• State Resolved
  • Locked Locked
  • Replies 22 replies
  • Answers 2 answers
  • Subscribers 42 subscribers
  • Views 2976 views
  • Users 0 members are here
Support feedback
Options
Options
Similar topics

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.

Design of COMP components for TPS5432 in TINA - TI

Babu Ramamurthy
Prodigy 140 points
Other Parts Discussed in Thread: TINA-TI, TPS5432

As per datasheet Power stage Gain (Gpwrstg) needs to be estimated from TINA to calculate Rcomp. Can you let me the procedure to get this in TINA? From there I can calculate the other components of COMP. Currently I am using WebBench for my simulation..

  • 0
    TI__Guru**** 191445 points

    the TINA and pspice average models are located here:

    I don't really use TINA much, but in pspice the power stage gain and phase are plotted by subtracting dB(V(Vout)) - dB(V(COMP)) and P(V(Vout)) - P(V(COMP)).  The procedure in TINA is probably similar.  I'll move this post to the modelling forum.  Someone there should be more familiar with it. 

    Most users of the models are already are very familiar with working within those tool environments.  If you are not comfortable with it, then maybe you should just use the webench modeling tool.

  • 0
    TI__Mastermind 39210 points
    Babu,

    If you are already using WEBENCH then that is the preferred method since it gives you the component values directly. If you only use TINA-TI, you need to calculate the component values yourself. Once you have designed the circuit using WEBENCH, you can simulate it within WEBENCH itself.

    Thanks,
  • 0 in reply to Nikhil Gupta (Product Folder Models)
    Prodigy 140 points

    Thank you Nikhil for the response. My design parameters are: I/p V=3.3V, O/p=1.8V, 1A Ta=65C. When I do WebBench simulation, I get Lout & Cout as 4.7uH and 22uFd. But due to my ripple current requirement (or ripple voltage) I wanted to use 10uH inductor. Then due to my load transient I have to increase Cout to 330uFd. Given this scenario, when I edit the WebBench schematic for 10uH and 330uFd, I see the following:
    1> With Electrical simulation (Bode plot) I am not seeing any value change for Rcomp, Ccomp and Ccomp2, for design using 4.7uH/22uFd and for design using 10uH/330uFd. Since the Bode plot simulation doesn't show any value change for COMP components, Shall I use same values of COMP components for both the designs, provided the Phase margin and Cross over freq are acceptable as per theory? Also, from your response I understood that tool will calculate the COMP values, but it is not happening when I changed the L & C.

    2> After changing the L & C values, WebBench tool doesn't provide Gain margin, Phase margin and Cross over frequency in the report once I edit the L & C values. But without editing the L & C values, tool provides those values in report. In such a case, when I try to interpret the margins from Graph, I am not able to relate the values I get from graph and the values provided by report (without editing L & C). Here I apply simple theory to calculate Gain and Phase margins. ie., Phase margin = Phase angle at 0dB - 180.
    Report says 55 degrees but interpretation from graph (in same report) 45-180 = -155. Here I have a doubt, the Phase scale (in graph) is between -30, -20, -10, 0, 10, 20.. like that it continues to 160 degrees. In this scale, the phase curve shows somewhere around +45 degree (with 0dB gain). Assuming 0 as 180 degree (in phase angle scale) still I get around +45 degree, not +55 as reported.

    Please clarify on what I am missing, for both the above cases?

    Further to that, when I refer the TPS5432 datasheet to calculate RCOMP values, I need PWRSTG gain. ie., to start with calculation of Rcomp I want this Gain. All other parameters like Transconductance of EA, Vout and Vref are known. Once Rcomp is calculated then the other COMP related components are easy to derive. Now please let me know, how to obtain this PWRSTG gain from WebBench?

  • 0 in reply to Babu Ramamurthy
    TI__Guru**** 191445 points
    to have this work properly in webench, the "Re-comp" feature must be activated. TPS5432 webench model does not support that feature. Do you have access to pspice? If so I can show you haw to plot the power stage gain. If I get some spare time I might try to figure out how to do it in TINA. I'm sure it must be possible.
  • 0 in reply to JohnTucker
    Prodigy 140 points
    Hi John Tucker, Unfortunately I don't have pspice. Can you please help me to get the Power stage gain using TINA. With that value I shall estimate the RCOMP component values and continue with WebBench using new RCOMP values to plot the Gain and Phase graphs..
  • 0 in reply to Babu Ramamurthy
    TI__Mastermind 39210 points
    Babu,

    I apologize for the inconvenience with using WEBENCH. There seems to be a bug with the Operating Value calculation when you change components, hence some of them are missing after this step. I have asked the owner to look into this.

