kopia lustrzana https://github.com/jaseg/gerbolyze
711 wiersze
32 KiB
ReStructuredText
711 wiersze
32 KiB
ReStructuredText
Gerbolyze high-fidelity SVG/PNG/JPG to PCB converter
|
|
====================================================
|
|
|
|
.. note::
|
|
|
|
The command-line usage and SVG template format of gerbolyze changed between v2.0 and v3.0. You can find details on
|
|
the new format below under command_line_usage_
|
|
|
|
Gerbolyze renders SVG vector and PNG/JPG raster images into existing gerber PCB manufacturing files.
|
|
Vector data from SVG files is rendered losslessly *without* an intermediate rasterization/revectorization step.
|
|
Still, gerbolyze supports (almost) the full SVG 1.1 spec including complex, self-intersecting paths with holes,
|
|
patterns, dashes and transformations.
|
|
|
|
Raster images can either be vectorized through contour tracing (like gerbolyze v1.0 did) or they can be embedded using
|
|
high-resolution grayscale emulation while (mostly) guaranteeing trace/space design rules.
|
|
|
|
Try gerbolyze online at https://dyna.kokoroyukuma.de/gerboweb
|
|
|
|
.. figure:: pics/pcbway_sample_02_small.jpg
|
|
:width: 800px
|
|
|
|
Drawing by `トーコ Toko <https://twitter.com/fluffy2038/status/1317231121269104640>`__ converted using Gerbolyze and printed at PCBWay.
|
|
|
|
|
|
Tooling for PCB art is quite limited in both open source and closed source ecosystems. Something as simple as putting a
|
|
pretty picture on a PCB can be an extremely tedious task. Depending on the PCB tool used, various arcane incantations
|
|
may be necessary and even modestly complex images will slow down most PCB tools to a crawl.
|
|
|
|
Gerbolyze solves this problem in a toolchain-agnostic way by directly vectorizing SVG vector and PNG or JPG bitmap files
|
|
onto existing gerber layers. Gerbolyze processes any spec-compliant SVG and "gerbolyzes" SVG vector data into a Gerber
|
|
spec-compliant form. Gerbolyze has been tested against both the leading open-source KiCAD toolchain and the
|
|
industry-standard Altium Designer. Gerbolyze is written with performance in mind and will happily vectorize tens of
|
|
thousands of primitives, generating tens of megabytes of gerber code without crapping itself. With gerbolyze you can
|
|
finally be confident that your PCB fab's toolchain will fall over before yours does if you overdo it with the high-poly
|
|
anime silkscreen.
|
|
|
|
Gerbolyze is based on gerbonara_.
|
|
|
|
.. image:: pics/process-overview.png
|
|
:width: 800px
|
|
|
|
.. contents::
|
|
|
|
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:
|
|
|
|
.. code::
|
|
|
|
$ 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:
|
|
|
|
.. code::
|
|
|
|
$ gerbolyze paste --top template_top_edited.svg [--bottom ...] my_gerber_dir output_gerber_dir
|
|
|
|
Quick Start Installation (Any Platform)
|
|
---------------------------------------
|
|
|
|
.. code-block:: shell
|
|
|
|
python -m pip install --user gerbolyze resvg-wasi
|
|
|
|
If you already have resvg installed, you can omit the resvg-wasi package.
|
|
|
|
To uninstall, run
|
|
|
|
.. code-block:: shell
|
|
|
|
python -m pip uninstall gerbolyze gerbonara resvg-wasi svg-flatten-wasi
|
|
|
|
To update, run
|
|
|
|
.. code-block:: shell
|
|
|
|
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 <https://gitlab.com/gerbolyze/gerbolyze/-/pipelines?scope=tags&page=1>`__ 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.
|
|
|
|
|
|
Build from source (any distro)
|
|
~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
|
|
|
|
.. code-block:: shell
|
|
|
|
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.
|
|
|
|
.. image:: pics/test_svg_readme_composited.png
|
|
:width: 800px
|
|
|
|
* 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
|
|
------------------
|
|
.. _command_line_usage:
|
|
|
|
Generate SVG template from Gerber files:
|
|
|
|
.. code-block:: shell
|
|
|
|
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:
|
|
|
|
.. code-block:: shell
|
|
|
|
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:
|
|
|
|
.. code-block:: shell
|
|
|
|
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:
|
|
|
|
.. code-block:: shell
|
|
|
|
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.
|
|
|
|
.. code-block:: shell
|
|
|
|
svg-flatten [options] --format kicad --sexp-mod-name My_Module [input_file.svg] [output_file]
|
|
|
|
``gerbolyze template``
|
|
~~~~~~~~~~~~~~~~~~~~~~
|
|
|
|
Usage: ``gerbolyze template [OPTIONS] INPUT``
|
|
|
|
Generate SVG template for gerbolyze paste from gerber files.
|
|
|
|
INPUT may be a gerber file, directory of gerber files or zip file with gerber files. The output file contains a preview
|
|
image of the input gerbers to allow you to position your artwork, as well as prepared Inkscape layers corresponding to
|
|
each gerber layer. Simply place your artwork in this SVG template using Inkscape. Starting in v3.0, gerbolyze
|
|
automatically keeps track of which board side (top or bottom) is contained in an SVG template.
|
|
|
|
Options:
|
|
********
|
|
``--top | --bottom``
|
|
Output top or bottom side template. This affects both the preview image and the prepared Inkscape layers.
|
|
|
|
``--vector | --raster``
|
|
Embed preview renders into output file as SVG vector graphics instead of rendering them to PNG bitmaps. The
|
|
resulting preview may slow down your SVG editor.
|
|
|
|
``--raster-dpi FLOAT``
|
|
DPI for rastering preview
|
|
|
|
``--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.
|
|
|
|
|
|
``gerbolyze paste``
|
|
~~~~~~~~~~~~~~~~~~~
|
|
(see `below <vectorization_>`__)
|
|
|
|
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 <subtraction_script_>`_)
|
|
|
|
``--no-subtract``
|
|
Disable subtraction (see `below <subtraction_script_>`_)
|
|
|
|
``--dilate FLOAT``
|
|
Default dilation for subtraction operations in mm (see `below <subtraction_script_>`_)
|
|
|
|
``--trace-space FLOAT``
|
|
Passed through to svg-flatten, see `below <svg_flatten_>`__.
|
|
|
|
``--vectorizer TEXT``
|
|
Passed through to svg-flatten, see `its description below <svg_flatten_>`__. Also have a look at `the examples below <vectorization_>`_.
|
|
|
|
``--vectorizer-map TEXT``
|
|
Passed through to svg-flatten, see `below <svg_flatten_>`__.
|
|
|
|
``--exclude-groups TEXT``
|
|
Passed through to svg-flatten, see `below <svg_flatten_>`__.
|
|
|
|
|
|
.. _outline_layers:
|
|
|
|
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_script:
|
|
|
|
Subtraction scripts
|
|
*******************
|
|
|
|
.. image:: pics/subtract_example.png
|
|
:width: 800px
|
|
|
|
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:
|
|
|
|
.. code-block::
|
|
|
|
{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:
|
|
|
|
.. code-block::
|
|
|
|
out.silk -= in.mask
|
|
out.silk -= in.silk+0.5
|
|
out.mask -= in.mask+0.5
|
|
out.copper -= in.copper+0.5
|
|
|
|
.. _svg_flatten:
|
|
|
|
``svg-flatten``
|
|
~~~~~~~~~~~~~~~
|
|
|
|
Usage: ``svg-flatten [OPTIONS]... [INPUT_FILE] [OUTPUT_FILE]``
|
|
|
|
Specify ``-`` for stdin/stdout.
|
|
|
|
Options:
|
|
********
|
|
|
|
``-h, --help``
|
|
Print help and exit
|
|
|
|
``-v, --version``
|
|
Print version and exit
|
|
|
|
``-o, --format``
|
|
Output format. Supported: gerber, gerber-outline (for board outline layers), svg, s-exp (KiCAD S-Expression)
|
|
|
|
``-p, --precision``
|
|
Number of decimal places use for exported coordinates (gerber: 1-9, SVG: >=0). Note that not all gerber viewers are
|
|
happy with too many digits. 5 or 6 is a reasonable choice.
|
|
|
|
``--clear-color``
|
|
SVG color to use in SVG output for "clear" areas (default: white)
|
|
|
|
``--dark-color``
|
|
SVG color to use in SVG output for "dark" areas (default: black)
|
|
|
|
``-f, --flip-gerber-polarity``
|
|
Flip polarity of all output gerber primitives for --format gerber.
|
|
|
|
``-d, --trace-space``
|
|
Minimum feature size of elements in vectorized graphics (trace/space) in mm. Default: 0.1mm.
|
|
|
|
``--no-header``
|
|
Do not export output format header/footer, only export the primitives themselves
|
|
|
|
``--flatten``
|
|
Flatten output so it only consists of non-overlapping white polygons. This perform composition at the vector level.
|
|
Potentially slow. This defaults to on when using KiCAD S-Exp export because KiCAD does not know polarity or colors.
|
|
|
|
``--no-flatten``
|
|
Disable automatic flattening for KiCAD S-Exp export
|
|
|
|
``--dilate``
|
|
Dilate output gerber primitives by this amount in mm. Used for masking out other layers.
|
|
|
|
``-g, --only-groups``
|
|
Comma-separated list of group IDs to export.
|
|
|
|
``-b, --vectorizer``
|
|
Vectorizer to use for bitmap images. One of poisson-disc (default), hex-grid, square-grid, binary-contours,
|
|
dev-null. Have a look at `the examples below <vectorization_>`_.
|
|
|
|
``--vectorizer-map``
|
|
Map from image element id to vectorizer. Overrides --vectorizer. Format: id1=vectorizer,id2=vectorizer,...
|
|
|
|
You can use this to set a certain vectorizer for specific images, e.g. if you want to use both halftone
|
|
vectorization and contour tracing in the same SVG. Note that you can set an ``<image>`` element's SVG ID from within
|
|
Inkscape though the context menu's Object Properties tool.
|
|
|
|
``--force-svg``
|
|
Force SVG input irrespective of file name
|
|
|
|
``--force-png``
|
|
Force bitmap graphics input irrespective of file name
|
|
|
|
``-s, --size``
|
|
Bitmap mode only: Physical size of output image in mm. Format: 12.34x56.78
|
|
|
|
``--sexp-mod-name``
|
|
Module name for KiCAD S-Exp output. This is a mandatory argument if using S-Exp output.
|
|
|
|
``--sexp-layer``
|
|
Layer for KiCAD S-Exp output. Defaults to auto-detect layers from SVG layer/top-level group IDs. If given, SVG
|
|
groups and layers are completely ignored and everything is simply vectorized into this layer, though you cna still
|
|
use ``-g`` for group selection.
|
|
|
|
``-a, --preserve-aspect-ratio``
|
|
Bitmap mode only: Preserve aspect ratio of image. Allowed values are meet, slice. Can also parse full SVG
|
|
preserveAspectRatio syntax.
|
|
|
|
``--no-usvg``
|
|
Do not preprocess input using usvg (do not use unless you know *exactly* what you're doing)
|
|
|
|
``--usvg-dpi``
|
|
Passed through to usvg's --dpi, in case the input file has different ideas of DPI than usvg has.
|
|
|
|
``--scale``
|
|
Scale input svg lengths by this factor (-o gerber only).
|
|
|
|
``-e, --exclude-groups``
|
|
Comma-separated list of group IDs to exclude from export. Takes precedence over --only-groups.
|
|
|
|
.. _vectorization:
|
|
|
|
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]["," ...]``.
|
|
|
|
.. for f in vec_*.png; convert -background white -gravity center $f -resize 500x500 -extent 500x500 (basename -s .png $f)-square.png; end
|
|
.. for vec in hexgrid square poisson contours; convert vec_"$vec"_whole-square.png vec_"$vec"_detail-square.png -background transparent -splice 25x0+0+0 +append -chop 25x0+0+0 vec_"$vec"_composited.png; end
|
|
|
|
``--vectorizer poisson-disc`` (the default)
|
|
~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
|
|
|
|
.. image:: pics/vec_poisson_composited.png
|
|
:width: 800px
|
|
|
|
``--vectorizer hex-grid``
|
|
~~~~~~~~~~~~~~~~~~~~~~~~~
|
|
|
|
.. image:: pics/vec_hexgrid_composited.png
|
|
:width: 800px
|
|
|
|
``--vectorizer square-grid``
|
|
~~~~~~~~~~~~~~~~~~~~~~~~~~~~
|
|
|
|
.. image:: pics/vec_square_composited.png
|
|
:width: 800px
|
|
|
|
``--vectorizer binary-contours``
|
|
~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
|
|
|
|
.. image:: pics/vec_contours_composited.png
|
|
:width: 800px
|
|
|
|
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.
|
|
|
|
.. image:: screenshots/02import02.png
|
|
:width: 800px
|
|
|
|
2 Convert the image to grayscale
|
|
~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
|
|
|
|
.. image:: screenshots/06grayscale.png
|
|
:width: 800px
|
|
|
|
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.
|
|
|
|
.. image:: screenshots/08curve_cut.png
|
|
:width: 800px
|
|
|
|
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.
|
|
|
|
.. image:: screenshots/09retouch.png
|
|
:width: 800px
|
|
|
|
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.
|
|
|
|
.. image:: screenshots/10retouched.png
|
|
:width: 800px
|
|
|
|
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``.
|
|
|
|
.. image:: screenshots/11newsprint.png
|
|
:width: 800px
|
|
|
|
The following are examples on the detail resulting from the newsprint filter.
|
|
|
|
.. image:: screenshots/12newsprint.png
|
|
:width: 800px
|
|
|
|
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.
|
|
|
|
.. image:: screenshots/14result_cut.png
|
|
:width: 800px
|
|
|
|
.. image:: screenshots/15result_cut.png
|
|
:width: 800px
|
|
|
|
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
|
|
-----------
|
|
|
|
SVG raster features
|
|
~~~~~~~~~~~~~~~~~~~
|
|
|
|
Currently, SVG masks and filters are not supported. Though SVG is marketed as a "vector graphics format", these two
|
|
features are really raster primitives that all SVG viewers perform at the pixel level after rasterization. Since
|
|
supporting these would likely not end up looking like what you want, it is not a planned feature. If you need masks or
|
|
filters, simply export the relevant parts of the SVG as a PNG then include that in your template.
|
|
|
|
Gerber pass-through
|
|
~~~~~~~~~~~~~~~~~~~
|
|
|
|
Since gerbolyze has to composite your input gerbers with its own output, it has to fully parse and re-serialize them.
|
|
gerbolyze gerbonara_ for all its gerber parsing needs. Thus, gerbonara will interpret your gerbers and output will be in
|
|
gerbonara's gerber "dialect". If you find a corner case where this does not work and the output looks wrong, please file
|
|
a bug report with an example file on the gerbonara_ bug tracker. *Always* check the output files for errors before
|
|
submitting them to production.
|
|
|
|
Gerbolyze is provided without any warranty, but still please open an issue or `send me an email
|
|
<mailto:gerbolyze@jaseg.de>`__ if you find any errors or inconsistencies.
|
|
|
|
Trace/Space design rule adherence
|
|
~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
|
|
|
|
While the grayscale halftone vectorizers do a reasonable job adhering to a given trace/space design rule, they can still
|
|
produce small parts of output that violate it. For the contour vectorizer as well as for all SVG primitives, you are
|
|
responsible for adhering to design rules yourself as there is no algorithm that gerboyze could use to "fix" its input.
|
|
|
|
A design rule checker is planned as a future addition to gerbolyze, but is not yet part of it. If in doubt, talk to your
|
|
fab and consider doing a test run of your design before ordering assembled boards ;)
|
|
|
|
Gallery
|
|
-------
|
|
|
|
.. image:: pics/sample3.jpg
|
|
:width: 400px
|
|
|
|
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 <mailto:agpl.sucks@jaseg.de>`__ 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.
|
|
|
|
.. _usvg: https://github.com/RazrFalcon/resvg
|
|
.. _Inkscape: https://inkscape.org/
|
|
.. _pcb-tools: https://github.com/curtacircuitos/pcb-tools
|
|
.. _pcb-tools-extension: https://github.com/opiopan/pcb-tools-extension
|
|
.. _GIMP: https://gimp.org/
|
|
.. _gerbonara: https://gitlab.com/gerbolyze/gerbonara
|
|
.. _`Gerbolyze Protoboard Index`: https://dyna.kokoroyukuma.de/protos/
|
|
|