Kikakuka (企画課, きかくか, Planning Section) creates a few more dimensions for KiCad:
- Workspace and project management
- Revision management
- Build variants
- Panelization
- FreeCAD integration for flexible PCB bending and multi-board assembly
- Features
- Workspace Manager
- Schematic and PCB Differ
- PCB Build Variants
- PCB Panelization
- FreekiCAD Integration
- Flexible PCB Bending
- Kikakuka KiCad Library
- Technical Background and Evolution
- Run from source on Linux/macOS
- Run from source on Windows
- CLI Usage
- Gerber-to-KiCad Conversion
-
Kikakuka main program
- Workspace Manager
- Organize KiCad projects, FabPlans, FreeCAD documents, assemblies, and STEP files in
.kkkkworkspaces with relative paths and file descriptions - Open related schematic, PCB, and STEP files or launch Differ and FabPlan from the workspace
- Inspect project-specific symbol and footprint libraries and convert their paths to
${KIPRJMOD}-relative references
- Organize KiCad projects, FabPlans, FreeCAD documents, assemblies, and STEP files in
- Instance Manager UI
- Inspect same-user KiCad and FreeCAD processes and known file paths, with one row per FreeCAD document, the matched KiCad IPC socket basename, automatic mesh-event updates, manual reconciliation, and Go to actions
- Differ
- Highlight changed areas
- Schematic diff viewer
- PCB diff viewer
- Git support
- Fabrication Planner
- Panelizer
- Interactive arrangement with real-time preview
- Freeform placement not limited to M×N grid configurations
- Support for multiple different PCBs in a single panel
- Automatic or manual tab creation
- Automatic V-cut/mousebites selection
- Enable hole creation in panel substrate for extruded parts
- Load KiKit multiboard files as multiple separate boards
- No coding skills required
- Build Variants
- Single PCB without panelization can be done with frameless setting
- Each PCB can have its own flag settings
- Reproducible workflows
- Create and edit fabrication plans interactively in the GUI.
- Save configurations in a portable, JSON-based
.kkkk_fabfile. - Generate outputs from the saved plan using either the GUI or CLI.
- Panelizer
- Gerber handling
- Available in the fabrication planner (panelizer)
- Or direct conversion to .kicad_pcb
- Compared with KiCad output
- Better restoration of oval drill holes
- Allow attaching BOM/CPL (converted to reference-only footprints)
- CLI - Convert saved fabrication plans (
.kkkk_fab, or legacy.kikit_pnl) to KiCad files in one command
- Workspace Manager
-
FreekiCAD (FreeCAD Addon)
- Reloadable KiCad PCB Object
- Optional copper and solder-mask import, with outer copper, inner copper, and mask controlled independently
- Solid stiffeners from annotated
F.StiffenerandB.Stiffeneruser-layer areas - Flex PCB bending driven by bend lines and parameters defined in KiCad
- Automatic coupler-based PCB alignment using matching
CouplerFixedandCouplerMovingfootprints or an absoluteCouplerAt, with coupler plane markers for inspection - A sketch is provided for real-time board outline editing in FreeCAD
- Components moved in FreeCAD are synced to KiCad in real time
- Reloadable STEP/STL Object
- Import and export assembly manifests (
.kkkk_asm) - CLI - Export saved assembly manifests (
.kkkk_asm) to STEP or STL in one command
- Reloadable KiCad PCB Object
-
KiCad Plugin/Library
-
Coupler footprints for Automatic coupler-based PCB alignment
-
Plugin actions for previewing and hiding coupler helpers in the 3D Viewer
-
Populate scaled placeholder 3D models for footprints without a valid model, using
SizeX,SizeY, andSizeZproperties- Tutorial Video
-
-
CADhoc / Instance Manager
- Seamless navigation among Kikakuka, KiCad, and FreeCAD across multiple instances and open documents
The .kkkk file saves workspace information in JSON format.
