Re: [SI-LIST] : effect of trace width on the performance

About this list Date view Thread view Subject view Author view

From: Muhammad S. Sagarwala (msagarwa@san-jose.tt.slb.com)
Date: Wed Nov 01 2000 - 09:35:03 PST


Here is the board stackup...

--------------- Top layer with all the active componenets
--------------- Ground layer
--------------- Vdd1 layer
--------------- Ground layer
--------------- Vdd2 layer
--------------- Ground layer
--------------- Signal Layer
--------------- Ground layer
--------------- Signal layer
--------------- Ground layer
--------------- Signal layer
--------------- Ground layer
--------------- Signal layer
--------------- Ground layer
--------------- Bottom layer (with decoupling caps and other discretes)

Just to sum it up.. there are two power layers pretty close to the device.
All the signals are routed as strip lines. The decoupling caps were placed on the bottom
side of the board because of space limitations on the top side. All the decoupling
caps are x7r (dielectric).

The layer stackup (arrangement) is exactly the same for both boards. The difference
is the thickness of the boards. Since traces on both boards are 50 ohms characteristic
impedence but since one board has 9 mil wide traces while the other has 7.5 mil
wide traces therefore the board with 9 mil wide traces is thicker. Also the board with
9 mil wide traces has 1 oz copper on all power/ground planes.

The reason I suspect ground bounce is the culprit in this case

(1) since we followed the same routing rules on both boards so cross talk could not be an issue
     (because if it were, we would see it in the first board i.e. the one with 9 mil wide traces)
(2) since the boards are made of Cynate Ester (loss tangent very low)...I do not think dielectric losses are a major
     problem.
(3) one of the tests that we performed was to operate the devices near the Vil threshold. We found that the board with
     9 mil wide traces and 1oz. power planes had no problems while the board with 7.5 mil wide traces did not work.

I hope this clarifies everything....

Muhammad
    

*

    -----Original Message-----
    From: Scott McMorrow <scott@vasthorizons.com>
    To: Muhammad S. Sagarwala <msagarwa@san-jose.tt.slb.com>
    Date: Wednesday, November 01, 2000 9:12 AM
    Subject: Re: [SI-LIST] : effect of trace width on the performance
    
    
    Muhammad,
    It would be helpful to the group if you were to provide a picture of
    the before and after of the stackups. It seems that we are all guessing
    about what your configuration really is at this time. I would also include
    the location of all ground and power planes.

    Also, a list of all things which have changed from the previous fab
    to this one would be helpful. This way we can eliminate possible
    causes of your problem.

    Finally, why do you think it is a ground bounce problem?
    Do you have root cause for your failures?

    regards,

    scott
      

    --
    Scott McMorrow
    Principal Engineer
    SiQual, Signal Quality Engineering
    18735 SW Boones Ferry Road
    Tualatin, OR 97062-3090
    (503) 885-1231
    http://www.siqual.com
      
      

    "Muhammad S. Sagarwala" wrote:

         Thanks a lot for your input Mike... The stackup is the same but the dielectric thickness is different...I mean the arrangement of the planes is the same but the thickness of thedielectric (and hence the boards is different).. The lengths of the traces on these boards is between 7-10 inches. One more question...I am suspecting ground bounce....do you think that copper weight and trace widths could play a major role... Muhammad
            -----Original Message-----
            From: Michael Nudelman <mnudelman@tellium.com>
            To: Muhammad S. Sagarwala <msagarwa@san-jose.tt.slb.com>
            Cc: si-list@silab.eng.sun.com <si-list@silab.eng.sun.com>
            Date: Wednesday, November 01, 2000 6:18 AM
            Subject: Re: [SI-LIST] : effect of trace width on the performance
             Muhammad:
            1. If your stackup is the same (dielectr. thicknesses etc) - then how does the impedance stays the same with traces' widths changed? (if it is different, than it is possible.)
            2. How long are the traces? In case of 7.5 mils your skin effect losses increase and at certain lengths they may impaire your signal quality.
            3. The pwr plane copper oz are not that important. Or at least I think so :-)))

            Mike.

            "Muhammad S. Sagarwala" wrote:

                 Hi SI Gurus, I am in a big problem. I designed two boards which are pretty much the same.The changes between them are: (1) One has traces that are 7.5 mils wide and the other has 9 mils wide traces (both have a characteristic impedence of 50 ohms)(2) The one that has 9 mil wide traces has 1 oz copper for the pwr planes and the one with 7.5 mil wide traces has 0.5 oz. copper on pwr planes. The stackup is pretty much the same.The Frequency of signals on the boards is 400 Mhz.The decoupling scheme on both boards is pretty much the same. The problems is the board with 9 mil wide traces and 1oz. copper is performing very good and the other board with 7.5 mil widetraces and 0.5 oz. copper is behaving very very bad. My question is "do you think these changes make a big difference or is there another variable(s) that I am missing?????" Comments suggestions are most welcome....(I need to be sure before I make a decision to respin the board ) Muhammad Muhammad S. Sagarwala
                Schlumberger SABER
                Ph. (408) 586 7065
                Fax (408) 586 4668
    
      

**** To unsubscribe from si-list or si-list-digest: send e-mail to
majordomo@silab.eng.sun.com. In the BODY of message put: UNSUBSCRIBE
si-list or UNSUBSCRIBE si-list-digest, for more help, put HELP.
si-list archives are accessible at http://www.qsl.net/wb6tpu
****


About this list Date view Thread view Subject view Author view

This archive was generated by hypermail 2b29 : Tue May 08 2001 - 14:29:57 PDT