Skip to content

Wiring and Nets

Wires connect component pins into electrical nets. This page covers drawing wires, connecting pins, placing net labels, and using power symbols.

Drawing Wires

Activating the Wire tool

Press W or click the Wire button on the toolbar.

How to draw a wire

  1. Click on a component pin (or any point on the canvas) to start a wire
  2. A temporary wire follows the cursor — drawn orthogonally (horizontal and vertical segments only)
  3. Left-click to add each corner vertex
  4. Right-click or press Esc to end the wire
Example — wiring R1 to C1:

  R1             C1
  ─┤├──────────+─|─
    Pin 2       |
                (corner vertex if needed)
Action Input
Start a wire Click on a pin or canvas point
Add a corner Left-click
End the wire Right-click or Esc
Cancel before starting Esc

Starting from a pin snaps automatically

When you click on a pin tip, WireFrame snaps the first vertex precisely to that pin — no manual alignment needed.

Connecting Wires to Pins and Existing Wires

To another pin

  • The final vertex snaps to the target pin position
  • Both pins are now on the same net

To an existing wire

  • The new wire shares the meeting point with the existing wire
  • WireFrame merges them into a single net
Example — GND bus connecting 3 points:

  C1    C2    R1
  ─|─   ─|─   ─┤├─
   │     │        │
   └─────┴────────┘
              │
             GND ⏚

Junction Dots

A junction dot appears when three or more wires meet at a single point:

  With junction:           Without junction (wires cross, not connected):
  ───●───                  ───┼───
     │                        │ (not connected)
  • Junction dots are placed automatically when three or more connections share a point
  • You can also place them manually with the Junction tool
  • Two crossing wires without a junction are not electrically connected

Editing Existing Wires

Operation How
Move a vertex Drag a point on the wire
Drag a segment Click and drag a segment between two vertices → adds two new vertices, moves orthogonally
Delete a wire Select + Del

Auto-simplification

After dragging a segment, WireFrame automatically removes redundant collinear vertices — keeping the wire geometry clean.

Net Labels

Net labels allow you to connect two points electrically without drawing a wire between them. Labels with the same name belong to the same net.

How to place a net label

  1. Press L or click the Label tool
  2. Click on the canvas to place a label
  3. Edit the Value in the Properties panel (e.g. SDA, SCL, +3V3, RESET)
  4. All wires connected to that label share the same net name
Example — connecting without a direct wire:

  MCU U1                Sensor U2
  ──[SDA]               ──[SDA]
  ──[SCL]               ──[SCL]

  → SDA and SCL are automatically connected
    even though no wire runs between them

Use consistent names

All labels with the same name (e.g. +3V3) merge into a single net — even on different parts of the sheet. This is the cleanest way to distribute power to multiple components.

Power Symbols (GND, VCC)

Symbol Shortcut Description
GND G Ground reference — implicitly connects all GND pins
VCC — (toolbar) Positive supply rail

Power symbols are single-pin components that automatically assign a net name to any wire connected to them.

Example power connections:

   +5V
    ↑ VCC
    │
   [C1] 100nF
    │
   ─┴─ GND ⏚

Net Highlighting

Click on any wire or net label: - All wires and pins on that net are highlighted in a distinct color - Useful for tracing connectivity in complex schematics

Click on empty canvas to clear the highlight.

How the Netlist is Built

WireFrame automatically constructs the netlist from all wires, pins, and labels:

  1. Groups all wires that share vertices into clusters
  2. Collects all pins attached to each cluster
  3. Determines the net name by priority:
    1. Net label / power symbol values (highest priority)
    2. Pin-based default names (e.g. Net_U1_1)
    3. Wire-based fallback names (e.g. Net_Wire_42)

This netlist is used for: - Net highlighting on the canvas - PCB netlist generation when converting to PCB - DRC consistency checks between schematic and PCB

See Also