tee trace...

[server]

Suppose one had a microstrip trace that was higher impedance than
ideal, but couldn\'t be made wider. One could reduce the distance to
the ground plane, but that might have capacitance consequences
elsewhere.

I wonder if one could add a vertical conductor, sort of a shark fin,
to make the conductor have a t-shaped cross section.

I guess ATLC could analyze that. I might try it after I actually wake
up.

One could also glue a chunk of dielectric to the top of the trace,
with optional copper on top. Make it into a sort of stripline.



--

I yam what I yam - Popeye

 

[Hul Tytus]

John - a possible approach: the higher the dielectric constant on which
a conductor sits, the lower it\'s impedence. So, maybe some tape
on top of your errant conductor.

Hul

jlarkin@highlandsniptechnology.com wrote:

Suppose one had a microstrip trace that was higher impedance than
ideal, but couldn\'t be made wider. One could reduce the distance to
the ground plane, but that might have capacitance consequences
elsewhere.

I wonder if one could add a vertical conductor, sort of a shark fin,
to make the conductor have a t-shaped cross section.

I guess ATLC could analyze that. I might try it after I actually wake
up.

One could also glue a chunk of dielectric to the top of the trace,
with optional copper on top. Make it into a sort of stripline.

--

I yam what I yam - Popeye

 

[Lasse Langwadt Christensen]

mandag den 13. december 2021 kl. 16.38.35 UTC+1 skrev jla...@highlandsniptechnology.com:

Suppose one had a microstrip trace that was higher impedance than
ideal, but couldn\'t be made wider. One could reduce the distance to
the ground plane, but that might have capacitance consequences
elsewhere.

so add an extra layer for a ground plane close to the microstrip,
but leave it blank where you need low capacitance

standard pcb expect for the special stackup and no extra production steps

 

[John Larkin]

On Mon, 13 Dec 2021 14:03:55 -0800 (PST), Lasse Langwadt Christensen
<langwadt@fonz.dk> wrote:

mandag den 13. december 2021 kl. 16.38.35 UTC+1 skrev jla...@highlandsniptechnology.com:
Suppose one had a microstrip trace that was higher impedance than
ideal, but couldn\'t be made wider. One could reduce the distance to
the ground plane, but that might have capacitance consequences
elsewhere.

so add an extra layer for a ground plane close to the microstrip,
but leave it blank where you need low capacitance

standard pcb expect for the special stackup and no extra production steps

It\'s already a 6 layer board. Here\'s the trace, running from the IC to
C28. I want it to be 25 ohms but can\'t make it wide enough. Adding the
coplanar waveguide grounds only helped a little.

https://www.dropbox.com/s/97zkiqidwszo9le/T502_25r_Trace.jpg?raw=1

It might be OK... it\'s pretty short. But if not, maybe I can add
something to pull the impedance down.

I could TDR a microstrip and stick something on top, like a piece of
FR4 or maybe even just some epoxy or something. Yes, I\'ll try that
just to calibrate my expectations.






--

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

 

[Anthony William Sloman]

On Tuesday, December 14, 2021 at 12:36:19 PM UTC+11, John Larkin wrote:

On Mon, 13 Dec 2021 14:03:55 -0800 (PST), Lasse Langwadt Christensen
lang...@fonz.dk> wrote:

mandag den 13. december 2021 kl. 16.38.35 UTC+1 skrev jla...@highlandsniptechnology.com:
Suppose one had a microstrip trace that was higher impedance than
ideal, but couldn\'t be made wider. One could reduce the distance to
the ground plane, but that might have capacitance consequences
elsewhere.

so add an extra layer for a ground plane close to the microstrip,
but leave it blank where you need low capacitance

standard pcb expect for the special stackup and no extra production steps
It\'s already a 6 layer board. Here\'s the trace, running from the IC to
C28. I want it to be 25 ohms but can\'t make it wide enough. Adding the
coplanar waveguide grounds only helped a little.

https://www.dropbox.com/s/97zkiqidwszo9le/T502_25r_Trace.jpg?raw=1

It might be OK... it\'s pretty short. But if not, maybe I can add
something to pull the impedance down.

I could TDR a microstrip and stick something on top, like a piece of
FR4 or maybe even just some epoxy or something. Yes, I\'ll try that
just to calibrate my expectations.

If it is microstrip, you\'ve routed it on the surface of the board. If you used buried stripline the impedance will be lower for the same trace width.

