Dear,

I'm pretty new to Cadence's ADE and Ocean, therefore I would look some advice on the best 'way to go'.

Normally, I would sweep the phase difference (linear) between -2PI and 2PI, run a transient for each phase difference and extract the average output current.

Is this something that can be set up easily under ADE or would OCEAN be preferred?

Kind Regards

Peter

Dear Andrew,

I was able to set up the parametric analysis using ADE. However, it seems I cannot have this run over corners
using the Corner Analysis Tool.

Could it be that this can only be set up using OCEAN scripting (using a parametric analysis statement in combination with a corner run functional call?)

Kind Regards

Peter

Dear all,

in the meanwhile I have been able to let the anomalies 'disappear' (obtain a nice straight line through the origin)

by either applying restart=no (transient analysis options)
   or  skipdc sigrampup

However, from the manual, I do not understand WHY this helps...

Kind Regards

Peter

Dear Andrew,

I will try your suggestion out and let you know.

I personally am pretty sure it's no circuit problem, since the circuit is a 3-state PFD: all-digital, simulated under typical conditions.
This should result in a straight line (except maybe for some deadzone).

It's clear to me these 'dips' are simulator anomalies.

Now, restart = no helped me out, I'll see what your suggestion does...

Regards

Peter

Dear Andrew,

I understand your scepticism towards the circuit  :), but this time I'm 100% sure it's a simulator anomaly, since I actually simulated the circuit for the X-values which -according to the sweep analysis - would result in the large dips.

When I did that, the average output was a value that:
a) differs from the one shown by the sweep analysis
b) lies nicely on the expected straight line through the origin

Regards

Peter

Hi Peter,

Just because you simulated the circuit at the X points with the dips, and were then seeing good results, does not mean that all is OK with the world  

Effectively the two suggestions I made are telling spectre to rebuild the matrix from scratch, or to restart the simulator altogether (in the envSetVal case). This removes the history of what was done previously, and so that doesn't influence the operating point found.

What concerns me is that your circuit has more than one operating point. In the case where the simulator starts from scratch, it is finding the "good" operating point. In the case where you're doing a parametric analysis, it's sometimes finding the "bad" operating point. (I use the terms "good" and "bad" in quotation marks, because they are good and bad as far as how you want the circuit to behave; I'm not saying that the simulator is coming up with a false result). When you have multiple operating points, which one you end up in can be dependent on the starting conditions for solving the operating point - just because most of the time you end up in one does not mean that the other one is false.

Often when you have this kind of scenario, you can use nodesets to push the circuit into one solution or the other.

With spectre, false convergence is something that really doesn't happen. That said, you need to be careful about models - for example, a few years ago one of the large foundries has a veriloga resistor model which suddenly became a negative resistor when high voltages appeared across it - what could
happen during convergence iterations was that it could get a high voltage across it during an intermediate step along the way to convergence, the resistor went negative, and then it could get locked into this nonphysical convergence region - despite the fact that in normal operating ranges it would never occur. I've seen the same thing happen with verilog-a models of non-linear resistors (using some quadratic voltage dependency, say); again, the resistor value can have more than one solution.

Of course, circuits themselves can have more than one operating point.

So this is why I think you really need to look carefully at the waveforms you're getting from the points in the parametric simulation which show the dips - to see what is going on in the circuit. Perhaps you can write the operating point from one of these, and then try simulating that X point with that file as a nodeset, and see what happens?

Regards,

Andrew.