How to calculate the output resistance of a opamp circuit?

[ShowKemp]

Hi,
I'm reading a book about OpAmps and simulating the exercises with LTSpice. Here's the exercise and circuit i'm working with:

Using the basic 741 model (circuit below) direct PSpice to find the closed-loop parameters (Voltage Gain, Input resistance and output resistance) of an inverting amplifier implemented with R1=1k and R2 = 100k.

The circuit on the book:


The circuit built in LTSpice (i have not PSpice so i'm using LTSpice):


The results based on a Ideal OpAmp are:
Voltage Gain = -R4/R3 = -100k/1k = -100
Input resistance = R3 = 1k
Output resistance = 0

Results according to the book:
Voltage gain = -9.995E+01
Input resistance = 1.001E+03
Output resistance = 3.787E-02

To get the results on the simulation i run an AC Analysis and plot traces with algebraic expressions:
Voltage Gain: V(o)/V(i) = -99.949463 (Close to ideal)
Input resistance: V(i)/I(R3) = 1.0005004K (Close to ideal)

I don't know how to the output resistance  , i tried calculating V(o)/I(R2), but got ~100k, this isn't close to 0.
So my newbie question is how can i calculate the output resistance of the circuit?

Regards

[ShowKemp]

After further reading i "think" i found the way to calculate the output resistance:

Ro = Closed-loop output resistance
ro = Open-loop output resistance (75ohms)
L = Loop Gain
a = Open-loop Gain (200,000 V/V or 200 V/uV)

Based on the LTSpice schematic:
L = a / (1 + (R4/R3))
L = 200,000 / (1 + (100k/1k)) = 1980.198

Ro = ro / 1 + L
Ro = 75ohms / (1 + 1980.198)
Ro = 0.0379 ohms ~ 3.787E-02 (Close to the book result)

Still need to get more familiar with the "OpAmp circuit" terms.
Any suggestions on circuit simulations with LTSpice? is it possible to get all this data with one spice command?

[strawberry]

when you take Vgain=99,95 then it will be the same

[Audioguru]

The open loop gain of an opamp is not a fixed number, there is a range of gain, some are high and others even with the same part number are less.
The open loop gain of an opamp is high at DC and frequencies below 10Hz then it drops at higher frequencies due to its frequency compensation capacitor. Therefore the output impedance increases at higher frequencies.

[Zero999]

The calculations look right to me. As mentioned above, the open loop gain varies. Also note that this only applies when the op-amp is working in its linear region and with negative feedback. For example, if too much current is drawn, the op-amp's output will either saturate or the current limiting protection will kick in. It will no longer have any negative feedback and the output impedance will rise dramatically.

[T3sl4co1l]

Yes, this is only correct at DC, in the middle of the range where it's linear.  But for that condition, it is correct.

Tim

[danadak]

This might help -


http://www.ti.com/lit/an/slyt677/slyt677.pdf



Also the Laplace analysis for a single pole comped OpAmp pretty easy. Two pole a little more tedious,
use of partial fraction expansion reveals equivalent lumped model characteristics (which yield easy
insight into Zo behavior).


Regards, Dana.

[Cerebus]

Any suggestions on circuit simulations with LTSpice? is it possible to get all this data with one spice command?

The DC transfer function simulation will deliver you a transfer function (gain), input and output impedances:

Code: [Select]

.tf V(O) V1


[Kleinstein]

One way to "measure" the output impedance of a circuit simulated in Spice is adding a current source to the point of interest. The AC simulation with the extra current as source gives the response to output current and thus the output impedance. An offset current might upset the simple V(out)/I(out) formula. In the example I(out) would be from both resistors, not just the 75 Ohms.

[ShowKemp]

The DC transfer function simulation will deliver you a transfer function (gain), input and output impedances:

Code: [Select]

.tf V(O) V1


Thanks, i didn't knew that command, just tested it and the result seems to be the expected: