crosstalk...

J

John Larkin

Guest
https://www.dropbox.com/s/zaf7w7t71jmc820/Xtalk.jpg?raw=1

PCB layout people like to pack traces in nice tight bundles, which
encourages crosstalk and impedance issues.

Some general advice might be to separate microstrip traces by 2x the
trace width or 2x the distance to the ground plane, whichever is
greater.

I just made that up. What are your rules?



--

If a man will begin with certainties, he shall end with doubts,
but if he will be content to begin with doubts he shall end in certainties.
Francis Bacon
 
P

Phil Hobbs

Guest
John Larkin wrote:
https://www.dropbox.com/s/zaf7w7t71jmc820/Xtalk.jpg?raw=1

PCB layout people like to pack traces in nice tight bundles, which
encourages crosstalk and impedance issues.

Some general advice might be to separate microstrip traces by 2x the
trace width or 2x the distance to the ground plane, whichever is
greater.

I just made that up. What are your rules?

Ish. Alternating traces going in opposite directions is a big help,
because the coupling doesn\'t build up that way.

It depends on how far they go together, how fast the signals are, and
how vulnerable the receiving trace is.

Cheers

Phil Hobbs

--
Dr Philip C D Hobbs
Principal Consultant
ElectroOptical Innovations LLC / Hobbs ElectroOptics
Optics, Electro-optics, Photonics, Analog Electronics
Briarcliff Manor NY 10510

http://electrooptical.net
http://hobbs-eo.com
 
J

John Larkin

Guest
On Mon, 9 May 2022 17:06:08 -0400, Phil Hobbs
<pcdhSpamMeSenseless@electrooptical.net> wrote:

John Larkin wrote:

https://www.dropbox.com/s/zaf7w7t71jmc820/Xtalk.jpg?raw=1

PCB layout people like to pack traces in nice tight bundles, which
encourages crosstalk and impedance issues.

Some general advice might be to separate microstrip traces by 2x the
trace width or 2x the distance to the ground plane, whichever is
greater.

I just made that up. What are your rules?


Ish. Alternating traces going in opposite directions is a big help,
because the coupling doesn\'t build up that way.

It depends on how far they go together, how fast the signals are, and
how vulnerable the receiving trace is.

Cheers

Phil Hobbs

This board has a MicroZed that runs a lot of fast signals to 8 plugin
boards. The pinouts were selected (not by me) to minimize crossovers
and vias without much thought to signal speeds or directions. The easy
fix is to just spread them out.

The traces are, quite by accident, the correct 75 ohms, 8 mil wide
microstrips.

--

If a man will begin with certainties, he shall end with doubts,
but if he will be content to begin with doubts he shall end in certainties.
Francis Bacon
 
J

John Larkin

Guest
On Mon, 09 May 2022 17:18:02 -0700, John Larkin
<jlarkin@highland_atwork_technology.com> wrote:

On Mon, 9 May 2022 17:06:08 -0400, Phil Hobbs
pcdhSpamMeSenseless@electrooptical.net> wrote:

John Larkin wrote:

https://www.dropbox.com/s/zaf7w7t71jmc820/Xtalk.jpg?raw=1

PCB layout people like to pack traces in nice tight bundles, which
encourages crosstalk and impedance issues.

Some general advice might be to separate microstrip traces by 2x the
trace width or 2x the distance to the ground plane, whichever is
greater.

I just made that up. What are your rules?


Ish. Alternating traces going in opposite directions is a big help,
because the coupling doesn\'t build up that way.

It depends on how far they go together, how fast the signals are, and
how vulnerable the receiving trace is.

Cheers

Phil Hobbs

This board has a MicroZed that runs a lot of fast signals to 8 plugin
boards. The pinouts were selected (not by me) to minimize crossovers
and vias without much thought to signal speeds or directions. The easy
fix is to just spread them out.

The traces are, quite by accident, the correct 75 ohms, 8 mil wide
microstrips.

Playing with the diff pair calculator in Saturn, one would like a diff
pair to be 75 ohms per trace and 150 differential, which implies zero
coupling. I get that with about 50 mils between traces, 12 mils of FR4
to the ground plane.

With 8 mil traces and a 16 mil gap, 12 mils down to the plane, I see
75r per trace and 131 differential, which is mediocre isolation.

A 24 mil gap is better, 75 and 141 ohms. 24 is accidentally 2x the 12
mil dielectric thickness.

