Via Stitching

A KiCad action plugin that fills the overlap of a net's copper zones (the top and bottom GND pours, for example) with a grid of stitching vias. Through, micro, blind, and buried vias are all supported, spanning whichever two copper layers you pick. Works on KiCad 6, 7, 8, 9, 10, and later.

_{Board: the kit-dev-coldfire demo that ships with KiCad.}

Quick start

1. Fill the zones (B) so the pours have copper to read. "No filled copper for net ..." means this step was skipped.
2. Run Via Stitching from its button on the PCB editor's top toolbar, then pick the net (GND by default) and the via size.
3. Check the preview and click OK. The zones are refilled for you.

Install

From the Plugin and Content Manager: Tools > Plugin and Content Manager > Plugins, find Via Stitching, install it, and restart the PCB editor. It hands your KiCad the build it can run (see Two builds).

Manually: from the Releases page download via-stitching-x.y.z.zip for KiCad 10 and later, or via-stitching-swig-x.y.z.zip for KiCad 6 to 9. Install it with Tools > Plugin and Content Manager > Install from File..., or unzip the plugins/ contents into Documents/KiCad/<version>/3rdparty/plugins/via_stitching/. On KiCad 10 and later, then use Tools > External Plugins > Refresh Plugins.

Requirements

• KiCad 10 and later: the IPC API server, enabled under Preferences > Plugins. KiCad installs kicad-python, wxPython, and shapely itself on first run, from requirements.txt.
• KiCad 6 to 9: shapely, which KiCad doesn't ship. If the plugin reports it missing, install it into the Python KiCad uses:
  • Windows: "C:/Program Files/KiCad/<version>/bin/python.exe" -m pip install shapely
  • Linux, where KiCad uses the system Python: sudo apt install python3-shapely on Debian and Ubuntu. The Flatpak build of KiCad has not been tested.

Usage

Select an existing via before running the plugin to copy it: its type, layers, net, diameter, and drill pre-fill the dialog. Otherwise the dialog starts from what you set last time. Reset settings puts the built-in defaults back.

The settings that need explaining:

• Via Type: Through, Micro, Blind, Buried, or Blind/Buried. The start and end layer are free for every type except Through, which is always F.Cu to B.Cu. An unusual pairing, such as a microvia that doesn't touch an outer layer, shows a warning in the dialog but doesn't stop you.
• Via Pattern: Hexagonal (densest), Square, or Staggered. Spacing is the center-to-center pitch.
• X-Offset / Y-Offset shift the grid, so a second pass on the same net and area doesn't land on the first. Useful for separate front-side and back-side microvia passes, for example.
• Avoid footprints keeps vias out from under component bodies, for mechanical fit. It's off by default, because thermal-via arrays under a QFN or BGA ground pad are a normal use of stitching.
• Avoid zones of other nets and Avoid pads already on this net are covered under How clearance is handled.

Vias go where the net is poured on both layers the via connects. A through via only needs any two poured layers in its span, since its barrel crosses them all.

The preview

The right half of the dialog shows the run before anything is placed: the copper being stitched, every via at its real size, and in orange the ones moved off the grid to clear a pad or track. It redraws a moment after any setting changes and keeps your zoom while the copper stays the same. Scroll to zoom, drag to pan, double-click to fit. A setting that can't be stitched, such as a drill wider than the via or a net with no copper, is reported there, with the last good preview left in view. OK reads the board again, so editing the board after the last preview never places stale vias.

Grouping and undo

All the vias from one run go into a group named after it, for example ViaStitching GND F.Cu:B.Cu. That makes a run one thing rather than four hundred:

• Reset last run, at the top of the dialog, deletes the newest run and refills the zones. It names the run and its via count beside the button, asks before deleting, and only touches vias this plugin placed and grouped.
• Click any via to select its whole group, then press Delete.
• To delete one via, right-click it, choose Grouping > Remove from Group, then delete it.

On KiCad 10 and later Ctrl+Z also undoes a whole run, until the board is saved and reopened. On KiCad 6 to 9 a plugin can't put anything on KiCad's undo stack, so Reset last run is the only undo there.

