SPICE netlists

Run a SPICE deck and plot the results, export a circuit as a .cir file, or import a netlist as parts and wires.

Where it is

Run a SPICE deck… is in the editor's menu. Download SPICE and Open JSON or SPICE… are in the Save menu: the first writes a file, the second reads one. A file ending in .cir, .sp or .spice is read as a netlist; anything else is read as a Mokxi project.

Run a deck

Run a SPICE deck… opens a sheet with the deck in a text box. Paste one, pick one from Examples..., or press Open files and choose the deck together with any files it .includes. Press Run. Each analysis comes back as a result you pick from the list: a transient or a sweep as waveforms, with a box for every node voltage and branch current, an AC analysis as a Bode plot of gain and phase, a noise analysis as its spectrum, and an operating point, .tf or .meas as a table. Download CSV saves the result on screen.

What it reads. A title line, * and ; comments, + continuations and SPICE's scale suffixes; .param with expressions and .func; .subckt and .ends with parameters, nested to any depth; .include and .lib of the files you opened with it; .model cards; .ic, .nodeset, .options, .temp, .step and .end. Elements: R, C, L and K; independent V and I sources with DC, AC, SIN, PULSE, PWL, EXP, SFFM and AM; the controlled sources E, F, G and H, including POLY; B sources with the usual functions of v(), i() and time; S and W switches; T lossless transmission lines; D diodes with breakdown, capacitance and series resistance; Q Gummel-Poon bipolar transistors with the Early effect and junction capacitances; J JFETs; M MOSFETs of levels 1, 2 and 3 with their capacitances; and X subcircuit instances.

The analyses. .op; .tran, with UIC and a maximum step; .ac over dec, oct or lin; .dc, with a second, nested sweep; .tf; .noise; and .meas in its common forms (TRIG/TARG, WHEN, FIND, AVG, RMS, MIN, MAX, PP, INTEG). An operating point that plain Newton-Raphson cannot find is found by gmin stepping, source stepping or pseudo-transient continuation, and the result says which it needed.

How far to trust it. The engine is checked against ngspice 42 on 42 benchmark circuits, from a voltage divider and RC, RL and RLC filters through rectifiers, a Zener regulator, transistor and MOSFET amplifiers, a differential pair, current mirrors, op-amp amplifiers, integrators and active filters, to oscillators, a latch, a Schmitt trigger and a buck converter. Every one agrees within a stated tolerance: DC values within 1% or 1 mV, AC within 0.1 dB and 1 degree, waveforms within 1% of their range (2% for switching waveforms), oscillator frequencies within 1%. The same checks run on every change to the engine.

What it does not do. MOSFET models above level 3 (BSIM), MESFETs, lossy transmission lines, XSPICE and digital devices, Laplace and frequency-table sources, and the .four, .sens, .pz and .disto analyses. A deck that uses one gets a message naming the line. MOSFET level 3's KAPPA differs from ngspice's by up to about 4% in saturation, and level 2 does not model VMAX, DELTA, XJ or NFS (a card that sets them is warned about).

A deck runs on its own, apart from the canvas: the circuit on the canvas is not changed, and the deck's parts do not appear on it. To turn a netlist into parts and wires, import it (below).

Export

The file is an ngspice deck that runs as it is: ngspice -b circuit.cir. It holds:

In Mokxi	In the file
resistor, capacitor, inductor	R, C, L
potentiometer, slide pot	two resistors, with the wiper at mid travel
vcc, bench supply	a DC V source
signal generator, function generator	a V source: SIN for a sine, PULSE for a square, triangle or sawtooth
multimeter on a current range	a zero-volt V source, which is SPICE's ammeter
diode, Zener, LED	D, with a .model card
transistor	Q, with an NPN or PNP .model card
MOSFET	M with its body on its source, W=1 L=1, and a level 1 NMOS or PMOS card
op-amp	X, an instance of a subcircuit for its model

The model cards are the engine's own. Each .model card is written by the engine from the device it builds for that part's model, so a 1N4148 in the file has the same Is, N, Rs, junction capacitance and transit time as the one Mokxi solves. A property you set on the part that the card can carry goes into it: a transistor's beta becomes Bf, and a MOSFET's vto, beta and lambda become Vto, Kp and Lambda. That part then gets a card of its own, named after it. An override the card cannot carry (a diode's forward, a Zener's vz) is named in a * NOTE line.

The op-amp is its macromodel. Each op-amp model used gets one subcircuit (OPAMP_741, OPAMP_RAIL_TO_RAIL and so on), and each op-amp is an instance of it with its resolved numbers on the line: open-loop gain, gain-bandwidth product, slew rate, offset, headroom, negative rail, current limit and output resistance. Inside it is the same single pole, swing clamp and current limit the engine solves. A 741 in a non-inverting gain of 11 exported this way has its 3 dB corner within 1% of Mokxi's own in ngspice.

The run. The file ends with .op and a .tran. The run is as long as the widest scope window in the circuit, or five periods of the slowest generator, or 10 ms. If you set a longest step in Analysis… (the time step), it is the .tran line's fourth number, TMAX. A .print line lists the scope channels and op-amp outputs.

What is left out. A board, a logic gate, a display, a sensor or anything else with no SPICE element is left out, and the file says so in a comment line that names the part and why: * OMITTED uno1 (uno): a board runs firmware, which SPICE cannot. Instruments that only watch (a scope, a voltmeter) are listed in * INSTRUMENT lines with the nodes they watch. The TIP120 Darlington is left out too, since it is two transistors and a diode and has no one-card form. After a download, the note over the canvas says how many parts were left out, and What lists them.

Nodes are called n1, n2 and so on in the order the file first uses them, and ground is 0. A .options rshunt=1e12 line puts a teraohm from every node to ground, so a node left hanging by an omitted part cannot stop ngspice from solving.

Import

The importer reads the same set back, from a Mokxi file or from a textbook deck:

• R, C, L with SPICE's scale suffixes (4.7k, 100n, 10meg);
• V sources: a DC source to ground becomes a supply (vcc), a floating one a bench supply, SIN and PULSE a signal generator, a zero-volt source a multimeter on its current range, and a source with an AC magnitude a generator you can drive from Frequency response;
• D, Q and M with their .model cards;
• X instances of Mokxi's own op-amp subcircuits, with their numbers;
• .tran, whose TMAX becomes the transient's longest step.

A model card from Mokxi comes back as the same part model. A card from anywhere else is matched by name when it names one of Mokxi's models, and otherwise becomes the nearest part: an NPN card becomes a 2N2222 with the card's Bf as its beta, and an NMOS card a 2N7000 with its Vto, Kp W / L and Lambda. A diode card that is not one of Mokxi's becomes the default diode, and its parameters are not carried.

Nothing is dropped without a word. An element or statement the importer does not read is named: a current source (Mokxi has no current source part), a controlled source (E, F, G, H, B), a switch, a subcircuit that is not Mokxi's own, .param, .include, and a value it cannot read. They are listed in the Serial panel, and the note over the canvas has a What button that lists them in full.

The layout. A netlist has no picture, so the importer draws a first one: the sources in a column on the left, every other part in a column by how many parts stand between it and a source, a ground symbol under every pin that goes to ground, and the wires routed by Tidy wires. It is a starting point to move things about from, not a finished schematic.

Round trip

Export, import and export again gives the same netlist: the same elements, the same values and cards, joined in the same way. What changes is the picture, the part names where a deck numbered them, and anything that was never in the file: instruments, boards, and a scope's window.