AD633 Input Offset Problem

Simple AD633 circuit.

1. As AM Modulator per data sheet

2. Signal into Y1 is 1000Hz sine at 2V p-p (via 10uF cap)

3. Signal into Z is connected to Y1

4. Signal into X1 100Hz sine at 8V p-p (via 10UuF cap)

5. Y2 and X2 are grounded

6. Supply voltage is +/- 12V

Problem ...

This circuit simulates perfectly in multiSim.

However on the PCB ... the output is garbage.

I do see something I do not understand. That is ..

  - Although the X1 and Y1(Z) signals are coupled to the pins via a 10uF cap..

there are heavy DC offsets on the pins.. Vy,Z(pin-1/4) is offset -6V, Vx(PIN-7) is offset -2V

The input caps are not leaking .. the voltages on the circuit side of the caps are different.

Is ths a bad AD633 or is something wrong with using simple cap inputs to the AD633?

Thanks .... JCD

UPDATE ... 29 Dec 11

OK. So I bridged the input caps with a short wire and the AD633 produced the beautiful canoinical AM modulation output.  This way the AD633 inputs are direct to op amps (with zero volts dc level).

I don't know yet if it is pcb leakage or a characteristic of the AD633 but the input pins were accumulating charge as mentioned above and wacking the output. Now everythng is fine. In this circuit .. maybe everywhere .. the AD633 input pins cannot be driven via a capacitor.

The mulitSim simulation does, however, work fine with caps for input ????

Any comments/analysis will be appreciated.

/ ... JCD

  • 0
    •  Analog Employees 
    on Dec 31, 2011 5:42 AM

    Hi, JCD,

        I haven't seen your circuit, so this is guess work at best: now the inputs of the AD633 are just like most opamps, that they require some dc BIAS current to function (~ 0.8uA each  -- datasheet, p.5, under Input Amplifiers).  If there is no dc path (to ground, or to some dc supply), then dc levels at the pins will shift until they are railed.  Due to minute difference in the bias currents for the input pins, they don't necessarily rail to the same dc levels, resulting in a dc offset between each differential input pair. 

        If AC coupling is needed, then for each differential input pairs, you can terminate each input to ground with, say, a 1.00k ohm resistor.  Offset voltages can be nulled out with the method shown in Fig. 10 on the datasheet.

        Good luck, and have a Happy New Year!


  • Yes ,,

    I am sure you are correct.

    I see what you are talking about on the data sheet. Unfortunately I just

    ran the simulation and went from there.

    AND ... the * #^%$@*  the Analog Devices MultiSim Component Evaluator ,,,,

    DID simulate PERFECTLY with the capacitor inputs ... THAT REALLY FROSTS ME

    ... I put a lot of faith in that simulator and it totally fell down with

    this AD633 circuit.

    Anyway thanks ... I just wanted to check with you guys.

    Maybe you could tip off the guys who made the mulitSim AD633 model ... it

    should help the next person.

    / ... JCD

    On Fri, Dec 30, 2011 at 1:42 PM, bsam

  • Ahhhh. Touchstone .....

    Anyway ... thanks for the help.

    I don't have any problem with different classes of models. There are good

    reasons for each.

    What I do have a problem with .. and every honest engineer

    or scientist should .. are models which do not either make their

    performance capabilities known and/or expose their internals so one may

    figure it out.

    Last Rant .. It would seem that offset is such a a fundamental issue with

    certain classes of IC's that one might just expect it to be part of the

    mode - unless otherwise stated.

    Anyway .. we have it sorted out now and your help is much appreciated. The

    9833's and 633's are humming along now and look real good for the


    Thanks again ... JCD





    On Thu, Jan 5, 2012 at 12:17 PM, bsam

  • 0
    •  Analog Employees 
    on Jan 6, 2012 4:17 AM

    Hi, JCD,

       I can understand your frustration regarding the difference in simulated vs actual results.  I haven't used Multisim myself, so I'm not familiar with what's in the model.  I have, though, at some point participated in the development of models of other parts, and I can share my experience with you.

        There are always different levels of models that can be developed: from the simplest ac small-signal response, to something that would fully capture the non-linear characteristics, including dc offset and temperature effects.  When developing a model, one invariably has to trade off model complexity vs. development time as well as ease of use.  Most opamp macro models ended up ignoring non-linear effects, and offsets (which arise from mismatches) are not modeled.  So even if input bias currents were modeled, the two inputs in a differential pair could simple move together to some unreal dc levels.  Yet the output remains perfectly balanced, and nothing is saturated.  Back when I was running simulations with the Touchstone Program (a microwave linear circuit simulator), I never had to put in a dc source, but my amplifier always showed power gain :-)

        So, next time when your simulated amplifier output shows no distortion, be sure to check what is and what is not captured in the device models.

    Best regards,