SoloTrace

WORK IN PROGRESS: MANY FEATURES MAY BE BROKEN · version 0.10.1-wip · source-available, non-commercial

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.

Open SoloTrace in your browser: nothing to install, nothing uploaded (the editor's Python runs inside the page). Or download it and double-click a launcher (below).

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

Quick tour: your first board in 5 minutes

1. File > Open example > 555 LED flasher (or File > New board and set a size).
2. 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). R or Shift + click turns the part, Esc stops placing. Star parts you use a lot with the button under the preview.
3. Wire: press W, click one pin, then another (or drag from pin to pin). A green circle snaps onto the pin the click would hit (the lock reaches about 14 screen pixels beyond the pad edge, never less than 1.4 mm or more than 3 mm on the board), so you do not have to line the cursor up exactly. 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).
4. 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.
5. 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...).
6. Tweak: drag a trace section sideways to move it, use Trim (X) to cut a section out, and right-click anything for its menu.
7. Check, then Export.

Quick and dirty RF (Manhattan / deadbug): File > Open example > Manhattan RF amplifier (copper islands). Press I and click to drop copper islands, sit the parts' pins on them, and tick Board > Ground fill. No traces needed.

Resizing the panels (new in 0.10.1)

The parts panel and the selection panel can be dragged wider or narrower with the grey handle beside them, and the web UI also has a handle between the parts list and its preview (drag it down to give the list more room, up to read a long description). Double-click a handle to put it back.

Antennas and the coil generator (new in 0.10.0)

Antennas. In the parts list, Board bits > Antennas and keep-outs holds a meander antenna for each of 315, 433.92, 868, 915 and 2450 MHz, a matching wire whip (cut a wire of the length in its name) and five bare keep-out boxes. Place the antenna at the edge of the board, wire pin 1 to the radio's RF pin (through any matching parts) and pins 2 and 3 to ground, and keep the orange hatched box free: copper, ground fill and the back-side plane are all kept out of it, the autorouter goes round it and Check reports anything inside it. Open File > Open example > 433 MHz meander antenna to see one.

These are starting points, not tested designs. The copper length is the quarter wave on FR4 by a rule of thumb plus 10 % to trim: measure with a NanoVNA and scratch copper away from the tip (silk ticks every 2 mm; the longer tick is the formula length). A real antenna usually also needs a small matching network, which SoloTrace does not provide. Notes, sources and what was left out: docs/research/pcb-antennas.md.

Coil generator. The PCB coil generator... button under the parts list (also in the Parts menu). Type the outer width and height, then pick one mode:

1. Area + inductance: say how many uH you want and it finds the number of turns and the track spacing that come closest.
2. Area + turns: say how many turns and it works out the inductance, spreading the turns over the area.

Calculate shows the turns, gap, track length, estimated inductance, DC resistance and (if you gave a frequency) the parallel capacitor that would tune it. Save coil and place stores it under My parts and arms it for placing. On a one-sided board the inner end of the coil cannot come out without crossing the turns, so solder an insulated wire from pin 2 to pin 3 of the part; SoloTrace treats those two pins as already joined. Wire your circuit to pins 1 and 3. Open File > Open example > PCB coil from the generator to see one.

The inductance is an estimate for a coil in air; a ground fill or plane, ferrite or metal nearby changes it, so measure the real coil. Method and cross-check: docs/research/pcb-antennas.md. From a terminal: python3 src/main.py coil --width 30 --height 20 --uh 1.5 --freq 13.56 (or --turns 8; add --save to put the part under My parts).

Breakout boards (new in 0.9.0)

File > Open example now has three breakouts for the "postage stamp" ESP32 boards: XIAO ESP32-S3 / C3 (one board serves both, same footprint), ESP32-C3 SuperMini and ESP32-S3-Zero. Each is generated by the app from the module's own pad table, routed by the autorouter (no jumpers) and checked (no DRC problems).

• Every module pin has a hole strip: one bar of copper with four holes, touching the module's pad. Pick any hole for a pin header, a jumper wire or a component lead, or solder a wire or an SMD part flat on the bar (deadbug). With the module's own pad that is four extra connections per GPIO, all the same net.
• Three power rails of six holes each: 3V3, GND and 5V.
• Power in on a 2-pin screw terminal and on a 2-pin header, both on 5V (pin 1) and GND (pin 2). Fit one.
• No copper under the module, because many of these modules have pads on the back.
• Sizes: 52 x 30 mm (XIAO), 52 x 31.5 mm (SuperMini), 52 x 32.5 mm (S3-Zero).

