1
\$\begingroup\$

I want to turn on and turn off two mosfets from the asymmetric H bridge which is connected to SR motor at the same time.

I'm using IR2183 gate driver. The circuit connections from LTspice are show in the image. Why is my simulation taking very long? Is some thing wrong in my circuit?

enter image description here

\$\endgroup\$
5
  • 1
    \$\begingroup\$ what do you mean by "very long"? also, don't use ideal elements (like diodes) they make tons of problems. \$\endgroup\$
    – PlasmaHH
    Commented Feb 20, 2018 at 15:34
  • 1
    \$\begingroup\$ The simulation is running very slow for this circuit. It took more than 5 mins to perform a time stop of 0.05 sec. From the simulation window I still see that the circuit is still running which is currently at 13us. \$\endgroup\$
    – lomesh pudipeddi
    Commented Feb 20, 2018 at 15:41
  • 2
    \$\begingroup\$ Of curiosity why do you use bootstrap on the low side switch? what is the point? \$\endgroup\$
    – user103776
    Commented Feb 20, 2018 at 16:34
  • \$\begingroup\$ I was asked the same question by somebody else which made me think again. Now I'm working on the connections for the low side switching. I didn't mean to connect the bootstrap on low side switching. I only want to turn on both the mosfets at the same time. \$\endgroup\$
    – lomesh pudipeddi
    Commented Feb 20, 2018 at 16:52
  • \$\begingroup\$ @PlasmaHH That can be easily solved with epsilon (and/or revepsilon). The default "knee" is sharp and relies only on LTspice's internal solver to add 3 very small spaced points to try to make the derivative continuous, or at least no too "jumpy". \$\endgroup\$
    – a concerned citizen
    Commented Feb 21, 2018 at 7:32

1 Answer 1

Reset to default
4
\$\begingroup\$

I've had great success increasing LTSpice simulation speed using the convergence tips from ltwiki.org. Also, try adding a small series resistance, say 0.1 to 0.5 ohms, to the voltage sources.

If the simulation is only slow at the start, you can also try ramping the power supplies up from 0 to the final value using a PWL source instead of a hard turn on at t=0. The ideal ramp time is circuit dependent, but 100uSec to 1ms is a reasonable range to try.

\$\endgroup\$
11
  • \$\begingroup\$ I'm trying to understand how that could help to my circuit. I followed few suggestion from those tips but they didn't help. I guess in my case, I might have some problem with the values/components I chose. \$\endgroup\$
    – lomesh pudipeddi
    Commented Feb 20, 2018 at 15:56
  • 1
    \$\begingroup\$ I'm not sure if that is the best diode, but that probably isn't the problem. Do you have non-zero serial resistance on your voltage sources? \$\endgroup\$
    – crj11
    Commented Feb 20, 2018 at 16:01
  • 1
    \$\begingroup\$ It really depends on how hard the circuit is for the solver. Anything with large transients is harder to solve. 0.5 ohms is reasonable. I generally start with 0.1 ohms to see if it has an effect. \$\endgroup\$
    – crj11
    Commented Feb 20, 2018 at 16:13
  • 1
    \$\begingroup\$ 1n4148 is low-current diode with large series bulk resistance. I can use it, but edit that param to be 1 ohm, to allow large forward currents. \$\endgroup\$
    – analogsystemsrf
    Commented Feb 21, 2018 at 3:37
  • 1
    \$\begingroup\$ @crj11 The voltage source, if it doesn't have parasitics specified (Rpar, Cpar), it behaves like a voltage source, with zero internal resistance. LTspice's matrix solver uses MNA, so current sources are preferred (also mentioned in the manual). Adding Rser or Cpar makes LTspice convert internally the voltage source to a current source with a shunt resistor Rser (+Cpar, if added). In this case, I suspect even a Rser=1m (and/or Cpar=1m, or the likes) would have helped. \$\endgroup\$
    – a concerned citizen
    Commented Feb 21, 2018 at 7:29

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.