Editor Overview
The PCB editor turns the schematic's connections into footprints and copper geometry. Start with a saved schematic, assigned footprints, and a reviewed Update PCB from Schematic.
Set the board outline, layer stack, net classes, and manufacturing rules before routing. Keep the native .trace_pcb, paired .xo, and .kicad_pro together. Features below depend on a compatible build and host; native controls are not automatically available in Trace Plugin.
AI Layer Control
Choose the active copper layer and visible layers before inspecting or editing. In a supported session you can ask “Show the back copper layer,” then check the displayed layer. Visibility changes do not change the board's layer count or stackup.
Component Placement
Use the default Move (M), Rotate (R), and Flip (F) controls to arrange footprints. Check pad numbers, net assignments, component side, and footprint orientation.
Establish actual mechanical requirements first: mounting holes, enclosure openings, approved connector poses, internal access, component height, and thermal constraints. Not every connector belongs at an edge. A 2D layout or 3D preview does not certify access or enclosure fit.
AI Auto-Placement
Trace's advanced placement and routing offers Place only, Route only, and Place & route in compatible sessions. Review classification, preflight findings, preservation choices, time limit, and displayed cost before Run advanced layout.
How It Works
The reviewed board is submitted for hosted processing; returned changes must be applied and saved before you treat them as the project's layout. A started or completed job is not proof of successful application or engineering correctness.
Follow Placement and routing for the full procedure. These engines act on the whole board; a request to move one part or route one net is not permission for a global run.
Design Variants
Use Design Variants for fitted configurations, not branch history. Review the selected variant and actual manufacturing output; do not assume every exporter or CLI applies identical filtering.
Routing
Use Route Tracks (X with default shortcuts) for manual routing and the via control (V) to change copper layers. Check widths, clearances, return paths, and unrouted connections rather than relying on visual proximity.
Routing engines: Basic vs Advanced
- Basic routing, called Quick routing in older builds, is the free routing option, distinct from paid advanced layout. Review its settings card before Route board, then follow passes and the actual applied result. Account, connection and host availability still apply; routing may leave unresolved connections.
- Trace's advanced placement and routing can arrange components, route, or do both. Review the current billing, native settings, cost ceiling, and actual outcome.
Routing-only keeps placement and does not require classifying every footprint as Protected. All-Protected classification blocks placement, not routing.
Use Stop to request keeping the last basic routing result, or Switch to advanced routing to review a different engine. Opening advanced settings does not start it. Starting while basic is still running sets aside its partial routing; if basic already finished, advanced uses the current board. Follow Placement and routing for preservation, save and DRC checks.
Layer Stackup & Impedance Control
For controlled impedance, obtain the manufacturer's actual stackup and agree the geometry and tolerances. Configure corresponding widths and clearances in the board rules. A calculator estimate or DRC geometry check is not measured impedance.
Differential Pairs
Set the intended pair names, width, gap, and skew constraints, then use the native differential-pair routing tools where available. Inspect layer changes and reference-plane continuity separately; automatic routing does not certify the interface.
Signal Integrity Considerations
Review critical paths against device and interface requirements, including return paths, discontinuities, loading, and termination. Ask the assistant for a bounded review, not a universal signal-integrity approval.
Length Tuning & Matched Length Groups
Native interactive controls include Tune Length of a Single Track, Tune Length of a Differential Pair, and Tune Skew of a Differential Pair (default shortcuts 7, 8, and 9).
Set a requirement-derived target and tolerance. Check the displayed measurement domain and endpoints before tuning; added meanders can affect spacing and coupling.
Matched Length Groups
In compatible native builds:
- Select the intended nets and choose Route → Create Matched Length Group, or the corresponding Net Inspector action.
- Review membership, target policy, and tolerance in Properties.
- Confirm whether measurements are physical length or delay. Delay needs valid stackup and propagation assumptions.
- Tune members interactively and rerun DRC; creating a group alone does not route or tune them.
Native groups can represent signals split across series components. Inspect approximate or ambiguous path measurements, and the configured via and package contributions, before using a total as timing evidence.
AI length matching
Tell the assistant which signals, target, tolerance, and measurement domain to review. Inspect the actual native group or changes returned; do not infer auto-tuning from a matching report.
Trace Plugin's companion measurement is different: it measures routed tracks, excludes vias and pad escapes, and does not create persistent matched groups, auto-tune, or provide propagation-delay matching. Tune in the host and verify its own measurements.
Design Rule Check
Open Inspect → Design Rules Checker in the Full interface, refill zones, and click Run DRC. Review configured clearance, width, hole, courtyard, edge, and unconnected-item findings.
Choose the intended Rules Preset, including Default (no manufacturer) for baseline rules. Manufacturer presets do not cover every production requirement. See DRC Import and DRC Rule Editor.
Copper Pours
Add a filled zone, select its intended net and layers, draw its boundary, then refill zones (B with default shortcuts). Inspect isolated islands, thermal connections, return paths, and keepouts after every relevant change.
Track & Via Properties
Review width, layer, drill, and pad dimensions in the native properties controls. Special fabrication processes such as backdrilling need manufacturer agreement and matching output; a property field alone does not order that process.
Manufacturing Export
IPC-2581
Use this export only when the installed exporter and your manufacturer support the intended version and contents. Inspect the output's board profile, layers, references, and assembly data.
Standard Exports
Follow Exporting Designs for Gerbers, drills, BOM, positions, and mechanical files. Inspect the actual artifact before ordering.
Case Design Import
Use available mechanical-reference controls to compare the board with enclosure drawings. Confirm units, origin, rotation, and side before relying on alignment.
Supported Formats
DXF can provide 2D reference geometry. STEP can support 3D comparison through the installed model/viewer or mechanical-export workflow; it is not a universal enclosure-import command.
Use Cases
Review mounting-hole alignment, port openings, access direction, and component height against real mechanical requirements. Inspect access again after placement and before routing.
Importing from Other EDA Tools
See Importing from Other EDA Tools for supported native import paths and the required post-import checks.
If Layout Does Not Finish
Read the specific preflight, job, application, or save error. Preserve your last saved board and available recovery copy. Check returned geometry and unrouted connections before a new run; do not weaken a required fixed pose or rule just to bypass a refusal.