Thanks for the quick reply. Pls find below the answers to your queries:

?

Pls read the value of Cox as 8.5fF/um^2. It is the oxide capacitance per unit area. While implementing the formula fT = gm/2*3.14*W*L*Cox, W and L are MOSFET sizes in um.

?

The y-axis is in ohm-1 (ohm inverse or siemens). This is the unit of gm. In other words, while implementing the above fT formula, the y-axis is taking the units of gm only. It should be of frequency (in Hz or KHz etc)

?

Thanks again,

Arvind Gupta

?

On 06/07/2023 09:13, garvind25@... wrote:

I am trying to plot a few graphs in LTSPICE XVII and have a couple of queries. Hope someone will answer:

?

** Can I define a constant capacitance value in LTSPICE such as Cox = 8.5fF/u^2 so that after simulation, I can manipulate the graph to plot expressions like fT = gm/2*3.14*W*L*Cox? If I simply use the magnitude of Cox as 8.5f in Expression Editor, though I get the graph, the unit of the Y-axis isn’t frequency (as it should be). I event tried by saving the value in “plot.defs” file. I am still getting the same graph with the unit on Y axis as something else. Basically, the Farad quantity is getting neglected and only the numerical value is getting used. ?The x-axis is a voltage source (swept by a dc sweep command).



** As I know, after the simulation, I can manipulate the graph to plot expressions on the y-axis (such as for fT as in above query). Is it possible to plot a graph with expressions on both Y axis and X axis? For eg. how to plot a graph of fT vs gm/Id (where the fT expression will be on y axis and ‘gm/Id’ expression on x axis).

As a general rule, expressions in the waveform window can only comprise waveforms that are available in the "Add Traces to Plot" dialogue and constants. However, there are exceptions:

1. In .AC plots, Freq(uency) and Omega are also recognised.
2. Some other "constants" are also available for use in expressions: "k" or "K" is Boltzmann's constant and "q" or "Q", the elementary charge, pi, and "e" or "E" (2.7182..).
3. "K" is always recognised as Boltzmann's constant, unless it is immediately preceded by an number, when it reverts to 1000x. Ditto "E", when used as, e.g. 1E-6. All other range multipliers up to "T" (1E12) and down to "f" (1E-15) are unambiguous. There is no case distinction.
4. .Parameters defined in the schematic are normally not recognised, unless they are stepped, then they are available for use in expressions. It is not necessary to use braces, {}.
5. The only units that are accepted in expressions are V, A and s. But LTspice provides "derived" units in axes annotations, if it can work out what they should be. Whether that's a benefit or cause for confusion is an open question. So, normally, LTspice can easily work out annotations of V, A, W and ?. Siemens (or mhos) are denoted as ?^-1, but I guess it could have used the symbol, ?. Other units it might not present succinctly.

If you want to plot or use gm, then remember it is dI/dV, so you can use the d() operator.

?

Is it possible to plot a graph with expressions on both Y axis and X axis?

?

Did you try it? Depending on the analysis mode, expressions can be used for both axes. .AC plots can only use Frequency for the X-axis. It's not hard to work out why.

Except for plotting expressions, units are generally ignored in LTspice. So remember, 1F is the same as 1fF. When a range multiplier is encountered, it also acts as a delimiter, ignoring everything non-numeric that follows. So, 3k3=3300, but 1A=1V=1.

Certain things saved in plot.defs are very useful in plot expressions, but since customisation of plot.defs in kind of encouraged, it is inherently non-portable. So, for example, I have a function: dB(x)=20.log10(x), which makes trace titles much neater, but will cause an error for anyone else that does not have this function defined.

Nothing added to plot.defs will work until LTspice is closed down and re-started.

开云体育

What you want to do can be done. Note the following:

1. In the Cox formula, LTspice stops parsing after the 'f'. What is 'u' anyway? Is it a fixed voltage?
2. You say that the y-axis unit isn't frequency, but you don't help us by saying what it is. If it is volts, divide the formula by (1V*1s).
   