--

If a man will begin with certainties, he shall end with doubts,
but if he will be content to begin with doubts he shall end in certainties.
Francis Bacon
 
A

Anthony William Sloman

Guest
On Tuesday, May 10, 2022 at 6:52:05 AM UTC+10, John Larkin wrote:
https://www.dropbox.com/s/zaf7w7t71jmc820/Xtalk.jpg?raw=1

PCB layout people like to pack traces in nice tight bundles, which
encourages crosstalk and impedance issues.

Some general advice might be to separate microstrip traces by 2x the
trace width or 2x the distance to the ground plane, whichever is
greater.

I just made that up. What are your rules?

A ground strip between individual signal-carrying traces provides extra isolation between them. If John Larkin had read enough to become knowledgeable about PC traces. he would have seen that mentioned.

--
Bill Sloman, Sydney
 
W

whit3rd

Guest
On Monday, May 9, 2022 at 5:18:14 PM UTC-7, John Larkin wrote:
On Mon, 9 May 2022 17:06:08 -0400, Phil Hobbs
pcdhSpamM...@electrooptical.net> wrote:

Ish. Alternating traces going in opposite directions is a big help,
because the coupling doesn\'t build up that way.

This board has a MicroZed that runs a lot of fast signals to 8 plugin
boards. The pinouts were selected (not by me) to minimize crossovers
and vias without much thought to signal speeds or directions. The easy
fix is to just spread them out.

That\'s not a great fix for ground-loop (inductive) problems. Area inside
the loop is an interfering-signal coupler, so \'spread\' is a square-law
interference increaser.
 
J

John Walliker

Guest
On Tuesday, 10 May 2022 at 08:22:21 UTC+1, whit3rd wrote:
On Monday, May 9, 2022 at 5:18:14 PM UTC-7, John Larkin wrote:
On Mon, 9 May 2022 17:06:08 -0400, Phil Hobbs
pcdhSpamM...@electrooptical.net> wrote:

Ish. Alternating traces going in opposite directions is a big help,
because the coupling doesn\'t build up that way.
This board has a MicroZed that runs a lot of fast signals to 8 plugin
boards. The pinouts were selected (not by me) to minimize crossovers
and vias without much thought to signal speeds or directions. The easy
fix is to just spread them out.
That\'s not a great fix for ground-loop (inductive) problems. Area inside
the loop is an interfering-signal coupler, so \'spread\' is a square-law
interference increaser.
But not if there is a ground plane underneath as the loop is then the area
of the vertical cross section between the track and the ground plane
which does not depend on separation between tracks.
John
 
D

Dimiter_Popoff

Guest
On 5/9/2022 23:51, John Larkin wrote:
https://www.dropbox.com/s/zaf7w7t71jmc820/Xtalk.jpg?raw=1

PCB layout people like to pack traces in nice tight bundles, which
encourages crosstalk and impedance issues.

Some general advice might be to separate microstrip traces by 2x the
trace width or 2x the distance to the ground plane, whichever is
greater.

I just made that up. What are your rules?

For digital (where density is really needed) within 100-200 MHz
we have been doing 4 mil trace 4 mil spacing for ages now.
That on the visible (top and bottom layers), referenced to GND
planes beneath each.
No issue whatsoever. Well, actually I had one, an I2C line was
passing too close (probably not 4 mil, may be a whole mm) to a
flyback switch (IRF540-ish) for the HV which was doing nice
100V excursions and at times managed to upset the i2c.
Pulling the latter up with 1k on each line fixed it (was 2k IIRC).
 
J

John Larkin

Guest
On Tue, 10 May 2022 00:22:16 -0700 (PDT), whit3rd <whit3rd@gmail.com>
wrote:

On Monday, May 9, 2022 at 5:18:14 PM UTC-7, John Larkin wrote:
On Mon, 9 May 2022 17:06:08 -0400, Phil Hobbs
pcdhSpamM...@electrooptical.net> wrote:

Ish. Alternating traces going in opposite directions is a big help,
because the coupling doesn\'t build up that way.

This board has a MicroZed that runs a lot of fast signals to 8 plugin
boards. The pinouts were selected (not by me) to minimize crossovers
and vias without much thought to signal speeds or directions. The easy
fix is to just spread them out.

That\'s not a great fix for ground-loop (inductive) problems. Area inside
the loop is an interfering-signal coupler, so \'spread\' is a square-law
interference increaser.

But spreading the traces is a great fix for crosstalk. Try it.



--

If a man will begin with certainties, he shall end with doubts,
but if he will be content to begin with doubts he shall end in certainties.
Francis Bacon
 
J

John Larkin

Guest
On Tue, 10 May 2022 17:49:20 +0300, Dimiter_Popoff <dp@tgi-sci.com>
wrote:

On 5/9/2022 23:51, John Larkin wrote:

https://www.dropbox.com/s/zaf7w7t71jmc820/Xtalk.jpg?raw=1

PCB layout people like to pack traces in nice tight bundles, which
encourages crosstalk and impedance issues.