Adding or dropping a .kicad_pcb or .kicad_sch records its sibling
.kicad_pro project entry, even when that project file has not been created
yet. A virtual project row omits the .kicad_pro suffix; an existing project
file keeps it. Rows list only PCB/schematic files that currently exist.
Opening a missing project row reports the missing project instead of launching
KiCad.

- A diff sample of cynthion-hardware
The .kkkk_fab file saves panelization and build-variants settings in JSON format, with PCB paths stored relative to the file's location. Legacy .kikit_pnl files can still be opened or added; newly saved fabrication plans use .kkkk_fab.
Example: samples/build_variant.kkkk_fab and samples/build_variant.kicad_pcb.
Set BUILDEXPR in footprints' properties. This can be done quickly with Symbol Fields Table using the current sheet only scope. Remember to sync them to PCB afterward.
- Kikakuka extracts build flags from
BUILDEXPR. Selected flags are interpreted as true, and vice versa. - Footprints with the BUILDEXPR evaluated as false will be marked as DNP.
- Footprints with unset or empty BUILDEXPR will be kept as is.
A boolean expression with operators:
~Not&And|Or
It can be as simple as a build name as shown in the image above or an expression like (A | ~B) & C.
Panelization with different build variants

Single PCB without panelization can be done with frameless setting

Field#Flag or multiple flags like Field#FlagA#FlagB will set Field to the value where build flags contain all the flags.
Field#Opt=A, Field#Opt=B will be displayed as dropdown options.
Requires FreeCAD 1.0 or later, KiCad 9.0 or later,
psutil>=7.2.2, kicad-python>=0.8,<0.9, and shapely>=2.0.7. FreeCAD Addon
Manager may not automatically install packages where its allowed-package list
excludes them; install them manually inside FreeCAD if necessary. Installing
FreekiCAD from Kikakuka's Integration tab installs all three Python packages.
Note
FreeCAD installed through Snap is not supported. Snap confinement isolates the filesystem and local sockets, preventing FreekiCAD from connecting to KiCad's IPC endpoint. Selecting the Snap executable manually does not remove this isolation; use a non-Snap FreeCAD installation or the official AppImage.
FreekiCAD and Kikakuka discover each other on demand through local Unix sockets or Windows named pipes. FreeCAD can manage KiCad instances without the Workspace Manager running. No board, assembly, or usage data is sent to third parties.
When opening a FreeCAD file, Kikakuka first looks for an already open document or reuses a responding FreeCAD instance; see CADhoc for details.
KiCad .kicad_pcb boards and STEP models remain external files referenced by
path. When saved as .FCStd, the FreeCAD document caches their generated
objects and geometry, but the links remain reloadable from the source files. A
.kkkk_asm manifest stores source paths, settings, placements, and an optional
structured 3D viewport camera; it never contains cached objects or geometry.
Source paths are stored relative to the manifest whenever possible and resolved
from its directory on import, when every external source is loaded fresh. The
camera is restored field by field in FreeCAD's GUI, skipping unsupported or
invalid fields, and ignored by headless STEP/STL export.
AutoReload is enabled by default on both object types, so changing either
source file reloads its linked FreeCAD object. The option can be disabled
independently for each object.
Tip
You can use Kikakuka's Integration tab to install, update, or uninstall the
bundled KiCad plugin, KiCad library, and FreekiCAD addon. Close all instances
of the affected application before using an install or uninstall button.
Release builds already contain the addon packages. When running Kikakuka
from source, generate them first with
python3 build-tools/build_addon_archives.py (or
make archive-zips); the GUI loads the resulting runtime packages from
build/addons/.
For a standalone FreekiCAD deployment without Kikakuka, follow the FreekiCAD manual installation instructions.
- Activate
Preferences -> Plugins -> Enable KiCad API. Kikakuka or FreekiCAD can reuse a running matching KiCad editor or start one on demand. - FreekiCAD (FreeCAD Addon)
- Add PCB
- Drag and drop / Open / Import
- Drag a
.kicad_pcbfile into FreeCAD, or use FreeCAD's Open or Import command; switching workbenches is not required.
- Drag a
- FreekiCAD menu
- Switch to the
FreekiCADworkbench. - Menubar -> FreekiCAD -> Add KiCad PCB.
- Switch to the
- All of these entry points create the same linked PCB object.
- The selected
.kicad_pcbremains an external file and is represented by a linkedPcbObject. ItsAutoReloadproperty defaults to enabled.
- Drag and drop / Open / Import
- Add STEP
- Menubar -> FreekiCAD -> Add STEP
- The selected STEP model remains an external file. Its
AutoReloadproperty defaults to enabled, and its Placement is preserved when the source file is manually or automatically reloaded.
- Position and assemble linked objects
- Linked objects work with the
AssemblyandManipulatorworkbenches, as well as FreeCAD's built-in transform tool. - FreeCAD Assembly can place
PcbObjectLinks, but currently cannot resolve their child component or connector faces for joints. Use the Manipulator workbench to align those faces.
- Linked objects work with the
- Reload PCB
- Right-click on the board object -> Reload KiCad PCB
- Export or import an assembly manifest
- Use FreeCAD's standard Export command to write
.kkkk_asm, or its Import command to read.kkkk_asm; selectFreekiCAD Assembly (*.kkkk_asm)as the file type. - The JSON stores each external PCB or STEP source path, editable FreekiCAD settings, its placement, and—when exported from the GUI—the active 3D viewport camera. It contains no cached objects or generated geometry, and every external source is loaded fresh during import. Export prefers paths relative to the manifest and falls back to absolute paths only when necessary; relative paths are resolved from the manifest's directory. FreeCAD regenerates object names and labels during import. GUI import restores each available camera field independently after recomputation and skips fields that are invalid or unsupported; headless STEP/STL export ignores the camera.
- Selecting an original
PcbObjectorStepObjectexports its own Placement. Selecting one or moreApp::Linkinstances exports each linked source at that instance's final global placement. Selecting anAssembly::AssemblyObjectrecursively expands its direct and nested Links, including multiple instances of the same source. - Assembly and Link exports are flattened placement snapshots;
.kkkk_asmdoes not store Links, joints, constraints, remaining degrees of freedom, or the Assembly hierarchy. A linked PCB snapshot is exported withSnapToCouplerdisabled in the manifest so coupler alignment cannot overwrite its solved Assembly placement; the sourcePcbObjectin the current FreeCAD document is not modified. - When original PCB source objects are selected directly, Placement is omitted for a
CouplerMovingboard if the same export contains its matchingCouplerFixedboard; coupler alignment recalculates that placement after import. - Headless STEP export:
freecadcmd scripts/kkkk_export.py input.kkkk_asm output.step; the input may also be a single.kicad_pcb. See Headless STEP and STL Export for platform-specific paths and requirements.
- Use FreeCAD's standard Export command to write
- Edit Board Shape
- Expand the object's children.
- Open the sketch with the
_Outlinesuffix.
- Inspect Copper Layers
- FreekiCAD imports tracks, filled zones, pads, vias, and copper-layer graphics as separate
F.Cu,In*.Cu, andB.Cuchild objects. ImportOuterCopperindependently controlsF.CuandB.Cu;ImportInnerCoppercontrolsIn*.Cu. Both default to off.- Inner layers use their physical stackup Z and are normally hidden by the board body; hide the board or make it transparent to inspect them.
- Copper is rendered as one unioned zero-thickness face per layer, eliminating overlap between tracks, pads, vias, and zones. Each face retains its physical stackup Z, so inner layers follow the correct bend radius.
- The substrate remains one body. Imported outer copper reserves its physical stackup thickness at the body boundary; inner copper does not create expensive internal body cavities. Finished board thickness and component/coupler Z never change.
- FreekiCAD imports tracks, filled zones, pads, vias, and copper-layer graphics as separate
- Inspect Solder Mask
ImportSolderMaskimports translucentF.MaskandB.Maskchild objects, with pad/via openings computed by KiCad plus explicit mask-layer graphics. It defaults to off.- The resulting F/B mask-opening geometry is also subtracted from stiffener solids on the matching side.
