Multisim - how to do an ac sweep of voltage, not frquency?

I don't know Multisim anymore because I switched to LTSpice almost exclusively. Normally the way to test for linearity at frequency is to use the FFT display.

If you want to see where "things start to fall apart" you can do set .STEP command to step the input amplitude, then watch where the 3rd and

5th start rearing up.

--
Regards, Joerg 

http://www.analogconsultants.com/

.AC analysis does not work for this because the simulator _linearizes_ the model around the operating point, and the results are the same irrespective of amplitude.

You must use a sinusoidal source, in a .TRAN analysis. Step the amplitude and Fourier the result to see the harmonics.

Some simulators (such as PSpice) also have distortion analysis. You have to pre-specify the source frequency and then the simulator will give you a table of harmonics up to whatever number you request. ...Jim Thompson

--
| James E.Thompson                                 |    mens     | 
| Analog Innovations                               |     et      | 
| Analog/Mixed-Signal ASIC's and Discrete Systems  |    manus    | 
| San Tan Valley, AZ 85142   Skype: Contacts Only  |             | 
| Voice:(480)460-2350  Fax: Available upon request |  Brass Rat  | 
| E-mail Icon at http://www.analog-innovations.com |    1962     | 
              
I love to cook with wine.     Sometimes I even put it in the food.

yes .ac linearizes and you can get unrealistic stuff like megavolts in a transistor circuit.

instead, use .tran analysis, input with V(in) ramp source, pwl ?

I've often used [0, 0, 1, 1] not realistic , but hits the values.

after analysis, the time is the same as V(in), so simplifies if you do quite a few, else request the horizontal to BE V(in) that way you get V(out) vs V(in) labeled.

however the point is well taken to use fft, because small distortions show up bigtime!

PS: I envy you using Microsim, I miss the ability to easily plot the B-H curves of a coil. albeit in [spit, spit, curse begone!] English units.

Seriously get a free copy of LTspice [not certain, but it is FAST!! compared to my Microsim version], plus you can join the users group and then talk apples apples with contributors.

Thanks for the replies - bit more detail:- I bought an AC panel meter (from China) which has appalling linearity. e.g :- mV I/P Display

190 190 100 150 60 92 15 29 I found an internet post from a year or so ago where someone bought a similar model and found the same results. I traced the circuit from the pcb - apart from a couple of capacitor values - and tried simulating it in EWB 5.12, LTspice and Multisim to see if I could improve the action of the precision rectifier before the A-D and LCD driver. Gave up as unable to produce graphs and used scope on the TL082 chip - it was visibly clipping at less than 1/2 FSD! Eventually "cured" by attenuating the input to 1/3 and adjusting the dc input to the ADC (preset pot).