The Designer's Guide Community
Forum
Welcome, Guest. Please Login or Register. Please follow the Forum guidelines.
Nov 28th, 2020, 5:51am
Pages: 1
Send Topic Print
simulating transconductance of a OTA (Read 7210 times)
sharkies
New Member
*
Offline



Posts: 3

simulating transconductance of a OTA
Jul 04th, 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?
Back to top
 
 
View Profile   IP Logged
nrk1
Community Member
***
Offline



Posts: 81

Re: simulating transconductance of a OTA
Reply #1 - Jul 4th, 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
Back to top
 
 
View Profile   IP Logged
Mayank
Community Fellow
*****
Offline



Posts: 334

Re: simulating transconductance of a OTA
Reply #2 - Jul 4th, 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.
Back to top
 
 
View Profile   IP Logged
raja.cedt
Senior Fellow
******
Offline



Posts: 1516
Germany
Re: simulating transconductance of a OTA
Reply #3 - Jul 4th, 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
Back to top
 
 
View Profile WWW raja.sekhar86   IP Logged
sharkies
New Member
*
Offline



Posts: 3

Re: simulating transconductance of a OTA
Reply #4 - Jul 5th, 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.

Back to top
 

snapshot_005.png
View Profile   IP Logged
Mayank
Community Fellow
*****
Offline



Posts: 334

Re: simulating transconductance of a OTA
Reply #5 - Jul 6th, 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.
Back to top
 
 
View Profile   IP Logged
spring
New Member
*
Offline



Posts: 7
China ShangHai
Re: simulating transconductance of a OTA
Reply #6 - Jul 10th, 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
Back to top
 
 
View Profile   IP Logged
blue111
Community Member
***
Offline



Posts: 75

Re: simulating transconductance of a OTA
Reply #7 - Sep 3rd, 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

Back to top
 
 
View Profile   IP Logged
Pages: 1
Send Topic Print
Copyright 2002-2020 Designer’s Guide Consulting, Inc. Designer’s Guide® is a registered trademark of Designer’s Guide Consulting, Inc. All rights reserved. Send comments or questions to editor@designers-guide.org. Consider submitting a paper or model.