text height, text thickness or silkscreen overlap check of its own; after export, KiCad’s DRC is the one to read for those. The Gerber checklist covers what to look at on the silkscreen layer before ordering.