[SI-LIST] Re: PCB tracks
- From: ray_waugh@xxxxxxxxxxx
- To: si-list@xxxxxxxxxxxxx
- Date: Sun, 11 Aug 2002 20:15:48 -0600
Istvan...
You write "People with RF and microwave experience, and digital designers who
heard about RF design techniques, claim that 90 degree corners create impedance
discontinuities..."
At the risk of being contentious, I am one of those with experience - forty
years of it. I maintain that a properly mitered 90 degree bend in a 50 ohm
microstrip line cannot be detected by any TDR ever made, nor can it be detected
or "seen" by any frequency-domain network analyzer working up to 12 or 18 GHz.
The mitering removes the 10 to 100 femtoFarads of shunt capacitance that a
unmitered bend would have.
The most common form of right angle turn in a RF board is a mitered 90 degree
bend. Break open your cellphone and check.
Ray
Raymond W. Waugh
Agilent Technologies
ray_waugh@xxxxxxxxxxx
-----Original Message-----
From: Istvan Novak [mailto:istvan.novak@xxxxxxxxxxxxxxxx]
Sent: Saturday, August 10, 2002 6:32 AM
To: si-list@xxxxxxxxxxxxx
Subject: [SI-LIST] Re: PCB tracks
Hi,
I think the source of the confusion is the hystorical difference between RF
and digital circuits.
People with RF and microwave experience, and digital designers who heard
about RF design techniques, claim that: 90 degree corners
- create impedance discontinuities
- generate EMI radiation (if the trace is on the surface)
People doing digital designs in practice say that in dense high-speed
digital design
- impedance discontinuity of 90 degree bends does not matter
- have not seen systematic measured evidence that sharp corners are an EMI
problem
Who is right with these seemingly contradictory statements? The funny truth
is that both sets of statements are correct (please watch the wording of the
above statements very closely). Here is why:
It is true that 90-degree corners (and also 45-degree corners for that
matter) create impedance discontinuities and create standing waves with
portion of the standing wave leaking out, creating EMI radiation. However,
typical traditional RF and microwave circuits have (and obviously there are
always exceptions)
- wide and short traces, therefore resistive trace loss is minimal
- matched silicons, where not only the real part of the impedance is set
properly, but also the silicon's input capacitance is tuned out
- no or just the absolute minimal number of vertical via connections
For the above reasons (minimal resistive trace loss, minimal or no via
capacitance, minimal or no device capacitance), on traditional RF and
microwave circuits, the single biggest discontinuity contributor may come
from corners and (T) junctions. The equivalent capacitance of a 90-degree
corner can be measured in femtoFarads. Typical via capacitance is a
fraction of a pF, and (packaged silicon) device capacitance can be up to
several pF. If we take out the via and device capacitances, the
discontinuities created by right-angle bends become visible and show up as
the biggest problem to fight.
On today's dense digital boards, on the other hand, we do have vias and
through holes (if not for any other reason, just for testability), which are
typically several times higher in equivalent capacitance. We also have
silicons, which even if they are 'matched', the imaginary part of input
impedance (the input capacitance) most of the time is still not tuned out.
Packaged device input capacitances are usually two orders of magnitudes
higher than the capacitance of a bend. We also tend to use (because we have
to) narrow, resistive traces. For these reasons, in a typical digital
circuit, the impedance discontinuity of a right-angle bend does not matter
(though it is present), because it is masked out by the one and two-order of
magnitude bigger via and device discontinuities.
Similar arguments apply to the EMI radiation: the typical 'clean' and 'flat'
geometry of a RF or microwave circuit leave any sharp corner on the surface
'electrically visible', so its radiation can be measured and is not masked
out by bigger factors. But on dense digital circuits, we have many right
angle bends, even if not in the PCB itself: we have thousands of right-angle
corners where our package pins or balls connect to the PCB, also every pin
of a gull-wing package has the right-angle bend. Plus many silicon devices
are not packaged in EMI-tight case, and the high-current loops on the
package and on the silicon do radiate. The radiation from PCB bends, though
present, is being masked out by the other, bigger and/or more numerous
radiation components.
As digital designs become higher speed, and we are using more point-to-point
connections, with the lowest possible via count, time may come when
right-angle bends in digital designs will matter more.
Sharp right-angle bends on narrow traces increase the risk of opening at the
inner corners during the etching process, though this should not (and does
not) happen with proper manufacturing processes. This manufacturing risk
can be safely eliminated altogether by using 45-degree corners.