- With mask import enabled, the board body uses the configured dielectric stackup colors and KiCad opacity, or white with KiCad's default board-body opacity when no color is available. Mask opacity likewise follows its KiCad stackup color. Both display opacities are scaled to 70% in FreeCAD. With mask import disabled, the original opaque board color is preserved.
- Mask is a zero-thickness face at the finished outer surface. Imported mask reserves its physical outer stackup thickness in the single substrate body; when mask import is disabled, the body fills that thickness.
- Inspect Silkscreen
ImportSilkscreenimports board- and footprint-level graphics, references, values, fields, and free text fromF.SilkSandB.SilkS. It defaults to off.- Silkscreen is a zero-thickness face on the finished board surface. A Coin3D polygon offset resolves viewport z-fighting without moving the geometry, so measurements, bounds, and exports retain the exact finished dimensions.
- Flexible PCB Stiffener
- Import annotated stiffener solids automatically from
F.StiffenerandB.Stiffeneruser layers.
- Import annotated stiffener solids automatically from
- Coupler-Based PCB Alignment
- Place a
CouplerFixedfootprint on the reference PCB and aCouplerMovingfootprint on the PCB to be aligned. Couplers are matched by their KiCad reference. - Alternatively, place one
CouplerAton a PCB to align it with a virtualCouplerFixedat the absolute FreeCAD world coordinates given by itsTargetX,TargetY, andTargetZproperties. All three default to0 mm. Usually placeCouplerAton B.Cu so the PCB bottom surface is positioned atTargetZ; use F.Cu only when the top surface should be the reference. A PCB may contain only one positioning source: oneCouplerMovingor oneCouplerAt. - After any linked PCB reloads, positioning is recalculated for every linked PCB in dependency order. A concurrently reloading PCB is skipped until its fresh poses and bent markers are available; its completion triggers another full pass. A PCB with
SnapToCouplerenabled (the default) is moved as a whole so that its moving coupler plane meets the matching fixed coupler plane face-to-face; disabling it excludes that PCB from automatic positioning. Alignment uses each plane's position after flex-PCB bending. Each coupler is also available as a child object in FreeCAD; its plane marker is hidden by default and can be shown for inspection. - FreekiCAD checks the saved coupler list against KiCad's live document every second, including unsaved position, side, rotation,
Z,Offset,Tilt, andCouplerAttarget edits. A changed pose updates its marker and recalculates linked-board positioning. The coupler child object's footprint position and local-plane properties are editable in FreeCAD; edits update the marker and linked-board positioning immediately and are written back to the live KiCad footprint.Yis shown using FreeCAD's axis convention. Older footprints without anOffsetfield load as0 mm; editingOffsetin FreeCAD creates the missing hidden KiCad field automatically. Adding, removing, or changing the identity of couplers takes effect on the next PCB reload, which rebuilds the saved list. - The
kicad-addon/librarydirectory providesCouplerFixed,CouplerMoving, andCouplerAt. - Alignment example boards:
assembly-power.kicad_pcb,assembly-mcu.kicad_pcb,assembly-led.kicad_pcb, andassembly-mezzanine.kicad_pcb. - The coupler plane is defined by the footprint position, side, rotation, and these custom footprint properties:
CouplerFixedandCouplerMovinguseZto move the plane origin along the PCB surface normal. It defaults to0 mm; the origin starts at the PCB surface, including the board thickness on F.Cu, and the direction is reversed on B.Cu.Offsetmoves the plane origin on the PCB surface in the direction indicated by the footprint triangle. It defaults to0 mm.ZandOffsetaccept values without a unit as millimetres and supportmm,cm,in,mil(0.001 in), andum.Tilttilts the plane around the footprint's local X axis. It is specified in degrees and defaults to0.CouplerAtusesTargetX,TargetY, andTargetZas its absolute FreeCAD world target and does not have a localZproperty. The target properties default to0 mm; the same length units are supported. B.Cu is recommended for the usual bottom-surface placement atTargetZ; use F.Cu only to reference the top surface.