    I have also asked them to evaluate if we can enable the "Re-compensation" feature for this device.

    Thanks,
  • 0 in reply to Nikhil Gupta (Product Folder Models)
    TI__Guru**** 191445 points

    In TINA TI it is actually straightforward to get the power stage gain and phase.

    1.  Place a voltage pin from the METERS tab on the COMP pin in the schematic.

    2. Run Analysis - AC Analysis - AC Transfer Characteristic.  This will give you the basic closed loop and compensated error amplifier plots.

    3. In the plot window open the post processor (wavy lines with + sign).  Select VOUT and press the big down arrow to put it on the Line Edit. type "/" and then select whatever you called the COMP voltage pin meter.  Enter a function name such as PWRSTG and press create.  Now you can see the closed loop, compensated error amp and power stage gain and phase.

    Just as a note I am currently placing my Cff zeros and poles above the closed loop crossover rather than symmetrically about it.  so the equation for Rcomp will change.  Flip Vout and VREF in the numerator and denominator and remove the SQRT from each. 

  • 0 in reply to Nikhil Gupta (Product Folder Models)
    Prodigy 140 points
    Nikhil,
    Request you to clarify on graphical interpretation of gain and phase margins from Graph. I raised 3 queries in my previous post..
    Query:1-- Is about R-compensation estimation from WebBench. Here if you get the feature enabled please let me know, for this TPS5432.
    Query:2-- Graphical interpretation. This is a common thing. As mentioned in my query the value I am getting in the design report and value I am interpreting in Gain and Phase (Bode plot SIM report) is not matching. So, would like you to help me what I am missing?

    Thanks
    Babu
  • 0 in reply to JohnTucker
    Prodigy 140 points

    Hi John,

    I basically build the buck circuit in WebBench and do SIM-EXPORT to TINA. I started with step-1 as mentioned in your suggestion and when I proceeded to #2, tool gave following error..
    YOU MUST ADD AN INPUT TO THE SCHEMATICS....

    Then I introduced a Voltage Generator (VG1) in series, ie., before Rfbt. Rfbt and Rfbb are the Feedback resistors. Rfbt is top and Rfbb is bottom. Configured this VG for 100mV, sine wave. This generator is introduced in the feedback path, as how WebBench tool connects a Vac_1 source while performing Bode-plot simulation.Then proceeded with AC analysis, AC Transfer characteristics..
    Next, I followed with your #3 step, to estimate PWRSTG. Gave the freq sweep scale as 10Hz to 1MHz. Let me assume my Cross over freq is 50KHz. So, here when I measure the Gain in graph, it shows -51.71dB. I hope it is supposed to be greater than 3dB. While measuring Phase at 50KHz, I yield -158 degree. Please let me know what I am missing in both the cases?

    Thanks

    Babu

  • 0 in reply to Babu Ramamurthy
    TI__Guru**** 191445 points

    Rather than export from webench, I would suggest you down load the average TINA circuit from the product folder. It will already be set up for ac analysis.  You can modify the components to match your wb result.  If you post your  circuit here  I can take a look at it.

  • 0 in reply to JohnTucker
    Prodigy 140 points

    Good morning John..

    I have not done any change to the circuit in WebBench. All the values were retained as it is. I was told that their is no spice model available for TPS5432 to build a circuit in TINA-TI. So the only option is to do SIM-EXPORT from WebBench to TINA-TI...

    With that basic circuit, after adding voltage pin I got the error as "YOU MUST ADD AN INPUT TO THE SCHEMATICS". So I injected small signal (100mV, sine wave) as mentioned in above conversation..

    I referred AN-1889 How to Measure the Loop Transfer Function of Power Supplies, Figure-1 to connect this small signal generator..

