Most kinds of protection involve both a clamping (shunt) element
and one (in series) that limits current. Inductors (which ferrite
beads are) are just one particular type of series element.
Le 18/07/2023 à 10:59, Christoph a
écrit?:
toggle quoted message
Show quoted text
I didn’t follow the discussion, but allow me to throw in that
input protection against HF-transients like electrostatic
discharge ?sparks“ often can be achieved by ferrite beads put in
serial into the input line.
—
Christoph
Neon bulbs can be used for receiver or audio
amplifier input protection, modem input protection...etc.
Neon bulbs?cannot handle the power a ceramic gas tube
protector or varistor provides but they have similar
capacitance to a ceramic gas tube. Varistors have very
high capacitance and are not suitable for RF without say a
series choke. The phone/DSL line to your house has a
differential ceramic gas tube protector mounted in the NID
box provided by the phone company.?
One has to define what surge event could be expected. For
an RF receiver/audio amp, one could expect static buildup
or discharge by the user or a surge induced into the
feedline by a nearby lightning hit. In general a direct
lightning hit will destroy almost anything. Goal should be
to isolate the damage to a replaceable PCB/module or to an
external surge protector.?
|
Re: Is there a way to make node numbers appear on LTSpice schematics?
On 18/07/2023 03:33, Andy I wrote:
I don't understand
what you said about naming curves on a plot.? I do not think you
can do that (except by defining functions in the waveform
viewer).? But whatever node names you used on the schematic will
show in the plot window.
That's not quite true. As you say, you can define functions and save
them in plot.defs.
So, for example:
.func hFE() {Ic(Q1)/Ib(Q1)}
..allows you to label a plot hFE() - useful in device testjigs.
Another useful one is:
.func NF(R,T)
{10*log10(V(inoise)*V(inoise)/(4*k*(T+273.15)*R))}
..which allows the label NF(1k,25) to be used as the circuit's noise
figure as a function of source resistance and temperature (in °颁).
Using:
.noise V(out) V1 list 1k
..and stepping a parameter Rsrc as the source resistance, you can
plot the noise figure vs. source resistance at 1kHz:
NF({Rsrc},25)
--
Regards,
Tony
|
I didn’t follow the discussion, but allow me to throw in that input protection against HF-transients like electrostatic discharge ?sparks“ often can be achieved by ferrite beads put in serial into the input line.
— Christoph
toggle quoted message
Show quoted text
Neon bulbs can be used for receiver or audio amplifier input protection, modem input protection...etc. Neon bulbs?cannot handle the power a ceramic gas tube protector or varistor provides but they have similar capacitance to a ceramic gas tube. Varistors have very high capacitance and are not suitable for RF without say a series choke. The phone/DSL line to your house has a differential ceramic gas tube protector mounted in the NID box provided by the phone company.?
One has to define what surge event could be expected. For an RF receiver/audio amp, one could expect static buildup or discharge by the user or a surge induced into the feedline by a nearby lightning hit. In general a direct lightning hit will destroy almost anything. Goal should be to isolate the damage to a replaceable PCB/module or to an external surge protector.?
|
Neon bulbs can be used for receiver or audio amplifier input protection, modem input protection...etc. Neon bulbs?cannot handle the power a ceramic gas tube protector or varistor provides but they have similar capacitance to a ceramic gas tube. Varistors have very high capacitance and are not suitable for RF without say a series choke. The phone/DSL line to your house has a differential ceramic gas tube protector mounted in the NID box provided by the phone company.?
One has to define what surge event could be expected. For an RF receiver/audio amp, one could expect static buildup or discharge by the user or a surge induced into the feedline by a nearby lightning hit. In general a direct lightning hit will destroy almost anything. Goal should be to isolate the damage to a replaceable PCB/module or to an external surge protector.?
|
Re: ISL70444SEH declaration issue?
mliccione89, I uploaded "TIA_Another-way-to-look-at-it.asc" to the Temp folder.? It might help understand what's happening to the output as the pulsewidth of the photodetector varies.
Andy
|
Re: Is there a way to make node numbers appear on LTSpice schematics?
Chris,
You can not display the automatically generated node names on the schematic.? But you can see what they are when viewing the schematic.? Hover your mouse over any node (net).? The node name is shown in the lower left corner.
And as everyone advises you, you really should add your own node names (or numbers) as much as possible, and then they are visible too.
I don't understand what you said about naming curves on a plot.? I do not think you can do that (except by defining functions in the waveform viewer).? But whatever node names you used on the schematic will show in the plot window.
Andy
|
Re: ISL70444SEH declaration issue?
On 18/07/2023 01:44, Tony Casey wrote:
Even
for a 1st order transfer function, that will give you a rise time
of ?3.5/Fc => 45ns
Sorry, I meant 0.35/Fc => 4.5ns.
--
Regards,
Tony
|
Re: ISL70444SEH declaration issue?
Exactly what do you mean by non-linear? You haven't plotted the
response to varying input amplitude. All the information you have is
the response to two different input pulse widths.
No opamp is going to give you a full amplitude output voltage for a
500ps wide input pulse.
Did you plot the AC response of your circuit? The -3dB response is
about 77MHz. Even for a 1st order transfer function, that will give
you a rise time of ?3.5/Fc => 45ns, which is why you get a
fraction of the output voltage you might might expect from a 5mA
peak source current. According to the AC analysis, a critically
damped response is obtained with a feedback capacitance of 3.9pF,
which will give you a bandwidth of 114MHz.
You should also bear in mind that the AD8038 has a maximum slew rate
of 425V/μs, so the response to an input 5mA peak rectangular pulse
of 3.5ns width is never going to be greater than? 1.488V instead of
2.495V, even with an infinite small signal bandwidth.
Your stated requirement of: "pulse widths can range between 0.7ns
wide and ~4ns wide" needs to be refined. The narrower the pulse
width, the larger the input needs to be to get detected due to
limited bandwidth. So you need to consider the comparator too, in
addition to the opamp. If you set the comparator detection threshold
too low, you will get false positives; too high, and you will miss
valid pulses - false negatives. I'm assuming your target wavelength
is in the infra-red range, otherwise a photomultiplier tube might be
a better solution.
--
Regards,
Tony
toggle quoted message
Show quoted text
Thank you Andy. I
truly appreciate all of your help. I was able to find an opamp
that meets my environmental requirements. However the response
seems to be nonlinear.
Here is
the circuit
I commented out the unnecessary simulation directives and adjusted
the amplitude of the pulse to match the photodiode I selected so
you will notice some changes there.
|
Re: Is there a way to make node numbers appear on LTSpice schematics?
No, you can see what the node names before simulation are by:
View > SPICE Netlist
As you say, though, the net names are dynamic unless you explicitly
name them. Only explicitly named nets are visible on the schematic.
--
Regards,
Tony
On 17/07/2023 22:01, Jim Wagner wrote:
toggle quoted message
Show quoted text
Those run-time node and net numbers can vary from run to run,
especially after adding a component. AFIK, they are not known
until the sim runs.
Jim, Oregon Research Electronics
I believe that nodes (or nets) can be
user-named, and that curves on an LTSpice plot can also be
user-named, but sometimes it would be simplest to use the
node numbers assigned by the software during the building
of a schematic. Is there a way to cause those node numbers
to be displayed on the schematic. Thanks, Chris.
|
Re: Is there a way to make node numbers appear on LTSpice schematics?
You always should label nodes if they are being referenced in an equation or within a measure statement. Otherwise, they WILL change. leaving the reference invalid. Those labels are visible on the schematic until they are deleted.
But, the automatically assigned ones are not visible unless you do certain specific things (maybe probe with a voltmeter?)
Jim
toggle quoted message
Show quoted text
You can lable the nets with numbers or letters.? As for them showing up as you mentioned I am not sure about that.
|
Re: Is there a way to make node numbers appear on LTSpice schematics?
You can lable the nets with numbers or letters.? As for them showing up as you mentioned I am not sure about that.
|
Re: Is there a way to make node numbers appear on LTSpice schematics?