- Placement applies the footprint position and rotation, then
Offset,Z, andTilt.Tiltrotates around the footprint's local X axis at the offset origin; it does not redirect either displacement. The footprint's normal KiCad rotation supplies the rotation around its local Z axis.
- Place a
- Flex PCB Bending
- Name a KiCad graphical layer
FreekiCAD(case-insensitive) and draw bend lines on it as line segments. - Panel export maps every source PCB's
FreekiCADdrawings to one collision-free User layer and preserves thefreekicadlayer name, even when source boards use differentUser.xlayers. - Add bend parameters as text on the same
FreekiCADlayer near a bend line endpoint, for examplea=-70 r=0.5ora=-70 s=0.61.- The text anchor must be within
0.1 mmof a bend line endpoint. ais bend angle in degrees.ris bend radius.sis the full bend span and is used to deriverwhenris omitted, using the board thickness from stackup.- Both lengths accept
mm,cm,um(alsoµm/μm),in, andmil; omitted units mean mm. Unit suffixes are case-insensitive. Unsupported units are rejected. - Parameters may appear in any order, with whitespace around
=and before units:r = 5 mm a = 60is equivalent toa=60 r=5mm. If bothrandsare present,rtakes precedence.
- The text anchor must be within
- After loading the board in FreeCAD, each bend line appears as a child object with
Angle,Radius, andActiveproperties. - The linked PCB object also has an
EnableBendingproperty to toggle the deformation on or off. - Imported copper and solder mask are cut with the same board pieces. Rigid display faces follow each piece, while faces in a bend band are rebuilt with the wedge's curved point mapping.
- If no bend text is provided, the bend line still loads and can be configured directly in FreeCAD.
- Name a KiCad graphical layer
- Add PCB
Coupler plane markers are available as child objects in FreeCAD and are hidden by default.
Rename KiCad user layers to F.Stiffener and/or B.Stiffener
(case-insensitive). Each closed rectangle, circle, polygon, or connected
line/arc outline is imported automatically as one stiffener area; the KiCad
display fill may be on or off.
Put one text annotation inside each area and separate properties with / or
newlines:
Name=Tail reinforcement
Material=Polyimide
Color=#C87518
Opacity=0.65
Thickness=25 um
Material and Thickness are required. Name, Color, and Opacity are
optional and property names are case-insensitive. A non-empty Name becomes
the suffix of the FreeCAD child name and label (F_Stiffener_<Name> or
B_Stiffener_<Name>) and is included in bend-overlap warnings. Thickness
accepts mm, cm, in, mil (0.001 in), and um; a unitless value is
interpreted as millimetres.
Invalid annotations, annotations outside an area, and areas with multiple annotations are reported as errors and skipped. Unannotated areas are skipped with a warning.
| Material | Default color | Default opacity |
|---|---|---|
FR4 |
#C8B45A |
0.90 |
Polyimide |
#C87518 |
0.65 |
Stainless_Steel |
#A7ADB4 |
1.00 |
3M468 |
#F2E3BD |
0.28 |
tesa8854 |
#EEE8D8 |
0.45 |
3M9077 |
#DDE8EE |
0.30 |
Other material names are accepted with a warning. When Color or Opacity
is omitted for an unlisted material, the corresponding Polyimide default is
used.
Front stiffeners extend outward from the front silkscreen plane; back
stiffeners extend outward from the back silkscreen plane. They remain rigid
during flex bending. Pad, via, and explicit mask-graphic openings on F.Mask
are cut through front stiffeners; B.Mask openings are cut through back
stiffeners. This happens even when ImportSolderMask is disabled. If a
stiffener overlaps the full bend band, FreekiCAD prints a warning containing
the stiffener name, bend name, and overlap area.
Stiffener thickness is additive outside the finished PCB and is never counted in or subtracted from the board body.
Manual bending checks are currently done with these sample boards:
For the implementation details of the bending pipeline, see FreekiCAD/ARCHITECTURE.md.
