Application of 555 timer and OrCAD/PSpice simulation

This paper uses OrCAD/PSpice 10.5 as a tool to simulate and analyze three typical circuits composed of 555 timers, and draws some valuable conclusions.

The 555 timer is a small- to medium-sized monolithic integrated circuit that closely combines analog functions with digital (logic) functions. It has various functions and is widely used. It can form circuits such as monostable triggers, Schmitt triggers, and multivibrators by adding a few external resistors and capacitors. It is an important component for pulse waveform generation and conversion, and is widely used in signal generation and conversion, control and detection, household appliances, and electronic toys.

As one of the world's famous electronic design automation software, OrCAD/PSpice has the advantages of fast simulation speed and high precision. It can not only be used for circuit analysis and optimization design, but also can be used in conjunction with printed board design software to realize electronic design automation. It is recognized as one of the best software in general circuit simulation programs. For example: Based on this software, Essakhi et al. proposed a time domain model of microwave rectifier antenna; Du et al. proposed a method to extract S parameters from three-dimensional time domain field analysis; Zhang et al. simulated the characteristics of class E power amplifier and verified it experimentally; Sakuta et al. analyzed the characteristics of low phase noise oscillator and calculated the loaded Q value; Hayahara et al. designed a △-∑ A/D converter and simulated its signal-to-noise ratio; Brecl et al. proposed a one-dimensional and two-dimensional film model and simulated its contact resistance. These show that the software OrCAD/PSpice is a useful tool for modern electronic circuit design.


1 555 timer composition block diagram and working principle

The graphic symbol and pin diagram of the 555 timer are shown in Figure 1, where pin 1 is the common terminal, pin 2 is the trigger terminal, pin 3 is the output terminal, pin 4 is the reset terminal, pin 5 is the control voltage input terminal, pin 6 is the threshold terminal, pin 7 is the discharge terminal of the internal triode, and pin 8 is the power supply terminal.


The internal circuit block diagram of the 555 timer is shown in Figure 2. The integrated circuit consists of four parts: a resistor divider, a voltage comparator, a basic RS trigger, an output buffer, and a discharge transistor.

The reference voltage of the comparator is divided by three 5 kΩ resistors, which make the reference levels of the high-level comparator A1 in-phase comparison terminal and the low-level comparator A2 inverting input terminal 2Vcc/3 and Vcc/3 respectively. The output terminals of A1 and A2 control the RS trigger state and the discharge tube switch state. When the input signal is input and exceeds 2Vcc/3, the trigger is reset, the output terminal 3 of 555 outputs a low level, discharges at the same time, and the switch tube is turned on; when the input signal is input from pin 2 and is lower than Vcc/3, the trigger is set, the 3rd pin of 555 outputs a high level, charges at the same time, and the switch tube is turned off.

MR is the reset terminal. When it is 0, 555 outputs a low level. Usually this terminal is open or connected to Vcc.

CO is the control voltage terminal (pin 5), which usually outputs 2Vcc/3 as the reference level of comparator A1. When an input voltage is connected to pin 5, the reference level of the comparator is changed, thereby realizing another control of the output. When no external voltage is connected, a 0.01μF capacitor is usually connected to the ground to filter and eliminate external interference to ensure the stability of the reference level.

T is a discharge tube. When T is turned on, it will provide a low-resistance discharge circuit for the capacitor connected to pin 7.

2 Simulation analysis of monostable triggers

Monostable triggers are widely used in pulse shaping, delay and timing circuits. The monostable trigger has a steady state and a quasi-stable state. When there is no external trigger pulse, the circuit remains in the steady state. When there is an external trigger pulse, the circuit flips from the steady state to the quasi-stable state and outputs a rectangular pulse with a constant pulse width and amplitude. The output pulse width TW is equal to the duration of the quasi-stable state, and the duration of the quasi-stable state depends on R2 and C2. Then:


Run OrCAD/CaptureCIS, and use Schematics to draw a monostable trigger circuit composed of a 555 timer as shown in Figure 3. The input signal Vi is a pulse voltage source (VPULSE), and its parameters are set as follows:


It is worth noting that the repetition period of the input signal VPULSE must be greater than the output pulse width TW, and the pulse width of the input signal VPULSE should be less than TW to ensure that each positive and negative pulse works.

Use the transient analysis function of OrCAD/PSpice 10.5 for simulation. Transient analysis (Time Domain Transient) refers to calculating the transient response of the circuit output under the action of a given input excitation signal. Its essence is to calculate the time domain response. Set the transient analysis parameters to record data from zero to 4 ms, with a maximum step of 0.1 ms. After transient analysis, the output voltage waveform shown in Figure 4 is obtained, where the voltage across capacitor C2 is similar to a sawtooth wave, and the square wave is the voltage waveform at the output terminal Vout of 555.

As can be seen from Figure 4, capacitor C2 has an automatic charging and discharging process. When the trigger pulse arrives, the power supply Vcc charges capacitor C2 through R2. Before charging from 0 V to about 3.33 V, the output of the 555 timer always remains at a high level. Once the capacitor is charged to 3.33 V, the output of 555 immediately switches to a low level, and then capacitor C2 begins to discharge rapidly from 3.33 V to 0 V, and then a new charging and discharging process begins. Periodic rectangular pulses can be obtained at the output terminal Vout of 555, and the pulse width is about 1.09 ms, which is close to the theoretical calculated value 1.1R2C2. And the width of the output pulse is independent of the pulse width and amplitude of the input signal VPULSE.

