Non Linear Resistor in LTspice

Yes, left click, sorry.

Your file wouldn't run for me, so I added 1E9 ohms to ground on the floating bits and replaced the two capacitor values with 500uF (for some reason they were marked 500AuF - I've seen that before with a US schematic?). It then ran and did just what you said, so I changed the .tran to 0.1 seconds from 8 seconds and all was well.

So it looks like some sort of resolution/sampling issue. Of course, Helmut would know :-(

tirsdag den 16. juni 2020 kl. 04.51.52 UTC+2 skrev Ricketty C:

figure out why the voltage on a current sense resistor is not a nice sine wave-ish like the applied voltage to the circuit. I expected a bit of dist ortion around the zero crossing points but otherwise a rectified sine wave.

istor currents I realized the issue was MUCH more fundamental. The current through the resistor is as expected, pretty much a rectified sine wave wit h a bit of distortion near the zero crossing points... but the voltage is t erribly distorted. What finally sunk in was that these were the measuremen ts directly on the resistor as if the resistance was varying!!!

form for resistance much like the voltage waveform. The measured values ar e not weird extremes that might be from parasitic effects, ~3 volts, ~13 mA , 121 ohms. I even tried using a specific resistor part number to make sur e the resistor didn't have some weird default parasitic value on it.

uit simulator? The calculated resistance value over the cycle not near the zero crossings ranges from 120 ohms to 240 ohms.

pto, I don't see anything unusual. I(R6) and V(rect)-V(vsense) match and so does I(R2) and V(rect)-V(Ve)

nt???

There are no custom parts or anything that should upset LTspice. WTF!?

from the floating side, then made it 1 Meg and still get the distorted volt age waveforms.

resistor R6 in series with the opto LED. The voltages elsewhere are a bit large for this to show up for certain since the distortion is only about a volt on a 100 volt signal. With a 50 Vp signal those two resistor voltage waveforms are similarly distorted and the other waveforms are not.

there is something fishy going on, when ran yesterday it was on an old LTspice XVII(x64), May 3, 2017 on linux (wine), and everything looked as expected. I ran it today on LTspice XVII(x64), Sep 11, 2019 on win10 and there I see the same weirdness as you ...

BTW, I'm running LTspice IV.

he waveform display, I also entered it as a formula, V(x)-V(y) and saw the same waveform.

ted in the file for those two parts, so I replaced them. I've looked for n et name shorts and everything else I can think of. The commonality of thes e two resistors is a net from a zero volt voltage source to provide a curre nt measurement. The voltage on that of course is zero at all times.

ause a strange waveform, but not the current to deviate from the voltage.

Thanks. I never would have guessed it was something with the run time. We ird that it has an effect on resolution.

I reset sim settings to default and modified "Integration Method" to Trapaz oidal and the issue was resolved.

Strange that it could whack the voltage but not the current. I entered cal cs to measure resistance and it varies by over 2:1 not counting the transie nts around the zero crossing. It's just not something I expect to see in a simulation.

I really don't get what could be happening that the voltage is messed up bu t not the current.

to figure out why the voltage on a current sense resistor is not a nice sin e wave-ish like the applied voltage to the circuit. I expected a bit of di stortion around the zero crossing points but otherwise a rectified sine wav e.

nsistor currents I realized the issue was MUCH more fundamental. The curre nt through the resistor is as expected, pretty much a rectified sine wave w ith a bit of distortion near the zero crossing points... but the voltage is terribly distorted. What finally sunk in was that these were the measurem ents directly on the resistor as if the resistance was varying!!!

veform for resistance much like the voltage waveform. The measured values are not weird extremes that might be from parasitic effects, ~3 volts, ~13 mA, 121 ohms. I even tried using a specific resistor part number to make s ure the resistor didn't have some weird default parasitic value on it.

rcuit simulator? The calculated resistance value over the cycle not near t he zero crossings ranges from 120 ohms to 240 ohms.

opto, I don't see anything unusual. I(R6) and V(rect)-V(vsense) match and so does I(R2) and V(rect)-V(Ve)

rent???

. There are no custom parts or anything that should upset LTspice. WTF!?

d from the floating side, then made it 1 Meg and still get the distorted vo ltage waveforms.

he resistor R6 in series with the opto LED. The voltages elsewhere are a b it large for this to show up for certain since the distortion is only about a volt on a 100 volt signal. With a 50 Vp signal those two resistor volta ge waveforms are similarly distorted and the other waveforms are not.

ux(wine), and everything looked as expected.

e the same weirdness as you ...

The Integration Method seems to be the simulation setting that chases it aw ay. Different defaults between the two versions of LTspice? Trapezoidal a nd Gear seem to work, while Modified Trap does not.

he opto, I don't see anything unusual. I(R6) and V(rect)-V(vsense) match an d so does I(R2) and V(rect)-V(Ve)

urrent???

es. There are no custom parts or anything that should upset LTspice. WTF! ?

und from the floating side, then made it 1 Meg and still get the distorted voltage waveforms.

the resistor R6 in series with the opto LED. The voltages elsewhere are a bit large for this to show up for certain since the distortion is only abo ut a volt on a 100 volt signal. With a 50 Vp signal those two resistor vol tage waveforms are similarly distorted and the other waveforms are not.

inux(wine), and everything looked as expected.

see the same weirdness as you ...

away. Different defaults between the two versions of LTspice? Trapezoidal and Gear seem to work, while Modified Trap does not.

Just tried LTspice IV and the default Integration Method is the same Modifi ed Trap and it works. So the problem is something a bit more subtle in the differences department.

I just tried it in LTspice XVII and got the same result as you did (i.e. incorrectly). Use only LTspice IV. It works fine in that version.

rapezoidal >and Gear seem to work, while Modified Trap does not.

Mod trap + 'normal' solver iirc turns on some Engelhardt speed hacks that s ometimes cause artifacts. I almost always use plain trap with the 'alternat e' solver, which is a bit slower but better-behaved.

Cheers

Phil Hobbs

Ltspice expects LATIN-1, if you give it UTF-8 you get that error.

I don't know, but I'm thinking this is how LTspice saves the letter mu. I

s. XVII? Maybe not. When I run it in IV it works without complaining.

I guess it is something to do with computer settings??? When I look at the

to convert character sets?

I should try editing the file to using a 'u' instead and see if it still wo rks in LTspice. Maybe that is simply a convenience of the editing tool?

It's a control panel setting.

Cheers

Phil Hobbs