joe,

We work with EMI a little.  I hope these suggestions help.  If you
would like more explanation please let me know.  If this information
is already known, then I apologize.

1. planes should be on layer n-1, that is on a 10 layer board
   move the planes to layers 2, and 9.  This will shield the internal
   layers 3 thru 8. 
      - If you have a dense board with lots of vias, you may also
        consider using 2 oz copper for the planes.
      - If the planes are currently next to each other on the internal
        layer, the coupling or capacitance may be a concern.  Some board
        manufacturers offer buried capacitance.  Please let me know
        if you need an explanation or any other info.

2. Get with your design engineer and discuss termination for ALL clock
   signals.  No matter how short the trace is, Clocks are the biggest 
   source for radiation, and termination will help much.
      - my suggestion for termination would be AC termination on a 
        trace which is daisy chained.  AC termination is a series 
        resistor, and cap to ground at the end of the trace, near the
        last input pin. 

3. The termination makes a big difference in the radiation, but it is
   also important to route the siganl on the internal layers as much as 
   possible.  Again this will take advantage of the planes acting as 
   shields.

4. Also try designing with impedance in mind.  Though for most 
   frequencies simply specifying the dielectric thickness, and routing
   with the proper trace width is enough.  All the board shops I know will
   do an impedance calculation, and can provide you with a suggested 
   dielectric thickness and trace width.  The impedance should match the 
   input impedance of the receiver ICs.  I suggest you request the impedance 
   calculation from the board shop which will fab the board, you may find 
   the results change slightly from board shop to board shop. To the best of
   my knowledge, the change in the answers to the impedance calculation are 
   due to variables in materials, prepreg selections, and etc from one shop
   to the next.
      - In this case, you may provide the trace width, and impandance to 
        the board shop, and ask for the dielectric thickness.        

5. Finally, adding a copper pour to your outer layers will also help to 
   shield EMI, but it is important that there is NO floating copper.
   Make shure ALL your copper pour is connected to ground.

6. Eliminate ALL 90 degree angles on traces, and planes.  All 90 degree 
   angles radiate, it is important to run your clean up utilities if you
   haven't already.  Also consider the planes as capable of radiation
   especially at higher frequecies, so 45 all the corners.

I do not know how much time you have to make changes, but please choose
the suggestions which make the most sense for your circumstances.

joez
-----------------------------------------------------------------
 Joseph Zdybowicz                      FORE Systems
 CAD Engineer                          174 Thorn Hill Road
 Email:   [log in to unmask]                Warrendale, PA 15086-7586
 Direct:  412-772-6552                
-----------------------------------------------------------------



>                                _\\|//_ 
>                               (` O-O ')
> +==========ooO-(_)-Ooo=============================+
> Need help with EMI !
> 
> EMI emissions problem !
> What would be the best solution to reduce EMI on a ten layer board,
> surface
> mount components on both sides, 6 or 8 mil space/trace ?  Anyone with
> experience in this area ?
>   
> Telxon Corporation
> Principle PC Designer
> Joe Gee
> Email: [log in to unmask]
> 
> ****************************************************************************
> * The mail list is provided as a service by IPC using SmartList v3.05      *
> **************************************************************************** 
> * To unsubscribe from this list at any time, send a message to:            *
> * [log in to unmask] with <subject: unsubscribe> and no text. *
> ****************************************************************************
> 
> 

****************************************************************************
* The mail list is provided as a service by IPC using SmartList v3.05      *
**************************************************************************** 
* To unsubscribe from this list at any time, send a message to:            *
* [log in to unmask] with <subject: unsubscribe> and no text. *
****************************************************************************