` loads the named `.lib section … .endl` block; a bare `.lib ` with no section does not load the file's models. - **This server's default `kiltpsa`** (a PSPICE-family mode) is the reverse: a bare `.lib ` loads an unsectioned file, but a sectioned `.lib

` (the PDK corner-select form) is split by the `lt`/`ps` tokens into two plain includes that drop the section, and the run fails with `could not find include file`. Set `[simulator] ngbehavior = "hsa"` in `ltspice-mcp.toml` (or `LTSPICE_MCP_NGBEHAVIOR=hsa`) and restart the server to parse the section; `run_experiments` emits this hint when a failed run matches the pattern. - `.param` inside subcircuits is local scope (masks globals). Nesting up to 10 levels. - Subcircuit and model names are global — must be unique across the entire netlist. ### .save Directive ```spice .save V(out) I(Vin) $ save only these signals .save @m1[id] @m1[gm] $ save internal device parameters .save all @m2[vdsat] $ save defaults plus extras ``` - Without `.save`, all node voltages and source currents are saved (can create huge files). - Adding even one `.save` line drops all defaults — only listed signals are saved. - To keep defaults plus extras: `.save all @m2[vdsat]` - `.save @r1[i]` for resistor current (not available via `I()` syntax). - **Read internals back as named numbers** (no rawfile parsing, no `.control`): on a `.dc`/`.tran` sweep, an `analyze_results` `waveform` recipe over `['m1.gm','m1.id']` gives the gm/ID table in one call; a `value` recipe (`expr='m1.gm', at=...`) reads one point; `operating_point(device='M1')` gives the bias snapshot of one device. Address an internal by the `m1.gm` shorthand or the literal `@m1[gm]` (the tools resolve the `v()`/`i()` wrapping and subcircuit paths). This `.dc` + `.save` + read sequence is how to build a gm/ID characterization table; see the `spice://guide` resource. ### .control / .endc Blocks ngspice has a built-in scripting language for post-simulation analysis: ```spice .control run $ execute the simulation plot V(out) $ plot results print V(out) $ print to stdout let vmax = maximum(V(out)) $ create vector set filename = "results.csv" $ create string variable write $filename V(out) I(Vin) $ save to rawfile wrdata output.txt V(out) $ save as CSV-like text .endc ``` **Scripts without `write`/`wrdata`.** A `.control` block replaces ngspice's default raw output: the script runs instead of the `-r rawfile` write, so a script with no `write`/`wrdata` produces no rawfile for the analysis tools even though the run completes. When the deck has exactly one `.control` block and no `write`/`wrdata` anywhere, `run_experiments` inserts a `write ` just before `.endc`, so results still reach the `waveform`/`signal_stats` recipes. That inserted line is a bare `write` and captures only the current/last plot. A script that runs several analyses, or writes per iteration inside a Monte Carlo loop (see below), needs its own `write`/`wrdata` for each. If the script already contains any `write`/`wrdata`, nothing is inserted. **Variables vs vectors — a critical distinction:** - `set` creates string/shell variables: `set myvar = "hello"` — access with `$myvar` - `let` creates numeric vectors: `let x = 2*pi` — access with `$&x` to convert to number - Mixing them up causes silent failures. - `$¶m` dereferences a circuit `.param` into a control variable. **Control structures:** ```spice $ While loop while condition ... end $ Repeat repeat 10 ... end $ Foreach foreach val 1 2 3 4 5 echo value is $val end $ If/else if condition ... else ... end $ Also: dowhile, break [n], continue [n], label, goto ``` `foreach` values are space-separated (no commas). Can use variable expansion: `foreach var $myvariable`. **Key commands:** `run`, `plot`, `print`, `let`, `set`, `write`, `wrdata`, `alter`, `altermod`, `echo`, `meas`, `linearize`, `fft`, `define`, `source` ### Monte Carlo ngspice has **no `.mc` directive**. Monte Carlo is done via `.control` block loops: ```spice .control define unif(nom, var) (nom + nom*var * sunif(0)) define gauss(nom, var, sig) (nom + nom*var/sig * sgauss(0)) let mc_runs = 100 let run = 1 dowhile run <= mc_runs alter c1 = unif(1e-09, 0.1) alter r1 = gauss(10k, 0.05, 3) tran 1u 1m $ ... store/process results ... let run = run + 1 end .endc ``` **Random functions:** - `sunif(0)` — single uniform random number in [-1, 1] - `sgauss(0)` — single Gaussian random number (mean=0, stddev=1) - `.options seed=` or `seed=random` — set random seed **Statistical functions (.param context):** - `gauss(nom, rvar, sigma)` — Gaussian, relative variation - `agauss(nom, avar, sigma)` — Gaussian, absolute variation - `unif(nom, rvar)` — uniform, relative - `aunif(nom, avar)` — uniform, absolute - `limit(nom, avar)` — binary: nom+avar or nom-avar Using `.param` statistical functions requires multiple ngspice runs (each run re-evaluates). Using `.control` loops with `alter` varies within a single run. ### .options Flags **General:** | Flag | Effect | |-|-| | `SEED=val\|random` | Random number seed | | `TEMP=x` | Operating temperature (default 27C) | | `TNOM=x` | Nominal temperature (default 27C) | | `SAVECURRENTS` | Auto-save all device terminal currents | | `KLU` | Use KLU matrix solver (faster for large MOS circuits) | | `INTERP` | Interpolate output to fixed TSTEP grid | **Convergence:** | Flag | Default | Effect | |-|-|-| | `RELTOL` | 0.001 | Relative tolerance | | `ABSTOL` | 1e-12 | Absolute current tolerance | | `VNTOL` | 1e-6 | Absolute voltage tolerance | | `GMIN` | 1e-12 | Minimum junction conductance | | `ITL1` | 100 | DC iteration limit | | `ITL4` | 10 | Transient iteration limit | | `METHOD` | trap | Integration method: `trap` or `gear` | | `MAXORD` | 2 | Max integration order for Gear (2-6) | | `TRTOL` | 7 | Transient error tolerance factor | | `XMU` | 0.5 | Trapezoidal damping (reduce slightly to suppress ringing) | **Matrix conditioning:** ```spice .options rshunt=1e12 $ resistor from every node to ground .options rseries=1e-4 $ series resistor on every inductor .options cshunt=1e-13 $ capacitor from every node to ground ``` Use `rshunt` for "no DC path to ground" errors. Use `rseries` when inductors parallel voltage sources cause OP failure. Use `cshunt` for oscillation/noise issues. `AUTOSTOP` — stops transient analysis after all `.meas` conditions are satisfied. ### XSPICE Mixed-signal simulation with code models. A-devices (the `A` prefix) are the XSPICE code-model primitives, and XSPICE is enabled by default in the official/stock ngspice builds — no custom build needed. Only the experimental `XSPICE_EXP` extras (e.g. the capacitor/inductor code models) require a custom build. ```spice A1 [in] [out] lut1 .model lut1 d_lut(rise_delay=1n fall_delay=2n input_load=0.5p + table_values="0110") ``` Digital device types: `d_and`, `d_or`, `d_nand`, `d_nor`, `d_xor`, `d_inverter`, `d_buffer`, `d_flop`, `d_latch`, `d_lut`, etc. Digital nodes use `[name]` bracket syntax for buses. ### Key Differences from LTspice - **Inline comments**: `$` not `;` - **Conditional in B source**: ternary `?:` not `IF()` - **MOSFET bulk terminal**: required (4 pins), not auto-connected - **GND node**: must explicitly tie to 0 or use `.global` - No `startup` keyword in `.tran` - A-devices are the XSPICE code-model primitives (the `A` prefix) — available in stock/official builds (XSPICE enabled by default); only `XSPICE_EXP` extras need a custom build - No Unicode mu issue — ngspice preserves `u` as-is - `.func` definitions cannot be recursive — causes hang, not error - Different `.raw` file format (all doubles vs LTspice mixed precision) - `.backanno` is LTspice-only — ngspice rejects it (`unimplemented dot command '.backanno'`) and aborts the run. Probe currents with `.options savecurrents` (or `.probe`) instead