Delta Gerber

A Java library for parsing Gerber RS-274X and Excellon NC drill files with SVG and PNG rendering, realistic PCB visualization, and an interactive web viewer.

Try the online viewer at deltaproto.com — no install needed, runs in your browser.

Realistic PCB Rendering

Generate photorealistic top and bottom views of your PCB with proper layer stacking — FR4 substrate, copper with HASL/ENIG finish, semi-transparent soldermask, silkscreen, and drill holes with true SVG transparency.

Board Top	Board Bottom

All Layers	Realistic Top

Maven Dependency

<dependency>
    <groupId>com.deltaproto</groupId>
    <artifactId>delta-gerber</artifactId>
    <version>1.1.6</version>
</dependency>

Features

Gerber Parsing

• Full RS-274X support (.gbr, .ger, .gtl, .gbl, .gts, .gbs, .gto, .gbo, .gtp, .gbp, .gko, .gm, etc.)
• All standard apertures: circle (C), rectangle (R), obround (O), polygon (P)
• Aperture macros with primitives (circle, vector line incl. legacy code 2, center line, outline, polygon, moiré, thermal) with variable expressions
• Region fills (G36/G37) with multiple contours
• Arc interpolation (G02/G03) with single and multi-quadrant modes
• Layer polarity (LPD/LPC) with true SVG mask-based transparency
• Step and Repeat (%SR%) for panelized boards
• Block apertures (%AB%) with full flash expansion, nesting, transforms and LPC polarity toggling
• Aperture transforms: rotation (LR), scaling (LS), mirroring (LM)
• Full Gerber X3 / X2 attribute compliance — every standard attribute (TF file, TA aperture, TO object, TD delete) is parsed into a typed, queryable model verified against the Ucamco 2024.05 specification:
  • File: .FileFunction, .FilePolarity, .Part, .GenerationSoftware, .CreationDate, .ProjectId, .MD5, .SameCoordinates
  • Aperture: the complete .AperFunction set (32 values, typed enum), .DrillTolerance (mm-normalized), .FlashText
  • Object / X3 assembly: nets (.N), pins (.P), component refdes (.C) and the full .Cxxx component characteristics — value, mfr, MPN, mount, rotation, package, library, and height (.CHgt, mm-normalized) — plus pick-and-place centroid extraction
• Image polarity (%IP%): negative-image inversion rendering; image offset (%OF%) recognition

Excellon Drill Parsing

• Standard Excellon NC drill format (.drl, .txt, .xln, .drd)
• Tool definitions with diameter
• Drill hits and routed slots (G85, M15/M16/M17 routing mode)
• Plated (PTH) and non-plated (NPTH) hole distinction
• Absolute and incremental coordinate modes (G90/G91)
• Metric and inch units with automatic format detection

IPC-D-356A Netlist Parsing

• Bare-board electrical-test netlist reader (.ipc, .ipc356) for connectivity / test-point data
• Test points: 317 through-hole, 327 SMD, 367 non-plated tooling, 307 blind/buried via — with net, ref-des/pin (incl. VIA and mid-net M), hole + plating, access side, location, feature size and rotation, soldermask
• Conductor segments (378/078) with modal coordinates and space/asterisk-delimited chains, net adjacency (379/079), and board/panel outlines (389/089)
• Continuation records: 017/027 hole, 099 test-point location, 088 soldermask clearance
• Long-net-name aliases (P NNAME), resolved into full net names — tolerates the non-standard Allegro alias-as-comment quirk
• Coordinates and sizes normalized to mm at parse time (from CUST 0.0001 inch or SI 0.001 mm), sharing one coordinate space with Gerber/drill geometry
• Non-fatal parse warnings (missing P UNITS, unknown op codes, truncated records) instead of exceptions

CAD Tool Compatibility

• Altium Designer — Gerber X2 attributes, mechanical layer outlines (.GM, .GM1), format detection
• Cadence Allegro — Non-standard drill format with holesize comments, M00 tool separators, repeat codes (R02X...)
• EAGLE — Non-standard OC8/OCn octagon aperture type, combined FS+MO command blocks
• KiCad — Standard Gerber X2 output with file function attributes
• Legacy RS-274X — Deprecated G-codes (G54, G70/G71), deprecated extended commands (%IN, %LN, %AS, %MI, %SF, %IR%)
• UTF-8 BOM handling for files exported from Windows tools

SVG Rendering

• High-fidelity SVG output with native SVG elements (circles, arcs, paths)
• Polygonized mode for geometry processing
• Multi-layer composite rendering with configurable colors and opacity
• Realistic PCB rendering with physically accurate layer stacking:
  • FR4 substrate, copper (silver under mask / gold at exposed pads)
  • Semi-transparent soldermask with inverted mask for pad openings
  • Silkscreen nested inside soldermask (only visible where mask is present)
  • Drill holes punching through all layers as true SVG transparency
• Derived board outline when no GKO/outline layer is present — the board edge is reconstructed from the copper-union silhouette so the realistic view still works

