An easy PCB designer for single-sided, through-hole, quick-prototype boards. A small library of real full-size parts, traces up to 10 mm wide set with a slider, every corner chamfered (no pure 90° traces), an autorouter that avoids the "tangled string" look, and output for printing (toner transfer), Gerber fabs and a gantry diode laser (Elegoo Phecda) with a negative option and adjustable trace gap.
Screenshots are of the real program running on a Linux test machine with the built-in example boards.
Licence and no warranty. Copyright Matthew Armstrong. Licensed under the PolyForm Noncommercial License 1.0.0: free to use, change and share for non-commercial purposes; commercial use needs separate permission. It is source-available, not open source. GitHub shows the licence as "Other". This is not legal advice. The software is provided as is, with no warranty and no liability. Third-party parts keep their own licences (THIRD_PARTY.md).
Safety. Etching chemicals burn skin and eyes. A diode laser can blind you and start fires, and paint, resist and etchant fumes are harmful: wear laser safety glasses rated for your module, ventilate, never leave a running laser alone. The laser G-code has never been run on a real machine. Check every print against your real parts before etching.
What exists and what does not
| Area | Status |
|---|---|
| Place, wire, trace, trim and jumper tools, undo/redo, pan/zoom, flip view | Works in tests and the screenshots; lightly tested by hand |
| Right-click menus (trim, split, tidy, width, rotate, duplicate, wire from a pin, route one net...) | Works in tests and the screenshots |
| Rigid wires (Shift + Wire): a direct power trunk that the rest of the net branches off | Works in tests and on the demo; first suggested from real use |
| Auto-route retries (best of up to 6 net orders), jumpers optional globally or per net | Works on the test boards; slower (up to about 12 s plus one try) |
| Cut tool: one click removes a piece of trace from joint to joint (Shift: between two points) | Works in tests |
| Favourites & recently placed parts; Shift + click turns a part while placing | Works in tests |
| Branches stay joined when a trunk is widened or tidied; DRC warns about hanging trace ends | Works in tests and on rebuilds of real boards |
| Board > Keep traces out from under parts | Works on the test boards; can add jumpers on cramped boards |
| Pin labels (B C E, G D S, K A, IN GND OUT, optocoupler and DIP layouts) and part values on the board | Works; layouts are the common ones for each shape, check your datasheet |
| Dragging a trace section sideways (neighbours follow, 45° rules kept) | Works in tests; lightly tested by hand |
90 through-hole parts in a form-factor tree with a live preview, footprint wizard, KiCad .kicad_mod import |
Works; some parts excluded on purpose (see below) |
| Trace width slider 0.4–10 mm (segment, trace or net) + current readout + "fits up to" hint | Works |
| Wide traces leave pads straight and end on the pad centre (auto-tidy) | Works on the test boards; may leave a trace as it was when the tidy shape does not fit |
| Deadbug (surface-solder, no-drill) pads, per part or per pad | Works |
| Chamfered corners everywhere + DRC | Works |
| Auto-place and auto-route with jumper fallback | Works on the three demo boards and random test boards; pure Python, can be slow on big boards |
| Gerber + drill zip, 1:1 PDF/SVG, BOM CSV, netlist text | Written and re-read by an independent Gerber library in tests; not opened in a fab's own viewer |
| Laser G-code (negative / isolation / positive, test cards, frame file) | Geometry checked in tests; never run on a real Elegoo Phecda |
| Windows and macOS launchers, GitHub workflows | Not run (written but untested on those systems) |
| Floating slider pop-up beside the cursor | Not built: the slider is in the right-hand panel |
| Full PathFinder-style negotiated routing, topological router, C++ speed-up | Not built (see DESIGN_NOTES.md) |
| Soldermask and copper-pour layers, multi-layer boards, SMD | Out of scope |
Quick tour: your first board in 5 minutes
- File > Open example > 555 LED flasher (or File > New board and set a size).
