• State Resolved
  • Locked Locked
  • Replies 3 replies
  • Subscribers 37 subscribers
  • Views 692 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.

TPS53355 on TI-TINA

Graham Schwinn
Prodigy 60 points
Other Parts Discussed in Thread: TPS53355, TINA-TI

I am trying to run a transient simulation for the TPS53355 in TI-TINA but can't seem to get the part to turn on in the simulator.

VDD and VIN are stable, EN is @4V.

It wouldn't surprise me if I am missing something obvious, I haven't used SPICE much since school.

3V3_Global.TSC

  • 0
    TI__Mastermind 41310 points

    Graham,

    There are several things that needed to be changed. First, it is normally easier to start with the reference design .TSC file and modify it. The simulation parameters are set up in it to run properly. Second, most IC models do like to have some kind of resistive load during startup. It makes the matrix easier to solve. I added an RLOAD of 3 ohms to your simulation. I was not sure what R9 was used for, so I replaced it with a capacitor. With R9, the simulation regulated to 1.44V, not the 3.3V your FB resistors were trying to achieve.

    Third, a 200ms simulation is EXTREMELY long. The reference design runs for 1ms. I have changed the simulation to run for 5m with a transient load of 800us pulse with 100us rise/fall times to occur at 2ms. I have also changed the FAST value to 1 to make the simulation run quicker. You may change this back to 0 at your leisure, however, the simulation will take a very long time to simulate. I added a Vout probe and an inductor current probe as well.

    Since the load pulse is only an amp, there is very little deflection seen.

    Please see the attached .TSC file.

    3V3_Global_up.TSC

    Britt

  • 0 in reply to Britt Brooks - Online Design Tools
    Prodigy 60 points
    Thanks Britt,

    That is exactly what I was looking for. I didn't see a reference design for this part. I put in a request with my local FAE to get this part available in TINA, so I may have been the first person to actually download this simulation model. I pulled the TINA model from the main product page and didn't even bother to look in the "tools and software" tab. I will do what you suggested in the future.

    R9 was a mistake on my part. I was fiddling whatever knobs i could to get the thing up and running and I probably just messed that one up.

    The simulation time and values were also products of me trying fiddling knobs to get the part to turn on.

    Was the load resistor all that you changed to get the part to turn on? What is the minimum load required to get the part to turn on?

    Is there any way to ignore startup in the transient simulation to reduce actual simulation time?
  • 0 in reply to Graham Schwinn
    TI__Mastermind 41310 points

    Graham,

    The first thing I needed to fix was the simulation parameters. They can be seen at ANalysis-->Set Analysis Parameters...

    Anything highlighted in red was changed from the TINA-TI defaults. These values are the same as the reference design. Once these were applied, the device began working. I also changed the FAST variable to 1 (faster simulation than with 0). Next, the resistor was changed to a capacitor (based on the reference design and the fact that the sim was only getting to 1.44V). Then, RLOAD was added (and it is not really that necessary, but it does make the device a little happier from a simulation standpoint. No load is not very realistic with a 30A part...).

    If you really don't care that much about the startup, you can put an IC (Initial condition) on the output cap (C4) of your target voltage and the simulation will run very quick (less time during switching). I think mine finished in less than 500us. Try it out and see what you think. To put the IC on the cap, right double click on the capacitor. Initial DC voltage will be marked not used. Use the pull down and change it to 0, then change the value to 3.3.

    Let us know if you have any additional questions.

    Britt