LC oscillator sensitivity analysis

I'm designing a 125 MHz triggered LC oscillator. It's sufficiently
nonlinear that I need to Spice it in transient/time domain mode. I
want to explore frequency sensitivity to component values, supply
voltages, stuff like that.

But how to measure frequency accurately? Cursoring one cycle of
oscillation on the screen is pretty crude.

I guess I could use a delay line to compare the time of one edge to
the previous one, essentially zoom the period.

Or just note the absolute time of the zero cross of the 100th edge,
and calculate from that. Analyzing oscillators in time domain is
always tedious. I'm running this at 1 ps steps, so the sim runs are
slow even before I try to measure frequency. Running with the LT Spice
defaults does obviously weird things.

Any suggestions?



--

John Larkin Highland Technology, Inc

The cork popped merrily, and Lord Peter rose to his feet.
"Bunter", he said, "I give you a toast. The triumph of Instinct over Reason"

 

[Martin Brown]

On 04/03/2020 16:29, jlarkin@highlandsniptechnology.com wrote:

I'm designing a 125 MHz triggered LC oscillator. It's sufficiently
nonlinear that I need to Spice it in transient/time domain mode. I
want to explore frequency sensitivity to component values, supply
voltages, stuff like that.

But how to measure frequency accurately? Cursoring one cycle of
oscillation on the screen is pretty crude.

Add it to an equal amplitude reference frequency or two and use the
interference beats patterns to work out the frequency difference.

I guess I could use a delay line to compare the time of one edge to
the previous one, essentially zoom the period.

Or just note the absolute time of the zero cross of the 100th edge,
and calculate from that. Analyzing oscillators in time domain is
always tedious. I'm running this at 1 ps steps, so the sim runs are
slow even before I try to measure frequency. Running with the LT Spice
defaults does obviously weird things.

Any suggestions?

Classic trick once you have a rough period and an estimate of error on
that is to run for long enough to get a max cumulative error of 1/4
cycle and then knowing it was an exact number of cycles refine the estimate.


--
Regards,
Martin Brown

 

[Phil Hobbs]

On 2020-03-04 11:29, jlarkin@highlandsniptechnology.com wrote:

I'm designing a 125 MHz triggered LC oscillator. It's sufficiently
nonlinear that I need to Spice it in transient/time domain mode. I
want to explore frequency sensitivity to component values, supply
voltages, stuff like that.

But how to measure frequency accurately? Cursoring one cycle of
oscillation on the screen is pretty crude.

I guess I could use a delay line to compare the time of one edge to
the previous one, essentially zoom the period.

Or just note the absolute time of the zero cross of the 100th edge,
and calculate from that. Analyzing oscillators in time domain is
always tedious. I'm running this at 1 ps steps, so the sim runs are
slow even before I try to measure frequency. Running with the LT Spice
defaults does obviously weird things.

Any suggestions?

A long T-line and a bv source configured as a multiplier would give you
a delay discriminator, which can do a pretty good job if you filter the
output. The good news is that you average over many cycles, which gets
rid of the adaptive step size funnies.

Cheers

Phil Hobbs

--
Dr Philip C D Hobbs
Principal Consultant
ElectroOptical Innovations LLC
Optics, Electro-optics, Photonics, Analog Electronics

160 North State Road #203
Briarcliff Manor NY 10510

hobbs at electrooptical dot net
http://electrooptical.net

 

Frequency can only be as accurate as the time you are allowing for the measurement. Are you trying to get a cw measurement or the value of the frequency while in sweep mode

 

[John Larkin]

On Wed, 4 Mar 2020 14:37:01 -0500, Phil Hobbs
<pcdhSpamMeSenseless@electrooptical.net> wrote:

On 2020-03-04 11:29, jlarkin@highlandsniptechnology.com wrote:


I'm designing a 125 MHz triggered LC oscillator. It's sufficiently
nonlinear that I need to Spice it in transient/time domain mode. I
want to explore frequency sensitivity to component values, supply
voltages, stuff like that.

But how to measure frequency accurately? Cursoring one cycle of
oscillation on the screen is pretty crude.

I guess I could use a delay line to compare the time of one edge to
the previous one, essentially zoom the period.

Or just note the absolute time of the zero cross of the 100th edge,
and calculate from that. Analyzing oscillators in time domain is
always tedious. I'm running this at 1 ps steps, so the sim runs are
slow even before I try to measure frequency. Running with the LT Spice
defaults does obviously weird things.

Any suggestions?

A long T-line and a bv source configured as a multiplier would give you
a delay discriminator, which can do a pretty good job if you filter the
output. The good news is that you average over many cycles, which gets
rid of the adaptive step size funnies.

Cheers

Phil Hobbs

I can make fairly large changes to part values, and then zoom up one
cycle of oscillation, or maybe a few, and use the cursors to show me
period and frequency, and then calculate sensitivities. That assumes,
well, linearity of my non-linearities. Tedious, but it will mostly
work.

I'm running a time step of 1 ps. The defaults are obviously goofy.

One big nasty is the tempco of the FR4 PCB capacitances. Guarding is a
remote possibility.

I'd still like you to review this for us, when I can get organized
enough.


--

John Larkin Highland Technology, Inc
picosecond timing precision measurement

jlarkin att highlandtechnology dott com
http://www.highlandtechnology.com

 

[Phil Hobbs]

On 2020-03-04 14:50, John Larkin wrote:

On Wed, 4 Mar 2020 14:37:01 -0500, Phil Hobbs
pcdhSpamMeSenseless@electrooptical.net> wrote:

On 2020-03-04 11:29, jlarkin@highlandsniptechnology.com wrote:


I'm designing a 125 MHz triggered LC oscillator. It's sufficiently
nonlinear that I need to Spice it in transient/time domain mode. I
want to explore frequency sensitivity to component values, supply
voltages, stuff like that.

But how to measure frequency accurately? Cursoring one cycle of
oscillation on the screen is pretty crude.

I guess I could use a delay line to compare the time of one edge to
the previous one, essentially zoom the period.

Or just note the absolute time of the zero cross of the 100th edge,
and calculate from that. Analyzing oscillators in time domain is
always tedious. I'm running this at 1 ps steps, so the sim runs are
slow even before I try to measure frequency. Running with the LT Spice
defaults does obviously weird things.

Any suggestions?

A long T-line and a bv source configured as a multiplier would give you
a delay discriminator, which can do a pretty good job if you filter the
output. The good news is that you average over many cycles, which gets
rid of the adaptive step size funnies.

