Re: Question/ Problem with voltage source
Ok, Thank you all!
Hopefully I will somehow remember this when it happens next time :-)
|
Re: Question/ Problem with voltage source
Bernt wrote:
? ? "But why did this suddenly become a problem?
? ? ?My real circuit is an amplifier and when simulating it yesterday, I has no issues and suddenly today, none of it worked."
Something changed between yesterday and today.
Waveform compression depends on the whole circuit.? If your circuit has only the tiny voltage source, it might compress it all away.? If the circuit has other stuff too, it is likely to compress less.? It depends on ALL the waveforms, both voltages and currents.
Andy
|
Re: Question/ Problem with voltage source
Yes, its the data compression.
Look at the options table in the help file:
plotvntol - Absolute voltage error tolerance for waveform compression - default: 10¦ÌV
plotabstol - Absolute current error tolerance for waveform compression - default: 1nA
Both default values are not reached in any output data.
E.g. add
.options plotvntol=1e-8
as SPICE directive at the schematic.
Or lower the R1 value.
|
Re: Question/ Problem with voltage source
Aha, I have done this and it works.? ?Thank you to those who suggested the? .option
But why did this suddenly become a problem?
My real circuit is an amplifier and when simulating it yesterday, I has no issues and suddenly today, none of it worked.
The output stage even did not produce any waveforms.
Now, with the .option you suggested, is does work again.
Hmm...
Best regards
Bernt
|
Re: Question/ Problem with voltage source
Add ".opt plotwinsize=0" without quotes on the schematic.
|
Re: Question/ Problem with voltage source
What did you folks find out?
I have since tested it in steps of 1uV and it produces all sorts of weird and wonderful waveforms.
The first time it starts looking like a sort of sine wave (not quite) is at amplitude 25uV.
The first reasonable sine wave appears at 35uV.
So now how does one generate a working 1uV signal?
|
Re: Question/ Problem with voltage source
For some values of R1, you need to add .OPTION
plotwinsize=0. For other values, it isn't necessary.
On 2024-05-14 00:07, Berntd via
groups.io wrote:
Link to file
/g/LTspice/files/Temp/Bernt_Vtest1.asc
--
OOO - Own Opinions Only
Best wishes
John Woodgate, Rayleigh, Essex
UK
Keep trying
|
Re: Question/ Problem with voltage source
Link to file
/g/LTspice/files/Temp/Bernt_Vtest1.asc
|
Re: Question/ Problem with voltage source
It does not work and I am stumped since I am sure it has worked before.
I have not used LtSpice in a while so perhaps I forgot something.
I just tried it on a second computer, same problem.
I have uploaded the file: ?
Bernt_Vtest1.asc
|
Re: Question/ Problem with voltage source
Of course it's supposed to work. It has for more than 20 years. In order for anyone to figure out your problem, we have to see your schematic. I suggest you upload it, by going Files > Temp on the group website, and upload your schematic. If it uses any models or symbols that didn't come with LTspice, please include those in the upload,? by putting all files in a zip.
-- Regards, Tony
On 14 May 2024 00:37, "Berntd via groups.io" <berntau@...> wrote: Hello,
I am using a voltage set to
SINE(0 1u 50)
which is 1uV 50Hz.
Using transient analysis
.tran 100m?
It does not work. It just outputs / simulates to a straight line sloping from 1nV to -500nV over 100ms
I was sure this did work just yesterday and I got a sine wave as expected.
I suspect it stopped working earlier today after I did an AC analysis.
I have since restarted LTSpice and done a whole new schematic. Same problem.
It does work for bigger amplitudes such as 1V.
Is it supposed to work?
Best regards
Bernt
|
Re: Question/ Problem with voltage source
Just thought: are you simulating over 100n
instead of 100m, by chance?
On 2024-05-13 23:47, John Woodgate
wrote:
Yes, it should work, and I just tried it,
but without seeing your .ASC, we can't help much.
On 2024-05-13 23:37, Berntd via
groups.io wrote:
Hello,
I am using a voltage set to
SINE(0 1u 50)
which is 1uV 50Hz.
Using transient analysis
.tran 100m?
It does not work. It just outputs / simulates to a straight line
sloping from 1nV to -500nV over 100ms
I was sure this did work just yesterday and I got a sine wave as
expected.
I suspect it stopped working earlier today after I did an AC
analysis.
I have since restarted LTSpice and done a whole new schematic.
Same problem.
It does work for bigger amplitudes such as 1V.
Is it supposed to work?
Best regards
Bernt
--
OOO - Own Opinions Only
Best wishes
John Woodgate, Rayleigh, Essex
UK
Keep trying
--
OOO - Own Opinions Only
Best wishes
John Woodgate, Rayleigh, Essex
UK
Keep trying
|
Re: Question/ Problem with voltage source
Yes, it should work, and I just tried it, but
without seeing your .ASC, we can't help much.
On 2024-05-13 23:37, Berntd via
groups.io wrote:
Hello,
I am using a voltage set to
SINE(0 1u 50)
which is 1uV 50Hz.
Using transient analysis
.tran 100m?
It does not work. It just outputs / simulates to a straight line
sloping from 1nV to -500nV over 100ms
I was sure this did work just yesterday and I got a sine wave as
expected.
I suspect it stopped working earlier today after I did an AC
analysis.
