Tutorial - Capturing the Schematic in Altium Designer

You are now ready to begin capturing (drawing) the schematic.

Placing the Components

Main page: Searching for & Placing Components

When Altium Designer is connected to a Workspace, the Components panel will list all components available for use in a project design, from this Workspace. For such components, the Components panel supports the same search features that are available in the Manufacturer Part Search panel, including string-based searching, faceted searching, or a combination of both, and also the Find Similar Components feature.

With the Components panel, components acquired from the Manufacturer Part Search panel will be placed in the multivibrator circuit. Once you have placed the components, the schematic should look like the image below.

All the components have been placed, ready for wiring.

Placing the Transistors

1. Select View » Fit Document from the main menus to make the document fill the design space.

2. Open the Components panel. To do this, click the  button at the bottom right of the design space and select Components from the menu.

3. Click the  button at the top left of the Components panel to open the Categories pane. Select the All entry to access the Workspace library.

   

   After that, the Categories pane can be closed by clicking the  button.

4. Click the  button at the top of the Components panel and select Refresh from the menu to update the panel's content with the components acquired from the Manufacturer Part Search panel.

   

5. In the Search field at the top of the panel, type transistor BC547. Search results will be presented in the panel.

   

6. Click the entry of the found transistor in the search result grid to select it.

7. Display the Details pane of the panel using the  button so that you can explore the details of the selected component.

   

8. Click the required transistor in the results grid of the panel to select it then click the  button in the Details pane. The cursor will automatically move to be within the bounds of the schematic sheet and change to a crosshair, with a symbol of the transistor floating on it. You are now in component placement mode. If you move the cursor around, the transistor will move with it.

   Do not place the transistor yet!

   

9. While the transistor is still floating on the cursor, press the Tab key to open the Properties panel. As the most-used field, the Designator field will be automatically highlighted in the panel, ready for editing.

   • You can close the Components panel for now and make it visible again later using the  button menu.

   • Note that each region of the Properties panel can be individually expanded or collapsed, which means your panel might look different.

   

10. Type Q1 in the Designator field and confirm that the visibility control for the Comment field is set to visible (shown as ).

    

11. Leave all other fields at their default values and click the pause button ( ) in the design space to return to component placement.

12. Move the cursor, with the transistor symbol attached, to position the transistor a little to the left of the middle of the sheet. Once you are happy with the transistor's location, click to place it on the schematic. If necessary, the location can be changed later.

    

13. Move the cursor and you will find that a copy of the transistor has been placed on the schematic sheet, and you are still in component placement mode with the transistor symbol floating on the cursor. This feature allows you to place multiple components of the same type.

14. You are ready to place the second transistor. This transistor is the same as the previous one so there is no need to edit its attributes before you place it. Altium Designer will automatically increment the component designator when you place multiple instances of the same component. In this case, the next transistor will automatically be designated Q2.

    If you refer to the schematic diagram shown above, you will notice that Q2 is drawn as a mirror of Q1. To horizontally flip the orientation of the transistor floating on the cursor, press the X key on the keyboard.

15. Move the cursor to position the component to the right of Q1.

    To position the component more accurately using the grid lines, zoom in (Ctrl+Mouse Wheel) to see the grid.

    

16. Once you have positioned the component, click to place Q2. Once again, a copy of the transistor you are "holding" will be placed on the schematic, and the next transistor will be floating on the cursor ready to be placed.

17. Since both of the transistors have been placed, exit component placement by right-clicking or pressing the Esc key. The cursor will revert back to a standard arrow.

Placing the Capacitors

1. Return to the Components panel and use the panel's Search field to search for capacitor 22nF 16V 0603.

2. Select the entry of the found capacitor in the search result grid.

3. Many of the resistors and capacitors have several footprint models, for different density levels. Under the footprint preview in the Details pane, select the A variety (FP-C0603C-CF-IPC_A).

   This footprint selection can also be done during or after placement, using the Properties panel.

