Kind friends

I seem to have encountered a rather egregious 'precision error' Re: LtSpice

Granting that past experience suggests the problem is likely down to my-own misunderstanding of the application -- I will nonetheless be most grateful for assistance in settling the matter either way!

The circuit under study is a 'bone-basic' 1/2 wave rectifier/filter operating at 60kHz / 50kV (peak)

Cursors set as follows:
Cursor #1: For an amplitude of 49.999993Kv (For all intents and purposes 90°)
Cursor #2: Cursor 1 +100.6626ns (i.e. ≈ 2.1743° 'ahead' of cursor #1)

Hence I would expect an amplitude difference of ≈ -36V However the simulator returns a value of ≈ -40.9V??? --- The cited disparity would seem to exceed that ascribable to a 'rounding' error'?

Note that while the selected diode does not, in actuality, support the simulated frequency or EMF -- such should not be an issue inasmuch as LtSpice does not 'enforce' Trr or Vrrm

Please note that, for the convenience of the readers, I have annotated the screen capture...

Many, many advance thanks for any assistance or insight!!!

 

4v out of 50kv is egregious? Are you using it to design a probe to the next black hole?

 

4v out of 50kv is egregious? Are you using it to design a probe to the next black hole?

Perhaps 'egregious' is a bit strong Even so an error of 0.0098% is larger than one would expect? --- In any event I'm ok with it so long as I may be certain such is merely a rounding artifact

Many thanks for your response!

Best regards
HP

 

I cannot zoom in to see the text details of your entire circuit on my tablet but, as noted a 0.01% "error" could be that a diode has about 0.01% of the capacitance of a 10nF capacitor, that is 1pF. (I cannot see the numbers on your voltage source or any information on the o-scope)

Also, many simulators do not like capacitor circuits with no resistance. You can put a 0.01 ohm resistor in series with your diode or a multi-megOhm in parallel with your capacitor to meet the typical criteria while minimizing the impact to the circuit.

 

I cannot zoom in to see the text details of your entire circuit on my tablet but, as noted a 0.01% "error" could be that a diode has about 0.01% of the capacitance of a 10nF capacitor, that is 1pF. (I cannot see the numbers on your voltage source or any information on the o-scope)

Also, many simulators do not like capacitor circuits with no resistance. You can put a 0.01 ohm resistor in series with your diode or a multi-megOhm in parallel with your capacitor to meet the typical criteria while minimizing the impact to the circuit.

Many thanks for your reply!

FWIW Here's the ".asc"

 

Are you using the default Tolerances, or have you set them to something else in Control Panel?

 

Are you using the default Tolerances, or have you set them to something else in Control Panel?

I merely opened the program, selected new schematic, then drafted the circuit -- If it's of any assistance I've attached the .ASC file to post #5

Many thanks for your reply!

Best regards
HP

 

See

View attachment 102233

 

@Bordodynov (and anyone wishing to respond)

First of all many thanks for your time and effort in assisting me with this!

So... I have a few questions -- please be patient - I'm new to LtSpice (my experience with said application being confined principally to 'schematic entry').

But to begin:
Ltspice directive/statement:...............My Interpretation....................................Questiom
.param Tmax={7440.25/60000}........ Load Tmax = (7440 Cycles+90°) := 124ms --- Why 'add' the extraneous 7440 Cycles?


Please indicate whether I have correctly interpreted the following statements
Statement................................................My Interpretation
.meas Vmax Find V(a) at {Tmax}...............Load 'Vmax' := EMF at 90° ?
.meas Vsh Find V(a) at {t1} ......................Load 'Vsh' := EMF at 90° ± ≈ 2.1743° ?
.meas delta param Vmax-Vsh....................Load 'Delta' := Vmax-Vsh ?
.meas ph param 100.6624n*60000*360......Load 'ph' := calculated angle per T1 interval (≈2.1743°) ?

Please explain why this 'textual run' returns the correct result whereas the graphical simulation was in error? (IOW what was I doing wrong?)

With heartfelt thanks and very best regards!
HP

 

Why 'add' the extraneous 7440 Cycles?

HP I say it's to allow enough rc TCs to make sure c1 isn't messing with readings!

 

Hypatia's Protege.
Yes. Tmax=7465.25*60000
I looked at your chart. But the difference in the result not will be. You can take any period. You did not properly understand the results. I increased the calculation accuracy. Ask directive ".opt reltol=1u" and make calculations, and repeat your measurements. With the default settings the result was just as bad as you.

 

Hypatia's Protege.
Yes. Tmax=7465.25*60000
I looked at your chart. But the difference in the result not will be. You can take any period. You did not properly understand the results. I increased the calculation accuracy. Ask directive ".opt reltol=1u" and make calculations, and repeat your measurements.

So, as I understand your reply, my error owed to insufficient precision?

I've just attempted to set the Relative Tolerance to '1u' (i.e. 1*10^-6) as (shown below) -- however that seems to have compounded the error?
Please advise...?

Again, I entreat patience -- I apologize for my slow-wittedness in this matter! --- Many thanks!
HP

 

You are not there to change the accuracy. You have changed the graphical information. On the calculation is not affected. I prefer to write parameters on the circuit. See

 

HP. To improve the accuracy of graphic information pick you need to remove compression.
it is .option plotwinsize=0.

 

@Bordodynov -- Thanks!

I've run the simulation having issued the 'onscreen' directive: ".option plotwinsize=0." -- with much improved results (please see immediately below) - Howbeit not as accurate as your results (attached to post #8)

---Post continued 'below' image---


When attempting to run the simulator having issued the ".model" directive shown in post #8, I receive the following error/warning dialog:

---Post continued 'below' image---


And the erstwhile erroneous results on the 'plot' (Please see below) - Please advise? ---- Many thanks for your patience!



Best regards
HP

 

I recommend .option plotwinsize = 0 reltol = 1u. But remember that the raw-file is very large.

 

I recommend .option plotwinsize = 0 reltol = 1u. But remember that the raw-file is very large.

Thank you! -- I'll give it a try and post my results!

Very best regards
HP