The Designer's Guide Community Forum

The Designer's Guide Community Forum
https://designers-guide.org/forum/YaBB.pl
Simulators >> Circuit Simulators >> simulating transconductance of a OTA
https://designers-guide.org/forum/YaBB.pl?num=1278297885

Message started by sharkies on Jul 4^th, 2010, 7:44pm

Title: simulating transconductance of a OTA
Post by sharkies on Jul 4^th, 2010, 7:44pm

This has left me in the dark for quite a while now.
I've been trying to figure out how to plot the transconductance of the OTA for a while and I have been unsuccessful.

Let's say that my OTA is a differential pair with pmos active load. Now, I would like to plot gm vs Vid. There has been couple suggestions. As an example, refer to yixiusky's solution in http://www.edaboard.com/ftopic317940.html. Is this the correct way?
I can also try to simulate the transconductance by AC simulation. This is done by loading the OTA with a capacitor, then measuring the AC current at frequency of '1K hertz' of the capacitor while sweeping the DC input voltage by using the 'sweep design variable' option in the ac simulation. The thing is, these two different approaches give quite a different result, and I'm not sure which one I should take.

suggestions?

Title: Re: simulating transconductance of a OTA
Post by nrk1 on Jul 4^th, 2010, 8:58pm

The two should give you the same result. Doing dc analysis and differentiating will be inaccurate if the step size isn't small enough.

In ac analysis, the differentiation of the characteristics happens internally at the device level in the simulator. That way, ac analysis is the safer way. To get the "dc" transconductance. You've to choose a frequency that is low enough for currents flowing through the capacitors negligible.

Nagendra

Title: Re: simulating transconductance of a OTA
Post by Mayank on Jul 4^th, 2010, 9:02pm

Quote:

then measuring the AC current at frequency of '1K hertz' of the capacitor

As Nagendra pointed out, 1KHz should be much below your first pole / -3dB cutoff of your OTA.

As long as accuracy is maintained, both of them are bound to give same result.

--
Mayank.

Title: Re: simulating transconductance of a OTA
Post by raja.cedt on Jul 4^th, 2010, 9:34pm

hi guys,
if you terminate with capacitor how will you take o/p common mode. So my suggestion is terminate o/p with proper dc voltage and sweep the input voltage and find the current and differentiate (don't take so many point to avoid spike in differentiation)

Thanks,
Rajasekhar

Title: Re: simulating transconductance of a OTA
Post by sharkies on Jul 5^th, 2010, 4:39am

OK. I've actually simulated the transconductance and here are the results.

There are THREE plot lines.

CYAN
1ohm resistor connected between the output nodes
AC current through the resistor measured at 1K while sweeping input DC differential voltage

RED
1ohm resistor connected between the output nodes
Take derivative of DC current through the resistor while sweeping input DC differential voltage

PURPLE
cap C0 and cap C1 connected at output of the OTA, C0,C1=1F
AC current through the capacitors measured at 1K while sweeping input DC differential voltage

Clearly, results are different. Can somebody clarify this?

Also, If i try as raja.cedt proposed, I get a similar curve to the CYAN and RED plot.

Title: Re: simulating transconductance of a OTA
Post by Mayank on Jul 6^th, 2010, 1:31am

Is your transconductor Fully- Differential ?
If yes, then do as Raja says.
Set the Bias point for your FD ckt first. Then only can you measure any small signal params.

If your ckt is single Ended, the Output voltage will automatically be set by your Load.
In this case, you can use a cap & measure the ac current through the cap.
It's always better to use a DC voltage source at the output to set your output CM level.

Avoid placing resistors in b/w differential nodes, although in our case for measuring Gm, it should not matter as output is supposed to be AC GNDed.

That being said,

1. Place voltage sources on your output nodes to bias your ckt & measure currents through them.
2. If FD, Itot = Ipos - Ineg. If SE, Itot = Ioutput.
3. Differentiate Itot.
4. This curve is your Transconductance / GM.

Hope this is pretty clear.

Title: Re: simulating transconductance of a OTA
Post by spring on Jul 10^th, 2010, 7:35pm

For full differential circuit, does you circuit has a cmfb to determine the bias of the output point, if so, use a 0V voltage source to connect the two output, then use AC or pss simulation to see the transconduct.
Hope it can help you.
Spring

Title: Re: simulating transconductance of a OTA
Post by blue111 on Sep 3^rd, 2017, 9:51am

I have the following OTA which I think is not fully differential. If I use DC sweep of differential input voltage nodes, what should I do with the 1.8V bias voltage source at one of the input voltage node ?

What about AC method of determining transconductance for my OTA circuit below ?

I read from the various posts above, I have few options to connect the output node to, which are load resistor, load capacitor, or just a bias voltage such as middle of supply voltage.

Could anyone further advise ?

Note: this OTA circuit should be seen as gm-cell which is part of a larger gyrator circuit implementation of active inductor, so I wonder how I would measure the transconductance given that it is frequency-dependent as well ?

Further details of this active inductor could be found at http://www.designers-guide.org/Forum/YaBB.pl?num=1504336936