LTspice Export Guide

Pedal Bench's built-in simulator handles 95% of what you'll want to do. But LTspice is free, has been around forever, and has a community-maintained library of SPICE models for almost every weird transistor, op-amp, and J-FET ever used in a stompbox — including AC125s, OC44s, J201s, and other parts that are increasingly hard to source but easy to simulate.

If you're doing serious circuit research, recreating a vintage pedal, or you just want to overlay 12 frequency-response curves at once, exporting to LTspice is worth the five minutes it takes.

In Pedal Bench, open your project and go to the Netlist view. Hit Export → LTspice (.cir). The file you get back contains:

• Every component and net from your schematic.
• A header with the stock op-amp and transistor models Pedal Bench ships with (TL072, RC4558, J201, 2N3904, 1N4148, etc.).
• Sensible default simulation directives at the bottom — usually a DC operating-point analysis.

Save the file somewhere predictable; we'll add things to its directory in a moment.

LTspice can open .cir files directly: File → Open → set the filter to 'Netlists (*.cir)' → select your file. You'll see a text window, not a schematic. That's fine — LTspice simulates from the netlist text just as happily as from a graphical schematic.

If you want the picture too, run File → Convert Netlist to Schematic. LTspice will lay it out automatically; it'll look ugly the first time but you can drag parts around. Most builders skip the schematic step and just simulate the netlist directly.

Edit the .cir file's bottom lines to add the simulation you want. A few canonical directives:

• `.op` — DC operating point. Prints every node voltage.
• `.tran 10m` — transient analysis for 10 milliseconds. Use with a sine input to see clipping.
• `.ac dec 100 10 20k` — AC sweep, 100 points per decade, from 10 Hz to 20 kHz. The tone-stack tool of choice.
• `.step param Rf 1k 100k 10k` — sweep a parameter. Combine with the above to overlay multiple curves.

Hit the Run icon, and LTspice's plot pane appears. Click any node in the netlist (or, in schematic view, hover the probe over a wire) to plot it.

This is where LTspice shines. Say you want to simulate a real AC128 germanium transistor instead of a generic 2N3904. Grab an AC128.lib file from a community pedal forum or DIY site, drop it in the same folder as your .cir file, and add this line near the top of the .cir:

• `.include AC128.lib`

Then change your transistor line in the netlist from, say, `Q1 c b e 2N3904` to `Q1 c b e AC128`. Run the simulation again. Now you're seeing how that specific germanium model behaves in your circuit — leakage, low hFE, the works.

The same trick works for op-amps. Texas Instruments and Analog Devices publish .lib SPICE models for almost every op-amp they make. Drop them in, .include them, swap the model name in your X-line, done.