Burying two of them (with ground plane in between) and putting them in parallel would halve that impedance. It\'s two vias - one at each end - but you should be able to figure that in.

--
Bill Sloman, Sydney

--

 

[Lasse Langwadt Christensen]

tirsdag den 14. december 2021 kl. 02.36.19 UTC+1 skrev John Larkin:

On Mon, 13 Dec 2021 14:03:55 -0800 (PST), Lasse Langwadt Christensen
lang...@fonz.dk> wrote:

mandag den 13. december 2021 kl. 16.38.35 UTC+1 skrev jla...@highlandsniptechnology.com:
Suppose one had a microstrip trace that was higher impedance than
ideal, but couldn\'t be made wider. One could reduce the distance to
the ground plane, but that might have capacitance consequences
elsewhere.

so add an extra layer for a ground plane close to the microstrip,
but leave it blank where you need low capacitance

standard pcb expect for the special stackup and no extra production steps
It\'s already a 6 layer board. Here\'s the trace, running from the IC to
C28. I want it to be 25 ohms but can\'t make it wide enough. Adding the
coplanar waveguide grounds only helped a little.

https://www.dropbox.com/s/97zkiqidwszo9le/T502_25r_Trace.jpg?raw=1

It might be OK... it\'s pretty short. But if not, maybe I can add
something to pull the impedance down.

I could TDR a microstrip and stick something on top, like a piece of
FR4 or maybe even just some epoxy or something. Yes, I\'ll try that
just to calibrate my expectations.

is is very short and looks you could easily make it shorter

 

[Rick C]

On Monday, December 13, 2021 at 10:19:34 PM UTC-4, lang...@fonz.dk wrote:

tirsdag den 14. december 2021 kl. 02.36.19 UTC+1 skrev John Larkin:
On Mon, 13 Dec 2021 14:03:55 -0800 (PST), Lasse Langwadt Christensen
lang...@fonz.dk> wrote:

mandag den 13. december 2021 kl. 16.38.35 UTC+1 skrev jla...@highlandsniptechnology.com:
Suppose one had a microstrip trace that was higher impedance than
ideal, but couldn\'t be made wider. One could reduce the distance to
the ground plane, but that might have capacitance consequences
elsewhere.

so add an extra layer for a ground plane close to the microstrip,
but leave it blank where you need low capacitance

standard pcb expect for the special stackup and no extra production steps
It\'s already a 6 layer board. Here\'s the trace, running from the IC to
C28. I want it to be 25 ohms but can\'t make it wide enough. Adding the
coplanar waveguide grounds only helped a little.

https://www.dropbox.com/s/97zkiqidwszo9le/T502_25r_Trace.jpg?raw=1

It might be OK... it\'s pretty short. But if not, maybe I can add
something to pull the impedance down.

I could TDR a microstrip and stick something on top, like a piece of
FR4 or maybe even just some epoxy or something. Yes, I\'ll try that
just to calibrate my expectations.

is is very short and looks you could easily make it shorter

Yeah, he doesn\'t say what he\'s doing. I wonder if he\'s solving the right problem.

--

Rick C.

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

 

[server]

On Mon, 13 Dec 2021 18:19:30 -0800 (PST), Lasse Langwadt Christensen
<langwadt@fonz.dk> wrote:

tirsdag den 14. december 2021 kl. 02.36.19 UTC+1 skrev John Larkin:
On Mon, 13 Dec 2021 14:03:55 -0800 (PST), Lasse Langwadt Christensen
lang...@fonz.dk> wrote:

mandag den 13. december 2021 kl. 16.38.35 UTC+1 skrev jla...@highlandsniptechnology.com:
Suppose one had a microstrip trace that was higher impedance than
ideal, but couldn\'t be made wider. One could reduce the distance to
the ground plane, but that might have capacitance consequences
elsewhere.

so add an extra layer for a ground plane close to the microstrip,
but leave it blank where you need low capacitance

standard pcb expect for the special stackup and no extra production steps
It\'s already a 6 layer board. Here\'s the trace, running from the IC to
C28. I want it to be 25 ohms but can\'t make it wide enough. Adding the
coplanar waveguide grounds only helped a little.

https://www.dropbox.com/s/97zkiqidwszo9le/T502_25r_Trace.jpg?raw=1

It might be OK... it\'s pretty short. But if not, maybe I can add
something to pull the impedance down.

