+ Post New Thread
Results 1 to 8 of 8
  1. #1
    Full Member level 6
    Points: 3,934, Level: 14

    Join Date
    Jul 2006
    Location
    USA
    Posts
    347
    Helped
    6 / 6
    Points
    3,934
    Level
    14

    how to simulate the input refered noise of an integrator in cadence/spectre

    As the figure shows, do the noise simulation, but the output and negative input node of the amplifier is not "directly" biased, how to get the input referred noise data from simulation?
    Thanks

    Click image for larger version. 

Name:	12.png 
Views:	3 
Size:	1,021.3 KB 
ID:	129361

    •   AltAdvertisment

        
       

  2. #2
    Advanced Member level 5
    Points: 14,695, Level: 29
    pancho_hideboo's Avatar
    Join Date
    Oct 2006
    Location
    Real Homeless
    Posts
    2,222
    Helped
    606 / 606
    Points
    14,695
    Level
    29

    Re: how to simulate the input refered noise of an integrator in cadence/spectre

    Simply specify Iin as iprobe in noise analysis statement.


    1 members found this post helpful.

  3. #3
    Full Member level 6
    Points: 3,934, Level: 14

    Join Date
    Jul 2006
    Location
    USA
    Posts
    347
    Helped
    6 / 6
    Points
    3,934
    Level
    14

    Re: how to simulate the input refered noise of an integrator in cadence/spectre

    Thanks. One issue is that the output of the integrator is vdd or 0, since there is no dc feedback to control it, which gives a wrong simulation data.



    •   AltAdvertisment

        
       

  4. #4
    Advanced Member level 5
    Points: 14,695, Level: 29
    pancho_hideboo's Avatar
    Join Date
    Oct 2006
    Location
    Real Homeless
    Posts
    2,222
    Helped
    606 / 606
    Points
    14,695
    Level
    29

    Re: how to simulate the input refered noise of an integrator in cadence/spectre

    Quote Originally Posted by shanmei View Post
    One issue is that the output of the integrator is vdd or 0,
    since there is no dc feedback to control it,
    which gives a wrong simulation data.
    I can not understand what you want to mean at all.

    "noise analysis" is same as "ac analysis".
    So there is no problem even if there is no dc feedback to control output.


    1 members found this post helpful.

  5. #5
    Super Moderator
    Points: 251,591, Level: 100
    Awards:
    1st Helpful Member

    Join Date
    Jan 2008
    Location
    Bochum, Germany
    Posts
    43,812
    Helped
    13322 / 13322
    Points
    251,591
    Level
    100

    Re: how to simulate the input refered noise of an integrator in cadence/spectre

    Depending on the amplifier parameters, you can either achieve useful bias by setting an initial condition for the initial transient solution, or add a very high feedback resistor during simulation.


    1 members found this post helpful.

  6. #6
    Full Member level 6
    Points: 3,934, Level: 14

    Join Date
    Jul 2006
    Location
    USA
    Posts
    347
    Helped
    6 / 6
    Points
    3,934
    Level
    14

    Re: how to simulate the input refered noise of an integrator in cadence/spectre

    Thanks, Pancho_hideboo.

    For the dc analysis, it is not stable, the opamp behaves like a comparator.

    The integrator only works at the trans-simulation, the input current source keeps absorbing current from the feedback capacitor, and the opamp will keep the voltage of the inverse node of the opamp to be equal to Vref, the output node of opamp voltage is Vout=Iin.*t/C.

    For noise simulation, the negative loop seems not start to work, so the output voltage of the opamp is either vdd or 0. Then the simulation result is not right.

    - - - Updated - - -

    Thanks, FvM.

    It is a good idea for setting the initial condition.

    For adding a large resistor feedback, it might lead to output to be vdd or 0. Iin*Rf will form a voltage drop delta_V,
    then the output voltage of opamp is Vref+delta_V or Vref-delta_V, which might be Vdd or 0 separately.



  7. #7
    Advanced Member level 5
    Points: 14,695, Level: 29
    pancho_hideboo's Avatar
    Join Date
    Oct 2006
    Location
    Real Homeless
    Posts
    2,222
    Helped
    606 / 606
    Points
    14,695
    Level
    29

    Re: how to simulate the input refered noise of an integrator in cadence/spectre

    Use analysis dependent switch such as "analogLib/sp1tswitch".

    https://www.edaboard.com/thread354623.html#12

    If your circuit is truely unstable in DC, connect very large resistor parallel to capacitor. Here you should set inoisy=no in resistor.
    Or use "analogLib/dcfeed".
    Last edited by pancho_hideboo; 30th May 2016 at 16:07.


    1 members found this post helpful.

    •   AltAdvertisment

        
       

  8. #8
    Full Member level 6
    Points: 3,934, Level: 14

    Join Date
    Jul 2006
    Location
    USA
    Posts
    347
    Helped
    6 / 6
    Points
    3,934
    Level
    14

    Re: how to simulate the input refered noise of an integrator in cadence/spectre

    Quote Originally Posted by pancho_hideboo View Post
    I can not understand what you want to mean at all.

    "noise analysis" is same as "ac analysis".
    So there is no problem even if there is no dc feedback to control output.
    You are right. Thanks.



--[[ ]]--