Some general advice might be to separate microstrip traces by 2x the
trace width or 2x the distance to the ground plane, whichever is
greater.

I just made that up. What are your rules?




For digital (where density is really needed) within 100-200 MHz
we have been doing 4 mil trace 4 mil spacing for ages now.
That on the visible (top and bottom layers), referenced to GND
planes beneath each.
No issue whatsoever. Well, actually I had one, an I2C line was
passing too close (probably not 4 mil, may be a whole mm) to a
flyback switch (IRF540-ish) for the HV which was doing nice
100V excursions and at times managed to upset the i2c.
Pulling the latter up with 1k on each line fixed it (was 2k IIRC).

Some of our traces will be fast 8b10b data streams. At powerup time we
\"train\" the receivers to adapt to the actual data timing. Crosstalk
from other signals can wobble the bit edges and potentially make data
errors.

--

If a man will begin with certainties, he shall end with doubts,
but if he will be content to begin with doubts he shall end in certainties.
Francis Bacon
 
D

Dimiter_Popoff

Guest
On 5/10/2022 19:56, John Larkin wrote:
On Tue, 10 May 2022 17:49:20 +0300, Dimiter_Popoff <dp@tgi-sci.com
wrote:

On 5/9/2022 23:51, John Larkin wrote:

https://www.dropbox.com/s/zaf7w7t71jmc820/Xtalk.jpg?raw=1

PCB layout people like to pack traces in nice tight bundles, which
encourages crosstalk and impedance issues.

Some general advice might be to separate microstrip traces by 2x the
trace width or 2x the distance to the ground plane, whichever is
greater.

I just made that up. What are your rules?




For digital (where density is really needed) within 100-200 MHz
we have been doing 4 mil trace 4 mil spacing for ages now.
That on the visible (top and bottom layers), referenced to GND
planes beneath each.
No issue whatsoever. Well, actually I had one, an I2C line was
passing too close (probably not 4 mil, may be a whole mm) to a
flyback switch (IRF540-ish) for the HV which was doing nice
100V excursions and at times managed to upset the i2c.
Pulling the latter up with 1k on each line fixed it (was 2k IIRC).

Some of our traces will be fast 8b10b data streams. At powerup time we
\"train\" the receivers to adapt to the actual data timing. Crosstalk
from other signals can wobble the bit edges and potentially make data
errors.

I have done something around 100-150 MHz clocked video squeezed into
lvds (don\'t know how much faster the lvds was clocked, some 8 times
I believe) using the same routing but not many times and over a
short distance, well within an inch. No problems there, either.
 
W

whit3rd

Guest
On Tuesday, May 10, 2022 at 9:52:52 AM UTC-7, John Larkin wrote:
On Tue, 10 May 2022 00:22:16 -0700 (PDT), whit3rd <whi...@gmail.com
wrote:
On Monday, May 9, 2022 at 5:18:14 PM UTC-7, John Larkin wrote:

... to minimize crossovers
and vias without much thought to signal speeds or directions. The easy
fix is to just spread them out.

That\'s not a great fix for ground-loop (inductive) problems. Area inside
the loop is an interfering-signal coupler, so \'spread\' is a square-law
interference increaser.

But spreading the traces is a great fix for crosstalk. Try it.

How to apply that fix, though, to a cat5 cable\'s four pairs?
In one instance, I found a DC/DC converter that needed its input
power through a common-mode bead, because it crosstalked to components a
foot and three circuit boards away. Freeze mist on the converter
changed the frequency of the interference, after other inspections
didn\'t find the problem.
 
D

Dimiter_Popoff

Guest
On 5/10/2022 22:30, whit3rd wrote:
On Tuesday, May 10, 2022 at 9:52:52 AM UTC-7, John Larkin wrote:
On Tue, 10 May 2022 00:22:16 -0700 (PDT), whit3rd <whi...@gmail.com
wrote:
On Monday, May 9, 2022 at 5:18:14 PM UTC-7, John Larkin wrote:

... to minimize crossovers
and vias without much thought to signal speeds or directions. The easy
fix is to just spread them out.

That\'s not a great fix for ground-loop (inductive) problems. Area inside
the loop is an interfering-signal coupler, so \'spread\' is a square-law
interference increaser.

But spreading the traces is a great fix for crosstalk. Try it.

How to apply that fix, though, to a cat5 cable\'s four pairs?
In one instance, I found a DC/DC converter that needed its input
power through a common-mode bead, because it crosstalked to components a
foot and three circuit boards away. Freeze mist on the converter
changed the frequency of the interference, after other inspections
didn\'t find the problem.