I could TDR a microstrip and stick something on top, like a piece of
FR4 or maybe even just some epoxy or something. Yes, I\'ll try that
just to calibrate my expectations.

is is very short and looks you could easily make it shorter

That trace is about 0.12\" long, roughly 20 ps, but I\'ve made it about
as short as I can. There are all sorts of other parts around.

The RF boys measure flatness in dBs but we need PPMs. This is for a
laser modulator for people with extreme expectations.





--

I yam what I yam - Popeye

 

[Clifford Heath]

On 14/12/21 2:47 pm, Rick C wrote:

On Monday, December 13, 2021 at 10:19:34 PM UTC-4, lang...@fonz.dk wrote:
tirsdag den 14. december 2021 kl. 02.36.19 UTC+1 skrev John Larkin:
On Mon, 13 Dec 2021 14:03:55 -0800 (PST), Lasse Langwadt Christensen
lang...@fonz.dk> wrote:

mandag den 13. december 2021 kl. 16.38.35 UTC+1 skrev jla...@highlandsniptechnology.com:
Suppose one had a microstrip trace that was higher impedance than
ideal, but couldn\'t be made wider. One could reduce the distance to
the ground plane, but that might have capacitance consequences
elsewhere.

so add an extra layer for a ground plane close to the microstrip,
but leave it blank where you need low capacitance

standard pcb expect for the special stackup and no extra production steps
It\'s already a 6 layer board. Here\'s the trace, running from the IC to
C28. I want it to be 25 ohms but can\'t make it wide enough. Adding the
coplanar waveguide grounds only helped a little.

https://www.dropbox.com/s/97zkiqidwszo9le/T502_25r_Trace.jpg?raw=1

It might be OK... it\'s pretty short. But if not, maybe I can add
something to pull the impedance down.

I could TDR a microstrip and stick something on top, like a piece of
FR4 or maybe even just some epoxy or something. Yes, I\'ll try that
just to calibrate my expectations.

is is very short and looks you could easily make it shorter

Yeah, he doesn\'t say what he\'s doing. I wonder if he\'s solving the right problem.

Chances are it\'s the 11GHz/25ps laser diode driver from last week, and
he wants to manage the impedance from the die to the coupling capacitor,
at least.

John, you need to use a field solver.

CH

 

[server]

On Tue, 14 Dec 2021 15:31:53 +1100, Clifford Heath
<no.spam@please.net> wrote:

On 14/12/21 2:47 pm, Rick C wrote:
On Monday, December 13, 2021 at 10:19:34 PM UTC-4, lang...@fonz.dk wrote:
tirsdag den 14. december 2021 kl. 02.36.19 UTC+1 skrev John Larkin:
On Mon, 13 Dec 2021 14:03:55 -0800 (PST), Lasse Langwadt Christensen
lang...@fonz.dk> wrote:

mandag den 13. december 2021 kl. 16.38.35 UTC+1 skrev jla...@highlandsniptechnology.com:
Suppose one had a microstrip trace that was higher impedance than
ideal, but couldn\'t be made wider. One could reduce the distance to
the ground plane, but that might have capacitance consequences
elsewhere.

so add an extra layer for a ground plane close to the microstrip,
but leave it blank where you need low capacitance

standard pcb expect for the special stackup and no extra production steps
It\'s already a 6 layer board. Here\'s the trace, running from the IC to
C28. I want it to be 25 ohms but can\'t make it wide enough. Adding the
coplanar waveguide grounds only helped a little.

https://www.dropbox.com/s/97zkiqidwszo9le/T502_25r_Trace.jpg?raw=1

It might be OK... it\'s pretty short. But if not, maybe I can add
something to pull the impedance down.

I could TDR a microstrip and stick something on top, like a piece of
FR4 or maybe even just some epoxy or something. Yes, I\'ll try that
just to calibrate my expectations.

is is very short and looks you could easily make it shorter

Yeah, he doesn\'t say what he\'s doing. I wonder if he\'s solving the right problem.

Chances are it\'s the 11GHz/25ps laser diode driver from last week, and
he wants to manage the impedance from the die to the coupling capacitor,
at least.

John, you need to use a field solver.

CH

I can easily calculate the trace impedance, but I want 25 ohms and
that\'s not practical on this layout. The source chip is basically an
80 mA 25 ohm CML source, if you can imagine such a thing. It would
source terminate a 25 ohm trace.

