One netlist had different simulation result in QSpice compared to in LTspice

Hi, Mike.
The following circuit had different simulation.
LTspice gave a sawtooth Vout with max value 1V.
But Qspice gave 1kV max Vout.
Please help me review it. Thank you.

BTW, do we plan to have an option to customize the hotkey by setting a config file? Is it possible to give a simulator option to let user to select local simulator like hspice or ngspice for circuit simulation?

*********** netlist ************************

  • .\Fig1_34.asc
    Vin Vin 0 pulse (-1 1 0 1u 1u 2m 4m) AC 1
    XX1 Vm 0 Vout ideal_op_amp
    Rin Vin Vm 1k
    C1 Vout Vm 1u

  • block symbol definitions
    .subckt ideal_op_amp Vinm Vinp Out
    G1 Out 0 Vinm Vinp 1Meg
    R1 Out 0 1
    .ends ideal_op_amp

.tran 10m
.ic V(Vout)=0
.plot V(Vout)

SPICE can have strange ways of dealing with initial conditions. QSPICE simply asserts them with a 1mΩ impedance. If you don’t want to increase the impedance of your “Op-Amp” you can either change

Vin Vin 0 pulse (-1 1 0 1u 1u 2m 4m) AC 1


Vin Vin 0 pulse (-1 1 0 1u 1u 2m 4m) DC 0 AC 1

Or you can add “UIC” or “SKIPBP” to the .tran command.