[SI-LIST] Re: Traces don't cause EMI - really?

Actually, the thickness depends on where you measure it; thinner (~.5 mils)
on top of the trace and much thicker between traces.  Between trace
thickness varies with trace pitch and can easily be as much as trace
thickness + thickness on top of the trace.  

Aubrey Sparkman 
Enterprise Engineering Signal Integrity Team 
Dell, Inc. 
Aubrey_Sparkman@xxxxxxxx 
(512) 723-3592


> -----Original Message-----
> From: si-list-bounce@xxxxxxxxxxxxx
> [mailto:si-list-bounce@xxxxxxxxxxxxx]On Behalf Of Lee Ritchey
> Sent: Monday, February 02, 2004 10:37 AM
> To: MikonCons@xxxxxxx; weirsp@xxxxxxxxxx
> Cc: si-list@xxxxxxxxxxxxx
> Subject: [SI-LIST] Re: Traces don't cause EMI - really?
> 
> 
> Actually, present day soldermasks are rarely more than 0.5 
> mils thick and the er is on the order of 3.  The impact on 
> impedance is quite small.
> Lee
> 
> 
> ----- Original Message ----- 
> From: 
> To: weirsp@xxxxxxxxxx;leeritchey@xxxxxxxxxxxxx
> Cc: si-list@xxxxxxxxxxxxx
> Sent: 2/2/2004 8:18:46 AM 
> Subject: Re: [SI-LIST] Re: Traces don't cause EMI - really?
> 
> 
> Steve:
> 
> You (and Lee) are absolutely correct that techniques have 
> changed (for the better), and indeed a "buried microstrip" 
> will reduce the radiated emissions relative to a surface 
> microstrip. I also use that technique when appropriate. The 
> tests I referred to only had a soldermask thickness of ~3 
> mils, but the relative dielectric constant was ~5.5. The 
> present day soldermasks tend to fall in the 1.5-2.0 mil 
> thickness and have an Er value of ~3.5, which would worsen 
> the test results I obtained for surface microstrips.
> 
> Equally important is the placement of surface high-speed 
> traces in-board of the PCB edges. As much as 20 dB reduction 
> in emissions can be achieved relative to traces very near 
> (<50 mils) to the PCB edges. My tests were of traces in-board 
> by more than 500 mils; therefore, the results would have been 
> far worse for traces near the PCB edges.
> 
> Note that these not so obvious details are critical to 
> achieving acceptable performance as Lee has reported. Again, 
> my concern is that less experienced designers will ignore the 
> radiation potential of surface traces and fail to meet 
> regulatory requirements without a respin of the PCB.
> 
> 
> 
> Mike
> 
> Michael L. Conn
> Owner/Principal Consultant
> Mikon Consulting
> 
> 
> *** Serving Your Needs with Technical Excellence ***
> 
> ------------------------------------------------------------------
> To unsubscribe from si-list:
> si-list-request@xxxxxxxxxxxxx with 'unsubscribe' in the Subject field
> 
> or to administer your membership from a web page, go to:
> http://www.freelists.org/webpage/si-list
> 
> For help:
> si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field
> 
> List technical documents are available at:
>                 http://www.si-list.org
> 
> List archives are viewable at:     
>               http://www.freelists.org/archives/si-list
> or at our remote archives:
>               http://groups.yahoo.com/group/si-list/messages
> Old (prior to June 6, 2001) list archives are viewable at:
>               http://www.qsl.net/wb6tpu
>   
> 

------------------------------------------------------------------
To unsubscribe from si-list:
si-list-request@xxxxxxxxxxxxx with 'unsubscribe' in the Subject field

or to administer your membership from a web page, go to:
http://www.freelists.org/webpage/si-list

For help:
si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field

List technical documents are available at:
                http://www.si-list.org

List archives are viewable at:     
                http://www.freelists.org/archives/si-list
or at our remote archives:
                http://groups.yahoo.com/group/si-list/messages
Old (prior to June 6, 2001) list archives are viewable at:
                http://www.qsl.net/wb6tpu

Other related posts: