Overview#
SPICE (Simulation Program with Integrated Circuit Emphasis) solves circuit equations numerically. Rather than building hardware, you can check that a voltage divider gives the expected voltage, an RC filter has the right cutoff, or a transistor stage biases correctly. Fusion Electronics includes a copy of ngspice (an open-source mixed-level, mixed-signal simulator based on Berkeley spice3f5) that you run from the schematic. Whether it is available on Personal use is not stated in Autodesk's help (see the availability section).
Where to find it#
- On the Schematic Design toolbar: Simulate (runs the analysis), Simulate > Add Model, Simulate > Analog Source Setup, Simulate > Digital Source Setup, Voltage Probe and Phase Probe.
- Every component must be mapped to a SPICE model (primitive or model-based). The supplied libraries ngspice-simulation and ngspice-digital are pre-mapped; in a library, Add Model on the Component toolbar maps a model file (
.mdl).
Step by step#
- Build a simple schematic from ngspice-simulation and ngspice-digital library parts and assign values.
- Add probes: a Voltage Probe (or Phase Probe for AC sweeps) at the nodes you want; current probes are AMMETER parts from ngspice-simulation placed in line.
- Add Model. Select the circuit and click Simulate > Add Model; answer Yes to convert GND parts to SPICE ground. Green check marks in the Done column mean mapped; an alert icon with a Map button marks unmapped parts.
- Set up sources with Analog Source Setup (DC value, AC value, optional transient function) or Digital Source Setup (Time/value table or CSV).
- Choose an analysis in the SIMULATION dialog: Operating Point, DC Sweep, AC Sweep or Transient.
- Click Simulate; graphs appear (the gear icon switches the frequency display between logarithmic and linear).
- Iterate. Adjust component values, rerun, and update the schematic.
Options reference#
| Analysis | What it computes | Typical use |
|---|---|---|
| Operating Point | Voltages and currents at all nodes; no options | Biasing and startup check |
| DC Sweep | Vary one independent voltage or current source between start and end values | Transfer curves |
| AC Sweep | Frequency response; Dec (decade, log) or Lin scale, start and end frequency | Filters, amplifiers |
| Transient | Time domain; Start and End time; TMAX optional maximum time step | Power-up, switching, RC charging |
Autodesk lists exactly these four SPICE simulation types; noise, Fourier and Monte Carlo analyses are not documented. For AC, DC and Transient set Points (Autodesk suggests 200 to 500) and Max points (1000).
Tips and pitfalls#
Warning: A simulation is only as accurate as its models. Idealized models hide real-world effects like switching losses, saturation and parasitics.
Tip: Start small. Simulate one stage, not the whole board.
Warning: Convergence errors usually mean a floating node, a missing ground, an ideal switch with no series resistance, or a loop of ideal sources. Add small series resistance or initial conditions.
Tip: Pick time step and stop time based on the fastest event you want to see. Too coarse hides oscillation, too fine wastes time.
Warning: If simulation is unavailable on your plan, an external SPICE tool is an option (general guidance); Fusion can export a netlist with
EXPORT NETLIST, but Autodesk's pages do not describe a SPICE-format export.
Tip: Keep a copy of the exact model files with the project; library updates can change behavior.
Practice exercise#
Simulate an RC low-pass filter with R = 1 kOhm and C = 100 nF. Run an AC analysis from 10 Hz to 1 MHz. The -3 dB point should be near 1.6 kHz (1 / (2 pi R C)). Then run a transient with a 1 kHz square wave and compare the rise and fall time to the time constant of 100 microseconds.
Availability and plan notes#
Autodesk's Electronics workflow page says Fusion Electronics provides access to a SPICE simulator and that a Signal Integrity extension is available for more advanced uses. The Extensions pages now state the Signal Integrity Extension is no longer available for new purchases or trial. Electronics cooling is part of the Simulation Extension (it simulates board temperature in the 3D model). Whether SPICE runs on Personal use is not stated in Autodesk's help mirror, so try an operating-point run on a voltage divider before planning a project around it.
Worked example: a voltage divider and an operating point#
A 5 V source feeds R1 = 10 kohm in series with R2 = 4.7 kohm to ground, loading a 100 kohm ADC input.
- Without the load, Vout = 5 x 4.7 / (10 + 4.7) = 1.599 V.
- With a 100 kohm load in parallel with R2, R2' = 4.7 x 100 / (4.7 + 100) = 4.489 kohm, so Vout = 5 x 4.489 / (10 + 4.489) = 1.549 V.
