Keywords: circuit design software PROTELDXP placement components circuit design software is a commonly used software, a good circuit design software will provide great convenience for our work, and Protel DXP is such a circuit design software. In "circuit design software series tutorial (1)", we have made a corresponding introduction to the basic operation of Protel DXP circuit design software. In this article, we will detail how to place components in a Protel DXP schematic.

Please note that this tutorial is inherited from "Circuit Design Software Series Tutorial (1), Basic Operation of Protel DXP Circuit Design Software".

The first components we will place in the schematic are the two transistors, Q1 and Q2.

1. Select View > Fit Document (hotkeys V, D) from the menu to make sure your schematic is displayed in the entire window.

2. Click the Libraries tab to display the Libraries panel.

3. Q1 and Q2 are BJT transistors, click the Miscellaneous Devices.IntLib library to make it the current library.

4. Use filters to quickly locate the components you need. The default wildcard (*) will list all symbols found in the library. Type * 3904 * in the filter field under the library name to set the filter. A list of components with "3904" as the component name will be displayed.

5. Click 2N3904 in the list to select it, then click the Place button. Alternatively, you can double-click the component name.

The cursor will turn into a cross with the outline of a transistor "floating" over the cursor. Now you are in the component placement state. If you move the cursor, the transistor outline moves with it.

6. Before placing a component on the schematic, edit its properties first. While the transistor is hovering over the cursor, press the TAB key. This will open the Component Properties dialog. We are now going to set the dialog options as shown in the image below.

7. In the Properties unit of the dialog box, type Q1 in the Designator column to use its value as the first component number.

8. Next we will examine the packages used to represent the components in the PCB. In this tutorial, we have used integrated libraries that already include models for packaging and circuit simulation. Make sure that the model name BCY-W3/D4.7 is included in the model list. Leave the remaining columns as default.

Now ready to place components

1. Move the cursor (with the transistor symbol) to the left of the middle of the drawing.

2. When you are satisfied with the placement of the transistor, left click or press ENTER to place the transistor on the schematic.

3. Move the cursor, you will find that a replica of the transistor has been placed on the schematic sheet, and you are still in the component placement state with the component outline hovering over the cursor. This feature of Protel DXP allows you to place many components of the same type. Now let's put the second transistor. This transistor is the same as the previous one, so there is no need to edit its properties before placing it. Protel DXP automatically increments the number value of a component when you place a series of components. In this example, the second transistor we drop is automatically labeled Q2.

4. If you look at the schematic (Figure 1), you will find that Q2 and Q1 are mirror images. To flip the transistor hovering over the cursor, press the X key. This flips the element horizontally.

5. Move the cursor to the position to the right of Q1. To position the element more precisely, press the PAGEUP key twice to zoom in twice. Now you can see the grid lines.

6. After you have determined the position of the component, left-click or press ENTER to drop Q2. Once a duplicate of the transistor you dragged is placed on the schematic again, the next transistor will hover over the cursor ready to be placed.

7. Since we have placed all the transistors, we exit the component placement state by right-clicking the mouse or pressing the ESC key. The cursor returns to the standard arrow.

Next we are going to put four resistors ( resistors )

1. In the Libraries panel, confirm that the Miscellaneous Devices.IntLib library is current.

2. Type res1 in the filter field under the library name to set the filter.

3. Click RES1 in the Components list to select it, then click the Place button. You will now have a resistor symbol hovering over the cursor.

4. Press TAB to edit the properties of the resistor. In the Properties section of the dialog, type R1 in the Designator field to use its value as the first element number.

5. Confirm that the model named AXIAL-0.3 is included in the model list.

6. The settings for the parameter column of the resistor will be displayed in the principle and will be used by DXP when running circuit simulations later in this tutorial. The =Value rule can be used during simulation as general information about components, except for individual components. We can also set Comment to read this value, which will also reflect the Comment information in the PCB design tool. Instead of entering the value twice (in the =Value and Comment fields in the rule), DXP provides "indirect references", which replace the content of the Comment field with characters in the rule.

Click Add in the rule list cell to display the Parameter Properties dialog. Enter Value in name and 100K in value. Make sure String is selected as the rule type and the Visible box for value is checked. Click OK.

7. In the Properties section of the dialog box, click the Comment column and select =Value from the drop-down list to turn off Visible. Click the OK button to return to placement mode.

8. Press SPACEBAR to rotate the resistor 90°.

9. Place the resistor on top of the base of Q1 (see schematic in Figure 1) and left-click or press ENTER to drop the component.

10. Next put another 100K resistor R2 on top of the base of Q2.

11. The remaining two resistors, R3 and R4, have a resistance value of 1K. Press the TAB key to display the Component Properties dialog box and change the Value column to 1K (press the Edit button when Value is selected in the Parameters list). Click the OK button to close the dialog.

12. Position and place R3 and R4 as shown in the schematic in Figure 1.

13. After placing all the resistors, right-click or press ESC to exit the component placement mode

Now place two capacitors ( capacitors ):

1. The capacitive element is also in the Miscellaneous Devices.IntLib library, which should have been selected in the Libraries panel.

2. Type cap in the Component Filter field of the Libraries panel.

3. Click CAP in the component list to select it, then click the Place button. There is now a capacitor symbol hovering over your cursor.

4. Press the TAB key to edit the properties of the capacitor. In the Properties section of the Component Properties dialog, set the Designator to C1 and check that the PCB footprint model is added to the Models list as RAD-0.3.

5. The settings of the rule bar will be displayed in the schematic diagram. Click Add in the rules list to display the Parameter Properties dialog. Enter the name Value and the value 20n. Make sure String is selected as the rule type and the Visible box for value is checked. Click OK.

6. In the Properties section of the dialog box, click the Comment column and select =Value from the drop-down list to turn off Visible. Click the OK button to return to placement mode.

7. Place the two capacitors in the same way as the previous components.

8. Right-click or press ESC to exit placement mode.

The last component to be placed is the connector ( connector ), in the Miscellaneous Connectors.IntLib library.

1. The connector we want is a two-pin socket, so set the filter to *2*.

2. Select HEADER2 in the component list and click the Place button. Press TAB to edit its properties and set the Designator to Y1, check the PCB footprint model as HDR1X2. Since I will use this component as a circuit when simulating the circuit, no rule setting is required. Click OK to close the dialog.

3. Press X to flip horizontally before placing the connector. Drop the connector on the schematic.

4. Right-click or press ESC to exit placement mode.

5. Select File > Save from the menu (hotkeys F, S) to save your schematic.

Now you have placed all the components. Note the spacing between the components in Figure 2 so that there is plenty of room to connect wires to each component pin. This is important because you can't pass a wire under a lead to connect to another pin in its range. If you do this, both pins are connected to the wire.

If you need to move the component, click and drag the component body and drag the mouse to reposition it.

connection circuit

Wires serve to establish connections between the various components in your circuit. To wire in the schematic, refer to the illustration in Figure 1 and complete the following steps:

1. Make sure your schematic sheet has a good view, select View > Fit All Objects from the menu (hotkey V, F).

2. First connect the resistor R1 to the base of the transistor Q1 using the following method. Choose Place > Wire (hotkeys P, W) from the menu or click the Wire tool from the Wiring Tools toolbar to enter Wiring mode. The cursor will change to a cross shape.

3. Place the cursor on the lower end of R1. When you put it in the right place, a red connection marker (big star) will appear at the cursor. This indicates that the cursor is on an electrical connection point of the component.

4. Left-click or press ENTER to fix the first wire point. Move the cursor and you will see a wire extending from the cursor to the fixed point.

5. Move the cursor to the horizontal position of the base of Q1 below R1, left-click or press ENTER to fix the wire at this point. The wire is placed between the first and second anchor points.

6. Place the cursor on the base of Q1 and you will see the cursor change to a red connection mark. Left click or press ENTER to connect to the base of Q1.

7. Complete the placement of this part of the wire. Notice that the cursor is still in the shape of a cross, indicating that you are ready to place additional wires. To fully exit drop mode and restore the arrow cursor, you should right-click again or press ESC -- but you can't do that just yet.

8. Now we are going to connect C1 to Q1 and R1. Place the cursor on the connection point to the left of C1 and left-click or press ENTER to start a new connection.

9. Move the cursor horizontally to the connection between the base of Q1 and R1. A connection marker will appear.

10. Left-click or press ENTER to place the wire segment, then right-click or press ESC to indicate that you have finished placing the wire. Notice how the two wires are automatically connected.

11. Refer to Figure 3 to connect the rest of the circuit.

12. After finishing all the wires, right-click or press ESC to exit placement mode. The cursor returns to an arrow shape.

Network and Network Labels

A set of component pins connected to each other is called a net. For example, a net consists of the base of Q1, a pin of R1, and a pin of C1.

Identifying important nets in your design is easy, and you can add net labels.

Place net labels on both power nets:

1. Select Place > Net Label from the menu. A dotted box will hover over the cursor.

2. Edit the net label before placing it. Press the TAB key to display the Net Label dialog box.

3. Type 12V in the Net field, then click OK to close the dialog.

4. Put the net label on the principle, so that the lower left corner of the net label is close to the uppermost wire.

5. After placing the first net label, you are still in net label placement mode, press TAB to edit it before placing the second net label.

6. Type GND in the Net field and click OK to close the dialog and place the Net label.

7. Select File > Save (hotkeys F, S) to save the circuit.

Congratulations! You have completed your first schematic with Protel DXP. Before we turn the schematic into a board, let's set up the project options.