3. You often have to divide a node voltage or current (which is what can be plotted) by '1 unit' to get the y-axis unit correct. For example, if you apply a 1 A current generator to a node and plot the node voltage, to get the y-axis to be 'ohms', you plot 'Vnode/1A'.
   
4. You can plot an expression on the x-axis, unless you have done an AC sweep. Right-click on it and you get a pane in which you can type the variable you want to plot. For example, you can enter 'V(in)' to use the input voltage as the x-axis. With an AC sweep, you can only have frequency as the x-axis.
   

Hi,

?

? I am trying to plot a few graphs in LTSPICE XVII and have a couple of queries. Hope someone will answer:

?

** Can I define a constant capacitance value in LTSPICE such as Cox = 8.5fF/u^2 so that after simulation, I can manipulate the graph to plot expressions like fT = gm/2*3.14*W*L*Cox? If I simply use the magnitude of Cox as 8.5f in Expression Editor, though I get the graph, the unit of the Y-axis isn’t frequency (as it should be). I event tried by saving the value in “plot.defs” file. I am still getting the same graph with the unit on Y axis as something else. Basically, the Farad quantity is getting neglected and only the numerical value is getting used. ?The x-axis is a voltage source (swept by a dc sweep command).



** As I know, after the simulation, I can manipulate the graph to plot expressions on the y-axis (such as for fT as in above query). Is it possible to plot a graph with expressions on both Y axis and X axis? For eg. how to plot a graph of fT vs gm/Id (where the fT expression will be on y axis and ‘gm/Id’ expression on x axis).

?

Looking towards your pointers.

?

Thanks and regards,

Arvind Gupta

On Wed, Jul 5, 2023 at 02:36 PM, Tim Hutcheson wrote:

it seems that 2^n-1 switches would be needed

Surely this is not Sam Ben-Yaakov's intention, as he readily describes a natural self-balancing behaviour (propagation indeed) permitting the use of 2 switches per cell in case it is acceptable that the full cells string balancing takes 5 hours. Such a natural self-balancing propagation happens with a 94% efficiency in case of balancing a string of 10 Ah cells, using two inexpensive 125 milliohm 12 VDC mosfets (as switches) per cell, and using one inexpensive 12 VDC 20 microfarad polarized capacitor (as charge exchanger) per cell. Plus a microcontroller (possibly a $0.20 one). But at this moment, I don't know if Sam Ben-Yaakov is talking about a 4-cell string, or a 104-cell string.

开云体育

On 05/07/2023 23:57, mliccione89@... wrote:

I'm trying to use the ISL70444SEH model and a basic circuit to confirm that the model works correctly before moving on to anything more complicated. I'm having issues with the simulation. The sim fails to run and I get the error "Time step to small, etc....".

Any help is appreciated.

It helps if you upload a schematic that actually runs. You have a ".lib ISL70444SEH.lib" directive in the schematic, but the model file you uploaded is "ISL70444SEH.cir" and there are no analysis directives.. However, when I change the .lib directive to match the file name and add a .tran directive, I don't get initially "Time step to small, etc....". Instead, I get "Analysis failed: Iteration limit reached", and there are a bunch of errors in the ErrorLog, concerning the diode models. I am running LTspice 17.1.9, you may have a different version.

I made minor changes to the model file and added ".options cshunt 1e-14", and the analysis now runs fine. I have uploaded a working schematic to Files > Temp.

You should note that although the datasheet says "unity gain stable", the circuit is barely stable with 8dB peaking at unity gain. I added a bit of compensation to help a bit with that.

This happens sometimes where there are signals with fast edges (aka zero rise or fall times), discontinuities or indeterminate derivatives. An indeterminate derivative happens at a corner. See if you can simplify the simulation by doing an .op and stepping a parameter.

You forgot the .TRAN statement, and your .INC command references the wrong filename.? Those are minor but not insignificant omissions.? I get suspicious whenever it is obvious that you did not simulate using the files you uploaded.

