# Two simulations are different. Mine V.S. Paper's

After reading the Fig3 (Asymmetrically pre-damped piezoelectric charger),explanation of its process,i make a schematic(a.) and simulate(c.).However,my simulation and its simulation(d.) are different,i think the time of my switch close or open are right.so i can't find the place i do wrong.

From the first picture,you can find that i use a "vsin" instead of "isin" or "cccs/vccs",this is because i saw a unload wave from another paper,and the PZT output voltage is a sine wave.

Can anyone guess or know where am i wrong?

$V_{CAP}$=$V_{PZ}$,1 means connect and 0 means disconnect for two switch signal

(a)

(b)

(c)

(d)

• Using a voltage source in parallel with a capacitor is useless, since the internal resistance of the source is, ideally, zero, thus the cap is shorted. Using a current source means the voltage will be the integral of the current. It makes a huge difference. – a concerned citizen Apr 15 '18 at 6:16
• @aconcernedcitizen after replacing voltage source with current source"isin",the waveform is still wrong – XM551 Apr 15 '18 at 6:38

You should really try to keep after the example in the paper. Using a capacitor in parallel with a voltage source is not the same as with a current source -- the first simply shorts out the capacitor due to the internal, ideally null resistance, the other forms an integrator.

Looking at your pictures, it looks like you're using a ns scale, while the paper has ms scale. Also, it looks like you'e using a pulsed voltage for the battery(?) instead of a DC. I don't know where did you get the information about the control voltage, but it doesn't look like any of them should be conducting over a whole half-cycle.

So I gave it a try, guessing the values and timings (edit: I accidentally switched the control voltages, reversed them):

The current is a sine, the battery is simplified as a large valued capacitor, precharged to 2V.

I am using LTspice, you are using something different. It doesn't make sense to search for what I used in your library. Whatever voltage controlled switch your library has, that should be used. Additionally, I have plotted controlling waveforms, explained when the switch turns on and off, described the signal of the current source, I am sorry, but you have all you need to build the schematic. The same way you tried to build it from the picture in the pdf, the same way you can see the similarities between my schematic and the picture. I cannot draw things for you, I don't have what you have.

Still, I redid the schematic and I will describe it, maybe LTspice's interface is so unfamiliar to you that you cannot understand what is drawn (but then I don't understand how you managed to understand the picture in the .pdf):

• I1 is a current source, set to be a sine waveform with 5uA (micro) amplitude and 50Hz frequency (or 20ms period);
• C1 is a 15nF capacitor, with an additional flag which specifies that the initial voltage across it is zero (ic=0);
• S1 is a voltage controlled switch with the "on" resistance 1mOhm (milli), "off" resistance 1MegOhm (1e6), threshold voltage Vt=0.5V and Vh=0.5V hysteresis. The switch is turned "on" when the controlling voltage is greater than , or equal to Vt+Vh, and turns off when it's less than, or equal to Vt-Vh;
• V1 is the controlling voltage source for S1;
• S2 is a voltage controlled switch with the same parameters as S1;
• V2 is the controlling voltage source for S2;
• L1, together with its parasitic Rser form the series LR as seen in the picture, same values;
• C2 is the equivalent of the battery, modeled as a large capacitor precharged at 2V.

The waveforms are:

• V(pz) -- the voltage across C1;
• V(c1) -- the control voltage for S1, blue waveform: a pulsed waveform from 0V to 1V, 10ms period, and 1% duty-cycle, no delay;
• V(c2) -- the control voltage for S2, red waveform, same parameters as V1.
• Thankyou,can i ask that what does the blue pulse and red pulse mean?can you show me the cos wave and switch relation?i think maybe i am wrong there – XM551 Apr 15 '18 at 6:48
• It could be that you're not familiar with LTspice, but, then again, neither am I with whatever you used. If you look at the labels, c1 and c2 represent some net labels on the schematic (with red). Those are the controlling voltages (V1, V2) for the two switches (S1, S2). As they show, they are of PULSE type, both with a period of 10ms, 10us rise/fall times, and 1% duty cycle. Out of the two, V1 is delayed by 5ms (as seen in the waveform viewer). I1 is the current source, with a sine waveform of 5uA amplitude and 50Hz frequency, or 20ms period. – a concerned citizen Apr 15 '18 at 6:55
• @a concerned citizen My simulation is not the same as yours,so i want to ask your ideal switch name,and does the "1" mean connected or open for your switch? – XM551 Apr 15 '18 at 9:09
• If you had read my comment carefully you would have seen I named them S1 and S2, clearly visible in the schematic. S1 would be Spz and S2 would be Sb. Surely it's not that difficult to make correlations between the schematic I drew and the picture from the paper? A 1 means closed, 0 means opened. As for why you don't get the same waveforms, I cannot tell. Even your schematic is not only hard to read, but also unfamiliar to me. For example, to me it looks like one end from each the switches is grounded. Note that I am not saying you should use what I use. – a concerned citizen Apr 15 '18 at 9:22
• well i mean the component name,for example:vdc,isin,vsin,etc.Because my ideal switch is different from you,(i don't know how to use my analog switch),and i can't find your switch type in my analog library either.So i make a switch by myself,however,our $V_{PZ}$ are not the same,so i want to find where is the problem.our schematic should be the same,except that switch.but the simulation of testing switch alone is right(almost). – XM551 Apr 15 '18 at 9:33