SPICE output

SPICE support in TinyCAD v4 works the same way as v3: TinyCAD generates a SPICE text file from your schematic using symbol-level templates.

What SPICE is used for

SPICE (Simulation Program with Integrated Circuit Emphasis) is a family of circuit simulation formats and tools. A SPICE simulator lets you test circuit behavior before building hardware, for example:

DC operating points and bias conditions
Transient (time-domain) behavior
AC/frequency response
Parameter sweeps and “what-if” analysis

TinyCAD does not run the simulation itself. Instead, it exports a SPICE file that you run in your chosen SPICE engine.

SPICE file format and general layout

Different SPICE engines vary slightly, but most SPICE files follow the same overall shape:

Optional header/comments
Device/model includes and definitions
Circuit element lines (one line per component instance)
Analysis/control commands
End marker (commonly .end)

In practice, this means your exported file usually has:

“Setup” text at the top (models, includes, options)
A body containing generated components and their connected nets
“Run” or analysis text at the bottom

TinyCAD’s SPICE generation is designed to map directly onto this layout.

How TinyCAD generates SPICE

TinyCAD uses a string template system on each SPICE-enabled symbol. Each symbol can define:

Model template: inserted for every instance of that component in the schematic
Prologue template: inserted near the top of the file, once per component type
Epilogue template: inserted near the bottom of the file, once per component type

Open these fields from symbol properties in the symbol library editor (SPICE tab).

Template expansion

Templates can include:

%(pin) for pin/net substitutions
$(attribute) for symbol attribute substitutions

Example model template for a resistor:

R$(refnum) %(1) %(2) $(NAME)

If the resistor instance is reference R3, connected between nets 7 and 9, with NAME=10K, TinyCAD writes:

R3 7 9 10K

refnum is handled specially so the SPICE device letter in the template is preserved.

Prologue/epilogue order and deduplication

Prologues and epilogues are deduplicated when identical
Each has a priority (0 to 9)
Prologues are written from low to high priority
Epilogues are written so priority 0 appears last in the file

This makes it possible to control where setup and analysis text appears.

Required schematic setup for SPICE export

To generate a valid SPICE file, your drawing must include:

SPICE-enabled symbols for the simulated circuit
A special RUN symbol
A net named 0 (SPICE ground)

RUN symbol

The RUN symbol is a normal TinyCAD symbol with no pins and no model template, but with prologue/epilogue text used to inject simulation control statements.

Set RUN prologue and epilogue priorities to 0 so its text appears at the very start and very end of the generated file.

Use one RUN symbol per simulation circuit.

The `0` net

SPICE requires ground to be net 0.

In TinyCAD, create this by naming a connection 0 using either:

A net label, or
A power symbol with value 0

Creating the SPICE output

After the symbols, RUN node, and 0 net are in place, generate the SPICE output from TinyCAD’s SPICE export command in the UI.

Export options are intentionally minimal because run-time behavior is expected to be controlled through your RUN symbol templates.

Advanced template conditionals

For more advanced symbols, template conditionals are supported (same behavior as v3), including tests for:

Attribute present/not present
Attribute empty/not empty
Pin connected/not connected

Conditional syntax:

?( defined(attributename), true string, false string )
?( not_defined(attributename), true string, false string )
?( empty(attributename), true string, false string )
?( not_empty(attributename), true string, false string )
?( connected(pinnumber), true string, false string )
?( not_connected(pinnumber), true string, false string )

Conditionals can be nested.

Back to Advanced
Back to v4 contents

Edit this page on GitHub