|
Re: LTspice XVII error work around
#Time-step-too-small
开云体育On 27/02/2025 11:33, Robert via
groups.io wrote:
While changing the time base in some way can apparently cure the #Time-step-too-small problem, it can also do the reverse, as can any other circuit change. You also don't mention whether you have set a maximum time step. Sometimes this also makes the issue disappear. The underlying issue remains that one or more of the models is dodgy in some way. -- Regards, Tony |
|
Re: LTspice XVII error work around
#Time-step-too-small
I have also found that altering the start time of switching regulators can stop singular matrix (SM), time step (TS) and/or femtosecond crawl issues.
The MC34036 switcher invariable causes problems if permitted to start on its own.
Precharging its timing capacitor with ic=1.5 added to the capacitor's value causes the regulator to start later because the capacitor must discharge down to 1.24V before the requlator starts pumping.
In one instance, this was all it took to eliminate my singular matrix issue.
?
In another case, changing a capacitor ESR value in a charge pump eliminated a time step issue.
Also, I often find that reducing the tolerance values of trtol, abstol, vntol and chgtol help convergence and to reduce the likelyhood of SM, TS or femtosecond pace issues as a circuit grows.
?
I have a simulation that only runs with the level3a op-amp that comes with LTspice with its parameters set to mimic my desired op-amp.
Replacing the level3a with almost any "real" op-amp's model immediatly causes a singular matrix in some diode or transistor in some other part of my project that has nothing to do with the amplifier circuit where the op-amp was replaced.
Erasing that semiconductor with modifications to keep things working, simply shifts the complaint to another unrelated semiconductor and then another and so on, until I go back to the level3a op-amp.
I have tried dozens of "real" op-amp models and most cause the ascribed failure.
The ones that don't, have been so far removed from my desired op-amp, they are of no use to me in this instance.
Every one of those op-amp models works as it should when in a simple test circuit. ?
At times, I have to add a V source between ground and the output of switching requlator to prop up that output.
Doing so elimintes any ripple at the switcher's output and most likely reduces transient currents within the regulator circuit.
It can take a lot of trial error problem solving from there to eliminate the return of SM or TS issues when the prop is removed.
?
I push the go button and hold my breath each time after adding to or altering something in my project
?
All for now ?
Sent:?Thursday, February 27, 2025 at 5:33 AM
From:?"Robert via groups.io" <birmingham_spider@...> To:[email protected] Subject:?Re: [LTspice] LTspice XVII error work around #Time-step-too-small Well after a day of fiddling about with the values in my .OPTIONS and different integration methods (including the suggestions in the FAQ), I finally got my circuit modelling with just:
?
.OPTIONS ITL4=100 ABSTOL=1E-9 VNTOL=1E-3 RELTOL=0.01
?
You'll notice I took out CSHUNT. 5e-12 was the value I had to use (with LTSpice XVII) before I added the LT1375HV. Now I have got the model to converge with the LT1375HV (for the moment, at least; I have more things I need to add), I found that I could make CSHUNT anything from 5e-20 to 5e-12, with no obvious effect, so I then removed CSHUNT completely and it still converges. So what did I do to make it converge?
?
What I'm trying to determine is inrush current, so I have a PWL voltage source set to mirror what the external power supply will do when the test is performed for real. I happened to have it going from 0 volts at 1 ms to 28 V at 2 ms (because the test is defined in ms, and I like to steer clear of whatever SPICE does at time 0). Sometimes it's good to leave a problem overnight, and in the middle of the night I realised the model always fell apart before it got to 1 ms.? ?So this morning I simply changed the voltage generator to go from 0 at 1 ?s to 28 V at 1 ms, and the problem went away >doh!<. I do still need the .OPTIONS line above, but I'm using the default integration method (which is trapezoidal on LTSpice 24).
?
So there's another way to address the problem; timeshift the model so the circuit is doing something different at the time when the non-convergence kicks off.
|
|
Re: .MEAS Failure
On Wed, Feb 26, 2025 at 12:19 AM, Andy wrote:
?
