Improvements to Same-Net Clearance Rule

This document is no longer available beyond version 16.0. Information can now be found here: Clearance Design Rule for version 24


In Altium Designer 16, improvements have been made to the Same-Net Clearance Rule that produce violations only for significant cases, i.e., ignoring cases that are not as significant. In previous Altium Designer versions, the Same-Net Clearance Rule could be defined, of course; however, it was applied in many cases that were not appropriate. In this release, we have improved the rule so that it ignores cases that are not valid violations. The most common case that is now ignored is when a track crosses the perimeter of another primitive, such as a pad or fill area. The Same-Net Clearance Rule is also useful for defining the “first corner rule” when exiting a pad and thus ensuring that tuning doesn’t create traces that are too close together.

How to Access

The Same Net Only clearance rule is defined in the PCB Rules and Constraints Editor dialog (from a PCB document, click Design » Rules). In the Constraints region, hover the cursor on or near the current constraint and click the down arrow to access a drop down menu of choices that are specific for that rule and constraint. Click Same Net Only.

New Violation Parameters

Using the Same-Net Clearance Rule now produces violations for the following:

Violations for Track to: Via, Pad, Fill, Region, or Polygon:

  • If a track centerline doesn't cross the perimeter of the other primitive.
  • For same-net track whose centerline does not cross the via-edge, a track-edge to via-edge and the distance that is less than the All Clearance rule.

Violations for Track to Track:

  • If parallel: if track segments are parallel and clearance is less than is set in rule = violation.
  • If not parallel: if two same-net track segments are found to be too close, check to see if there is ONE track segment connecting them. If that is the case, then it is the expected result. 
  • All other same-net track segments that are too close together = violation.

Track - Track

Example of Parallel Tracks with overlap:

Examples of Parallel Tracks without overlap: if the two tracks are connected by another primitive, the violation is invalid if it is in the connect area, as in the following examples:


Examples of Non-parallel Tracks: if the two tracks are connected by another primitive, the violation is invalid if it is in the connect area, as in the following examples:


If two tracks touch each other, the violation is invalid.

Track - Non-Track

Examples of Track-Non-Track: If the track centerline doesn't touch the non-track primitive and there is no connection between them, the violation is valid; otherwise the violation is invalid.


Non-Track – Non-Track

If the two primitives touch each other, the violation is invalid, otherwise the violation is valid.


Example of Same-Net Clearance Rule Set to 0.1mm 

In this example, the Same-Net Clearance Rule was set to 0.1mm. 


If you find an issue, select the text/image and pressCtrl + Enterto send us your feedback.

The features available depend on your Altium product access level. Compare features included in the various levels of Altium Designer Software Subscription and functionality delivered through applications provided by the Altium 365 platform.

If you don’t see a discussed feature in your software, contact Altium Sales to find out more.