The KiCad library is stored under kicad-addon/library.
You can install it from Kikakuka's Integration tab. For a manual installation,
add kicad-addon/library/footprints/Kikakuka.pretty
to KiCad's footprint library table (for example, as Kikakuka). Its
Kikakuka.3dshapes directory
contains the unit-cube placeholder and optional coupler helper models.
Variabledisplays itsValueon the board. In the Kikakuka Fabrication Planner, use build-variant fields such asValue#FlagorValue#Option=Choiceto show a value selected by the active build flags or options.StringTemplateformats itsValueduring Kikakuka Fabrication Planner export. Braced placeholders are replaced with matching footprint properties or build options after build-variant fields have been applied.CouplerFixedandCouplerMovingdefine matching planes for coupler-based PCB alignment. Give a pair the same reference and use theirZ,Offset, andTiltproperties as needed.CouplerAtaligns its PCB to absolute FreeCAD worldTargetX,TargetY, andTargetZcoordinates, all defaulting to zero. Place it on B.Cu for the usual behavior, where the PCB bottom surface is positioned atTargetZ; use F.Cu only to reference the top surface.
For coupler length properties (Z, Offset, TargetX, TargetY, and TargetZ), unitless values are millimetres; supported suffixes are mm, cm, in, mil, and um/µm. Tilt is in degrees and may optionally use deg or °.
All three coupler footprints use the Unspecified type, placing their helper models under Virtual Models in KiCad's 3D Viewer.
The separate Kikakuka Tools IPC plugin provides Coupler 3D Viewer and Hide Couplers actions. Coupler 3D Viewer applies each coupler's Z, Tilt, and Offset to its helper model and opens KiCad's 3D Viewer; Hide Couplers marks these models hidden without removing them and also opens the Viewer. Populate Placeholder 3D Models likewise opens the Viewer after populating models. To omit couplers from STEP export, enable Ignore 'Unspecified' components.
Kikakuka is mainly built on top of KiKit, Shapely, modified pcb-tools, OpenCV, pypdfium2 and PUI.
Its FreeCAD integration is inspired by KiCadStepUp and KiConnect.
Kikakuka, formerly Kikit-UI, began as an interactive GUI for KiKit and later expanded to include a workspace manager. File-to-instance tracking was introduced to make navigation from the workspace manager to KiCad reliable, with the workspace manager initially serving as the central orchestrator. After FreekiCAD was introduced, that mechanism evolved into CADhoc, a mesh of peer nodes running in Kikakuka and FreekiCAD without a permanent central orchestrator. The mesh also includes a client-only node in the KiCad add-on. CADhoc maintains a shared view of KiCad and FreeCAD instances and their open documents, so navigation no longer depends on the workspace manager.
Make sure your python can import pcbnew
> python3 -c "import pcbnew; print(pcbnew._pcbnew)"
<module '_pcbnew' from '/usr/lib/python3/dist-packages/_pcbnew.so'>
On macOS, I have to use the python interpreter bundled with KiCAD
PYTHON=/Applications/KiCad/KiCad.app/Contents/Frameworks/Python.framework/Versions/Current/bin/python3
On Linux, you should be able to just use the your default python3
PYTHON=python3
Create a virtual environment and install dependencies
${PYTHON} -m venv --system-site-packages env
./env/bin/pip3 install -r requirements.txt
On Debian/Ubuntu, PySide6's X11 platform plugin also needs these system libraries:
sudo apt install libxcb-cursor0 libxkbcommon-x11-0 libxcb-icccm4 libxcb-image0 libxcb-keysyms1 libxcb-render-util0 libxcb-xkb1
Kikakuka uses opencv-python-headless for image processing and PySide6 for its
windows. If an existing environment has opencv-python installed, replace it
before reinstalling requirements (both packages provide the same cv2 module):
./env/bin/pip3 uninstall opencv-python
./env/bin/pip3 install -r requirements.txt
Update submodule
git submodule update --init --recursive
Run
./env/bin/python3 -m kikakuka
# Equivalent directory entry point:
./env/bin/python3 kikakuka/
On Windows the Python interpreter is at C:\Program Files\KiCad\10.0\bin\python.exe.
