AC analysis at fixed frequency and plot against sweep parameters other than frequency

[niuniuaba]

Hello there,

I am trying to do an AC analysis at a fixed frequency (250KHz) with DC voltage as a sweep parameter. After the analysis I want to plot something defined by Nutmeg equation against the DC sweep rather than frequency. But no data plotted in the graph and I noticed there is a 'invalid' at the end of the name of Y axis. Did I do anything wrong? (engine is Ngspice).

schematic and plot is here in png

I also attached the netlist and dataset file here. Any help will be greatly appriciated.

netlist_dataset.zip

Best regards,
niuniuaba

TODO list

• Add example for CV curve simulation

[ra3xdh]

I am aware about this problem. The fixed point AC analysis in Ngspice is a hack. And parameter sweep is also implemented in Qucs-S using hack with for loop, because Ngspice doesn't have .STEP analysis mode like XYCE. If you are trying to implement AC(1-point) with Par.Sweep in will produce a set of 1x1 point plots instead a smooth curve. Look also here #156 and #161. These two issues describe the same problem. There is no workaround for this issue. And it still be unclear how to fix it in the application.

[holvo]

Please have a look at https://ngspice.sourceforge.io/ngspice-control-language-tutorial.html#step for the capability of the control language for loops and .step emulation.

A modified netlist for use in plain ngspice is attached, which enables plotting of ac data versus dc sweep voltage.
niuniuaba_mod.zip

[holvo]

These discussions lead to new ideas and options: On ngspice git branch pre-master there is a new control language function cvector, which creates a complex vector, to store ac loop results directly.

niuniuaba_mod_2.zip

[ra3xdh]

Hello Holger, thanks for looking into this. I have added an example of Qucs-S schematic implementing CV-curve plotting based on your netlist example. This example uses "Nitmeg script" simulation mode. @niuniuaba , I hope this may help you. I will include this example into the Qucs-S distribution. This may be help for other users trying to plot CV-curve.

The attached screenshots show simulation example and plot settings.

[ra3xdh]

I have uploaded CV-curve simulation example schematic in the recent commit.

[niuniuaba]

Hello @ra3xdh and @holvo

Thank you very much for you help. Now I can plot CV curve in my case.
It's a bit off topic but I noticed that there is kind of difference in the curve from that of LTspice if I use tenary_fcn explicitly but if I use if() function and set ngbehavior=ltpsa I get almost same curve as LTspice.
One more question, is it possible for qucs-s to read local .spiceinit file when it invokes ngspice binary so that one doesn't have to put a .spiceinit section in every schematic?

Best regards,
niuniuaba

[ra3xdh]

if I use if() function and set ngbehavior=ltpsa I get almost same curve as LTspice

This should be reported to Ngspice team. Please provide a minimal example that can reproduce the different behavior. This may be not directly to if operator, but some other fucntions may work differently if compatibility mode is applied.

is it possible for qucs-s to read local .spiceinit file when it invokes ngspice binary

No, there is no way to set the global .spiceinit from the Qucs-S GUI. You should include the settings in schematic.

[ra3xdh]

Closing this as resolved.