TraceForge

Signal paths, trace cleanup, via stitching, RF fencing, BGA fanout and live net colors for KiCad 10 on Windows.

TraceForge 0.12.1 groups signal analysis, Via Tools, BGA fanout, Trace Tools, and Visualization in one colored panel. Trace Tools includes cleanup, teardrops, and rounded corners with persistent restore. It reads the open board through KiCad's native pcbnew bindings, including unsaved routing changes. No official IPC API setup, API token, or pip runtime dependencies are needed.

Current TraceForge in PCB Editor on the 03-MANAGEMENT-SWITCH-BOARD project. The selected signal path is highlighted on the board.

Install

Requirements: Windows and KiCad 10 with its bundled Python/scripting support.

KiCad Plugin and Content Manager

Download TraceForge-<version>-KiCad10-PCM.zip from a GitHub release. In KiCad Manager, open Plugin and Content Manager > Install from file, select that ZIP, then close all KiCad windows and reopen PCB Editor. Once KiCad accepts TraceForge into its official catalog, you can instead install or update it directly from the Manager's Repository tab.

The first launch may assign KiCad's unused Ctrl+Alt+Shift+F12 shortcut for native net focus. If TraceForge asks, restart PCB Editor once more. An existing user.hotkeys file is backed up as user.hotkeys.traceforge.bak; shortcut conflicts are reported without changing the existing binding. PCM installation does not require PowerShell or a manually created plugin junction.

Standalone Windows ZIP

1. Download the TraceForge KiCad10 Windows ZIP from this repository's Releases page. Extract it completely into a permanent folder, for example C:\Tools\TraceForge. Do not run the plugin from inside the ZIP.

2. Save your work and close all KiCad windows, including KiCad Manager.

3. Open the extracted folder, right-click inside it and choose Open in Terminal. In PowerShell run:

   powershell.exe -NoProfile -ExecutionPolicy Bypass -File .\tools\install_native_bridge.ps1

   This applies the script policy to that process only. Administrator access is normally unnecessary. The installer creates a junction at %APPDATA%\kicad\10.0\scripting\plugins\traceforge_native_bridge pointing to the extracted native_bridge folder. Keep the extracted files there.

4. Start PCB Editor, open and save a board, then click the TraceForge toolbar icon or Tools > External Plugins > TraceForge.

5. Open a feature tab. Use F5 or Refresh to read the open board on demand.

Cloning this repository into a permanent folder and running the same installer also works. No separate Python installation is needed to use the plugin.

Update or remove a standalone installation

Close PCB Editor and extract the new version. If its folder differs from the old installation, run the installer from the new folder with:

powershell.exe -NoProfile -ExecutionPolicy Bypass -File .\tools\install_native_bridge.ps1 -ReplaceExisting

This switches the plugin junction and preserves the previous installation folder. The installer refuses to replace an ordinary folder. Restart PCB Editor afterward. For a Git checkout already linked by the installer, pull updates, rerun the installer with all KiCad windows closed, and restart PCB Editor.

To uninstall, close PCB Editor and remove only the junction at the plugin path above; keep your board files and TraceForge sidecars. Removing the installation folder while the junction exists leaves a broken plugin link.

Choose a tool

Tab	Workflow
Signals / xSignals	Detect paths through series passives, inspect chain length/timing, highlight differential pairs, export CSV and write reviewed DRC targets.
Via Tools	Use the selector at the top right to switch between Via Stitching, Via Fencing, and Via Array. Stitching previews symmetric or staggered grids and manages placed sets. Fencing follows an RF trace on either or both sides. Array evens out selected existing vias.
BGA Fanout	Analyze a selected BGA, check geometric fit, and preview dogbone, via-in-pad, or bounded escape-to-edge routes.
Trace Tools	Use the selector at the top right for Trace Cleanup, Teardrops, or Round Corners. Cleanup previews redundant copper and dangling ends, supports bulk selection, and removes reviewed tracks with Undo. Teardrops use KiCad's native generator. Round Corners previews a selected radius across all copper layers, rounds eligible existing trace junctions, and restores selected generated corners.
Visualization	Color net groups and individual nets live, and focus the ratsnest on selected components.

