Gerbolyze

Tl;dr: Produce high-quality artistic PCBs in three easy steps!

Gerbolyze works in three steps.

1. Generate a scale-accurate template of the finished PCB from your CAD tool's gerber output:

   $ gerbolyze template --top template_top.svg [--bottom template_bottom.svg] my_gerber_dir
   

2. Load the resulting template image Inkscape or another SVG editing program. Put your artwork on the appropriate SVG layer. Dark colors become filled gerber primitives, bright colors become unfilled primitives. You can directly put raster images (PNG/JPG) into this SVG as well, just position and scale them like everything else. SVG clips work for images, too. Masks are not supported.

3. Vectorize the edited SVG template image drectly into the PCB's gerber files:

   $ gerbolyze paste --top template_top_edited.svg [--bottom ...] my_gerber_dir output_gerber_dir
   

Quick Start Installation (Any Platform)

python -m pip install --user gerbolyze

To uninstall, run

python -m pip uninstall gerbolyze gerbonara resvg-wasi svg-flatten-wasi

To update, run

python -m pip install --user --upgrade --upgrade-strategy eager gerbolyze

Speeding up gerbolyze using natively-built binaries

This will install gerbolyze's binary dependency resvg and gerbolyze's svg-flatten utility as pre-built cross-platform WASM binaries. When you first run gerbolyze, it will take some time (~30s) to link these binaries for your system. The output is cached, so any future run is going to be fast.

WASM is slower than natively-built binaries. To speed up gerbolyze, you can natively build its two binary dependencies:

1. Install resvg natively using rust's cargo package manager: cargo install resvg
2. Install gerbolyze's svg-flatten utility natively. You can get pre-built binaries from gerbolyze's gitlab CI jobs at this link by clicking the three dots on the right next to the version you want. These pre-built binaries should work on any x86_64 linux since they are statically linked. You can also build svg-flatten yourself by running make inside the svg-flatten folder from a gerbolyze checkout.

Gerbolyze will pick up these binaries when installed in your $PATH. resvg is also picked up when it is installed by cargo in your home's ~/.cargo, even if it's not in your $PATH. You can override the resvg, usvg or svg-flatten binary that gerbolyze uses by giving it the absoulute path to a binary in the $RESVG, $USVG and $SVG_FLATTEN environment variables.

git clone --recurse-submodules https://git.jaseg.de/gerbolyze.git
cd gerbolyze

python3 -m venv
source venv/bin/activate
python3 setup.py install

Features

Input on the left, output on the right.

• Almost full SVG 1.1 static spec coverage (!)
  • Paths with beziers, self-intersections and holes
  • Strokes, even with dashes and markers
  • Pattern fills and strokes
  • Transformations and nested groups
  • Proper text rendering with support for complex text layout (e.g. Arabic)
  • <image> elements via either built-in vectorizer or built-in halftone processor
  • (some) CSS
• Writes Gerber, SVG or KiCAD S-Expression (.kicad_mod) formats
• Can export from top/bottom SVGs to a whole gerber layer stack at once with filename autodetection
• Can export SVGs to .kicad_mod files like svg2mod (but with full SVG support)
• Beziers flattening with configurable tolerance using actual math!
• Polygon intersection removal
• Polygon hole removal (!)
• Optionally vector-compositing of output: convert black/white/transparent image to black/transparent image
• Renders SVG templates from input gerbers for accurate and easy scaling and positioning of artwork
• layer masking with offset (e.g. all silk within 1mm of soldermask)
• Can read gerbers from zip files
• Limited SVG support for board outline layers (no fill/region support)
• Dashed lines supported on board outline layers

Gerbolyze is the end-to-end "paste this svg into these gerbers" command that handles all layers on both board sides at once. The heavy-duty computer geometry logic of gerbolyze is handled by the svg-flatten utility (svg-flatten directory). svg-flatten reads an SVG file and renders it into a variety of output formats. svg-flatten can be used like a variant of the popular svg2mod that supports all of SVG and handles arbitrary input <path> elements.

Algorithm Overview

This is the algorithm gerbolyze uses to process a stack of gerbers.

• Map input files to semantic layers by their filenames
• For each layer:
  • load input gerber
  • Pass mask layers through gerbv for conversion to SVG
  • Pass mask layers SVG through svg-flatten --dilate
  • Pass input SVG through svg-flatten --only-groups [layer]
  • Overlay input gerber, mask and input svg
  • Write result to output gerber

This is the algorithm svg-flatten uses to process an SVG.

• pass input SVG through usvg
• iterate depth-first through resulting SVG.
  • for groups: apply transforms and clip and recurse
  • for images: Vectorize using selected vectorizer
  • for paths:
    • flatten path using Cairo
    • remove self-intersections using Clipper
    • if stroke is set: process dash, then offset using Clipper
    • apply pattern fills
    • clip to clip-path
    • remove holes using Clipper
• for KiCAD S-Expression export: vector-composite results using CavalierContours: subtract each clear output primitive from all previous dark output primitives

Web interface

You can try gerbolyze online at https://dyna.kokoroyukuma.de/gerboweb

The web interface does not expose all of gerbolyze's bells and whistles, but it allows you to simply paste a single SVG file on a board to try out gerbolyze. Upload your design on the web interface, then download the template for either the top or bottom side, and put your artwork on the appropriate layer of that template using Inkscape. Finally, upload the modified template and let gerbolyze process your design.

Command-line usage

Generate SVG template from Gerber files:

gerbolyze template [options] [--top|--bottom] input_dir_or.zip output.svg

Render design from an SVG made with the template above into a set of gerber files:

gerbolyze paste [options] artwork.svg input_dir_or.zip output_dir_or.zip

Use svg-flatten to convert an SVG file into Gerber or flattened SVG:

svg-flatten [options] --format [gerber|svg] [input_file.svg] [output_file]

Use svg-flatten to convert an SVG file into the given layer of a KiCAD S-Expression (.kicad_mod) file:

svg-flatten [options] --format kicad --sexp-layer F.SilkS --sexp-mod-name My_Module [input_file.svg] [output_file]

Use svg-flatten to convert an SVG file into a .kicad_mod with SVG layers fed into separate KiCAD layers based on their IDs like the popular svg2mod is doing:

Note:

Right now, the input SVG's layers must have ids that match up KiCAD's s-exp layer names. Note that when you name a layer in Inkscape that only sets a name attribute, but does not change the ID. In order to change the ID in Inkscape, you have to use Inkscape's "object properties" context menu function.

Also note that svg-flatten expects the layer names KiCAD uses in their S-Expression format. These are different to the layer names KiCAD exposes in the UI (even though most of them match up!).

For your convenience, there is an SVG template with all the right layer names and IDs located next to this README.

svg-flatten [options] --format kicad --sexp-mod-name My_Module [input_file.svg] [output_file]

gerbolyze paste

(see below)

Usage: gerbolyze paste [OPTIONS] INPUT_GERBERS OVERLAY_SVG OUTPUT_GERBERS

Render vector data and raster images from SVG file into gerbers. The SVG input file can be generated using gerbolyze template and contains the name and board side of each layer. Note that for board outline layers, handling slightly differs from other layers as PCB fabs do not support filled Gerber regions on these layers.

Options:

--bbox TEXT

Output file bounding box. Format: "w,h" to force [w] mm by [h] mm output canvas OR "x,y,w,h" to force [w] mm by [h] mm output canvas with its bottom left corner at the given input gerber coördinates. This must match the ``--bbox`` value given to template!

--subtract TEXT

Use user subtraction script from argument (see below)

--no-subtract

Disable subtraction (see below)

--dilate FLOAT

Default dilation for subtraction operations in mm (see below)

--trace-space FLOAT

Passed through to svg-flatten, see below.

--vectorizer TEXT

Passed through to svg-flatten, see its description below. Also have a look at the examples below.

--vectorizer-map TEXT

Passed through to svg-flatten, see below.

--exclude-groups TEXT

Passed through to svg-flatten, see below.

Outline layers

Outline layers require special handling since PCB fabs do not support filled G36/G37 polygons on these layers. The main difference between normal layers and outline layers is how strokes are handled. On outline layers, strokes are translated to normal Gerber draw commands (D01, D02 etc.) with an aperture set to the stroke's width instead of tracing them to G36/G37 filled regions. This means that on outline layers, SVG end caps and line join types do not work: All lines are redered with round joins and end caps.

One exception from this are patterns, which work as expected for both fills and strokes with full support for joins and end caps.

Dashed strokes are supported on outline layers and can be used to make easy mouse bites.

Subtraction scripts

Subtraction scripts tell gerbolyze paste to remove an area around certain input layers to from an overlay layer. When a input layer is given in the subtraction script, gerbolyze will dilate (extend outwards) everything on this input layer and remove it from the target overlay layer. By default, Gerbolyze subtracts the mask layer from the silk layer to make sure there are no silk primitives that overlap bare copper, and subtracts each input layer from its corresponding overlay to make sure the two do not overlap. In the picture above you can see both at work: The overlay contains halftone primitives all over the place. The subtraction script has cut out an area around all pads (mask layer) and all existing silkscreen. You can turn off this behavior by passing --no-subtract or pass your own "script".

The syntax of these scripts is:

{target layer} -= {source layer} {dilation} [; ...]

The target layer must be out.{layer name} and the source layer in.{layer name}. The layer names are gerbolyze's internal layer names, i.e.: paste, silk, mask, copper, outline, drill

The dilation value is optional, but can be a float with a leading + or -. If given, before subtraction the source layer's features will be extended by that many mm. If not given, the dilation defaults to the value given by --dilate if given or 0.1 mm otherwise. To disable dilation, simply pass +0 here.

Multiple commands can be separated by semicolons ; or line breaks.

The default subtraction script is:

out.silk -= in.mask
out.silk -= in.silk+0.5
out.mask -= in.mask+0.5
out.copper -= in.copper+0.5

Gerbolyze image vectorization

Gerbolyze has two built-in strategies to translate pixel images into vector images. One is its built-in halftone processor that tries to approximate grayscale. The other is its built-in binary vectorizer that traces contours in black-and-white images. Below are examples for the four options.

The vectorizers can be used in isolation through svg-flatten with either an SVG input that contains an image or a PNG/JPG input.

The vectorizer can be controlled globally using the --vectorizer flag in both gerbolyze and svg-flatten. It can also be set on a per-image basis in both using --vectorizer-map [image svg id]=[option]["," ...].

--vectorizer poisson-disc (the default)

--vectorizer hex-grid

--vectorizer square-grid

--vectorizer binary-contours

The binary contours vectorizer requires a black-and-white binary input image. As you can see, like every bitmap tracer it will produce some artifacts. For artistic input this is usually not too bad as long as the input data is high-resolution. Antialiased edges in the input image are not only OK, they may even help with an accurate vectorization.

GIMP halftone preprocessing guide

Gerbolyze has its own built-in halftone processor, but you can also use the high-quality "newsprint" filter built into GIMP instead if you like. This section will guide you through this. The PNG you get out of this can then be fed into gerbolyze using --vectorizer binary-contours.

1 Import your desired artwork

Though anime or manga pictures are highly recommended, you can use any image including photographs. Be careful to select a picture with comparatively low detail that remains recognizable at very low resolution. While working on a screen this is hard to vizualize, but the grain resulting from the low resolution of a PCB's silkscreen is quite coarse.

2 Convert the image to grayscale

3 Fine-tune the image's contrast

To look well on the PCB, contrast is critical. If your source image is in color, you may have lost some contrast during grayscale conversion. Now is the time to retouch that using the GIMP's color curve tool.

When using the GIMP's newsprint filter, bright grays close to white and dark grays close to black will cause very small dots that might be beyond your PCB manufacturer's maximum resolution. To control this case, add small steps at the ends of the grayscale value curve as shown (exaggerated) in the picture below. These steps saturate very bright grays to white and very dark grays to black while preserving the values in the middle.

4 Retouch details

Therer might be small details that don't look right yet, such as the image's background color or small highlights that merge into the background now. You can manually change the color of any detail now using the GIMP's flood-fill tool.

If you don't want the image's background to show up on the final PCB at all, just make it black.

Particularly on low-resolution source images it may make sense to apply a blur with a radius similar to the following newsprint filter's cell size (10px) to smooth out the dot pattern generated by the newsprint filter.

In the following example, I retouched the highlights in the hair of the character in the picture to make them completely white instead of light-gray, so they still stand out nicely in the finished picture.

5 Run the newsprint filter

Now, run the GIMP's newsprint filter, under filters, distorts, newsprint.

