Design Rules Improvements (New Feature Summary)

Created: May 11, 2016 | Updated: December 14, 2017

Altium Designer 17.0 brings with it a number of enhancements to PCB Design Rules. From simplification of the minimum clearance matrix, and the ability to check clearances between split planes, to hole-to-primitive clearance checking, and checking for bad connections as part of the Un-Routed Net rule, these improvements collectively enhance your ability to constrain your board designs exactly as needed.

Clearance Rule Enhancements

The following enhancements have been implemented for the Clearance rule.

Simplified Clearance Matrix

For many users, there is no great difference between Track and Arc primitives. And when it comes to Fill, Region, and Polygon objects, most users just see these as more 'copper'. With this in mind, the minimum clearance matrix for the Clearance rule has been enhanced to operate in two modes:

  • Simple - in this mode, Track and Arc objects are combined into the single Track entry. Fill, Poly, and Region objects are combined into the single Copper entry.
  • Advanced - this mode is the traditional matrix, present in previous versions of the software, with all objects presented.

Simplifying the objects involved in the minimum clearance matrix by introducing a Simple mode.
Simplifying the objects involved in the minimum clearance matrix by introducing a Simple mode.

Aspects of the feature to be aware of:

  • The Simple mode is the default mode, regardless of whether opening an existing design or a new design.
  • If you specify different clearances for the individual objects in Advanced mode, then the maximum clearance value from the cells associated to those applicable non-combined objects will be used for the combined entries (Track and/or Copper) in Simple mode.
  • If you specify a clearance for a combined entry (Track and/or Copper) in Simple mode, that value will be entered into the cells associated to those applicable non-combined objects when switching to Advanced mode.

Ignore Pad-to-Pad Clearances in a Footprint

Streamlining DRC and reducing the clutter of error markers flagging violations that are not real, an option has been added to the Clearance rule's constraints that allows you to specify that clearances between pads in the same component footprint be ignored. This option - Ignore Pad to Pad clearances within a footprint - is disabled by default.

Prevent violations associated to pad clearances within the same component footprint, with the option to ignore such clearances.
Prevent violations associated to pad clearances within the same component footprint, with the option to ignore such clearances.

Hole-to-Object Clearance Checking

Adding another element to its clearance checking capabilities, Altium Designer 17.0 brings the ability to check clearances between the edges of drill holes and neighboring copper objects on signal layers. An additional row is now available at the bottom of the Clearance rule's minimum clearance matrix with which to define the desired clearances. This is particularly beneficial in preventing the routing of track too near to a drilled hole, which could otherwise suffer from any potential wandering of the drill during board fabrication.

Set clearance values to catch any copper objects that are too close to the edges of drill holes in the design.
Set clearance values to catch any copper objects that are too close to the edges of drill holes in the design.

For the default Clearance rule, all cells for the Hole row of the matrix will have the vaule 0. Similarly, when saving the PCB in a previous version of the software (that does not support Hole-to-Object clearance checking) any defined Hole-to-Object clearances will be lost, and when the file is opened again in Altium Designer 17.0, all cell entries will be set to 0.

Split Plane Clearance Checking

The Clearance rule in Altium Designer 17.0 also now supports checking of clearances between split plane regions on internal plane layers. How clearance is defined depends on the mode in which you are using the minimum clearance matrix:

  • Simple mode - specify the required split plane-to-split plane clearance value using the Copper-Copper cell.
  • Advanced mode - specify the required split plane-to-split plane clearance value using the Region-Region cell.

A violation will appear in the form:

Clearance Constraint: (<CurrentClearance> < <DefinedClearance>) Between Polygon Region (<NumberOfHolesinRegion1> hole(s)) <InternalPlaneLayerName> And Polygon Region (<NumberOfHolesinRegion2> hole(s)) <InternalPlaneLayerName>,

for example:

Clearance Constraint: (20.173mil < 34mil) Between Polygon Region (0 hole(s)) Internal Plane 1 And Polygon Region (1 hole(s)) Internal Plane 1

Clearance checking between split plane regions on an internal layer. In this case, the clearance value of 34mil has been entered in the Region-Region cell, as clearances

are being defined using the Advanced mode of the matrix.
Clearance checking between split plane regions on an internal layer. In this case, the clearance value of 34mil has been entered in the Region-Region cell, as clearances
are being defined using the Advanced mode of the matrix.

