[SI-LIST] Re: Traces don't cause EMI - really?
- From: Aubrey_Sparkman@xxxxxxxx
- To: leeritchey@xxxxxxxxxxxxx, MikonCons@xxxxxxx, weirsp@xxxxxxxxxx
- Date: Mon, 2 Feb 2004 12:40:26 -0600
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:
> //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:
> //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:
//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:
//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:
