GBW of an OpAmp simulation problem

I have GBW specification for an OpAmp GBW>=10MHz. How to check this in Cadence? I did stb analysis and got PhaseMargin=63deg @ 12.5MHz. I thought that GBW is frequency at which the open loop gain reduces to 1 (0dB), so my GBW is 12.5MHz. But, when I do gainBwProd of output signal of stb schematic I get 2.5KHz!
Which is real GBW of my OpAmp, what measure calculator and is GBW requency at which I have Phase Margin?

How is the opamp supposed to be configured in application?
On silicon, we inject a sine wave, and find the frequency in which its gain drops to half.

The best method is to find the closed loop response, and get the product of the -3dB bandwidth and the DC gain.
The problem with open loop for gbwp is that the response must resemble that of a pure single-pole system in order for the measurement to accurate.

Connect a high L (10H) from output to neg input of opamp and a high C (10F) from neg input to ground. connect a AC source with AC-Mag=1V. add a cap at the output of the opamp to GND( depends on your load, typ 1p F). now run a AC analysis, sweep freq from 1Hz to 10Ghz. plot dB20(Vout_Opamp) and phase(Vout_Opamp) to get gain and phase response (where Vout_Opamp is the opamp output node).

Find the freq at which gain drops to 0dB. thats your unity gain BW!

Make sure your phase margin is more than ~50 degree at 0dB gain for better step response.

I would like to add that as you have a very powerful cadence tool, always check your ac simulations with transient simulations. AC simulation is just a linearized response. For phase margin and bandwidth unity gain configuration will give you the answers you need. Apply sine waves and see if they get distorted (Linearity error, or slew rate error). Apply square waves and observe the settling behaviour.

For a small example; in the last year I've designed an Opamp with very high phase margin like 80 degrees or so. It was supposed to be used in a switched capacitor circuit. But later I've found out that the output is ringing. After a while I've found out that I've increased the zero resistor unnecessarily high. So my ac results seemed perfect yet I had awful transient results. Always check transient.

Thank you all. findsriharsha's method is closer to me. I did AC simulation as you said, but circuit for this simulation is unity buffer, so when I plot db20(Vout_Opamp) it is constantly 0dB till about 200KHz an then is getting lower (-30dB at 5MHz). Do I have to set some specific DC voltage of Vsin source (supply of OpAmp is single 1.8V, DC voltage of Vsin I set to 1V)

BTW, I forgot to mention in my last post:AC source with AC-Magnitude should be connected to positive input of opamp

Dont forget the input common mode voltage to add. you can use a DC source in series with the AC source. if your supply is 1.8, then input CM voltage should be near 0.9, but check you design to make sure!

Ok, AC source is on + input I set CM at 1V, AC magnitude 1V, it seems to be ok. I run simulation and get on db20(Vout_Opamp) graph that characteristic (gain) is constantly 0dB till about 10MHz and then goes down. You said: "Find the freq at which gain drops to 0dB. thats your unity gain BW!" My question is: how to find one point where gain drops to 0 when gain is equal to 0 for range 0-10MHz?

Spliter said:

Ok, AC source is on + input I set CM at 1V, AC magnitude 1V, it seems to be ok. I run simulation and get on db20(Vout_Opamp) graph that characteristic (gain) is constantly 0dB till about 10MHz and then goes down. You said: "Find the freq at which gain drops to 0dB. thats your unity gain BW!" My question is: how to find one point where gain drops to 0 when gain is equal to 0 for range 0-10MHz?

Click to expand...

if your gain in unity-gain buffer configuration starts to drop down at 10 MHz, this is your GBW!

The point when the gain meets 0 dB is the GBW that you can measure open-loop

Hello there guys,

I hope someone can help me out here.

I am designing a 2 stage OTA with the following specs: Av = 80dB, BW = 15kHz, PM = 60º, Cload = 20fF, Idd of 150uA and a Dynamic Range of 1V.

I want to calculate the gm1 of the differential pair, and for that I can use GBW = (1/2pi) * gm1 / Cc. We can estimate Cc as being 2 to 3 times smaller that Cload. However, I don't know how to get the GBW. Can someone tell me how I can do it?

Apart form that, if I wanted to get the value of gm1 from the gain, how I could do it? I have done some calculations based on this:

r0 = VA/I;
Av = gm * r0;

gm = I / (Vov)

Av = gm * VA/I

From here we can get the gm, however, I don't know if it's the solution to calculate gm based on this because of the Va voltage (which I have determined for several W/L).

How can I estimate VA taking in to account the Av?

To finish, I saw in some book that the expression of the gm can be written as: gm = 2 ID / (Vgs - Vt). If we use this expression, that ID is the value of the current that enters in the differential pair? (PMOS differential pair)

Regards.