translate2geda

Update - March 2019 - refactoring, code cleanup, incorporation of Kicad MOdule and Footprint conversion, and enhanced support for polygons in footprints, padstacks, padstack rotation, arbitrary text features in footprints, arbitrary text rotation, and line elements on top copper in footprints has been effected in the translate2corelEDA utility which exports to pcb-rnd ( see http://repo.hu/projects/pcb-rnd/ ) lihata (.lht) format by default, which natively supports all of these features. The gerber importer has also been improved in translate2coralEDA to support copper arcs and polygons on top copper layer in footprint (aka subcircuit in pcb-rnd) features.

Users are encouraged to upgrade their tool chain to pcb-rnd, which can import Eagle, Kicad, Protel Autotrax, HPGL, Specctra, and gEDA PCB layouts, and save in its fully featured native lihata (.lht) file format, as well as export to various non native formats, subject to the limitations of other formats.

translate2geda, a utility for converting:

• Kicad (.mod, .lib) (refactoring in progress, please use kicadModule2geda or kicadSymbol2geda)
• Eagle (.lbr) (mostly working, minus polygons)
• BXL (.bxl) (working)
• IBIS (.ibs) (working)
• gschem symdef (working), and
• BSDL (.bsd) (working)
• LT-Spice (.asc) (working, if .asc file saved in utf-8 text format, not ISO-8859-*)
• QUCS (.sch) (nets convert, and preliminary symbol support working)
• gerber file (.gbr, .gbo, .gto, .gbs, .gts, .gbl, .gtl, .pho) ... a preliminary implementation
• hersheydata.py EggBot font definition files (working)

symbols and footprints and LT-Spice schematics and QUCS schematics and gerbers and fonts to geda compatible formats.

The Kicad portion of the utility is based on the KicadModuleToGEDA and KicadSymbolToGEDA utilities.

This utility extends the functionality of the software classes to allow additional formats to be converted.

Export to Kicad is planned once conversion functionality is in place and satisfactorily tested. This should not be difficult, since the utility uses nanometres internally and also uses many of the dimensions and flags internally that the Kicad format is based on. KiCad eeschema users needing to extract schematic symbols from BXL files can use the BXL2text utility until the export to KiCad eeschema (.lib) code is integrated into translate2geda.

Export to Eagle was planned, as Eagle was good enough to use an easily parsed XML format.

BXL files are a package and vendor agnostic device description format that includes pad, symbol and footprint definitions in a single binary file encoded with adaptive Huffman encoding. The adaptive Huffman decoding code was ported to Java from vala code originally written by Geert Jordaens.

Gerber files are parsed and decoded by code originally written by Phillip Knirsch to render and print gerbers: http://www.wizards.de/phil/java/rs274x.html The code has been modified to generate pins/pads and traces as footprint elements, and now detects inch/mm units. More work needs to be done to convert the gerber parsing routines to long int nanometres, unbreak the graphics exporting, and possibly generate PCB layout files which try to put traces into their own layer, distinct from footprint elements, although the heuristics will be subject to high false positive rates in some cases due to some EDA tools rendering pins/pads/polygons with painted strokes, instead of flashed apertures or polygons. Footprint elements are uniquely numbered, so that mouse over actions which show the pin number allow groups of pins to be identified with simple searches in the text .fp file and copied/combined if extracting device footprints from larger gerbers, etc...

BSDL files are boundary surface description language files that include a pin map which can be used to create a symbol.

IBIS files are similar in that a pin map allows a symbol to be generated.

Recent XML format Eagle .lbr files contain a set of layer definitions, packages (footprints), and symbols, but the pin mapping between symbols and footprints is defined in a "deviceset" section, to allow symbols to map to different packages. This has been dealt with by exporting an individual symbol with a pin mapping for each of the packages supported in the deviceset, with a distinct "_FOOTPRINTNAME" appended to each of the pin mappings defined in the deviceset, i.e. a symbol with three different pin mappings will result in three different symbols being generated with unique footprint=SPECIFICFP fields.

LT-Spice .asc files are text files exported by LT-Spice and capture the schematic used in LT-Spice for circuit modelling. The .asc file contains "WIRE"s which connect discrete components, references to component symbols, and attributes for the components such as their value and refdes. Until the code is updated to cope, use .asc files saved in utf-8 to avoid generating empty .sch files.