    Below is my circuit, for your comments.. Please let me know if it is not successfully attached..webench_design_4165567_41 - autosave 15-11-16 10_12.TSC

  • 0 in reply to Babu Ramamurthy
    TI__Guru**** 191445 points
    Not true...there are models available on line here:

    www.ti.com/.../toolssoftware

    I'll take a look at what you have later today.
  • 0 in reply to JohnTucker
    Prodigy 140 points
    Hi John, I tried with Average Pspice model from the product folder. It was giving "Invalid device:$CDNENCSTART"
    Now, I will give a try with TPS5432 TINA-TI Average Spice Model
  • 0 in reply to Babu Ramamurthy
    TI__Guru**** 191445 points

    I'm not sure what WB exported.  I modified the TINA-TI average model with your component values.  I get Fco = 76.7 kHz and PM = 42 deg.  You can probably do better by modifying the compensation.

    slvm950_wb_e2e.TSC

  • 0 in reply to JohnTucker
    Prodigy 140 points

    Thank you John for your timely support..

    I further edited your circuit for 1A load, 10uH, 47uFd and 3.3V input. Inductor and capacitor values were modified for ripple current and load transient requirements. Attached is the modified circuit. Now the Fco = 25.47KHz, PM=33.6dB & Pwrstg = -15.1dB.

    When I attempted to modify the compensation components by using the Pwrstg gain, I am not able to see improvisation. Using the formula in TP5432 datasheet I have estimated R3, C4,C7 & C5. The values I am getting are; R3=10.4K, C4=3nF, C7=477pF, C5=0.2nF.

    Used 245u for transconductance, as per datasheet..

    Can you provide your comments on what I am missing?

    Attached the modified circuit..

    slvm950_wb_e2e_Edited.TSC

  • 0 in reply to Babu Ramamurthy
    TI__Guru**** 191445 points
    I should be able to look at this further tomorrow during lunch.
  • 0 in reply to JohnTucker
    Prodigy 140 points
    Hi John, Continuation to my previous post I am done with all the simulations and calculations. Once the COMP circuit design is done, I will be freezing my design with circuit I posted in my previous communication..
    Basically I am following the calculations method mentioned in datasheet. Below are the steps I followed..
    1> With new circuit ie inductor, capacitor, I/p voltage and load current modified; I tried plotting the Power stage Gain and Phase characteristics.
    2> Measured the power stage gain at intended cross over frequency (50 KHz) as -15.1dB. With this I tried calculating R3, then C4 and then C7.
    3> Then calculated Fp to get C5

    When I modify my COMP circuit with above new values, I am not seeing any improvement in Fco and PM. The present circuit has Fco of 25.47 KHz and PM of 33.6 degrees.

    My intention is to bring Fco close to 50 KHz and PM between 50 to 70 degrees..

    Please let me know, what I am missing to close this design..

    Thanks
    Babu
  • 0 in reply to Babu Ramamurthy
    TI__Mastermind 39210 points
    Babu,

    The Phase Margin that you see in the Operating Values table is using analytical equations, which the Bode plot in the Simulation page is using spice models. Since they are not exactly identical, there may be some discrepancy. I would trust the spice results more as these do not make many approximations.

    Thanks,
  • 0 in reply to Babu Ramamurthy
    TI__Guru**** 191445 points

    I have been tied up in meetings all day.  I did not get a chance to work on your file.  I was hoping you could handle it once I set the model up for you.  I'll see how my schedule  looks for tomorrow, but it will be meeting intensive also.  Normally I do not actually do design work for customers except extremely large accounts,

  • 0 in reply to JohnTucker
    TI__Guru**** 191445 points
    I did take a quick look. Looks like there is too much phase loss to increase the crossover. In fact you may need to lowerer it with that output capacitance. If you absolutely need higher BW, you may wantto consider a SP cap witha little ESR, maybe 100uF with 9to 12 mohm ESR.
  • 0 in reply to Babu Ramamurthy
    TI__Intellectual 980 points

    Babu,

    We have fixed the GUI so the OpVals (Gain margin, Phase margin, etc) will still appear after editing component values.  We are working to add the re-compensation feature to this device so the COMP components will be recalculated for any design changes.

    Thanks & regards,

    LaRita Gwie

  • 0 in reply to LaRita Gwie
    TI__Intellectual 980 points

    Babu,

    We have added the re-compensation feature to this device so the COMP components will be recalculated for any design changes.  This will allow advanced users the opportunity to see the effects of component changes to the overall design stability.

    Thanks & regards,

    LaRita Gwie