Simulation of radio reception in conditions of noise and interference. Encyclopedia of radio electronics and electrical engineering

Encyclopedia of radio electronics and electrical engineering / Radio amateur designer

 Comments on the article

Computer modeling is becoming an integral part of amateur radio design today, as it allows you to avoid many circuitry errors in the early stages. Of course, modeling does not solve all problems: anyway, at the final stage, prototyping and adjustment of a real device are necessary, but, most likely, serious improvement will not be required.

Despite the enormous possibilities of the programs, there are always tasks that go beyond the standard techniques described in the user manual. The author of the article proposes a non-standard approach to solving the problem of simulating the reception of radio signals under conditions of noise and interference using the PSpice system. This technique can be adapted to any simulator available to the radio amateur.

Simulation of transceiver equipment on a computer is a very difficult task. The essence of radio reception is the selection of a useful signal against the background of noise and interference. And if a separate study of the transmitter and receiver usually does not cause difficulties, then when trying to consider their joint work, the problem arises of adequately describing the signal at the receiver input, which is a mixture of a useful signal transmitted through a radio channel with interference and noise. Simulation of radio reception without interference and noise, of course, makes it possible to evaluate the performance of the device, but does not allow assessing the quality of the technical solutions used, which are inherent in radio reception.

The modeling system PSpice, included, for example, in the OrCAD v.9.2 software package, contains tools for noise analysis. However, they are intended for the small signal mode, when the elements of the device are considered linear near the operating point. In addition, only analog devices can be investigated, and only noise spectral densities can be calculated.

The proposed technique makes it possible to analyze the combined transmission of the useful signal, noise and interference in the large signal mode. Let's consider it on the example of modeling a simple remote control system with a radio channel for a car.

Obviously, one should start with studying the specific conditions of radio reception and creating a mathematical model of the interference-noise environment. In the general case, the model of a signal with interference, which comes from the antenna to the input of the radio receiver, can be represented by the following formula:

where UΣ(t) is the total mixture signal at the output of the receiver antenna; Uс(t,λс) - useful signal; λc - information parameter of the useful signal; Up(t,λp) - industrial interference signal; λp - information parameter of interference; Um(t) - white noise.

The useful signal after passing through the radio channel undergoes various distortions. We assume that the front of the signal is distorted and its amplitude decreases, which is typical for transmission over communication channels. In our case, this is sufficient, since the transmission occurs over a short distance.

Industrial interference can be very diverse, and their level is such that reception becomes completely impossible. Having eliminated intentional interference (although this topic can be very interesting for computer analysis), consider the case when the source of interference is a car. All other noise and interference will be represented as white noise.

The most powerful source of radio interference in a car is the secondary circuit of the ignition system [1; 2]. The reason for the occurrence of interference is a spark discharge in spark plugs, which results in current pulses with steep fronts, which explains the significant width of their spectrum. The pulse repetition rate, depending on the speed of the crankshaft of a four-cylinder engine, varies from about 20 to 200 Hz.

Combining everything, we get the resulting circuit (Fig. 1) of the mixture generator at the output of the receiver antenna. Thus, in order to start modeling radio reception under conditions of interference and noise, we need PSpice models of the useful signal source with distortions UС, the generator of the interference voltage envelope from the car Uon , the noise voltage source from the car Un and the voltage source of the rest of the noise Ush.

PSpice NOISE SOURCE MODEL

The scheme of the random noise generator is shown in fig. 2.

When modeling it, you should pay attention to the following:

Eout is a voltage controlled voltage source. Enter it using the name with the letter E at the beginning. It acts as a buffer and scaling amplifier. Instead, you can use the analog GAIN block, which is available in the distribution library called ABM.lib and performs similar functions;

Vnoise is a piecewise linear voltage source whose values ​​are read from an input file stored in the working directory. The voltage source VPWL_FILE has been used, which has the attribute , since the values ​​will be read from the input file. Attribute defined by entry: [pathl\pwlnoise.txt.

The directory should be the one in which all project files are saved, including schematic *.dsn files. Save the schema in a file named pwlnoise.dsn.

The source Vnoise generates a random voltage, the effective value of which is 1 V. We will call this signal "RAW" - the primary noise source (workpiece). The Rfil and Cfil elements filter the RAW signal, and Eout amplifies it to a voltage (effective value) specified by the user.

The primary noise signal V(NOISE_RAW) (Fig. 3, upper graph) is uniformly distributed in frequency. The shape factor of such a signal is approximately 1,8. The noise voltage has a triangular shape, where each corner is a discontinuity. This waveform leads to a sin(x)/x spectrum that contains harmonics extending up to very high frequencies, and the amplitude of the signal decreases with increasing frequency.

The RC filter eliminates convergence problems caused by the discontinuous nature of the raw noise signal. The filtered noise signal V(NOISE_FIL) (Fig. 3, bottom graph) is more like real noise.

RANDOM VOLTAGE GENERATION PROGRAM

The program for generating random stresses is written in the GW-BASIC language (Table 1). To type its text or make changes, it is permissible to use any text editor.

(click to enlarge)

The text of the program must be saved in ASCII codes under the name pwlnoise.bas (for example, in Microsoft Word, the program must be saved as a text file). In table. 2 provides explanations for the lines of the program.

First of all, pay special attention to line 20 of the program. In it, you need to define the path to the working directory with the project files.

After starting the program in dialog mode, you should enter three values: TIME STEP - time step in seconds - timestamps between steps in the PWL source. This parameter partially controls the bandwidth of the spectrum and the speed at which the source values ​​file is scanned. For example, if the step is reduced, random noise values ​​change faster over time, the width of the noise spectrum increases, and the speed of viewing the value file decreases; FINAL TIME - final time in seconds - time of noise generator operation. Increasing it increases the number of steps that are included in the PWL of the noise source; RMS NOISE is the effective noise voltage value in volts.

This parameter also affects the speed of viewing the file and the width of the spectrum of the noise generator: the larger it is, the greater the steepness of the front and, consequently, the width of the signal spectrum.

The program will calculate and display four parameters: Points - the number of points that will be included in the PWL noise source; Bandwidth - bandwidth at the level of -3 dB from the maximum of the spectrum envelope; Maximum Slew Rate - approximate maximum file processing speed; CFIL is the capacitance of the filter capacitor.

When all the necessary calculations are completed, the program will remind you to record the parameters TIME STEP, RMS NOISE and CFIL, which will later be needed to create a simulation task.

To take advantage of the results of the program, some preparatory work needs to be done. Enter the OrCAD Capture schematic editor, open the pwlnoise.dsn file, in which the noise source model diagram should be drawn (see Figure 2), and make the following changes.

Set the capacitance of the CFIL capacitor to the value calculated by the program.

Set the GAIN Eout attribute to the RMS value entered when the program was run. Make sure you enter a number without a dimension (gain is dimensionless). For example, you need to enter "0.125", not "0.125V".

Set the duration of the transient analysis time (TRANSIENT) to FINAL TIME, the value of which was entered when the program was executed.

You can now simulate in PSpice and use the PROBE program in the usual way. Global ports (RAW and FIL) make it easier to use the noise generator model in other parts of the circuit design that require a similar source. But don't forget to re-run the pwlnoise.bas program whenever you need to change the noise source parameters.

PSpice-MODEL OF INTERFERENCE GENERATOR

To create a model of interference from a car, an interference voltage envelope generator is needed (Fig. 4).

The shape of the envelope is a signal that sharply increases exponentially, and then also exponentially gradually decreases to zero. And it is filled with oscillations that have a random character. To obtain a signal of the desired shape, we use a pulsed voltage from the source V1, after "passing" it through the integrating circuit R1C1. By selecting the voltage amplitude and the time constant of the RC circuit, we obtain the required envelope of the interference signal (Fig. 5).

