Importing SPICE netlists
On this page
Kessetsu 1.6.0 can convert the supported Ngspice-compatible netlist subset into editable
Kessetsu source. For a complete first example, save this as filter.cir:
.title RC low-pass
VIN IN 0 AC 1
R1 IN OUT 1k
C1 OUT 0 159.154943n
.ac dec 40 10 100k
.end
With the CLI and Ngspice installed, you can check, simulate, test against .kessreq requirements,
render a schematic or export to KiCad directly from the SPICE file (--input auto is the default):
kess check filter.cir
kess simulate filter.cir
kess test filter.cir --requirements filter.kessreq
kess render filter.cir --output filter.svg
kess export filter.cir --target kicad --output filter.kicad_sch
To save the converted, editable .kess file explicitly, use kess import:
kess import filter.cir --output filter.kess
If --output is omitted for a file input, kess import uses the same basename with .kess.
Existing files require --force. Standard input is supported with
kess import - --output circuit.kess (or kess check - --input spice); it never chooses an
implicit file destination.
In Web Hub, choose File → Import SPICE netlist… or drop a supported
netlist onto the editor. Conversion runs locally through the same Core contract. A complete
import opens as an unsaved editable circuit; a rejected import leaves the current document intact.
The rejection panel names the file, shows the first diagnostic and keeps the complete Core
diagnostic list under All import diagnostics. Line numbers refer to the original SPICE
file, not your open .kess. Correct the original file, then use Choose another netlist…;
the panel also links to this guide and the RC example above. It does not delete unsupported
lines, substitute models or detach the existing save destination. A changed circuit while the
file picker/read is pending requires a fresh import rather than replacing your new edits.
For the example above, wait for Source valid, then press Run in Simulation and select
V(out) for the low-pass response. Import preserves the AC analysis but does not invent
engineering requirements: pass --requirements limits.kessreq in the CLI/MCP workflow or add
assert statements in the generated .kess if you want PASS/FAIL checks. See the
first-circuit tutorial and agent design workflow.
What the supported subset accepts
| SPICE form | Kessetsu result |
|---|---|
R, C, L with literal quantities and European RKM notation (4k7, 1u5) |
resistor, capacitor, inductor (trailing parameters like tc1, tol, ic tolerated with KES-N011) |
K coupled inductors (K1 L1 L2 0.99, K1 L1 L2 L3 0.98) |
couple statements (two-winding and multi-winding with uniform coupling) |
Independent V and I |
DC, AC, three-field SINE, seven-field PULSE, six-field EXP (exp(...)), or comma/space-paired PWL source, plus combined DC bias + AC (V1 in 0 DC 5 AC 1 0 -> ac(1, 5)) |
Linear dependent sources: E (VCVS), G (VCCS), F (CCCS), H (CCVS) |
vcvs, vccs, cccs, ccvs (folds independent 0 V sense branches into Kessetsu's canonical 4-pin controlled sources) |
Voltage-controlled switch S with .model ... SW |
switch component and model switch declaration (or default KESSETSU_SW_V1) |
D, Q, J (JFET), three-terminal M, and four-terminal M (MOSFET) |
built-in models (1N4148, 1N4007, Schottky 1N5819, LEDs LED_RED, LED_GREEN, LED_BLUE, LED_WHITE, Zener diodes 1N4733A, BZX84C*, 2N3904, 2N3906, 2N2222, BC547, BC557, 2N5457, J2N5457, J201, 2N5460, IRF540, IRF9540, 2N7000, BSS84, KESSETSU_*) or inline .model. Four-terminal MOSFETs (M1 d g s b model) with bulk tied to source fold to 3-pin mosfet, while explicit separate bulk nodes (b != s) import with all 4 pins (d, g, s, b) connected. Four-terminal BJTs fold grounded substrate (0/GND) or emitter with KES-N011 warning |
5-terminal X op-amp (in_p in_n vcc vee out with KESSETSU_OPAMP_V1, KESSETSU_OPAMP_V2, LM358, TL072, or OPAMP) |
native opamp component (with op-amp ERC and schematic symbol) |
| Inline `.model NAME D | NPN |
.op, bounded .tran, .ac, single-source .dc |
typed simulate statements |
.ic V(<node>)=<value> (space- or comma-separated pairs, literals or {expr}) |
native initial V(<NET>) = <value> declarations (round-trip supported without warning) |
.param NAME=literal or evaluated arithmetic/math {...} |
typed editable parameter, evaluating arithmetic and math functions (+ - * / ^ **, pi, e, sin, cos, tan, sqrt, ln, log10, exp, abs, min, max, pow) with unit inferred from supported uses |
Source-embedded .SUBCKT plus root X instances |
editable module/use, preserving ports, local topology and literal typed overrides |
First-line plain title, .control ... .endc, .print, .plot, .probe, .save, .meas, .nodeset, .options |
tolerated and skipped with informational/warning diagnostics (KES-N010..KES-N012) because Kessetsu owns simulation runner control and measurement evaluation |
Continuation lines beginning with +, comments, .title and .end are understood. SPICE node
0 becomes the explicit GND net. Other node, component and inline-model names are preserved when
valid or mapped deterministically when Kessetsu identifiers or built-in model names require it.
--format json returns the kessetsu.spice-import.v1 report, source hash, name mappings,
diagnostics, summary and verified editable source.
SPICE suffix meaning is preserved rather than copied blindly. In SPICE, 10M means 10 milliohms,
while Kessetsu uses SI casing where 10M would mean 10 megaohms. The importer therefore writes a
normalized number and canonical recompilation confirms the resolved value.
Fail-closed limits
The importer rejects electrical constructs that cannot be represented truthfully in Circuit IR instead of guessing or silently removing components:
- non-linear arbitrary behavioral sources (
Bcards produceKES-N002, as doVALUE,POLY,TABLE,LAPLACE,FREQ); - arbitrary external
.include/.libfile paths (KES-N003); - simulator control directives such as
.stepparameter sweeps (KES-N003); - transmission lines (
T,TX) and unsupported component families; - unknown
.modelfamilies or unsupported model parameters; - parameter expressions with conflicting units or unresolved circular definitions;
- invalid
.icdirectives (empty.ic, unknown node, ground node0/GND, duplicate node, orI(...)inductor-current initial conditions fail withKES-N002); - unknown semiconductor models without an inline
.model, non-zero AC source phase, or analysis options that the typed Kessetsu IR cannot represent.
Embedded subcircuits are intentionally structural, not raw simulator text. A .SUBCKT must have
explicit interface nodes and may contain the same supported component subset as the root circuit.
Literal defaults declared after PARAMS: and named literal/root-parameter overrides on a root X
instance remain typed module parameters. Nested X instances, body directives, implicit global
node 0, positional parameters and expression-valued defaults/overrides are rejected rather than
flattened or guessed. Expose ground as an ordinary subcircuit port and pass root node 0 to it.
An external .include/.lib is different from an embedded topology: its bytes, entry pins,
provenance, license and redistribution policy cannot be inferred safely from a path. Import
therefore rejects it. Bind such a dependency through Kessetsu's hash-pinned typed external model
contract; the importer never opens an arbitrary path or silently substitutes a generic device.
An error includes the original source line and no .kess file is written. This is intentionally
narrower than the complete SPICE language. Support expands only when connectivity, values, models
and analysis meaning can be represented and verified without a raw-SPICE bypass.
PySpice
Generate a netlist in the user's own Python environment, save it, then import that file with the same command. Kessetsu does not execute Python and does not claim to preserve Python loops, functions or intent that are absent from the generated netlist.
For example, this PySpice 1.5 circuit emits only constructs in the supported import subset:
from PySpice.Spice.Netlist import Circuit
from PySpice.Unit import u_V, u_kOhm
circuit = Circuit("Voltage divider")
circuit.V("IN", "IN", circuit.gnd, 10 @ u_V)
circuit.R(1, "IN", "OUT", 1 @ u_kOhm)
circuit.R(2, "OUT", circuit.gnd, 1 @ u_kOhm)
circuit.raw_spice += ".op\n"
with open("divider.cir", "w", encoding="utf-8") as output:
output.write(str(circuit))
Then run kess import divider.cir --output divider.kess. Compatibility is determined by the
generated SPICE text, not by the Python library version: unsupported devices or directives still
fail closed with a source-line diagnostic.
The successful .kess file is the normal save, share, edit, simulation and export artifact. Keep
the original netlist beside it when provenance matters; its exact SHA-256 identity appears in the
generated source header and JSON report. Imported simulation remains model-based evidence, not a
guarantee of physical hardware behavior.