-
Place parts: pick from Favourites & recent at the top of the parts panel, or open a group in the parts panel on the left (the little arrows show the sub-types, such as Resistors standing), pick a part, check the drawing under the list, then click on the board. Or type in the search box (
dip 8,to-220,standing).Ror Shift + click turns the part,Escstops placing. Star parts you use a lot with the button under the preview. -
Wire: press
W, click one pin, then another (or drag from pin to pin). A yellow rubber-band line shows the connection. Hold Shift for a rigid wire (see below). Click a rubber-band line to name its net or give it a class (Signal 0.8 mm, Power 2 mm, High current 5 mm; change them in Board > Board size and rules). - Auto-place, then Auto-route (toolbar). A progress bar with Cancel shows while it works. Routes use 0°, 45° and 90° moves, and a 90° turn is always built as two 45° turns (a chamfer). If a trace can't get through, a wire-link jumper (blue dashed) is added on the component side.
- Label: select a part and type its Value / type (NE555, BC547, 10k...), and pick its Pin labels (B C E, G D S, IN GND OUT...).
-
Tweak: drag a trace section sideways to move it, use Trim (
X) to cut a section out, and right-click anything for its menu. - Check, then Export.
Feature by feature
Library and parts. 90 parts, sorted by shape (form factor) rather than by maker code. Each group has an arrow that opens its sub-types:
| Group | Sub-types |
|---|---|
| Chips (DIP) | Narrow (7.62 mm rows) DIP-4 to DIP-28, wide (15.24 mm rows) DIP-28 and DIP-40 |
| Transistors & regulators | TO-92, TO-220 (2-pin, 3-pin, with heatsink outline), TO-247 / TO-3P |
| Resistors, diodes & inductors | Resistors lying flat (1/4 W to 5 W), resistors standing (1/4 W at 2.54 and 5.08 mm, 1/2 W and 1 W at 5.08 mm), diodes lying flat and standing, axial and radial inductors |
| Capacitors | Ceramic disc, film / box, electrolytic |
| LEDs | 3 mm and 5 mm |
| Pots, switches & crystals | Inline pots (2.54 and 5.08 mm), triangle trimmer, 6 mm tactile switch, HC-49 crystal |
| Connectors | Pin headers 1-row and 2-row, screw terminals, JST-XH |
| Board bits | Wire links, mounting holes, solder and surface pads |
| My parts | Parts you made or imported |
Click a part and a drawing of it (copper, holes, outline, pin numbers, pitch and drill) appears under the list, in the sidebar, with no pop-up. Names say what the part is ("Electrolytic cap, 5 mm pitch"), not an obscure model number. Left out on purpose because their sizes vary too much between makers: relay, USB-B, barrel jack, buzzer, fuse holder, panel pots with lugs, TO-126, bridge rectifiers. Make those with the wizard. Body outlines, the inductor, pot and trimmer layouts, and the standing-part pitches are generic: check them against your real part.
Your own parts. Parts > New footprint... opens the wizard: type a pad table (name, x, y, pad size, drill), or click on the canvas to drop pads, or start from a DIP or header preset, then save. Saved parts live in ~/.solotrace/parts (Parts > Open my parts folder). Parts > Import KiCad .kicad_mod... reads the text format of a KiCad footprint (through-hole pads and silkscreen lines only).
Trace width. Press T and click along the board to draw a trace (Enter, a double-click or Finish trace here on the right-click menu finishes it; corners are chamfered for you). To change a width, click a trace section on the drawing, or click a yellow rubber-band line to set the width of a whole net, then drag the slider in the right panel (0.4–10 mm; preset buttons 0.4, 0.8, 1.5, 2.5, 5, 10). Choose whether it applies to the section, the whole trace or the whole net. The panel shows roughly how many amps that width carries (IPC-2221 outer-layer formula; board settings give copper weight and temperature rise; a guide only) and how wide the trace can go where it is before it breaks the clearance rule.
Rigid wires (power trunks). A net with more than two pins is normally routed by joining the nearest pins first, so a ground net can end up as one long chain (transistor to capacitor to terminal). If you want a direct trace between two particular pins, hold Shift while wiring them (click or drag), or right-click a pin > Rigid wire from this pin, or right-click an existing rubber band > Make ... rigid. The router routes every rigid pair first, as its own pin-to-pin trace, then connects the rest of the net to the nearest point of that trunk, so a capacitor becomes a short branch. "Rigid" fixes which two pins are joined, not the path: the trunk bends round other parts like any trace, can be moved by a re-route, and you can drag or cut it. Rigid rubber bands are thicker and orange; the routed trunk is drawn in orange copper (it is ordinary copper in every export). The net panel lists the rigid pairs, each with a make normal button.