Ouch... Sounds nightmarish. Many years ago I had a share of nightmarish
inductive coupling, a tiny (20mm side IIRC) fan turned out to get into
the input signal of a moderately sensitive amp (tens of MHz bandwidth,
the interference was well visible at hundreds of mV fullscale at the
input).
There was nothing I could do other than just get rid of the fan as part
of the design. Which worked, luckily it turned out I had enough margin
for that.
 
R

Ricky

Guest
On Monday, May 9, 2022 at 4:52:05 PM UTC-4, John Larkin wrote:
https://www.dropbox.com/s/zaf7w7t71jmc820/Xtalk.jpg?raw=1

PCB layout people like to pack traces in nice tight bundles, which
encourages crosstalk and impedance issues.

Some general advice might be to separate microstrip traces by 2x the
trace width or 2x the distance to the ground plane, whichever is
greater.

I just made that up. What are your rules?

Crosstalk is negligible between traces on the same plane. It is between traces on different planes running along the same paths that create crosstalk. Very easy to avoid by paying attention when routing... if you don\'t use an auto-router.

--

Rick C.

- Get 1,000 miles of free Supercharging
- Tesla referral code - https://ts.la/richard11209
 
E

Edward Hernandez

Guest
The John Doe troll stated the following in message-id
<sdhn7c$pkp$4@dont-email.me>:

> The troll doesn\'t even know how to format a USENET post...

And the John Doe troll stated the following in message-id
<sg3kr7$qt5$1@dont-email.me>:

The reason Bozo cannot figure out how to get Google to keep from
breaking its lines in inappropriate places is because Bozo is
CLUELESS...

And yet, the clueless John Doe troll has continued to post incorrectly
formatted USENET articles that are devoid of content (latest example on
Sat, 14 May 2022 17:46:49 -0000 (UTC) in message-id
<t5opu8$aeb$2@dont-email.me>).

NOBODY likes the John Doe troll\'s contentless spam.

Further, Troll Doe stated the following in message-id
<svsh05$lbh$5@dont-email.me> posted Fri, 4 Mar 2022 08:01:09 -0000
(UTC):

Compared to other regulars, Bozo contributes practically nothing
except insults to this group.

Yet, since Wed, 5 Jan 2022 04:10:38 -0000 (UTC) Troll Doe\'s post ratio
to USENET (**) has been 60.5% of its posts contributing \"nothing except
insults\" to USENET.

** Since Wed, 5 Jan 2022 04:10:38 -0000 (UTC) Troll Doe has posted at
least 1364 articles to USENET. Of which 148 have been pure insults and
677 have been Troll Doe \"troll format\" postings.

This posting is a public service announcement for any google groups
readers who happen by to point out that the John Doe troll does not even
follow the rules it uses to troll other posters.

Fr7RG8qvqnxH
 
J

John Doe

Guest
Eddie wants so badly to nym-shift. That\'s a no-no here, Eddie!

Eddie has never posted anything NORMAL except when it got a spanking...

https://groups.google.com/g/sci.electronics.repair/c/MesPLcGU4BE

See also...
John Doe <always.look@message.header> (astraweb)
Peter Weiner <dtgamer99@gmail.com>
Edward H. <dtgamer99@gmail.com>
Edward Hernandez <dtgamer99@gmail.com>

Eddie is an example for all newbies. Don\'t get spanked!

Spanked Eddie...

--
Edward Hernandez <dtgamer99@gmail.com> wrote:

Path: eternal-september.org!reader02.eternal-september.org!feeder1.feed.usenet.farm!feed.usenet.farm!news-out.netnews.com!news.alt.net!fdc2.netnews.com!peer02.ams1!peer.ams1.xlned.com!news.xlned.com!peer03.ams4!peer.am4.highwinds-media.com!news.highwinds-media.com!fx02.ams4.POSTED!not-for-mail
From: Edward Hernandez <dtgamer99@gmail.com
Subject: Re: crosstalk
Newsgroups: sci.electronics.design,free.spam
References: <a7vi7h5nupq2957c34b4u33r5mb9nra511@4ax.com> <04748706-31ca-4f62-8cc2-c3aa63f35f1en@googlegroups.com> <t5opu8$aeb$2@dont-email.me
Lines: 40
Message-ID: <UWRfK.3399724$u91.925699@usenetxs.com
X-Complaints-To: https://www.astraweb.com/aup
NNTP-Posting-Date: Sat, 14 May 2022 17:47:32 UTC
Date: Sat, 14 May 2022 17:47:32 GMT
X-Received-Bytes: 2094
Xref: reader02.eternal-september.org sci.electronics.design:668987 free.spam:18249

The John Doe troll stated the following in message-id
sdhn7c$pkp$4@dont-email.me>:

The troll doesn\'t even know how to format a USENET post...

