Debugging and Ability to see the Real netlist

[tomhajjar]

Ran into a problem caused by a typo but the error messages from ngspice referenced nodes, vectors and subcircuits hidden from the User. This is especially true for schematics containing subcircuits and Library devices.

To see the REAL netlist requires running ngspice.exe which brings up it's console so one can type commands to dump variables and the REAL netlist. It makes the Error messages make a lot more sense.

At a minimum the ability to see the REAL netlist would be a big help. Too many times the Error messages are impossible to decipher.

1. Use the commands 'display' and 'edisplay' to see what vectors are available in the current plot.
2. Use command 'listing e' (e for expanded) to see what netlist is finally simulated in ngspice after all the nested subcircuits have been inserted and expanded.

https://sourceforge.net/p/ngspice/discussion/120973/thread/73d9549257/?limit=25#a46f

[ra3xdh]

The requested feature is not possible to implement within Qucs-S. Closing issue.

[tomhajjar]

@ra3xdh

Holger says just insert the following line into the netlist.
listing e > filename

I made a test netlist and it worked. I added the commands below to the control section. Placement is critical. Best to add to end of control loop.

display > variable.txt
edisplay > variable_e.txt
listing e > netlist_e.txt

https://sourceforge.net/p/ngspice/discussion/120972/thread/6035934769/?limit=25

[tomhajjar]

@ra3xdh

I added a Nutmeg script with the commands but I'm having an issue. The file netlist_e.txt looks OK but the two variable files variable.txt and variable_e.txt are wrong. The problem is caused by the "destroy all" and "reset" commands in the netlist between the tran statement and the 3 netlist/variable commands.

I thought moving the 3 netlist/variable commands before the tran statement would help but that also caused the two variable files to be wrong. The tran statement must be first. Included are my test files.

Bottom line the netlist can be written to the spice4qucs folder with a single statement "listing e > netlist_e.txt" in a Nutmeg script. It could be viewed using the method the Qucs-S netlist is viewed.

Using Qucs-S files get written to spice4qucs.
Using DuSpice files get written to ngspice/bin.

[ra3xdh]

Moved to Discussion/Ideas. Probably someone will implement it. I have more important task for this and next release cycles.

[tomhajjar]

If you want plots using DuSpice, the Qucs-S netlist must be edited.

Below are my .control section edits and what command effects what. Some of the commands also corrupt the debugging files.

.control
tran 5e-05 0.005 0

*write spice4qucs.tr1.plot v(in) v(out1) v(out2) v(out3) v(out4) ; unneeded for debugging
plot v(in) v(out1) v(out2) v(out3) v(out4)

*destroy all ; Corrupts variable.txt & blocks plot
*reset ; Corrupts variable_e.txt

*Debugging files
listing e > netlist_e.txt
display > variable.txt
edisplay > variable_e.txt

*destroy all ; Closes plot
*reset ; Closes plot
*exit ; Closes plot
.endc
.END

ngspice netlist-variables.zip