Analog simulation (ngspice)

One of the kicad_skills usage guides for the eda CLI — all of them. Plain Markdown: read it directly, or hand it to whatever assistant you use.

ngspice runs inside the container (see the eda-environment guide), the same engine KiCad’s built-in simulator uses, so results agree with what the user sees in Eeschema.

Workflow

# 1. write the deck (plain SPICE, any editor/tool)
# 2. cheap syntax check before burning a run
./bin/eda.sh sim lint sim/rc.cir
# 3. run it: writes raw + CSV + measurements + PNG plots
./bin/eda.sh sim run sim/rc.cir -o sim/out

sim run returns JSON: ok, errors (parsed from the ngspice log), and one entry per analysis with csv, plot (PNG) and measurements. Read the PNG with the Read tool when the shape of the response matters — the numbers alone hide ringing, clipping and convergence artefacts.

Deck conventions that avoid the usual failures

* first line is ALWAYS the title - it is discarded
V1 in 0 DC 0 AC 1 SIN(0 1 1k)      * AC 1 = 1 V stimulus for .ac
R1 in out 1k
C1 out 0 159.155n
.ac dec 200 10 100k                * decade sweep, 200 points/decade
.tran 10u 5m
.end

• Node 0 is ground and must exist, otherwise ngspice reports a singular matrix.
• Give the AC source AC 1 so gains come out in dB directly.
• .include/.lib paths are resolved relative to the deck; model files next to the deck (*.lib, *.mod, *.sub) are copied into the work directory.
• Sweep at least a decade beyond the region of interest; use dec (log) for AC.
• For transient runs, make the step small enough (≥20 points per period of the fastest signal) or the measurements will be wrong rather than noisy.

What is measured automatically

THD needs the fundamental, so it is a separate call:

./bin/eda.sh sim measure sim/out/work/sim.raw --thd "v(out)" --fundamental 1000 --skip 1m

Will it still work with real parts? (tolerance analysis)

A nominal simulation is the one circuit you will never build. Vary the parts inside their tolerance and look at the spread of the number you actually care about:

./bin/eda.sh sim montecarlo sim/rc.cir -o sim/mc \
    --vary R1=1% --vary C1=10% \
    --metric ac.v(out).f_minus_3db_hz \
    --trials 200

Returns statistics (mean, stdev, min/max, p05/median/p95, spread_pct), nominal_metric for reference, a histogram.png and trials.csv. The metric is a path into the usual measurements: <analysis>.<signal>.<key> — e.g. ac.v(out).gain_db_max, tran.v(out).overshoot_pct, or op.v(out).

Which part is responsible

The same run also answers “so which component do I need to buy tighter?”. sensitivity ranks every varied part, with sensitivity.png as the picture:

{"explained_pct": 99.7,
 "parameters": [{"parameter": "C1", "contribution_pct": 99.3, "elasticity": -0.99},
                {"parameter": "R1", "contribution_pct":  0.7, "elasticity": -0.96}]}

• contribution_pct — that part’s share of the spread. Here the 10 % capacitor is the whole problem and the 1 % resistor is irrelevant, so a tighter C is the only change worth paying for.
• elasticity — how many percent the metric moves per percent of that part. -0.99 says the corner frequency falls almost exactly in proportion, which is what fc = 1/(2πRC) predicts.
• explained_pct — how much of the spread a straight line accounts for. Well below 100 means the circuit does not respond linearly over that tolerance band, and the per-part split is indicative rather than exact. Look at the histogram before trusting the ranking.

It costs no extra simulation — it is the trials you already ran, read column-wise. It needs at least three trials and more trials than varied parts.

• --distribution normal (default) treats the tolerance as ±3σ, clipped to the band — how reels of parts actually behave.
• --distribution uniform is the honest choice when you know nothing about the distribution.
• --distribution worst samples only the two extremes, which finds the corners fastest.
• --vary also accepts .param names, so anything parameterised in the deck can be swept, not just R/C/L.
• --seed makes a run reproducible; quote the seed when you quote the result.

Judge the result against the requirement, not against the nominal: “fc = 1000 Hz nominal, 5th–95th percentile 968–1035 Hz with 1 % parts, spec is ±5 % → passes with margin”.

Does it survive the temperature range?

./bin/eda.sh sim temperature sim/bias.cir -o sim/temp \
    --temperatures -40 0 25 85 125 --metric op.v(out)

Runs the deck at each temperature (.temp) and reports the metric per point plus drift_per_celsius. Only models with temperature coefficients will move — ideal R and C do not, so a flat result means the models are ideal, not that the circuit is stable.

Simulating a KiCad schematic

./bin/eda.sh sim netlist hardware/amp.kicad_sch -o sim/amp.cir   # kicad-cli export
./bin/eda.sh sim run sim/amp.cir -o sim/out

The export only produces a usable deck when the symbols carry Spice model fields (Spice_Primitive, Spice_Model, .model/.subckt includes). For a plain schematic it is usually faster and more honest to hand-write a deck for the sub-circuit under investigation and say so in the report.

Interpreting the result honestly

• State the operating point first — a simulation of a circuit biased into the rail is meaningless however pretty the AC plot is.
• Compare against the closed-form expectation (fc = 1/(2πRC), A = -Rf/Rin, …). If simulation and theory disagree, the deck is usually wrong.
• Convergence failures, singular matrix, timestep too small are reported in errors; fix the circuit (add a DC path to ground, .options relaxation) rather than ignoring them.
• Ideal parts are ideal: op-amp models without supply pins never clip, real regulators have ESR-dependent stability. Say which effects the model omits.
• Report value (analysis, conditions) and keep the generated PNG/CSV in the repository next to the design when the result matters.