Via Array

Select 1–64 vias of the same net, size, drill and layer pair in PCB Editor. Open Via Tools, choose Via Array in the selector at the top right, then click Read & preview selection. Auto detect fits the existing row and column layout by finding the arrangement requiring the least movement. The two diagrams show current positions and the proposed array. To override the detected shape, choose Rows or Columns, enter a fixed count starting at 1, and click Preview array. TraceForge calculates the other dimension and center-to-center X/Y pitch from the selected via centers' bounding rectangle. A partial final row or column is centered. It assigns each via to a target that minimizes total movement; no vias are added.

The preview lists old and new centers. Apply is available only when the array stays inside the board, passes copper and via spacing checks, and keeps existing same-net copper contact on connected layers. Apply only moves the vias; it does not refill zones. Press B in PCB Editor whenever you want to update zone fills. Undo restores the original positions. This tool rearranges existing vias; Via Stitching creates managed new vias.

Visualization

The Visualization tab assigns a single color to each group of nets. Enter exact net names, comma-separated glob patterns such as DDR_DQ*, or a KiCad net class as class:DDR_BYTE0. Groups must be disjoint. Individual net colors are available for nets outside groups, such as separate voltage rails. TraceForge rejects conflicting assignments and stores group definitions in <board>.traceforge-visual.json; the applied colors are saved in KiCad's project file. Applying a color switches KiCad's net-color display to All, which colors pads, traces, vias, and copper zones. Reset all net colors to defaults clears every net color assignment on the open PCB and removes TraceForge's saved group and individual color definitions.

The separate Ratsnest visibility section offers Show all, Hide all, and Add PCB selection. Select a footprint or one of its pads in PCB Editor, then click Add PCB selection. The first click isolates that component's nets; later clicks add nets without hiding previously focused components. The focus list lets you remove a component while retaining nets shared with others. Show all and Add PCB selection also turn KiCad's global ratsnest display on if it was set to None. The first focus action filters the board; later additions update only newly included nets. A fully routed board has no ratsnest lines to show. These controls affect visibility only; they do not change connectivity. To edit teardrops, open Trace Tools, choose Teardrops, set the options, then click Apply to PCB. KiCad generates the teardrops as an undoable editor operation.

Signals and path detection

The screenshot above shows the current Signals / xSignals tab on the management switch board, including chain timing, pair status, and the PCB highlight.

Select two pads, vias, tracks or components, then use Detect path between 2 selected PCB items. Alternatively choose Pick first, then second and click each endpoint in PCB Editor. The Chain Editor supports the same guided workflow.

The detector crosses series resistors and enabled AC-coupling capacitors across different net names. Review crossed parts, inferred differential partners and any existing-chain matches before saving. A resistor limit is optional. Component selections with multiple candidate signals offer a path choice.

Click a chain to highlight and zoom to it. Highlights stay visible during panning and zooming; changing the native selection or pressing Esc clears them. Green, amber, red, blue and gray states distinguish matched, warning, error, routed and pending results. Signals refresh preserves scrolling and expanded groups.

Selecting a path automatically keeps the chain's nets bright while KiCad dims unrelated copper. This also applies to endpoint detection and both differential legs. Other branches belonging to those same nets remain bright. Clear, Esc or a changed native selection releases the effect; panning/zooming keeps it.

For a PCM installation, TraceForge assigns Ctrl+Alt+Shift+F12 to KiCad's Highlight Net (selected nets) action on first launch if the action is unassigned and that shortcut is unused. Restart PCB Editor when prompted. For a standalone installation, rerun the installer with all KiCad windows closed. Existing custom bindings are preserved; a changed hotkey file is backed up as user.hotkeys.traceforge.bak. A conflict is reported instead of overwritten. The native Clear Net Highlighting action also needs its shortcut enabled. TraceForge sends these actions directly to KiCad's visible canvas, without global keyboard input or a polling loop. Net focus is automatic; no checkbox is needed.

