Computer-aided design systems for electrical circuits. Automated design of electrical devices in a CAD environment

Goal of the work

Master the capabilities of the PCAD 2001 computer-aided design system in the field of creating electrical circuit diagrams.

Progress

The design of the electrical circuit diagram was carried out in the computer-aided design system PCAD 2001.

During the design of the electrical circuit diagram, the PCAD Schematic program was used.

BUILDING A SCHEME DRAWING

The construction of an electrical circuit diagram is carried out using a mouse manipulator moved along the horizontal surface of the desktop; at the same time, the cursor in the form of a cross moves synchronously on the display screen. A convenient feature of using the mouse in the PCAD 2001 environment is the availability of functions for scrolling and scaling the diagram.

CREATE A SCHEME

Schemes are constructed from symbols. Creating a diagram is the process of visually placing components on a workspace and connecting them to each other.

You can also create a drawing file containing graphic information, which can be used to obtain a circuit drawing. The placement of components is set using the Insert / Component command. In this case, the system opens the active library, which contains UGO components.

The library manager, Library Executive, is responsible for creating component libraries in P-CAD 2001. The P-CAD 2001 system has the ability to create integrated component libraries. Three types of data are entered into such a library: text information about components (components), UGO (symbols) and images of component bodies (patterns). The graphics of housings and UGOs are created in the graphic editors P-CAD Schematic and P-CAD PCB or in special editors Symbol Editor and Pattern Editor. The last two are similar to the schematic editors and printed circuit boards, in the set of commands only those commands that are necessary for creating UGO and component designs are left, and the so-called masters of samples and symbols are added. Another important feature of the Symbol Editor and Pattern Editor is the ability to directly edit UGO/component designs. In addition, Library Executive includes commands for searching components in libraries using a given set of attributes.

After selecting a component, you should place it on the workspace. In this case, you can control the orientation of the element, set the mirror mode, etc.

After installing an element, it is possible to reproduce it using the copy / paste command from the clipboard.

To make connections, use the insert/wire command. When conducting, the initial and end point. Unconnected contacts of microcircuits are marked with a diagonal cross. To connect two nets, you need to make them global and then assign identical names by connecting them to the bus.

To designate elements, use the properties command from the context menu (activated by right-clicking on the corresponding element). Next, its designation is given.

Saving data to a file and loading from a file is carried out using commands from the File menu. The diagram is saved in the PCAD 2001 system format and has the sch extension.

Conclusion: In the course of the work done, the PCAD 2001 Schematic program was mastered, which is part of the PCAD 2001 CAD system and is intended for constructing electrical circuit diagrams.

Entering the electrical circuit diagram

In this section on simple example techniques for placing components, conductors, busbars, etc. on the UGO diagram are considered. Shows how to create a multi-page diagram.

Creating a Multi-Page Project

For the sake of generality of presentation, we will immediately create a multi-page project in which the basic electrical circuit will be placed on several sheets of A4 format.

Create a two-page project

1) Launch the schematic editor and load the Schematic.sch Settings template into it.

3) Activate the Option/Configure… command

4) In the Option Configure panel, in the Title Sheets frame, click the Edit Title Sheets... button (editing page design).

5) In the Option Sheets panel (see Fig. 6−1), open the Sheets tab and in the Sheet Name window type Sheet2. Click the Add button. The new name will appear in the Sheets: (pages) window.

Rice. 6−1. Adding a second page to the project

The purpose of the remaining buttons on this page is given in Table 6−1

Design the pages in formats in accordance with the ESKD

1) In the Option Sheets panel, go to the Titles tab.

2) Select the first page Sheet1 from the list, as shown in Fig. 6−2.

Rice. 6−2. Design of the project in formats

3) Check the Custom checkbox and click the Select button.

4) Using the standard Windows dialog, find and open the file A4_1_list.ttl on the disk, created when performing section 4.

5) On the Options Sheets panel (Fig. 6−2), click the Modify button to changes made came into force.

6) In the Sheets window of the Options Sheets panel, click on the first line of the list - Global.

7) Press the Select button and load the file of the second sheet of A4_2_sheet.ttl format from the catalog.

8) Click the Modify button again.

9) Click the Close button on the Options Sheets panel and the OK button on the Option Configure panel to complete the page design.

Fill out drawing title blocks with project information

1) Indicate the name of the project, its decimal number, developer, reviewer, approver and other necessary information. Working with the Field tab of the Design Info panel was discussed in detail in subsection 4.6.

2) Apply the text inscription Electrical circuit diagram on the format of the first sheet, as shown in Fig. 4−22.

Make sure the second page of the project is formatted correctly

1) In the status bar at the bottom of the screen (see Fig. 6−3) in the Select Sheets window, use the button to expand the list of pages and select the second page in it - Sheet2.

Rice. 6−3. Switching pages

2) An image of the second page will appear on the screen, designed approximately as shown in Fig. 6−4.

Rice. 6−4. Design of a stamp on the second page of the project

3) Save the project to disk by clicking .

The multi-page project has been completed.

Connecting libraries

Before entering and placing components on the diagram, you need to connect libraries with the necessary elements to the project and disable unnecessary ones. How to do this is described in detail in subsection 5.2.

Make sure that the library My library.lib is connected to the project

1) Select the Library/Setup command from the menu.

2) In the Library Setup panel that appears, view the list of connected libraries.

Entering and placing library component symbols on a diagram

The diagram of the first stage of the transistor amplifier, placed on the first sheet of the project, is shown in Fig. 6−5.

Rice. 6−5. Circuit diagram of the first amplifier stage

Select from the library and place resistors on the drawing

1) Set the grid spacing to 5mm.

2) Activate the Place/Part command (button on the toolbar) and left-click on the drawing field.

3) In the Place Part panel that opens (Fig. 6−6), select one of the connected libraries from the drop-down list in the Library window (in in this case– My Library.lib) and click the Browse button to display the graphics of the selected component in a separate window.

Rice. 6−6. Selecting an item from the library

4) In the Name Component list window, find the name of the resistor with a dissipation power of 0.25 W - R250 and left-click on it.

5) In the RefDes window, set the initial value for the positional designation of resistors R1, and in the Value window, specify its value - 100k. Click OK to complete your selection.

6) On the drawing field, click the left mouse button and, without releasing it, move the element to the location of the resistor R1 in the drawing. To rotate a component, use the R key. Release the left mouse button.

7) Repeat step 6 to place resistors R2−R4 on the drawing. The positional designations of placed elements will increase automatically.

8) To finish entering resistors, click right click mice.

Select and place the remaining circuit elements on the drawing

1) Left-click on the drawing again and select capacitor C from the list.

2) Set the initial value for the reference designator - C1 and set the nominal value - 0.01 µF.

3) Place three capacitors on the drawing as shown in Fig. 6−5.

4) Place the transistor on the drawing (don't forget to assign it a positional designation), ground symbols and input contacts.

Adjust the relative position of elements on the diagram, the location and value of their attributes

2) Click on the element position or attribute value you want to change to highlight it.

3) To move a component, click the left mouse button inside the selection rectangle and drag it by the anchor point to the desired location.

4) To change attributes (value or designation), right-click inside the selection rectangle and select Properties from the drop-down menu.

5) To select not the entire component, but its individual attributes, you must press the SHIFT key (or CTRL depending on the position of the CTRL/Shift Behavior switch in the Mouse tab of the Option Preferences panel) and, without releasing it, click on the attribute with the left mouse button.

6) Moving and editing the properties of the selected attribute is also done as for the element as a whole. You can also use the R key to rotate the selected attribute.

