# Routing Traces

Trace routing connects pads on the PCB with copper paths under the board's design rules. This page covers drawing traces, changing layer through vias, mounting holes, and editing finished routes.

---

## Starting a Route

Press ++x++ or click **Route Trace** on the PCB toolbar (the vertical toolbar on the right edge of the canvas).

### Drawing a trace

1. **Click a pad** (or an existing trace or via) to start. The trace takes the net of what you clicked and the width of that net's class. Starting from a track continues on that track's layer.
2. Move the cursor. WireFrame previews the next leg with 45° or 90° steps, with corners rounded or mitred in the style set under **Properties → Board Settings → Corners**. ++slash++ flips the corner order (which way the 45° step goes first). The preview is exactly what a click lays — the same leg, snapped to the same point; inside a pad or via of the same net, the cursor snaps to its centre.
3. **Click** to commit each waypoint. ++backspace++ steps the route back one waypoint — the followers of a bus and any via dropped at that point included.
4. **Click the destination pad** to finish — or a trace of the same net, which joins the new trace to it. When the pad is on another copper layer, a via is dropped at the last point and a 45° leg reaches the pad on its layer. **Double-click** anywhere finishes the connection: a clean straight, 45° or L-shaped leg to the nearest pad of the net the trace does not reach yet, or, when there is no clean leg, [Route Assist](#route-assist) for that connection only. The ratsnest line disappears once the connection is complete.
5. ++esc++ ends the track and keeps the route tool, ready for the next one; a second ++esc++ leaves the tool. Picking another tool mid-route ends the route the same way — it is always one undo step.

### Image — Completed pad-to-pad route

![A completed +5V route on F.Cu, selected](../assets/wf/docs/pcb/routing/completed-pad-to-pad-route.png)
| Action | Input |
|---|---|
| Start on a pad, trace, or via | Click |
| Commit a waypoint | Click |
| Step the route back | ++backspace++ (also takes back a via dropped at that point) |
| Finish on the destination pad | Click the pad |
| Finish the connection from here | Double-click |
| End this track, keep routing | ++esc++ (a second ++esc++ leaves the tool) |
| Flip the corner order | ++slash++ |
| Thinner / wider trace | ++bracket-left++ / ++bracket-right++ (1 mil per press, within the net class limits) |
| Change layer (drops a via) | ++v++, ++tab++, or ++space++ — see below |
| Route the net under the pointer | ++ctrl+shift+w++ with nothing selected |

Routing keys only act while a route is running and never from a text field: ++backspace++ does not delete the track you started from, and ++space++ does not rotate a footprint that is still selected.

While you route, a small readout near the cursor shows the net, its class, the layer, the width, the clearance, how violations are handled, the routed length so far, and the keys that apply. For a net with high-speed rules it adds the return path, the plane edge and crosstalk of the track being drawn — see [High-Speed checks](../high-speed/checks-and-interfaces.md#while-you-route).

---

## Route Modes and Clashes

**Properties → Board Settings → Track → Mode** chooses how a click behaves:

| Mode | What happens |
|---|---|
| **Free (mark clashes)** (default) | The track goes exactly where you draw it. Anything it comes too close to — another net's track, pad, via, hole or the board edge — is measured on its real shape and **drawn** as you route, and DRC reports it afterwards. Nothing is refused, and nothing slows down on a dense board |
| **Walkaround** | Each click searches for a way around obstacles. Slower on dense boards |
| **Shove (push tracks)** | As Free, and the tracks of other nets in the way are **pushed off** by their clearance — the preview draws them where they will go before you click. A pushed track keeps its ends and its 0/45/90° shape, and pushes the tracks behind it in turn (a few deep). Pads, vias, a track that crosses yours, a track tied to a pad inside the clearance and your own route's copper are never moved: then nothing moves, the leg is laid as in Free and the clash is marked, with the reason beside it. The route and every track it pushed are **one undo step** |

How a clash is drawn follows the net class setting **Design Rules → Clearance → When violated**:

| Setting | Preview colour |
|---|---|
| **Block** (default) | Red — the segment is still laid; DRC reports it as an error |
| **Warn** | Amber — laid and marked |
| **Allow** | The layer's colour |

A route ends with a hint such as *too close to other copper · right-click › Reroute Clashing Tracks*. Fix clashes with [Route Assist](#route-assist), by moving the copper, or by changing the rule. Dragging a routed segment is never stopped by clearance either; its clashes are drawn the same way.