See endpoint detection for details. Saved chain timing sums whole-net copper, including branches; the endpoint preview follows one routed path. Neither is an exact reproduction of KiCad's point-to-point tuner. Timing requires validated project propagation profiles and stackup data. Review driver orientation and limits before writing DRC targets.

Via stitching

This capture precedes Preview; no stitching vias were added to the project. The 0.11.5 release has a condensed basic form.

Choose the net, via preset/netclass/custom size, and center-to-center X/Y spacing. Choose the whole board, a PCB zone/drawing, or draw a rectangle/polygon in the tab's overview, then Preview and Apply stitching. Accepted locations are green; rejected locations are amber. Symmetric is the default placement pattern; staggered/perimeter patterns, copper-contact rules, grid offsets and setbacks are under Advanced options. Whole-board grids are evaluated without a fixed 5,000-location limit; dense boards can take longer to preview and apply. The About tab and window title show the version currently running; About also shows the loaded code path and log location when checking an installation.

Select, edit/regenerate or remove tool-created sets from the list. Changes support KiCad Undo/Redo. Read stitching usage and checks.

Via fencing

Current fencing controls over the management board before a signal trace is chosen. No fence was applied to the project.

Type the Signal net to fence or use Pick signal net in PCB. For a specific section, select connected track segments/arcs and click Use selected trace. Type or pick the separate fence net, normally GND. Choose Both sides, Left or Right, copper-to-via gap, spacing and via dimensions, then Preview and Apply.

The RF spacing helper estimates wavelength/10 or wavelength/20 spacing from frequency and dielectric data. It does not calculate impedance or choose the lateral copper gap. Inspect the reported largest gap after skipped locations. See RF fencing.

BGA fanout

Live PCB Editor preview on a disposable 4 by 4 BGA test board: 16 pads escaped to the field edge. The management board has no BGA footprint.

Apply added 16 vias and 32 track segments. KiCad Undo removed them, Redo restored them, and Remove generated fanout returned the test board to zero tracks and vias. The removal itself also passed Undo and Redo.

Select a BGA footprint and open BGA Fanout. Review the detected local pitch, fabrication limits, offsets and filters. Rectangular arrays may have different spacing in different rows and columns, including an outer ring and inner array. Zero X/Y offset uses that pad's adjacent gap, with a short-stub cap across large empty spans. Fit guidance explains board-rule floors and nominal inter-ball space; Suggest settings evaluates candidates without placing them. Choose Dogbone, Via-in-pad, or Auto escape to BGA edge. The escape preview shows which selected single-ended pads have a connected route past the pad field and which are blocked. Apply only reviewed routes. Managed removal preserves edited routing.

Through vias are supported. Via-in-pad requires explicit fabrication confirmation. Escape endpoints still need onward routing to their destination. Microvias, HDI layer assignment, differential-pair escape and full-board autorouting are not implemented. See BGA fanout.

Trace Tools

The real management board reports all six enabled copper layers and track counts before Scan / Preview. Opening Cleanup does not start the full scan or change copper.

Scan the whole board or an exact net to find duplicate tracks, overlapping collinear tracks and native dangling endpoints. Filter findings by copper layer; partially overlapping same-net segments can be fused into one continuous track. Every enabled copper layer appears in the summary, including hidden and empty layers; counts show findings and scanned track objects per layer. Preview rows highlight in PCB Editor. Redundant copper starts checked; dangling tracks require review and start unchecked. Select all and Unselect all affect the shown layer's findings. Cleanup is undoable. Recheck length matching returns to Signals and refreshes the measurements. Partial overlaps, vias, locked and grouped copper are preserved. See trace cleanup.