Before editing the position of the attributes, set the grid spacing to a finer size, for example 1 mm. You can cycle through grid steps without leaving the current command using the G key

Input of group communication lines (buses)

To facilitate working with drawings, group communication lines (buses) are often used in diagrams. Since in the P-CAD system the conductors connected to these lines acquire the right type automatically, group communication lines must be placed on the drawing before connecting the elements with wires.

Draw on the drawing the group communication line BUS_1

1) Select the Place/Bus command from the menu or click the button on the toolbar.

2) Using the O key, set the orthogonal line drawing mode (there should be an inscription on the right side of the status line) if the tire should not have kinks. Set the grid pitch to 5 mm.

3) Point the cursor to the beginning of the line and click the left mouse button. Without releasing it, drag the cursor to the end of the bus. Release the left mouse button.

4) Right-click to “break” the line.

Give the input bus a name and display it in the drawing

1) Go to object selection mode (button pressed)

2) Left-click on a group link to highlight it.

5) On the Bus Properties panel in the Bus Name window, type BUS_1 (see Fig. 6−7)

Rice. 6−7. Setting a bus name

6) Check the Display check box to display the name on the drawing, and click OK to finish setting the bus properties.

Change the position of the bus name

1) Set the grid pitch to 1 mm

2) Press and hold the SHIFT key and left-click on the bus name to highlight it.

3) Click the left mouse button inside the selection rectangle and, without releasing it, drag the bus name to the desired location on the drawing.

4) Release the left mouse button.

Connecting component pins with conductors

Connect input connectors X1, X2 and capacitor C1 to BUS_1

1) Set the style of connecting conductors to the bus using the Option/Display command (see Fig. 6−8).

Rice. 6−8. Selecting a Tire Style

2) Select the Place/Wire command from the menu or click the button on the toolbar.

3) Use the O key to set the orthogonal line drawing mode. Set the grid pitch to 5 mm.

4) Left-click on the yellow square at the end of the X1 element.

5) Move the cursor horizontally to the bus and left-click on it. The wire will “break” automatically.

5) Repeat paragraphs. 4−5 for elements X2 and C1.

Connect connectors X3 and X4 to each other and the ground symbol

1) Consistently click the left mouse button on the yellow squares at the end of the pins of elements X3, X4 and ground. They will be connected by a conductor.

2) Right-click for “wire break.”

Enter the remaining conductors in the diagram

To move around the drawing, use the scroll bars, to change the scale, use the “+” and “-” keys on the main and additional keyboards.

Do not forget to “break” the conductors.

The last entered chain segment can be deleted using the BACKSPACE key.

Naming Nets

By default, the system names nets in the format NET00006, numbering them sequentially. If necessary, you can rename the circuit by specifying any other name. Meaningful net names can be useful later in your project.

Change the name of the net connected to the base of the transistor

1) Go to object selection mode (button pressed)

2) Left-click on the circuit segment connected to the base of transistor VT1.

3) Right-click to bring up the drop-down menu.

4) Select the Properties command from the drop-down menu.

5) In the Wire Properties panel, in the Wire tab, check the Display checkbox to display the net name on the diagram.

6) On the Net tab in the Net Name entry window, type BASE (see Fig. 6−9) and click OK to end the dialog.

Rice. 6−9. Naming a circuit

This name will automatically be assigned to all segments of this circuit. Note that this approach does not allow combining segments of the same chain that do not have “physical” contact with each other, for example, located on different pages.

To connect circuits with segments spaced apart in the drawing, special elements are used - ports.

Name the circuit using the port

1) Select the Place/Port command from the menu or click the button on the toolbar.

2) On the Place Port panel in the Net Name input window, enter +12V (see Fig. 6−10).

Rice. 6−10. Setting port properties

3) In the Pin Cont frame, check the One Pin checkbox.

4) In the Pin Length frame, select the Short checkbox.

5) In the Pin Orientation box, select the Vertical checkbox.

6) In the Port Shape frame, click on the (None) button - no frame.