I have since restarted LTSpice and done a whole new schematic.
Same problem.
It does work for bigger amplitudes such as 1V.
Is it supposed to work?
Best regards
Bernt
--
OOO - Own Opinions Only
Best wishes
John Woodgate, Rayleigh, Essex
UK
Keep trying
|
Question/ Problem with voltage source
Hello,
I am using a voltage set to
SINE(0 1u 50)
which is 1uV 50Hz.
Using transient analysis
.tran 100m?
It does not work. It just outputs / simulates to a straight line sloping from 1nV to -500nV over 100ms
I was sure this did work just yesterday and I got a sine wave as expected.
I suspect it stopped working earlier today after I did an AC analysis.
I have since restarted LTSpice and done a whole new schematic. Same problem.
It does work for bigger amplitudes such as 1V.
Is it supposed to work?
Best regards
Bernt
|
Re: Simulation problem concerning the use of the same variable twice in a formula
By the way, there should be no difficulty having two R's in the formula.? It should handle any number of R's.
Are you aware that your resistor value's formula has a Boolean XOR?? In this part of the formula:
(R + 7981113806679325/4503599627370496)^2
the "^" operator means XOR.? Is that what you really wanted?
Perhaps you meant that to be "**2".
The only time "^" means exponentiation is when it is used within a Laplace function.
Andy
|
Re: Simulation problem concerning the use of the same variable twice in a formula
Elien,
Your resistor's expression?
{(((7216103745845419*R)/281474976710656 - 48730063831763729805207428564385/1267650600228229401496703205376)/((R + 7981113806679325/4503599627370496)^2 + 4937677430752859/281474976710656) + 2691614897875927/1125899906842624}
has unbalanced parentheses.
I think that is the cause of LTspice's inability to process the parameter R.? Fixing the parentheses results in a different error message ("Singular deck expression"), but apparently it is not fatal and the simulation proceeds.? I think it results in math overflow when calculating that resistor's value, so LTspice might make it infinite (effectively removing it from the circuit).
Andy
|
Simulation problem concerning the use of the same variable twice in a formula
Hello, In the second circuit of my LTspice schematic (Parallel_gains_R.asc) RLout_c gives the following error: Unknown parameter "*r". I suspect the problem is that I used the variable "R" twice in the formula. The "R's" I use refer to the same variable.? When I used just one "R" in the past, this problem did not occur.? Can someone help me find a solution to simulate it with the formula that consists of two "R's"? I would be very grateful as this is the final result I need to finish my master's thesis (that is due next week). Please see the files in the folder: /g/LTspice/files/Temp/Parallel_gains_R.zipElien
|
Re: Import LTspice simbol model of UCC5304 problem
john23, In your schematic "driving_mosfet.asc" which you uploaded today, you forgot to ground (or provide a path to ground from) the right-hand side of the UCC5304.? Its "VSS" pin should be grounded.? You forgot to do that. That is needed for two main reasons:
- SPICE insists on it.? Every part of every circuit MUST have a path to Ground.
- Your circuit depends on it.? The MOSFET that you drive from the UCC5304 is referenced to Ground.? Therefore, its gate drive signal (your node Vo1) must be referenced to Ground.
Andy
|
Re: Import LTspice simbol model of UCC5304 problem
I wrote, " What is the symbol SQ3426EV.asy for?? I don't see it on your schematic." Sorry, that is my mistake.? I do see it on your schematic (I was looking at the wrong schematic when I wrote what I did above). If you had used LTspice's NMOS symbol, you would not need to rotate it strangely on your schematic as you did with your custom symbol, and it would appear on the schematic like an actual MOSFET. As Tony already explained in #153652, it was unnecessary to create a custom symbol for a type of part that already exists in LTspice.? The custom, auto-generated symbol makes your schematic more difficult to read and understand. Andy
|
Re: Import LTspice simbol model of UCC5304 problem
john23 wrote, "How I got an error shown in the attached photo.What gone wrong when i tried to use the symbol created by eetech00 good model?"
It looks to me like you forgot to include the SPICE model in your simulation.
eetech00's test schematic, uploaded 27 April, had the line ".inc UCC5304.txt" to include the SPICE model.
Your schematic has nothing that I can see to include the SPICE model.? Therefore, the SPICE model (the subcircuit named "ucc5304") is missing from your simulation.? It can't find a subcircuit that is not there.
What is the symbol SQ3426EV.asy for?? I don't see it on your schematic.? Even if it were on the schematic, where is the model file needed for that device?? It's apparently in "C:\Users\yefimv\Documents\LTspice\sq3426\SQ3426EV_PS.LIB".
Why did you upload it twice?
Why did you create a symbol for what appears to be a FET?? LTspice already has FET symbols (NJF, PJF, NMOS, PMOS, NMOS4, PMOS4) which you should have used.? Having a FET symbol with the Gate on the upper right and Drain on the left is contrary to normal schematic standards.
Since SQ3426EV is an N-channel MOSFET, you should have used LTspice's "NMOS" symbol for that part.
You also wrote, "The LTspice files and models i made were uploaded into sim_mos_driver2 folder below."? Actually, you did not upload any models.? You uploaded only one schematic and two symbols, but no models.
Andy
|
Import LTspice simbol model of UCC5304 problem
|
John Woodgate
Tony Casey