Values and pin labels. Select a part: Value / type at the top of the right panel takes anything (NE555, BC547, IRF540, 7805, 10k, 100uF 25V) and is shown next to the part name on the board; double-click a part to jump to it. Pin labels offers the common layouts for that shape, not specific part numbers:
| Shape | Layouts offered |
|---|---|
| TO-92 | E B C, C B E, B C E, D G S, G D S, S G D, small regulator OUT GND IN / IN GND OUT |
| TO-220 3-pin | power transistor B C E, MOSFET G D S, IGBT G C E, regulator IN GND OUT, adjustable regulator ADJ OUT IN, negative regulator GND IN OUT, triac MT1 MT2 G, dual diode A K A |
| TO-220 2-pin | diode K A / A K |
| TO-247 | G D S, G C E, B C E |
| DIP-4 / DIP-6 | optocoupler A K E C; optocoupler with base pin; opto-triac |
| DIP-8 | 555-style timer, dual op-amp, single op-amp, dual optocoupler |
| DIP-14 / 16 / 20 | logic GND and VCC pins; quad op-amp (DIP-14) |
| Pots, connectors | 1 W 3, CCW W CW; + -, - +, AC AC, IN OUT, V+ GND V-, IN GND OUT |
Or type your own in pin order, separated by spaces (. skips a pin). Diodes and LEDs show K A, electrolytics + -, without asking. Pin orders differ between makers, so always check the datasheet of the part you have. Labels are shown in the editor; they are not yet written into the Gerber silkscreen.
Wide traces are tidied. When a trace is 1.2 mm or wider, SoloTrace makes it leave each pad with a straight vertical or horizontal run (about the pad radius plus the trace width) before it turns, ends it exactly on the pad centre, and makes the chamfers bigger where there is room. This happens after auto-routing and, with Auto-tidy when the width changes ticked (the default), whenever you change a width. If the tidier shape would touch other copper the trace is left as it was, and the clearance problem is marked in red. Tidy (right panel or right-click) does it on demand; Edit > Tidy all traces does the whole board.
Cutting a piece out of a trace. Press C and click a trace: the piece under the mouse goes, from the joint before it to the joint after it (a pad, a place where another trace meets it, a jumper pad). The rest of the trace and of the net stays. While you hover, the piece that would go is shown in red. Right-clicking a trace only opens its menu; rest the mouse on Cut this piece to see the piece in red, and choose it to remove it. To cut between two points of your own choosing, Shift + click the first point and Shift + click the second (or right-click > Cut between two points); Esc cancels.
Moving, trimming and splitting traces. With Select, drag a trace section sideways: it moves parallel to itself and the sections either side stretch to follow at their own angle, so no 90° corner appears. Ends on pads stay put (a 45° link is added). Trim (X, or right-click > Trim this section) cuts one section out and leaves the rest as separate pieces; Split trace here breaks a trace in two without removing copper. A trace you have moved or trimmed counts as hand-drawn, so Auto-route keeps it. Ctrl+Z undoes any of this.
Right-click menus. Right-click (without dragging) on a trace, pin, part, rubber-band line, jumper or empty board for the actions that fit: widths, trim, split, tidy, highlight or re-route the net, rotate either way, duplicate, lock, pad styles, wire or trace from a pin, disconnect, delete, and Undo/Redo. Right-drag still pans.
Small helpers. Hover over copper to light up its whole net (the net name shows in the corner). Arrow keys nudge the selected part by 1.27 mm (Shift: 2.54 mm), Ctrl+D duplicates it, Shift+R turns it back. File > Open recent lists your last boards. While a board has unsaved changes it is saved every 2 minutes to ~/.solotrace/autosave.solotrace; File > Recover autosave opens it (the file is removed when you quit normally). Hover over a toolbar button for a hint. The status bar shows the cursor position in mm and a green all routed or orange N to route badge.
Pads: through-hole or deadbug. Pick Through-hole, Deadbug or Both in the toolbar for new parts, or change it for a placed part in the right panel, or for one pad ("This pad only"). Deadbug pads have no hole and are drawn as a long oval that sticks out from the part so you can bend the lead flat and solder it on the copper side. "Both" keeps the hole and the extra copper.
Auto-place. Simulated annealing that moves, rotates and swaps unlocked parts to shorten the ratsnest and cut crossings. Tick Lock on a part to keep it where it is.
