+ Post New Thread
Results 1 to 3 of 3
  1. #1
    Junior Member level 3
    Points: 1,286, Level: 8

    Join Date
    Jul 2012
    Posts
    26
    Helped
    0 / 0
    Points
    1,286
    Level
    8

    How to define port in cadence which has a impedance value that is frequency dependent

    Hi Everyone,

    I am trying to use a port with complex value as a output termination in SP simulation of cadence. For example output port impedance value is 1/(2*pi*freq*C) which is also frequency dependent. Is there any idea how to do this in cadence? Thanks in advance.

    •   AltAdvertisment

        
       

  2. #2
    Advanced Member level 5
    Points: 28,215, Level: 40
    BigBoss's Avatar
    Join Date
    Nov 2001
    Location
    Turkey
    Posts
    4,069
    Helped
    1232 / 1232
    Points
    28,215
    Level
    40

    Re: How to define port in cadence which has a impedance value that is frequency depen

    Unfortunately "freq" variable cannot be used in Spectre s-parameters simulations.However it's possible to use in ADS.



    •   AltAdvertisment

        
       

  3. #3
    Advanced Member level 5
    Points: 14,423, Level: 28
    pancho_hideboo's Avatar
    Join Date
    Oct 2006
    Location
    Real Homeless
    Posts
    2,169
    Helped
    595 / 595
    Points
    14,423
    Level
    28

    Re: How to define port in cadence which has a impedance value that is frequency depen

    Quote Originally Posted by Ata-Va View Post
    I am trying to use a port with complex value as a output termination in SP simulation of cadence.
    What simulator do you use ?

    Use correct terminology.
    We can use many simulators, e.g. Synopsys HSPICE, Mentor Eldo, Keysight ADSsim, Keysight Goldengate, etc. in Cadence Virtuoso.

    Quote Originally Posted by Ata-Va View Post
    For example output port impedance value is 1/(2*pi*freq*C) which is also frequency dependent.
    Is there any idea how to do this in cadence?
    What do you mean by "in cadence" ?

    Quote Originally Posted by BigBoss View Post
    Unfortunately "freq" variable cannot be used in Spectre s-parameters simulations.
    Wrong.
    Frequency expressions are possible by using "$freq" even in Cadence Spectre.

    This is available for "analogLib/res", "analogLib/ind" and "analogLib/cap".

    However Spectre primitive, "resistor", "inductor" and "capacitor" don't have ability of treating frequency expressions actually.
    Spectre treats frequency expressions by Spectre primitive, "bsource" internally.
    See "spectre -h bsource".

    Currently, we can not use $freq for Spectre primitive, "port".

    So use "analogLib/res" and "analogLib/ind" instead of "analogLib/port".
    Here negative resistance is not available if you use $freq for r=func($freq) in "analogLib/res".

    It seems Spectre primitive, "bsource" can not reflect negative resistance.

    On the other hand, Spectre primitive, "resistance" can reflect negative resistance.

    "test_freq_expression.scs"
    Code:
    // Generated for: spectre
    // Generated on: Nov  2 13:55:42 2018
    // Design library name: My_RFDE_Test
    // Design cell name: test_freq_expression
    // Design view name: schematic
    simulator lang=spectre
    global 0
    
    // Library name: My_RFDE_Test
    // Cell name: test_freq_expression
    // View name: schematic
    PORT0 (x1 0) port r=50 x=0 num=1 type=dc
    R0 (x1 net1) resistor r=cos(2*acos(-1)/100M*$freq)
    L0 (net1 0) inductor l=sin(2*acos(-1)/100M*$freq)/(2*acos(-1)*$freq)
    simulatorOptions options psfversion="1.1.0" reltol=1e-3 vabstol=1e-6 \
        iabstol=1e-12 temp=25.0 tnom=25.0 scalem=1.0 scale=1.0 gmin=1e-12 \
        rforce=1 maxnotes=5 maxwarns=5 digits=5 cols=80 pivrel=1e-3 \
        sensfile="../psf/sens.output" 
    sp sp center=1G span=100M annotate=status 
    saveOptions options save=selected
    Last edited by pancho_hideboo; 2nd November 2018 at 11:59.


    1 members found this post helpful.

--[[ ]]--