The green circle while wiring (here from a module pin towards the 3V3 rail; the cursor was a little off the hole):

Build your own: Board bits > Hole strips (breakout) has strips of 2 to 16 holes. A strip is always through-hole and flat copper (the Pads of this part choice does not apply), is one net, and is not in the BOM. The "with lead-in" strip (BRK_STRIP4_LEAD) starts 0.3 mm past a module pad so that the two touch and need no wire. Details and the open points: docs/research/breakout-boards.md.

Check before you power one: nothing here has been built. The 5V pad of the XIAO is called VBUS in Seeed's symbol; whether it is safe to feed it from the screw terminal while USB is plugged in was not looked up. Read your module's documentation first.

Feature by feature

Library and parts. 90 through-hole parts plus 11 hole strips, 23 modules and 41 SMD parts, sorted by shape (form factor) rather than by maker code. Each group has an arrow that opens its sub-types:

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. Once routed, the trunk is drawn in the same copper colour as everything else, so joints look like the one piece of copper they will be, with a thin dashed orange line down its middle to show it is a rigid wire. Branches stop inside the trunk instead of poking out of its far side, and when you drag a trunk sideways the branches joined to it move with it and stay joined. The net panel lists the rigid pairs, each with a make normal button.

Copper islands (Island tool, I). Free-standing pads for Manhattan / deadbug building. Click on the board to drop one (5.08 mm square to start), or drag to draw one any size; Shift + click switches new islands between rectangular and round. With Select, drag an island to move it (0.635 mm steps, so it can sit under pins) and drag one of its white corner squares to resize it while the opposite corner stays put. The right panel takes an exact width, height and corner cut (rectangles get 45 degree corners like everything else; a round island with a different width and height is an oval), offers square/circle sizes from 2.54 to 15.24 mm, and has Turn 90, Duplicate (Ctrl+D) and Delete; arrow keys nudge it. Right-click an island for the same choices, or right-click empty board > Add a copper island here. An island hidden under a part's body: click the part, then click it again to pick the island.

An island has no net of its own: it joins the net of whatever touches it, a pin, a trace or a jumper pad, and islands that touch each other share a net. So sit a part's pins on islands (deadbug pads make that easy) and the connection is made, with no trace. The panel says which net an island is on and which pins sit on it. If pins of two different nets end up on one island, that is a short and Check reports it. The router treats islands as copper and routes round them, and they appear in every export.

Ground fill (Board > Ground fill). For quick and dirty RF and fast analogue: the whole board becomes copper, used as ground, and every other net is cut free from it with a gap. Settings are under Board > Ground fill settings...:

• Ground net: guessed (a net called GND, 0V, VSS, ground... otherwise the net with the most pins), or pick one; the net panel also has Use this net as the ground fill. The ground net is joined by the fill, so Auto-route does not route it, and its old automatic traces are removed when you turn the fill on.
• Gap round everything else (default 0.6 mm, never less than the board's copper-to-copper gap). For laser etching keep it at least 3 to 4 line intervals.
• Fatten other nets' copper by up to this much (default 1 mm): routed traces and pads grow into wide, low-inductance patches, but only where that keeps the gap from other nets, ground copper and the board edge. Copper islands you placed keep their size.
• Remove floating fill (on by default): a piece of fill that no ground pin sits on, boxed in by other nets, is cut away rather than left as floating copper. A ground pin that sits on a piece of fill cut off from the rest gets a yellow rubber band; join it with a trace or a jumper.
• Turning the fill on offers to make every pad a deadbug pad, since such boards are usually built with the parts soldered straight onto the copper.

The fill is drawn in the editor and is in the Gerber, the PDF/SVG prints and the laser G-code. In negative laser mode the laser then burns only the gaps (much faster); isolation mode burns the same thing on such a board.

Thermal reliefs (ground contact). A pad joined solidly to a big copper fill is hard to solder: the fill takes the heat away faster than a hobby iron supplies it. So every ground pad gets a ring of bare board bridged by spokes (a thermal relief), in the ground fill and in the back-side plane. Board > Ground fill settings > Ground contact sets the number of spokes (default 4), their width (default 0.8 mm) and the ring (0.5 mm), and shows the current the spokes carry together (IPC-2221 outer-layer formula, 1 oz copper, 10 °C rise: four 0.8 mm spokes are good for about 8 A). Ground usually carries the return current of the whole board, so there is also "size spokes for N amps": type the current and the spoke width is worked out for you. Round pads get radial spokes at 45°; deadbug ovals, rectangular pads and copper islands get spokes off their flat sides and ends (never a corner); islands over 4 mm get spokes scaled to their size. In a part's panel, Ground contact can be set to heavy (spokes twice as wide) or solid (no relief: for the heavy-current pads and for decoupling capacitors and RF grounds, where the industry rule is a direct connection). Check warns when the ground net's trace class is good for more current than its reliefs carry. A spoke that would touch another net is dropped, and a pad that would lose all its spokes stays solid, so a relief never cuts a pad off. Research and sources: docs/research/thermal-reliefs.md.