Cheers

Phil Hobbs

I can make fairly large changes to part values, and then zoom up one
cycle of oscillation, or maybe a few, and use the cursors to show me
period and frequency, and then calculate sensitivities. That assumes,
well, linearity of my non-linearities. Tedious, but it will mostly
work.

You have to do a whole run per time, so the delay discrim ought to work
fine. "Long" doesn't have to mean a million cycles--it's being done in
floating point after all. Ten or twenty cycles should be lots.

I'm running a time step of 1 ps. The defaults are obviously goofy.

One big nasty is the tempco of the FR4 PCB capacitances. Guarding is a
remote possibility.

I'd still like you to review this for us, when I can get organized
enough.

Sure, sounds like fun.

Cheers

Phil

--
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

 

On Wed, 04 Mar 2020 08:29:11 -0800, jlarkin wrote:

I'm designing a 125 MHz triggered LC oscillator. It's sufficiently
nonlinear that I need to Spice it in transient/time domain mode. I want
to explore frequency sensitivity to component values, supply voltages,
stuff like that.

But how to measure frequency accurately? Cursoring one cycle of
oscillation on the screen is pretty crude.

I guess I could use a delay line to compare the time of one edge to the
previous one, essentially zoom the period.

Or just note the absolute time of the zero cross of the 100th edge, and
calculate from that. Analyzing oscillators in time domain is always
tedious. I'm running this at 1 ps steps, so the sim runs are slow even
before I try to measure frequency. Running with the LT Spice defaults
does obviously weird things.

Any suggestions?

I put these statements in the sim:

..meas t1 find time when v(tank_p,tank_n)=0 cross=1 td=100u
..meas t2 find time when v(tank_p,tank_n)=0 cross=4001 td=100u
..meas f_tank param 2000/(t2-t1)

The td=100u is to skip the startup time of the oscillator. The 2000
cycles was arrived at after I kept increasing the number until the
measurement stabilised. There are still some rounding-error issues in
there I think.

I was using a max time step of 500 ps, which is about as much as I could
tolerate. There is probably some optimum combination of time step and
number of cycles, but I didn't spend much time trying to find it after
the other problems became apparent.

The real limitation of this approach is that the LTSPICE inductor doesn't
accurately model core losses, and how they change with current and
temperature (it just has a parallel resistance). The manufacturers don't
often quote this anyway, so I had to buy lots of samples and measure them.

If you're using an air-cored inductor, of course, a lot of these issues
go away, but you still have to deal with skin effect and dielectric loss
in the FR4, and the dependence of these on temperature.

On top of all of the above, it turned out that our first choice of
inductor was also sensitive to humidity, it looks like the wire
insulation is hygroscopic and the stray capacitance drifts over a period
of hours or days. That one caused a lot of head scratching.

Our application is trying to measure small changes in capacitance, about
1-2 pF with an offset of ~ 150 pF, so small changes in parasitics can
completely screw up the measurement.

This stuff is a lot harder than anybody imagined at the start of the
project. Good luck...

 

[Bill Sloman]

On Thursday, March 5, 2020 at 7:49:59 PM UTC+11, ne...@rblack01.plus.com wrote:
> On Wed, 04 Mar 2020 08:29:11 -0800, jlarkin wrote:

<snip>

The real limitation of this approach is that the LTSPICE inductor doesn't
accurately model core losses, and how they change with current and
temperature (it just has a parallel resistance).

LTSpice offers the John Chan model of a hysteretic inductor, which may be more realistic.

"The other non-linear inductor available in LTspice is a hysteretic core model based on a model first proposed in by John Chan et la. in IEEE Transactions On Computer-Aided Design, Vol. 10. No. 4, April 1991 but extended with the methods in United States Patent 7,502,723. "

I didn't have any trouble digging the parameter out of the data sheet for the core I was using

The manufacturers don't
often quote this anyway, so I had to buy lots of samples and measure them..

If you're using an air-cored inductor, of course, a lot of these issues
go away, but you still have to deal with skin effect and dielectric loss
in the FR4, and the dependence of these on temperature.

On top of all of the above, it turned out that our first choice of
inductor was also sensitive to humidity, it looks like the wire
insulation is hygroscopic and the stray capacitance drifts over a period
of hours or days. That one caused a lot of head scratching.

Our application is trying to measure small changes in capacitance, about
1-2 pF with an offset of ~ 150 pF, so small changes in parasitics can
completely screw up the measurement.

This stuff is a lot harder than anybody imagined at the start of the
project. Good luck...

Sounds like a job for a Blumlein bridge.

Centre-tapped transformers wound with twisted pair (and certain amount of attention to detail) offer a 1:1 ratio that is accurate to about one part in a billion.

Ratio transformers are somewhat more flexible, but the precision goes down to about one part in ten million.

These are a few of the many interesting facts you can find in

https://www.amazon.com/Coaxial-AC-Bridges-B-Kibble/dp/0852743890

The Kibble is the guy whose name got recorded in the Kibble balance

https://en.wikipedia.org/wiki/Kibble_balance

--
Bill Sloman, Sydney

 

On Thu, 5 Mar 2020 08:49:53 -0000 (UTC), news@rblack01.plus.com wrote:

On Wed, 04 Mar 2020 08:29:11 -0800, jlarkin wrote:

I'm designing a 125 MHz triggered LC oscillator. It's sufficiently
nonlinear that I need to Spice it in transient/time domain mode. I want
to explore frequency sensitivity to component values, supply voltages,
stuff like that.

But how to measure frequency accurately? Cursoring one cycle of
oscillation on the screen is pretty crude.

I guess I could use a delay line to compare the time of one edge to the
previous one, essentially zoom the period.

Or just note the absolute time of the zero cross of the 100th edge, and
calculate from that. Analyzing oscillators in time domain is always
tedious. I'm running this at 1 ps steps, so the sim runs are slow even
before I try to measure frequency. Running with the LT Spice defaults
does obviously weird things.

Any suggestions?

I put these statements in the sim:

.meas t1 find time when v(tank_p,tank_n)=0 cross=1 td=100u
.meas t2 find time when v(tank_p,tank_n)=0 cross=4001 td=100u
.meas f_tank param 2000/(t2-t1)

The td=100u is to skip the startup time of the oscillator. The 2000
cycles was arrived at after I kept increasing the number until the
measurement stabilised. There are still some rounding-error issues in
there I think.

That's cool. I haven't used .meas. I'll have to learn that.

I was using a max time step of 500 ps, which is about as much as I could
tolerate. There is probably some optimum combination of time step and
number of cycles, but I didn't spend much time trying to find it after
the other problems became apparent.

I'm running 5 ps time steps, for a 1 us run, which seems good enough.
Smaller steps don't seem to change my frequency. The LT Spice default
step delivers nonsense.

The real limitation of this approach is that the LTSPICE inductor doesn't
accurately model core losses, and how they change with current and
temperature (it just has a parallel resistance). The manufacturers don't
often quote this anyway, so I had to buy lots of samples and measure them.

If you're using an air-cored inductor, of course, a lot of these issues
go away, but you still have to deal with skin effect and dielectric loss
in the FR4, and the dependence of these on temperature.

I'll be using a high-Q Coilcraft air-core inductor. I do wonder how it
interacts with the PCB copper planes.

Skin effect shouldn't much affect my 125 MHz Colpitts oscillator, but
FR4 is a horrible capacitor.

https://www.dropbox.com/s/nur4f8aw7akiz7h/FR4_Tempco.JPG?raw=1

I have also been experimenting with measuring risetimes of short
microstrips on FR4, between two SMA connectors. We have an ongoing
debate here about when it's necessary to pay for exotic laminates.

On top of all of the above, it turned out that our first choice of
inductor was also sensitive to humidity, it looks like the wire
insulation is hygroscopic and the stray capacitance drifts over a period
of hours or days. That one caused a lot of head scratching.

I used one coil that was wound on a plastic coil former. It looked
very nice but it slowly changed inductance as the coil tension made
the thermoplastic flow. The time constant was months. The short-term
fix was to bake all the inductors to relieve the stress. The long-term
fix was to buy something else.

Our application is trying to measure small changes in capacitance, about
1-2 pF with an offset of ~ 150 pF, so small changes in parasitics can
completely screw up the measurement.

This stuff is a lot harder than anybody imagined at the start of the
project. Good luck...

Yes. I'm doing an instant-start, instant-stop, phase-locked
oscillator, with a goal of 1 ps RMS jitter on every edge. Pray for me.



--

John Larkin Highland Technology, Inc

The cork popped merrily, and Lord Peter rose to his feet.
"Bunter", he said, "I give you a toast. The triumph of Instinct over Reason"

 

[Bill Sloman]

On Friday, March 6, 2020 at 3:29:16 AM UTC+11, jla...@highlandsniptechnology.com wrote:

On Thu, 5 Mar 2020 08:49:53 -0000 (UTC), news@rblack01.plus.com wrote:

On Wed, 04 Mar 2020 08:29:11 -0800, jlarkin wrote:

<snip>

Yes. I'm doing an instant-start, instant-stop, phase-locked
oscillator, with a goal of 1 ps RMS jitter on every edge. Pray for me.

It's a diabolically cheap and nasty approach to precision timing.

Exorcism is the kind of prayer mode that would be appropriate.

Use two time-to-digital converters to locate the leading and trailing edges with respect to the edges of a stable and continuously running clock - I was looking at a clock running at 800MHz when I did it, thirty years ago, but that was driven by a manager who wanted something that he could make silly claims about when he was selling it.

This approach gets expensive when you want it to deliver up edge-to-edge times at MHz rates - fast A/D converters aren't cheap - but it does lend itself to frequent auto-calibration.

Obviously you have to pay for a fast, stable low jitter oscillator, but these are off-the-shelf parts (if not all that cheap).

--
Bill Sloman, Sydney

 

On Thu, 05 Mar 2020 05:30:32 -0800, Bill Sloman wrote:

On Thursday, March 5, 2020 at 7:49:59 PM UTC+11, ne...@rblack01.plus.com
wrote:
On Wed, 04 Mar 2020 08:29:11 -0800, jlarkin wrote:

snip

The real limitation of this approach is that the LTSPICE inductor
doesn't accurately model core losses, and how they change with current
and temperature (it just has a parallel resistance).

LTSpice offers the John Chan model of a hysteretic inductor, which may
be more realistic.

"The other non-linear inductor available in LTspice is a hysteretic core
model based on a model first proposed in by John Chan et la. in IEEE
Transactions On Computer-Aided Design, Vol. 10. No. 4, April 1991 but
extended with the methods in United States Patent 7,502,723. "

You mean this one?
http://ltwiki.org/LTspiceHelp/LTspiceHelp/L_Inductor.htm (bottom of page)
http://ltwiki.org/index.php?title=The_Chan_model

I had a quick play with it, using the example example model in the second
link. I don't have time to look into it in any more depth right now, but
worth adding to the toolbox.

I didn't have any trouble digging the parameter out of the data sheet
for the core I was using.

I'm using 1210 surface-mount inductors from the likes of TDK, Murata,
Wurth. I think one of the Murata ones had a SPICE model but it didn't
include non-linearity or behaviour over temperature. The other vendors
just have bare data sheets with 'typical' values or impedance curves at
room temperature. Measuring the parts ended up being quicker than trying
to model them.

[snip]

Sounds like a job for a Blumlein bridge.

Centre-tapped transformers wound with twisted pair (and certain amount
of attention to detail) offer a 1:1 ratio that is accurate to about one
part in a billion.

Ratio transformers are somewhat more flexible, but the precision goes
down to about one part in ten million.

These are a few of the many interesting facts you can find in

https://www.amazon.com/Coaxial-AC-Bridges-B-Kibble/dp/0852743890

The Kibble is the guy whose name got recorded in the Kibble balance

https://en.wikipedia.org/wiki/Kibble_balance

Custom magnetics would be an absolute last resort for this one. The
whole PCB is about the size of a stick of gum, none of the cores I can
find would fit. Plus this is an area I have very little experience of,
throwing another steep learning curve into the mix at this point wouldn't
endear me to my boss.

I do have a reference capacitor, being measured by an identical circuit,
and doing the ratiometric stuff in software, which works well enough to
correct the temperature drift. The humidity drift is a harder problem,
mainly because it takes so much longer to measure.

 

On Thu, 05 Mar 2020 08:29:04 -0800, jlarkin wrote:

On Thu, 5 Mar 2020 08:49:53 -0000 (UTC), news@rblack01.plus.com wrote:

On Wed, 04 Mar 2020 08:29:11 -0800, jlarkin wrote:

I'm designing a 125 MHz triggered LC oscillator. It's sufficiently
nonlinear that I need to Spice it in transient/time domain mode. I
want to explore frequency sensitivity to component values, supply
voltages, stuff like that.