Well, except for net 0, common or ground. That is known as the schematic is built.
toggle quoted message
Show quoted text
Those run-time node and net numbers can vary from run to run, especially after adding a component. AFIK, they are not known until the sim runs.
Jim, Oregon Research Electronics
I believe that nodes (or nets) can be user-named, and that curves on an LTSpice plot can also be user-named, but sometimes it would be simplest to use the node numbers assigned by the software during the building of a schematic. Is there a way to cause those node numbers to be displayed on the schematic. Thanks, Chris.
|
Re: Is there a way to make node numbers appear on LTSpice schematics?
Those run-time node and net numbers can vary from run to run, especially after adding a component. AFIK, they are not known until the sim runs.
Jim, Oregon Research Electronics
toggle quoted message
Show quoted text
I believe that nodes (or nets) can be user-named, and that curves on an LTSpice plot can also be user-named, but sometimes it would be simplest to use the node numbers assigned by the software during the building of a schematic. Is there a way to cause those node numbers to be displayed on the schematic. Thanks, Chris.
|
Is there a way to make node numbers appear on LTSpice schematics?
I believe that nodes (or nets) can be user-named, and that curves on an LTSpice plot can also be user-named, but sometimes it would be simplest to use the node numbers assigned by the software during the building of a schematic. Is there a way to cause those node numbers to be displayed on the schematic. Thanks, Chris.
|
Re: ISL70444SEH declaration issue?
Thank you Andy. I truly appreciate all of your help. I was able to find an opamp that meets my environmental requirements. However the response seems to be nonlinear. Here is the circuitI commented out the unnecessary simulation directives and adjusted the amplitude of the pulse to match the photodiode I selected so you will notice some changes there.
|
PULSE default rise and fall times (Trise=0 Tfall=0) (was: ISL70444SEH declaration issue?)
I suspect it was a large data file that slowed mine down.
My run times were between 12 and 14 seconds, up from ~200 ms
?
V(B) was what I expected, once I realized what the SIN parameters did!
One big spike at 4ms.
?
toggle quoted message
Show quoted text
From: [email protected] < [email protected]> On Behalf Of
Andy I
Sent: Sunday, July 16, 2023 5:38 PM
To: [email protected]
Subject: EXTERNAL: Re: : Re: : Re: [LTspice] PULSE default rise and fall times (Trise=0 Tfall=0) (was: ISL70444SEH declaration issue?)
?
Dave wrote, "Certainly slowed down the entire .TRAN period, though."
That should not have happened.? It should slow it down over only 1 ps of the 10 ms simulation -- so about 0.00000001% of it.
LTspice says it took about 0.4 seconds longer to simulate.? What did it do on your computer?
I wonder if we have run across another bug??? If you plot V(B), what do you see?
Anyway, just to clarify, when you wrote "but no longer works below 10ps!"? That's not quite true.? Your PULSE voltage source does have wicked fast rise and fall times down to
1 femtosecond or faster if you ask for them, but the internal Timestep isn't able to show it.? THAT is the issue, not the PULSE source.
Andy
|
Re: PULSE default rise and fall times (Trise=0 Tfall=0) (was: ISL70444SEH declaration issue?)
Dave wrote, "Certainly slowed down the entire .TRAN period, though."
That should not have happened.? It should slow it down over only 1 ps of the 10 ms simulation -- so about 0.00000001% of it.
LTspice says it took about 0.4 seconds longer to simulate.? What did it do on your computer?
I wonder if we have run across another bug??? If you plot V(B), what do you see?
Anyway, just to clarify, when you wrote "but no longer works below 10ps!"? That's not quite true.? Your PULSE voltage source does have wicked fast rise and fall times down to 1 femtosecond or faster if you ask for them, but the internal Timestep isn't able to show it.? THAT is the issue, not the PULSE source.
Andy
|
Re: PULSE default rise and fall times (Trise=0 Tfall=0) (was: ISL70444SEH declaration issue?)
Well, that’s true!? My mind didn’t conceive of a PHz burst!
Certainly slowed down the entire .TRAN period, though.
I would have guessed PSICE would only slow down for the 1000 cycles of the burst.
