Documentation / Design

PCB Layout

Bring your schematic to the board, shape the outline, place and route parts, and check the result.

The board editor turns your schematic's connections into footprints and copper. You can do every step by hand, ask the assistant, or hand placement and routing to Trace's engines.

The Simple layout shows a small action bar (Route, Via, Zone, Add footprint, DRC, 3D, Ask Trace, Chat). Menus such as Tools, Route and Inspect, and the full toolbar, show in the Full layout; on a Mac the menu bar is always there. Switch in Preferences > Interface > Layout.

Editor Overview

A typical board goes like this:

  1. Bring the parts over from the schematic.
  2. Set the board outline, layers, mounting holes and your manufacturer's rules.
  3. Place the parts.
  4. Route the connections and pour copper.
  5. Run DRC, then export the fabrication files.

AI Layer Control

Ask the assistant to show or hide layers, for example "Show only the back copper and silkscreen". This changes what you see, not the board's layer count.

Bring the Schematic to the Board

Save the schematic, then use Tools > Update PCB from Schematic (F8) in the board editor, or ask the assistant to update the board. Review the list of parts and nets that will be added, changed or removed before you apply it.

When the assistant updates a board whose footprints are not linked to the schematic, for example a board imported or edited on its own, it stops before adding a second copy of every part. It lists the references that would be doubled and can update the footprints in place by matching their references instead. New in Trace 3.2.

Board Outline and Mounting Holes

Draw the outline on the Edge.Cuts layer as one closed shape, or ask the assistant for it, for example "Make the board a 50 x 30 mm rectangle with M3 mounting holes in the corners".

  • Mounting holes land exactly where you ask. If one cannot go there, because it would be off the board, inside a cut-out or too close to the edge, the assistant tells you why instead of moving it.
  • Keep-out and cut-out areas can be placed by their centre or by their corner.

Shape the Board From an Enclosure Drawing

New in Trace 3.2: give the assistant your enclosure's DXF drawing and it cuts the board outline from it.

  1. Attach the DXF with the paperclip in the chat. Trace saves the drawing in your project.
  2. Ask, for example: "Shape the board from this drawing. The outline is on the BOARD layer."
  3. The assistant cuts the outline only from the drawing's outline layer. If you don't name one, it uses a layer named like an outline (OUTLINE, EDGE, PROFILE, CONTOUR, BOARD or PCB), or else the outer contour.
  4. It then reports every other feature in the drawing, such as holes, keep-outs, openings and light pipes, with where each one is and whether anything on the board covers it.
  5. Ask it to place mounting holes, keep-outs or cut-outs at those positions.

Check units, origin and orientation against the drawing before you place parts.

Component Placement

Use Move (M), Rotate (R) and Flip (F) to arrange footprints. Settle the mechanical side first: mounting holes, connectors that must face out of the case, buttons and LEDs under openings, and tall parts.

AI Auto-Placement

Trace's advanced placement and routing can place parts, route, or both, on the whole board or on the parts and nets you name. Mark the parts that must stay put first.

How It Works

You review a settings card, press Run advanced layout and watch the board update as the engine works. The result lands as moved parts and new copper, and the whole run is one Undo step. Follow Placement and Routing for the full procedure, including Stop, Finish here, Keep going and Revert to pre-layout.

Design Variants

Use Design Variants for fitted and not-fitted versions of the same board.

Routing

Use Route (X) to route by hand and press V to add a via and change layers. The board editor shows remaining connections as thin lines (the ratsnest).

Routing engines: Basic vs Advanced

  • Basic routing is free. It routes the parts you placed and shows its progress on a card in the chat. Stop keeps everything routed so far.
  • Trace's advanced placement and routing places and routes with Trace's advanced engine and is billed on compute time. It keeps your locked traces and protected parts.

You can start with basic routing and Switch to advanced routing from the same card. See Placement and Routing.

The Assistant Can Finish Your Board

New in Trace 3.2: in Agent mode, the assistant lists every open connection, moves or rotates parts with checks for overlaps, the board edge and clearance, and routes single connections with the board editor's own router. Each step is one Undo. See Let the Assistant Finish the Board.

Layer Stackup & Impedance Control

Set the layer count and stackup in Board Setup. For controlled impedance, get your manufacturer's stackup and set the matching track widths and gaps in your net classes. A calculator estimate is a starting point; your manufacturer confirms the real impedance.

Differential Pairs

Name both halves of a pair (for example USB_D+ and USB_D-), set their width and gap, and route them with Route Differential Pair (6). Keep the pair on a continuous reference plane.

Signal Integrity Considerations

Ask the assistant to review critical nets: return paths, layer changes, pair spacing and lengths. Treat its answer as a review aid alongside the datasheets and your interface's requirements.

Length Tuning & Matched Length Groups

Tune lengths with Tune Length of a Single Track (7), Tune Length of a Differential Pair (8) and Tune Skew of a Differential Pair (9). Set the target and tolerance from the interface's requirements.

Matched Length Groups

  1. Select the nets and choose Route > Create Matched Length Group.
  2. Check the members, target and tolerance in Properties.
  3. Choose whether the group matches length or delay. Delay needs a correct stackup.
  4. Tune the members and run DRC. Creating the group does not tune anything by itself.

A group can follow a signal through series parts, such as a resistor in line.

AI length matching

Tell the assistant which nets to match, and to what target and tolerance. In the Trace app it creates a matched length group with those settings and reports each member's length; you then tune the members. In the Trace Plugin, the assistant can also tune Altium Designer boards; in KiCad and Autodesk Fusion it measures lengths only. See Altium Designer.

Design Rule Check

Open Inspect > Design Rules Checker (or press DRC in the Simple layout), keep Refill all zones before performing DRC ticked, and press Run DRC. Click a finding to jump to it.

Choose your manufacturer in the Preferred Manufacturer list, then check Rules Preset in the DRC window. Default (no manufacturer) uses the board's own rules. See DRC Import, DRC Rule Editor and Design Review.

Copper Pours

Draw a zone, pick its net and layers, then fill all zones (B). Refill after every change near a pour, and check for isolated islands and thermal relief on pads.

Track & Via Properties

Select a track or via to change its width, layer, drill and pad size in Properties. Special processes such as blind vias or backdrilling need your manufacturer's agreement.

Enclosures and 3D

  • Press 3D to see the board with its 3D models.
  • Trace Mechanical designs a 3D-printable case around the board and warns you when a connector moves off its opening or a part gets too tall for the lid. Open it from View > Mechanical.
  • File > Export > IDFv3 writes each part's real height (from its 3D model or Height field), the heat it gives off and any height limits, for mechanical CAD. File > Import > IDFv3 Board brings a board outline, holes and keep-outs in. Parts from an IDF file arrive as placeholders, and Update PCB from Schematic swaps each one for the real footprint in the same place. Export again any IDF files made with Trace before 3.2.

Manufacturing Export

IPC-2581

Use IPC-2581 when your manufacturer asks for it, and open the file in a viewer to check the outline, layers and parts.

Standard Exports

Follow Exporting Designs for Gerbers, drill files, BOM and positions, or Send to Manufacturer. Files the assistant makes go to your project folder, or the folder you name.

Importing from Other EDA Tools

See Importing from Other EDA Tools for Altium, KiCad, EAGLE and other projects.

In the Trace Plugin

The plugin works on the board open in Altium Designer, KiCad or Autodesk Fusion, using that tool's own editor, DRC, save and undo. In KiCad, the assistant can shape the outline from a DXF that sits in your project folder. In Fusion, parts and connections come from the schematic, so add or remove parts there. See Trace Plugin.

If Layout Does Not Finish

Read the message on the card or in the chat: it names the part, net or rule. Fix that, save, and try again. Keep your required fixed positions and rules; don't loosen them only to get a run through. Undo or Revert to pre-layout takes back an advanced run.