Grounding of Mixed Signal PCBs

Grounding of Mixed Signal PCBs

A question that I hear often is:  How do I prevent digital logic ground currents from contaminating my low level analog circuitry?  This is a good question without a simple answer.  Most A/D converter manufacturer's data books and application notes provide little if any useful information on the subject.  If they do provide information, it is usually only applicable to a simple system containing only one A/D converter.

Some people suggest splitting the ground plane in order to isolate the digital ground currents from the analog ground currents.  Although the split plane approach can be made to work, it has many potential problems especially in large complicated systems.  Can you list some of these problems?  One of the major ones is that you can not route a trace over the split in the plane (see Tech Tip Slots in Ground Planes).It is always better to have only a single reference plane for a system.

If you do split the ground plane and run traces across the split (left hand figure below), there will be no return path near the trace and the current will have to flow in a big loop.  Current flowing in big loops produce radiation and high ground  inductance. If you must split the ground plane and run traces across the split, you should do it as shown in the right hand figure below.  By connecting the planes together at one point (a bridge) and routing all the traces so that they cross at this bridge point, you will have provided a return path for the current directly underneath each of the traces (hence a very small loop area).

High frequency digital ground return currents want to return directly underneath the signal trace.  This is the lowest impedance (lowest inductance) path.  The digital ground currents have no desire to flow through the analog portion of the ground plane and corrupt your analog signal.  Why then do we need to split the ground to prevent the digital current from doing something that it does not want to do anyhow?  Therefore, I prefer the approach of using only one ground plane and partitioning the PCB into digital and analog routing sections.  Analog signals can then  be routed only in the analog section of the board (on any layer), and digital signals can  be routed only in the digital section of the board (on any layer).  What causes problems is when a digital signal is routed in the analog section of the board, or visa versa.

A PCB with a single ground plane, partitioned into analog and digital sections, and discipline in routing the signals can usually solve an otherwise difficult layout problem, without creating the additional problems caused by  a split ground plane.  If the layout is done properly, the digital ground currents will remain in the digital section of the board and will not interfere with the analog signals.  The routing, however, must be checked carefully to assure that the above mentioned routing restrictions are adhered to one hundred percent!   The key to a successful mixed signal PCB layout, therefore, is proper partitioning and routing discipline, not a split ground plane.

Many A/D converter manufacturers, while suggesting the use of split ground planes, state the following in their data sheets or application notes:  "The AGND and DGND pins must be connected together externally to the same low impedance ground plane with minimum lead length.  Any extra external impedance in the DGND connection will couple more digital noise into the analog circuit through the stray capacitance internal to the IC."  Their recommendation is to connect both the AGND and the DGND pins of the A/D converter to the analog ground plane.  This approach has the potential of creating a number of additional problems.  Can you list some of these problems?  What do you connect the ground side of the digital power decoupling capacitor to?  The analog plane or the digital plane?

A much better way to satisfy the requirement of connecting AGND and DGND pins together through a low impedance, and not create additional problems in the process, is to use only one ground plane to begin with.

The key to deterring the optimum board layout is to think, how and where do the return currents flow?

If you are still skeptical about using a single ground plane on your mixed signal boards I suggest you do the following experiment.  Layout the board with a split ground plane, but provide means for connecting the two planes together every 1/2 inch with jumpers or zero ohm resistors.  Route the board properly, with no digital traces (on any layer) over the analog plane and no analog traces (on any layer) over the digital plane. Build the board and test it's  functionality and EMC performance.  Connect the planes together and test the board again for functionality and EMC performance.  I think that you will find that in almost all cases, both the functional performance and the EMC performance of the board will be better with the single ground plane.  If you do the experiment  send me an e-mail letting me know of your results.

It is almost always better to have only a single reference plane for a system!

Summary:

• Partition your PCB with separate analog and digital sections.
• Do not split the ground plane.  Use one solid ground plane under both analog and digital sections of the board.
• Route digital signals only in the digital section of the board.  This applies to all layers.
• Route analog signals only in the analog section of the board.  This applies to all layers.
• The key to a successful PCB layout is the use of routing discipline.