ATLC could calculate a microstrip with a slab of dielectric added on
top. But ATLC is basically a 2D analysis and life is 4D : X Y Z T.

And I don\'t have device models, which I\'d need for a serious
simulation. Modifying trace impedances up is easy with an x-acto
knife. Maybe piling on dielectric or the shark fin would let me tune
impedances down.



--

I yam what I yam - Popeye

 

[Anthony William Sloman]

On Tuesday, December 14, 2021 at 4:18:21 PM UTC+11, jla...@highlandsniptechnology.com wrote:

On Tue, 14 Dec 2021 15:31:53 +1100, Clifford Heath
no....@please.net> wrote:

On 14/12/21 2:47 pm, Rick C wrote:
On Monday, December 13, 2021 at 10:19:34 PM UTC-4, lang...@fonz.dk wrote:
tirsdag den 14. december 2021 kl. 02.36.19 UTC+1 skrev John Larkin:
On Mon, 13 Dec 2021 14:03:55 -0800 (PST), Lasse Langwadt Christensen
lang...@fonz.dk> wrote:

mandag den 13. december 2021 kl. 16.38.35 UTC+1 skrev jla...@highlandsniptechnology.com:
Suppose one had a microstrip trace that was higher impedance than
ideal, but couldn\'t be made wider. One could reduce the distance to
the ground plane, but that might have capacitance consequences
elsewhere.

so add an extra layer for a ground plane close to the microstrip,
but leave it blank where you need low capacitance

standard pcb expect for the special stackup and no extra production steps
It\'s already a 6 layer board. Here\'s the trace, running from the IC to
C28. I want it to be 25 ohms but can\'t make it wide enough. Adding the
coplanar waveguide grounds only helped a little.

https://www.dropbox.com/s/97zkiqidwszo9le/T502_25r_Trace.jpg?raw=1

It might be OK... it\'s pretty short. But if not, maybe I can add
something to pull the impedance down.

I could TDR a microstrip and stick something on top, like a piece of
FR4 or maybe even just some epoxy or something. Yes, I\'ll try that
just to calibrate my expectations.

is is very short and looks you could easily make it shorter

Yeah, he doesn\'t say what he\'s doing. I wonder if he\'s solving the right problem.

Chances are it\'s the 11GHz/25ps laser diode driver from last week, and
he wants to manage the impedance from the die to the coupling capacitor,
at least.

John, you need to use a field solver.

I can easily calculate the trace impedance, but I want 25 ohms and
that\'s not practical on this layout.

It ought to be with parallel traces, stacked vertically if necessary.

The source chip is basically an 80 mA 25 ohm CML source, if you can imagine such a thing. It would source terminate a 25 ohm trace.

ATLC could calculate a microstrip with a slab of dielectric added on
top. But ATLC is basically a 2D analysis and life is 4D : X Y Z T.

And I don\'t have device models, which I\'d need for a serious simulation. Modifying trace impedances up is easy with an x-acto knife.

Not with buried stripline.

> Maybe piling on dielectric or the shark fin would let me tune impedances down.

Or putting two traces in parallel.

This calls for the opposite of a helicopter view - a moles-eye view might work.

11GHz has a wavelenght of about an inch in air - 2.7cm. About 1.8cm in regular dielectrics. It\'s hard to see 0.3cm of track creating much of a problem.

--
Bill Sloman, Sydney

 

[Gerhard Hoffmann]

Am 14.12.21 um 05:27 schrieb jlarkin@highlandsniptechnology.com:

On Mon, 13 Dec 2021 18:19:30 -0800 (PST), Lasse Langwadt Christensen
langwadt@fonz.dk> wrote:

tirsdag den 14. december 2021 kl. 02.36.19 UTC+1 skrev John Larkin:
On Mon, 13 Dec 2021 14:03:55 -0800 (PST), Lasse Langwadt Christensen
lang...@fonz.dk> wrote:

mandag den 13. december 2021 kl. 16.38.35 UTC+1 skrev jla...@highlandsniptechnology.com:
Suppose one had a microstrip trace that was higher impedance than
ideal, but couldn\'t be made wider. One could reduce the distance to
the ground plane, but that might have capacitance consequences
elsewhere.

so add an extra layer for a ground plane close to the microstrip,
but leave it blank where you need low capacitance

standard pcb expect for the special stackup and no extra production steps
It\'s already a 6 layer board. Here\'s the trace, running from the IC to
C28. I want it to be 25 ohms but can\'t make it wide enough. Adding the
coplanar waveguide grounds only helped a little.

https://www.dropbox.com/s/97zkiqidwszo9le/T502_25r_Trace.jpg?raw=1

It might be OK... it\'s pretty short. But if not, maybe I can add
something to pull the impedance down.

