+ Post New Thread
Results 1 to 11 of 11
  1. #1
    Advanced Member level 3
    Points: 5,456, Level: 17
    Achievements:
    7 years registered

    Join Date
    Jan 2012
    Location
    Italy
    Posts
    952
    Helped
    41 / 41
    Points
    5,456
    Level
    17

    deviding Y value by X values in Cadence Virtuoso calculator

    Hello,

    I need to calcultae the input capacitance of the amplifier from

    Cin_diff=imag(Yin_diff)/(2*pi*freq)

    the frequency is the sweeping parameter comes by running the AC simulation in the x-axsis. How can I put in the formula of Cin ?

    Thank you

  2. #2
    Advanced Member level 5
    Points: 17,003, Level: 31
    pancho_hideboo's Avatar
    Join Date
    Oct 2006
    Location
    Real Homeless
    Posts
    2,613
    Helped
    701 / 701
    Points
    17,003
    Level
    31

    Re: deviding Y value by X values in Cadence Virtuoso calculator



    1 members found this post helpful.

    •   AltAdvertisement

        
       

  3. #3
    Advanced Member level 3
    Points: 5,456, Level: 17
    Achievements:
    7 years registered

    Join Date
    Jan 2012
    Location
    Italy
    Posts
    952
    Helped
    41 / 41
    Points
    5,456
    Level
    17

    Re: deviding Y value by X values in Cadence Virtuoso calculator

    Quote Originally Posted by pancho_hideboo View Post
    Dear Pancho,

    Thank you for your help,

    I used the xval function as shown below

    Click image for larger version. 

Name:	cin2.PNG 
Views:	11 
Size:	37.1 KB 
ID:	155568

    where i7 represent imag_Y which is measured at d from balun for CMOS fully differential amplifier.

    the differential input capacitance is given below

    Click image for larger version. 

Name:	cin1.PNG 
Views:	6 
Size:	25.2 KB 
ID:	155569

    I wondering why input capacitance is decreasing at a higher frequency, I was expecting it to increase as the parasitics starts to appear at high frequency

    Thank you



  4. #4
    Advanced Member level 5
    Points: 17,003, Level: 31
    pancho_hideboo's Avatar
    Join Date
    Oct 2006
    Location
    Real Homeless
    Posts
    2,613
    Helped
    701 / 701
    Points
    17,003
    Level
    31

    Re: deviding Y value by X values in Cadence Virtuoso calculator

    Simply your equation is wrong.
    You have to apply imag() for numerator.

    Generally Capacitance is nearly constant over frequency.
    Last edited by pancho_hideboo; 17th September 2019 at 18:43.


    1 members found this post helpful.

  5. #5
    Advanced Member level 3
    Points: 5,456, Level: 17
    Achievements:
    7 years registered

    Join Date
    Jan 2012
    Location
    Italy
    Posts
    952
    Helped
    41 / 41
    Points
    5,456
    Level
    17

    Re: deviding Y value by X values in Cadence Virtuoso calculator

    Quote Originally Posted by pancho_hideboo View Post
    Simply your equation is wrong.
    You have to apply imag() for numerator.

    Generally Capacitance is nearly constant over frequency.
    Dear Pancho,

    Thank you for your response

    indeed that was the imaginary part, but it is not showing in the calculator. When I draw the i7 from result browser in ADE, I selected signal type as "Imaginary"



    •   AltAdvertisement

        
       

  6. #6
    Advanced Member level 5
    Points: 17,003, Level: 31
    pancho_hideboo's Avatar
    Join Date
    Oct 2006
    Location
    Real Homeless
    Posts
    2,613
    Helped
    701 / 701
    Points
    17,003
    Level
    31

    Re: deviding Y value by X values in Cadence Virtuoso calculator

    Quote Originally Posted by Junus2012 View Post
    indeed that was the imaginary part
    No.
    It is absolute value.

    Don’t believe Cadence ADE.


    1 members found this post helpful.