And the John Doe troll stated the following in message-id
sg3kr7$qt5$1@dont-email.me>:

The reason Bozo cannot figure out how to get Google to keep from
breaking its lines in inappropriate places is because Bozo is
CLUELESS...

And yet, the clueless John Doe troll has continued to post incorrectly
formatted USENET articles that are devoid of content (latest example on
Sat, 14 May 2022 17:46:49 -0000 (UTC) in message-id
t5opu8$aeb$2@dont-email.me>).

NOBODY likes the John Doe troll\'s contentless spam.

Further, Troll Doe stated the following in message-id
svsh05$lbh$5@dont-email.me> posted Fri, 4 Mar 2022 08:01:09 -0000
(UTC):

Compared to other regulars, Bozo contributes practically nothing
except insults to this group.

Yet, since Wed, 5 Jan 2022 04:10:38 -0000 (UTC) Troll Doe\'s post ratio
to USENET (**) has been 60.5% of its posts contributing \"nothing except
insults\" to USENET.

** Since Wed, 5 Jan 2022 04:10:38 -0000 (UTC) Troll Doe has posted at
least 1364 articles to USENET. Of which 148 have been pure insults and
677 have been Troll Doe \"troll format\" postings.

This posting is a public service announcement for any google groups
readers who happen by to point out that the John Doe troll does not even
follow the rules it uses to troll other posters.

Fr7RG8qvqnxH
 
E

Edward Hernandez

Guest
The John Doe troll stated the following in message-id
<sdhn7c$pkp$4@dont-email.me>:

> The troll doesn\'t even know how to format a USENET post...

And the John Doe troll stated the following in message-id
<sg3kr7$qt5$1@dont-email.me>:

The reason Bozo cannot figure out how to get Google to keep from
breaking its lines in inappropriate places is because Bozo is
CLUELESS...

And yet, the clueless John Doe troll has itself posted yet another
incorrectly formatted USENET posting on Sat, 14 May 2022 17:53:48 -0000
(UTC) in message-id <t5oqbb$aeb$5@dont-email.me>.

Further, Troll Doe stated the following in message-id
<svsh05$lbh$5@dont-email.me> posted Fri, 4 Mar 2022 08:01:09 -0000
(UTC):

Compared to other regulars, Bozo contributes practically nothing
except insults to this group.

Yet, since Wed, 5 Jan 2022 04:10:38 -0000 (UTC) Troll Doe\'s post ratio
to USENET (**) has been 60.5% of its posts contributing \"nothing except
insults\" to USENET.

** Since Wed, 5 Jan 2022 04:10:38 -0000 (UTC) Troll Doe has posted at
least 1367 articles to USENET. Of which 148 have been pure insults and
679 have been Troll Doe \"troll format\" postings.

This posting is a public service announcement for any google groups
readers who happen by to point out that the John Doe troll does not even
follow the rules it uses to troll other posters.

LujEfVNcdpEE
 
A

Anthony William Sloman

Guest
On Sunday, May 15, 2022 at 3:46:55 AM UTC+10, John Doe wrote:
Anthony William Sloman <bill....@ieee.org> wrote:
On Tuesday, May 10, 2022 at 6:52:05 AM UTC+10, John Larkin wrote:
https://www.dropbox.com/s/zaf7w7t71jmc820/Xtalk.jpg?raw=1

PCB layout people like to pack traces in nice tight bundles, which
encourages crosstalk and impedance issues.

Some general advice might be to separate microstrip traces by 2x the
trace width or 2x the distance to the ground plane, whichever is
greater.

I just made that up. What are your rules?

A ground strip between individual signal-carrying traces provides extra isolation between them. If John Larkin had read enough to become knowledgeable about PC traces. he would have seen that mentioned.

An utterly loony Australian.

The sort of thing that John Doe likes to post. He doesn\'t have a clue about transmission lines, so imagines he can get away with posting a false and totally unreasonable claim.

In fact what I was proposing was the use of multiple grounded coplanar waveguides on the same board.

https://www.microwavejournal.com/blogs/1-rog-blog/post/24374-comparing-microstrip-and-grounded-coplanar-waveguide

If I spent enough time at it I could probably find a specific example, but John Doe wouldn\'t understand that either, and John Larkin would ignore it.

--
Bill Sloman, Sydney
 

Welcome to EDABoard.com

Sponsor

Top