I downloaded this demo circuit from https://www.analog.com/en/design-center/evaluation-hardware-and-software/lt-spice-demo-circuits.html
When I attempt to run the simulation it never converges. Any suggestions? Thanks.
The demo is tilted "LT6200 & LTC2050 Demo Circuit - Low Noise, Low Power Photodiode Transimpedance Amplifier with DC Precision"
I tested this schematic and indeed the simulation doesn't start due to a convergence problem.The reason may be that one of the opamp models have changed since the schematic had been created…
I tested this schematic and indeed the simulation doesn't start due to a convergence problem.The reason may be that one of the opamp models have changed since the schematic had been created.
When LTspice starts a simulation, it firstly try to find the DC-operating point. The table below shows the order and the methods which are used.
From the help pages:
The circuit simulation with the circuit LTC2050_LT6200_DN308F2.asc fails with all four methods.
I often try then with the pseudo transient option "ptrantau".
LTspice has now found the DC operating point after some time, because it tried the three other methods before.One can skip the thirst three methods to quickly get the simulation done. See the combined SPICE-directive below.
.options noopiter gminsteps=0 srcsteps=0 ptrantau=100n
I have attached the circuit with the added SPICE-directive.
You are a wizard! Thank you my friend.