Flow_Controller/scripts/Readme.md

Install kikit

Install kikit:

pipx install --system-site-packages kikit

KiKit Fixture Post-Processor

Post-processing script for KiKit panelized PCBs that places any generated panel inside a fixed CNC fixture coordinate system.

The script:

• Centres the finished panel inside a predefined fixture opening
• Adds mechanical alignment pin holes
• Draws fixture reference geometry
• Moves the complete design so the fixture origin is always at (0, 0)

The resulting output is intended for repeatable CNC manufacturing workflows where drilling, routing, and UV exposure all share the same physical fixture and machine datum.

---

Fixture Geometry

Outer Fixture Frame

Parameter	Value
Width	200.0 mm
Height	130.0 mm

Inner Fixture Opening

Parameter	Value
Width	153.4 mm
Height	87.0 mm

The inner opening defines the usable panel area.

The region between the outer frame and inner opening forms the fixture rails.

---

Alignment Pins

The script inserts four non-plated alignment holes:

• Diameter: Ø 3.172 mm NPTH
• Naming: PIN1–PIN4
• Positioning: fully user-defined absolute coordinates

This allows:

• deterministic CNC coordinates
• compatibility with existing jigs
• custom asymmetric fixtures
• reuse across multiple panel layouts

---

Coordinate System

After processing:

• The fixture outer top-left corner is positioned at (0, 0)
• All PCB data is translated accordingly
• Every generated panel shares the same global coordinate system

This creates deterministic CAM output suitable for automated tooling and repeatable fixture-based manufacturing.

---

Usage

Place fixture_postprocess.py next to the source .kicad_pcb file and run KiKit:

kikit panelize \
    -p myPreset.json \
    ../Flow_Controller.kicad_pcb \
    panel/Flow_Controller_Panel.kicad_pcb

---

Panel Layout Parameters

Grid Layout

Adjust the panel dimensions using:

rows: <n>
cols: <n>

Examples:

• 1×1
• 1×2
• 2×2

The script automatically recalculates centering offsets for the resulting panel size.

---

Tool Diameter Compensation

The following values should match the routing tool diameter:

space
slotwidth

Example:

space: 2.1mm
slotwidth: 2.1mm

This is typically equal to the outline routing bit diameter.

---

Processing Pipeline

The post-processing script performs the following operations:

1. Reads the fully panelized KiKit output
2. Calculates the panel bounding box
3. Calculates the offset required to centre the panel inside the fixture opening
4. Translates the complete board dataset:
   • footprints
   • tracks
   • vias
   • zones
   • drawings
   • board outlines
   • substrate geometry
   • locked items
5. Places four NPTH alignment pin footprints
6. Draws fixture reference rectangles on the User.1 layer
7. Repositions the design so the fixture outer top-left corner equals (0, 0)

---

Fixture Visualization

The script draws two rectangles on the User.1 layer:

• Outer fixture boundary
• Inner fixture opening

These graphics:

• are visible in KiCad
• help verify positioning visually
• are NOT placed on Edge.Cuts
• are NOT exported into manufacturing Gerbers or NC drill files

They exist purely as fixture reference geometry.

---

CNC Workflow

Operation	File	Purpose
Drilling	Excellon .drl	PCB holes + fixture alignment pins
Routing	Edge.Cuts Gerber	Board outlines and mousebite tabs
UV exposure	Copper Gerbers	Soldermask/alignment registration

Because all outputs share:

• identical (0,0) origin
• identical alignment pin locations
• identical fixture geometry

the PCB can remain mounted in the same physical fixture for the complete process.

No re-alignment or re-fixturing is required between operations.

---

Alignment Pins

The script inserts four non-plated alignment holes:

• Diameter: Ø 3.172 mm NPTH
• Naming: PIN1–PIN4

Users may override any coordinate manually.

---

Default Pin Placement Calculation

For the default fixture dimensions:

OUTER_W_MM = 200.0
OUTER_H_MM = 130.0

INNER_W_MM = 153.4
INNER_H_MM = 87.0

the resulting suggested coordinates are:

Pin	X (mm)	Y (mm)
PIN1 (top)	100.0	10.75
PIN2 (right)	188.35	65.0
PIN3 (bottom)	100.0	119.25
PIN4 (left)	11.65	65.0

---

Fixture Configuration

Edit the constants at the top of fixture_postprocess.py:

# ============================================================
# Fixture geometry
# ============================================================

OUTER_W_MM = 200.0
OUTER_H_MM = 130.0

INNER_W_MM = 153.4
INNER_H_MM = 87.0

# ============================================================
# Alignment pins
# Absolute fixture-space coordinates in millimetres
# ============================================================

PIN_DIAMETER_MM = 3.172

# Suggested defaults:
# top    = centered in top rail
# right  = centered in right rail
# bottom = centered in bottom rail
# left   = centered in left rail

PIN1_X_MM = 100.0
PIN1_Y_MM = 10.75

PIN2_X_MM = 188.35
PIN2_Y_MM = 65.0

PIN3_X_MM = 100.0
PIN3_Y_MM = 119.25

PIN4_X_MM = 11.65
PIN4_Y_MM = 65.0

These values may be adjusted freely without changing the placement logic.

Design Constraints

The generated panel must fit completely inside the inner fixture opening.

If the panel exceeds the available space, the script emits:

WARNING: panel … is larger than the inner opening

Possible solutions:

• reduce rows
• reduce cols
• reduce KiKit frame width
• reduce spacing
• use a smaller PCB design

---

Intended Use Case

This workflow is intended for:

• CNC isolation milling
• UV mask alignment systems
• repeatable prototyping fixtures
• hybrid PCB manufacturing workflows
• automated or semi-automated PCB handling

The primary design goal is deterministic panel placement independent of PCB size.

Exporting gcode files from KiCad

Adapt milling and drilling parameters in millproject. Look up pcb2gcode/wiki for help.

nano millproject

Run the export by providing the .kicad_pcb file as a first argument:

chmod +x export.sh
./export.sh panel/Flow_Controller_Panel.kicad_pcb

The script will first generate gerber files in the output directory and then convert them into ngc format in the gcode directory.

Launch the gSender program.

• Load the gcode/drill.ngc file for drilling holes.
• Load the gcode/outline.ngc file for milling the board outlines.
• Load the gcode/back.ngc file if you want to mill the isolation traces.

Milling tip: Increase the thermal spoke and trace width

When routing for milling, use the widest traces possible. 1mm, 2mm and wider, the machine doesn't care, but later you won't be soldering leads to small fragile strips of copper. You can use copper pours for routing too.

Set up the entire back side as one big GND pour. Then, increase the thermal spoke width to be larger than 1mm. This avoids small features and gives more room for error if a larger drill is used for the holes.