do LTspice have .Sens analysis (can perform the sensitivity analysis)?

john23 wrote, "I read that i should use 100Mega Ohm resitor to solve my ltspice problem."

Where did you read that?

Do you think that the advice came from a reliable source?? Exactly what problem was the 100 Megohm resistor supposed to solve?

The circuit you uploaded in UCC5304_Simplis_Test2.asc has a mistake.? There are two voltage sources driving the net VDD.? V2 on the left drives VDD, and V4 in the upper right corner also drives VDD.? They should not be the same net.? Also, the 1 uF capacitor (C2) at the output of the UCC5304 taxes its ability to switch.

What have you done to diagnose your circuit?

Andy

UPDATE:
I read that i should use 100Mega Ohm resitor to solve my ltspice problem.
i did referenced the Vdd as you said.
Is it possible? to make the circuit at #153738 work in LTSPICE so the output will follow that input and not just charge and stay constant?
Thanks.

Hello Andy, Exactly I have referenced the output VDD to the VSS so VDD=VSS+8 as shown in the attached LTSpice circuit and models below.However as you can see in the attached photo ,The output is not toggling at the same rate as the input pulse.

Its just charging and stays constant.Where did i go wrong?

Thanks.
/g/LTspice/files/Temp/john23/UCC5304_Simplis_Test2.asc
/g/LTspice/photo/294810/3777899?p=Created%2C%2C%2C20%2C2%2C0%2C0

?

?

The power source to the UCC5304's "VDD" pin also should be referenced to its "VSS" pin.? If it is not, imagine what happens when your circuit drives M1 to switch ON.? Its source pin pulls up towards +45 V.? Now you have a problem, because the UCC5304's VSS pin is around +40 V, but its VDD pin is only at +10 V (relative to the same Ground), so it has backwards DC power and it doesn't work.

Oops.? I wrote that using Rser=1n for the upper two inductors fixes the math errors (-1.#IND, 1.#QNAN) for the K=1 case.? But I was mistaken.? Sorry.

Andy

Elien wrote, "if one doesn't define the mutual inductances (and leakage inductances, which I did not apply in my circuit), how would this change my circuit?"

You define their inductances and coupling coeficients.? LTspice applies them to effectively change the mutual and leakage inductances, automatically, and you don't need to see them.? They are equivalent circuits of one another.? One circuit has explicit mutual and leakage inductors.? The other does not need them and doesn't use them.

This would change your circuit because you would draw it as only two inductors (oriented vertically and connected to ground), and one K coupling coefficient.? It is drawn like the real transformer.

Andy

Elien,

Please stop uploading your .RAW and .LOG files.? Those should not be uploaded to this group.? Please take a minute and re-read the instructions on the group's main website.

Actually, K can be 0, but this causes some difficulty in YOUR circuit.? When K = 0, then LM = 0 Henrys, and now that it also has Rser = 0, that makes its impedance invalid (Z = 0), causing the singular error.? You can avoid that by using Rser = 1n or something similarly small.? When looking at your results, just realize that its value is not EXACTLY zero.? But it fixes the Singular error problem.

Likewise there is a problem (which you probably saw already) when K = 1.? That makes "L1-LM" and "L2-LM" equal to zero Henrys.? It simulates, but your output data has values of -1.#IND and 1.#QNAN when K=1, which messes up those plots.? Those "values" are error messages from your computer's math routines (probably from Windows).? Again, setting Rser=1n for the upper two inductors helps avoid those errors when K=1.

Andy

Hi,
I was curious what VCO model is used by SIMetrix. I did some translation of the model to LTSpice.
There are strange solutions, negative references, etc. ...
The file is here:
/g/LTspice/files/SIMetrix_HC4046_VCO.asc
Cheers

开云体育

You can't set k to 0,

Andy,

Thanks for your suggestions.

I uploaded a modified version of my schematic, "IPT_LM_modified.zip" in which I have solved the syntax error.

When I rerun the simulation, I encounter a "singular matrix" error.
I read that this error occurs when a part of the circuit floats. However, my circuit is grounded.

