Post Go back to editing

SPICE model of AD549 is incorrect?

Hi every one!

I think that spice model work incorrectly, because bias currents not correspond specifications

Test circuit:

Bias currents is in pico-ampere range:

What is reason of it?



  • Your circuit is invalid.  You cannot operate op amps open loop.  Connect as a follower.

    Second, Spice puts a large resistor on every node.  But for femtoamps, you have to change GMIN.

    See the text in the .cir file and google GMIN.


  • Hi, Harry

    In reality I will not use op-amp in this configuration, this is demonstration only. Now let's have an interesting experiment: place on sheet LMC6001, all settings is default

    Result of simulation

    Bias currents corresponds specification.

    Usually, in SPICE model input part of op-amp very different from real device, for example, bias currents simulate as ideal current sources, therefore configuration of external circuit cannot affect on this parameter. To demonstrate this, I configure op-amps as followers.

    Bias currents of AD549 as follower

    Bias currents of LMC6001 as follower

    I saw this trouble with bias current before, when I simulated TIA on AD549.

  • I tried to run a simulation with the new gmin value, and now behavior of op-amp is adequate.

    I want to understand why this is happening? In my opinion, conductances with GMIN value cause bias current error, because they connect to current sources, which imitate bias currents in model and direct part of this currents to other branches. I am correct understand it?



  • Hi Kirill,

    I think your assessment of the effect of GMIN is accurate. For nodes with very high input impedances, if you set GMIN too low, you're essentially introducing a shunt path from the node which may carry enough current that is significant compared to the currents flowing through that node.

    So, for parts with very low input bias current like AD549, having a large GMIN value is important. Here is what the AD549 spice mode text file states, as Harry had already noted:

    * BEGIN Notes: CAUTION!! To aid in convergence, most Spice simulators add a
    * conductance on every node to insure that no node is floating.
    * This is GMIN, and the default value is usually 1E-12. To properly
    * simulate the low input bias current and low current noise, the
    * Spice simulator options have to be set to the following:
    * .OPTIONS GMIN=0.1f (in LTspice I had to enter this as 1e-16 instead).
    * .OPTIONS ABSTOL=0.001pA (in LTspice I had to enter this as 1e-15 instead).
    * In many simulations, .OPTIONS STEPGMIN may have to be used.



  • I repeat my experiments in LTSpice. I got unreal results: offset voltage in nanovolt range and bias current in attoampere range. I set GMIN and ABSTOL as this is recommend in notes

    Typical value of bias current is 3.3780799e-005fA

    Also, I tested example circuit in LTSpice, but I got the same values

    Please, help me understand it!


  • Hi,

    AD549 spice model version in LTspice did not include bias current and offset voltage inside the model.

Reply Children
No Data