But how to measure frequency accurately? Cursoring one cycle of
oscillation on the screen is pretty crude.

I guess I could use a delay line to compare the time of one edge to
the previous one, essentially zoom the period.

Or just note the absolute time of the zero cross of the 100th edge,
and calculate from that. Analyzing oscillators in time domain is
always tedious. I'm running this at 1 ps steps, so the sim runs are
slow even before I try to measure frequency. Running with the LT Spice
defaults does obviously weird things.

Any suggestions?

I put these statements in the sim:

.meas t1 find time when v(tank_p,tank_n)=0 cross=1 td=100u .meas t2 find
time when v(tank_p,tank_n)=0 cross=4001 td=100u .meas f_tank param
2000/(t2-t1)

The td=100u is to skip the startup time of the oscillator. The 2000
cycles was arrived at after I kept increasing the number until the
measurement stabilised. There are still some rounding-error issues in
there I think.

That's cool. I haven't used .meas. I'll have to learn that.


I was using a max time step of 500 ps, which is about as much as I could
tolerate. There is probably some optimum combination of time step and
number of cycles, but I didn't spend much time trying to find it after
the other problems became apparent.

I'm running 5 ps time steps, for a 1 us run, which seems good enough.
Smaller steps don't seem to change my frequency. The LT Spice default
step delivers nonsense.

[snip]

I'll be using a high-Q Coilcraft air-core inductor. I do wonder how it
interacts with the PCB copper planes.

I did consider an air-core inductor, but I need a few tens of uH, and it
wouldn't fit in the product. Also there is no overall shielding in this
one apart from the PCB ground plane, and I can see it would end up
becoming a Theremin.

Skin effect shouldn't much affect my 125 MHz Colpitts oscillator, but
FR4 is a horrible capacitor.

https://www.dropbox.com/s/nur4f8aw7akiz7h/FR4_Tempco.JPG?raw=1

Cool. That is a much straighter line than I would expect. Was that done
using a DMM?

I have also been experimenting with measuring risetimes of short
microstrips on FR4, between two SMA connectors. We have an ongoing
debate here about when it's necessary to pay for exotic laminates.

I've never done anything high enough frequency to have to worry about
dispersion etc. But the FR4 was definitely part of the humidity drift
problem. None of the PCB laminate vendors we approached would commit to
the orders-of-magnitude lower moisture absorption we were asking for, so
we're sticking with FR4 for now.

On top of all of the above, it turned out that our first choice of
inductor was also sensitive to humidity, it looks like the wire
insulation is hygroscopic and the stray capacitance drifts over a period
of hours or days. That one caused a lot of head scratching.

I used one coil that was wound on a plastic coil former. It looked very
nice but it slowly changed inductance as the coil tension made the
thermoplastic flow. The time constant was months. The short-term fix was
to bake all the inductors to relieve the stress. The long-term fix was
to buy something else.

It turns out the customer can accept nulling out the drift at the start
of each day, they have a lot of other measurements where they have to do
this so it's not too big a deal. It's a lot easier to hit than our
originally planned 12 month calibration interval.

 

On Thu, 05 Mar 2020 08:29:04 -0800, jlarkin wrote:

On Thu, 5 Mar 2020 08:49:53 -0000 (UTC), news@rblack01.plus.com wrote:

On Wed, 04 Mar 2020 08:29:11 -0800, jlarkin wrote:

I'm designing a 125 MHz triggered LC oscillator. It's sufficiently
nonlinear that I need to Spice it in transient/time domain mode. I
want to explore frequency sensitivity to component values, supply
voltages, stuff like that.

But how to measure frequency accurately? Cursoring one cycle of
oscillation on the screen is pretty crude.

I guess I could use a delay line to compare the time of one edge to
the previous one, essentially zoom the period.

Or just note the absolute time of the zero cross of the 100th edge,
and calculate from that. Analyzing oscillators in time domain is
always tedious. I'm running this at 1 ps steps, so the sim runs are
slow even before I try to measure frequency. Running with the LT Spice
defaults does obviously weird things.

Any suggestions?

I put these statements in the sim:

.meas t1 find time when v(tank_p,tank_n)=0 cross=1 td=100u .meas t2 find
time when v(tank_p,tank_n)=0 cross=4001 td=100u .meas f_tank param
2000/(t2-t1)

The td=100u is to skip the startup time of the oscillator. The 2000
cycles was arrived at after I kept increasing the number until the
measurement stabilised. There are still some rounding-error issues in
there I think.

That's cool. I haven't used .meas. I'll have to learn that.


I was using a max time step of 500 ps, which is about as much as I could
tolerate. There is probably some optimum combination of time step and
number of cycles, but I didn't spend much time trying to find it after
the other problems became apparent.

I'm running 5 ps time steps, for a 1 us run, which seems good enough.
Smaller steps don't seem to change my frequency. The LT Spice default
step delivers nonsense.

[snip]

I'll be using a high-Q Coilcraft air-core inductor. I do wonder how it
interacts with the PCB copper planes.

I did consider an air-core inductor, but I need a few tens of uH, and it
wouldn't fit in the product. Also there is no overall shielding in this
one apart from the PCB ground plane, and I can see it would end up
becoming a Theremin.

Skin effect shouldn't much affect my 125 MHz Colpitts oscillator, but
FR4 is a horrible capacitor.

https://www.dropbox.com/s/nur4f8aw7akiz7h/FR4_Tempco.JPG?raw=1

Cool. That is a much straighter line than I would expect. Was that done
using a DMM?

I have also been experimenting with measuring risetimes of short
microstrips on FR4, between two SMA connectors. We have an ongoing
debate here about when it's necessary to pay for exotic laminates.

I've never done anything high enough frequency to have to worry about
dispersion etc. But the FR4 was definitely part of the humidity drift
problem. None of the PCB laminate vendors we approached would commit to
the orders-of-magnitude lower moisture absorption we were asking for, so
we're sticking with FR4 for now.

On top of all of the above, it turned out that our first choice of
inductor was also sensitive to humidity, it looks like the wire
insulation is hygroscopic and the stray capacitance drifts over a period
of hours or days. That one caused a lot of head scratching.

