• State TI Thinks Resolved
  • Locked Locked
  • Replies 3 replies
  • Answers 1 answer
  • Subscribers 47 subscribers
  • Views 1671 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.

OPA564: Negative Capacitance Circuit

Tarek Mostafa
Prodigy 60 points
Part Number: OPA564
Other Parts Discussed in Thread: OPA549, TINA-TI, OPA828

Hello,

I Used a negative capacitance circuit to act as an inductor in LCR resonant circuit. I simulated the circuit with Ideal OpAmp, and the results were excellent and consistent with expectation, however, When I Simulated by using OPA564 or OPA549, I didn't get any output. Please help me!

In the enclosed link, you will find: The schematic, a screenshot of the I deal OpAmp results, and the simulation files of OPA564 and OPA 549

www.dropbox.com/.../AABAdm2NLsNd7ACsbsSUH8PWa

Thanks in advance and looking forward to your feedback

  • 0
    TI__Guru* 93105 points

    Hello Tarek,

    It looks to me like there is a problem with your U3 op amp input pin connections; they appear to be are reversed. As connected the feedback is positive around the U3 stage and the inverting input is being driven directly at the summing node. When I simulate the circuit using TINA-TI Spice where U1 thru U3 are OPA564, the outputs lock up to the supply rails. When I reverse the U3 input pin connections the circuit goes into linear operation and a band-pass filter response is observed at the output of U3.

    On at least one occasion I found that running Spice simulations on an active filter circuit having crossed op amp inputs resulted in nearly correct filter response. That may be what is occurring with your ideal circuit.

    I use TINA-TI Spice so I had to build your negative capacitance circuit from the ground up. I used OPA564 op amps for U1 thru U3. The filter center frequency comes out a little below 1 MHz, but I think that may be because the OPA564 gain-bandwidth is only 17 MHz and there isn't a lot of loop gain at 1 MHz to work with. Low loop gain can affect an active filter's response characteristics. I am not sure why you are using a power op amp such as the OPA564 unless you need the high power output. If you don't, then there are plenty of other TI op amps that have higher gain bandwidth. Note that the OPA549 power op amp would not have enough gain-bandwidth to be considered for this application.

    I have attached my TINA-TI Spice simulation circuit file should you wish to evaluate the OPA564 negative capacitance circuit using our simulator.

    Regards, Thomas

    Precision Amplifiers Applications Engineering

    OPA564_NegCapFil_02.TSC

  • 0 in reply to Thomas Kuehl
    Prodigy 60 points

    Hi Thomas,

    I want to thank you so much for the great help and support, I really appreciate it, and I am so sorry that I made you built the circuit from scratch on Tina. 

    Let me first tell you what I want to do precisely. I will use this circuit as a compensation circuit in capacitive wireless power transfer. At this stage, I want to deliver 5 watts or more to the load (that's why I am trying to use Power OPAmps OPA564 and OPA54). There is no specific frequency for the system, and any frequency between 100 kHz to 13.56 MHz would be acceptable. The same thing for Rload (R13, which is equal to 200 now), We can change this value to another which help the system to deliver.

    I applied your changes, which was so useful plus a couple of more things,

    - I changed (R7) to (2*R) value.

    - I also changed the value of C1 to 100p to follow the resonance equation

    The results from the Ideal OpAmp was better and I the small difference in voltage and power across the load disappeared

    The Transient in OrCad allow me only for 1 V amplitude but still, I could get exactly the same as I am using an Inductor as you can see here

    So I moved to Tina and I made Transient simulation, The results are strange As you can see here 

    I got the same results of course from OrCad. I swept the parameters (On Orcad sorry I don't know how to make parameter sweep on Tina):

    -Frequency (@R= 100)

    -R (accordingly C1) (@Freq=500 kHz),

    but unfortunately I couldn't get 5 W at the output or even any useful output just mW or uW. 

    Would you please if you don't mind help me?

    In the same link, you will find the files after editing including Tina file you kindly made

    www.dropbox.com/.../AABAdm2NLsNd7ACsbsSUH8PWa

    A lot of thanks in advance and looking forward to your feedback



  • 0 in reply to Tarek Mostafa
    TI__Guru* 93105 points

    Hello Terak,

    I suspect the reason things don't look good at 500 kHz is the limited OPA564 gain-bandwidth and slew rate relative to the application frequency. Normally, you want to make sure that the op amp has plenty of gain bandwidth and slew rate capability such that they are not a factor affecting performance at the frequency and amplitudes of interest.

    I do think a better approach to this application is to use high performance op amps having high gain-bandwidth and slew rate to generate the desired bandpass response. Once the response is achieved by those op amps follow them a power op amp running in minimum closed-loop gain. Preferably, in unity gain (+1 V/V) to maximize the loop gain.

    The Precision Amplifiers that I support max out with a 50 MHz gain bandwidth - that should be sufficient for the lower to mid end of the 100 kHz to 13.56 MHz frequency range. You also want to use a high slew rate op amp because you are working with 10 Vpk amplitude levels. I would suggest the OPA828 which is specified with a 50 MHZ gain bandwidth and 150 V/us slew rate. If it doesn't have high enough bandwidth or slew rate, then TI's High Speed Amplifiers group picks up from there with very high gain bandwidth and slew rate op amps.

    Once you have the bandpass filter working to your satisfaction, then to apply the OPA564 as a unity gain power amp. If the frequency selected is towards the low end or possibly in the mid range the OPA564 may be able to keep up with the input signal coming from the filter. The resulting output signal and power level may achieve what you are after. The datasheet does indicate that the full-power bandwidth is10 VPP at 1.3 MHz, so it will be less at 20 VPP. Use datasheet Fig. 15 as a guide - OUTPUT VOLTAGE SWING vs FREQUENCY. If it doesn't achieve the level of performance needed, then a high frequency power op amp may be required. Unfortunately, TI's highest gain bandwidth power op amp is the OPA564.

    Regards, Thomas

    Precision Amplifiers Applications Engineering