Explanations of the PCB123 DRC Violation Types

PCB123 DRC Violation Types

All DRC categories reported by the Design Rule Checker in PCB123 are listed here, with either an explanation of what causes the error, or a description of how to resolve the error. At this writing, such information is not included in the PCB123 User’s Manual; look for it in future versions of the manual.



Spacing Conflicts:  when objects are placed on the circuit board too close to other objects with which they are incompatible.  Spacing requirements are set both by the physical demands of PCB manufacture and by the needs of the board’s designer.

Copper to copper:  all copper objects assigned to a net have a required spacing set within the net by which they must be separated from copper objects of other nets.  There are minimum clearances set by Sunstone for assured PCB fabrication.  Those minimum net-wide clearances can be extended by the customer based upon his/her own requirements.  For fine tuning of the copper to copper spacing requirement, the required copper clearance can be set on individual copper pours within the same net.  The DRCs use these values to report netted objects that are too close together.

Non-plated hole to copper:  to ensure that non-plated holes are not plugged with solder, Sunstone has a minimum spacing requirement for those holes from copper objects.  This minimum is exposed in each net for the customer to expand to the requirements of their project.  Additionally, this spacing requirement can be manipulated on an individual copper pour basis if the circuit board needs a finer tuned capability.  When the DRCs are run, any non-plated holes too close to copper objects based upon these spacing requirements will be reported as an error.

Copper object to board edge:  for manufacturability, Sunstone requires all objects to be at least 10 mils from the edge of the board (the outline and any of the board’s cutouts).  Copper objects violating this rule receive a DRC error.

Blowouts:  when drilled holes are positioned too close to other drilled holes on the circuit board.  This is a manufacturing minimum spacing requirement for proper fabrication.

Nonplated holes:  these must be no closer that 10 mils to eachother, circumference of hole to circumference of hole.

Pins with drilled holes:  these must be no closer that 17 mils to each other, measured from the outer extents of the drill’s circumference.  The required distance for plated through holes is wider because plated holes are drilled with larger drills.  The larger holes become smaller in diameter when plated.

Unrouted net connections:  when two or more objects of the same net have no conductive path to each other through objects or planes of the same net, the DRCs will report an error.  Unrouted net connections are believed by the design rule checker to be unintended open circuits.

Dangling traces:  when a routed track does not end at a pad, via, copper pour or at another routed track of the same net, the DRCs will emit a dangling trace warning.  Such traces may be intentional to provide an antenna effect, but the program reports a warning as a precaution.

Through hole pin pad annular rings:  the pad annular ring is the required minimum pin pad radius around the drilled hole that assures the drilled hole will be properly fabricated within the pad given that the drilling machine may not be able to register upon the exact center of  the location specified for the through hole.  The required annular ring is a function of the drilled hole size and the copper weight.  Generally, the greater the drill size and the greater the copper weight, the larger the pin pad’s annular ring must be to assure the drilled hole will not breakout of the outer circumference of the pin pad.  When a pin is discovered with an insufficiently large pad based upon Sunstone’s fabrication rules, it will report a DRC error.

Boardsize:  this DRC is intended to help the customer enforce the minimum and maximum sizes allowed for circuit boards manufactured from a design created in PCB123.

Objects outside the board outline:  any board object that is placed outside the board outline or which intersects it will be issued a DRC error.

Overlapping components:  the physical placement of a component from its footprint is determined in one of two ways:  1)  the extent of its pins and any geometric shapes drawn in silkscreen, or 2)  by a polygon drawn on an assembly layer that has a text property labeled “EXTENT”.  When a component’s extent is found to intersect another’s, an overlapping components DRC error is emitted.

Overlapping copper pours:  any copper polygons assigned to different nets that intersect will generate a DRC error indicating a short.  Additionally copper pours that have net assignments that are placed on plane layers will also cause a DRC error.

Non-plated holes:  any non-plated holes that have net assignments will cause a DRC error as will any non-plated hole that is too large for manufacturing to assure it will not become plated.

Plane layer net assignments:  all layers defined as plane layers that do not also have a net assignment get a DRC error.  A DRC warning is issued for plane layers that have multiple net assignments.

Pins isolated on copper pours:  when traces or other copper outline shapes of one net are drawn crossing filled copper polygons of another net, clearances are made by the software to separate those objects from the copper pour.  Should any of those clearances result in the copper pour becoming fragmented into two or more pieces, and if more than one piece of the resulting copper pour has pins within it assigned to the same net, a DRC error is emitted to alert the designer to a potential open circuit because there is no path within the copper pour that connects the two pins.