I am trying to construct an amplifier circuit using a fully differential op amp (THS4503) to interface with an ADC (ADS5232). I will be reading a 0-5V sensor, which needs to be converted to a 1Vpp differential signal. I have the circuit constructed according to the datasheets of the respective components along with the help of a TI app note (sloa054e.pdf) (p.17-19), since my sensor requires a 50 ohm termination. I'm simulating the circuit in LTSpice using models created by TI for the amplifiers. When I sweep the input voltage, I am getting some weird nonlinearities at the end of the range, and I'm not sure how to resolve it. I checked the datasheets and I am within the voltage swing of the amp, and I checked current flowing through the components and I am within the current rating of the amp. Plus, it doesn't quite make sense, since the amp is able to provide the same voltages at the beginning of the input range, just not at the end.

Here is the circuit (V1 is the sensor, the regular op-amp is just used as a voltage buffer to bias the sensor): Circuit

And when sweeping the voltage input from 0-5V linearly, this is the output: Sim

Thank you for your help!


4 Answers 4


Your opamp is not rail to rail, the datasheet says:

Common-mode input range 1-4V typical 25°C, 1.6-3.4V worst case for 5V supply.

You must make sure your resistors set the DC operating points to the proper voltages.

Also the output is not rail to rail either. Check "Differential output voltage swing".

"Differential output voltage swing RL = 1 kΩ, Referenced to 2.5 V ±3.3 ±2.8 ±2.6 ±2.6 V Min"

Taking "±2.6 V Min" this means the outputs will swing to 1.3V away from 2.5V, that is from 1.2V to 3.7V.

You require a 1Vpp differential signal, so the non rail-to-rail output would not be a problem, except you set VOCM to 1.5V, which makes me think the next thing in the signal path is a 3V3 ADC, so even if it works in simulation, I'd be very cautious of using this opamp...

  • \$\begingroup\$ This all makes sense - but in the ADC's datasheet they recommend exactly this amp and I designed my circuit to roughly match the application example they provide. \$\endgroup\$ Aug 23, 2017 at 19:45
  • \$\begingroup\$ Yeah, this opamp seems a bit weird, especially the big warning in bold on the front page of the datasheet which says "if it heats up a little bit, it will oscillate!" If I were you, I'd make pretty damn sure to find an opamp with the same foortprint and same specs as second source... you know, Murphy's law and stuff... \$\endgroup\$
    – bobflux
    Aug 23, 2017 at 19:47

Try putting a sensible supply on the TL072. It won't run effectively with a single 5 volt supply. Data sheet recommended supply range is +/- 5 volts to +/- 15 volts. Also note that the diff amp has input and output level restrictions you may be breaking.

Also note that the TL072 cannot be loaded with 110 ohms as you show. You need a much higher impedance load on the output of most opamps.

  • \$\begingroup\$ I will certainly try that! But this problem exists even when removing the TL072 and connecting the two DC sources in series. \$\endgroup\$ Aug 23, 2017 at 18:42
  • \$\begingroup\$ I suspect there are multiple issues and input and output restrictions on the diff amp are still a problem. Also, just because the TL072 problem doesn't show up in a sim doesn't mean you are magically exempt from it being a problem in reality. \$\endgroup\$
    – Andy aka
    Aug 23, 2017 at 19:13
  • \$\begingroup\$ Of course - just trying to deal with one issue at a time. I will figure out the voltage buffering after I resolve the issue with the diff amp. \$\endgroup\$ Aug 23, 2017 at 19:17

Why do you use a TL072 to provide a 2.5V bias voltage.

I suspect that it cannot provide the required output current when V1 is producing a larger voltage.

Remove U2 and directly connect V4 to the positive terminal of V1.

You can also verify by plotting the output voltage of U2 while doing a sweep.

You have not defined the common mode voltage - connect VOCM to 2.5V

  • \$\begingroup\$ I directly connected V4 in series with V1 and the problem persisted. \$\endgroup\$ Aug 23, 2017 at 18:42
  • \$\begingroup\$ Have you plotted the input voltage to R5? \$\endgroup\$ Aug 23, 2017 at 18:47
  • \$\begingroup\$ Is it acceptable that VOCM is open circuit? \$\endgroup\$ Aug 23, 2017 at 18:51
  • \$\begingroup\$ I just plotted input voltage to R5. It varies linearly from 2.5V to -2.5V. Vocm must be set to 1.5V - in reality it will be set to the OCM output of the ADC which is approximately 1.5V. \$\endgroup\$ Aug 23, 2017 at 18:56

I figured it out. Since the signal was oriented in reverse, when the signal was at its maximum, it caused the highest negative voltage, which was lower than the negative supply of the differential amp. Thanks for all your help!


Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge that you have read and understand our privacy policy and code of conduct.

Not the answer you're looking for? Browse other questions tagged or ask your own question.