I used one coil that was wound on a plastic coil former. It looked very
nice but it slowly changed inductance as the coil tension made the
thermoplastic flow. The time constant was months. The short-term fix was
to bake all the inductors to relieve the stress. The long-term fix was
to buy something else.

It turns out the customer can accept nulling out the drift at the start
of each day, they have a lot of other measurements where they have to do
this so it's not too big a deal. It's a lot easier to hit than our
originally planned 12 month calibration interval.

 

[Bill Sloman]

On Friday, March 6, 2020 at 7:40:18 PM UTC+11, ne...@rblack01.plus.com wrote:

On Thu, 05 Mar 2020 05:30:32 -0800, Bill Sloman wrote:

On Thursday, March 5, 2020 at 7:49:59 PM UTC+11, ne...@rblack01.plus.com
wrote:
On Wed, 04 Mar 2020 08:29:11 -0800, jlarkin wrote:

snip

The real limitation of this approach is that the LTSPICE inductor
doesn't accurately model core losses, and how they change with current
and temperature (it just has a parallel resistance).

LTSpice offers the John Chan model of a hysteretic inductor, which may
be more realistic.

"The other non-linear inductor available in LTspice is a hysteretic core
model based on a model first proposed in by John Chan et la. in IEEE
Transactions On Computer-Aided Design, Vol. 10. No. 4, April 1991 but
extended with the methods in United States Patent 7,502,723. "


You mean this one?
http://ltwiki.org/LTspiceHelp/LTspiceHelp/L_Inductor.htm (bottom of page)
http://ltwiki.org/index.php?title=The_Chan_model

I had a quick play with it, using the example example model in the second
link. I don't have time to look into it in any more depth right now, but
worth adding to the toolbox.

I didn't have any trouble digging the parameter out of the data sheet
for the core I was using.

I'm using 1210 surface-mount inductors from the likes of TDK, Murata,
Wurth.

Ouch. You'd need to identify the core material.

I think one of the Murata ones had a SPICE model but it didn't
include non-linearity or behaviour over temperature. The other vendors
just have bare data sheets with 'typical' values or impedance curves at
room temperature. Measuring the parts ended up being quicker than trying
to model them.

[snip]


Sounds like a job for a Blumlein bridge.

Centre-tapped transformers wound with twisted pair (and certain amount
of attention to detail) offer a 1:1 ratio that is accurate to about one
part in a billion.

Ratio transformers are somewhat more flexible, but the precision goes
down to about one part in ten million.

These are a few of the many interesting facts you can find in

https://www.amazon.com/Coaxial-AC-Bridges-B-Kibble/dp/0852743890

The Kibble is the guy whose name got recorded in the Kibble balance

https://en.wikipedia.org/wiki/Kibble_balance

Custom magnetics would be an absolute last resort for this one. The
whole PCB is about the size of a stick of gum, none of the cores I can
find would fit. Plus this is an area I have very little experience of,
throwing another steep learning curve into the mix at this point wouldn't
endear me to my boss.

Perhaps, but getting stuck with complicated job and a half-baked scheme to tackle it is the kind of thing that inept bosses do to their subordinates.

There are some fairly compact cores designed to be integrated with printed circuit windings

http://www.farnell.com/datasheets/1524995.pdf

https://au.mouser.com/datasheet/2/400/tdk_B65523J0000R608-1222076.pdf

You might be able to integrate one of them into a fairly compact solution (and a compact solution is the kind of thing bosses do promise their customers, and have trouble backing away from).

I do have a reference capacitor, being measured by an identical circuit,
and doing the ratiometric stuff in software, which works well enough to
correct the temperature drift. The humidity drift is a harder problem,
mainly because it takes so much longer to measure.

Bridge circuits - particularly one-to-one bridges - don't have that kind of problem.

--
Bill Sloman, Sydney

 

[John S]

On 3/5/2020 10:29 AM, jlarkin@highlandsniptechnology.com wrote:

On Thu, 5 Mar 2020 08:49:53 -0000 (UTC), news@rblack01.plus.com wrote:

On Wed, 04 Mar 2020 08:29:11 -0800, jlarkin wrote:

I'm designing a 125 MHz triggered LC oscillator. It's sufficiently
nonlinear that I need to Spice it in transient/time domain mode. I want
to explore frequency sensitivity to component values, supply voltages,
stuff like that.

But how to measure frequency accurately? Cursoring one cycle of
oscillation on the screen is pretty crude.

I guess I could use a delay line to compare the time of one edge to the
previous one, essentially zoom the period.

Or just note the absolute time of the zero cross of the 100th edge, and
calculate from that. Analyzing oscillators in time domain is always
tedious. I'm running this at 1 ps steps, so the sim runs are slow even
before I try to measure frequency. Running with the LT Spice defaults
does obviously weird things.

Any suggestions?

I put these statements in the sim:

.meas t1 find time when v(tank_p,tank_n)=0 cross=1 td=100u
.meas t2 find time when v(tank_p,tank_n)=0 cross=4001 td=100u
.meas f_tank param 2000/(t2-t1)

The td=100u is to skip the startup time of the oscillator. The 2000
cycles was arrived at after I kept increasing the number until the
measurement stabilised. There are still some rounding-error issues in
there I think.

That's cool. I haven't used .meas. I'll have to learn that.


I was using a max time step of 500 ps, which is about as much as I could
tolerate. There is probably some optimum combination of time step and
number of cycles, but I didn't spend much time trying to find it after
the other problems became apparent.

I'm running 5 ps time steps, for a 1 us run, which seems good enough.
Smaller steps don't seem to change my frequency. The LT Spice default
step delivers nonsense.


The real limitation of this approach is that the LTSPICE inductor doesn't
accurately model core losses, and how they change with current and
temperature (it just has a parallel resistance). The manufacturers don't
often quote this anyway, so I had to buy lots of samples and measure them.

If you're using an air-cored inductor, of course, a lot of these issues
go away, but you still have to deal with skin effect and dielectric loss
in the FR4, and the dependence of these on temperature.

I'll be using a high-Q Coilcraft air-core inductor. I do wonder how it
interacts with the PCB copper planes.

Skin effect shouldn't much affect my 125 MHz Colpitts oscillator, but
FR4 is a horrible capacitor.

https://www.dropbox.com/s/nur4f8aw7akiz7h/FR4_Tempco.JPG?raw=1

Very good data, John. Thanks. I did some analysis to try to understand
your ppm results on the right hand side of your graph. I can't come up
with the same numbers. Did you perhaps mean 89pF rather than 99pF?

