The size of the plane has less to do with noise introduction than the location of the plane relative to the signal paths.

You should think of every signal as a complete loop. The ground (or power) return side is as much a part of the signal path as the trace you normally think about. If you chose your ground (power) layout such that the analog return part of the loop is forced to pass through the digital signal area, you are likely to have digital noise introduced. If you chose common ground (power) copper areas that are shared by both analog and digital returns, you must look at the separation of the signal loops - you don't want digital signal current on the return side of the loop modulating the analog signal return (or vice-versa for that matter).

Your goal should be to provide the shortest return signal path, and to have the paths defined such that digital and analog loops are not restricted to sharing the same return path.

There are mathematical methods, software, etc. for doing simulations. However, you can use your finger and trace the signal loop in the layout - in most circuits, a good visualization of the signal loops will work as well for you as most of the fancy software and math.

I might add that the rule that inexperienced engineers frequently use without thought - to connect analog and digital grounds at a single point - is often the worst thing to do. The single point ground only works if no significant signal current is going to pass through the common connection point, or the impedance of the single point is negligible. Forcing digital and analog returns through a common point results in modulation across the impedance of the single pad/via/pin.

The short answer is - look at your signal loops; keep the appropriate ground or power return near / parallel to the critical signal paths; avoid forcing digital and analog loops through the same regions of copper. Only you can answer the question for your layout by looking at how you have placed your components, and where your sensitive signal loops are located. Hopefully, you have grouped your analog components away from the digital side - the situation of grounds will then naturally fall into two obvious logical groupings. Each of the two regions can then be properly routed to the appropriate supply/return.


At 03:09 AM 12/10/03, you wrote:
If a double-sided pcb has a very large DIGITAL GND net and a small ANALOG GND net would you connect the two GROUND planes created on the two layers to the DGND or AGND?

Connecting DGND would mean better current handling and thus presumably reduce digital noise but would the large plane then act as an transmitter to the AGND?
Connecting AGND would mean a cleaner audio path but would it then act as an aerial to all of the DGND nets on the board?


The application is an audio synth using, fundamentally, digital components (for the VCOs, Noise and controllers) but linear devices for the final audio paths (VCF, VCA and audio output).
snip



* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
*
* To leave this list visit:
* http://www.techservinc.com/protelusers/leave.html
*
* Contact the list manager:
* mailto:[EMAIL PROTECTED]
*
* Forum Guidelines Rules:
* http://www.techservinc.com/protelusers/forumrules.html
*
* Browse or Search previous postings:
* http://www.mail-archive.com/[EMAIL PROTECTED]
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

Reply via email to