The first important settings is the spot size, which should be larger than your PCB's minimum detail size (about 10px with gerbolyze render default settings for good-quality silkscreen). In general the cheap and fast standard option of chinese PCB houses will require a larger detail size, but when you order specialty options like large size, 4-layer or non-green color along with a longer turnaround time you'll get much better-quality silk screen.

The second important setting is oversampling, which should be set to four or slightly higher. This improves the result of the edge reconstruction of gerbolyze vectorize.

The following are examples on the detail resulting from the newsprint filter.

6 Export the image for use with gerbolyze vectorize

Simply export the image as a PNG file. Below are some pictures of the output gerbolyze vectorize produced for this example.

Manufacturing Considerations

The main consideration when designing artwork for PCB processes is the processes' trace/space design rule. The two things you can do here is one, to be creative with graphical parts of the design and avoid extremely narrow lines, wedges or other thin features that will not come out well. Number two is to keep detail in raster images several times larger than the manufacturing processes native capability. For example, to target a trace/space design rule of 100 µm, the smallest detail in embedded raster graphics should not be much below 1mm.

Gerbolyze's halftone vectorizers have built-in support for trace/space design rules. While they can still produce small artifacts that violate these rules, their output should be close enough to satifsy board houses and close enough for the result to look good. The way gerbolyze does this is to clip the halftone cell's values to zero whenevery they get too small, and to forcefully split or merge two neighboring cells when they get too close. While this process introduces slight steps at the top and bottom of grayscale response, for most inputs these are not noticeable.

On the other hand, for SVG vector elements as well as for traced raster images, Gerbolyze cannot help with these design rules. There is no heuristic that would allow Gerbolyze to non-destructively "fix" a design here, so all that's on the roadmap here is to eventually include a gerber-level design rule checker.

As far as board houses go, I have made good experiences with the popular Chinese board houses. In my experience, JLC will just produce whatever you send them with little fucks being given about design rule adherence or validity of the input gerbers. This is great if you just want artistic circuit boards without much of a hassle, and you don't care if they come out exactly as you imagined. The worst I've had happen was when an older version of gerbolyze generated polygons with holes assuming standard fill-rule processing. The in the board house's online gerber viewer things looked fine, and neither did they complain during file review. However, the resulting boards looked completely wrong because all the dark halftones were missing.

PCBWay on the other hand has a much more rigurous file review process. They <em>will</em> complain when you throw illegal garbage gerbers at them, and they will helpfully guide you through your design rule violations. In this way you get much more of a professional service from them and for designs that have to be functional their higher level of scrutiny definitely is a good thing. For the design you saw in the first picture in this article, I ended up begging them to just plot my files if it doesn't physically break their machines and to their credit, while they seemed unhappy about it they did it and the result looks absolutely stunning.

PCBWay is a bit more expensive on their lowest-end offering than JLC, but I found that for anything else (large boards, multi-layer, gold plating etc.) their prices match. PCBWay offers a much broader range of manufacturing options such as flexible circuit boards, multi-layer boards, thick or thin substrates and high-temperature substrates.

When in doubt about how your design is going to come out on the board, do not hesitate to contact your board house. Most of the end customer-facing online PCB services have a number of different factories that do a number of different fabrication processes for them depending on order parameters. Places like PCBWay have exceptional quality control and good customer service, but that is mostly focused on the technical aspects of the PCB. If you rely on visual aspects like silkscreen uniformity or solder mask color that is a strong no concern to everyone else in the electronics industry, you may find significant variations between manufacturers or even between orders with the same manufacturer and you may encounter challenges communicating your requirements.

Limitations

Gallery

For a demonstration of gerbolyze convert, check out the Gerbolyze Protoboard Index, where you can download gerber files for over 7.000 SMD and THT protoboard layouts.

Licensing

This tool is licensed under the rather radical AGPLv3 license. Briefly, this means that you have to provide users of a webapp using this tool in the backend with this tool's source.

I get that some people have issues with the AGPL. In case this license prevents you from using this software, please send me an email and I can grant you an exception. I want this software to be useful to as many people as possible and I wouldn't want the license to be a hurdle to anyone. OTOH I see a danger of some cheap board house just integrating a fork into their webpage without providing their changes back upstream, and I want to avoid that so the default license is still AGPL.