The Designer's Guide Community Forum

The Designer's Guide Community Forum
https://designers-guide.org/forum/YaBB.pl
Simulators >> Circuit Simulators >> question on convergence
https://designers-guide.org/forum/YaBB.pl?num=1138064547

Message started by ah_bhong on Jan 23^rd, 2006, 5:11pm

Title: question on convergence
Post by ah_bhong on Jan 23^rd, 2006, 5:11pm

Hi,
I have 2 questions on the convergence of the spectre simulator.

1) what is the different between setting the "node set" and "initial condition" in the convergence aids menu ?

2) I am working on a biquad filter design as shown in attached picture,
the DC point, where i indicated in the picture, is always giving me the wrong value.
i have to do a node set at that point for the filter to work properly.
My question is, why the DC operating point is giving me the wrong result, and
by doing the "node set" am i looking at the correct result ?

thanks and cheers
bhong

Title: Re: question on convergence
Post by Marc Murphy on Jan 25^th, 2006, 3:05pm

It looks like that's a floating node at DC. You've got a resistor connecting to two capacitors. At DC that node is just the dangling end of a resistor.

Nodeset is an initial guess to help the tool converge faster for DC analysis or the initial value in transient analysis.

Initial condition is for transient simulations.

Title: Re: question on convergence
Post by ah_bhong on Jan 25^th, 2006, 6:07pm

Hi Murphy,
Thanks for the reply.

Yes, i agreed with you that there is a floating node at DC.
In fact, this is the place that i feel most uncomfortable with after checking through the DC operation of the circuit.
But i am uncertain by putting a nodeset at that point, does it guarantee that the circuit will work ?
Have you encountered similar problem before ?

cheers
bhong

Title: Re: question on convergence
Post by Ken Kundert on Jan 26^th, 2006, 12:38am

I don't see a floating node. Clearly terminal 1 of the second opamp is not floating as it is driven by the output of the first opamp.

Nodesets would not fix a floating node (but an initial condition would).

Why do you think you are getting the wrong value? Remember that a nodeset will not guarantee a particular value, it is merely a suggestion. In the end, with nodesets, the resulting values must represent a valid operating point.

-Ken

Title: Re: question on convergence
Post by huber on Jan 26^th, 2006, 9:02am

I agree, there are no floating nodes in the schematic you've given. Presumably the DC value should be determined by the CM output of the first opamp, which in turn should be determined by its Vocm terminal. Are you sure your CMFB is working properly? If you simulate the amplifier by itself, does it give the correct CM output? What type of CMFB are you using? If it's a switched-capacitor CMFB circuit then it probablly contains floating nodes that need to be initialized.
-Dan

Title: Re: question on convergence
Post by ah_bhong on Jan 26^th, 2006, 5:14pm

Hi thanks for all the reply and suggestion ...

1st thing, the CMFB i used is similar to the one in the book from Paul Gray " Analysis and Design of Analog Integrated Circuits" pg839

and the reason why i suspect the node is foating or not in the correct DC is because,
upon simulation on the OpAmp alone, the output CM is working fine.

and when i simulate the attached circuit using a DC sweep on the input CM,
the DC value at that particular node is different from the DC op point reflected after annotation.
(i hope i have explain myself clearly ... )

To Ken,
I do not quite understand the reason of using the nodeset means to the simulator.
could you kindly elaborate more ?

To huber,
I will not rule out that my CMFB is not working properly,
especially the simulation on the feedback path, which i am quite unsure at this point.
Could you kindly suggest is there any reference that talk about simulation on the feedback of the CMFB ?

thanks again and cheers
bhong

Title: Re: question on convergence
Post by Marc Murphy on Jan 27^th, 2006, 8:02pm

ah_bhong wrote on Jan 25^th, 2006, 6:07pm:

Sorry if I led you astray with my earlier comment...it doesn't make sense to me now! It seemed similar to a problem I had with floating-gate MOSFETs. :-?

Disclaimer: I'm not sure this is relevant to the problem at hand, but it's true for the floating-gate stuff I've been looking at lately! :)

For a capacitively-coupled floating node, the simulator can't figure out what the right DC voltage is. Whatever you tell it is what it uses. So, I don't think it can find the 'right' value on its own...whatever you tell it is right. The way to make it work involves adding a resistor network that at DC gives the same node voltage that the cap-coupled charge distribution gives.

To answer your question more clearly, I don't think using a nodeset is going to give you a right answer unless you've already decided what the voltage at that node should be! The best it can do is get your simulation running because the DC solution can be found.

Title: Re: question on convergence
Post by deltasigmaADC on Dec 7^th, 2016, 12:00am

I was searching for the difference between nodeset and initial condition. I stumbled upon this old post. I would recommend this following cadence link.

https://community.cadence.com/cadence_technology_forums/f/33/t/29843

I'm not sure if ah_bhong is interested in the circuit after 12 years.
Like ken said there is no floating node in the circuit. But it's true that there is no DC feedback for an actrive RC integrator. But for a Biquad there is DC feedback around both the integrators which will sets the DC differntial voltage.

I think one thing that you need to see where the poles are located once you put in the real opamp( with finite DC gain and finite bandwidth). Finite DC gain shifts your biquad pole towards LHP and finite bandwidth pushes your poles towards RHP. If you don't have enough bandwidth in your opamp you could very well end up with a circuit with poles on RHP which is unstable.

I hope this help.

Thanks