There were other error messages, referring to the diode .MODEL statements.? I think the cause of those is the "LEVEL=2" in each of those .MODEL statements.? I don't know what those are supposed to do, but I think LTspice probably does not know what to do with the "LEVEL=2" and it gets confused by what comes after.? Removing "LEVEL=2" does not fix the "time step too small" error.

"Time step too small" errors are among the more troublesome ones to afflict SPICE users, worldwide.? You should get some help by reading the "FAQ" file in our group's archives:

/g/LTspice/files/z_yahoo/FAQ/faq_17-2.txt

Read it and find the section about "time step too small" errors.? It has several things you can try.? None of them are guaranteed.? If there was a foolproof solution to "time step too small" errors, we wouldn't have them anymore.

In your circuit, I found that ".options cshunt=1e-14" seemed to tame it.? YMMV ("your mileage may vary" -- your results might differ from mine).

Andy

Hello all-

I'm trying to use the ISL70444SEH model and a basic circuit to confirm that the model works correctly before moving on to anything more complicated. I'm having issues with the simulation. The sim fails to run and I get the error "Time step to small, etc....".

Any help is appreciated.

Here are the files

Depends on what you mean by economical.? Looking at some of Sam Ben-Yaakov's earlier videos and papers of his grad students in Switched Capacitor Controllers, it seems that 2^n-1 switches would be needed...? Yikes, my calculator says that's more than? 2.028e31 switches.
But I'm no expert
Tim

开云体育

Hi, my attention got caught by



Amazing, isn't?

开云体育

On Wed, Jul 5, 2023 at 03:59 PM, Jerry Lee Marcel wrote:

Just like the nominal inductance largely varies between 50Hz and 16kHz, so does the leakage. The magnetic permeability decreases significantly at HF, so te fraction that goes through the air becomes proportionally higher.

So, you mean that the impedance Z of the leakage inductance, is somehow proportional to F^2 (since Z=wL is proportional to F already).

Not so much. Actually leakage inductance does not vary too much, but since the effective inductance of the winding decreases, the leakage factor increases.

For instance, to allow some flux leakage to exist, the transformer should have 2 separate bobbins, not one.

Leakage exists even when there is a single bobbin. The flux lines cannot be concentrated 100% in the core.

Two separate bobbins allow reducing mutual capacitance, but increase leakage.

?

On Wed, Jul 5, 2023 at 02:30 PM, Donald H Locker wrote:

I understand that, but the resonant winding is not visible to users. Ferroresonant xformers appear to be two-winding devices for all practical purposes.

Yes, this is a practical solution in many applications.
In fact, my first thought was to look if there is a hidden third resonant winding. But I found out that the inverter transformer is indeed a normal one, though it has two bobbins instead of one which is usually used to reduce the flux leakage.

On Wed, Jul 5, 2023 at 03:59 PM, Jerry Lee Marcel wrote:

Just like the nominal inductance largely varies between 50Hz and 16kHz, so does the leakage. The magnetic permeability decreases significantly at HF, so te fraction that goes through the air becomes proportionally higher.

So, you mean that the impedance Z of the leakage inductance, is somehow proportional to F^2 (since Z=wL is proportional to F already).
For instance, to allow some flux leakage to exist, the transformer should have 2 separate bobbins, not one.
?

Just like the nominal inductance largely varies between 50Hz and 16kHz, so does the leakage. The magnetic permeability decreases significantly at HF, so te fraction that goes through the air becomes proportionally higher.

You may insist, but the? OP gives contrary evidence:

"pure sinewave inverters which use conventional two-winding iron core transformers. Their transformer is driven by a MOSFET bridge"... " driven by a sinewave PWM"

It seems all here agreed that the other element in LPF is Rpar(hi) which represent the various core losses at the PWM high frequency.
Now I have to find out a rather simple practical test to measure, even approximately, this Rpar(hi) of the unknown cores that the local retailers offer.

For instance, aren't the leakage inductances independent of frequency (at least for this application), so that they can be measured simply at 50 Hz?.

开云体育

Rpar = R(af+bf^2) near enough, for suitable values or R, a and b. You need data on the core material to determine them. af is eddy-current loss and bf^2 is hysteresis loss.