Is there something else that triggers this particular error?

Regarding Jerry Lee Marcel's note: if one doesn't define the mutual inductances (and leakage inductances, which I did not apply in my circuit), how would this change my circuit? But this as a side note.

Elien

Andy,

Thanks for your suggestions.

I uploaded a modified version of my schematic, "IPT_LM_modified.zip" in which I have solved the syntax error.

When I rerun the simulation, I encounter a "singular matrix" error.
I read that this error occurs when a part of the circuit floats. However, my circuit is grounded.

Is there something else that triggers this particular error?

Regarding Jerry Lee Marcel's note: if one doesn't define the mutual inductances (and leakage inductances, which I did not apply in my circuit), how would this change my circuit? But this as a side note.

Elien

Hello Andy,
Thanks for your replay.
I am playing around PLL average models, comparing results with time models. Using MODULATE won't give AC response but using BV with V=sin(2*pi*(fc*time+df*idt(V(m)))) works for both, time and frequency analysis.?
My long term goal is to model the integer boundary spurs of a (fractional) PLL. Because of the frequency division I need square wave vco, which is not the problem. The problem is to have average model of a duty cycle for integer or fractional division. I am trying zero order hold laplace, COMB/MAF filters, etc, inserting them into averaged model here and there.
And again, because I am not sure how to do it, I do comparison with the time models. Something like this:
/g/LTspice/files/Temp/phase_mod2za.asc
Probably my approach is not the right one.
Cheers

bb_petrov,

This error message happens because the original code you used has an A-element (one whose name begins with an A) that is unique to another SPICE program, and doesn't work in LTspice.? In particular, this line:

? ? A1 %vd(1,2) %vd(3,4) ASQRVCO?

In LTspice, all A-elements have 8 pins (or nodes), but this one has only two.? Hence, the error message.? But that is only the symptom; the cause is trying to use an incompatible A-element, so it's a good thing they use different numbers of pins.? Also the .MODEL definition is not compatible.? It is unique to another SPICE program.

The document you referred to about Altium says that its simulator is based on XSpice.? Even though XSpice was based on Berkeley SPICE, it has many features that depart from Berkeley SPICE, and this example uses some of those features.

All of LTspice's A-elements are special and unique to LTspice.

It sounds like you already had a VCO, with the B-source.? But why did you ask, "I am not sure how to add FM:"?? If you have a VCO, then you have FM.? Every VCO is an FM generator.? What are you trying to do, which makes you think you need more than what you already have?

By the way, LTspice has a Modulate/Modulate2 element built-in which also is a handy VCO.? It generates sine waves, which you can easily turn into square waves if that is what you need.? It is not necessarily better or worse than using the idt(V(x)) function to do the same thing.

Andy

Bernt wrote:


To be portable, the "ModelFile" attribute must NOT have any of the "path".? In MS-Windows, the path is the directory structure, leading up to the filename itself.? (Some would say that it includes the filename, but I'm ignoring that for purposes of this.)? Your ModelFile attributes should have ONLY the filename.ext, so in this case it should be "INA826.lib" and nothing else.

To change that, DO NOT open the symbol file in any text editor where you see lines starting with "SYMATTR".? Don't do that.? Instead, open that symbol file in LTspice itself.? If you double-click on the symbol file, it should open it directly in LTspice.? Once it is open in LTspice, then press Ctrl-A (hold down the Ctrl key and click the A key), and then edit only the ModelFile attribute, which is the bottom line.? Edit that line so that the contents have just the filename.ext (such as INA826.lib).? Then click OK, and then Save.

Tony offered another alternative, which is to delete the ModelFile attribute completely, and add a ".lib filename.ext" to each schematic that uses that symbol.? That works perfectly well too.? It is very slightly more complicated because you would need to edit the schematics to add the ".lib" command to every schematic that uses that symbol.

Either way, the purpose of the ".lib" command and of the ModelFile attribute are the same.? Both Either of them loads the model file into LTspice for the simulation.? Your schematic and symbol combination should use one or the other, not both.