3 Schmitt trigger simulation analysis

The Schmitt trigger composed of 555 timer connects the threshold end and the trigger end together as the input end. Run OrCAD/CaptureCIS, and the Schmitt trigger circuit composed of 555 timer drawn by Schematics is shown in Figure 5. The input signal Vi is a triangular wave voltage source (VPWL), and its parameters are set as follows:


Use the transient analysis function of PSpice for simulation, set the transient analysis parameters to record data from zero time to 3 ms, and the maximum step length is 1μs. The voltage waveform of the output terminal Uout of 555 and the input voltage waveform are shown in Figure 6.


As can be seen from Figure 6, the circuit can convert the input triangular wave into a square wave output. When the input triangular wave voltage increases and the output level changes, the corresponding threshold voltage is about 8 V, and when the input triangular wave voltage decreases and the output level changes, the corresponding threshold voltage is about 4 V, that is, the upper threshold voltage is different from the lower threshold voltage, and there is a hysteresis characteristic between the input and the output. After the input signal is replaced with a sinusoidal signal, the waveform of the input/output voltage is shown in Figure 7, which still shows hysteresis characteristics, and the upper threshold voltage and the lower threshold voltage are still 8 V and 4 V respectively, which is exactly the working characteristic of the Schmitt trigger circuit. The simulation results are consistent with the upper threshold voltage (2/3 Vcc) and the lower threshold voltage (1/3 Vcc) of the theoretical calculation results.

4 Multivibrator simulation analysis

The multivibrator is a self-excited oscillator that can automatically generate rectangular pulses without an external trigger signal after the power is turned on. Run OrCAD/Capture CIS, and the multivibrator circuit composed of a 555 timer drawn using Schematics is shown in Figure 8.


The circuit consists of a 555B chip, two resistors and two capacitors. The resistors charge and discharge the capacitor C1 to generate oscillations, thereby outputting rectangular pulses. Start the PSpice transient analysis function, observe the terminal voltage of the capacitor C1 and the voltage of the output terminal Vout of the 555, and obtain the waveform shown in Figure 9. It can be seen from Figure 9 that the output voltage Vout of the multivibrator composed of the 555 timer always remains at a high level and does not produce the expected oscillation.

4.1 Reasons why the 555 multivibrator cannot oscillate in OrCAD/PSpice

From the analysis, we can know that the reason why the 555 multivibrator in PSpice cannot oscillate is the oscillation source. The actual oscillation circuit can oscillate by itself because of the existence of the oscillation source. The oscillation source of the actual oscillation circuit is mainly composed of two factors: one is caused by the noise inside the oscillation circuit transistor and the circuit noise (resistor thermal noise, etc.); the other is caused by the surge current when the circuit is connected to the power supply. When PSpice is used directly to simulate the circuit in Figure 6, PSpice will idealize the 555 timer, resistors, capacitors, power supply and other components in the circuit and the connection process of the circuit, that is, no noise and interference can be generated in the circuit. Therefore, without an oscillation source, oscillation cannot be generated.

4.2 Effective oscillation method

After consulting relevant literature [10] and verifying it through multiple experiments, it is found that there are many ways to make the circuit oscillate. Here we introduce two of the simplest methods for your reference:

(1) Add an initial value (IC value) to the capacitor. In this example, only the IC of C1 and C2 is set to 0. The initial voltage on the capacitor only stimulates the oscillation of the oscillation circuit, does not change the output waveform after the circuit starts oscillating, and does not affect the study of the oscillation characteristics of the oscillation circuit.

(2) In the transient analysis simulation settings, activate the Skip the Initial Transient Biaspoint Calculation option and directly use the starting conditions of each component for transient analysis.

Both methods can successfully start the 555 multivibrator and continuously output pulse waveforms.

4.3 Comparison of simulation results and theoretical calculation values

​​4.3.1 Calculation index theoretical value

4.3.2 Simulation value

In OrCAD/PSpice, the rectangular pulse voltage waveform at the output end of the 555 oscillation circuit is obtained by using the start-up method of the simulated oscillation circuit proposed above, as shown in Figure 10.


As shown in Figure 10, the power supply Vcc first charges C1 through R1 and R2, so that the capacitor C1 is charged from 0 V to 2Vcc/3, then discharged from 2Vcc/3 to Vcc/3, and then charged from Vcc/3 to 2Vcc/3. The capacitor C1 forms a periodic charging and discharging process, thereby forming a periodic rectangular pulse wave at the output end Vout of 555, forming a multivibrator. As shown in Figure 10, the output rectangular pulse characteristic parameters can be obtained:


The simulation results show that the simulation values ​​of the output pulse period and duty cycle coefficient are basically consistent with the theoretical values. At the same time, it can be seen from the analysis that its value is only related to the resistance and capacitance values. The initial voltage on the capacitor only excites the oscillation of the oscillation circuit, and will not change the output waveform after the circuit starts oscillation, nor will it affect the study of the oscillation characteristics of the oscillation circuit.

5 Conclusion

OrCAD/PSpice 10.5 is used to simulate and analyze the characteristics of the monostable trigger, Schmitt trigger and multivibrator composed of the 555 timer. At the same time, the problem of the multivibrator not oscillating during the simulation process was discussed, and an effective oscillation method for the oscillation circuit was proposed. The simulation results are basically consistent with the theoretical calculated values, indicating that OrCAD/PSpice is one of the basic tools that electronic circuit designers must master.