How can I calculate this band-pass filter input impedance?
I know from the datasheet that the Ri and the R0 of the ampop are 2M\$\Omega\$ and 75 \$\Omega\$ and the Gain at the central frequency is 30 dB
\$\begingroup\$
\$\endgroup\$
5
-
\$\begingroup\$ At what frequency? \$\endgroup\$– a concerned citizenCommented May 2, 2018 at 6:33
-
2\$\begingroup\$ Use a simulation tool. \$\endgroup\$– Andy akaCommented May 2, 2018 at 10:25
-
\$\begingroup\$ the frequency is 1Khz \$\endgroup\$– Pedro LopesCommented May 2, 2018 at 12:25
-
\$\begingroup\$ @PedroLopes If it's just that, you can easily determine it through a simulation, plenty of tools available these days. If it's calculations, what have you done so far? \$\endgroup\$– a concerned citizenCommented May 2, 2018 at 14:20
-
\$\begingroup\$ Wich simulation tool do you recommend I use? So far I only know the Gain at the central frequency \$\endgroup\$– Pedro LopesCommented May 2, 2018 at 14:53
Add a comment
|
1 Answer
\$\begingroup\$
\$\endgroup\$
Perhaps the easiest way to determine this without using any math is to simulate it in a program such as LTSpice. If you aren't familiar with this tool, I strongly encourage you to look into how to use it, but I think a general overview is outside the scope of this answer.
To simulate it, you must find a Spice model for the opamp in question (TI conveniently provides one here, but in general you'll need to look around online for the model). The extracted file(s) should be saved to the same directory you plan to create your schematic and simulation in.
Once this is done, open your instance of LTSpice and draw up the schematic. I used the "opamp2" model for the model and entered "UA741" under the "Value" field in the component attribute editor. Then, be sure to add a Spice directive (the ".op" menu item) stating ".include filename.foo" (UA741.301 in this case) to point the simulator to the correct file.
Once the schematic is drawn, set your AC source voltage to something reasonable (I used 0.1V to make sure I didn't saturate the opamp) and configure an AC sweep (Decade, 1 to 100kHz, 1000 steps per decade here) to run. Probe the circuit, and then edit the probe function to be something like "V(Vin)/I(R2)" or "V(Vin)/(I(V1)" to show the input impedance as a function of frequency. Be sure to set the Y axis to "Linear" or it may show it in decibels (not sure how that's supposed to work...).
The result shows an input impedance of ~118k approaching DC, ~18.5k as f->infinity, a minimum impedance of ~13.4k around 1.25kHz, and a "nominal" impedance of 14.25k at 1kHz. Zoom in to see these values.
Sanity Check
Rather than accepting these blindly, lets also verify the center frequency gain is what you say (30dB):
Seems right to me.
Analytical Method
Now, what about if we don't want to simulate it? I won't go into full detail on this, but the process will involve using replacing the opamp with an appropriate small signal model, using Laplace transforms to convert the system into the Laplace domain, then developing a system of equations to describe the circuit. Once this is done, find the input impedance by placing a "test" source on the input and solving for the resulting ratio between Voltage and Current in. Boom, you will have some function of frequency describing the input impedance. The same can be done for the output impedance (test source on output) or any of the gains (voltage, current, transimpedance).