?
toggle quoted message
Show quoted text
From: [email protected] <[email protected]>
On Behalf Of John Woodgate
Sent: Sunday, July 16, 2023 3:08 PM
To: [email protected]
Subject: EXTERNAL: Re: : Re: : Re: [LTspice] PULSE default rise and fall times (Trise=0 Tfall=0) (was: ISL70444SEH declaration issue?)
?
That's the whole point of V2: it forces LTspice to have a very small timestep indeed. Obviously it takes time to plot lots of cycles of 1 petahertz.
======================================================================================
Best wishes John Woodgate OOO-Own Opinions Only
Rayleigh, Essex UK
I hear, and I forget. I see, and I remember. I do, and I understand. Xunzi (340 - 245 BC)
On 2023-07-16 22:53, Bell, Dave wrote:
Andy, your model here does work all the way down to 1fs.
But:
- It’s much slower as-is, so
- I deleted the SIN source, V2/B
Now, it runs as fast as before, as far as I could sense (didn’t compare runtime in the logs), but no longer works below 10ps!
?
Dave
?
?
For grins, here is another one to try.? It shows one way to control SPICE's internal timestep while not imposing a harshly small Maximum Timestep across the whole simulation (which would make it crawl):
V1 A 0 PULSE(0 1 4m {Trf} {Trf} 1m 2m)
V2 B 0 SIN (0 1 1000T 4m 0 0 1000)
.step param Trf list 1f 10f 11f 20f 50f 100f 1p
.meas T0 WHEN V(A)=0.01 rise=1
.meas T1 WHEN V(A)=0.99 rise=1
.options plotwinsize=0
? ? ?1 1.01915e-015? <-- 1.02 fs
? ? ?2 9.80032e-015? <-- 9.8 fs
? ? ?3 1.07796e-014? <-- 10.8 fs
? ? ?4 1.95998e-014? <-- 19.6 fs
? ? ?5 4.90007e-014? <-- 49.0 fs
? ? ?6 9.79997e-014? <-- 98.0 fs
? ? ?7 9.8e-013? <-- 0.98 ps
Andy
|
Re: .FERRET directive does not work.
Thanks Tony,
I have reported this to Anolog Devices.
Regards,
Dan
|
Re: PULSE default rise and fall times (Trise=0 Tfall=0) (was: ISL70444SEH declaration issue?)
That's the whole point of V2:
it forces LTspice to have a very small timestep indeed.
Obviously it takes time to plot lots of cycles of 1 petahertz.
======================================================================================
Best wishes
John Woodgate OOO-Own Opinions Only
Rayleigh, Essex UK
I hear, and I forget.
I see, and I remember.
I do, and I understand.
Xunzi (340 - 245 BC)
On 2023-07-16 22:53, Bell, Dave wrote:
toggle quoted message
Show quoted text
Andy, your model here does work all the way
down to 1fs.
But:
- It’s much
slower as-is, so
- I deleted
the SIN source, V2/B
Now, it runs as fast as before, as far as I
could sense (didn’t compare runtime in the logs), but no
longer works below 10ps!
?
Dave
?
?
For grins,
here is another one to try.? It shows one way to control
SPICE's internal timestep while not imposing a harshly small
Maximum Timestep across the whole simulation (which would make
it crawl):
V1 A 0 PULSE(0 1 4m {Trf} {Trf} 1m 2m)
V2 B 0 SIN (0 1 1000T 4m 0 0 1000)
.step param Trf list 1f 10f 11f 20f 50f
100f 1p
.meas T0 WHEN V(A)=0.01 rise=1
.meas T1 WHEN V(A)=0.99 rise=1
.options
plotwinsize=0
? ? ?1 1.01915e-015? <-- 1.02 fs
? ? ?2 9.80032e-015? <-- 9.8 fs
? ? ?3 1.07796e-014? <-- 10.8 fs
? ? ?4 1.95998e-014? <-- 19.6 fs
? ? ?5 4.90007e-014? <-- 49.0 fs
? ? ?6 9.79997e-014? <-- 98.0 fs
? ? ?7
9.8e-013? <-- 0.98 ps
Andy
|
Tony Casey
Christoph
Dan
Bell, Dave
John Woodgate