Un-Routed Net Rule Enhancement

The PCB Editor's Design Rule Checking system typically sees a net as being routed if all nodes in that net (component pads) are connected through the use of net-aware design objects (tracks, arcs, pads, vias, polygons). These objects are considered connected if they touch each other. However, while simply touching makes a perceived connection to the software, when it comes time to fabricate the board, the fragility of some of these 'connections' can cause critical issues, especially where the objects - for example two contiguous track segments or a track entering a pad/via - are only slightly touching. Such connections are often referred to as 'Bad Connections,' 'Poor Connections,' or 'Incomplete Connections.'

In Altium Designer 17.0, enhanced checking for the existence of such fragile connectivity is available, courtesy of the Check Incomplete Connections option - a new constraint of the Un-Routed Net rule.

With this option enabled, the following additional checks on connectivity between applicable design objects are made:

  • Track/Arc to Track/Arc - checking that the centerlines, or centers of the ends of the connecting track/arc segments, coincide.
  • Track/Arc to Via - checking that the centerline, or center of the end of a track/arc segment, is placed on the center of the via.
  • Track/Arc to Pad - checking that the centerline, or center of the end of the track/arc segment, is placed on the shape of the pad.
  • Via to Pad - checking that the center of the via is placed on the shape of the pad.
  • Via to Via - checking that the centers of the two vias coincide.
  • Polygon to Track/Arc - checking that the center of the end of a track/arc segment is overlapped by the polygon.
  • Polygon to Pad/Via - checking that the center of the Pad/Via is overlapped by the polygon.

A poor connection will be flagged in the workspace using the detailed violation marker, , with a corresponding message appearing in the Messages panel. As before, and where applicable, a connection line will be drawn between unconnected objects in the net, with data regarding the Unrouted net length reflected in the PCB panel (in Nets mode).

Catch poor connections in your designs as part of the enhanced Un-Routed Net rule.
Catch poor connections in your designs as part of the enhanced Un-Routed Net rule.

Power Plane Connect Style Rule Enhancement

The Power Plane Connect Style rule has been given two modes of operation in Altium Designer 17.0:

  • Simple - this mode is the generic setting for how pads/vias connect to a power plane, as present in previous versions of the software.
  • Advanced - in this mode, you have the ability to define specific thermal connections for pads and vias separately.

Roll the mouse over the image to compare the two modes available.
Roll the mouse over the image to compare the two modes available.

Aspects of the feature to be aware of:

  • The Simple mode is the default mode, for a newly created rule of this type.
  • After setting and applying constraints in Advanced mode, be aware that switching back to Simple mode is considered a modification - clicking Apply or OK will effect the simple definition, overriding the individual advanced definitions specified previously.

Polygon Connect Style Rule Enhancement

The Polygon Connect Style rule has also been given two modes of operation in Altium Designer 17.0:

  • Simple - this mode is the generic setting for how pads/vias connect to a polygon pour, as present in previous versions of the software.
  • Advanced - in this mode, you have the ability to define specific thermal connections for thru-hole pads, SMD pads, and vias, separately.

Roll the mouse over the image to compare the two modes available.
Roll the mouse over the image to compare the two modes available.

Aspects of the feature to be aware of:

  • The Simple mode is the default mode, for a newly created rule of this type.
  • After setting and applying constraints in Advanced mode, be aware that switching back to Simple mode is considered a modification - clicking Apply or OK will effect the simple definition, overriding the individual advanced definitions specified previously.

Additional Enhancements

 

Found an issue with this document? Highlight the area, then use Ctrl+Enter to report it.

Contact Us

Contact our corporate or local offices directly.

We're sorry to hear the article wasn't helpful to you.
Could you take a moment to tell us why?
200 characters remaining
You are reporting an issue with the following selected text
and/or image within the active document: