Electrical Rule Types

The set of net objects returned by the rule scope can be further narrowed down using the drop-down at the top of the Constraints region (), in the following ways:

• Different Nets Only - constraint is applied between any two primitive objects belonging to different nets (e.g., two tracks on two different nets).

• Same Net Only - constraint is applied between any two primitive objects belonging to the same net (e.g., between a via and pad on the same net, or two track segments in the same net).

• Any Net - constraint is applied between any two primitive objects belonging to any net in the design. This is the most comprehensive of the three options and covers the possibility of the objects belonging to the same net, or different nets.

• Different Differential Pair - constraint is applied between any two primitive objects belonging to different nets of different differential pairs (e.g., a track in DiffPair1 and a track in DiffPair2). The rule does not apply between primitives in the two nets in the same differential pair (e.g., DiffPair1_P and DiffPair1_N). Use this constraint to configure the clearance between the differential pairs.

• Same Differential Pair - constraint is applied between any two primitive objects belonging to the different nets in the same differential pair (e.g., a track in TX_P and a track in TX_N). Use this constraint to configure the clearance when the nets in the differential pair must be closer together than allowed by the general clearance. Learn more about Differential Pair Clearance Checking.

  • If the constraints are defined in the Constraint Manager, the Connective Checking dropdown is only available in Advanced Rules (). This is because the tasks that the dropdown supports – targeting a specific sub-set of nets (such as Different Differential Pair (), or Same Net Only () – is performed in the grid region of the Constraint Manager.

  • When defining the constraints for the rule, the Connective Checking option would typically be set to Different Nets Only. An example of when Same Net Only or Any Net could be used to test for vias being placed too close to pads or other vias on the same net or any other net.

  • For a defined Same-Net Only Clearance rule, the general approach is that if two objects are touching (i.e. connected), then they are not deemed to be in violation of the rule. The exception to this is when checking the clearance between via and SMD pad objects in the same net. When a via and SMD pad have soldermask clearance, and the two are too close together, the soldermask bridge between the two objects can disappear and solder paste will flow down into the via during the soldering process, creating a bad solder joint on the SMD pad. Even if a via and SMD pad are connected with a trace or overlapping, they are deemed to be in violation when the distance between them is less than the Via-SMD Pad clearance in the Same-Net Clearance rule.

  • Configure the minimum distance allowed between a via and SMD pad by setting the Via-SMD Pad clearance in the Same-Net Clearance rule. If the via and SMD pad must touch or overlap, you also need to define a suitable Via Under SMD design rule (High Speed category) and enable the Allow Vias under SMD Pads constraint.

Provides the ability to fine-tune clearances between the various object-to-object clearance combinations in the design.

In the Minimum Clearance Matrix, the Simple mode is the default mode (). In the Advanced mode all objects are presented () (this is the traditional matrix).

• In the Simple mode, Track and Arc objects (including Track Keepout and Arc Keepout objects) are combined into the single Track entry. Fill, Poly, and Region objects (including Fill Keepout and Region Keepout objects) are combined into the single Copper entry.

• If you specify a clearance in Simple mode for a combined entry (Track and/or Copper), that value will be entered into the cells associated to those applicable non-combined objects when switching to Advanced mode. 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.

• In the Constraint Manager, Advanced mode in the matrix is only available if the rule is added as an Advanced Rule, in the All Rules page of the Constraint Manager ().

Definition of clearance values in the matrix can be performed in the following ways:

• Single-cell editing – to change the minimum clearance for a specific object pairing. Click on a cell to select it for editing.

• Multi-cell editing – to change the minimum clearance for multiple object pairings:

  • Use Ctrl+Click, Shift+Click, and Click+Drag to select multiple cells in a column.

  • Use Shift+Click, and Click+Drag to select multiple contiguous cells in a row.

  • Use Click+Drag to select multiple contiguous cells across multiple rows and columns.

  • Click on a row header to quickly select all cells in that row.

  • Click on a column header to quickly select all cells in that column.

• Applying edits – with the required selection made (either a single cell or multiple cells), making a change to the current value is simply a case of typing the new value required. To submit the newly entered value, either click away on another cell, or press Enter. All cells in the selection will be updated with the new value ().

• Switching back to a single value for all – to set a single clearance value for all possible object pairings, simply set the required value for the Minimum Clearance constraint. On clicking Enter, this value will be replicated across all applicable cells of the matrix. Alternatively, click the blank grey cell at the top-left of the matrix, or use the Ctrl+A shortcut. This selects all cells in the matrix, ready to accommodate a newly-entered value.

Tips on working with the matrix:

• The minimum clearance matrix applies irrespective of the connective checking method specified. If different clearances are required between objects on the same net, to those defined for objects on different nets, be sure to define separate clearance rules as required to suit.

• The applicable use of the clearance matrix depends on the rule scoping. For example, with scoping of ALL-ALL, all cells in the matrix are applicable (i.e. all possible object pairings). However, if scoping were set to IsVia-IsTrack, then only the single cell for the Via-Track object pairing would be applicable, and all other cells in the matrix would be left unused.

• While the DRC can test the clearance of any object kind to any object kind using any sort of rule scoping, the routing engines do not support this level of granularity. For example, the base clearance rule might require all tracks to have a clearance of 1 mm, with a higher priority rule requiring tracks greater than 10 mm in length to have a clearance of 2 mm. In this situation, the interactive routing engine will obey the base clearance rule, ignoring the higher priority, greater than 10 mm in length, rule. Another example is routing with arcs in corners. If the clearance rule specifies a higher clearance for arcs than for tracks, and you are interactively routing with arcs in the corners, the interactive routing engine will ignore the arc setting and obey the track setting, placing the corner arcs to have the same clearance as the track segments. In both of these examples, as soon as routing is completed, the Online DRC will flag those situations as violations.

• When defining a clearance rule for a polygon, it is the primitives of the polygon that the rule is actually applied to rather than the polygon itself. The keyword entry InPolygon (or InPoly) should be included in the Full Query in this case instead of IsPolygon (or IsPoly). The specific polygon clearance rule must also be given a higher priority than any general clearance rule if it is to have any effect.

• Same-net clearance constraints are considered when pouring polygons around other objects of the same net. In this case, the pouring behavior depends on the Pour Over Same Net option selected for polygons. Also, Design Rule Checking (DRC) observes such constraints. Refer to the Polygons on Signal Layers page to learn more.

Designers can check clearances between the edges of drill holes and neighboring copper objects on signal layers. This is particularly beneficial in preventing the routing of track too near to a drilled hole, which could otherwise suffer from potential wandering of the drill during board fabrication. The row at the bottom of the Clearance rule's minimum clearance matrix is used to define the desired clearances (). Set clearance values to catch any copper objects in the design that are too close to the edges of drill holes.

This rule can also check 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 Split Plane (<NetName>) on <InternalPlaneLayerName> And Split Plane (<NetName>) on <InternalPlaneLayerName>,

for example ():

Clearance Constraint: (32.36mil < 34mil) Between Split Plane (GND) on Internal Plane 1 And Split Plane (NetC6) on Internal Plane 1

Differential pairs present unique design challenges, often requiring a specific within-pair clearance as well as a pair-to-pair clearance, and potentially a third rule to control the pair-to-all other nets, clearance. To support this, the Constraints region includes the dropdown where you can choose Same Differential Pair and Different Differential Pair options.

• For example, if the nets within the differential pairs require a tighter clearance than the general board clearance, this can be achieved by using the Same Differential Pair constraint option (). Note that even though the rule scope applies to All net objects in the design, the Constraint setting restricts it to only apply to objects in the Same Differential Pair.

• This result could also be achieved by scoping the rule to only apply to differential pair objects (e.g., InAnyDifferentialPair) (). Note that this rule would also apply between a net in a differential pair to any other net object in the design, so this approach should only be used if you have other higher priority rule(s) that define the DiffPairNet-to-DiffPairNet and/or DiffPairNet-to-Any requirements. If this approach is used, the Priority of the differential pair rules must also be configured correctly, with the rule with a tighter clearance requirement having a higher priority.

• A similar approach can be used to control the clearance between differential pairs, using the Different Differential Pair constraint ().

• As with the previous example, it could also be achieved using the rule scope, instead of the Different Differential Pairs constraint (). Remember that the rule priorities must be configured so the rule with the tighter clearance requirement has a higher priority.

• To define a different clearance from a differential pair net to any other net object, use the InAnyDifferentialPair query in combination with the Different Nets Only constraint setting (). This could be further refined so that it only applies between differential pair objects and non-differential pair objects by including the Not operator ().

Learn more about Differential Pair Routing. Learn more about scoping Differential Pair design rules.

By default, clearance checking applies to all layers in the design. If the design constraints are defined in the Constraint Manager, the clearance can also be constrained by layer ().

• Click the appropriate tab to constrain by Inner Layer or Outer Layers.

• Or use the +Add link to add a specific copper layer (). Note that the values in the All Layers tab will update to reflect the range of all settings across all of the layer tabs ().

• When using the Dielectric Shapes Generator (in Printed Electronics) in Auto mode, the dielectric shape is automatically expanded to satisfy the requirement of the applicable Clearance Constraint design rule.

• In Printed Electronics, net-to-net clearances are tested on all layers, not just the same layer.

Online DRC, Batch DRC, interactive routing, autorouting, and polygon placement.

This rule tests the completion status of each net that falls under the scope (full query) of the rule. If a net is incomplete then each completed section (sub-net) is listed along with the routing completion. The routing completion is defined as:

(connections complete / total number of connections) x 100

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

• Track/Arc to Track/Arc – check that the centerlines, or centers of the ends of the connecting track/arc segments, coincide.

• Track/Arc to Via – check that the centerline, or center of the end of a track/arc segment, is placed on the shape of the via.

• Track/Arc to Pad – check that the centerline, or center of the end of the track/arc segment, is placed on the shape of the pad.

• Via to Pad – check that the center of the via is placed on the shape of the pad.

• Via to Via – check that the center of one via is placed on the shape of another via.

• Polygon to Track/Arc – check that the centerline, or center of the end of a track/arc segment, is overlapped by the polygon.

• Polygon to Pad/Via – check that the center of the Pad/Via is overlapped by the polygon when the Pad/Via uses a direct connection to the polygon.

• A poor connection is flagged using the detailed violation marker, , with a corresponding message appearing in the Messages panel.

• Where applicable, a connection line will be drawn between unconnected objects in the net, with data regarding the un-routed net length reflected in the PCB panel (in Nets mode).