Using an MSLA (Masked Stereolithography Apparatus) resin printer for creating PCBs is a technique known as "Direct UV Exposure." Instead of printing a plastic part, you use the printer's LCD screen as a dynamic digital mask to cure photosensitive materials (etch resist, solder resist and silkscreen) on a copper board.

The "Matrix LED" ensures uniform light distribution across the entire build area. When exposing a photosensitized board, uneven lighting can cause some areas to be under-exposed (washing away traces) or over-exposed (causing traces to merge). The matrix source ensures the center and corners of your PCB receive the same energy, resulting in a reliable etch.

The objective

KiCad PCB layers need to be converted to .pm4n files for direct UV exposure on an Anycubic Photon Mono 4 (9024×5120 px, 17 µm/px, 1494.12 DPI) on the screen size of 153.408 x 87.040 mm.

Hardware

A resin 3D printer (e.g., Anycubic Photon Mono 4)
Photosensitive PCB. For consistent results, a pre-sensitized board like the Bungard positive photoresist boards is highly recommended due to its uniform coating. A good example is Bungard 160x100 double-sided 3,49 €.
UV light curing Solder Mask e.g. from Mechanic. Use green as the solder mask and white for the silkscreen.

Software

1. Install KiCad

Ensure you have kicad installed:

sudo apt update
sudo apt install kicad

2. KiCad: Set your design grid (Optional)

In KiCad's PCB editor, go to Preferences → Preferences → PCB Editor → Grids and add a custom grid of 0.017 mm (your MSLA printer's pixel size). This ensures trace edges land on pixel boundaries and avoids the sub-pixel rounding that causes the ±1px size error people see with arbitrary grids.

3. Export gerbers from KiCad

If you want to automate the conversion of gerber to printing files, you can jump to the section Appendix: Automated script.

Open your PCB project in the KiCad PCB Editor.
Go to File -> Plot and select Plot format as SVG and set the Output directory.
In the Include Layers section select layers F.Cu, B.Cu, B.Mask and F.Silkscreen. Each layer will be ploted as a separate SVG file.
Optionaly, select additional layer(s) e.g. Edge.Cuts in the Plot on All Layers section. This way you can merge layers i.e. add board outset into each file generated. This is usually not needed.
Click Plot and Close.

4. Install `CHITUBOX Basic`

Follow the offical installatin guide for Ubuntu

5. Create the `Dummy.pm4n` file

Open CHITUBOX Basic slicer (or any other slicer that works for your resin printer), select printer Anycubic Photon Mono 4, slice any tiny STL (e.g.: 1×1×0.05 mm box), and save as Dummy.pm4n.

This file is reused for every job — it carries the correct LCD resolution metadata.

MSLA PCB Exposure

UVtools has a dedicated PCB Exposure tool that converts a Gerber file to a pixel-perfect image given your printer's LCD resolution, specifically for exposing copper traces.

1. Install `UVtools`

Install UVtools dependencies

sudo apt-get install -y curl
sudo bash -c "$(curl -fsSL https://raw.githubusercontent.com/sn4k3/UVtools/master/Scripts/install-dependencies.sh)"

Install UVtools

Grab the Linux release and extract it

LATEST=$(curl -fsSL https://api.github.com/repos/sn4k3/UVtools/releases/latest \
    | grep '"tag_name":' \
    | cut -d '"' -f4)

wget -P ~/Downloads \
    "https://github.com/sn4k3/UVtools/releases/download/${LATEST}/UVtools_linux-x64_${LATEST}.zip"

mkdir ~/UVtools
cd ~/UVtools
unzip ~/Downloads/UVtools_linux-x64_${LATEST}.zip

2. Run `UVtools`

cd UVtools
./UVtools

To automate the conversion of gerber to printing files, you can jump to the section Appendix: Automated script.

3. Export `.pm4n` file from Gerber layer

You export Gerber from KiCad (not SVG), which natively gives you positive/negative control per layer.
You open the Dummy.pm4n file in UVtools (a minimal valid .pm4n sliced by Chitubox or Photon Workshop with any tiny model), then use Tools → PCB Exposure to inject your Gerber layer e.g.: Flow_Controller_Panel-Front.gbr.
You control inversion, invert and the exposure time at the bottom of the PCB exposure dialog.
You save it as e.g.: Flow_Controller_Panel-Front.pm4n file.

4. Check the printer exposure

Open Chitubox

cd /opt/CBD/CHITUBOX_Basic
./CHITUBOX_Basic.sh

Open the Flow_Controller_Panel-Front.pm4n file to visually verify before printing.

If you want to automate the conversion of gerber to printing files, you can jump to the section Appendix: Automated script.

5. Print

Place the presensitized copper board on the Anycubic Photon Mono 4 printer's LCD screen. Copy the file Flow_Controller_Panel-Front.pm4n on the USB drive and 3D print it.

6. Developing

After exposure, you must develop the board to reveal the pattern.
- For a positive photoresist board (like the Bungard brand), the developer is a weak alkaline solution. A common and effective developer is a 1% solution of Sodium Hydroxide (NaOH) in distilled or demineralised water.
- For the UV light curing solder mask, allow more time to it to harden. Clean the uncured part with Izopropanol afterwards.
Safety First: When working with chemicals like NaOH, always wear gloves and eye protection.
Submerge the board in the developer solution and gently agitate it. This should take 30-90 seconds, depending on the resist and developer freshness.
Rinse the board thoroughly with water.

7. Etching

For the developed Bungard photoresist PCB, etch the board using either sodium persulfate or ferric chloride.

For sodium persulfate, prepare a solution with approximately 200–250 g/L and heat it to 40–50 °C.
For ferric chloride, use a ready-to-use solution or prepare it according to the manufacturer's instructions and maintain a temperature of 35–45 °C.

Immerse the board in the etchant and agitate gently until all exposed copper has been removed, typically within 5–15 minutes. Rinse the board thoroughly with water after etching. To remove the remaining photoresist, immerse the board in a 2–5% sodium hydroxide (NaOH) solution at room temperature for 1–2 minutes, then rinse thoroughly with water and dry the board.

8. Drilling holes and milling board outlines

Use the project kicad2gcode to generate G-Code for CNC driling and outlines milling.

Appendix: Automated script

Automate the conversion from KiCAD to print files using a CLI.

1. The `Dummy.pm4n` file

Make sure you have the Dummy.pm4n file specific to your printer. See the section 5. Create the Dummy.pm4n file above.

2. Setup the `UVtools` wrapper

Make sure UVtools is installed - follow the section 1. Install UVtools.

By default pcb-expose.sh looks for ~/UVtools/UVtoolsCmd. Override with:

export UVTOOLSCMD=~/UVtools/UVtoolsCmd

3. Export KiCAD gerbers

kicad-cli pcb export gerbers \
    -o gerbers \
    -l F.Cu,B.Cu,F.Mask,B.Mask,F.SilkS,B.SilkS \
    ../kicad2panel/panel/Flow_Controller_Panel.kicad_pcb

Output:

Plotted to 'gerbers/Flow_Controller_Panel-Front.gtl'.
Plotted to 'gerbers/Flow_Controller_Panel-Back.gbl'.
Plotted to 'gerbers/Flow_Controller_Panel-F_Silkscreen.gto'.
Plotted to 'gerbers/Flow_Controller_Panel-B_Silkscreen.gbo'.
Plotted to 'gerbers/Flow_Controller_Panel-F_Mask.gts'.
Plotted to 'gerbers/Flow_Controller_Panel-B_Mask.gbs'.

4. Exposure

We need to invert copper and soldermask layers: F.Cu,B.Cu,F.Mask,B.Mask,F.SilkS,B.SilkS.

We need to mirror all front layers: F.Cu,F.Mask,F.SilkS.

Traces should appear black on white background.

background = UV exposed = resist removed = etched away
traces = dark = resist kept = copper stays

Start with --exposure 60 and bracket from there — Bungard presensitized at 405nm typically lands between 30–180s depending on board vintage and storage.

UV light curing Solder Mask from Mechanic needs 15 minutes when prebaked (heat it to 80C for 15 minutes) otherwise 30 minutes. Use green as the solder mask and white for the silkscreen.

4.1. Export print files for copper layers

Export the front and back copper layers for 120 seconds exposure

pcb-expose.sh Dummy.pm4n gerbers/Flow_Controller_Panel-Front.gtl \
    --invert --mirror --exposure 120 \
    --output pm4n/Flow_Controller_Panel-Front.pm4n

pcb-expose.sh Dummy.pm4n gerbers/Flow_Controller_Panel-Back.gbl \
    --invert --exposure 120 \
    --output pm4n/Flow_Controller_Panel-Back.pm4n

4.2. Export print files for soldermask layers

Export the front and back soldermask layers for 900 seconds exposure

pcb-expose.sh Dummy.pm4n gerbers/Flow_Controller_Panel-F_Mask.gts \
    --invert  --mirror --exposure 900 \
    --output pm4n/Flow_Controller_Panel-F_Mask.pm4n
    
pcb-expose.sh Dummy.pm4n gerbers/Flow_Controller_Panel-B_Mask.gbs \
    --invert --exposure 900 \
    --output pm4n/Flow_Controller_Panel-B_Mask.pm4n

4.1. Export print files for silkscreen layers

Export the front and back silkscreen layers for 900 seconds exposure

pcb-expose.sh Dummy.pm4n gerbers/Flow_Controller_Panel-F_Silkscreen.gto \
    --mirror --exposure 900 \
    --output pm4n/Flow_Controller_Panel-F_Silkscreen.pm4n
    
pcb-expose.sh Dummy.pm4n gerbers/Flow_Controller_Panel-B_Silkscreen.gbo \
    --exposure 900 \
    --output pm4n/Flow_Controller_Panel-B_Silkscreen.pm4n

5. Verify

Open the .pm4n files in Chitubox Basic slicer to visually verify before printing. See the section 4. Check the printer exposure.

Troubleshooting

kicad-cli: command not found — add KiCad to PATH:

export PATH="/usr/lib/kicad/bin:$PATH"

Or on Flatpak:

alias kicad-cli='flatpak run --command=kicad-cli org.kicad.KiCad'

Expected Gerber not found — KiCad's layer→filename mapping:

Layer	Filename stem
`F.Cu`	`Front`
`B.Cu`	`Back`
`F.Mask`	`F_Mask`
`B.Mask`	`B_Mask`
`F.SilkS`	`F_Silkscreen`

Readme.md Unescape Escape

MSLA PCB Exposure: KiCad → Photon Mono 4

Why MSLA?