The Designer's Guide Community Forum

The Designer's Guide Community Forum
https://designers-guide.org/forum/YaBB.pl
Simulators >> AMS Simulators >> Blowing up of current in Cadence Spectre simulation
https://designers-guide.org/forum/YaBB.pl?num=1361310201

Message started by batmanbeginz on Feb 19^th, 2013, 1:43pm

Title: Blowing up of current in Cadence Spectre simulation
Post by batmanbeginz on Feb 19^th, 2013, 1:43pm

Hi all,

I am trying to simulate a simple 2 stage comparator in Cadence Spectre.
However in the transient simulation, its taking a long time with warnings like mentioned below, and finally terminates the simulation:

"
tran: time = 10.05 us (1 %), step = 15.63 ns (1.56 m%)
tran: time = 10.05 us (1 %), step = 57.5 fs (5.75 n%)
tran: time = 10.05 us (1 %), step = 7.019 as (702 f%)

Warning from spectre during transient analysis `tran'.
WARNING (SPECTRE-16266): Error requirements were not satisfied because of convergence difficulties.

Error found by spectre during transient analysis `tran'.
ERROR (SPECTRE-16384): Signal I(M1:d_s_flow) = 1.00277 GA exceeds the blowup limit for the quantity `I' which is (1 GA). It is likely that the circuit is unstable. If you really want signals this large, set the `blowup' parameter of this quantity to a larger value.

Analysis `tran' was terminated prematurely due to an error.
finalTimeOP: writing operating point information to rawfile.
"

I know this blow up is a common problem, still I am not able to bypass this. I introduced cmin=0.1fF still no luck. Also the current values are so low [I am using a verilog a based look up table based model] so that I am wondering how can it exceed GA ? The initial transistor sizing was also not that big to cause so much difference in current.

I relaunched with the attached netlist, but its taking hours to finish 1%. Normally it crashes at 22% of transient.

Can anyone help with this ?

Thanks and regards,

Title: Re: Blowing up of current in Cadence Spectre simulation
Post by Ken Kundert on Feb 21^st, 2013, 7:01pm

This is not a simulator problem. It is a problem with your circuit. Or more specifically, the problem is probably in your models.

To figure out what is going wrong, you need to look at the signal it mentions and find out why the current is exceeding 1GA.

I expect that you will find that:
1. you have a negative resistor, capacitor, or inductor value
2. you have a verilog model that is exhibiting a negative resistance, capacitance or inductance.
3. you have a coupled inductor model and some of the terms were set to zero or ignored (breaking the passivity of the model).

-Ken

Title: Re: Blowing up of current in Cadence Spectre simulation
Post by Geoffrey_Coram on Feb 26^th, 2013, 7:48am

batmanbeginz wrote on Feb 19^th, 2013, 1:43pm:

Also the current values are so low [I am using a verilog a based look up table based model] so that I am wondering how can it exceed GA ?

What does your table look-up say to do when the voltages are outside the table (what extrapolation method)? If the voltages somehow get outside the modeled range, is your model set up to guide the simulator back to reasonable values?