[SI-LIST] Re: Traces don't cause EMI - really?
- From: Bob Patel <whizplayer@xxxxxxxxx>
- To: Aubrey_Sparkman@xxxxxxxx, leeritchey@xxxxxxxxxxxxx,MikonCons@xxxxxxx, weirsp@xxxxxxxxxx
- Date: Tue, 3 Feb 2004 18:42:29 -0800 (PST)
Hi! Aubrey, You are missing the point, the topic is on thickness of the trace
when routed microstrip, i.e. the thickness of soldermask and which I understand
is measured by fab vendors. It is approximate and varies between different fab
suppliers.
What do you mean by between traces, are you referring to pairs, if yes then you
are confusing thickness with pitch....
Bob
Aubrey_Sparkman@xxxxxxxx wrote:
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
---------------------------------
Do you Yahoo!?
Yahoo! SiteBuilder - Free web site building tool. Try it!
------------------------------------------------------------------
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:
