Skip to content

Routing Traces

Trace routing connects pads on the PCB with copper paths, enforcing electrical and design-rule constraints. This page covers the full routing workflow: drawing traces, placing vias, adding holes, and routing helpers.

Starting a Route

Press X or click Route Trace on the PCB toolbar.

Drawing a trace

  1. Click on a pad (or an existing trace/via) to start routing
  2. The trace follows the cursor with 45° helper points computed automatically
  3. Left-click to confirm each corner vertex
  4. Click the destination pad to complete the trace — the ratsnest line disappears
  5. Or right-click / Esc to cancel
Example — routing U1 to R1:

  [U1.Pin3]══════════════[R1.Pad1]
               ↑
       completed trace (red = F.Cu)

  ╌╌╌╌╌╌ ratsnest line disappears once routed
Action Input
Start on a pad Left-click
Add a corner Left-click
Finish on the destination pad Left-click on target pad
Cancel Right-click or Esc
Switch layer (place via) V while routing

Real-Time Clearance Checking

During routing, WireFrame checks for violations and warns immediately if the trace is too close to:

Check Example
Trace ↔ Trace Two traces on the same layer too close together
Trace ↔ Pad Trace overlapping a pad from a different net
Trace ↔ Via/Hole Trace crossing through a drill area
Trace ↔ Board Edge Trace too close to Edge.Cuts
  • A red indicator appears at the violation point
  • The trace cannot be completed while a clearance violation is active

Vias — Switching Layers

A via is a plated hole that connects F.Cu and B.Cu, allowing a trace to change board sides.

Placing a via while routing

  1. While routing on F.Cu, press V
  2. A via is placed at the current cursor position
  3. The active routing layer switches to B.Cu
  4. Continue routing on B.Cu from the via
  F.Cu:  [U1]══════●
                    │  ← Via (through-hole)
  B.Cu:             ●══════[R5]

Manual via placement

  1. Select the Draw Via tool from the toolbar
  2. Click on the board to place a via
  3. Assign a net in the Properties panel if needed

Via properties

Property Description
Diameter Copper annular ring outer diameter
Drill Drill hole diameter
Net The electrical net the via belongs to

Mechanical Holes

Use the Place Hole tool to add non-electrical holes (screws, standoffs):

  1. Select Place Hole from the toolbar
  2. Click on the board to place it
  3. Set parameters in the Properties panel:
Property Description Example
diameter Hole diameter 3.2 mm for M3 screws
plated Whether the hole has copper plating Usually false
netName Net if plated (e.g. for GND stitching) GND

Editing Existing Traces

Operation How
Move an entire trace Select + drag
Drag a segment Click and drag a segment between two vertices
Delete a trace Select + Del (ratsnest reappears)

Automatic net update

Deleting or modifying a trace marks the affected net as dirty → the ratsnest is automatically recomputed to show any missing connections.

Gloss Trace — Cleaning Up

After routing, WireFrame can automatically clean up trace geometry:

  • Removes redundant vertices (collinear points)
  • Simplifies short zig-zag segments
  • Makes 45° corners clean and precise
Before Gloss:          After Gloss:
  ──╮                   ──╲
    ╰──╮                   ╲──
        ╰─                    ─
  (redundant vertices)    (clean 45°)

Use: context menu → Gloss or the corresponding shortcut.

Smart Drag

WireFrame maintains connections during drag operations:

  • Moving a via — attached traces keep their endpoints connected to the via
  • Moving a footprint — connected trace endpoints adjust automatically to maintain pad attachment

See Also