7) Click OK to end the dialog.

8) Left-click on the top net near where it connects to the bus. Port images will appear.

9) Left-click on the net connected to component X1 to give it the same name.

10) First right-click to reset the command parameters, and then, placing the cursor in an area unoccupied by elements, left-click to open the Place Port panel.

11) Repeat paragraphs. 2−10 to assign global names to the remaining nets.

Applying text inscriptions to the diagram

Often there are explanatory notes on the diagrams. The sequence of work on placing texts on the drawing is discussed in detail in subsection 4.2.

Design of the second sheet of the diagram

On the second page we will draw the second amplifier stage.

Copying schematic fragments

The P-CAD system allows you to copy drawing elements and transfer them from page to page (and from project to project!) via the Windows clipboard. In this case, the component designations change automatically.

Copy part of the drawing on the first sheet and transfer it to the second

1) Go to the object selection mode (the button is pressed).

2) Select with a window the part of the drawing to the right of the BUS_1 bus.

3) Press CTRL/C (Edit/Copy command) – copy to the clipboard.

4) Go to the second page using the page switcher in the status line (or press the key with the letter L - page forward; SHIFT/L - back).

5) Press CTRL/V (Edit/Past command) – paste from the clipboard.

6) Press the left mouse button and, without releasing it, position the drawing fragment in the center of the sheet.

On the second sheet a diagram of the second amplifier stage should appear in the form shown in Fig. 6−11.

Rice. 6−11. Diagram on the second sheet after copying from the clipboard

Editing a diagram

Remove unnecessary components from the circuit

1) Click on the input capacitor C4 with the left mouse button to highlight it and press the DELETE key.

2) Similarly, remove the Input and Output ports, the input circuit segment and the final +12V circuit segment.

3) Remove the net name NET00012. To select a name, left-click on it while pressing the SHIFT key.

Edit some schema elements

1) Click on the initial segment of the input circuit with the left mouse button to select it.

2) Point the cursor to the right end of the selected segment, press the left mouse button and stretch the conductor until it aligns with the right edge of the +12V circuit.

3) If necessary, move the +12V port to the right.

Add components to the second sheet

1) Press the letter L key to go to the first sheet

2) Click on element X1 with the left mouse button to select it.

3) Copy it to the clipboard (CTRL/C).

4) Return to the second sheet and paste the element from the buffer into the diagram (CTRL/V). Place it in the output circuit of the cascade.

5) Name the input circuit of the stage OUTPUT using the Place/Port command. The chain name can be selected from the drop-down list.

Positioning designations

From Fig. 6−11 it is clear that the positional designations of some elements are assigned incorrectly (the order is broken - left-to-right, top-to-bottom). You can change them manually or automatically. Manually - through the properties of the elements.

Change component tags automatically

1) Enter the Utils/Renumber command.

2) On the Utils Renumber panel (Fig. 6−12) in the Type frame, select the RefDes checkbox.

Rice. 6−12. Relabeling options

3) In the Direction frame, the direction of redesignation is set – top to bottom (Top to Bottom) or left to right (Left to Right). Let's choose the second one.

4) In the RefDes frame, it is determined whether all sections will be used in multi-section components (Auto Group Parts checkbox) or whether the number of used sections specified by the developer will remain in each case (Keep Parts Together checkbox). If you choose the first option, the number of multi-part components used may be reduced.

5) In the Starting Number and Increment Value windows, the starting position designation and number increment are set, respectively.

6) Set the parameter values ​​as shown in Fig. 6−12 and click OK.

The system will warn you that this operation cannot be cancelled. You can cancel it or continue. Click OK.

The result of working on the second sheet of the diagram is shown in Fig. 6−13.

Rice. 6−13. Scheme on the second sheet after editing

Save the project file with the same name.

Arranging Page Connectors

To make it easier to work with complex diagrams that occupy several sheets of large formats, the P-CAD system provides special elements - Sheet Connectors, which automatically display information about which sheets and in which areas of the drawing there is a continuation of a particular circuit.

Arrange page connectors in the diagram

1) Connect the Demo.lib library supplied with the P-CAD system to the project. It is located in the \P-CAD 2001\Demo directory (Library/Setup command).

2) Find in this library and place the SHEETOUT components on the first and second sheets of the circuit, connecting them to the +12V and OUTPUT circuits, as shown in Fig. 6−14 (Fig. 6−14,a first sheet, Fig. 6−14,b - second).

3) Edit the position of interstitial links if they overlap other elements of the image.

4) Save the project with the same name.

Lessons on P-CAD. Lesson 7, part 2

Manual and interactive routing of printed circuit boards in the PCB editor. Route/Manual command – manual routing. T-shaped routing. Route/ Interactive command – interactive routing. Route/Miter command - smoothing of conductors. Route/Fanout command – alignment of conductors. Route/Bus command – laying buses. Route/MultiTrace command – simultaneous laying of several routes. Creation of internal metallization areas. Metallized areas in signal layers. Create cutouts in fill areas. Polygons.

Lessons on P-CAD. Lesson 6

Creating components. Launch of the Library Operating System. Creating a component symbol. Setting up the Symbol Editor. Creating a symbol using the wizard. Creating a component body. Creating a component in Library Executive. Components with hidden and common leads. Creating a component with heterogeneous sections.

Creating a drawing of an electrical circuit diagram in CAD "P-CAD 2006 SP2"

Electrical diagrams are not drawn to scale. The actual location of components on the wiring field is not taken into account when drawing electrical diagrams. The selected format size of the sheet on which the diagram drawing is displayed should ensure compactness and clarity when reading the details of the diagram.

An electrical diagram shows symbols of components, electrical connections between them, text information, tables, alphanumeric symbols and basic inscriptions on the circuit format.

The lines on all diagrams of one project are made with a thickness of 0.2 to 1 mm. Connections and symbols components are made with lines of the same thickness. Thickened lines draw harnesses (common busbars). Each connection, when connected to the harness, is marked with a number or its name and must be connected at a right angle or at an angle of 45°.

After setting up the configuration of the P-CAD Schematic graphic editor and if the library contains all the component symbols contained in a given electrical diagram (current project), you can begin to create the latter. The sequence of actions is as follows:

Download the P-CAD Schematic graphic editor.

Configuring the Editor . When setting up, click the EditTitleSheets button, then in the Titles splash screen in the TitleBlock area, click the Select button, select the file with the finished format and click the Open button. Let's close all previous windows. An image of a format with fields will appear on the screen.

Let's execute the command to fill in information about the project File/DesignInfo/Fields, then sequentially highlight the necessary lines, click the Properties button and fill the Value window with the desired text in the FieldProperties splash screen. After entering each category of data, click OK. Data entered when editing the diagram:

The list of data can be expanded (Add button) or reduced (Delete button).

Current data, which is updated periodically:

Current Date - current date;

Current Time - current time;

Filename - file name;

Number of Sheets - number of sheets of the project;

Sheets Number - number of the current sheet.

Let's execute the Place/Field command. As a result, a dialog box of the same name will open, in which we select the name of the information field Title (name of the drawing) and click OK. Then place the cursor in the desired format field (the field should be sufficiently scaled) and click the mouse. Text will appear with the name of the project or current sheet if the name was previously entered using the Options/Sheets command.

Guidelines

For PCB design using

P-CAD and AutoCad.

For course and diploma design.

Annotation.

The guidelines consider the main issues of computer-aided design of printed circuit components of electronic devices, including the preparation of design documentation in accordance with ESKD standards. P-CAD and AutoCad software packages were used as automation tools.

The guidelines are intended for the implementation of course projects in the courses “Fundamentals of ES Design” in specialty 210201 and “Automation of Structural and Technological Design” in specialty 230104, as well as for diploma design in these specialties.

