• State
  • Locked Locked
  • Replies 3 replies
  • Subscribers 47 subscribers
  • Views 3629 views
  • Users 0 members are here
Support feedback
Options
Options
Related

This thread has been locked.

If you have a related question, please click the "Ask a related question" button in the top right corner. The newly created question will be automatically linked to this question.

OPA128 input bias current in SPICE model

Bob Lerwill
Prodigy 110 points
Other Parts Discussed in Thread: TINA-TI, LMC6001

I am modelling a transimpedance amplifier using a 100G feedback resistor with both an LMC6001A and an OPA128 using the PSPICE files provided by TI. Our current design uses the OPA128, and I am considering switching to the LMC6001, so I want to model the differences. (I notice that the format for these two files is slightly different, presumably because they came from two different companies that TI bought: NS & BB respectively). I am using LTSPICE because I know it better than TINA-TI. The two simulations were essentially the same (apart from rail voltage change) but gave significiantly different output offsets with zero input current. The LMC6001A gave -1.65mV and the OPA128 gave -3.06V. Having trimmed back the circuit to its basics, the difference is repeatable changing the definition of the Op Amp back and forth. The cause is easy to trace: the input bias current of the LMC6001A model was around 20fA but for the OPA128 it was 30pA. This seems odd because the datasheet for the OPA128 says the maximum inbut bias current is 150fA at 25C. Is there an error in the model or am I doing something wrong?

P.S. I should have mentioned that since we actually use the OPA128 in a 100G transimpedance amplifier at the moment, I know it behaves as I would expect from the data sheet. The offset at the output when the input current is zero is less than 30mV. When I ask "am I doing something wrong?", I mean am I doing something wrong in modelling the circuit, not am I using this device incorrectly.  I would like to get using the OPA128 model right as it helps me optimise the circuit.


PPS there is no tag for the OPA128, presumably because of its NRND status.

  • 0
    TI__Guru 68541 points

    Bob,

    OPA128 macro-model is 20 years old and in fact improperly simulates IB.  I have modified the netlist to correct the problem by adding two dummy resistor, Rdummy1 and Rdummy2 - please see attached. The input bias current is now 40fA - see below.

    OPA128fix.TSC
  • 0 in reply to Marek Lis
    Prodigy 110 points

    Marek,

    Thank you for your prompt response. I am afraid that i do not agree with your analysis. I have tried copying the TINA model you sent and sure enough I get a 15pF input bias current. However if I reduce the GMIN value from its default 1pS to 1fS, I get an input bias current of 30.54pA. I think this is the right thing to do and this makes the TINA analysis agree with the LTSPICE analysis I mentioned in the original post. Fitting two 1T dummy resistors does not cancel out this 30pA current. (I originally thought this difference was becasue you used a different SPICE model, but now I see it was because you had left the analysis parameters at their default values. Please ignore earlier post.)

    I have tried a similar solution to the one you suggest, but using two 500G dummy resistors in the PSPICE model instead of two 1T resistors. This leaves me with about 570fA and an offset of around 57mV. Could you please look at this and see if this solution is appropriate. I am a bit worried that I am just curing the symptom rather than curing the disease.

  • 0 in reply to Bob Lerwill
    TI__Guru 68541 points

    Bob, 

    I am puzzled why 1T dummy resistors I suggested don't cancel IB in your simulation down to 40fA I see in my own simulations - make sure to set the Shunt Conductance to zero (go to: Analysis->Set Analysis Parameters-> scroll to the bottom until you find Shunt Conductance); otherwise, 1pS conductance will cause the 15pA input bias current with (V-)=-15V you report to see – you may want to try to use the attached netlist with Shunt Conductance in Analysis set to 0. 

    If you don't eliminate the effects of shunt conductance on IB by setting it to zero, your solution of using 500G dummy resistors instead of 1T I suggested will work ONLY for -15V supply.

    If you need more help, please send me email directly to: lis_marek@ti.com