PNG / Raster Output

• Per-layer PNG export for single Gerber or drill layers (SVGRenderer.renderPng, DrillSVGRenderer.renderPng) — ideal for feeding individual layers to vision models
• Realistic top/bottom PNGs (renderRealisticSidePng), dimension-clamped to keep memory bounded on large boards
• Scale-aware export (renderRealisticSidePngWithScale → PngWithScale) carrying px↔mm geometry, embedded directly in the PNG via pHYs + tEXt chunks
• Board overview PNG (renderBoardOverviewPng) — composites the realistic board over an all-layers underlay so off-board annotations (drill charts, stackup tables, fab notes) stay visible; scales to dense multi-layer boards via a raster silhouette path

Parse Diagnostics

• Both Gerber and drill documents expose a de-duplicated list of parse warnings
• Malformed, truncated, or hostile files degrade gracefully with a recorded warning instead of crashing or producing a blank render

Web Viewer

• Interactive pan/zoom with mouse wheel and drag
• Three visualization modes: All Layers, Board Top, Board Bottom
• PNG Top/Bottom export of the realistic view
• Warnings tab listing per-file parse warnings (disabled when there are none)
• Layer type auto-detection from filename and content analysis
• Layer type dropdowns for manual override
• Select all/none checkbox with tri-state indicator
• Top/Bottom quick-filter buttons
• Hover-to-solo: preview individual layers by hovering
• Center-truncated filenames with instant tooltips
• Browser-side ZIP extraction and file persistence (IndexedDB)
• Recent project history with re-open support
• Stateless server architecture (browser owns the data)

Quick Start — Download and Run

Download the standalone JAR from the latest release and run:

java -jar delta-gerber-1.1.6-jar-with-dependencies.jar

Open http://localhost:938 and drop a Gerber ZIP file onto the viewer, or click "Try Example" to load the bundled Arduino Uno board.

Requires Java 17+. No other dependencies needed.

Build from Source

mvn clean package
java -jar target/delta-gerber-1.1.6-jar-with-dependencies.jar

Usage as Library

// Parse a Gerber file
GerberParser parser = new GerberParser();
GerberDocument doc = parser.parse(gerberContent);

// Render a single layer to SVG
SVGRenderer renderer = new SVGRenderer();
String svg = renderer.render(doc);

// Parse an Excellon drill file
ExcellonParser drillParser = new ExcellonParser();
DrillDocument drillDoc = drillParser.parse(excellonContent);

Multi-Layer Rendering

MultiLayerSVGRenderer renderer = new MultiLayerSVGRenderer();
List<MultiLayerSVGRenderer.Layer> layers = new ArrayList<>();
layers.add(new MultiLayerSVGRenderer.Layer("top-copper", copperDoc)
    .setColor("#e94560").setOpacity(0.85));
layers.add(new MultiLayerSVGRenderer.Layer("drill", drillDoc)
    .setColor("#00ffff"));

String svg = renderer.render(layers);

Component Placement (Pick-and-Place / Centroid)

KiCad and other EDA tools can export component placement data as Gerber X2 files with %TF.FileFunction,Component,...*%. The parser extracts the centroid of each component and makes it available as a List<ComponentPlacement>.

GerberParser parser = new GerberParser();
GerberDocument doc = parser.parse(pnpFileContent);

if (doc.isComponentFile()) {
    String side = doc.getComponentSide(); // "Top" or "Bottom"
    List<ComponentPlacement> components = doc.getComponents();

    for (ComponentPlacement c : components) {
        System.out.printf("%s\t%s\t%s\t%.4f\t%.4f\t%.1f\t%s%n",
            c.getRefdes(),     // e.g. "R1"
            c.getValue(),      // e.g. "10k"
            c.getFootprint(),  // e.g. "R_0402_1005Metric"
            c.getX(),          // centroid X in mm
            c.getY(),          // centroid Y in mm
            c.getRotation(),   // degrees
            c.getSide());      // "Top" or "Bottom"
    }
}

Export to CSV:

StringBuilder csv = new StringBuilder("Designator,Value,Footprint,MountType,X_mm,Y_mm,Rotation_deg,Side\n");
for (ComponentPlacement c : doc.getComponents()) {
    csv.append(String.format(Locale.US, "\"%s\",\"%s\",\"%s\",\"%s\",%.4f,%.4f,%.2f,\"%s\"%n",
        c.getRefdes(), c.getValue(), c.getFootprint(), c.getMountType(),
        c.getX(), c.getY(), c.getRotation(), c.getSide()));
}
Files.writeString(Path.of("centroid.csv"), csv.toString());

If you have separate top and bottom PnP files, parse each one independently and combine the lists:

GerberParser parser = new GerberParser();
List<ComponentPlacement> all = new ArrayList<>();
all.addAll(parser.parse(pnpTopContent).getComponents());
all.addAll(parser.parse(pnpBottomContent).getComponents());

Each coordinate is in millimetres, normalised at parse time regardless of the source file unit. The mountType field is "SMD" or "TH" as declared in %TO.CMnt*%.

