Transimpedance amplifier dynamic range in Capture

[[email protected]]

Hi,
I have a transimpedance amplifier and i want to get a plot of Output
current (ac) versus Input current (ac) in one capture spice simulation
at a particular frequency. An I versus V curve will give me the
dynamic range of the TIA. Can it be done with one simulation.

 

[Bob Penoyer]

Hi,
I have a transimpedance amplifier and i want to get a plot of Output
current (ac) versus Input current (ac) in one capture spice simulation
at a particular frequency.

A TIA accepts a current and turns it into a voltage, not a current.

An I versus V curve will give me the
dynamic range of the TIA. Can it be done with one simulation.

I'll assume you're using PSpice. You should do two simulations. In
one, drive the input with a current pulse. Give the pulse's rise time
and fall time some lengthy times so that they act like ramps. Now run
a Time Domain (Transient) simulation and see how the ramping output
voltage compares with the ramping input current.

In the second simulation, drive the input with an IAC component. Now
do an AC Sweep/Noise simulation. Let the frequency sweep over a large
range, say, 10 Hz to 100 MHz. You might want to change these limits
after you see the results. When the sweep is complete, plot DB(Vout)
where Vout is the name you've assigned to the output node. This will
tell you what the TIA's wideband behavior is.

 

[qrk]

Hi,
I have a transimpedance amplifier and i want to get a plot of Output
current (ac) versus Input current (ac) in one capture spice simulation
at a particular frequency. An I versus V curve will give me the
dynamic range of the TIA. Can it be done with one simulation.

Short answer: Yes.
We'll ignore that a transimpedance amp has a voltage output.
Since you're using Capture, lets assume that you're using PSpice. With
PSpice as your spice engine, this is easy using parametric analysis
and performance analysis.

You need to do a transient analysis since you're looking for
compression versus amplitude. AC analysis won't give you the
information you're looking for.

You need to do a parametric analysis which is another setup box in the
Analysis Setup menu (Analysis Setup is the Schematics program
terminology - find the equivalent in Capture). Set up your parametric
analysis to run a bunch of different input amplitudes from small to
large.

Run the analysis. You will get lots of plots overlaying another. Those
are the plots for each input amplitude value.

This is where PSpice shines... In PSpice (not Crapture), select Trace
in the top menu bar. Select "Performance Analysis". Click on Wizard
and fill in the blanks. You'll probably want to use "Swing_XRange"
which will measure the peak to peak amplitude over a specified time
range. This will give you a nice graph of output amplitude versus
input amplitude. With enough trickery, you can subtract this from a
straight line approximation to see where you get significant deviation
from expected.

This is the main reason I like PSpice's graphing capability.

 

[[email protected]]

That works,
Thank you all.