Hi ayounis,

What's the strange behavior? What's your accuracy setting? What's the ref/output frequency of your PLL?


Yawei

I have tried all accuracy settings that I know. Here is what I remember of them. Remember that there are two cases that I experimented with; case1 is the simulation that runs for 10us and case2 is the simulation that runs for 100us. I saw improper behavior for case2, when it is compared to case1 and also when it is compared to same setup but running hspice. hspice was consistent for the two time durations.
a. From Cadence:
1. setting maxstep for case2 to be smaller or larger than that case1 did not seem to solve the problem.
2. I changed the "step" for case2 to be smaller/larger than that of case1. That did not solve the problem.
3. I tried the different integration methods, no luck.
4. I tried "conservative", "moderate" and "liberal", ... no luck.
5. Changed "reltol" to a much smaller value, no luck.
6. there might be other things that I also did but don't remember now.

b. From command line:
1. I only changed "stop" in input.scs to go from case1 to case2 and I saw the problem. What I mean here is that all other simulator options in input.scs file remained the same, but spectre's behavior was different.
2. I tried different versions of spectre, no luck.

Thats when I gave up and posted this issue!

Ahmed

Thanks Sheldon,
When I run the setup for 10us using spectre, I get what I expect.
When I change the simulation time *only* from 10us to 100us and rerun, I get a totally different behavior of the control voltage. All blocks are working; vco is oscillating with the correct frequency, pfd is working as expected, but the in the first 10us of the simulation, I don't see the same behavior of the control voltage. i.e., the control voltage will look different when you set the stop to 10us and let the simulation finish, and when you set stop to 100us and then stop the simulation after 10us.
Am I making sense here?

Ahmed

The problem came when you specified 0 for a transition time. It makes no sense for the transition function to produce a zero duration transition as it causes a variety of numerical problems. So if you specify a 0 for a transition function, it will do its best to choose a reasonable non-zero value to use. Such behavior is required for every Verilog-A/MS simulator. How that default value is chosen is left up to the simulator, and choosing it as some fraction of the simulation interval is very natural as it scales with the problem.

Bottom line, specify a non-zero transition time.