开云体育

Dear subscribers of the LTSpice-List,

I uploaded the concerned Schematic and the model of AD734 to

(files->temp->AD734 4 Quadrants Multiplier)

I am not sure, if my problem is actually related to my schematic or the model or if it is rather an LTSpice-operator problem (i.e. me).
Here it comes:

I run the transient analysis with 100 kHz sine waves on both inputs which converges thanks to the .options that I found in AD734_test.asc in the "files->lib->ad734" folder. The resulting waveform is a sine with 452 mV amplitude, 200 kHz, offset about 400 mV. Fine so far. I can play with phases between the inputs etc. It is not giving surprising results.
When I run an AC analysis the result depends on what I include in the sine wave parameters, especially on the phase.
Confer also the to jpg's in "files->temp->AD734 4 Quadrants Multiplier".
Example: Parameters of the input function 1 and 2 are sine waves (100 khz, 3 V). The Bode Plot shows a magnitude of 7.5 mV at 200 kHz.
When the first input is changed to the same sine wave but at a phase of 45°, the output changes to 643 mV at 200 kHz.

Now two questions arise for me:
a) Why is the .ac simulation influenced at all by the parameters of the transient simulation?
b) Why does the amplitude of the output in the transient analysis not coincide with the magnitude in the Bode plot at 200 khz (452 mV vs. 7.5 mV or 643 mV)?

I hope I could make my point clear. I would be very glad if someone could point me how to solve these issues.
Regards,
Maren

Maren (distheo@...) wrote:

a) Why is the .ac simulation influenced at all by the parameters of the

transient simulation?

In an .ac analysis, LTspice first needs to find the operating point. All
voltage and current sources are set to their values at t=0.

Since you specified a SINE source with a phase shift of 45 degrees, the t=0
value is 0.707* 3.0 = 2.12132V.

Regards,
Andy

FYI ... after running an AC analysis, if you hover the mouse pointer over
any net, look in the lower left corner where LTspice will tell you the DC
operating point voltage on that net.

Andy

b) Why does the amplitude of the output in the transient analysis not
coincide with the magnitude in the Bode plot at 200 khz (452 mV vs. 7.5 mV
or 643 mV)?

You also need to realize that an .AC analysis is a small-signal linearized
analysis. The multiplier, which is an inherently nonlinear device, is
presumably linearized at the operating point, and treated as a linear gain
block.

Thus, if you were to input (say) 100 kHz to both input ports (as you have),
you would not find any 200 kHz on the output ... and LTspice would not plot
the amplitude of the 200 kHz (that this chip actually outputs) ... because
an .AC analysis does not generate sum-and-difference frequencies. If
anything, it will only tell you how much of the 100 kHz goes through
because of leakage/imbalance, and because of the fact that the other port's
bias voltage was not 0.0V.

One might even question if you can do an .AC analysis at all. Whether you
get anything meaningful, depends on what's inside the model for this part.
Depending on how they modeled it, it might work correctly in a .TRANsient
analysis, but not in an .AC analysis. I'm just sayin'.

Regards,
Andy