   

4. Click the  button in the Details pane.

5. While the capacitor is floating on the cursor, press the Tab key to open the Properties panel.

6. Type C1 in the Designator field.

7. Click the Show More link in the panel's Parameters region to show the full list of component parameters. Make sure that the visibility of the Value parameter is only enabled. The value of this parameter will be shown next to the component in the design space.

   

8. Leave all other fields at their default values and click the pause button ( ) in the design space to return to component placement.

9. Press Spacebar to rotate the component in 90° increments until it has the correct orientation.

10. Position the capacitor above the transistors and click to place the component.

    

11. Position and place capacitor C2.

    

12. Right-click or press Esc to exit the component placement.

Placing the Resistors

1. Return to the Components panel and use the panel's Search field to search for resistor 100K 5% 0805.

2. Select the entry of the found 100K resistor in the search result grid.

3. Under the footprint preview in the Details pane, select the M variety (RESC2013X70X40ML20T20).

4. Click the  button in the Details pane.

5. While the resistor is floating on the cursor, press the Tab key to open the Properties panel.

6. Type R1 in the Designator field.

7. Click the Show More link in the panel's Parameters region and make sure that the visibility of the Value parameter is only enabled.

8. Leave all other fields at their default values and click the pause button ( ) in the design space to return to component placement.

9. Press Spacebar to rotate the component in 90° increments until it has the correct orientation.

10. Position the resistor above and to the left of the base of Q1 and click to place the component.

    

11. Next, place the other 100K resistor, R2, above and to the right of the base of Q2. The designator will automatically increment when you place the second resistor.

    

12. Right-click or press Esc to exit the component placement.

13. Return to the Components panel and use the panel's Search field to search for resistor 1K 5% 0805 fixed.

14. Select the entry of the found 1K resistor in the search result grid.

15. Under the footprint preview in the Details pane, select the M variety (RESC2013X70X40ML20T20).

16. Click the  button in the Details pane.

17. While the resistor is floating on the cursor, press the Tab key to open the Properties panel.

18. Type R3 in the Designator field.

19. Click the Show More link in the panel's Parameters region and make sure that the visibility of the Value parameter is only enabled.

20. Leave all other fields at their default values and click the pause button ( ) in the design space to return to component placement.

21. Press Spacebar to rotate the component in 90° increments until it has the correct orientation.

22. Position and place R3 directly above the collector of Q1, then place R4 directly above the collector or Q2.

    

23. Right-click or press Esc to exit the component placement.

Placing the Connector

1. Return to the Components panel and use the panel's Search field to search for connector male straight.

2. Select the entry of the found connector in the search result grid.

3. Click the  button in the Details pane.

4. While the resistor is floating on the cursor, press the Tab key to open the Properties panel.

5. Type P1 in the Designator field.

6. Leave all other fields at their default values and click the pause button ( ) in the design space to return to component placement.

7. Press Spacebar to rotate the component in 90° increments until it has the correct orientation.

8. Click to place the connector on the schematic.

   

9. Right-click or press Esc to exit the component placement.

10. Save the schematic document locally by right-clicking its entry in the Projects panel and selecting Save from the context menu.

Wiring up the Circuit

Main page: Creating Circuit Connectivity in Your Schematics

Wiring is the process of creating connectivity between the various components of your circuit. To wire up your schematic, refer to the sketch of the circuit () and the video shown below.

Use the wiring tool to wire up your circuit. Toward the end of the video, you can see how wires can be dragged.

1. First, wire the lower pin of resistor R1 to the base of transistor Q1 in the following manner. Select the Place » Wire command from the main menus (or use the Ctrl+W shortcut) to enter the wire placement mode. The cursor will change to a crosshair.

2. Position the cursor over the bottom end of R1. When you are in the right position, a red connection marker (red cross) will appear at the cursor location. This indicates that the cursor is over a valid electrical connection point on the component.

3. Click to anchor the first wire point. Move the cursor, and a wire will extend from the cursor position back to the anchor point.

4. Position the cursor over the base of Q1 until you see the cursor change to a red connection marker. If the wire is forming a corner in the wrong direction, press Spacebar to toggle the corner direction.