Choose Teardrops in the Trace Tools selector. Choose Add or Remove, the whole board or selected PCB items, and via, PTH, or SMD targets. For Add, set curved or straight edges, best length and width percentages, and optional maximums. Illustrations beside each target show where the teardrop appears; d is the pad/via minor size, L is the teardrop length, and W is its width. Click Apply to PCB to use KiCad's native teardrop generator and Undo. KiCad 10 uses one specified size rule for pad and via targets. Track-to-track teardrops use Board Setup defaults and must be applied separately. Selected-only scope does not support track-to-track teardrops. Use Open advanced KiCad dialog for additional KiCad filters. Run KiCad DRC after applying.

Choose Round Corners to enter a maximum radius in millimeters. By default, TraceForge fits a smaller radius where the full value cannot clear adjacent copper or fit a short segment; uncheck the fit option to require an exact radius. Use the optional exact-net field to inspect one net. Preview corners checks all copper layers of the open PCB, or only the selected tracks. It counts eligible corners, fitted smaller bends, and reasons for skipped junctions. Round eligible corners replaces qualifying straight corners with tangent copper arcs in one undoable KiCad edit. Branches, pads, vias, existing arcs, locked copper, and corners that cannot fit the radius are left alone. Select a generated arc or its adjacent track and click Restore selected rounded corner(s) to recover the original straight corner. Restore all rounded corners resets every TraceForge fillet on the open board, including differential-pair traces. Both work after reopening the saved board. Keep the fillet sidecar with the PCB. Recheck length matching and run KiCad DRC after rounding; the preview is conservative but does not replace the full DRC, including zones and custom rules. KiCad's shove router cannot drag copper arcs.

Keep project metadata

Save the PCB normally and keep these sidecars alongside it when copying a project:

File	Stores
<board>.traceforge.json	Signal-chain definitions and reviewed limits
<board>.traceforge-stitching.json	Stitching/fencing recipes and owned via UUIDs
<board>.traceforge-fanout.json	Generated fanout ownership and recipes
<board>.traceforge-fillets.json	Original corner geometry and generated arc ownership for selective restore

Removal/regeneration preserves locked or manually altered generated items. Missing ownership sidecars prevent managed removal. Legacy xsignals.json can be imported.

Refresh, shortcuts and troubleshooting

Opening a tab or returning from PCB Editor checks for changes once and refreshes stale data. There is no continuous board/selection polling or automatic retry loop. F5 forces a refresh. All board operations share one worker; large previews and zone refills can briefly occupy KiCad's GUI thread.

Default shortcuts: Ctrl+Alt+H highlight chain, Ctrl+Alt+G highlight group, Ctrl+Alt+C clear, Ctrl+Alt+W write DRC targets, Ctrl+Alt+E export CSV, Ctrl+Alt+T show/hide. Configure them through Shortcuts.

• Plugin missing: confirm the installer succeeded and restart PCB Editor.
• Old panel after updating: close TraceForge and restart PCB Editor.
• Pick waiting: click one item in PCB Editor; Esc cancels. Picks expire after 90 seconds.
• No path: check that routing is continuous and passive traversal is enabled.
• No via candidates: refill zones, check fence/stitch net copper on two layers, and review the preview's clearance/keepout rejection reasons.
• Multiple boards open: launch TraceForge from the intended editor's toolbar.
• Logs: %APPDATA%\TraceForge\traceforge.log.

Scope and development

Run KiCad DRC after generated placement; custom-rule and RF validation are incomplete. Live parallel multirouting is planned, not implemented. This release targets KiCad 10 on Windows and uses its legacy pcbnew bindings; KiCad 11 is not supported. See feature scope and native access.

Development checks:

python -m pip install -e ".[dev]"
python -m ruff check .
python -m compileall -q signal_path_analyzer native_bridge tools
python tools/build_release.py

The build writes a standalone ZIP and SHA256SUMS.txt under dist/, using an explicit public-file allowlist. Tests, fixtures, logs, caches, credentials and user boards are ignored. tools/build_chains.py is an optional offline chain builder; tools/make_icons.py regenerates icons with Pillow installed.

See PCM publishing steps, release notes, changelog and MIT license.