By choosing the parameters V1, V2, TD, TR TF, PW, PER of the pulse source and the time constant of the RC circuit, we set the necessary temporal characteristics of the envelope, which are inherent precisely in the interference from the car ignition system. The voltage buffer amplifier GAIN 1 is needed in order to scale the amplitude of the envelope to a value of 1 V.

Next, we multiply the voltage of the envelope signal by the voltage of the noise using the analog block MULT1 and get the desired noise signal (Fig. 5, bottom diagram). By varying the parameter PER of the pulse source V1, it is possible to simulate a change in the engine crankshaft speed, and by changing the parameter TD, the moment of occurrence of interference relative to the useful signal.

Using the proposed approach, it is easy to model many other types of industrial interference, not just automobile ones.

PSpice-MODEL OF USEFUL SIGNAL

Let us assume that the transmitter of the remote control system consists of a digital and an analog part. Pulse code is used to transmit commands. From the point of view of Pspice, such a transmitter is an ordinary digital-to-analogue device, and there are no special problems with its modeling. However, the time spent on the calculation is very high. This is because the PSpice system is forced to choose the integration step based on the rate of change of the signal with the highest frequency. Therefore, it makes sense to create a simplified high-speed model of the transmitter output signal equivalent (Fig. 6) on ideal sources.

This is much more convenient, since such a source is much easier to control (when simulating real reception conditions, it may be necessary to vary the carrier frequency, amplitude, phase). To take into account signal distortions in the radio channel, a signal shape distortion generator is added - in our case, a simple RC circuit.

PSpice - MIXTURE SIGNAL MODEL

Now that all the models are ready, let's merge them. In fact, this is the equivalent of a receiving antenna (see Fig. 1), from the output of which the total signal arrives at the input of the radio receiver. It is obvious that for the convenience of analysis in the model it is necessary to provide for the possibility of adjusting the signal-to-noise and signal-to-noise ratios, as well as the level of the total signal to simulate attenuation with increasing distance.

This is implemented using intermediate amplifiers GAIN1-GAIN4, included at the inputs and output of the adder (see Fig. 1), the gain of which can be quickly changed before the next start of the simulation.

PSpice RADIO SIMULATION

It is better to prepare a task for modeling for the TRANSIENT mode in a graphical form. To do this, instead of an antenna, I connect a mixture signal model to the radio receiver.

But before you start modeling, you need to create files of values ​​of two independent noise sources and calculate the capacitance CFIL of antialiasing filters. The pwl-noise.bas program will have to be used twice because the noise sources must be independent.

At the first start of the program, let's create the initial data for the noise source, which is part of the noise generator from the car's ignition system. Let's set, for example, TIME STEP=6E-6 FINAL TIME=0.05, RMS NOISE=1. As a result, we get CFIL=1,88 nF, and rename the generated file named pwlnoise.txt to pwlnoise2.txt.

In the second case, we write the initial data to launch the source of random noise. Set TIME STEP=5E-6 FINAL T|ME= 0 05 RMS NOISE=1 Get CFIL=1,6 nF and leave the file with the name pwlnoise.txt.

Now you can run the simulation program and see the results.

Literature

1. Maltiysky A.N., Podolsky A.G. Broadcasting receiver in a car. - M.: Communication, 1974
2. Kovalev VG Radio reception in the car. - M.: Energy, 1974.

Author: O. Petrakov, Moscow

See other articles Section Radio amateur designer.

Read and write useful comments on this article.

