Wire, Net Label, Break Wires, & Set Net Colors



A wire is a polyline electrical design primitive that is used to form electrical connections between points on a schematic. It is analogous to a physical wire.

Net Label

 Net labels identify and electrically connect different points in a schematic.

Net labels identify and electrically connect different points in a schematic.

Electrical connectivity between schematic component pins can be created by placing a wire between those pins. This is called physical connectivity since the pins are physically connected with a wire. Connectivity can also be created logically by using suitable net identifiers, such as net labels. As well as providing a human-friendly identifier for a net, a net label allows you to connect points on a circuit without actually physically wiring them together.

Break Wires

The Break Wires command is used to break a segment of a polyline object (wire, bus, or signal harness) into two pieces at a chosen location on the schematic sheet. The Break Wires command can be accessed from the schematic editor in the following ways: 

  • Select Tools | Convert | Break Wires from the main menus. 

  • Right-click over the segment of the polyline object then select Break Wire from the context menu. 

After launching the command, the cursor will appear in accordance with settings defined for the Cutter Box, and Extremity Markers, on the Schematic - Graphical Editing page of the System Preferences.

Position the cursor over the segment of wire, bus, or signal harness that you want to effectively break into two then click, or press Enter. The indicated length of the segment will be removed, thereby breaking the segment into two.

Continue breaking further polyline objects, or right-click, or press Esc, to exit.

While in break wire mode, the following additional actions can be performed:

  • Press the Spacebar to cycle through the following cutting length modes:
    • Snap To Segment - in this mode, the cutter will auto-size to snap to an entire polyline segment.
    • Snap Grid Size Multiple - in this mode, the cutter is sized to a defined multiple of the current snap grid.
    • Fixed Length - in this mode, the cutter is sized to a defined fixed length.


  • Regardless of the size of the cutter, other than Snap To Segment, the cutter will shrink to accommodate smaller-sized wire segments in their entirety - as it passes over them - as though Snap To Segment were selected.
  • You can also remove selected wire segments (not segments of bus or signal harness objects) with the tap of the Delete key, with auto-junctions also accounted for - allowing you to remove a segment of a wire up to that junction only (and including that junction if only two other wire segments would otherwise remain connected to it). Simply click twice (with a pause in between) on a particular segment of wire to select it, denoted by its end-point editing handles turning red. You can delete multiple segments across different wires, ensure that each is selected (Shift+click twice on each subsequent segment to include it in the overall segment selection).

Set Net Colors

Net color commands are accessed from the schematic editor by choosing Tools | Net Colors | Set Net Colors from the main menus. 

As the design builds up it quickly becomes dense and detailed - the schematic busy with wiring and the board a maze of connection lines and routed nets. To help bring clarity and visibility, the designer can apply color to the schematic wiring, PCB connection lines, and routing. 

The ability to selectively override the color of specific nets is known as Net Color Override. Color can be applied to schematic nets and those color settings transferred to the PCB, or color settings can be applied directly from the PCB Editor's PCB panel

Toggle Net Color Override on or off in the schematic seditor with the F5 shortcut key.

Applying Color to the Schematic Nets

Click on a pin, wire, bus, or net identifier (net label, sheet entry, port, power port, or offsheet connector) to apply the selected color to that net (or all the nets in a bus). The command remains active after clicking on the first net, ready to color subsequent nets in that same color if required.

When a color is applied to a net or a bus, it overrides any previous color setting. Note that net color settings cannot be undone, to remove a color setting use the Clear Net Color command or the Clear All Net Colors command.

The color is automatically applied to all sections of the net, on all schematic sheets in the project. This occurs automatically when the background compiler updates the connectivity of each sheet.

To include color on a net or bus that connects two sheet symbols, include a net label on the net/bus running between the sheet symbols.

Color is not applied to a component pin or a power port, drag them apart to add a wire if there is no color showing on that section of net.

The color setting for a net is not stored with the various objects placed on the sheets. The color settings are actually stored in the project file as a net-level setting and are applied on each schematic sheet after it is opened and the background compiler has compiled that sheet.
If you find an issue, select the text/image and pressCtrl + Enterto send us your feedback.