FYI, that is not what I suggested.? Leave the Start and Stop (or Left and Right) values alone.? Let LTspice figure them out on its own.? Change the text in the "Quantity Plotted" box.? THAT is the thing that shifts the entire waveform horizontally.
?
Thank you for removing my blinders.
It's the Quantity Plotted box located within the Horizontal Axis dialog.
That box that has no drop-down arrow that always just says "time".
Forgive me, I'm a Quantity Plotted virgin.
I use LTspice to develop entire PCB's using multiple logic, op-amp, reference, regulator, and discrete parts.
.TRAN simulations of "time" on the abscissa is all I've ever asked of LTspice.
I have had no use for the Quantity Plotted box for so long that it became invisible to me.
?
A side note for the ADI folks:
According to the help file under Axis Control;
"For example, for real data, if you move the mouse to the bottom of the screen and left click, you can enter a dialog to change the horizontal?quantity?plotted."
?
A right click enters the Quantity Plotted box, not left click as stated in the help.
?
?
But I suggested it only as a way to visually see smaller increments of time, which you do not need to do if you don't want to.
?
Yes, now I understand where the disconnect in communication occured.
I sought to enquire of LTspice if a certain signal ever went below 2 volts.
I then sought to enquire of the group, why less-than (<) errored out, in my search for that signal to go below 2 volts.
You explained how LTspice uses interpolation to obtain the precise time when the signal would have reached exactly 2 volts.
?
Looking for the time when it happened was only secondary to my investigation.
The exact time when it happened to 15 digits was not on my radar screen.
I was seeking the time value of the first sample that was found to be less than 2 volts so I could know where to zoom the plot window.
I simply needed to locate the event in the plot pane to support further visual analysis of the plots.
The correct answer to a question that was not asked confused me.
?
Beware observer bias.
?
All for now
?
_._,_._,_
|
|
Re: Stepping MOSFETs
开云体育On 27/02/2025 04:45, Andy I via
groups.io wrote:
As of 24.1.4, it is still broken. I tried the original method, which failed, before adding the modification suggested by Matthias.But it was temporarily broken when V24.1 was first introduced.Is it still broken? An equally serious issue, IMHO, is that the new method is not supported by older versions of LTspice. Obviously, there is a workaround by including both options on a new schematic, with a note to enable only one of them, but that is no help for people with old schematics wanting to use the new LTspice version. -- Regards,
Tony |
|
Re: Stepping MOSFETs
开云体育On 26/02/2025 18:12,
larry.gunseor@... wrote:
Is it possible to STEP 2 different MOSFETs in a simulation run.? I've read about stepping models, and about basic subcircuits, but can you call one MOSFET file for the first step run and another MOSFET file for the second step run.Yes, it can easily be done with the simple use of the AKO: syntax. But it was temporarily broken when V24.1 was first introduced. A modification of this method is now required, example: Stepping_Models_post-V24.1.zip. -- Regards, Tony |
|
Re: LTspice XVII error work around
#Time-step-too-small
开云体育It looks like a corrupt download to me: an
error in the PDF code. Delete the .ZIP and try downloading
again. On 2025-02-26 16:31, ehernan3 via
groups.io wrote:
--
OOO - Own Opinions only If something is true: * as far as we know - it's science *for certain - it's mathematics *unquestionably - it's religion |
|
Re: LTspice XVII error work around
#Time-step-too-small
开云体育On 26/02/2025 16:58, Robert via
groups.io wrote:
5pF is very high capacitance to add to every node in your circuit. It could significantly change the behaviour of many circuits. Does the supplied LT1375HV example circuit simulate OK in your version of LTspice without any .options? I just tried it in XVII V17.1.15 and it worked fine. I guess your schematic must have other components on it, since you "added the LT1375HV"? Most likely, it would be one of those that was causing problems. The LT-supplied models usually don't cause any problems at all, but other proprietary models, often do. If you still have trouble, you might consider uploading your schematic to Files > Temp, together with all models and symbols that didn't originally come with LTspice. Multiple files should be uploaded in a zip. Someone will take a look. -- Regards, Tony |
Tony Casey
eewiz
F.an
John Woodgate