Introduction.

The design of a modern electronic device (ES), as is known, is organized in the form of a hierarchical multi-stage process with return operations. Since the basis of the ES design is a printed circuit board (PCB), the process of developing the PP and its result, in the form of design documentation (CD), represent one of the main components of the activity of the ES designer.

The urgent need to increase the efficiency of design design on the one hand, and the rapid development of information processing technologies on the other hand, have led to the opportunity to dramatically reduce economic and time costs through the use of new information design technologies.

In the context of the use of modern ES design technologies, the process is presented in the form of the following stages.

The first is to assign a schematic diagram of the ES to the design system. In this case, the P-CAD system, its Schematic graphic editor and element libraries.lib are used.

The next stage is usually the verification (compliance analysis) of the resulting circuit required by the assignment. (This stage is not considered in this educational work)

Next follow two closely related stages - the layout (placement) of components on the PCB and the wiring (routing) of electrical connections according to schematic diagram. It is these actions that are the most labor-intensive during “manual” design, before the introduction of automation of actions.

In this manual, the already mentioned P-CAD PCB package is used to solve such problems.

The final design stage is the preparation of design documentation in the form of two drawings:

    Part drawing (printed chamber);

    Assembly drawing of the PP, with the corresponding specification.

Experience shows that different software packages can be used for these purposes. Most often, students use the previously studied AutoCad package, therefore the guidelines consider the preparation of documents that comply with the standards of ESKD and STP MGUPI 2068752-5-06 in the AutoCad system.

In addition, the P-CAD and AutoCad complexes can be informationally combined due to the ability to export a description of the design result from P-CAD to the AutoCad system.

Further, the guidelines provide the most important information about the electrical circuit diagrams of electronic devices, the printed circuit board drawing, the PCB assembly drawing and the stages of their development using the specified software components.

1. Creation of a circuit diagram in graphic editor p-cad 2004 Schematic

To present information about an electronic device, various descriptions are used in the form of diagrams: electrical structural diagram, electrical functional diagram, connection diagram, etc.

In this case, the development of an electrical circuit diagram is considered, as it most fully describes the ES.

1.1. Electrical circuit diagram.

An important stage of ES design is to obtain a device diagram.

Electrical circuit diagram determines the complete composition of elements and connections between them, gives a detailed understanding of the principles of operation of the product and the possibility of monitoring electrical processes in it.

When drawing up a scheme in accordance with the ESKD standards, it is necessary to take into account certain rules and recommendations. Some of them are presented below.

As an example, using the existing electrical circuit diagram, let’s create a stabilizer circuit:

Elements of circuits are shown using graphic symbols established by ESKD standards.

It is recommended to record the characteristics of input and output circuits and the addresses of their external connections in tables. Tables are placed instead of conventional graphic symbols of input and output elements - connectors, boards, etc.

All product elements shown in the diagram are assigned positional designations containing information about the type of element and its serial number within this type. A positional designation usually consists of three parts that have independent semantic meaning:

    in the first part, indicate the type of element (for example: R – resistor, C – capacitor, etc.);

    in the second - the serial number of the element within a given type (for example: R1, R2, ..., C1, C2);

    in the third part it is allowed to indicate the corresponding functional purpose in the form of a letter code (for example: C1I - integrating).

Serial numbers are usually assigned counting, usually from top to bottom in a left to right direction.

Positional designations are placed next to the conventional graphic designation of the elements on the right side or above them.

All information about the elements that make up the electronic device and presented in the diagram is recorded in list of elements , which is placed on the first sheet of the diagram or performed in the form of an independent design document.

The list columns indicate the following data:

    position designation of the element;

    name of the element in accordance with the documents on the basis of which this element is applied;

    technical data of an element not contained in its name.

The element is recorded in the list in groups in alphabetical order of letter positional designations.

