Strange simulation results about qucs_s HOT 5 CLOSED

Hi @dsm , consider checking the number of point on settings transient, maybe that will help.

from qucs_s.

tran 0.001 3
works just fine

from qucs_s.

@dsm

You are using a default diode model in the first circuit. LTspice and Qucs-S have the different default diode model. You have BV=10V in Qucs-S by default and diode goes to breakdown producing wrong output. Set the BV=1000V and everything will work as expected. The another issue is that you have used default transient points number. Ngspice is able to adjust transient time step but only to some extension. You have to set the points numbers manually for long transient simulation durations. Espesially if Tstop is greater than 5-10 waves of the input signal source. You have Tstop=3s and F=50Hz. Ngspice may skip the sine waves and show wrong result.

The convergence issues with 1N4007 model is not a Qucs-S bug. It is related to Ngspice bug: https://sourceforge.net/p/ngspice/mailman/ngspice-devel/?viewmonth=202205 I have reported this once, but it seems it has appeared again. The workaround is to set Ikf=1e-20 in the diode parameters. I can patch the diodes libraries to provide this workaround for all users.

from qucs_s.

BV=1000V will solve the problem and number of the point not set to default but not as high as 32768. thank you for your explanation.

from qucs_s.

I am transferring this to discussion. The issue with Ikf parameter probably should be reported to Ngspice team after providing a minimal netlist example to reproduce.

from qucs_s.