- Run an operating-point analysis. The simulated node voltage should match step 2 to three digits; a mismatch means a wrong value, a missing ground, or a source not set to 5 V.
- Compute the error: 1.599 - 1.549 = 0.050 V, or 3.1 percent. Decide whether that matters for your ADC.
Worked example: RC filter in the frequency and time domains#
R = 1 kohm, C = 100 nF. Cutoff f = 1 / (2 x pi x R x C) = 1 / (2 x 3.1416 x 1000 x 100e-9) = 1591.5 Hz.
| Analysis | Setup | Expected result |
|---|---|---|
| AC sweep (Dec) | 10 Hz to 1 MHz, 1 V AC source (set via Analog Source Setup) | -3.01 dB at 1.59 kHz; phase -45 degrees there; roll-off 20 dB per decade above |
| Transient | 1 kHz square wave 0 to 5 V, End time 5 ms, TMAX 5 us | 63 percent rise (3.16 V) after one time constant of 100 us; reaches 99 percent after about 460 us |
| Transient (fast) | 10 kHz square wave | Output no longer reaches 5 V because the half period (50 us) is shorter than tau (100 us); peak-to-peak is about 1.2 V |
For a 10 kHz, 0 to 5 V square wave the steady-state output swings between roughly 1.9 V and 3.1 V around the 2.5 V average. Checking a result you can predict is the quickest way to find whether your setup is right.
Choosing time step and stop time#
| Event you want to see | Rule of thumb |
|---|---|
| Rise time of a logic edge | Max step at most one tenth of the rise time |
| RC or RL transient | Stop at five time constants; step at tau / 50 |
| Power-up of a regulator | Stop long enough to include soft-start (for example 5 ms) |
| Oscillator at frequency f | Step at most 1 / (50 f); stop after at least 10 cycles |
| PWM at 100 kHz | Step 100 ns; stop 200 us for 20 cycles |
Large simulations with a small step and long stop time can take minutes; split the work into stages.
Preparing parts and models#
| Part type | What is needed | Pitfall |
|---|---|---|
| R, C, L | Value only | Capacitors get ideal behavior; add ESR for a realistic ripple |
| Diodes and transistors | A SPICE model mapped with Add Model | Unmapped parts cannot be simulated |
| Op-amps and ICs | Manufacturer model file, loaded with MAP > Load Model | Map the component pins to the model inputs one by one |
| Sources | Type and parameters | Missing amplitude is a common cause of "no output" |
| Ground | Convert GND parts to SPICE ground when prompted | Exactly one reference (general SPICE practice) |
When you import a vendor SPICE model, read the first lines of the file: the .subckt line lists the node order (general SPICE practice). Map those nodes to the component pins one by one. A swapped input pair on an op-amp produces positive feedback and a flat, saturated output.
Convergence problems#
| Symptom | Likely cause | Fix |
|---|---|---|
| "Singular matrix" or "no DC path to ground" | Floating node (a capacitor-only connection) | Add a large resistor (1 Mohm) to ground |
| "Timestep too small" | Ideal switch with zero on-resistance, or unrealistic edges | Add 1 mohm series resistance; use an edge rise time |
| Voltage-source loop | Two ideal sources in parallel | Insert a small resistance |
| Output stuck at one rail | Wrong feedback polarity | Check op-amp pin order |
| Transient takes forever | Step too small for the stop time | Increase max step or reduce stop time |
Using external SPICE and exports#
If SPICE is not available to you, a general alternative is an external simulator such as ngspice or LTspice. Autodesk's pages do not describe exporting a SPICE-format netlist, so this is not confirmed.
Practice exercise#
Verify two circuits by hand and by simulation.
-
Build the divider example (5 V, 10 kohm, 4.7 kohm, 100 kohm load) from ngspice-simulation parts with a Voltage Probe. Predict 1.549 V, run an Operating Point, and write the difference.
-
Build the RC filter (1 kohm, 100 nF). Run the AC sweep and read the -3 dB frequency with a cursor; it should be within 2 percent of 1.59 kHz.
-
Run a transient with a 1 kHz square wave and measure the time to reach 63 percent; expect about 100 us.
-
Change C to 10 nF and predict the new cutoff (15.9 kHz) before simulating.
-
Remove the ground connection on purpose and note the error message; restore it.
-
Save screenshots with parameter values in the project notes.
-
Record the model file names and versions used, so the same results can be reproduced when the project is reopened months later.
Related#
- Schematic Capture
- Libraries, Symbols, Footprints and Devices
- Electronics Limits in Personal Use