Ending a route on a pad of a **different net** is allowed — a pad or via of another net is a waypoint, not an end — and DFM/DRC reports the short. Always run [DFM & DRC](dfm-and-drc.md) after routing.

---

## Route Assist

Route Assist routes for you, on the board as it is, and applies the result as **one undo step**. It runs in the background (++esc++ stops it) and only touches the nets you gave it.

| Command | Where | What it does |
|---|---|---|
| **Auto-route Net** / **Auto-route Bus** | Right-click a track; the **Auto-route** button on the PCB toolbar; ++ctrl+shift+w++ | Lays what is still ratsnest on the selected net(s), around every other net's copper |
| **Auto-route** with nothing selected | ++ctrl+shift+w++ | Routes the net under the pointer |
| **Reroute Track(s)** | Right-click a track | Takes the selected tracks up and routes their nets again, clear of everything else |
| **Reroute Clashing Tracks (N)** | Right-click a track | Reroutes only the tracks of these nets that are too close to another net's copper |
| Double-click while routing | Canvas | Finishes one connection (see above) |

Route Assist reads the board's design rules and stackup, and joins at track ends inside pads. Review its copper like your own, and run DRC.

---

## Vias — Switching Layers

A via is a plated hole that connects copper layers so a trace can change layer.

### Changing layer while routing

| Key | Via goes to |
|---|---|
| ++v++, ++tab++, or ++space++ | The other layer of the via pair (F.Cu ↔ B.Cu by default) |
| ++equal++ / ++minus++ (or keypad ++num-plus++ / ++num-minus++) | The next / previous copper layer of the stackup |
| ++page-up++ / ++page-down++ | F.Cu / B.Cu |
| ++shift+v++ | A layer you pick from a list |

The via is dropped at the last waypoint and routing continues on the new layer. Move away from the start point first — a via cannot be dropped on it. The via type (through, blind/buried, or micro) follows **Properties → Board Settings → Vias → Type**, which defaults to the net class.

### Image — Route changing layer through a via

![The LED feed rerouted through the back: it leaves D3 on F.Cu, V drops a via, it crosses on B.Cu, a second V brings it back up to R8 — and DFM stays clean](../assets/wf/docs/pcb/routing/route-changing-layer-through-a-via.png)
### Placing a via by itself

1. Select **Place Via** on the toolbar (++v++ when not routing).
2. Click on the board. On a track's centre line the via lands on it and takes its net; elsewhere it snaps to the grid and takes the net of the pad under the cursor. If it lands too close to another net, the tool says so at once.

### Via properties

Select one or more vias to edit them in **Properties**. Edits apply to every selected via.

| Field | Description |
|---|---|
| Lock | Locked vias cannot be moved or deleted |
| Type | **Through**, **Blind/Buried**, or **Micro**, with the layers it spans |
| **Diameter** / **Drill** | Copper pad and hole size; **Ring** shows the annular ring left around the hole |
| **Reset to net class** | Takes diameter and drill from the net class in Design Rules |

---

## Mounting Holes

Use **Place Mounting Hole** (++h++) for holes such as screws and standoffs:

1. Select the tool and click on the board.
2. Select the hole and set it in **Properties → Hole Properties**:

| Field | Description | Example |
|---|---|---|
| **Diameter** | Hole diameter, in mil with the mm value beside it | 3.2 mm for M3 screws |
| **X** / **Y** | Position | |
| **Plated (PTH)** | Copper-plated hole | Usually off |
| **Net** | Net of a plated hole (shown when **Plated** is on) | `GND` |

---

## Editing Existing Traces

| Operation | How |
|---|---|
| Select a segment | Click it |
| Select a whole net | Double-click a trace — every trace and via of that net is selected and highlighted |
| Move | Drag the selection, or nudge it with the arrow keys (5 mil per press) |
| Delete | ++delete++, or right-click → **Delete Segment(s)** / **Delete Track(s)**. The ratsnest reappears |
| Change layer, width, or corners | Right-click → **Edit** (below), or **Properties → Trace Properties → Layer** |

Moving a via or a footprint keeps the attached trace endpoints connected.