Realistic PCB Rendering

MultiLayerSVGRenderer renderer = new MultiLayerSVGRenderer();
List<MultiLayerSVGRenderer.Layer> layers = new ArrayList<>();

layers.add(new MultiLayerSVGRenderer.Layer("outline", outlineDoc)
    .setLayerType(LayerType.OUTLINE));
layers.add(new MultiLayerSVGRenderer.Layer("copper", copperDoc)
    .setLayerType(LayerType.COPPER_TOP));
layers.add(new MultiLayerSVGRenderer.Layer("mask", soldermaskDoc)
    .setLayerType(LayerType.SOLDERMASK_TOP));
layers.add(new MultiLayerSVGRenderer.Layer("silk", silkscreenDoc)
    .setLayerType(LayerType.SILKSCREEN_TOP));
layers.add(new MultiLayerSVGRenderer.Layer("drill", drillDoc)
    .setLayerType(LayerType.DRILL));

String realisticSvg = renderer.renderRealistic(layers);

Soldermask Color

The realistic view (and the PNG paths built on it) defaults to a realistic dark green soldermask. Pick one of the standard fab colors with setSoldermaskColor. Each color carries its paired silkscreen color — white on every color except white soldermask, which uses black silkscreen:

MultiLayerSVGRenderer renderer = new MultiLayerSVGRenderer()
    .setSoldermaskColor(SoldermaskColor.RED);   // green (default), purple, red, yellow, blue, white, black

String realisticSvg = renderer.renderRealistic(layers);

The SoldermaskColor palette matches the colors common fabricators (e.g. JLCPCB) offer. SoldermaskColor.GREEN keeps a deliberately darker mask shade (#004200) rather than the brighter advertised swatch green — at the soldermask's semi-transparent opacity over copper/FR4 it blends to a realistic board green. For a color outside the palette, pass explicit mask + silkscreen hex fills:

renderer.setSoldermaskColor("#102a4c", "#ffffff");   // custom navy mask, white silk

PNG Export

All renderers can rasterize straight to PNG through the shared Batik pipeline.

// A single layer to PNG (e.g. a fab drawing or drill legend for a vision model)
byte[] layerPng = new SVGRenderer().renderPng(copperDoc, 1024);
byte[] drillPng = new DrillSVGRenderer().renderPng(drillDoc, 1024);

// Realistic top/bottom views to PNG (dimension-clamped for bounded memory)
MultiLayerSVGRenderer renderer = new MultiLayerSVGRenderer();
byte[] topPng = renderer.renderRealisticSidePng(layers, MultiLayerSVGRenderer.Side.TOP, 1024);

// One image with the realistic board plus all off-board annotations
// (drill charts, stackup tables, fab notes) composited around it
byte[] overviewPng = renderer.renderBoardOverviewPng(layers, MultiLayerSVGRenderer.Side.TOP, 1024);

Files.write(Path.of("board-top.png"), topPng);

When you need to map pixels back to real-world coordinates, renderRealisticSidePngWithScale returns a PngWithScale carrying the px↔mm scale, the mm rectangle the image covers, and the datum origin — the same geometry is also embedded in the PNG via pHYs + tEXt chunks.

MultiLayerSVGRenderer.PngWithScale r =
    renderer.renderRealisticSidePngWithScale(layers, MultiLayerSVGRenderer.Side.TOP, 1024, 0, false);
double pxPerMm = r.pxPerMm;   // e.g. overlay a 10 mm grid behind the board
Files.write(Path.of("board-top.png"), r.png);

Aperture Visual Test

The library includes a comprehensive visual test catalog with 127 test cases covering all aperture types, macros, regions, polarity, transforms, and legacy format support.

View Aperture Visual Test

Project Structure

• src/main/java/com/deltaproto/deltagerber/parser — Gerber and Excellon parsers
• src/main/java/com/deltaproto/deltagerber/lexer — Tokenizer for Gerber files
• src/main/java/com/deltaproto/deltagerber/model — Data model for Gerber/drill documents
• src/main/java/com/deltaproto/deltagerber/renderer/svg — SVG rendering engine
• src/main/java/com/deltaproto/deltagerber/web — Web viewer server
• src/main/resources/web — Web viewer HTML/CSS/JS
• testdata — Sample Gerber projects for testing

License

MIT