Build an Op Amp SPICE Model from Its Datasheet – Part 2

Share this page on Facebook
Share this page on Twitter
Share this page on Google Plus
Share this page on Linkedin
Share this page on Pinterest
Email this page

Part 1 of this article ( shows how to create a behavioral model of an operational amplifier based on the following parameters found in the datasheet: Input and output resistance, input capacitance, DC gain, and offset voltage. As an example I chose Analog Devices’ ADA4004. Let’s continue building this model to simulate the Gain Bandwidth Product.

Gain Bandwidth Product

The Gain Bandwidth Product, describes the op amp behavior with frequency. Op amps have a dominant pole, inserted by manufacturers on purpose, so that the op amp is stable at any gain down to zero dB. See this article for more details: Op Amp Gain Bandwidth Product. In that article I showed that ADA4004 has a cutoff frequency at 24 Hz. This frequency is not identified in the datasheet, but can be easily calculated from the open-loop minimum gain of 500000 and the gain bandwidth product of 12 MHz.

Starting with the cut-off frequency, the open loop gain versus frequency plot has a drop of 20dB for every decade of frequency. To simulate this we need to introduce this pole in our SPICE model. Question is, how?

We could introduce a pole as in the following figure. This circuit shows a simple RC network with its cutoff frequency at 1/(2 π RC).

One pole network with voltage source

Figure 1

However, I prefer its Norton equivalent as in Figure 2.

Figure 2

My opinion is that it is easier to work with Norton sources, especially when one builds such pole and zero circuits. As with any current source, the frequency response depends on the load impedance. If we take an ideal current source generator with infinite bandwidth and load it with a resistor in parallel with a capacitor, the frequency response will be exactly one pole response.

The circuit in Figure 3 shows a voltage controlled current source (VCCS) connected at a resistor-capacitor parallel network. Its input is driven by a voltage AC generator.

VCCS with RC network

Figure 3

The transfer function of the current source has A/V = Mho units, so this is a transconductance amplifier. The circuit shown in Figure 3 has the following transfer function.

One pole transfer function with VCCS (1)

where with VCCS  I noted the voltage-controlled-voltage-source transfer function which has units of Mho, and &#x3C9 is the function variable.

This transfer function can be adapted for ADA4004 if we choose the VCCS gain as 1 Mho, the resistor R = 500 kOhm and the capacitor C = 13.263 nF. The product between 1 Mho and 500 kOhm gives us the op amp gain of 500000 and the RC time constant sets the cutoff frequency at 24 Hz.

With this in mind, we can go back to our op amp model and replace the voltage-controlled-voltage-source (VCVS) with VCCS. However, we run into a problem. How do we isolate the RC network from our output resistor? If we simply replace the VCVS with the VCCS circuitry we just discussed, the output resistor and the op amp load will appear in parallel with the RC network, affecting our pole. The answer is simple. Add another VCVS with the transfer function of 1V/V.

The following figure shows the new ADA4004 model with all the elements we discussed until now.

ADA4004 macro model 2
Expand this figure

Figure 4

A Multisim simulation of the op amp open loop response is shown in Figure 5.

ADA4004 open-loop bode plot
Expand this figure

Figure 5

This Bode plot resembles ADA4004 open-loop gain characteristic as shown in its datasheet (Rev. F) Figure 14. However, there is a difference between my model’s Bode plot and the one shown in the datasheet. In the datasheet graph the phase starts to drop after 1 MHz. This means that there is another pole exactly where the phase becomes 45 degrees. We will see in the next article how to include that pole in the model.


10 thoughts on “Build an Op Amp SPICE Model from Its Datasheet – Part 2

  1. I would like to thank you for the efforts you have put in writing this web site. I am hoping the same high-grade blog post from you in the upcoming as well. Actually your creative writing abilities has encouraged me to get my own blog now. Actually the blogging is spreading its wings rapidly. Your write up is a good example of it.

    • I do not have any signal with a duty-cycle in this article. If you want me to help you need to tell me what article/schematic/figure you are taking about. Or, if this is a general question, let me know in what context.

    • Place a positive power supply and a negative power supply at the op amp output. Connect a diode with the anode at the output and cathode at the positive supply. Connect another diode with the cathode at the output and the anode at the negative supply. The positive power supply value has to be the maximum op amp’s output trip plus 0.6V (a diode drop) and the negative supply value has to be the minimum op amp’s output trip minus a diode drop.

Leave a Reply to damu Cancel reply

Show Buttons
Hide Buttons