Regards
Istvan Novak
SUN Microsystems
----- Original Message -----
From: <ray_waugh@xxxxxxxxxxx>
To: <si-list@xxxxxxxxxxxxx>
Sent: Friday, August 09, 2002 9:52 AM
Subject: [SI-LIST] Re: PCB tracks
>
> Changes in characteristic impedance do not matter as long as the
mismatched section is shorter than a tenth wavelength at the highest
operating frequency, and as long as it is offset by a second mismatch. For
example, a short section of narrow line (high impedance) can be nicely
offset by a short section of wide line (low impedance), forming a low pass
filter with a cutoff frequency higher than your highest operating frequency.
>
> Radiation in TEM mode microstrip lines is a function of frequency, board
thickness and board dielectric constant. Thin boards and boards with a high
dielectric constant restrict the E-fields of the line (keep them close to
the ground plane) and inhibit radiation. 32 mil FR4 works very nicely to 6
or 8 GHz, and 16 mil FR4 would not radiate anything you can measure at 15
GHz.
>
> Ray
>
> Raymond Waugh
> Agilent Technologies
> ray_waugh@xxxxxxxxxxx
>
> -----Original Message-----
> From: Ismail B - CTD, Chennai. [mailto:ismailb@xxxxxxxxxxxxxxx]
> Sent: Friday, August 09, 2002 3:09 AM
> To: gurunath.kulkarni@xxxxxxxxx; cadpro2k@xxxxxxxxxx; SI-LIST
> Subject: [SI-LIST] Re: PCB tracks
>
>
>
> Hi GVK,
>
> I think there will be a sudden change in charateristic impedance at 90 deg
> bends due to increase in trace width at those points. This change in
> impedance will set up reflections on the trace. As far as EMI is concerned
I
> have a feeling that pointed edges do radiate more that curved edges.
> However, Im not sure about other members comments (Perhaps, I have not
> experimented on this ). Generally, We prefer 45 deg bends on our boards.
>
> Regards,
> Ismail
>
>
> -----Original Message-----
> From: gurunath vinayakrao kulkarni [mailto:gurunath.kulkarni@xxxxxxxxx]
> Sent: Friday, August 09, 2002 3:18 PM
> To: cadpro2k@xxxxxxxxxx; SI-LIST
> Subject: [SI-LIST] Re: PCB tracks
>
>
> Hi Mitch,
>
> I meant 45 deg and not 90 deg. If you have 90 deg , there will problems
when
> the current flows through the trace, the steep edge ( 90 deg) will act as
> antenna and there will some EMI problems( emit radiations). When the
> electrons hit the edge , there will sudden change in the direction of the
> flow of the current, so this creates the emission effects. Please anybody
> correct me if I am wrong.
>
> GVK
> ----- Original Message -----
> From: <cadpro2k@xxxxxxxxxx>
> To: "SI-LIST" <si-list@xxxxxxxxxxxxx>
> Sent: Thursday, August 08, 2002 11:00 PM
> Subject: [SI-LIST] Re: PCB tracks
>
>
> > Hi GVK,
> >
> > I think you misspoke. I'm sure you meant to say "usually 90 deg is OK"
> > CAD tools make it so easy to do the 45s, and we, the PCB designers, have
> > been asked to make them all 45 for the longest time, since the
> > engineering community drove the CAD tool vendors for the 45 degree
> > option. Still, so much time is wasted day in and day out on "cleansing"
> > the board ("NO! I can't have 90 degree bends on my board with a clock
> > speed of 100Mhz!"), and making all the buried layers look appealing. I
> > still contend the 45 degree theory is a fallacy, and I think it's been
> > proven time and again (see http://www.ultracad.com , notes section).
> >
> > Ranting over.
> >
> > Mitch
> >
> > ---------Included Message----------
> > > Date: Thu, 8 Aug 2002 17:45:38 +0530
> > > From: "gurunath vinayakrao kulkarni"
> > > I agree with Philippe Robert as I have not seen the PCB with
> > curved traces
> > > usually 45 deg is O.K
> > >
> > > GVK
> > _____________________________________________________________
> >
> >
> > ------------------------------------------------------------------
> > 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 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
> >
> >
>
>
>
> -- Attached file included as plaintext by Ecartis --
> -- File: Wipro_Disclaimer.txt
>
> **************************Disclaimer************************************
>
> Information contained in this E-MAIL being proprietary to Wipro Limited is
> 'privileged' and 'confidential' and intended for use only by the
individual
> or entity to which it is addressed. You are notified that any use,
copying
> or dissemination of the information contained in the E-MAIL in any manner
> whatsoever is strictly prohibited.
>
>
***************************************************************************
>
>
> ------------------------------------------------------------------
> 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 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 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 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 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 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:
