Stats

Locked Locked
Replies 2
Subscribers 126
Views 4851
Members are here 0

This discussion has been locked.

You can no longer post new replies to this discussion. If you have a question you can start a new discussion

DC sweep results do not match DC operating point results

I'm simulating a negative impedance convertor as shown below (the vcvs's gain is set to 100k, and the output range is 0-1.5V, R0 = 10k, R1 = 1k, R2 = 20k):

I swept the voltage at Vin from 0-1.5V and got the result below (Vcm is set to 0.75V):

The result is as expected - it behaves like a -200k resistor in the range of 0.1-1.4V.

However, when I connect another resistor (from analogLib) in series with this block, it behaves weird.

R0 here is 300k, and I was expecting to get a 100k equivalent resistance (300k-200k=100k) at node Vtest. I got the satisfying result indeed if I set Vtest to 1V and print the DC operating point after running a DC simulation (as shown in the picture above).

However, if I sweep the voltage at node Vtest, I get a different result - the current flowing into the node is 3.125uA now. Unfortunately, this value matches with the transient simulation, in which I set up a ramp input.

I checked the DC voltage at each node based on the transient simulation, it also makes sense (the circuit is now working out of the expected range of 0.1-1.4V). Does this mean that the simulator might have found 2 solutions for this circuit? Does this mean that the circuit has some kind of 'unstable' behaviour in terms of operating points?

Doronzzz over 1 year ago

I plot the i-v curve of the external resistor onto the i-v curve of the negative impedance convertor to find the possible solutions.

There are multiple solutions (intersections) indeed. Does spectre have warnings when finding multiple solutions in a DC simulation?
Cancel
Vote Up 0 Vote Down

Cancel
Frank Wiedmann over 1 year ago in reply to Doronzzz

Not in a simple DC analysis because it does not check for multiple solutions there. You can use nodesets to guide it towards the desired solution. For a systematic check, you can do a Hysteresis Sweep, see support.cadence.com/.../techpubDocViewerPage
Cancel
Vote Up 0 Vote Down

Cancel

Community Guidelines

The Cadence Design Communities support Cadence users and technologists interacting to exchange ideas, news, technical information, and best practices to solve problems and get the most from Cadence technology. The community is open to everyone, and to provide the most value, we require participants to follow our Community Guidelines that facilitate a quality exchange of ideas and information. By accessing, contributing, using or downloading any materials from the site, you agree to be bound by the full Community Guidelines.