1. Forum
  2. Usenet
  3. SCI.ELECTRONICS.DESIGN

  • crosstalk

    From John Larkin@21:1/5 to All on Mon May 9 13:51:53 2022
    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

    --- SoupGate-Win32 v1.05
    * Origin: fsxNet Usenet Gateway (21:1/5)
  • From Phil Hobbs@21:1/5 to John Larkin on Mon May 9 17:06:08 2022
    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

    --- SoupGate-Win32 v1.05
    * Origin: fsxNet Usenet Gateway (21:1/5)
  • From John Larkin@21:1/5 to jlarkin@highland_atwork_technology. on Mon May 9 17:36:36 2022
    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

    --- SoupGate-Win32 v1.05
    * Origin: fsxNet Usenet Gateway (21:1/5)
  • From John Larkin@21:1/5 to pcdhSpamMeSenseless@electrooptical. on Mon May 9 17:18:02 2022
    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

    --- SoupGate-Win32 v1.05
    * Origin: fsxNet Usenet Gateway (21:1/5)
  • From Anthony William Sloman@21:1/5 to John Larkin on Mon May 9 20:10:42 2022
    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

    --- SoupGate-Win32 v1.05
    * Origin: fsxNet Usenet Gateway (21:1/5)
  • From whit3rd@21:1/5 to John Larkin on Tue May 10 00:22:16 2022
    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.

    --- SoupGate-Win32 v1.05
    * Origin: fsxNet Usenet Gateway (21:1/5)
  • From John Walliker@21:1/5 to All on Tue May 10 01:53:46 2022
    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

    --- SoupGate-Win32 v1.05
    * Origin: fsxNet Usenet Gateway (21:1/5)
  • From Dimiter_Popoff@21:1/5 to John Larkin on Tue May 10 17:49:20 2022
    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).

    --- SoupGate-Win32 v1.05
    * Origin: fsxNet Usenet Gateway (21:1/5)
  • From John Larkin@21:1/5 to All on Tue May 10 09:52:40 2022
    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

    --- SoupGate-Win32 v1.05
    * Origin: fsxNet Usenet Gateway (21:1/5)
  • From John Larkin@21:1/5 to All on Tue May 10 09:56:36 2022
    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

    --- SoupGate-Win32 v1.05
    * Origin: fsxNet Usenet Gateway (21:1/5)
  • From Dimiter_Popoff@21:1/5 to John Larkin on Tue May 10 20:24:20 2022
    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.

    --- SoupGate-Win32 v1.05
    * Origin: fsxNet Usenet Gateway (21:1/5)
  • From Dimiter_Popoff@21:1/5 to All on Tue May 10 22:52:16 2022
    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.

    --- SoupGate-Win32 v1.05
    * Origin: fsxNet Usenet Gateway (21:1/5)
  • From whit3rd@21:1/5 to John Larkin on Tue May 10 12:30:24 2022
    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.

    --- SoupGate-Win32 v1.05
    * Origin: fsxNet Usenet Gateway (21:1/5)
  • From Ricky@21:1/5 to John Larkin on Tue May 10 19:26:11 2022
    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

    --- SoupGate-Win32 v1.05
    * Origin: fsxNet Usenet Gateway (21:1/5)
  • From John Doe@21:1/5 to Anthony William Sloman on Sat May 14 17:46:49 2022
    XPost: free.spam

    An utterly loony Australian.

    Bozo Bill Sloman, the most frequent troll in this group, is an attention- craving chronic liar who cannot be reasoned with.

    "the user has posted under the same name in other places, so not
    nym-shifting" (Bozo sucks at logic)

    "the Mueller investigation was about Trump only because Trump made it so"
    (Bozo being Bozo)

    "the concepts "male" and "female" are essentially social constructions"
    (Bozo is a textbook cannibal leftist)

    --
    Anthony William Sloman <bill.sloman@ieee.org> wrote:

    X-Received: by 2002:ae9:de43:0:b0:69f:7585:8276 with SMTP id s64-20020ae9de43000000b0069f75858276mr13923501qkf.706.1652152243589; Mon, 09 May 2022 20:10:43 -0700 (PDT)
    X-Received: by 2002:a81:134a:0:b0:2f8:6751:bd66 with SMTP id 71-20020a81134a000000b002f86751bd66mr17383455ywt.340.1652152243275; Mon, 09 May 2022 20:10:43 -0700 (PDT)
    Path: eternal-september.org!reader02.eternal-september.org!usenet.blueworldhosting.com!feed1.usenet.blueworldhosting.com!peer02.iad!feed-me.highwinds-media.com!news.highwinds-media.com!news-out.google.com!nntp.google.com!postnews.google.com!google-
    groups.googlegroups.com!not-for-mail
    Newsgroups: sci.electronics.design
    Date: Mon, 9 May 2022 20:10:42 -0700 (PDT)
    In-Reply-To: <a7vi7h5nupq2957c34b4u33r5mb9nra511@4ax.com>
    Injection-Info: google-groups.googlegroups.com; posting-host=118.208.108.19; posting-account=SJ46pgoAAABuUDuHc5uDiXN30ATE-zi-
    NNTP-Posting-Host: 118.208.108.19
    References: <a7vi7h5nupq2957c34b4u33r5mb9nra511@4ax.com>
    User-Agent: G2/1.0
    MIME-Version: 1.0
    Message-ID: <04748706-31ca-4f62-8cc2-c3aa63f35f1en@googlegroups.com>
    Subject: Re: crosstalk
    From: Anthony William Sloman <bill.sloman@ieee.org>
    Injection-Date: Tue, 10 May 2022 03:10:43 +0000
    Content-Type: text/plain; charset="UTF-8"
    X-Received-Bytes: 1793
    Xref: reader02.eternal-september.org sci.electronics.design:668762

    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


    --- SoupGate-Win32 v1.05
    * Origin: fsxNet Usenet Gateway (21:1/5)
  • From Edward Hernandez@21:1/5 to All on Sat May 14 17:47:32 2022
    XPost: free.spam

    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

    --- SoupGate-Win32 v1.05
    * Origin: fsxNet Usenet Gateway (21:1/5)
  • From John Doe@21:1/5 to Edward Hernandez on Sat May 14 17:53:48 2022
    XPost: free.spam

    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




    --- SoupGate-Win32 v1.05
    * Origin: fsxNet Usenet Gateway (21:1/5)
  • From Edward Hernandez@21:1/5 to All on Sat May 14 17:57:03 2022
    XPost: free.spam

    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

    --- SoupGate-Win32 v1.05
    * Origin: fsxNet Usenet Gateway (21:1/5)
  • From Anthony William Sloman@21:1/5 to John Doe on Sat May 14 21:03:57 2022
    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

    --- SoupGate-Win32 v1.05
    * Origin: fsxNet Usenet Gateway (21:1/5)