I could TDR a microstrip and stick something on top, like a piece of
FR4 or maybe even just some epoxy or something. Yes, I\'ll try that
just to calibrate my expectations.

is is very short and looks you could easily make it shorter

That trace is about 0.12\" long, roughly 20 ps, but I\'ve made it about
as short as I can. There are all sorts of other parts around.

The RF boys measure flatness in dBs but we need PPMs. This is for a
laser modulator for people with extreme expectations.

You could use 2 parallel coplanar wave guides on different
layers or load the top one with additional vias, or use a
higher eps-r material on the top level.

This here is harmless.

In that 10 GBPS XFP transeiver from 15 years ago the laser diode
had to float mechanically, so we used a Kapton tape to connect
it. It also had to switch the layer.

<
https://www.flickr.com/photos/137684711@N07/51746690140/in/dateposted-public/
>

The RF boys used a lot of HFFS simulation time to get it right.
Simulia CST, Keysight EMPRO, HFFS or Sonnet are your friends.

Gerhard

 

[Gerhard Hoffmann]

HFSS, sorry

oh
article
must
contain
real
content

 

[server]

On Tue, 14 Dec 2021 10:29:29 +0100, Gerhard Hoffmann <dk4xp@arcor.de>
wrote:

Am 14.12.21 um 05:27 schrieb jlarkin@highlandsniptechnology.com:
On Mon, 13 Dec 2021 18:19:30 -0800 (PST), Lasse Langwadt Christensen
langwadt@fonz.dk> wrote:

tirsdag den 14. december 2021 kl. 02.36.19 UTC+1 skrev John Larkin:
On Mon, 13 Dec 2021 14:03:55 -0800 (PST), Lasse Langwadt Christensen
lang...@fonz.dk> wrote:

mandag den 13. december 2021 kl. 16.38.35 UTC+1 skrev jla...@highlandsniptechnology.com:
Suppose one had a microstrip trace that was higher impedance than
ideal, but couldn\'t be made wider. One could reduce the distance to
the ground plane, but that might have capacitance consequences
elsewhere.

so add an extra layer for a ground plane close to the microstrip,
but leave it blank where you need low capacitance

standard pcb expect for the special stackup and no extra production steps
It\'s already a 6 layer board. Here\'s the trace, running from the IC to
C28. I want it to be 25 ohms but can\'t make it wide enough. Adding the
coplanar waveguide grounds only helped a little.

https://www.dropbox.com/s/97zkiqidwszo9le/T502_25r_Trace.jpg?raw=1

It might be OK... it\'s pretty short. But if not, maybe I can add
something to pull the impedance down.

I could TDR a microstrip and stick something on top, like a piece of
FR4 or maybe even just some epoxy or something. Yes, I\'ll try that
just to calibrate my expectations.

is is very short and looks you could easily make it shorter

That trace is about 0.12\" long, roughly 20 ps, but I\'ve made it about
as short as I can. There are all sorts of other parts around.

The RF boys measure flatness in dBs but we need PPMs. This is for a
laser modulator for people with extreme expectations.

You could use 2 parallel coplanar wave guides on different
layers or load the top one with additional vias, or use a
higher eps-r material on the top level.

Vias are death at these speeds.

Most microwave laminates are lower Er than FR4, and are exotic and
expensive.

Eval boards for exotic amps are usually very skinny coplanar waveguide
on very thin microwave laminates, and assume external bias tees and DC
blocks and manually tweaked power and bias supplies.

https://www.dropbox.com/s/eeypzso4dz4wz25/HMC_Eval_Board.webp?raw=1

which is fine if that\'s all you want to do.

This here is harmless.

In that 10 GBPS XFP transeiver from 15 years ago the laser diode
had to float mechanically, so we used a Kapton tape to connect
it. It also had to switch the layer.


https://www.flickr.com/photos/137684711@N07/51746690140/in/dateposted-public/


The RF boys used a lot of HFFS simulation time to get it right.
Simulia CST, Keysight EMPRO, HFFS or Sonnet are your friends.