1.2. Basic procedures for creating an electrical circuit in Schematic p-cad.

Let us now move on to a description of the process of constructing an electrical circuit diagram of an electronic device using P-CAD Schematic.

The diagram is assembled on the working field (sheet) using the mouse and keyboard.

When building and editing diagrams, the following operations are performed:

    selecting a component from the appropriate library;

    object selection;

    moving an object;

    copying;

    deleting objects;

    connecting circuit components with conductors;

    installation of positional designations of components, etc.

Further actions are described as a set of procedures.

1) Open the program P- CAD 2004 Schematic from the Start menu or at C:\ ProgramFiles\ P- CAD 2004 Trial\ Sch. exe:

2) Set up the worksheet parameters (grid pitch and worksheet size):

Setting the sheet size: Optionsconfigure… in the Workspace Size section, set the User marker and set the size of the workspace; for example, A4 sizes: Width: 297 mm and Height: 210 mm. The transition to mm is carried out in the same menu in the Units section. Next Ok.

Setting Grid Sizes: OptionsGrids… in the Grid Spacing line, the grid spacing is set to 1.25 and added by clicking the add button. Next Ok.

Before drawing any circuit element, you need to add a library with this element to the library database Library→ setup. Then we proceed directly to the implementation of the given circuit diagram. Libraries with the necessary elements are located in the folder:

« ProgramFiles\ P- CAD 2004 Trial\ Lib\Libraries for lab-main"

These libraries contain most of the elements required for the circuit. If there are no elements in the libraries, then they should be looked for in additional libraries located in “Program Files\P-CAD 2004 Trial\Lib\Other Libraries”. Libraries can also be found on the Internet (libraries for P-Cad with the extension libraries.lib)

3) To add an element to the worksheet, click Placepart or click on the icon highlighted in the picture:

To view how the element will look in the drawing, you need to click the button “ Browse>>”

In field " Library” select the required library.

Select the required element from the list of library components, click “ OK” and place the element by pressing the left mouse button on the worksheet:

An element can be flipped by selecting it and pressing the key “ R” . To mirror an element you need to use the key “ F” .

4) To connect the elements together, you need to click Placewire

On the stabilizer diagram (example page 5) it is necessary:

    for the DA1 KR140UD60V chip, download the “k140.lib” library: PROGRAM FILES\P-CAD 2004 TRIAL\LIB\LIBRARY FOR LAB-MAIN\K140.LIB

    Let's take all resistors from the library “res.lib”

If the necessary elements are not available in the library, similar elements are used for educational design. For example, instead of the KD521V diode and the KS133A zener diode, it is allowed to use the KD521 diode and the KS133 zener diode (due to the similarity of the parameters) from the “DIOD.lib” library

Instead of the D818G zener diode, use D818ZH from the library “DIODES AND THYRISTORS.LIB”

Instead of the AL307BM LED, you can take the AL307 LED from “OPTO.LIB”

Instead of transistors KT209Zh, KT825D and KT315D, use their closest analogues from the “TRANZ.lib” library

The input and output pins are an XS component from the "KONTACT.LIB" library

We will connect all these elements together as indicated in the diagram.

5) After the circuit is assembled, we prepare it for tracing.

First, let’s fix the library of used elements by pressing the key LibraryArchiveLibrary. Let's save it, for example, on the desktop in the “pcad” folder under the name “stabilizator” stabilizer. lib”

After saving the library, the program will issue an error report. If errors were found, you should carefully read the report, correct the errors and save the libraries again. If everything is in order, then you should close the report and create a list of element connections Netlist: press Utils- GenerateNetlist, then specify the path to save the sheet “ c:\Documents and Settings\User\Desktop\pcad\stabilizer. net” , select the sheet format Tango and press « ok». That's it for working with the schematic editor. P- CADSCHEMATIC completed.

Now you can begin to solve the problem of arranging (placing) elements on the PCB and designing a set of conductors.