  7. #7
    Advanced Member level 3
    Points: 5,456, Level: 17
    Achievements:
    7 years registered

    Join Date
    Jan 2012
    Location
    Italy
    Posts
    952
    Helped
    41 / 41
    Points
    5,456
    Level
    17

    Re: deviding Y value by X values in Cadence Virtuoso calculator

    Quote Originally Posted by pancho_hideboo View Post
    No.
    It is absolute value.

    Don’t believe Cadence ADE.
    Dear Pancho,

    it will be nice and very kind of you if you could then tell me the right procedure,

    do you mean I first plot the current (which represent the admittance) in Magnitude, then I send this value to calculator and use the function "imag" ?

    Thank you very much



  8. #8
    Advanced Member level 5
    Points: 17,003, Level: 31
    pancho_hideboo's Avatar
    Join Date
    Oct 2006
    Location
    Real Homeless
    Posts
    2,613
    Helped
    701 / 701
    Points
    17,003
    Level
    31

    Re: deviding Y value by X values in Cadence Virtuoso calculator

    Surely see legend of ViVA.
    imag() is not applied.

    Simply apply imag() in numerator.

    If you plot complex value without applying any function, Cadence ViVA plots absolute value.
    Last edited by pancho_hideboo; 18th September 2019 at 11:37.


    1 members found this post helpful.

  9. #9
    Advanced Member level 3
    Points: 5,456, Level: 17
    Achievements:
    7 years registered

    Join Date
    Jan 2012
    Location
    Italy
    Posts
    952
    Helped
    41 / 41
    Points
    5,456
    Level
    17

    Re: deviding Y value by X values in Cadence Virtuoso calculator

    Dear Pancho,

    Thank you again for your kind answer

    I am applying the "imag" function to the magnitude signal and the result are the same, it shows both have the exact value as you see from the third image (result signal is the one with image fucntion applied)

    below is the admitance in magnitude

    Click image for larger version. 

Name:	cin1.PNG 
Views:	5 
Size:	84.0 KB 
ID:	155582

    here I sent the signal to calculator

    Click image for larger version. 

Name:	cin2.PNG 
Views:	5 
Size:	78.6 KB 
ID:	155583

    here is the result after calculator

    Click image for larger version. 

Name:	cin3.PNG 
Views:	4 
Size:	86.3 KB 
ID:	155584

    Thank you very much



  10. #10
    Advanced Member level 5
    Points: 17,003, Level: 31
    pancho_hideboo's Avatar
    Join Date
    Oct 2006
    Location
    Real Homeless
    Posts
    2,613
    Helped
    701 / 701
    Points
    17,003
    Level
    31

    Re: deviding Y value by X values in Cadence Virtuoso calculator

    Quote Originally Posted by pancho_hideboo View Post
    If you plot complex value without applying any function,
    Cadence ViVA plots absolute value.
    See attached figure.

    Rather I suspect your test bench, since you still can not understand linear circut basics such as differentail mode, common mode, ideal transfomer and etc. at all.
    https://www.edaboard.com/showthread.php?386628

    Show me netlist regarding signal sources, loads, balun and analysis statements.

    "test_Junus2012.scs"
    Code:
    // Generated for: spectre
    // Generated on: Sep 19 09:28:54 2019
    // Design library name: My_RFDE_Test
    // Design cell name: test_Junus2012
    // Design view name: schematic
    simulator lang=spectre
    global 0
    
    // Library name: My_RFDE_Test
    // Cell name: test_Junus2012
    // View name: schematic
    V0 (net2 0) vsource dc=1 mag=1 type=dc
    IPRB0 (net2 net1) iprobe
    R0 (net1 0) resistor r=10
    C0 (net1 0) capacitor c=100p
    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" checklimitdest=psf 
    ac ac start=10M stop=1G dec=50 annotate=status 
    save IPRB0:in 
    saveOptions options save=selected
    Last edited by pancho_hideboo; 19th September 2019 at 14:53.


    1 members found this post helpful.

