how to run the simulaiton for 1 ns step interval ..?

Sunil,

I understand that English is almost certainly not your first language, but your question makes absolutely no sense at all and so it's virtually impossible to give you an answer.

Please take extra care and re-formulate your question such that we might have some chance of understanding it.

Best Regards,

Andrew.

Hi Sunil

I am guessing here so please correct me if I am wrong. Let me just try to help interpret the question:

You have a design that has 1 million nodes and it currently takes 10 days to simulate. You found that the simulation time step is sometimes in fs or ps range and so would like to increase the time step to 1ns in an attempt to speed up the simulation. But you found that even after setting time step to 1ns, the actual steps shown in the log file are still in fs or ps range. Why is this so?

1 lakh = Indian numbering systeming for 100 thousand.

Best regards
Quek

Hi,

Sorry - I am little bit busy and so can't able to concentrate on what Iam typing -

I have a circuit with 1 million components and i need it to simulate for 1 microsecond.

But simulator is taking 10 days time -

In time analysis options, I have seen an option and kept step as 1ns and max_step as 4 ns but the simulator again calculating for 30 fs and 3 ps etc.,

So, is there any chance to tell the simulator to calculate only for 1 ns, 2ns, 3ns etc,. upto 1us.

Or is there any other way to increase the simulation speed.

regards
Sunil

Sunil,

You cannot constrain the "minimum" simulation time. If the simulator is taking very short timesteps, it does so in order to ensure it accurately follows the signals - if you were able to stop it doing this, it could easily become inaccurate as it would then miss vital detail.

What can cause short timesteps? Here's a few suggestions:

1. Check that you don't have very sharp edges on voltage or current sources. The simulator will need to zoom the timestep in to follow the sharp edges, so that's not a good thing.
2. Very large component values (e.g. very large inductors and capacitors) can cause instability and oscillation
3. Are you over-tightening the tolerances? Start by leaving as many settings (e.g. reltol, vabsol, iabstol, etc) at default, and just use errpreset=liberal or errpreset=moderate on the transient analysis
4. Discontinuities in device models can cause problems, especially if there is insufficient parasitic capacitance to damp out the discontinuities. Using cmin=1f or cmin=0.1f as a transient option can help (this adds a capacitance to ground from every node). Be careful of this though...
5. Try using APS (spectre +aps in the latest releases) to see if that helps to speed up the simulation
6. Speak to Cadence Customer Support to get more advice - and maybe somebody can look at your simulation setup and output logs to give more specific advice.

Regards,

Andrew.