Noise Analysis of AD8021 in LTSPICE

Hello
I am trying to perform SPICE Analysis of Operational Amplifier Voltage Noise Analysis for the AD8021 Low Noise Operational Amplifier.  
As per the data sheet the Voltage Noise specification is as follows :
Voltage Noise Spectrum of AD8021 Opamp
The Flicker Noise is at about 40nV/rt.Hz at 10 Hz and tapers down to a broadband white noise of about 2.1nV/rt.Hz at about 100kHz.
I am trying to generate the same results in LTSpice using a buffer operational amplifier circuit as shown below :
LTSpice Simulation of AD8021 SPICE Macromodel
The results obtained are as follows:
LTSPICE Noise Simulation Results
Now in the above Output Noise Plot, I am seeing the flicker noise start off in agreement with the datasheet noise spec of around 40nV/rt. Hz at 10Hz and tapers down to a value which is far off from the data sheet specs at 1kHz.  Then proceeding further down, we are finding that the White Noise (Broadband) Component is of the order of 7.55nV /rt.Hz at 100kHz whereas the datasheet lists a 2.1nV/rt.Hz value.  This reading seems to be significantly off.
I tried replicating the results with other SPICE Simulators like TINA-TI from TI.  The Flicker Noise component starting point and trend seems to be matching in that case, but the White Noise Component is steady at 5.52nV/rt. Hz., which is also more than twice the figure quoted in the datasheet specs.
Am I doing something wrong or is there an accuracy limitation in the AD8021 SPICE Model provided in the Analog Devices Page for Noise Simulations ?
Parents Reply Children
  • Thank you Hooman.  Much appreciated.  Will wait for the response from the team.  

    Regards

    Ajith

  • +1
    •  Analog Employees 
    •  Super User 
    on Jan 7, 2021 5:09 PM in reply to ajith.peter

    Hi Ajith,

    I've heard back from folks in charge of AD8021 macromodel.

    They have updated the pspice macromodel of AD8021 to correct for the noise discrepancy you had pointed out. They will also update the web site with the updated model.

    Thanks for bringing this to our attention. Here is the updated model:

    ad8021.txt
    * AD8021 Spice Model 
    * Modified by Tim Green on 5/21/2020 to fix Vn and In to match DS.            
    * Description: Amplifier
    * Generic Desc: 250MHz very low noise op amp
    * Developed by: TRW
    * Revision History: 08/10/2012 - Updated to new header style
    * 4.0 (10/2001)
    * Copyright 2001, 2012 by Analog Devices, Inc.
    *
    * Refer to http://www.analog.com/Analog_Root/static/techSupport/designTools/spiceModels/license/spice_general.html for License Statement.
    * Use of this model indicates your acceptance with the terms and provisions in the License Statement
    *
    * BEGIN Notes:
    *
    * Not Modeled:
    *       distortion is not characterized       
    *       disable is not characterized
    *
    * Parameters modeled include:
    *       open loop gain and phase vs. frequency
    *       output voltage 
    *       Common Mode Rejection
    *       input common mode voltage range
    *       slew rate
    *	Voltage noise
    *	Current noise
    *	Output current to supplies
    *
    * END Notes
    *
    * Node assignments
    *                   non-inverting input
    *                   |    inverting input
    *                   |    |    positive supply
    *                   |    |    |    negative supply
    *                   |    |    |    |    output
    *                   |    |    |    |    |     Ccomp
    *                   |    |    |    |    |     | 
    .subckt AD8021      1    2    99   50   45    10
    
    ***** Input stage
    
    Rc1 99 4 rmod 1190
    Rc2 99 5 rmod 1190
    Q1 4 1 6 nbjt
    Q2 5 3 7 nbjt
    Re1 6 8  rmod 1128
    Re2 7 8  rmod 1128
    
    Ibias 8 50 840u
    
    ***** Input Error Sources
    *Rshort 2 3 rmod 1E-3
    eos 2 3 poly(2) 30 98 64 98 39.6e-3 1 1e-3
    gnoise1 98 1 33 98 1e-4 
    gnoise2 98 2 33 98 1e-4
    
    Cin+ 1 0 2pF
    Cin- 2 0 2pF
    Rin 1 2 rmod 10Meg
    
    ****** CMR Stage
    
    Gcmrr 98 64 97 98 13n
    Rcmrr 64 65 rmod 1e6
    Lcmrr 65 98 1.59
    
    ****** Gain Stage & Dominant Pole
    
    Rgain1a 98 10 rmod 1.3263Meg
    Ggain 98 10 4 5 13.48m
    Cgain1a 98 10 2e-12
    
    Dpvc 10 80 diode
    Vpvc 99 80 2.28
    
    Dnvc 81 10 diode
    Vnvc 81 50 2.68
    
    ****** Second Pole
    
    Ggain2a 98 13 98 10 0.01
    Rgain2a 98 13 rmod 100
    Cgain2a 98 13 0.80p
    
    
    ****** Reference Stage
    
    Eref1 98 0 poly(2) 99 0 50 0 0 0.5 0.5
    
    Eref2 97 0 poly(2) 1 0 2 0 0 0.5 0.5
    
    ****** Voltage noise stage
    
    rnoise1 39 98 7.3e-4
    
    vnoise1 39 98 0
    vnoise2 31 98 0.75
    dnoise1 31 39 dn
    fnoise1 30 98 vnoise1 1
    *rnoise2 30 98 1
    rnoise2 30 98 0.01
    
    ****** Current noise stage
    
    rnoise3 32 98 0.166e-3
    vnoise3 32 98 0
    vnoise4 34 98 0.545
    dnoise2 34 32 dn
    fnoise2 33 98 vnoise3 1
    rnoise4 33 98 1
    
    ****** Output Stage
    
    Dout1 13 11 diode
    Dout2 12 13 diode
    V1 11 44 -0.884
    V2 44 12 -0.884
    
    Vo1 91 99 0
    Go1 91 44 13 99 15.823
    Go2 44 51 50 13 15.823
    Vo2 50 51 0
    
    Rout1 91 44 rmod .0632
    Rout2 44 51 rmod .0632
    
    Vout 44 45 0
    
    Fout 98 72 Vout 1
    Diout1 72 74 diode
    Diout2 73 72 diode
    Viout+ 74 98 0
    Viout- 73 98 0
    
    Fsy+ 99 0 poly(2) viout+ Vo1 6.25e-3 1 1
    Fsy- 0 50 poly(2) viout- vo2 6.243e-3 1 1
    
    
    .model rmod RES(t_abs=-273.15)
    .model diode D(IS=1e-15,AF=0,KF=0)
    .model nbjt npn(bf=56)
    *.model dn d(kf=1e-13,af=0.55)
    .model dn d(kf=1e-9,af=0.55)
    
    .ends
                          
    
    
    
    
    
    

    I had to change the file extension to *.txt to be able to upload here. To use it in pspice or LTspice, you'd have to change the file extension back to *.lib please.

    Regards,

    Hooman

  • Thank you Hooman and AD team.  This helps a lot.  Much appreciated.