Loop Analysis Problems in Ltspice

Simulation description:

Hi LinXue ,

Thank you for reaching out. I will be transferring this inquiry to other group - LTSpice. Hopefully, your questions could be answered more accurately. 

Best regards,

Noel

I work in ADI's modeling group, tried to duplicate your reported error,  and now have some comments:

1)  I could not read all the component values so I could not exactly duplicate your circuit.  If you would like me to try your actual circuit please send the LTSPICE schematic to Brooks.Leman@Analog.com.

2)  In each case I tried, I was able to plot the Bode data.  If you would like to try my version then please send me an email message and I will then send you my version of your LTSPICE schematic.

3)  You may have to wait longer for the circuit to settle (at least 2 mS)

4) Output voltage is so high (40V) that we can increase the AC signal magnitude up to 1V

5)  We may need to see bode plot data at much lower frequency to reveal gain crossover.  This will take longer to plot.

Hope this helps...

Regards,

Brooks

some additonal comments:

- In the FAQ section of the help file in LTSpice is a section on the bode plot. Do a search for 'bode' and you will find it easily.

- the max output voltage of the LTC1871 is 35V so your output voltage is too high, maybe the LT3757 is a better choice in this case.

- you can change your .tran statement to: ".tran 0 {t0+10/freq} {t0} startup"
(10 i.s.o. 25) this will greatly reduce the simuation time and still be accurate enough.The "startup" option will get rid of some of the errors in your log file.

- If your converter is not stable, the bode plot will not tell you anything. Therefore you have to start with enough (or too much) compensation and see how much Phase Marging you have and then reduce your compensation to optimize.

To see if your converter is stable you best do a step response in a normal transient analysis (step your load) and if the output voltage is ringing or oscillating after the load step it is not stable. I believe that it is already oscillating with a fixed load (if I copied your circuit correclty) So you need to change you compensation first before you can make a good bode plot. (try 2.2n+16.5K with 100pF in parallel on the ITH pin)

best regards

Paul

I'm sorry, I didn't notice your reply recently,I still want to know how to solve this problem,so I sent this model for you by email.

2)This is my email:mzixuelin@163.com,I hope you can send your LTSPICE model to this email,because I still a newbie,I want to learn more about loop  stability.

3)I can understand at least 2 mS for the circuit to settle,but but I can not understand AC signal magnitude up to 1V,we have to inject sufficient AC voltage,But how much is suitable?What is the theoretical basis?

Best Regards

Thoughts as your additional comment：

1） LTC1871 really is not suitable for 40V,I will use the LT3757 for simulation next.

2） Some questions about loop compensation,I do not understand that 2.2n+16.5K with 100pF in parallel on the ITH pin?I mean why is such parameter chosen？I really hope you can explain it when you have time.

best regards

LinXue

Please see my email message about the LT1871 bode plot problems and resolution.

Regarding the iTH pin components; this network allows you to compensate the internal transconductance amplifier for a good closed loop Bode plot.  To really see the effects please download LTPowerCAD and practice with the LTC3786 Boost Controller.  Unfortunately LTPowerCAD does not support the LT1871 or LT3757 but, with a little practice with the LTC3786 in LTPowerCAD then you should be able to go back to LTSPICE and make the adjustments for your LT3757.

Please see my email message about the LT1871 bode plot problems and resolution.

Regarding the iTH pin components; this network allows you to compensate the internal transconductance amplifier for a good closed loop Bode plot.  To really see the effects please download LTPowerCAD and practice with the LTC3786 Boost Controller.  Unfortunately LTPowerCAD does not support the LT1871 or LT3757 but, with a little practice with the LTC3786 in LTPowerCAD then you should be able to go back to LTSPICE and make the adjustments for your LT3757.

Thank you very much for your reply, I didn't expect you to reply so detailed in your email! I will download the LTC3786 model to do a pratice in LTPowerCAD as you said.