From (complete_reference):

Bxxx n1 n2 V=<expression>
Bxxx n1 n2 I=<expression> [Rpar=<value>] *[Cpar=<value>]
+ [[ic=<value>] tripdv=<value>] [tripdt=<value>]
+ [Laplace=<func(s)> [window=] [nfft=<num>] [mtol=<num>]]
* + [[units] Freq=<valuelist> [delay=<value>]] <=================
* + [NoJacob]
* Bxxx n1 n2 R=<expression>
* Bxxx n1 n2 P=<expression> [VprXover=<value>]

-marcel

开云体育

I guess so. LTspice comes with lots of models for them from Schaffner and Würth. Do you have a part number for yours?

F2 > [Contrib] > Schaffner > EMI
F2 > [Contrib] > Wurth > EMC-Components > CommonMode_Chokes

Or you could try to make one from two coupled inductors. It's easier than you probably thought.

Not quite so easy to tune it to exactly fit your table though, but there's usually significant tolerance on EMC chokes, anyway.

开云体育

Yes, as a piece of circuit or a subcircuit. But the data you have is all expressed in series component terms, whereas the circuit needs, at least,? parallel resistance and capacitance elements, which possibly could be calculated from your data. Obviously, the inductor does not have a physical series capacitor. Have you asked the manufacturer for a SPICE (not 'LTspice') model?

is it possible to build a "Frequency dependent common mode inductor" in LTspice?

?

f	Ls	Cs	Rs
[HZ]	[uH]	[pF]	[ohm]
50	2040.3	4966800000	0.11861
100	2023.6	1251600000	0.13833
500	1997.3	50727000	0.47052
1000	1962.3	12905000	1.2977
5000	1636	619260	15.796
10000	1320.2	191850	36.245
50000	710.19	14266	144.23
100000	520.68	4864.9	247.12
500000	212.64	476.5	958.8
1000000	15.536	1631.6	1963.6
5000000	6.5795	154.02	79.92

1. SPICE/LTspice is a discrete time simulator.? There is no continuous time.
2. .MEASURE is a POST-processing step.? All .MEAS commands are processed AFTER the simulation is over and done with.? It does not command the simulator to re-simulate until it finds the exact point where the voltage was 2.00000000000.? It interpolates between the closest simulated points that straddle it.? The chance that one of those simulated points hits 2.00000000000 volts exactly is astronomically small.? It will 'never' happen.

1. Verify that the comparator model's subcircuit has the same number of pins in the same order: In+ In- V+ V- OUT.
2. Change (edit) the name next to the opamp2 symbol, from "opamp2", to the actual name of the subcircuit of your comparator.? The name of the subcircuit is the name that you see immediately after the command ".SUBCKT", when you examine the contents of the library file.? It is NOT the filename name of the file.
3. Additionally, include the library file into the simulation, by adding this SPICE Directive anywhere on your schematic: ".lib filename.ext" where you use the actual filename.ext of the library file.? If that library file is not already in the same folder with the schematic, nor in one of your Model Library areas that you may have already set up in LTspice's Control Panel, then the filename should also have the relative or absolute path to the library file.

• .lib MyComparator.lib
• .lib models\MyComparator.lib
• .lib ..\models\MyComparator.lib
• .lib \Mymodels\comparators\MyComparator.lib
• .lib "C:\Users\MyName\My Documents\My LTspice Models\comparators\MyComparator.lib"

开云体育

From the ADI data sheet: 110 MHz gain bandwidth (G = 1000) 8 MHz bandwidth (G = 10)

On Tue, Feb 25, 2025 at 03:06 AM, john23 wrote:

Hello , is there an alternative I could use for AD797 , LTspice model will be best.

Have you tried the product selection guides, which most IC vendors and many distributors offer on their websites?

The model I got is very bad and its oscilating for no good reason.

There probably is a reason.? It might be worth investigating why.? High-bandwidth amps are more susceptible.? Maybe your circuit into which you plugged the AD797 was the cause.

Gain bandwidth: 100 MHz
-3 dB bandwidth: 8 MHz

Certainly that figure requires qualifications.? I know of no op-amps that would have an 8 MHz open-loop -3dB bandwidth.? So it is likely a closed-loop measure - and? then, at what closed-loop gain is that measured?? It makes all the difference in the world.

?

Andy

?

?

开云体育

This is also true with .MEAS. The time points are printed in single precision in the logfile, by default. You can get double precision by adding .option measdgt=15. This is true whether or not you also use .option numdgt=15.

Having just installed V24.1.4, I noticed that:

.option measdgt=x

..appears to have been disabled, and doesn't appear to do anything now - the .MEAS time points are now always double precision.

The log file content has changed a bit from 24.0.12 to 24.1.4. The listed circuit is now the .net file instead of the .asc, and the active .options are now listed, which is useful.

.option numdgt=x

..seems to works the same as before, but the raw files contents differ slightly.

--

开云体育

When temperature increases, the current resulting from the reverse-biased gate-drain junction increases exponentially, so yes, noise increases with temperature.

开云体育

Tony, I was not out to prove that 2.000000000 volts never happens.

I was out to prove that 2.000000000 volts did not happen in my case.

So that I could therefrom propose that the test ".MEAS = something FALL=1" in my case does not test for equality to something because that something does not exist.

Until someone can show me proof of interpolation to obtain the .MEAS result in my case, I will assume that it is actually doing the more efficient test for a value that was more than something and now has become less than something.

?

When it comes to plotting, that's a different story.

If your pixels are a certain size and your two data points span more than two pixels then interpolate to find the missing pixel coordinates.

But would you interpolate 100 new coordinates if you know you only have to locate 14 pixels between the given data points.

No, that would be inefficient to crank an interpolation a 100 times to fix the coordinates of 14 missing points.

?

The same logic applies to using interpolation at all, when the task at hand is to analyse the data stream to find any data value greater than something followed by any data value less than something.

That simply requires if(X <= something && priorX >= something) to be true [C syntax not precisely correct] which is considerably simpler than interpolation.

How would you know how many times to turn the interpolator crank to find if any interpolated point could be found that was exactly 2.00000000 volts so that it could be compared for equality to 2.

?

I predict that the .MEAS statement never tests for equality.

Even in this example from the help file, I posit that:

.MEAS TRAN res2 FIND V(out)*I(Vout) WHEN V(x)=3*V(y)

Print the value of the expression V(out)*I(Vout) the first time the condition V(x)=3*V(y) is met. This will be labeled res2.

Does not ever test that V(x) becomes exactly equal to 3*V(y).

It does this; "if((V(x) <= 3*V(y) && priorV(x) >= 3*V(y) || (V(x) >= 3*V(y) && priorV(x) <= 3*V(y)))" == true" then it would be known that the data has passed through the point 3*V(y) without ever having to resort to a test of equality between floating point numbers.

Nobody ever said that LTspice tests for equality. It can't if the data doesn't exist. LTspice uses interpolation to estimate it. I thought that had been made clear. The closer the data points, the better the estimation is likely to be. You can, of course, choose to believe anything you wish to.

BTW, in case you hadn't realised, when using the waveform cursor, pressing the → and ← keys advances or retards the cursor position to the next actual data point. Any reading of the cursor position between data points is also interpolated. Note that if you don't have .option plotwinsize=0 enabled, not all actual analysis data points are stored in the .raw file, and therefore cannot be displayed or used for interpolation. The line display appears to be a spline fit, but zooming-in shows this to be realised as a series of linear approximations.

--
Regards,
Tony