KB: Updating Net Name of Entire Track in a Single Operation

Created: September 24, 2025 | Updated: September 26, 2025

Altium Designer

When schematic changes are made—such as renaming nets or adding new components—some routed tracks in the PCB layout may retain outdated net names. This can lead to clearance violations and inconsistencies between the schematic and PCB. This article explains why this happens and outlines two methods to update the net names of affected tracks efficiently, either by reconnecting them to component pads or manually updating them via the Properties Panel.

Solution Details

Why Tracks Retain Old Net Names After Schematic Changes

After renaming nets in the schematic, the PCB should reflect these changes automatically. However, during design revisions, if tracks become disconnected from component pads, they may retain their original net names. These unconnected tracks are not updated by ECO and can cause clearance violations due to mismatched net associations.

Why This Happens

Net names are assigned based on connections to net-defining objects such as component pins, net labels, or ports. If a track is no longer connected to such objects, it becomes a free primitive and retains its previous net name. ECO processes do not update these free primitives, which leads to inconsistencies and potential design rule violations.

Available Solutions to Update Track Net Names

To resolve this issue, you can use one of the following methods:

Solution 1: Reconnect tracks to component pads and update netnames via the netlist.
Solution 2: Manually select and rename track segments using the Properties Panel.

Step-by-Step Instructions

Solution 1: Reconnect Tracks and Update via Netlist

1. Start Interactive Routing.
2. Set routing mode to Ignore Obstacles.
3. Route the disconnected tracks to their respective component pads.
4. Navigate to Design » Netlist » Update Free Primitives from Component Pads.
5. Confirm the update to apply the correct net names.

Solution 2: Manually Update Net Names via Properties Panel

1. Select a segment of the track.
2. Press Tab to select the entire track on the same layer.
3. Press Tab again to include all objects belonging to the same net across other layers.
4. Open the Properties Panel.
5. Change the Net Name to the updated name from the schematic.

Additional Notes

Tracks disconnected from pads are treated as "free primitives" and are not automatically updated by ECO.
Always verify connections after schematic changes to ensure net integrity.
Clearance violations often indicate lingering outdated net names.