开云体育

Nope im referring to the "symbol" of the voltage source located in the left diagram not the results...
*note that there is a sine wave in the symbol itself..


I found the left side diagram somewhere, and tried to plot my own in the right diagram, but the symbol of the voltage source is different.

That makes me wonder if I am getting the same results as the diagram on the left.


Regards,

Desmond



------------------------------------

Yahoo! Groups Links

--- In LTspice@..., Landrum Haddix <lhaddix@> wrote:

Hi,
I may be missing something obvious. I've been measuring lots of ripple voltages on DC power supply votages.
Is there a way to get a waveform showing RMS AC volts regardless of offest.

I did a crude work around and temporatily place a 15pf cap in series with a 10meg resistor hanging off the node I want to measure.
I'm calling this an AC coupled 'Scope probe'. What is the regualr way to do this.

Landrum Haddix
lhaddix@

Hello Landrum,

You questions are somewhat ambiguous, since there is no such thing in this context as an RMS AC waveform.

If you just want to look at the AC portion of the waveform in the viewer, you have several choices:
- Change the Y-axis plot range to only show the portion of the waveform, you're interested in. This method has the disadvantage that every time the viewer re-plots, it will autoscale so you will have to repeat the scaling exercise. An alternative is to save a .plt file with your preferred axis settings, and reload it each time the waveform is re-plotted. Hint: assign a Hotkey to do this. I use [spacebar] like others have mentioned recently
- Plot the quantity V(ACnodename)-DCOffset (where DCOffset is the numerical value for the estimated offset.

Of necessity, this will be a manual process, as the waveform viewer has no way of knowing what you mean it to plot. Alternatively, you can carry on doing it your way, but with the same advantages and disadvantages as AC-coupling with a real scope.

If you actually want to measure the rms value, as suggested by the title of your post, you can use post-processing scripts to calculate that from the simulation data.

Add the following lines in a SPICE directive:
.meas TRAN Vavg avg V(out); calculates the DC offset
.meas TRAN Vrms rms (Vavg-V(out)); calculates rms after substracting the average

You will find the results of these calculations in the logfile after each simulation. Of course having found the average value by this means, you can then substitute its value into your viewer plot expression. This is helpful since if you are also performing a .stepped simulation, the Waveform Viewer won't calculate the average and rms values of a waveform.

One more tip: if the AC voltage is small compared to the DC offset, you will also need to add the directive:
.option plotwinsize=0

...too, or the waveform compression will distort the ripple voltage and the rms calculation will be wrong.

There's also a really nerdy way to display exactly what you want to see in the waveform viewer, but it requires some subterfuge, and can only show the ripple voltage right at the end of your tran time, since it calculates the DC offset on the fly. This will only work if your DC offset is stable over time. You can find this example as RMS_Value.zip in Files>Temp

Hope this helps.

Regards,
Tony

Now that I have well over 100 different diode types in Ltspice I think

Helmut bottom posts, and it's his group.

In Rome, shouldn't we do what the Romans do?

--
JF

--- In LTspice@..., "gasoltroll" <johan.lans@> wrote:

Hi
i'm looking at an impedance curve of a non-ideal tantalum capacitor in LTSpice. The test circuit and impedance curve is seen in this screengrab:

The spice file is here .
So, the imdpedance curve shows the expected impedance minimum, but also an unexpected maximum at about 100MHz, where there is also a polarity switch in phase. This feature does not show up if I do an impedance plot in octave:


octave:1> f = [1000:1000:1e9];
octave:2> C = 2e-3C = 0.0020000
octave:3> R = 2e-3R = 0.0020000
octave:4> L = 1e-9L = 1.0000e-09
octave:5> z = R + f.*2*pi*j*L-1./(f.*2*pi*j*C)
octave:6> loglog(f,abs(z))
octave:7> semilogx(f,atand(imag(z)./real(z)))

Which result in these plots



The parameters in the octave code are the same as in LTSpice component. Anyone know where this comes from? The phases look pretty different, is there something wrong with the test circuit?

Hello Johann,

Please set a value for Cpar when you have set Lser.

Right-mouse-click on the capacitor. Then set the following.

Equivalent parallel capacitance(Cpar): 0p

Best regards,
Helmut