Gerhard

Unfortunately, we don\'t have device models for the critical parts, and
certainly not nonlinear Spice models. So it\'s faster to etch boards
and futz with them than buy and learn and run and fight licensing
issues on expensive simulators.

We\'re doing large-signal high precision pulses with RF parts. The RF
specs are only suggestive and often deceptive.



--

I yam what I yam - Popeye

 

[Phil Hobbs]

jlarkin@highlandsniptechnology.com wrote:

Suppose one had a microstrip trace that was higher impedance than
ideal, but couldn\'t be made wider. One could reduce the distance to
the ground plane, but that might have capacitance consequences
elsewhere.

I wonder if one could add a vertical conductor, sort of a shark fin,
to make the conductor have a t-shaped cross section.

I guess ATLC could analyze that. I might try it after I actually wake
up.

One could also glue a chunk of dielectric to the top of the trace,
with optional copper on top. Make it into a sort of stripline.

I suspect that a fin would be disappointing for that use--the fringing
fields aren\'t that different unless the fin is tall, and in any case
they have to take a long path in air before reaching the ground plane.

Thin copperclad Kapton tape would probably work for this. There will be
issues at low frequency because of the capacitive impedance in series
with the return current from the top copper layer, but for a trace that
short, you don\'t care about low frequency reflections very much. It
should be pretty doable if there aren\'t a lot of top-level traces nearby
to cause crosstalk.

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

 

[server]

On Tue, 14 Dec 2021 10:08:03 -0500, Phil Hobbs
<pcdhSpamMeSenseless@electrooptical.net> wrote:

jlarkin@highlandsniptechnology.com wrote:
Suppose one had a microstrip trace that was higher impedance than
ideal, but couldn\'t be made wider. One could reduce the distance to
the ground plane, but that might have capacitance consequences
elsewhere.

I wonder if one could add a vertical conductor, sort of a shark fin,
to make the conductor have a t-shaped cross section.

I guess ATLC could analyze that. I might try it after I actually wake
up.

One could also glue a chunk of dielectric to the top of the trace,
with optional copper on top. Make it into a sort of stripline.

I suspect that a fin would be disappointing for that use--the fringing
fields aren\'t that different unless the fin is tall, and in any case
they have to take a long path in air before reaching the ground plane.

Thin copperclad Kapton tape would probably work for this. There will be
issues at low frequency because of the capacitive impedance in series
with the return current from the top copper layer, but for a trace that
short, you don\'t care about low frequency reflections very much. It
should be pretty doable if there aren\'t a lot of top-level traces nearby
to cause crosstalk.

Cheers

Phil Hobbs

I should have cut away solder mask so I could hang some tiny caps
between the trace and the cpw grounds, to pull the impedance down, or
possibly use resistors for damping. The mask could be scraped.



--

I yam what I yam - Popeye

 

[Lasse Langwadt Christensen]

tirsdag den 14. december 2021 kl. 05.27.11 UTC+1 skrev jla...@highlandsniptechnology.com:

On Mon, 13 Dec 2021 18:19:30 -0800 (PST), Lasse Langwadt Christensen
lang...@fonz.dk> wrote:

tirsdag den 14. december 2021 kl. 02.36.19 UTC+1 skrev John Larkin:
On Mon, 13 Dec 2021 14:03:55 -0800 (PST), Lasse Langwadt Christensen
lang...@fonz.dk> wrote:

mandag den 13. december 2021 kl. 16.38.35 UTC+1 skrev jla...@highlandsniptechnology.com:
Suppose one had a microstrip trace that was higher impedance than
ideal, but couldn\'t be made wider. One could reduce the distance to
the ground plane, but that might have capacitance consequences
elsewhere.

so add an extra layer for a ground plane close to the microstrip,
but leave it blank where you need low capacitance

standard pcb expect for the special stackup and no extra production steps
It\'s already a 6 layer board. Here\'s the trace, running from the IC to
C28. I want it to be 25 ohms but can\'t make it wide enough. Adding the
coplanar waveguide grounds only helped a little.

https://www.dropbox.com/s/97zkiqidwszo9le/T502_25r_Trace.jpg?raw=1

It might be OK... it\'s pretty short. But if not, maybe I can add
something to pull the impedance down.

