Post Go back to editing

ADA4625 simulation fails

Category: Software
Software Version: 17.2.2

Good day -

When trying to simulate a voltage regulator based on the ADA4625, I ran into a problem.

Here is the schematic:

5808.upload.asc

 

Expected output voltage is 30V. Raw DC input is 34V with a 100mV / 10ms sawtooth ripple applied on it to be able to see if the circuit operates properly. When I swap out the ADA4625 for theAD825 the simulation runs just as expected: nicely flat DC voltage just under target 30V and all voltages and currents check out. But with the ADA4625 it won't run - I see this:

"Pseudo-Transient Analysis: x ms inter=x fill-ins: x (Press ESC to quit)"


LTspice never gets past that (waveform viewer never appears if I wait long enough for the algorithm to complete and shows garbage data if I escape out of the loop).With the AD825 in the schematic the waveform viewer pops up instantly when I run the simulation and shows data that makes sense.
I found a post asking a similar question here. I am having trouble if the answer there applies to my simulation as well. Datasheet says the input voltage is up to just over the supply voltage. Supply voltage maximum is 36V, mine is (supposed to be) 30V. What am I missing?

Would anyone be able to help me understand what's going on here?
  • Hi Kunlun121:  I tried this and it simulated quickly as soon as I ESCaped through the "Pseusdo-Transient" analysis.  You can also try chaning solvers under "tools" "control panel" "spice".   Different models can have different sensitivities to convergence issues.

  • Hi Glen,

    Thank you for looking into this. Are you sure the simulation is working after you ESC out of pseudo-transient analysis? When I ESC out, I do get a waveform viewer. The simulation, however, is not working as expected Let me show you what I see. 

    My working version of this simulation (with the AD825 opamp) shows this:

    That is the 34V + sawtooth of the input and the output (at the emitter of Q1) that is right around where it should be: 30V (minus a bit).

    In the version that fails (with the ADA4625 opamp), I get this image at the emitter of Q1 after ESC-ing out of the pseudo-transient analysis:

    That's not what this schematic should be doing.

    What does your screen look like?

    I have tried playing around with the settings in the control panel, but none of the options I tried improved the situation.

  • Hi  ,

    cc:  ,  

    Sorry for the *very* long delay on this one. I did find a well-hidden problem with the schematic, namely in setting the parameters for D44H11. The + sign in front of NC should not be there. No doubt this is a vestigial line break:

    .MODEL D44H11 NPN(IS=6.99994e-12 BF=91.0001 NF=1.04634 VAF=40.7259 IKF=10 ISE=7e-11 NE=3 BR=1.97064 NR=1.50008 VAR=22.902 IKR=35.9467 ISC=4.75e-12 +NC=3.59375 RB=4 IRB=0.1 RBM=0.1 RE=0.0001 RC=0.130733 XTB=0.337319 XTI=1.40625 EG=1.13125 CJE=1.03578e-09 VJE=0.651779 MJE=0.35303 TF=3.07008e-09 XTF=1.35721 VTF=0.995654 ITF=1 CJC=3.98764e-10 VJC=0.429208 MJC=0.35114 XCJC=0.803125 FC=0.533449 CJS=0 VJS=0.75 MJS=0.5 TR=4.30593e-07 PTF=0 KF=0 AF=1)

    You can replace that directive with the following, for readability, note that the +NC is correct here, because it is a line break:

    .MODEL D44H11
    +NPN(IS=6.99994e-12 BF=91.0001 NF=1.04634 VAF=40.7259 IKF=10 ISE=7e-11
    +NE=3 BR=1.97064 NR=1.50008 VAR=22.902 IKR=35.9467 ISC=4.75e-12
    +NC=3.59375 RB=4 IRB=0.1 RBM=0.1 RE=0.0001 RC=0.130733
    +XTB=0.337319 XTI=1.40625 EG=1.13125
    +CJE=1.03578e-09 VJE=0.651779 MJE=0.35303
    +TF=3.07008e-09 XTF=1.35721 VTF=0.995654 ITF=1
    +CJC=3.98764e-10 VJC=0.429208 MJC=0.35114 XCJC=0.803125 FC=0.533449
    +CJS=0 VJS=0.75 MJS=0.5 TR=4.30593e-07 PTF=0 KF=0 AF=1)

    I made this change and reran: simulation produced a 29.367958V output with a very small droop and HF ringing at 10ms:

  • Hi  ,

    If you are interested, we have a beta release of LTspice 24.1, which features stricter parsing of the netlist. I ran this schematic in 24.1 and this error is discovered and communicated. 

    mike

  • Thanks MStokowski, especially for taking the time to look into his after so long. I am still interested as I never got this to work. Unfortunately, there is no change in that status for me. The plus sign was well spotted. I must have forgotten it when taking out line breaks. With the directive you provide I'm still stuck in perpetual Pseudo-Transient analysis. Something else must be broken. I simply can't run this simulation with this opamp. On none of my machines. The ADA4625 breaks it, whereas with the AD825 it runs fine. Perhaps I should it rebuild the circuit from scratch some time.

  • Hi  ,

    You're right! It does not work in 24.0.x even with the + fix. If you want, I can set you up on LTspice 24.1 beta, which runs your simulation, and as a bonus, finds syntax bugs such as that +.

    mike

  • Hi Mike,

    could I please get the 24.1 beta release if possible? Thanks a lot!

    Vilem