Dear All,
I am trying a first simulation with KiCad and logic gates.
I downloaded the library of 74LS00 and tried to create a circuit.
I always get the error message:
Dot command ‘.probe alli’ and digital nodes are not compatible.
Evtcheck_nodes: Auto bridging is switched off but node probe_int_net-_u1-pad1__xu1_1 is mixed-type.
Error: circuit not parsed.
How can I proceed? with standard DC circuit it works
please help!!
In KiCad 7.99:
Inspect → Simulator → Ctrl+N (opens New Simulation Tab):
Uncheck the tick boxes of ‘Save all currents’ and ‘Save all power dissipations’.
In digital mode the currents and power cannot be simulated. Checkbox ‘Save all currents’ directly involves the ngspice dot command ‘.probe alli’.
Open all existing simulation tabs and do the same.
I try to follow step 7.2 of this guide: https://ngspice.sourceforge.io/ngspice-eeschema.html#digi
Aparently this doesn’t work as expected with the German version of KiCad 8.0.5.
Although both simulation options “Alle Ströme Speichern” and “Alle Verlustleistungen speichern” are deselected, still the errormessage “Dot command ‘.probe alli’ and digital nodes are not compatible.” appears.
In the spice netlist, there is no ‘.probe alli’. Still the error message is present.
.title KiCad schematic
.include "C:/Projects/ngspice/74xx/74HC00m.lib"
.save all
.op
V1 /a1 0 DC 3.3
V2 /b1 0 DC 0
R1 /y1 0 1Meg
XU1 /a1 /b1 /y1 NC-U1-0 NC-U1-1 NC-U1-2 NC-U1-3 NC-U1-4 NC-U1-5 NC-U1-6 NC-U1-7 NC-U1-8 NC-U1-9 NC-U1-10 74HC00m
.end
Seems to be a bug in ngspice. The old error flag is not reset when receiving a new netlist without ‘.probe alli’ (after having removed the current and power measurement flags).
I will care for this bug.
For now it is only possible removing the flags before the first simulation is started.
Or you create a workbook file after the flags have been removed, leave simulator and Eeschema and then return.
I have puished a fix to ngspice git development branch ‘pre-master-44’ (ngspice / ngspice / [458982]). It will appear in ngspice-44 in early January.