Compatibility

20. KiCad And Solver Compatibility

20.1 KiCad Files

KiCad	File format number of the release	Status
older	no (version ...)	read best-effort with a warning, as format 20201115, as KiCad reads such a file
BZR builds of 2013-2014	3	the lower end of the tested range (Run.KICAD_VERSION_MIN); 6 public boards; the layer names those builds wrote in Italian, Polish and French are understood
4	4	19 public boards saved by KiCad 4
5	20171130	25 public boards saved by KiCad 5; KiCad 5 arcs (start = centre, angle), zones filled with segments only (fill_segments), net names written with the old overbar (~RESET~)
6	20211014	25 public boards, among them development builds of 6 (formats 20201116 to 20210925, read as KiCad 6); featureTest/20a_format_kicad6, written by hand in KiCad 6's format
7	20221018	25 public boards; the three example boards of Input/, tests/boards/synthetic and most of featureTest/, saved by KiCad 7 itself
8	20240108	25 public boards; tests/boards/one_layer and featureTest/20c_format_kicad8, small hand-written files in KiCad 8's format
9	20241229	25 public boards; tests/boards/six_layer and featureTest/20d_format_kicad9, likewise hand-written; per-via (tenting front back) is parsed; tracks and drawings left bare by the solder mask, (layers "F.Cu" "F.Mask") with an optional (solder_mask_margin ...), are read (in featureTest/08b_copper_graphics_nets)
10	20260206	the upper end of the tested range (Run.KICAD_VERSION_MAX); five hand-written feature boards (03b_vias_k10, 06_padstacks, 08b_copper_graphics_nets, 19b_skipped_items_k10, 20e_format_kicad10); net names stored directly on items and per-via (tenting (front yes) (back no)) are read
newer	above 20260206	read best-effort with a warning; raise Run.KICAD_VERSION_MAX once checked. A bold text's thickness after format 20260826 is read as its base pen, drawn 1.6 times as wide, as KiCad's development version does

The 150 public boards (25 for each release from 4 to 9, six of the "KiCad 4" ones saved by the builds before it) were downloaded for testing and are not kept in the repository; every complete one of them runs, and the Verifier passes on all but one, whose file places two pin headers of different nets on the same spot. One more KiCad 5 file is cut short (it ends inside a pad) and is refused with a message that says so, as KiCad refuses it. Every rule that depends on the version is in one file, kese/s1_read/parse_kicad_version.py, and follows KiCad's own board parser:

Rule	Files it applies to
copper layers are read by their place in the leading run of copper layers (first = F.Cu, last = B.Cu, inner ones In1.Cu, In2.Cu, ... unless already named so)	every version; KiCad 3 to 5 files whose layers the user renamed get a warning that lists them
a text with no size is 1.524 mm (60 mils)	KiCad 4
a solder_mask_margin of 0 means "use the board's value"	up to format 20240201 (KiCad 8)
an overbar is text between two ~, converted to ~{...}	before format 20210606 (KiCad 5 and early 6)
a zone fill is drawn with a pen of min_thickness	before format 20250210, unless the zone says (filled_areas_thickness no)
a zone with only fill_segments is filled with those segments	KiCad 4 and 5
via tenting and protection off unless stated	before format 20250228
a bold text's thickness is its base pen	after format 20260826

What is read from the file is listed in Checks, Errors And Warnings; KiCad itself is not needed, only the .kicad_pcb file. Footprints are read from the board file (KiCad embeds them), so libraries are not needed either.

