A simple RC low pass circuit generates the following netlist:
.title KiCad schematic
.save all
.probe alli
.probe p(R1)
.probe p(C1)
.probe p(V1)
.ac dec 10 10 100k
R1 Net-_R1-Pad1_ /v_out 10k
C1 unconnected-_C1-Pad1_ GND 10n
V1 Net-_R1-Pad1_ GND DC 0 SIN( 0 0 0 0 0 0 ) AC 1
.end
Given the command probe alli don’t the specific .probe get redundant?
The specific probes are to measure power. In an ac simulation this does not make much sense, so the results are not shown in the signal list, and you better switch off “Save all power dissipations” in the SPICE command window of the ac simulation.
Thanks @holger.
I’m from a school of thought where “all” means “all inclusive”, it seems I’ve to become accostumated to the Ngspice terminology 
On the other hand, I would like to suggest that power measurements are not that unsensical in AC sweeps, as it may appear at first sight, as a counter example, to compute the dissipation of non ideal reactive components in RF power filters¹.
Again thanks for the repplies and the patience with a new, but enthusiastic, user of Ngspice.
Regards
[1] One user (@kevinz) asked for a way to obtain similar information, although not power per se, but in a more complete simulation, will get there.
What does “all you can eat” in your school then?
Is it everything that fits in your stomach at one particular time, or is it all edible resources this planet has to offer at a particular time?
Do you agree (at least in English and other languages I command) that can already encompasses the Universe of edible things, and the you has as enthymeme human beings (so to avoid edible things by goats, for example?).
The context of the simulation “probes” are the nicknames given for the generation of data vectors (that in the SPICE 3f5 were called “plots”) mimicking the use of pertaining instruments in the circuit under analysis.
Spice simulators have a long history and I recall thirty years ago when the way to obtain a current in a branch was to insert a zero voltage independent source in it to be able to get the “plot”, nowadays this is almost bygone, except in some implementations.
So as Ngspice is in constant evolution, is a learning curve – at least to me – to see what the terminology decided by the project team may mean in corner cases, as I found this one.
In other cases the manual is clear that Ngspice does different and directs to the syntax the team deemed correct or adherent to their objectives.
HTH
See the ngspice manual section 11.6.5 which describes using .probe for saving current, voltage, and power.
.probe alli is described as “General form for current measurements on all devices”.
In other words, alli means all (all) current (i), not all (gestures broadly).
Unambiguously yes. (20char)
Thanks for engaging, @gkeeth !
Could you please check the results if you capture the RC circuit I posted in the start of this thread, or at your discretion the one proposed in page 309 of current (ver 43), and see if in your simulation pane also all the voltages appear as well?
In my Kicad 8.0.4 release I get four voltages for ploting, and interestingly no way to see the power in simulation pane!
Thanks
I’m not sure exactly what you’re asking. This is what I get when I capture an RC lowpass filter schematic that matches what I assume your intent is:
You have not shared your schematic, so I can’t say for sure, but based on your netlist I think you have an error in your schematic where the capacitor is not connected to your v_out node. Note the unconnected-_C1-Pad1_ node name on the C1 line. I don’t know if this is causing the issue you describe or not.
The very first post in this thread has an schematic!
Your results (in the panes you post) are similar to mine, so:
I see two (complex) voltages as a result of the machinery Kicad+ngspice, or four as we have gain + phase.
IMNSHO it contradict your twenty chars assertion that probe alli only would collect currents.
Also, as the three power probes as clarified by @holger do not have a means to be ploted in the present implementation of the simulation panes I stumbled in the understanding of the human machine interface as is.
I’m positive the warning does not cause the appearing of voltages in the ngspice output
Thanks
This thread does not have a schematic, just a netlist…
.save all command.probe alli command.probe P(<device>) commandsYou can check this in the ngspice manual, or by editing your simulation settings in KiCad (check and uncheck the save voltage/current/power checkboxes in the simulation setup, and compare the netlist).
I agree you can’t plot powers in the GUI in an AC sim. If you do a transient sim, you can.
OK, so to be clear and check my understanding:
probe has a p(<something>) as argument, then it saves powers.I believe this state of affairs happen due the incremental development of Ngspice and so the atavisms are now a legacy which would be expensive from the point of view of development and backwards compatibility, so I’ll take notes of this to avoid confusion from my part.
OK about power only available in transient simulations.
Thanks,
Eh, that’s not really a fully accurate list. The .save all line saves all the node voltages (i.e. referenced to ground) including internal nodes. External node voltages are saved by default, even without the .save all. And .probe can be used to measure arbitrary differential voltages, in addition to current and power.
From my read of the manual, the thing that all the .probe varieties have in common is that in all modes (voltage/current/power) it internally adds an additional source to your netlist to accomplish the measurement (0V voltage source for current, unity gain VCVS for differential voltage, and both for power).
The manual gives all the hairy details of all of these.
This topic was automatically closed after 90 days. New replies are no longer allowed.