Problem with Multisim Transient Analysis TSTOP

[EDL1]

Reference the attached PDF.  Page 1 is the circuit.  Page 2 is the transient simulation using nothing but default settings (TSTOP=1ms).  Not convinced that the result is correct but that is not the issue.  At least the result is within the range expected and the circuit is oscillating.  Page 3 is the same transient simulation with TSTOP = 100u.  Page 3 is with TSTOP=10u.  

This is a circuit I simulated with good results in PSpice yesterday.  I'm a long time (20yr) pspice user who is converting over to Multisim.  I have been playing with this circuit for many hours, changing options, playing with initial conditions, applying a current pulse to the inductor to start the simulation.  I get a wide variety of outputs, some in the kV range.  After much effort it seems to be related to the TSTOP and TMAX settings.  If I alter either of these settings from the defaults I get results outside the power supply rails.  I have also tried changing TSTEP, changing initial conditions.  Everything I do keeps the results the same or makes it worse.  

Suggestions?     

[johnsold]

I do not use Multisim, so I cannot comment on specific issues regarding that.

The resonant frequency of the tank circuit is ~4 MHz. The settling time for the OPA637 with a 200 pF load is 1.5 us and more than 3 us at 250 pF. The graph in the data sheet does not go any higher than that. The reactance of C2 at the resonant frequency is ~36 ohms. That implies ~275 mA at 10 V, which is much greater than the 55-75 mA short circuit current capability.  The DC gain is 1. The OPA637 is not unity gain stable.

I doubt this circuit would work in hardware.  The simulators may not model these out-of-normal-conditions situations accurately. Also your time step should be considerably smaller than the period of the oscillation (~225 ns).

Lynn

[EDL1]

DC gain is not relevent to the stability of an opamp circuit.  What is necessary is that the noise gain (1/B or 1/beta) at high frequency (AvB=1) be greater than 5 for the OPA637.  For this circuit it is 6.6 which is sufficient to make the circuit stable.

You are correct about the settling time, however the slew rate is sufficient for the circuit to oscillate at 4MHz.  Settling to 0.1% is not needed.  And it actually does work fine on the bench.  

You are right about the timestep.  That is why I tried changing TMAX to 1ns.  However changes to TMAX or TSTOP cause the high voltage results.  I do not think the issue is the model or the topology.  There is something in the assumed bias point or the initial conditions that is causing the simulation to give results that are far out of bounds. 

[Tien_P]

Hi EDL,

If you are getting a large result a KV output you maybe using a three pin opamp model, use a five pin model instead. 

http://digital.ni.com/public.nsf/allkb/50638645C2D0D363862571B900646F6E

I built the oscillation circuit and I added a pulse to kick start it, please have a look at it.

[EDL1]

Tien, Thanks. I ran your schematic and get reasonable results. Now I need to go and see if I can adjust mine to perform similarly...probably this weekend. Thanks for your help. I'll let you know if I have any other problems before closing this thread. Tim