Board feature	Support
Copper layers	boards with 2, 4, 6 and 8 declared copper layers are in the repository (one of them single-sided: tracks only on F.Cu, and on B.Cu only its two through-hole pads); more than 8 are modelled with a warning; F.Cu and B.Cu must be declared. copper layers are read as KiCad reads them, by their place in the list: the first is F.Cu, the last B.Cu, and the ones between In1.Cu, In2.Cu, ... unless already named so; a file whose copper layers the user renamed ((0 TOP_L1.Sig mixed), (1 GND.Cu power)) gets a warning that lists the names; a signal-typed User.n layer after the copper is not copper
Stack-up from Board Setup	thickness, type, material, εr, tanδ per dielectric; copper thickness per layer; mask thickness; mask and silk colours; copper finish; edge plating and castellated pads flags
Tracks, arc tracks, vias (through, blind, buried, micro)	yes; "remove unused layers" with KiCad 7+'s zone_layer_connections, and KiCad 10's start_end_only; a track the solder mask leaves bare (KiCad 9 and later) opens the mask over itself, grown by its own mask margin or the board's pad-to-mask clearance
Pads: circle, rect, oval, roundrect, trapezoid, custom	yes; round and oval drills, drill offsets (which move the copper, not the hole), per-pad mask margins; chamfered corners; copper rings on non-plated holes where KiCad flashes them; "remove unused layers" on through-hole pads
Zones	stored fills only (fill in KiCad first); rule areas skipped; KiCad 5 fills drawn with a pen of min_thickness grown by half of it, as KiCad does on reading
Graphics: line, arc, circle, rect, polygon (with arc segments), Bézier, ellipse and elliptical arc (KiCad's development version)	on copper, mask and silk layers; outline from Edge.Cuts; rectangles with rounded corners (KiCad 10), on every layer and on Edge.Cuts; copper drawings the mask leaves bare (KiCad 9 and later) open it as tracks do
Text: gr_text, fp_text, footprint properties	KiCad's stroke font and layout; markup drawn as KiCad draws it (~{overbar}, ^{superscript}, _{subscript}, nested); the pen KiCad uses when the file gives none (a fifth of the width for bold, an eighth otherwise), and never more than a quarter of the smaller of width and height; knockout text; TrueType faces from the glyphs KiCad saves with them (render_cache), else with the stroke font
Text boxes, dimensions, images, groups, tables, generated items; grid items, drill charts and drill maps (KiCad's development version)	skipped; counted when they sit on a copper, silk or mask layer (text boxes, dimensions) or at the top level of the file (images, groups, tables, generated items, grid items, drill charts, drill maps), otherwise left out without a count. For groups and generated items (such as length-tuning patterns) only the record itself is skipped: the tracks, footprints and graphics they hold are read as usual
Footprint 3D models	skipped (bare board)
Padstacks (KiCad 9 and later: another pad or via shape on the inner layers or on the back)	yes: front / inner / back and custom (per layer) modes; each copper layer gets its own pad shape or via size; the back mask opening follows the back shape
Backdrills, tertiary drills, counterbores and countersinks of pads and vias; covered, plugged, capped and filled vias, also when the board setup makes them so (KiCad 10)	not modelled: the hole is drilled and plated through its whole span and left open; counted under skipped in report.txt, with a warning
Item kinds KESE does not know	skipped; counted under skipped in report.txt as <kind> items (unknown to KESE), with a warning
Hatched fills of graphics (KiCad 10)	not modelled: the shape is drawn as its outline only
Edge connector flag of Board Setup ((edge_connector yes) or bevelled)	not read: the fingers are the pads they are, and a bevelled edge stays square
Rigid-flex, multiple stack-up regions	not modelled

20.2 Output Formats

Format	What is in it	Units	Written by
GLB (binary glTF 2.0)	one mesh per part, PBR materials, vertex normals, bufferView targets	Run.UNITS (viewers expect m)	KESE (kese/s7_write/glb.py)
STEP AP214	one named shape per part whose role is in Run.STEP_WRITE_ROLES: the part's closed solids from stage 6, one per separate body, with planar faces (curves are polygons, as in the meshes), or with Run.STEP_EXACT_ARCS circular arcs (CIRCLE) and cylindrical walls (CYLINDRICAL_SURFACE) where the outline is round; mask and silk off by default	Run.UNITS: the file declares millimetres or metres	KESE (kese/s7_write/step.py)
STL (binary)	one file per part	Run.UNITS	KESE (kese/s7_write/stl.py)
OBJ + MTL	one object per part, normals, colours	Run.UNITS	KESE

Visual mode writes GLB and OBJ only.

20.3 Tools

None of these imports has been tried with KESE output yet: the routes follow each tool's documented import formats and the presets in parameters/run.py, and are to be confirmed. Research underway.

Tool	Route	Notes
Ansys HFSS	STEP, mm, KiCad origin (--for hfss)	one solid per net and dielectric to assign materials and ports
CST Studio Suite	STEP, plus STL per part (--for cst)
openEMS / CSXCAD	STL per part, mm (--for openems) with materials.json	openEMS Workflow
COMSOL, FEKO	STEP, mm
FreeCAD, Fusion, SolidWorks, Onshape	STEP	vias and round pads are faceted, as in the meshes
Blender	GLB or OBJ (visual mode for renders)
<model-viewer>, three.js	GLB, m, centred (--for viewer)	the visual-mode skin is made to avoid z-fighting (Output Modes)
Thermal / FEA tools reading STL (CalculiX, Elmer with a mesher)	STL per part, mm	closed solids per part (a part can hold several separate bodies); mesh them with the tool's own mesher

20.4 Python And Packages

	Version
Python	3.12 or later with the pinned versions (numpy 2.5.3 requires it); 3.11 with the packages installed unpinned, as requirements.txt describes, or through pyproject.toml (requires-python >= 3.11, not tested); tested on 3.13
numpy 2.5.3, shapely 2.2.0, mapbox_earcut 2.1.0	the versions in requirements.txt
cadquery-ocp 7.9.3.1 or later below 8.0	optional, for the tests only: they read STEP files back with OpenCascade, and skip that check without it
gltf_validator (Khronos, command line)	optional; used by the Verifier when on the PATH

Operating systems: anything the packages above run on. Tested on Linux.

Previous	Next
Project Output Organization	openEMS Workflow