Stats

  • Locked Locked
  • Replies 4
  • Subscribers 126
  • Views 18373
  • 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

Problem with initial conditions for large Capacitor value

palz

Hi,

I am quite new to Cadence spectre. I was trying to simulate a simple RC circuit (with time constant 0.05 s ) with sinusoidal input supply with frequency of 250 Hz.

I have a problem with the initial conditions in the capacitor. The initial condition seems to be ignored when the capacitor value is greater than 1 mF.
What could be the problem?  Kindly help me find a solution to this issue.

Parents
  • Andrew Beckett

    Hi Pallavi,

    The issue is actually caused by the resistors being so small, not the capacitors being large. In fact in the last case, spectre gives you a warning telling you about the problem (probably does in case 3 too - I didn't go back and re-check):


    Notice from spectre during IC analysis, during transient analysis `tran'.
       C0: Initial condition computed for node out is in error by 9.52381 mV
         (95.2381 %).
         Decrease `rforce' to reduce error in computed initial conditions.
         However, setting rforce too small may result in convergence
         difficulties or in the matrix becoming singular.

    Initial conditions are met by applying a voltage source in series with a resistor, rforce which defaults to 1ohm. So with a 5 ohm resistor, you'd expect to get the initial condition of approx 5/6*10mV - which is 8.333mV which is pretty much what you see. With a 50mOhm resistor, you're going to get a tiny proportion of the initial condition - hence the message above. If I set the option rforce=1m then you get closer to the initial condition (I would be wary of setting it too much lower than this though - generally speaking tiny resistors are bad for convergence). This rforce can be set on Simulation->Options->Analog or by adding:

    myopts options rforce=1m 

    in the netlist.

    Of course, your circuit is presumably rather artificial - 1F capacitors are not very common on IC circuits... and spectre has been optimised to work with real-life circuits rather than artificial ones like this (so be wary of using excessively large or small component values).

    Regards,

    Andrew.

Reply
  • Andrew Beckett

    Hi Pallavi,

    The issue is actually caused by the resistors being so small, not the capacitors being large. In fact in the last case, spectre gives you a warning telling you about the problem (probably does in case 3 too - I didn't go back and re-check):


    Notice from spectre during IC analysis, during transient analysis `tran'.
       C0: Initial condition computed for node out is in error by 9.52381 mV
         (95.2381 %).
         Decrease `rforce' to reduce error in computed initial conditions.
         However, setting rforce too small may result in convergence
         difficulties or in the matrix becoming singular.

    Initial conditions are met by applying a voltage source in series with a resistor, rforce which defaults to 1ohm. So with a 5 ohm resistor, you'd expect to get the initial condition of approx 5/6*10mV - which is 8.333mV which is pretty much what you see. With a 50mOhm resistor, you're going to get a tiny proportion of the initial condition - hence the message above. If I set the option rforce=1m then you get closer to the initial condition (I would be wary of setting it too much lower than this though - generally speaking tiny resistors are bad for convergence). This rforce can be set on Simulation->Options->Analog or by adding:

    myopts options rforce=1m 

    in the netlist.

    Of course, your circuit is presumably rather artificial - 1F capacitors are not very common on IC circuits... and spectre has been optimised to work with real-life circuits rather than artificial ones like this (so be wary of using excessively large or small component values).

    Regards,

    Andrew.

Children
No Data

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.