2
\$\begingroup\$

I started working on a single series lithium to 15V / 2A Boost converter based on this design: https://www.ti.com/tool/PMP8921. I got this PSpice simulation model from TI themselves here: https://www.ti.com/lit/zip/slvm706. After changing the file so that it works like described here: Issue using pspice .lib in ltspice - Unknown Parameter, I then got a simulation working: Schematic of working spice simulation

Then, after saving everything and doing something else on my computer I returned to the project and now the results make no sense anymore: Output node of not wokring SMPS (output of the converter) enter image description here (switching node of the converter) enter image description here (EN node of the TPS43061 (has to stay over 1.14V ?!)

Why doesn't the output smoothly increase to 16V? Where do these weird transients come from? I don't remember changing any simulation parameters, so they must be the standard ones. Are there some parameters I could change to omit these strange errors? The design has been proven to work before.

Files: https://1drv.ms/u/s!Ai1WNGQ9wFb7g5hYmVUygiMGqTib5w?e=Ww1wg7

Schematic of working circuit: Schematic of wokring SMPS

Cheers

\$\endgroup\$

2 Answers 2

0
\$\begingroup\$

Unfortunately, models made by TI are known to be heavily behavioural in nature, with plenty of discontinuities which cause convergence issues. This is no exception. The model was made for their WEBENCH, PSpice, or maybe TINA, so if it should run somewhere, it's there. It's not about a lack of compatibility, but about a difference in "thinking".

You could try to soften up the overall stiffness by adding Rser to the output capacitor (BTW, 4 are useless, just make one), maybe adding Rser=10m Cpar=100u to the input source, there's not much to do if you want to use these models in particular. I couldn't make it run, but then I just got your models as they are, not from TI, so I don't know what changes you made. Though I'm sure it would have been the same hiccups.

That "working circuit" is from the application note (or close), which doesn't mean that it has to run everywhere. It may even fail in PSpice (I don't know, I don't have it). It's just a test schematic to be able to run it on the breadboard, not simulator.

But, you should know that models hardly ever match the devices in real life. I don't expect this one to be any different. This is particularly since right in the beginning of the subcircuit there is this note:

This model is subject to change without notice. Texas Instruments Incorporated is not responsible for updating this model.

I don't know about you, but when someone says "here's a model, don't bother me anymore, unless I bother myself" that doesn't exactly inspire confidence in the model.

However, to solve your problem, there may be two ways, provided, again, that you're not fixed in this choice, and you need to work with LTspice:

  • Build your own model based on the datasheet. It doesn't look very different than many others, and if you use the A devices, you should come up with a model that seriously outperforms this one. I do not work for ADI, I am not making a selling point. I have worked with LTspice for many years and I can say quite sure of myself that it excells in switching aplications; this would be no problem.
  • If building a model is not your choice (for whatever reasons), you could use an equivalent one from LTspice's database, there are synchronous boost converters in there.

If your intent is to actually see how they perform before buying them, use the tools they used, but a simulator is not a breadboard. Whatever results you'll see, take them with an appropriately sized grain of salt.

\$\endgroup\$
2
  • \$\begingroup\$ I have found that the Half Bridge Mosfet CSD86330Q3D causes some problems. If I use some discrete MOSFETs from the LTSpice library, the mode work better. \$\endgroup\$ Commented Feb 27, 2021 at 9:17
  • \$\begingroup\$ Well, I'm glad it worked out but, to be frank, I didn't expect that to be the cause. The library is made of primitives, no behavioural expression in sight. At any rate, I'd suggest to also run one of LTspice's own synchronous boost converter test jigs, just to see the differences in speed and similarities in response. You might be surprised. \$\endgroup\$ Commented Feb 27, 2021 at 10:49
0
\$\begingroup\$

I usually try to make the simulation match the real world as much as possible, sometimes this helps and sometimes it's the model.

Do these things:

  1. Make sure all energy storage components have parasitics, inductors and capacitors should have series resistance. Capacitors should have some lead inductance like 1nH. L1 should have at least a few mΩ's , the output caps should have some ESR. C5 should also have some ESR and ESL

  2. Try putting a small amount of ESL and ESR on the gate drives LDRV and HDRV, similar to what a copper trace would be, like 1nH and a few mΩ's. You may also want to modify the fet to have some ESR in between FET's

  3. turn up cpar (I think that is the parameter name anyway), the global parameter for parallel capacitance to everything.

  4. Put a small amount of capacitance to put an LPF on the feedback pin, make sure the LPF is higher than the switching frequency.

  5. C2 should also have a really small amount of ESR and ESL

  6. Turn the soft start off or shorten it.

\$\endgroup\$

Your Answer

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

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