Not a big deal in any case. I just want to know if I understand it
correctly.

 

On Fri, 6 Mar 2020 09:02:22 -0000 (UTC), news@rblack01.plus.com wrote:

On Thu, 05 Mar 2020 08:29:04 -0800, jlarkin wrote:

On Thu, 5 Mar 2020 08:49:53 -0000 (UTC), news@rblack01.plus.com wrote:

On Wed, 04 Mar 2020 08:29:11 -0800, jlarkin wrote:

I'm designing a 125 MHz triggered LC oscillator. It's sufficiently
nonlinear that I need to Spice it in transient/time domain mode. I
want to explore frequency sensitivity to component values, supply
voltages, stuff like that.

But how to measure frequency accurately? Cursoring one cycle of
oscillation on the screen is pretty crude.

I guess I could use a delay line to compare the time of one edge to
the previous one, essentially zoom the period.

Or just note the absolute time of the zero cross of the 100th edge,
and calculate from that. Analyzing oscillators in time domain is
always tedious. I'm running this at 1 ps steps, so the sim runs are
slow even before I try to measure frequency. Running with the LT Spice
defaults does obviously weird things.

Any suggestions?

I put these statements in the sim:

.meas t1 find time when v(tank_p,tank_n)=0 cross=1 td=100u .meas t2 find
time when v(tank_p,tank_n)=0 cross=4001 td=100u .meas f_tank param
2000/(t2-t1)

The td=100u is to skip the startup time of the oscillator. The 2000
cycles was arrived at after I kept increasing the number until the
measurement stabilised. There are still some rounding-error issues in
there I think.

That's cool. I haven't used .meas. I'll have to learn that.


I was using a max time step of 500 ps, which is about as much as I could
tolerate. There is probably some optimum combination of time step and
number of cycles, but I didn't spend much time trying to find it after
the other problems became apparent.

I'm running 5 ps time steps, for a 1 us run, which seems good enough.
Smaller steps don't seem to change my frequency. The LT Spice default
step delivers nonsense.

[snip]

I'll be using a high-Q Coilcraft air-core inductor. I do wonder how it
interacts with the PCB copper planes.

I did consider an air-core inductor, but I need a few tens of uH, and it
wouldn't fit in the product. Also there is no overall shielding in this
one apart from the PCB ground plane, and I can see it would end up
becoming a Theremin.

Skin effect shouldn't much affect my 125 MHz Colpitts oscillator, but
FR4 is a horrible capacitor.

https://www.dropbox.com/s/nur4f8aw7akiz7h/FR4_Tempco.JPG?raw=1

Cool. That is a much straighter line than I would expect. Was that done
using a DMM?

I used my faithful AADE capacitance meter. I have a Boonton 72 too.

I should measure microstrip and stripline prop delay vs temperature
too. I have a kitchen-sink 4-layer proto board coming up soon, so I
can throw in some test traces for that. And a couple versions of my
Colpitts. And a couple of LTM8078 tests in lieu of having a Spice
model. The Spice model ETA remains unknown; LT Spice is in turmoil.

I'm going to try guarding/bootstrapping the critical node of my
oscillator by an inner-layer PCB plane patch driven from the emitter
of the Colpitts transistor.

I have also been experimenting with measuring risetimes of short
microstrips on FR4, between two SMA connectors. We have an ongoing
debate here about when it's necessary to pay for exotic laminates.

I've never done anything high enough frequency to have to worry about
dispersion etc. But the FR4 was definitely part of the humidity drift
problem. None of the PCB laminate vendors we approached would commit to
the orders-of-magnitude lower moisture absorption we were asking for, so
we're sticking with FR4 for now.

On top of all of the above, it turned out that our first choice of
inductor was also sensitive to humidity, it looks like the wire
insulation is hygroscopic and the stray capacitance drifts over a period
of hours or days. That one caused a lot of head scratching.

I used one coil that was wound on a plastic coil former. It looked very
nice but it slowly changed inductance as the coil tension made the
thermoplastic flow. The time constant was months. The short-term fix was
to bake all the inductors to relieve the stress. The long-term fix was
to buy something else.

It turns out the customer can accept nulling out the drift at the start
of each day, they have a lot of other measurements where they have to do
this so it's not too big a deal. It's a lot easier to hit than our
originally planned 12 month calibration interval.

Our newer designs self cal every powerup, or startup from idle, so
they accept whatever frequency the oscillator wants to run at. That
eliminated piston caps and worries about long-term drift.

It's interesting to phase-lock an arbitrary-frequency triggered LC
oscillator to a 10 MHz OCXO. I invented one scheme and on a good day,
with lots of coffee, I can still mostly understand how it works.



--

John Larkin Highland Technology, Inc

The cork popped merrily, and Lord Peter rose to his feet.
"Bunter", he said, "I give you a toast. The triumph of Instinct over Reason"

 

On Fri, 6 Mar 2020 08:40:13 -0000 (UTC), news@rblack01.plus.com wrote:

On Thu, 05 Mar 2020 05:30:32 -0800, Bill Sloman wrote:

On Thursday, March 5, 2020 at 7:49:59 PM UTC+11, ne...@rblack01.plus.com
wrote:
On Wed, 04 Mar 2020 08:29:11 -0800, jlarkin wrote:

snip

The real limitation of this approach is that the LTSPICE inductor
doesn't accurately model core losses, and how they change with current
and temperature (it just has a parallel resistance).

LTSpice offers the John Chan model of a hysteretic inductor, which may
be more realistic.

"The other non-linear inductor available in LTspice is a hysteretic core
model based on a model first proposed in by John Chan et la. in IEEE
Transactions On Computer-Aided Design, Vol. 10. No. 4, April 1991 but
extended with the methods in United States Patent 7,502,723. "


You mean this one?
http://ltwiki.org/LTspiceHelp/LTspiceHelp/L_Inductor.htm (bottom of page)
http://ltwiki.org/index.php?title=The_Chan_model

I had a quick play with it, using the example example model in the second
link. I don't have time to look into it in any more depth right now, but
worth adding to the toolbox.

I didn't have any trouble digging the parameter out of the data sheet
for the core I was using.

I'm using 1210 surface-mount inductors from the likes of TDK, Murata,
Wurth. I think one of the Murata ones had a SPICE model but it didn't
include non-linearity or behaviour over temperature. The other vendors
just have bare data sheets with 'typical' values or impedance curves at
room temperature. Measuring the parts ended up being quicker than trying
to model them.

Did you get any tempcos? Most air-wound inductors have positive TCs in
the roughly +100 PPM/K range. But if the coil is stretched by the FR4
TCE, that has an effect too.

I'm about to learn some more about that.

Sounds like a job for a Blumlein bridge.

Centre-tapped transformers wound with twisted pair (and certain amount
of attention to detail) offer a 1:1 ratio that is accurate to about one
part in a billion.

Ratio transformers are somewhat more flexible, but the precision goes
down to about one part in ten million.

These are a few of the many interesting facts you can find in

https://www.amazon.com/Coaxial-AC-Bridges-B-Kibble/dp/0852743890

The Kibble is the guy whose name got recorded in the Kibble balance

https://en.wikipedia.org/wiki/Kibble_balance

Custom magnetics would be an absolute last resort for this one. The
whole PCB is about the size of a stick of gum, none of the cores I can
find would fit. Plus this is an area I have very little experience of,
throwing another steep learning curve into the mix at this point wouldn't
endear me to my boss.

I had to wind my own air-core power inductors, to tolerate skin-loss
heating. #14 wire wound on a reference Sharpie.

https://www.dropbox.com/s/27px827y9ed4mev/T850_L1_Tinned.jpg?raw=1

https://www.dropbox.com/s/o2hz6oi08agzdy8/T850_Inductor.JPG?raw=1

I do have a reference capacitor, being measured by an identical circuit,
and doing the ratiometric stuff in software, which works well enough to
correct the temperature drift. The humidity drift is a harder problem,
mainly because it takes so much longer to measure.

--

John Larkin Highland Technology, Inc

The cork popped merrily, and Lord Peter rose to his feet.
"Bunter", he said, "I give you a toast. The triumph of Instinct over Reason"

 

On Fri, 6 Mar 2020 06:50:13 -0600, John S <Sophi.2@invalid.org> wrote:

On 3/5/2020 10:29 AM, jlarkin@highlandsniptechnology.com wrote:
On Thu, 5 Mar 2020 08:49:53 -0000 (UTC), news@rblack01.plus.com wrote:

On Wed, 04 Mar 2020 08:29:11 -0800, jlarkin wrote:

I'm designing a 125 MHz triggered LC oscillator. It's sufficiently
nonlinear that I need to Spice it in transient/time domain mode. I want
to explore frequency sensitivity to component values, supply voltages,
stuff like that.

But how to measure frequency accurately? Cursoring one cycle of
oscillation on the screen is pretty crude.

I guess I could use a delay line to compare the time of one edge to the
previous one, essentially zoom the period.

Or just note the absolute time of the zero cross of the 100th edge, and
calculate from that. Analyzing oscillators in time domain is always
tedious. I'm running this at 1 ps steps, so the sim runs are slow even
before I try to measure frequency. Running with the LT Spice defaults
does obviously weird things.

Any suggestions?

I put these statements in the sim:

.meas t1 find time when v(tank_p,tank_n)=0 cross=1 td=100u
.meas t2 find time when v(tank_p,tank_n)=0 cross=4001 td=100u
.meas f_tank param 2000/(t2-t1)

The td=100u is to skip the startup time of the oscillator. The 2000
cycles was arrived at after I kept increasing the number until the
measurement stabilised. There are still some rounding-error issues in
there I think.

That's cool. I haven't used .meas. I'll have to learn that.


I was using a max time step of 500 ps, which is about as much as I could
tolerate. There is probably some optimum combination of time step and
number of cycles, but I didn't spend much time trying to find it after
the other problems became apparent.

I'm running 5 ps time steps, for a 1 us run, which seems good enough.
Smaller steps don't seem to change my frequency. The LT Spice default
step delivers nonsense.


The real limitation of this approach is that the LTSPICE inductor doesn't
accurately model core losses, and how they change with current and
temperature (it just has a parallel resistance). The manufacturers don't
often quote this anyway, so I had to buy lots of samples and measure them.

If you're using an air-cored inductor, of course, a lot of these issues
go away, but you still have to deal with skin effect and dielectric loss
in the FR4, and the dependence of these on temperature.

I'll be using a high-Q Coilcraft air-core inductor. I do wonder how it
interacts with the PCB copper planes.

Skin effect shouldn't much affect my 125 MHz Colpitts oscillator, but
FR4 is a horrible capacitor.

https://www.dropbox.com/s/nur4f8aw7akiz7h/FR4_Tempco.JPG?raw=1


Very good data, John. Thanks. I did some analysis to try to understand
your ppm results on the right hand side of your graph. I can't come up
with the same numbers. Did you perhaps mean 89pF rather than 99pF?

Not a big deal in any case. I just want to know if I understand it
correctly.

Did I mess that up? That would be bad, but FR4 isn't consistant
anyhow.

Looks like roughly +750 PPM.

I bought a special-made reel of 3.3 pF caps with specified TC of -4700
PPM (measured close to -5000, not bad shootin') to compensate my LC
and CCRO oscillators. First article, I pad one of these with an NPO to
fine-tune the overall TC.

https://www.dropbox.com/s/llucpbgq411ysoa/CCRO_Temp_Comp.jpg?raw=1




--

John Larkin Highland Technology, Inc

The cork popped merrily, and Lord Peter rose to his feet.
"Bunter", he said, "I give you a toast. The triumph of Instinct over Reason"

 

[Phil Hobbs]

On 2020-03-06 09:58, jlarkin@highlandsniptechnology.com wrote:

On Fri, 6 Mar 2020 08:40:13 -0000 (UTC), news@rblack01.plus.com wrote:

On Thu, 05 Mar 2020 05:30:32 -0800, Bill Sloman wrote:

On Thursday, March 5, 2020 at 7:49:59 PM UTC+11, ne...@rblack01.plus.com
wrote:
On Wed, 04 Mar 2020 08:29:11 -0800, jlarkin wrote:

snip

The real limitation of this approach is that the LTSPICE inductor
doesn't accurately model core losses, and how they change with current
and temperature (it just has a parallel resistance).

LTSpice offers the John Chan model of a hysteretic inductor, which may
be more realistic.