Back-side ground plane (double-clad board). Board > Back-side ground plane uses the component side of a double-sided copper-clad board as one solid ground plane while all traces stay on the copper side as usual. Every ground lead that passes through the board is soldered on both sides; a via (Via tool, V; a hole with a bit of bare wire through it, soldered both sides) joins deadbug or SMD ground pins, ground islands and the ground fill to the plane; every other hole gets a bare ring in the plane (default hole + 1.1 mm: 0.25 mm of electrical clearance plus 0.3 mm for front-to-back misalignment). The dialog has Via at every ground pin without a hole and Add stitching vias (a grid, default 10 mm), and says up to what frequency that spacing keeps the plane and the front ground one low-impedance mesh (lambda/20 in FR4: 10 mm is good to about 700 MHz).

The "big LC circuit" worry: two copper sheets joined at one point do form a resonant cavity, but on a 100 mm FR4 board its first resonance is near 700 MHz, far above most hobby circuits, and joining the sheets at every ground pin plus a loose grid of vias turns the cavity into a mesh, which is exactly how commercial multilayer boards are built. What you gain even at audio and low MHz: every trace has its return path directly underneath, so loops, crosstalk and radiated noise shrink. Sources and the numbers: docs/research/back-side-ground-plane.md.

Two ways to make the back: (1) etch or burn it: Export > Gerber gains a top-copper layer, Export > Back-side ground plane gives a 1:1 PDF/SVG (seen from the component side, so not mirrored), and the laser dialog has a Back-side ground plane choice (burns only the rings and reliefs); front-to-back registration must then be within the ring allowance. (2) Leave it solid, the ham way: drill every hole, then clear the copper round each non-ground hole with a 2 to 2.5 mm drill tip or countersink; Export > Countersink list lists those holes, and nothing needs aligning. Ground leads and vias get thermal reliefs in the plane (same spoke settings) so they can be soldered. Check reports a via whose back-side connection a clearance ring would cut, a ground lead trapped inside another hole's ring, a plane nothing joins, and a note on how far the stitching is good for.

SMD parts. The big SMD parts button under the parts search (with the little SOT-23 picture) swaps the whole list for the SMD parts; it then reads Through-hole parts (with a TO-92 picture) and clicking it again brings the normal list back. The SMD list holds the common, large, hand-solderable surface-mount packages (chips 0603 to 2512; SMA, SMB, SMC, SOD-123, MELF diodes; SOT-23 with 3, 5 and 6 pins; SOT-223; DPAK and D2PAK; SOIC-8/14/16 narrow, SOIC-16 to 28 wide, SOP-8 5.3 mm; tantalum cases A to D; SMD electrolytics 4 to 10 mm; two shielded inductors). Every pad size is taken from a maker's land-pattern drawing (TI, Diodes Inc, Vishay, KEMET, Nichicon, Sumida), using the roomier wave-solder or "level A" pattern where there was a choice, and every gap between pads is at least 0.3 mm, so the parts can be soldered without a solder mask; finer packages (SOT-363, TSSOP, TQFP) are left out on purpose. SMD parts sit on the copper side: in the component-side view they appear mirrored, press M to see the board as you will solder it; their outlines go to a bottom silkscreen Gerber and they have no holes. Pin-label presets cover SOT-23 transistors and MOSFETs, SOT-223 and DPAK regulators and transistors, and the SOIC equivalents of the DIP layouts. SoloTrace stays a through-hole program first: it starts in through-hole mode and remembers which list you had open. Where the numbers came from, and what was left out and why: docs/research/smd-land-patterns.md.

Modules & displays. A new group in the through-hole list holds the boards people actually build with, each on 2.54 mm headers with every pin already labelled as it is printed on the module:

Every board works both ways: through-hole (solder header pins and plug the module in, or solder it straight down), or deadbug (Pads of this part > Deadbug): no holes, longer pads, so a castellated "postage stamp" board (XIAO, SuperMini, Zero, Pico) can be soldered flat onto the copper, or header pins bent flat. Each part's note gives the GPIO number behind every pin name and says where the data came from; where the sources were thin or disagreed (the SuperMini's exact position along the board, the ESP32-S3-Zero and RP2040-Zero outlines, the DOIT board outline, the SPI OLED's header position, the SD modules' pin order), the note says so. Some sellers swap VCC and GND on the OLEDs: Pin labels has VCC GND SCL SDA for those. Always check the print on your module before etching. The research, with a source and a confidence word for every number: docs/research/mcu-modules.md.

Moving a part after routing. Traces do not follow a part. When you drag a part over laid copper, every pad and trace it would touch is ringed in red as you move (in the browser the ghost turns red), and when you let go the status bar says how many collisions there are: drag it clear, or right-click it > Route this part's nets. The same happens when you turn, nudge, mirror, duplicate or place a part. Check also warns when a module mounted under the board and soldered flat would sit on another net's trace.

Mirrored parts (under the board). Shift+M (or right-click > Mirrored, or the tick box in the part's panel) mounts a part on the other side: a display that should look out of the copper side, a module plugged in from below so the board sits flat in a box. Its pins swap left to right in the component-side view (the part flips about its pin 1), its outline moves to the bottom silkscreen, the BOM says copper side (MIRRORED), and Check lists it as a reminder. While placing, Shift+M places the next part mirrored. A mirrored part is drawn so it can't be missed: a thick dashed pink frame, a pink MIRRORED (under board) band, pink outline, and a pink note in the panel. (SMD parts already live on the copper side, so they are only shown pink if you mirror one onto the component side.) Example: File > Examples > XIAO ESP32-C3 logger, with its OLED mirrored under the board.

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:

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, Shift+M mirrors it (mounts it under the board). 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. Board > Auto-place algorithm also offers Routability (experimental): the same moves plus an estimate of where copper will not fit (RUDY congestion) and a penalty for pads boxed in by other parts, with VPR's adaptive cooling. In measurements it was no better than Annealing (DESIGN_NOTES.md), so Annealing stays the default.

Auto-route. A grid router that remembers its heading, so it prefers straight runs and clean 45° bends instead of staircases, and prefers not to run under part bodies. Three ways to drive it (Board > Auto-route algorithm):

• Auto (default): negotiated congestion first; if that leaves a connection unrouted or needs a jumper, the classic tries follow within the time budget, and the best result is kept.
• Negotiated congestion: the PathFinder method FPGA tools use. Every net is routed at once, overlaps allowed; then the price of every contested cell rises pass after pass (and a history cost remembers where fights happened) until the nets have sorted themselves out, usually in 3 to 15 passes. A jumper is just another priced resource, dear until contested copper is dearer. It does not depend on the net order, so it needs no retries. On eleven test boards: everything routed, the same number of jumpers as classic, 7 to 9 % less copper, about two-thirds of the time.
• Classic: one net at a time against hard obstacles, wide nets first; a blocked net tears up the nets in the way and retries; a jumper is the last resort (unless Jumpers is unticked in the tool bar or for that net). The job is tried with up to six net orders (about 12 seconds at most, plus the try in progress) and the best result is kept.

After the best try is chosen, a polish step routes each net once more against the finished board and keeps the new copper only if it has fewer jumpers or is shorter, so it never makes a board worse. The same board always routes the same way (before 0.8.0 it could differ from run to run). How it compares with the first versions: DESIGN_NOTES.md (fewer jumpers than 0.3.4 on the test boards, the same total copper; sometimes a longer path where it saves a jumper).

Traces you drew by hand are kept by all three. 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).

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.

1. Finish the board and run DRC. Open Export > Laser G-code (Elegoo Phecda)...
2. 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 gap mm 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).
3. 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).
4. 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).
5. 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.
6. Controller assumptions: GRBL-style, $30 equal 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 eleven boards (the 555 flasher, 5 V regulator, 555 power oscillator, logic mix, RF oscillator with ground fill, Manhattan RF amplifier, SMD regulator, a XIAO ESP32-C3 logger with its OLED mirrored under the board, the 555 flasher with ground fill and back-side plane, a 433.92 MHz meander antenna board, and a 1.5 uH coil from the generator), each with its .solotrace file, Gerber zip, 1:1 copper-side SVG and PDF, BOM and laser G-code in both modes; the back-plane one also has the back-plane PDF/SVG, its laser job and the countersink list. Plus test cards.

More

• HOW_IT_WORKS.md: what it reads and writes, the coordinates, the router and the laser engine in plain English
• docs/research/breakout-boards.md: the breakout boards and hole strips
• DESIGN_NOTES.md: decisions, rejected ideas, measurements, what is untested
• docs/research/: the original research and plan, the Phecda notes, and the 0.5.0 notes on autorouters, thermal reliefs, the back-side ground plane and SMD land patterns
• 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