<< Back

Latest news of science and technology, new electronics:

A New Way to Control and Manipulate Optical Signals 05.05.2024

The modern world of science and technology is developing rapidly, and every day new methods and technologies appear that open up new prospects for us in various fields. One such innovation is the development by German scientists of a new way to control optical signals, which could lead to significant progress in the field of photonics. Recent research has allowed German scientists to create a tunable waveplate inside a fused silica waveguide. This method, based on the use of a liquid crystal layer, allows one to effectively change the polarization of light passing through a waveguide. This technological breakthrough opens up new prospects for the development of compact and efficient photonic devices capable of processing large volumes of data. The electro-optical control of polarization provided by the new method could provide the basis for a new class of integrated photonic devices. This opens up great opportunities for ... >>

Primium Seneca keyboard 05.05.2024

Keyboards are an integral part of our daily computer work. However, one of the main problems that users face is noise, especially in the case of premium models. But with the new Seneca keyboard from Norbauer & Co, that may change. Seneca is not just a keyboard, it is the result of five years of development work to create the ideal device. Every aspect of this keyboard, from acoustic properties to mechanical characteristics, has been carefully considered and balanced. One of the key features of Seneca is its silent stabilizers, which solve the noise problem common to many keyboards. In addition, the keyboard supports various key widths, making it convenient for any user. Although Seneca is not yet available for purchase, it is scheduled for release in late summer. Norbauer & Co's Seneca represents new standards in keyboard design. Her ... >>

The world's tallest astronomical observatory opened 04.05.2024

Exploring space and its mysteries is a task that attracts the attention of astronomers from all over the world. In the fresh air of the high mountains, far from city light pollution, the stars and planets reveal their secrets with greater clarity. A new page is opening in the history of astronomy with the opening of the world's highest astronomical observatory - the Atacama Observatory of the University of Tokyo. The Atacama Observatory, located at an altitude of 5640 meters above sea level, opens up new opportunities for astronomers in the study of space. This site has become the highest location for a ground-based telescope, providing researchers with a unique tool for studying infrared waves in the Universe. Although the high altitude location provides clearer skies and less interference from the atmosphere, building an observatory on a high mountain poses enormous difficulties and challenges. However, despite the difficulties, the new observatory opens up broad research prospects for astronomers. ... >>

Random news from the Archive Night lighting from living plants 22.09.2021 Bioengineers at the Massachusetts Institute of Technology (MIT) have developed eco-friendly night lighting. They say that night lights can soon be replaced by glow-in-the-dark plants. Specialists who are engaged in nanobionics made watercress, chamomile, tobacco, basil and "elephant's ear" glow. For this, a phosphor (a substance capable of absorbing energy and converting it into light radiation) was created from strontium aluminate nanoparticles. These particles formed a thin film on the leaf surface. The experiment showed that after 10 seconds of exposure to sunlight or a blue LED, the leaves could glow for an hour. They can be recharged continuously for two weeks. Moreover, this process does not violate the natural functions of plants, such as photosynthesis and water evaporation. Earlier, American scientists found that artificial night light threatens biodiversity. In particular, it confuses the fireflies and makes them unable to mate. This can take a toll on insect populations.

Other interesting news:

▪ Sound waves are the carrier of mass

▪ Found a way to fight flesh-eating bacteria

▪ Global warming asymmetry

▪ Wood is stronger than steel

▪ Microcontrollers STM32 Value Line

News feed of science and technology, new electronics

Interesting materials of the Free Technical Library:

▪ section of the site Security and safety. Article selection

▪ article Electric stoves from improvised means. Tips for the home master

▪ article How did spam exist when there were no computers? Detailed answer

▪ article Occupational injuries and their classification

▪ article Antenna Isotron for the range 14-30 MHz. Encyclopedia of radio electronics and electrical engineering

▪ article High-frequency power supply for a fluorescent lamp. Encyclopedia of radio electronics and electrical engineering

Leave your comment on this article:

All languages ​​of this page

Arabic	Hebrew	Polish
Bengali	Hindi	Portuguese
Chinese	Italian	Spanish
English	Japanese	Turkish
French	Korean	Ukrainian
German	Malay	Vietnamese

Home page | Library | Articles | Website map | Site Reviews

www.diagram.com.ua
2000-2024