Auto-route. A grid router that remembers its heading, so it prefers straight runs and clean 45° bends instead of staircases. Wide nets are routed first, and it prefers not to run under part bodies. If a net is blocked it tears up the nets in the way and retries; as a last resort it adds a jumper, unless you unticked Jumpers in the tool bar or for that net. The whole job is tried with up to six different net orders (about 12 seconds at most, plus the try in progress) and the best result is kept; it stops early when a try routes everything without jumpers. Traces you drew by hand are kept. Board > Remove automatic routes undoes only the automatic ones.
Jumpers. Press J to add one by hand. They are plain wire links on the component side, in 2.54 mm steps from 5.08 mm. They are listed in the DRC window.
View. M flips between the component side (how you place parts) and the copper side (how the etched board looks from below). Wheel zooms, right or middle drag pans, right-click opens the menu, F fits the board.
DRC. Check lists trace ends that are not joined to anything ("dangling"), copper too close to other copper or the board edge, parts sticking out of the board, traces thinner than the minimum, turns sharper than 45°, drilled pads with too little copper ring, jumpers that are the wrong length or cross each other, and pins that are not connected yet. Click a row to jump to it on the board.
Exports (Export menu).
| Output | Use |
|---|---|
| Gerber + drill (zip) | Copper (bottom), board edge, silkscreen, Excellon drill. Single layer; no soldermask layer |
| 1:1 PDF / SVG, mirrored | Toner transfer or photo-resist film: the copper side as you will see it. Always print at 100 % and measure a known distance before etching |
| 1:1 PDF, design view | Component-side print |
| Bill of materials (CSV) | Parts grouped by name and value |
| Netlist text | Round-trip text format for a quick board from a text editor |
| Laser G-code (Elegoo Phecda) | See below |
Laser etching with the Elegoo Phecda (gantry diode laser)
Read this first. A diode laser cannot remove bare copper. The method is: paint the copper, let the laser burn the paint away where copper must go, etch, then clean the paint off. Nobody has run these files on a Phecda yet. Treat every default as a starting guess and use the test cards.
- Finish the board and run DRC. Open Export > Laser G-code (Elegoo Phecda)...
-
Mode
- Negative (default): burns everything that is not copper, so paint is left only on the traces and pads. Slowest, cleanest.
-
Isolation: burns only a band of
gapmm around the copper. Fast; leftover paint between bands must be cleared by hand or by the etchant. - Positive: burns the copper shapes themselves (for a negative-working resist or marking).
-
Adjust (all live-previewed):
- Trace adjust (mm per side): positive grows the copper, negative thins it and widens every gap between traces. Use this to correct for the laser's spot size and your etch.
- Gap (isolation band width) and Border (keep paint at the board edge).
- Line interval (default 0.08 mm; the module's spot is about 0.06–0.13 mm depending on model), feed (default 1500 mm/min), power (default 70 % of S max), passes, crosshatch (second pass at 90°), bidirectional scanning, M4 dynamic power (default) or M3 with overscan, and drill dots (a tiny burn at every hole centre as a drilling guide).
- Click Save G-code.... Also use Frame file... (traces the board outline at 1 % power so you can line up the paint) and, on first use, Speed/power test... and Trace/gap test... (a grid of squares and a ladder of fine traces and gaps).
- In LaserGRBL or LightBurn: jog the laser to the lower-left corner of the board as seen from the copper side, set work zero there, open the file, check the preview, run the frame, then burn. The exporter mirrors X for you because the design view is the component side.
- Controller assumptions: GRBL-style,
$30equal to the S max in the dialog (default 1000) and$32=1(laser mode). The Elegoo manual names LaserGRBL and LightBurn but does not say "GRBL"; see docs/research/phecda-laser-notes.md.
Examples to look at without installing anything: examples/ has four boards, each with its .solotrace file, Gerber zip, 1:1 copper-side SVG and PDF, BOM and laser G-code in both modes, plus test cards.
More
- HOW_IT_WORKS.md: what it reads and writes, the coordinates, the router and the laser engine in plain English
- DESIGN_NOTES.md: decisions, rejected ideas, measurements, what is untested
- docs/research/: the original research and plan, and the Phecda notes
- CHANGELOG.md · CONTRIBUTING.md · SECURITY.md
Project page (after you enable GitHub Pages): https://The-Dorkknight.github.io/solotrace/
Source code: The-Dorkknight/solotrace on GitHub
Top comments (0)