    •   AltAdvertisement

        
       

  11. #11
    Advanced Member level 3
    Points: 5,456, Level: 17
    Achievements:
    7 years registered

    Join Date
    Jan 2012
    Location
    Italy
    Posts
    952
    Helped
    41 / 41
    Points
    5,456
    Level
    17

    Re: deviding Y value by X values in Cadence Virtuoso calculator

    Quote Originally Posted by pancho_hideboo View Post
    See attached figure.

    Rather I suspect your test bench, since you still can not understand linear circut basics such as differentail mode, common mode, ideal transfomer and etc. at all.
    https://www.edaboard.com/showthread.php?386628

    Show me netlist regarding signal sources, loads, balun and analysis statements.

    "test_Junus2012.scs"
    Code:
    // Generated for: spectre
    // Generated on: Sep 19 09:28:54 2019
    // Design library name: My_RFDE_Test
    // Design cell name: test_Junus2012
    // Design view name: schematic
    simulator lang=spectre
    global 0
    
    // Library name: My_RFDE_Test
    // Cell name: test_Junus2012
    // View name: schematic
    V0 (net2 0) vsource dc=1 mag=1 type=dc
    IPRB0 (net2 net1) iprobe
    R0 (net1 0) resistor r=10
    C0 (net1 0) capacitor c=100p
    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" checklimitdest=psf 
    ac ac start=10M stop=1G dec=50 annotate=status 
    save IPRB0:in 
    saveOptions options save=selected
    Dear Pancho thank you for your reply and sorry to make you upset,

    here is the netlist
    Code:
    // Library name: analogLib
    // Cell name: ideal_balun
    // View name: schematic
    subckt ideal_balun d c p n
        K0 (d 0 p c) transformer n1=2
        K1 (d 0 c n) transformer n1=2
    ends ideal_balun
    // End of subcircuit definition.
    
    // Library name: sen_In_Amp_fully_11_layout2
    // Cell name: In_Amp_fully_11_layout_AC3_test
    // View name: schematic
    V3 (net4 0) vsource dc=1.65 type=dc
    V4 (net17 0) vsource dc=VCM type=dc
    V1 (net018 0) vsource dc=1.65 type=dc
    V0 (vdd! 0) vsource dc=3.3 type=dc
    PD_S (PD 0) vsource dc=PD type=dc
    XPD_S (XPD 0) vsource dc=XPD type=dc
    R5 (Vout_diff 0) resistor r=200k
    R1 (Vout\+ net33) resistor r=100
    R2 (net33 net32) resistor r=100k
    R3 (net32 Vout\-) resistor r=100
    C1 (Vout_diff 0) capacitor c=2.5p
    V11 (VID 0) vsource mag=1 type=sine ampl=1.6 freq=1K
    I6 (0 PD net17 vdd! XPD net28 Vin\+ net4 Vout\+ Vout\- net4 vin\-) \
            In_Amp_fully2
    I10 (vdd! net28) isource dc=Ibias type=dc
    I7 (VID net018 Vin\+ vin\-) ideal_balun
    I19 (Vout_diff VOC Vout\+ Vout\-) ideal_balun
    simulatorOptions options reltol=100e-6 vabstol=1e-6 iabstol=1e-12 temp=27 \
        tnom=27 homotopy=all limit=delta scalem=1.0 scale=1.0 \
        compatible=spice2 gmin=1e-12 rforce=1 maxnotes=5 maxwarns=5 digits=5 \
        cols=80 pivrel=1e-3 sensfile="../psf/sens.output" checklimitdest=psf 
    dcOp dc write="spectre.dc" maxiters=150 maxsteps=10000 annotate=status
    dcOpInfo info what=oppoint where=rawfile
    ac ac start=1 stop=100M dec=100 annotate=status 
    designParamVals info what=parameters where=rawfile
    primitives info what=primitives where=rawfile
    subckts info what=subckts  where=rawfile
    save I7:1 
    saveOptions options save=allpub
    and the circuit is

    Click image for larger version. 

Name:	cin4.PNG 
Views:	3 
Size:	25.4 KB 
ID:	155649

    The circuit about is fully differential instrumentatin amplifier, it employes the same concept of fully differential amplifire where I want to test Cin



--[[ ]]--