FAQ: How to Model a Platinum RTD Sensor in SPICE

Introduction/Overview

KWIK (Technical Tips and Tricks) circuit application notes provide step-by-step guides to address specific design challenges. Given a set of application circuit requirements, this article shows how to address these requirements using general formulas and easily extend them to other similar application specifications. This sensor model supports SPICE simulation of the electrical and physical characteristics of a resistance temperature detector (RTD). The SPICE model uses parameters that characterize the physical behavior of the RTD, which converts temperature into resistance. It also provides a typical excitation and signal conditioning circuit that can be used to demonstrate the behavior of the RTD model.

RTD Overview

RTDs are resistive elements whose resistance changes as temperature changes. The behavior of RTDs is well understood and can be used to make precise temperature measurements with an accuracy of less than 0.1°C. RTDs are usually made of a length of wire wrapped around a ceramic or glass core, but can also be made of thick film resistors plated onto a substrate. The resistor wire used is usually platinum, but can also be nickel or copper. A common RTD is the PT100, which is made of platinum and has a resistance of 100 Ω at 0°C. Other RTD elements are available with resistances of 200, 500, 1000, and 2000 Ω at 0°C. The relationship between the resistance of a platinum RTD and temperature is described by the Callendar-Van Dusen (CVD) equation. Equation 1 describes the RTD resistance of a PT100 RTD below 0°C, and Equation 2 describes its RTD resistance above 0°C.

For T < 0:

For T > 0:

The coefficients in the Callendar-Van Dusen equation are defined by the IEC-60751 standard. R0 is the resistance of the RTD at 0°C. For a PT100 RTD, R0 is 100 Ω. For an IEC 60751 standard PT100 RTD, the coefficients are:

The resistance change of a PT100 RTD from -200°C to 850°C is shown in Figure 1.

Figure 1. PT100 RTD resistance from –200°C to 850°C

Design Description

This RTD model (Figure 2) is simulated using LTSPICE, but is also compatible with PSPICE. With this model, the user can simulate the sensor load with reference excitation current and connect the signal conditioning circuit to the RTD. This allows all common-mode, differential, and source impedance effects to be simulated. The model assumes that the RTD resistance changes with temperature. Only the nominal sensor specifications are modeled. T1 is a parameter used by the model to represent the temperature in the equations that describe the behavior of the RTD. This is different from the variable temp used in SPICE, which represents the global temperature. This approach enables the model to demonstrate the behavior of only the RTD without affecting the performance of other components in the circuit.

Design Tips/Notes

1. Use a current source to excite the sensor model. The purpose of the current source is to make the RTD resistance measurable as a voltage.

2. Connect the RTD sensor output to any high input impedance signal conditioning circuit for common mode, differential, full scale, and accuracy simulations.

3. Use SPICE parameter stepping (.step param) in conjunction with DC analysis (.op) to sweep from the minimum to the maximum temperature acting on the sensor model.

Design Steps

1. Run a SPICE simulation (using swept parameters) to confirm that the RTD output voltage is consistent with the expected output for a given temperature. Note that Vrtd = (Vrtd+) – (Vrtd-)

   
   

2. Connect the sensor model to excitation circuits and signal conditioning circuits to simulate a complete application.

Design Simulation

The simulation used a 1mA excitation current to sweep the RTD temperature from -200°C to 850°C. Table 1 shows an example of simulated and calculated values ​​(using the Callendar-Van Dusen equation) for the RTD output voltage.

Figure 2. Schematic showing RTD model and simulation parameters

Figure 3. Simulated voltage vs. temperature plot using the PT100 SPICE RTD sensor model and 1mA excitation current

The typical application circuit of the sensor model is shown in Figure 4. Vc is generated by dividing the 4.096V reference voltage. The Vc value should be selected to be within the DC common-mode range of the AD8538 operational amplifier, and when it is applied to the high-precision (0.1%) 3.01kΩ resistor, it will produce an RTD excitation current of approximately 1mA. The high loop gain set by the AD8538 forces the excitation current through the RTD model to be:

Two 499Ω resistors provide ESD protection for the input and output pins of the AD8538, 1nF capacitors are used for EMI and RFI filtering, and 2.2nF capacitors are used to ensure loop stability. The RTD output voltage is conditioned by the AD8422 instrumentation amplifier, which has a 2.21kΩ resistor placed between its RG terminals to set its gain to 9.959. This gain value is chosen to keep the output voltage of the AD8422 within the input range of the ADC, which also uses a 4.096V reference voltage. The resistors and capacitors at the input of the AD8422 serve to perform differential and common-mode filtering of the noise injected into the cable in the actual application. The resistor and capacitor values ​​for gain and filtering are selected according to the AD8422 data sheet. Figure 5 shows a plot of the simulated output voltage vs. temperature for the application circuit. Although this application circuit uses a 2-wire RTD model, it can be easily adapted to a 3-wire or 4-wire RTD model as shown in Figure 6. V1rtd and V4rtd are 0V voltage sources, which are included in the schematic so that node labels do not conflict (SPICE simulation tools do not support two different node names referring to the same node). The 0V voltage sources have no effect on the simulation results (they appear as short circuits) and help the RTD models better simulate how the RTD sensor is physically wired in an actual application. Similarly, these models can be adjusted for PT200, PT500, PT1000, and PT2000 RTDs by simply setting the R0 value in the schematic to the appropriate value (resistance at 0°C) for the desired RTD. Table 2 shows that the RTD voltage is within the required input range for linear operation of the AD8422 over temperature, and the overall output voltage of the application circuit is within the input range of the ADC using a 4.096V reference voltage. Note that the LT1461 can be used to provide this reference voltage, but it is not included in the figure for the sake of simplifying the schematic.

Figure 4. PT100 2-wire RTD application circuit showing excitation and signal conditioning circuits

Figure 5. Simulated output voltage vs. temperature for a 2-wire RTD application circuit.

Figure 6. Adjusting the 2-wire RTD model to accommodate 3-wire and 4-wire RTD applications

Design Device

References

"Practical Design Techniques for Sensor Signal Conditioning"

Edited by Walt Kester, Analog Devices, Inc., 1999, ISBN-0-916550-20-6.

Instrumentation Amplifier Diamond Plot Tool

The Diamond Plot Tool is a web application that generates a configuration-specific output voltage range versus input common-mode voltage plot, also known as a diamond plot, for ADI instrumentation amplifiers.

LTSpice® is a high-performance SPICE III simulation software, schematic capture tool, and waveform viewer with integrated enhancements and models that simplify the simulation of switching regulators, linear regulators, and signal chain circuits.

Acknowledgements

ADI's main consultants:

Tim Green, Senior Application Engineer, Linear Products Group, Precision Technology and Platforms