Henry Ott Consultants

Part 6. Return Path Discontinuities

One of the keys in determining the optimum printed circuit board layout is to understand how and where the signal return currents actually flow.  Most designers only think about where the signal current flows (obviously on the signal trace), and ignore the path taken by the return current.  Of course, the fact that many designers think this way helps to keep EMC engineers employed

To address the above concern we must understand how high-frequency currents flow in conductors.  First, the lowest impedance return path is in a plane directly underneath the signal trace (irrespective of whether this is a power or ground plane) since this provides the lowest inductance path.  This also produces the smallest current loop area possible.  Secondly, due to the "skin effect," high frequency currents cannot penetrate a conductor, and therefore, at high-frequency all currents in conductors are surface currents.  This affect will occur at all frequencies above 30 MHz for 1 oz. copper layers in a PCB.  Therefore, a plane in a PCB is really two conductors not one conductor.  There will be a current on the top surface of the plane, and there can be a different current or no current at all on the bottom surface of the plane.

A major EMC problem occurs when there are discontinuities in the current return path.  These discontinuities cause the return current to flow in larger loops, which increases the radiation from the board as well as increases the crosstalk between adjacent traces and causes waveform distortion. In addition in constant impedance PCBs the return path discontinuity will change the characteristic impedance of the trace.  The most common return path discontinuities are discussed below.
 

Slots in Ground/Power Planes.  When a trace crosses a slot in the adjacent power or ground plane, the return current is diverted from underneath the trace in order to go around the slot. This causes it to flow through a much bigger loop area.  The longer the slot the bigger the loop area becomes. The most important thing that I can say about slots in ground planes, is don't have them!  If you do have slots, make sure that no traces cross over them on adjacent layers.

If you absolutely must route a signal across a power or ground plane slot, place a few small stitching capacitors across the slot, one on either side of the trace (0.001 or 0.01 uF should be adequate).  This will provide high-frequency continuity across the slot for the return current.  To be effective the capacitors should be located within 0.1" of the trace.

For more information on slots in power/ground planes see our Tech Tip, Slots in Ground Planes.
 

Split Ground/Power Planes.  When a trace crosses a split in the adjacent plane, as in the 4-layer board example shown below, the return current path is interrupted.  The current must find another way to get across the split, which forces it to flow in a much bigger loop.
 
 

 __________________------------>_I_____________________Signal Trace

 _____I <--------------______             _____I_<------------____Split Power Plane

 ____________________I <------------____________________Solid Ground Plane

 ___________________________________________________Signal Trace

The best solution to this problem is to avoid crossing split planes with critical signal traces.  In the case of the above example the signal should have been routed on the bottom signal layer since that was adjacent to the solid ground plane.

If you absolutely must route the signal across the split plane, place a few small stitching capacitors across the split, one on either side of the trace.  This will provide high-frequency continuity across the split while maintaining dc isolation between the isolated sections of the split plane.  The capacitors should be located within 0.1" of the trace and have a value of 0.001 to 0.01 uF according to the frequency of the signal.  This is far from an ideal solution, however, since the return current must now flow through a via, a trace, a mounting pad, a capacitor, a mounting pad, a trace, and finally a via to the other section of the split plane.  This adds considerable additional inductance in the return path (5 to 10 nH minimum).

If in the above example both the power and ground planes are split, you are really in trouble.  I leave it to you to figure out how the current gets across the split plane boundary.  In some instances it may have to go all the way back to the power supply.  If you have a split power and split ground plane the only acceptable solution may be to make sure that no signal traces cross the split plane boundary.

For additional information on split planes see our Tech Tip on Grounding of Mixed Signal PCBs.
 

Changing Reference Planes.  When a signal trace changes from one layer to another on a PCB, the return current path is interrupted since the return current must also change reference planes (see right hand figure below).  The question then becomes how does the return current get from one plane to another?  As was the case for the split planes mentioned above the interplane capacitance is not usually large enough to be effective, so the return current will have to flow through the nearest decoupling capacitor in order to change planes.  This obviously increases the loop area and is undesirable for all the reasons previously stated.  One solution to this problem is to avoid switching reference planes for critical signals (such as clocks), if at all possible.  If you must switch the return path from a power plane to a ground plane you should place an additional decoupling capacitor adjacent to the signal via in order to provide a high-frequency current path between the two planes for the signal return current.  This is not an ideal solution, however, since the return current must now flow through a via, a trace, a mounting pad, a capacitor, a mounting pad, a trace, and finally a via to the other  plane.  This adds considerable additional inductance in the return path (typically 5 to 10 nH).

Note, that if the two reference planes are of the same type (either both power, or both ground) you can put a via (ground to ground or power to power) instead of a capacitor immediately adjacent to the signal via.  This is a much better solution than  using  a capacitor to connect the planes together, since the added inductance in the return path will be considerably less.
 

Referencing the Top and Bottom of the Same Plane.  Whenever a signal switches layers and references first the top and then the bottom of the same plane we must still ask the question, how does the return current get from the top to the bottom of the plane.  Do to the "skin effect" the current cannot flow through the plane, it can only flow on the surface of the plane.

In order to drop a signal via through a plane a clearance hole must be provided in the plane, otherwise the signal would be shorted to the reference plane.  The clearance hole provides a surface connecting the top and bottom of the plane and provides a path for the return current to flow from the top to the bottom of the plane (see left hand figure).  Therefore, when a signal passes through a via and continues on the opposite side of the same plane a return current discontinuity does not exist.  This is, therefore, the preferred way to route a critical signal if two routing layers must be used.
 

Summary.  High-Speed clocks and other critical traces should be routed (in order of preference):

1. On only one layer adjacent to a plane.
2. On two layers that are adjacent to the same plane.
3. On two layers adjacent to two separate planes of the same type (ground or power) and connect the planes together with vias wherever the signal changes planes.
4. On two layers adjacent to two separate planes of different types (ground and power) and connect the planes together with capacitors wherever the signal changes reference planes.
 

Avoid routing clocks or other critical traces across slots or splits in the adjacent plane.  The above guidelines are important for all PCBs carrying high-frequency signals, but are critically important in the case of boards with constant impedance transmission lines.

If you follow the guidelines presented in this series of articles, with respect to layer stack-up and the avoiding of return current discontinuities, you will produce better PCBs and avoid many of the most common EMC problems associated with boards.  It will not guarantee you a perfect PCB layout but it will go a long way towards reducing the emission, increasing the immunity, and improving the signal quality of your boards.
 

© 2002 Henry W. Ott                                                Henry Ott Consultants,  48 Baker Road  Livingston,  NJ  07039  (973) 992-1793

Return to top of page.

Return to HOC home page.