QUCS .sym files are text files exported by QUCS (Quite Universal Circuit Simulator) and capture the schematic used in QUCS for circuit modelling. The .sch file contains "WIRE"s which connect discrete components, references to component symbols, and attributes for the components such as their value and refdes.

EggBot hersheydata.py files containing NIST style font definitions are converted into font definitions that are compatible with gEDA PCB/pcb-rnd. The font definitions are printed to the console and need to be captured in a file for subsequent use. There are currently 51 fonts available under either the NIST Hershey Font licence or the SIL Open Font Licence.

Main differences:

X and Y coordinate systems are the same in gEDA and Kicad, with Y +ve downwards, but Kicad uses +ve CW rotation and decidegrees for arcs and circles.

Both gEDA and Eagle use degrees, and CCW +ve for rotation, but in Eagle the X and Y coordinate system has Y up +ve.

BXL files have +ve up, but +ve CCW for rotation and degrees, like gEDA.

Eagle files can specify zero line widths, relying on default line width value for silk features. This utility defaults to 10mil (0.010 inch) line width if a zero line width is encountered.

Eagle can specify polygons in footprint definitions, which are not supported in geda PCB. The utility flags converted footprints with polygons that could not be converted.

LT-Spice has +ve Y down, unlike gschem. Rotation is in the opposite direction to gschem. The grid in LT-Spice increase in mutiples of 16, and a conversion factor of 12.5 achieves pin spacings which are multiples of 100, and suited to gschem. For the WIREs in LT-Spice to connect properly in the converted gschem schematic, custom gschem symbols have been generated which match the dimensions and pinouts of the default LT-Spice components. These end in -LTS.sym, and need to be in the default search path of gschem when gschem is used to view and edit the converted schematic.

QUCs has +ve Y down, unlike gschem. Rotation is +ve CCW. Grid increments are in units of 10, and most symbols have pin spacings of 60, allowing for a magnification factor of 10 to be applied. Custom symbols also need to be installed in the gschem search path, as with LT-Spice.

Disclaimer:

This utility aims to avoid excessive reinvention of the wheel and aims to facilitate sharing of design efforts. As always, converter output is not guaranteed to be error free, and footprints should be carefully checked before using them in designs for which gerber files will be sent off for manufacture.

Issues:

• other EDA tools do not necessarily enforce sane pin spacings in their symbols, or grid aligned pins. Work is underway to flag such symbols and offer enforced grid spacing, at the risk of wrecking silk features/overall aesthetics.
• pin mappings in other EDA suites do not necessarily conform to gEDA guidelines, but replacing the pin mappings with non-text, i.e. numbers, risks a loss of information and the introduction of errors - an aim is to minimise information loss as much as possible during conversion.
• trapezoidal pads in Kicad and polygonal pads in Eagle are not supported yet, but work is underway to convert them to gEDA PCB compatible features.
• polygonal pads in BXL files are unsupported but identified, at which point a message to stdout is generated, and the pad is replaced with a readily identifiable, small circular pad, and BXL file processing continues.
• Eagle is very flexible in how it defines "slots", and a relatively foolproof way of converting Eagle "gates" into geda "slots" eludes me for now.
• LTSpice components have their position, value and refdes converted.
• QUCS components have their position and refdes converted, but component values are only ported for resistors, inductors and capacitors.
• BXL conversion uses Adaptive Huffman Decoding. This takes a lot of shuffling of nodes within trees. You can still wander off and make some coffee while it decodes, but it is much much faster now thanks to better String handling suggested by https://github.com/wlbaker who identified the bottleneck and remedied it.
• QUCS compatible symbols included in the symbols directory should have the correct geometry in the converted schematic, but pinouts need to be checked before proceeding to allocate footprints and generating a PCB layout, since QUCS is not very explicit about which physical pin goes where.
• kerning in converted Eggbot Fonts may need fine tuning.

Usage:

Install a git client, java virtual machine, and java compiler to suit your operating system

git clone https://github.com/erichVK5/translate2geda.git
cd translate2geda
javac *.java
java translate2geda someFile.lbr [-o optional/output/directory/path/including/slashes/]

The utility will use the file ending of the provided file (.symdef, .mod, .lib, .bxl, .ibs, .bsd, etc) to determine which parser is required.

To do:

• open JSON format conversion
• Kicad import/export
• Kicad trapezoidal pad support
• Eagle polygons
• flagging +/- optional enforcement of desired symbol pin spac