Quickstart guide to run ngspice

1. CMOS inverter netlist

C5_inverter_VTC.cir
*** SPICE deck for C5_inverter_VTC.cir

.global gnd vdd

* MOSTs models
.include ../../class/models/C5_models_bsim3.mod

* circuit (CMOS inverter)
Mnmos out in gnd gnd NMOS L=0.6U W=3U
Mpmos vdd in out vdd PMOS L=0.6U W=6U
Vin in gnd DC 0V
VDD VDD 0 DC 5

* Analysis (VTC)
.DC Vin 0 5 1m

* Outputs
.PLOT DC V(out) v(in)
.END

2. Browse to the location of the netlist

$ cd //VBOXSVR/talarico/ngs406/Electric

3. Create an initialization file .spiceinit with the following configurations

.spiceinit
set ngbehavior=hs
set ng_nomodcheck
set color0=white
set color1=black
set xbrushwidth=2

the behavior of ngspice is set in hspice compatibility mode
any model parameter check is suppressed
color0 is the background
color1 is the text and the grid
xbrushwidth is the Linewidth of the graphs

4. Start ngspice in interactive mode

$ ngspice

5. Have ngspice parsing the netlist

ngspice 1 -> source C5_inverter_VTC.cir

6. Run the simulation

ngspice 2 -> run

Doing analysis at TEMP = 27.000000 and TNOM = 27.000000

Warning: Pd = 0 is less than W.
Warning: Ps = 0 is less than W.
Warning: Pd = 0 is less than W.
Warning: Ps = 0 is less than W.

No. of Data Rows : 5001

7. Display all vectors

ngspice 3 -> display

Here are the vectors currently active:

Title: *** spice deck for cell c5_inverter_vtc{sch} from library c5_cmos
Name: dc1 (DC transfer characteristic)
Date: Fri Nov  5 20:28:26  2021

    in                  : voltage, real, 5001 long
    out                 : voltage, real, 5001 long
    v-sweep             : voltage, real, 5001 long [default scale]
    vdd                 : voltage, real, 5001 long
    vdd#branch          : current, real, 5001 long
    vin#branch          : current, real, 5001 long

8. Display all voltages

ngspice 4 -> display allv

    in                  : voltage, real, 5001 long
    out                 : voltage, real, 5001 long
    v-sweep             : voltage, real, 5001 long [default scale]
    vdd                 : voltage, real, 5001 long

9. Display all currents

ngspice 5 -> display alli

    vdd#branch          : current, real, 5001 long
    vin#branch          : current, real, 5001 long

10. Plot v(in) and v(out)

ngspice 6 -> plot v(in) v(out)

11. Other common commands that can be used with the interactive interpreter are:

listing
show
showmod
history
shell [command]
getcwd
cd
load [rawfile]
write [rawfile]

12. For more information look up the ngspice manual