How clearance is handled

There's no clearance field, on purpose. A via's drill crosses every copper layer in its span: the whole board for a through via, only the layers it connects for a micro, blind, or buried via. Six things keep the vias legal:

• The fill inset. A via sits at least its own radius (plus a small epsilon) inside the fill on every layer the net is poured on. KiCad has already pulled those fills back by the board clearance, so this keeps the via off other-net copper on those layers.
• Other nets' tracks are avoided on every layer in the span, poured or not. A via on another net's track is a real DRC error, so this is always on.
• Other nets' pads are avoided the same way. The keepout follows the pad's rotated rectangle, so a large rectangular pad doesn't also block the pour at its corners. A through-hole pad blocks any span; an SMD pad only blocks a span that includes a layer it has copper on.
• Rule areas that forbid vias are respected on every layer in the span, whichever layers they were drawn on.
• Existing holes: via and pad drills get a 0.25 mm hole-to-hole margin. A milled slot gets a capsule along its long axis, not a circle as wide as the slot is long. An existing via only counts if its layer span overlaps the new via's, so a front-side microvia pass doesn't block a back-side one.
• Clearance values come from the board's netclasses, taking the larger of the two nets involved, as KiCad's own rules do. A netclass that inherits the board minimum reports no value of its own, so those fall back to 0.2 mm.

A blocked grid position isn't dropped. The via moves to the nearest clear spot within a quarter of the spacing, so the grid keeps its coverage beside pads. The hole-to-hole margin caps that distance too, so two neighbors moved toward each other still clear each other's drills, and a grid with no room to spare stays exactly on pitch.

Avoid zones of other nets is off by default, because a via through another net's zone is not a DRC error: KiCad pulls that fill back around the via during the refill. Tick it if you'd rather not perforate an inner power plane at all, and expect far fewer vias, since on a typical 4-layer board that plane covers most of the board.

Avoid pads already on this net is off by default, so a via array can land on a same-net ground pad. Tick it to keep vias off same-net pad copper too. Pads on other nets are avoided either way, with their full clearance.

Known limitations

• The KiCad 10 build needs the IPC API server (see Requirements). Without it the plugin can only tell you to switch it on.
• On KiCad 10 and later the plugin has only its toolbar button, no entry under Tools > External Plugins. KiCad lists only the older SWIG plugins there, and plugins on the new API have no way to add one. The KiCad 6 to 9 build shows up in that menu as usual.
• On a large board each preview update can take a few seconds, and the dialog waits for it. Untick Update automatically and use Update preview to redraw only when you ask.

Localization

The dialog follows KiCad's own language setting (Preferences > General): English, Dutch, German, French, or Chinese (Simplified), and English for anything else. The catalogs are in plugins/locale/, keyed by the English strings and shared by both builds.

Two builds

KiCad	Build	Sources	Version numbers
10 and later	IPC (kicad-python / kipy)	plugins/	3.x
6, 7, 8, 9	SWIG (pcbnew bindings)	plugins_legacy/	1.x

KiCad is retiring the SWIG bindings: KiCad 10 already lacks the via type constants this plugin needs, and KiCad 11 removes the bindings altogether. KiCad 6 to 8 have no API server, and KiCad 9's is missing the call the IPC build uses to check that the board kept its vias. The two APIs even number copper layers differently, so each build is its own implementation of the same dialog, tested against the KiCad versions it claims (the SWIG build on real KiCad 6, 7, 8, and 9 in CI). The SWIG version number always stays lower, so moving from KiCad 9 to 10 arrives as an ordinary package update.

Development

python build.py builds dist/via-stitching-<version>.zip (IPC), and python build.py --legacy builds dist/via-stitching-swig-<version>.zip (SWIG). Each writes its archive's SHA-256 and sizes into metadata.json. One tag builds and publishes both, and tools/check_release.py refuses a tag that disagrees with metadata.json.

Tests live in tests/ipc/ and tests/legacy/. The IPC suites run offline against a fake board. The SWIG suites need a real pcbnew, so run those with KiCad's own interpreter:

"C:/Program Files/KiCad/6.0/bin/python.exe" tests/legacy/test_helpers_legacy.py

License

GPL-3.0-or-later. Independent IPC re-implementation of the via-stitching idea from JS Reynaud's earlier plugin.