"The other non-linear inductor available in LTspice is a hysteretic core
model based on a model first proposed in by John Chan et la. in IEEE
Transactions On Computer-Aided Design, Vol. 10. No. 4, April 1991 but
extended with the methods in United States Patent 7,502,723. "


You mean this one?
http://ltwiki.org/LTspiceHelp/LTspiceHelp/L_Inductor.htm (bottom of page)
http://ltwiki.org/index.php?title=The_Chan_model

I had a quick play with it, using the example example model in the second
link. I don't have time to look into it in any more depth right now, but
worth adding to the toolbox.

I didn't have any trouble digging the parameter out of the data sheet
for the core I was using.

I'm using 1210 surface-mount inductors from the likes of TDK, Murata,
Wurth. I think one of the Murata ones had a SPICE model but it didn't
include non-linearity or behaviour over temperature. The other vendors
just have bare data sheets with 'typical' values or impedance curves at
room temperature. Measuring the parts ended up being quicker than trying
to model them.


Did you get any tempcos? Most air-wound inductors have positive TCs in
the roughly +100 PPM/K range. But if the coil is stretched by the FR4
TCE, that has an effect too.

I'm about to learn some more about that.





[snip]


Sounds like a job for a Blumlein bridge.

Centre-tapped transformers wound with twisted pair (and certain amount
of attention to detail) offer a 1:1 ratio that is accurate to about one
part in a billion.

Ratio transformers are somewhat more flexible, but the precision goes
down to about one part in ten million.

These are a few of the many interesting facts you can find in

https://www.amazon.com/Coaxial-AC-Bridges-B-Kibble/dp/0852743890

The Kibble is the guy whose name got recorded in the Kibble balance

https://en.wikipedia.org/wiki/Kibble_balance

Custom magnetics would be an absolute last resort for this one. The
whole PCB is about the size of a stick of gum, none of the cores I can
find would fit. Plus this is an area I have very little experience of,
throwing another steep learning curve into the mix at this point wouldn't
endear me to my boss.

I had to wind my own air-core power inductors, to tolerate skin-loss
heating. #14 wire wound on a reference Sharpie.

https://www.dropbox.com/s/27px827y9ed4mev/T850_L1_Tinned.jpg?raw=1

https://www.dropbox.com/s/o2hz6oi08agzdy8/T850_Inductor.JPG?raw=1


I do have a reference capacitor, being measured by an identical circuit,
and doing the ratiometric stuff in software, which works well enough to
correct the temperature drift. The humidity drift is a harder problem,
mainly because it takes so much longer to measure.

Single-layer coils obey the approximate relation

L = a**2 N**2/(9a + 10b),

where L is in uH, a is the mean radius in inches, and b is the length in
inches.

You can use that to choose a coil form material so that the increase in
length balances out the increase in diameter.

There's probably some value at which B&W Miniductor stock has zero
tempco--the plastic expands 10 times more than the copper, which
stretches out the coil.

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

 

[John S]

On 3/6/2020 10:59 AM, jlarkin@highlandsniptechnology.com wrote:

On Fri, 6 Mar 2020 06:50:13 -0600, John S <Sophi.2@invalid.org> wrote:

On 3/5/2020 10:29 AM, jlarkin@highlandsniptechnology.com wrote:
On Thu, 5 Mar 2020 08:49:53 -0000 (UTC), news@rblack01.plus.com wrote:

On Wed, 04 Mar 2020 08:29:11 -0800, jlarkin wrote:

I'm designing a 125 MHz triggered LC oscillator. It's sufficiently
nonlinear that I need to Spice it in transient/time domain mode. I want
to explore frequency sensitivity to component values, supply voltages,
stuff like that.

But how to measure frequency accurately? Cursoring one cycle of
oscillation on the screen is pretty crude.

I guess I could use a delay line to compare the time of one edge to the
previous one, essentially zoom the period.

Or just note the absolute time of the zero cross of the 100th edge, and
calculate from that. Analyzing oscillators in time domain is always
tedious. I'm running this at 1 ps steps, so the sim runs are slow even
before I try to measure frequency. Running with the LT Spice defaults
does obviously weird things.

Any suggestions?

I put these statements in the sim:

.meas t1 find time when v(tank_p,tank_n)=0 cross=1 td=100u
.meas t2 find time when v(tank_p,tank_n)=0 cross=4001 td=100u
.meas f_tank param 2000/(t2-t1)

The td=100u is to skip the startup time of the oscillator. The 2000
cycles was arrived at after I kept increasing the number until the
measurement stabilised. There are still some rounding-error issues in
there I think.

That's cool. I haven't used .meas. I'll have to learn that.


I was using a max time step of 500 ps, which is about as much as I could
tolerate. There is probably some optimum combination of time step and
number of cycles, but I didn't spend much time trying to find it after
the other problems became apparent.

I'm running 5 ps time steps, for a 1 us run, which seems good enough.
Smaller steps don't seem to change my frequency. The LT Spice default
step delivers nonsense.


The real limitation of this approach is that the LTSPICE inductor doesn't
accurately model core losses, and how they change with current and
temperature (it just has a parallel resistance). The manufacturers don't
often quote this anyway, so I had to buy lots of samples and measure them.

If you're using an air-cored inductor, of course, a lot of these issues
go away, but you still have to deal with skin effect and dielectric loss
in the FR4, and the dependence of these on temperature.

I'll be using a high-Q Coilcraft air-core inductor. I do wonder how it
interacts with the PCB copper planes.

Skin effect shouldn't much affect my 125 MHz Colpitts oscillator, but
FR4 is a horrible capacitor.

https://www.dropbox.com/s/nur4f8aw7akiz7h/FR4_Tempco.JPG?raw=1


Very good data, John. Thanks. I did some analysis to try to understand
your ppm results on the right hand side of your graph. I can't come up
with the same numbers. Did you perhaps mean 89pF rather than 99pF?

Not a big deal in any case. I just want to know if I understand it
correctly.

Did I mess that up? That would be bad, but FR4 isn't consistant
anyhow.

No, it is not bad. It doesn't make that much difference. I was just
checking my understanding. Great info, sir.

> Looks like roughly +750 PPM.

That's what I came up with. Thanks for the confirmation.

I bought a special-made reel of 3.3 pF caps with specified TC of -4700
PPM (measured close to -5000, not bad shootin') to compensate my LC
and CCRO oscillators. First article, I pad one of these with an NPO to
fine-tune the overall TC.

https://www.dropbox.com/s/llucpbgq411ysoa/CCRO_Temp_Comp.jpg?raw=1

That's great! Love to see your data. Thank you.