Modeling a Photodiode in Multisim: The Direct Answer

If you are searching for a native "photodiode" component in the standard NI Multisim library that magically responds to virtual light, you will not find one. Multisim is a SPICE-based electrical simulator, not an optical physics engine. To simulate a photodiode in Multisim, you must build a behavioral SPICE equivalent model using a standard signal diode in parallel with a DC current source.

The current source represents the photocurrent ($I_{ph}$), which scales linearly with optical irradiance in the real world. In your simulation, you manually set this current value to mimic specific light levels—typically 1 µA to 100 µA for standard benchtop lighting conditions. By combining this current source with a diode to model the dark current and junction capacitance, you can accurately simulate the electrical behavior of the sensor and design your front-end amplification before ever ordering physical PCBs.

Photodiode Symbol, Pinout, and SPICE Equivalent

Before wiring the simulation, you need to understand the physical component you are mimicking. The standard schematic symbol for a photodiode is a typical PN-junction diode with two arrows pointing inward toward the junction, representing incoming photons.

The device has two pins: the Anode (A) and the Cathode (K). In physical TO-46 metal-can packages, the cathode is often tied to the metal case or marked with a flat edge on the tab. In surface-mount variants, a dot or line denotes the cathode. Photocurrent flows conventionally from the cathode to the anode when illuminated.

Building the SPICE Model in Multisim

Follow these numbered steps to construct an accurate photodiode macro-model on your Multisim schematic:

  1. Place the Junction Diode: Drop a standard fast-switching diode (like a 1N4148 or BAS316) onto the schematic. This models the PN junction, the forward voltage drop, and the non-linear junction capacitance ($C_j$).
  2. Add the Photocurrent Source: Go to Place > Sources > Signal Current Sources > DC_CURRENT. Place it in parallel with the diode. Point the arrow from the Cathode node to the Anode node. Set the value to your target simulated light level (e.g., 5 µA).
  3. Model Shunt Resistance ($R_{sh}$): Place a high-value resistor in parallel with the diode. For a standard PIN photodiode, set this to 1 GΩ. This models the reverse-bias leakage path across the depletion region.
  4. Model Series Resistance ($R_s$): Place a small resistor (typically 10 Ω to 50 Ω) in series with the Anode pin. This represents the bulk semiconductor and contact resistance, which limits high-frequency performance.
Bench Tip: If you are simulating high-speed optical communications (10 MHz+), the default SPICE model for a 1N4148 has too much junction capacitance. Swap the diode component for a BAS316 or manually edit the SPICE model parameters to lower the zero-bias junction capacitance (CJO) to around 1 pF to 5 pF.

Operation Regions and Biasing Strategies

How you bias the simulated diode dictates the circuit's performance. You must select the biasing strategy based on whether your application prioritizes precision (low noise) or speed (high bandwidth). Below is the operational breakdown to help you decide how to bias and select the topology for the job.

Table 1: Photodiode Operation Regions and Typical Parameters
Operation Mode Bias Voltage ($V_R$) Typical Current Range Bandwidth / Speed Primary Use Case
Photovoltaic (Zero Bias) 0 V pA to low nA Slow (kHz range) Precision DC light measurement, spectrophotometry, low-noise environments.
Photoconductive (Reverse Bias) -5 V to -50 V nA to mA Fast (MHz to GHz) Fiber optic receivers, LIDAR, high-speed pulse detection.
Avalanche (APD) -50 V to -200 V µA to mA (with gain) Very Fast Single-photon counting, long-range time-of-flight sensors.

In Multisim, to simulate Photoconductive mode, place a DC voltage source (e.g., -12V) connected to the Anode, while the Cathode connects to your amplifier's virtual ground. This reverse bias widens the depletion region, dropping the junction capacitance and increasing speed, at the cost of higher shot noise from the dark current.

Complete Transimpedance Amplifier (TIA) Circuit in Multisim

A photodiode outputs current, but your microcontroller's ADC reads voltage. The standard interface is a Transimpedance Amplifier (TIA). Below is a complete, stable TIA circuit you can build in Multisim using the custom photodiode model described above.

Component Selection and Values

  • Op-Amp: OPA657 (Texas Instruments). This is a FET-input op-amp with a 1.6 GHz gain-bandwidth product (GBW) and ultra-low input bias current (1 pA), making it ideal for high-impedance photodiode front-ends. You can find this in the Multisim component database under Texas Instruments op-amps.
  • Feedback Resistor ($R_f$): 1 MΩ. This sets your transimpedance gain. With 1 MΩ, an input of 1 µA yields 1V of output.
  • Feedback Capacitor ($C_f$): 1.5 pF. This is critical. Without it, the photodiode's junction capacitance interacting with $R_f$ creates a pole in the feedback loop, causing severe ringing or oscillation. $C_f$ provides pole-zero cancellation.
  • Power Supply: ±5V DC sources connected to the op-amp's V+ and V- pins.

Wiring Steps

  1. Connect the photodiode model's Cathode directly to the Inverting Input (-) of the OPA657.
  2. Connect the photodiode model's Anode to Ground (0V) for Photovoltaic mode, or to a -5V source for Photoconductive mode.
  3. Connect the Non-Inverting Input (+) of the op-amp to Ground.
  4. Place the 1 MΩ resistor and 1.5 pF capacitor in parallel with each other, routing them from the Inverting Input (-) to the Output pin of the op-amp.
  5. Attach an oscilloscope probe or a Bode plotter to the Output pin to verify stability and bandwidth.
Stability Check: Run an AC Sweep analysis in Multisim from 1 Hz to 100 MHz. If you see a massive gain peak before the rolloff, your $C_f$ value is too small. Increase it in 0.5 pF increments until the frequency response is flat or exhibits a slight Butterworth roll-off. For exact calculations, refer to the TI OPA657 datasheet and TIA application notes.

Real-World Part Selection and Multimeter Testing

When you transition from Multisim to the physical workbench, you need real components. Here are the safe default part numbers with their critical ratings for general-purpose and high-speed designs.

Safe Default Part Numbers

  • Vishay BPW34: The undisputed workhorse for visible to near-infrared (NIR) broadband detection. It features a large active area (7.5 mm²), high shunt resistance (~1 GΩ), and a responsivity of ~0.6 A/W at 900nm. Ideal for low-frequency precision and pulse-oximetry prototypes.
  • OSRAM SFH203: A high-speed PIN photodiode with an integrated daylight-blocking filter (IR pass). Junction capacitance is exceptionally low (~1 pF at 5V reverse bias), making it perfect for IR remote control receivers and high-speed data links.
  • First Sensor PIN-10D: A premium TO-5 package option for scientific instrumentation, offering extremely low dark current (< 1 nA) and high shunt resistance, optimized for zero-bias photovoltaic operation.

How Photodiodes Fail and How to Test Them

Photodiodes rarely fail catastrophically unless subjected to extreme reverse voltage breakdown or physical window damage. The most common failure mode is shunt resistance degradation caused by moisture ingress or surface contamination, which manifests as excessive low-frequency noise and DC offset drift in your TIA circuit.

Testing with a Digital Multimeter (DMM):

  1. Diode Test Mode: Set your DMM to the diode test setting. Place the red probe on the Anode and black on the Cathode. A healthy IR photodiode (like the BPW34) will show a forward voltage drop between 0.3V and 0.5V. Visible-light diodes will read closer to 0.5V - 0.7V. Reverse the probes; the meter should read OL (Over Limit). If it reads near 0V in reverse, the junction is shorted.
  2. Photovoltaic Generation Test: Set your DMM to DC millivolts (mV). Connect the probes across the Anode and Cathode (red to Anode). Shine a bright LED flashlight directly onto the sensor window. A functioning BPW34 will generate an open-circuit voltage between 100 mV and 350 mV depending on the light intensity. If it reads 0 mV under bright light, the internal bond wire is broken.

Frequently Asked Questions

How do I simulate varying light intensity in Multisim?

To simulate a changing light source (like a pulsing heartbeat signal or an optical encoder), replace the static DC_CURRENT source in your SPICE model with a PWL (Piecewise Linear) current source or an AC_CURRENT source. For a pulsing signal, use a sine wave current source with a DC offset. For example, set the DC offset to 10 µA (ambient room light) and the AC peak amplitude to 5 µA (the optical pulse). Run a Transient Analysis to watch your TIA output track the light variations in real-time.

Why is my Multisim photodiode TIA circuit oscillating in simulation?

Oscillation in a TIA simulation is almost always caused by missing or undersized feedback capacitance ($C_f$). The photodiode's junction capacitance ($C_j$) and the op-amp's input capacitance create a low-pass filter in the feedback path, introducing a 90-degree phase shift that destroys the phase margin. You must add $C_f$ in parallel with $R_f$ to introduce a zero that cancels this pole. Calculate the minimum required $C_f$ using the formula: $C_f = \sqrt{\frac{C_j}{2 \pi R_f f_{GBW}}}$. If your simulation still rings, increase $C_f$ slightly above the calculated theoretical minimum.

Can I use an LED as a photodiode in my Multisim simulation?

Electrically, an LED is just a PN junction and can act as a photodiode, generating a small photocurrent when illuminated by light of a shorter wavelength than its emission color. In Multisim, you can swap the standard diode in your macro-model with an LED symbol. However, be aware that physical LEDs have terrible responsivity (often 100x lower than a dedicated PIN photodiode), very high junction capacitance, and lack anti-reflective coatings. If you are simulating an "LED-as-sensor" hack, you must drastically reduce the value of your current source (into the nA range) and increase your TIA feedback resistor into the 10 MΩ to 100 MΩ range to get a usable voltage output.

What is the difference between a photodiode and a phototransistor in Multisim?

A photodiode is a two-terminal device that generates current linearly proportional to light, requiring an external op-amp (TIA) for amplification. It offers high speed and excellent linearity. A phototransistor is a three-terminal device (Base, Collector, Emitter) where the base current is generated by light, and the transistor's internal $h_{FE}$ (current gain) amplifies it. In Multisim, you model a phototransistor by placing a standard NPN BJT and connecting a current source to the Base pin. Phototransistors yield much higher raw output current (mA range) without needing an op-amp, but they are significantly slower (kHz bandwidth) and highly non-linear compared to photodiodes. Use a photodiode for precision and speed; use a phototransistor for simple, low-cost optical switches.