Andy

I don't know if this was answered.? Bernt wrote, "However, what I do not understand is how to then place my symbols. In the Place component, it only shows stuff from the .lib (which includes Autogenerated) but nothing else so it is not possible to see other folders and components there."

When you first open the (Add) Component menu, it has things on the top half and the bottom half of its pop-up window.? At the very top of that pop-up menu, there is a choice for "Top Directory".? That is how you can select between the current directory (the one that holds the schematic you are editing), and LTspice's libraries.

Click that to change it to the current directory, and now the bottom half should show only the symbols in the current directory.? If you have not yet saved the current schematic, you may need to save it once first, so that LTspice knows what is the current directory.

Click that "Top Directory" choice at the top of the pop-up window again, when you want to change it back to LTspice's libraries.

The only choices for the "Top Directory" are LTspice's libraries, the user-defined library path that you optionally told LTspice about, and the current working directory with the schematic being edited.

Andy

Elien,

It is also worth noting -

In your circuit, where you have a resistor in series with your inductors L1-LM and L2-LM, you can move the resistors into the inductors by setting Rser = 1.3 ohms on each of those two inductors.? And set LM's Rser to 0.? You don't have to do that, but it can make the simulation run a little faster, and perhaps slightly more accurately than having a separate inductor and resistor in series.

On the other hand, you might want to keep the inductance and the resistance separate on the schematic, especially if the schematic will be published for others to see.

Regarding Jerry Lee Marcel's note about simulating coupled inductors using the TEE (or T) equivalent circuit, I agree, but some people just need to do it the other way.? Some schools teach the TEE equivalent as if it is the way to analyze coupled inductors, without recognizing the fact that SPICE does not need to do that.? To each his/her own.

Andy

Elien,

Unrelated to your question - Be aware of these things, which might affect your simulation's apparent accuracy:

1. Non-coupled inductors in LTspice have a default series resistance of 1 m = 0.001 ohm.? If you want ideal inductors, right-click on each inductor and write "0" for the Series Resistance.
2. LTspice uses waveform compression, which is a lossy compression (you can't restore the un-compressed original) but it can significantly reduce the size of the .RAW output file.? All results, including .MEAS command calculations, are affected by that.? If you don't want any impairment from that, disable waveform compression by adding ".options plotwinsize=0" to your schematics.

Footnote about waveform compression:? The .tran command in this simulation specified a Maximum Timestep of 1e-8 = 10 ns.? Yet LTspice compresses the saved waveforms with a larger effective timestep of around 250 ns.? If you really need the timestep to be 10 ns or less, always disable the waveform compression.? Internally, LTspice simulates the circuit with 10 ns or smaller timesteps, but it might not save the simulated waveforms with increments that small, unless you disable the compression.

Andy

开云体育

When you define k<1, you don't need to define the mutual inductance, nor the leakage inductances. LTspice does it automatically.

Elien wrote about an error "Missing inductance value".? There were several other errors too.

Elien, the reason is simple, but might not be obvious.? You used parameters named L1 and L2, but you never defined them.? You are probably thinking, "But wait, I did define them."? Well, not exactly.? You had these two lines:
which LOOK as if they have the dot-commands ".param".? But they did not.? There is a space between the dot (period) and the word "param", so they were seen by LTspice as non-commands.

Edit both lines to get rid of that extra space, and all will be well.

Andy

Hello,

I want to simulate a mutual inductance LM in function of a coupling factor k. The mutual inductance also depends on the self-inductances L1 and L2, which are constant values.
The T-circuit gives an error message due to a missing value for the inductance L1-LM.

Can someone help me find a solution to simulate this circuit??

Please see the files in the folder:
IPT_LM

Thanks in advance,
Elien

开云体育

Please be advised that anyone can ask me for special access for this Undocumented page.? You have to have an account with ltwiki.org, then request this special access.? I had to limit this page because the late analogspiceman spent a lot of time getting this page right.? Thanks for supporting the wiki.