0
\$\begingroup\$

The circuit that I am simulating is a Vishay PTC thermistor model number PTCTL7MR100SBE.

I have a timestep too small error when trying to simulate.

The link for the SPICE model.

I tried running the PTC through a pulse voltage of 500V with a rise time of 0.4us and a fall time of 1ps. The error seems to be happening at the fall time.

Can anybody advise me on how to solve the error?

Simulation Error

Circuit Diagram

Spice Settings

\$\endgroup\$
6
  • \$\begingroup\$ What happens if you set the fall time to a more realistic value? \$\endgroup\$ Commented Dec 23, 2020 at 7:56
  • \$\begingroup\$ Only at 1ms fall time, the simulation will work. The thing is I am trying to simulate an instantaneous drop \$\endgroup\$
    – Sandra
    Commented Dec 23, 2020 at 8:12
  • \$\begingroup\$ What exactly are you trying to simulate? By that, I mean what metric are you trying to determine from this simulation? The current through the PTC? The wattage? Something else? \$\endgroup\$
    – Ste Kulov
    Commented Dec 23, 2020 at 8:59
  • 1
    \$\begingroup\$ The voltage you're simulating is a very narrow and unrealistic peak, with the specified rise and fall times, and with zero on time. Are you sure this is what you want? \$\endgroup\$ Commented Dec 23, 2020 at 10:12
  • \$\begingroup\$ Actually the rise and fall time is so specific because I am doing lightning surge protection and this is the voltage after going through a few surge protection components. \$\endgroup\$
    – Sandra
    Commented Dec 23, 2020 at 10:26

2 Answers 2

1
\$\begingroup\$

As already stated in the comments the problems seems to lie in the fall time of your supply. This can sometimes be overcome by either changing the solver or checking whether your simulation makes sense at all as described in this question.

After tweaking the simulation a bit, I manage to make it run by slightly increasing the fall time from 1ps to 100ps and reducing the maximum stepsize to 0.1ps.

circuit

\$\endgroup\$
2
\$\begingroup\$

Like mentioned in the comments, your source is too ideal and creates a very extreme and impractical \$\frac{dV}{dt}\$. That ideal triangle shape you're simulating will also never show up in real life. I've done DO-160 Lighting Tests, and their waveform specifications always have some kind of RC smoothing on them to be more realistic.

I was able to get your simulation to simulate using a slightly less intense waveform via an RC and also forcing the maximum time step size to 1p (see the .tran statement). But keep in mind this takes a long time to simulate.

enter image description here

Since you didn't explain what you're trying to measure, I have to assume the following might be important too. If you need to avoid current limiting via loading from that series resistor, then you can pass the smoothed waveform through a Gain=1 voltage buffer like so:

enter image description here

\$\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.