### The trace context menu

Right-click a selected trace:

| Group | Item | What it does |
|---|---|---|
| **Route Assist** | **Auto-route Net** / **Auto-route Bus**, **Reroute Track(s)**, **Reroute Clashing Tracks** | See [Route Assist](#route-assist) |
| **Select** | **Connected Track Chain** | Every track joined end-to-end to the selection, through vias, up to the pads |
| | **All Copper of Net(s)** | Every track and via of the selected nets |
| | **Highlight Net** | Highlights the net on the canvas |
| **Edit** | **Move to Layer ▸** | Moves the selected tracks to another copper layer |
| | **Width ▸** | Type a width and **Apply**, or use **Net class width** or **Match widest** |
| | **Corners ▸** | Set a radius, then **Miter 45°** or **Arc** |
| | **Merge Collinear Segments** | Joins pieces that continue along the same line |
| **Bus** (several parallel tracks) | **Distribute Evenly** | Keeps the two outer tracks and spaces the ones between evenly |
| | **Pack to Top / Left**, **Pack to Bottom / Right** | Closes the gaps to width + clearance toward one side; ends on pads stay put |
| | **Set Pitch ▸** | Centre-to-centre spacing from the top or left track |
| **High-speed ▸** | Tune length, pairs, and groups | See [Length tuning and pairs](length-tuning.md) |
| | **Delete Segment(s)** / **Delete Track(s)** | Removes the selected segments, or whole tracks |

Review clearance after every group operation and re-run DFM.

---

## Consolidate Collinear Trace Segments

After routing, select the segments, right-click, and choose **Edit → Merge Collinear Segments** to remove boundaries between pieces that continue along the same line. It does not simplify zig-zags or redesign the route; use **Corners ▸** to round or mitre corners instead. Inspect the result and re-run DFM/DRC.

### Image — Route before and after trace consolidation

![Right-click a selected /12V_filtered track: Merge Collinear Segments joins the pieces that run along one straight line](../assets/wf/docs/pcb/routing/route-before-and-after-trace-consolidation.png)
---

## Routing Several Traces Together

Select two or more existing traces, choose **Route Trace**, and click one of the selected traces to continue them all at once. The other traces follow in parallel at their current spacing. When the leading trace lands on its pad, each follower lands on its own pad — with a clean leg, or with Route Assist when a clean leg would clash — and the whole bus is one undo step. ++backspace++ steps all of them back together.

---

## Length Tuning and Differential Pairs

Routing a declared pair routes both halves together; meanders add length where a net is short against its pair, its group or its target; a live gauge shows the difference while you route. See [Length Tuning and Differential Pairs](length-tuning.md).

---

## AI-Assisted Routing

The AI Copilot can propose placement and routing for the whole board with `/layout`. Proposals run on a copy and change nothing until you apply them. See [Placement and Routing Assistant](../ai/auto-placer-router.md).

---

## See Also

- [Footprints & Placement](footprints-and-placement.md) — place footprints before routing
- [Layers & Views](layers-and-views.md) — manage layers during routing
- [Zones & Planes](zones-and-planes.md) — copper fills interact with trace clearances
- [Design Rules & Net Classes](design-rules.md) — configure clearance and trace width rules
- [DFM & DRC](dfm-and-drc.md) — check clearances and widths after routing
- [Length Tuning & Differential Pairs](length-tuning.md) — pairs, groups and meanders
- [High-Speed Workbench](../high-speed/index.md) — impedance, return path, crosstalk and power on the routed copper
- [Placement and Routing Assistant](../ai/auto-placer-router.md) — AI-assisted placement and routing review