I could TDR a microstrip and stick something on top, like a piece of
FR4 or maybe even just some epoxy or something. Yes, I\'ll try that
just to calibrate my expectations.

is is very short and looks you could easily make it shorter
That trace is about 0.12\" long, roughly 20 ps, but I\'ve made it about
as short as I can. There are all sorts of other parts around.

just move C28 to the left, right up against the IC ?

 

[Clifford Heath]

On 14/12/21 8:29 pm, Gerhard Hoffmann wrote:

Am 14.12.21 um 05:27 schrieb jlarkin@highlandsniptechnology.com:
The RF boys used a lot of HFFS simulation time to get it right.
Simulia CST, Keysight EMPRO, HFFS or Sonnet are your friends.

Exactly what I told him also. Anything else is just a stab in the dark.
It\'s not like you can probe it afterward to see why it\'s not working well.

CH

 

[Gerhard Hoffmann]

Am 14.12.21 um 22:26 schrieb Clifford Heath:

On 14/12/21 8:29 pm, Gerhard Hoffmann wrote:
Am 14.12.21 um 05:27 schrieb jlarkin@highlandsniptechnology.com:
The RF boys used a lot of HFFS simulation time to get it right.
Simulia CST, Keysight EMPRO, HFFS or Sonnet are your friends.

Exactly what I told him also. Anything else is just a stab in the dark.
It\'s not like you can probe it afterward to see why it\'s not working well.

Esp. when the problem at hand has nothing to do with
nonlinearities. This is a 2.5 or 3D electromagnetics problem.
And that includes the TO-whatever box of the laser.

It could be co-simulated with ADS/EMpro, ADS taking care
of the spice-like parts. pHEMT support/modelling is probably
better in (ADS or similar) than in LTspice.

cheers, Gerhard

 

[Anthony William Sloman]

On Wednesday, December 15, 2021 at 1:31:14 AM UTC+11, jla...@highlandsniptechnology.com wrote:

On Tue, 14 Dec 2021 10:29:29 +0100, Gerhard Hoffmann <dk...@arcor.de
wrote:
Am 14.12.21 um 05:27 schrieb jla...@highlandsniptechnology.com:
On Mon, 13 Dec 2021 18:19:30 -0800 (PST), Lasse Langwadt Christensen
lang...@fonz.dk> wrote:

tirsdag den 14. december 2021 kl. 02.36.19 UTC+1 skrev John Larkin:
On Mon, 13 Dec 2021 14:03:55 -0800 (PST), Lasse Langwadt Christensen
lang...@fonz.dk> wrote:

mandag den 13. december 2021 kl. 16.38.35 UTC+1 skrev jla...@highlandsniptechnology.com:

<snip>

is is very short and looks you could easily make it shorter

That trace is about 0.12\" long, roughly 20 ps, but I\'ve made it about
as short as I can. There are all sorts of other parts around.

The RF boys measure flatness in dBs but we need PPMs. This is for a
laser modulator for people with extreme expectations.

You could use 2 parallel coplanar wave guides on different layers or load the top one with additional vias, or use a higher eps-r material on the top level.
Vias are death at these speeds.

Except at the source and the termination.

Most microwave laminates are lower Er than FR4, and are exotic and expensive.

And a whole lot better behaved that FR4. The glass fibres that the FR4 epoxy resin ties together don\'t have a uniform density, so you get fluctuations in trace impedance along the trace.

If you want to push 11GHz through your board, epoxy resin-bonded glass fibre is a remarkably poor choice.

We didn\'t have any trouble getting stuff made on Rogers microwave substrates back in the late 1980s in the UK. They maybe somewhat exotic and a bit more expensive, but they are a whole lot more likely to give you a well behaved assembly. This ought to matter to you

> Eval boards for exotic amps are usually very skinny coplanar waveguide on very thin microwave laminates, and assume external bias tees and DC blocks and manually tweaked power and bias supplies.

So they know where to spend their money, even if you don\'t.

<snip>

> Unfortunately, we don\'t have device models for the critical parts, and certainly not nonlinear Spice models. So it\'s faster to etch boards and futz with them than buy and learn and run and fight licensing issues on expensive simulators.

It might help if you etched boards that used a more suitable substrate than FR4.

> We\'re doing large-signal high precision pulses with RF parts.

That\'s what you have been asked to, and may be what you are trying to do, but FR4 epoxy-glass substrates won\'t help it you need 11HGz bandwidth

> The RF-specs are only suggestive and often deceptive.

Particularly when you don\'t read them carefully.

--
Bill Sloman, Sydney