But however in my Windows environment venv is not working properly, here is how I run it with everything installed in the KiCad's environment.
# Powershell
# Initialize bundled submodules after cloning
git submodule update --init --recursive
# Git for Windows may check symlinks out as text files containing their target
# paths. Replace all tracked symlinks with physical files/directories so the
# source tree can run without Windows symlink support.
& .\tools\materialize-symlinks.ps1
&"C:\Program Files\KiCad\10.0\bin\python.exe" -m pip install -r requirements.txt
&"C:\Program Files\KiCad\10.0\bin\python.exe" -m kikakukaThe materialization only changes the working tree; Git still tracks those paths
as symlinks. Re-running the script refreshes the physical copies. If PowerShell
blocks local scripts, run
powershell -ExecutionPolicy Bypass -File .\tools\materialize-symlinks.ps1.
# Just open it
./env/bin/python3 -m kikakuka
# Start with PCB files
./env/bin/python3 -m kikakuka a.kicad_pcb b.kicad_pcb...
# Open KiCad files through the instance manager
./env/bin/python3 -m kikakuka --open a.kicad_pcb
# Run a foreground CADhoc node with request/mapping logs
./env/bin/python3 -m cadhoc
# The equivalent directory entry point is: ./env/bin/python3 cadhoc
# Open or focus a PCB and reload it from disk once its IPC API is ready
./env/bin/python3 -m kikakuka --open --fresh a.kicad_pcb
# In a mixed list, --fresh affects only .kicad_pcb files; schematics and
# projects are opened normally.
# Stop all same-user KiCad and FreeCAD GUI instances (not FreeCADCmd)
# Warning: unsaved work may be lost.
./env/bin/python3 -m kikakuka --killall
# Stop only one application (case-insensitive)
./env/bin/python3 -m kikakuka --killall freecad
./env/bin/python3 -m kikakuka --killall kicad
# Export a FreekiCAD assembly through the detected FreeCADCmd and bundled exporter
./env/bin/python3 -m kikakuka input.kkkk_asm output.step
./env/bin/python3 -m kikakuka input.kkkk_asm output.stp
./env/bin/python3 -m kikakuka input.kkkk_asm output.stl
# Run the detected FreeCADCmd with pass-through arguments
./env/bin/python3 -m kikakuka --freecadcmd FreekiCAD/scripts/kkkk_export.py input.kkkk_asm output.step
# Load file (.kkkk, .kkkk_fab, or legacy .kikit_pnl)
./env/bin/python3 -m kikakuka a.kkkk_fab
# Headless export for panelization or build variants
./env/bin/python3 -m kikakuka a.kkkk_fab out.kicad_pcb
# Differ
./env/bin/python3 -m kikakuka --differ a.kicad_sch b.kicad_sch
./env/bin/python3 -m kikakuka --differ a.kicad_pcb gerber_folder
./env/bin/python3 -m kikakuka --differ gerber.zip b.kicad_pcb
# Gerber to KiCAD Conversion
./env/bin/python3 -m kikakuka gerber.gbr out.kicad_pcb
./env/bin/python3 -m kikakuka gerber_folder out.kicad_pcb # BOM/CPL will be detected if they are in the folder
./env/bin/python3 -m kikakuka gerber.zip out.kicad_pcb
./env/bin/python3 -m kikakuka gerber.zip out.kicad_pcb bom_or_cpl_1.csv bom_or_cpl_2.csv # BOM/CPL files are determined by filename regardless of argument order
- Convert Gerber to .kicad_pcb with BOM/CPL using
Kikakuka - Footprint names are also exported, so
Tools -> Update Footprints from Librarycan bring back the footprint if the name matches - Lock the footprint, clean up with quick selection and deletion, unlock the footprint (you will need to set the
Selection Filter)
















