Hello, When trying to get the back annotation feature working. I have in place:

* Is this option needed, this option causes the ngspice error:
* "Warning from checkvalid: vector @m.xm1.msky130_fd_pr__pfet_01v8[ib] is not available or has zero length."
* .option savecurrents
.save all

When the

.option savecurrents

is specified, this causes no new RAW file to be created, but an error to occur, is this usage error or a bug ? When I attempt to "load waves" with code.sym "xschem raw_read $netlist_dir/testbench.raw tran" no error is shown, no indication an action was performed occurs and no update to visual seen. When I use the menu "Graphs -> Annotate Operating Point ... -> pick RAW file -> OK" the visual updates with question marks "? ?" the only data that is updated are the ammeter.sym and spice_probe.sym I added to the design. None of the transistors show values. I think I need to inject a wave graph into the schematic view, to provide an X axis time reference to show sample for, can''t see an obvious design/*.sym to insert for this, so hunting for a project with that configured. Also what is the best symbol to be using to inject test points for data collection (I and V for example), ideally with a quick toggle button list to disable/enable (without need to rework the schematic, to remove the injected symbol when you want to disable it). This would then modify the netlist creation and ngspice config accordingly to the disable/enable state of the individual test point. Also after some time in usage of xschem the application refuses to take any more mouse click input to select items in the main design area. Menu items work ok, a restart always fixes it. Is this is known matter maybe with Tk/X11, using Linux/Xwayland ? Thanks

To avoid the zero length error put a

remzerovec

instruction before the

write

command. All simulation variables like gm, vth, gds and so on need to be saved explicitly:

save @m.x1.xm5.msky130_fd_pr__nfet_01v8[gm]
save @m.x1.xm5.msky130_fd_pr__nfet_01v8[gds]
save @m.x1.xm5.msky130_fd_pr__nfet_01v8[gmbs]
save @m.x1.xm5.msky130_fd_pr__nfet_01v8[vth]

Thanks for the responses. It would be good to have

spice_ignore=0

an implicit default when inserting ammeter (then everyone can see it there), like the

savecurrent=true

is, then at least someone reading can lookup docs for it (or guess) at what it does. Success with

.option savecurrents

and then

.remzerovec

there is no error now in ngspice wiring out raw file, and see I(current) values next to all transistors. Just trying things out with your suggestion re voltages, am already using

spice_probe

for specific things, but when debugging showing voltage for all nets. Assigning a net name, means removing the default hash from in front of the default auto-generated name, or specifying your own

lab=

value that does not start with a hash.

inserting a net name means attaching a

lab_pin.sym

or

lab_wire.sym

(they only differ in text positioning) to a net:

Thanks for replies, one final quality of life query, the

devices/launcher.sym

how do you activate the launch function. When I click, double-click it is into 'edit properties', right click menu does not have 'launch' option. I try with modifiers as well Shift/Ctrl etc... I can not observe launch action occuring. Is that Xwayland inter-op issue?

Thank you for the reports. I have made a small commit such that if a tclcommand in a launcher does not run successfully an alert dialog box is shown.

Thanks very much for the improvements

Also a warning is displayed if a launcher does not have any action defined (url=... or tclcommand=...)

Hello, When I am trying to annotate operating points id, gm,cgg and vth into the schematic. While id, gm, and cgg have been updated and displayed in the schematic, vth is not appearing correctly and is instead showing a question mark. Am I missing something? Regards

the vth must saved with v(...): .save v(@m.xm5.msky130_fd_pr__pfet_01v8_lvt[vth])