5. Click to connect the wire to the base of Q1. The cursor will release from that wire.

6. Note that the cursor remains a crosshair indicating that you are ready to place another wire. To exit placement mode completely and go back to the arrow cursor, you would right-click or press Esc – but do not do this just now.

7. Next, wire from the lower pin of R3 to the collector of Q1. Position the cursor over the lower pin of R3 and click to start a new wire. Move the cursor vertically until it is over the collector of Q1, then click to place the wire segment. Again, the cursor will release from that wire and you remain in wiring mode, ready to place another wire.

8. Wire up the rest of your circuit, as shown in the video above.

9. When you have finished placing all the wires, right-click or press Esc to exit placement mode. The cursor will revert to an arrow.

Placing the Net Labels

Each set of component pins that you have connected to each other now forms what is referred to as a net. For example, one net includes the base of Q1, one pin of R1, and one pin of C1. Each net is automatically assigned a system-generated name, which is based on one of the component pins in that net.

To make it easy to identify important nets in the design, you can add net labels to assign names. For the multivibrator circuit, you will label the 12V and GND nets in the circuit, as shown below.

Net labels have been added to the 12V and GND nets, completing the schematic.

1. Select the Place » Net Label command from the main menus. A net label will appear floating on the cursor.

2. To edit the net label before it is placed, press Tab to open the Properties panel.

3. Type 12V in the Net Name field.

   

4. Click the pause button ( ) in the design space to return to object placement.

5. Place the net label so that its hotspot (the bottom left corner) touches the uppermost wire on the schematic, as shown in the images below. The cursor will change to a red cross when the net label is correctly positioned to connect to the wire. If the cross is light gray, it means there will not be a valid connection made.

   
   The net label in free space (the top image) and positioned over a wire (the bottom image), note the red cross.

6. After placing the first net label, you will still be in net label placement mode. Press the Tab key again to edit the second net label in the Properties panel before placing it.

7. Type GND in the Net Name field.

8. Click the pause button ( ) in the design space to return to object placement.

9. Place the net label so that the bottom left of the net label touches the lowermost wire on the schematic (as shown in the completed schematic image above). Right-click or press Esc to exit net label placement mode.

10. Save the schematic document locally by right-clicking its entry in the Projects panel and selecting Save from the context menu.

Congratulations! You have just completed your first schematic capture. Before you turn the schematic into a circuit board, you need to configure the project options and check the design for errors.

Setting up Project Options

Main page: Accessing, Defining & Managing Project Options

Project-specific settings are configured in the Project Options dialog. The project options include error reporting settings, a connectivity matrix, class generation settings, and more. Some project options are shown and described below.

❯ ❮ Javascript ID: Tutorial_Dlg_ProjectOptions_AD24

When you validate a project, Altium Designer checks for logical, electrical, and drafting errors between the schematic content and error reporting settings. The Error Reporting tab of the Project Options dialog is used to set up a wide range of checks. The Report Mode settings show the level of severity of a violation. If you want to change a setting, click on a Report Mode next to the violation you want to change and choose the level of severity from the drop-down list. As the design is coming along, a list of the pins in each net is built into memory. The type of each pin is detected (e.g., input, output, passive, etc.), then each net is checked to see if there are pin types that should not be connected to each other, for example, an output pin connected to another output pin. The Connection Matrix tab of the Project Options dialog is where you configure what pin types are allowed to connect to each other. For example, look at the entries on the right side of the matrix diagram and find Output Pin. Read across this row of the matrix until you get to the Open Collector Pin column. The square where they intersect is orange, indicating that an Output Pin connected to an Open Collector Pin on your schematic will generate an error condition when the project is validated. You can set each error type with a separate error level, i.e., from No Report to a Fatal Error. Click on a colored square to change the setting; it will cycle through the four possible settings. The Class Generation tab of the Project Options dialog is used to configure what type of classes are generated from the design (the Comparator and ECO Generation tabs are then used to control if classes are transferred to the PCB). The Comparator tab of the Project Options dialog sets which differences will be reported or ignored when comparing documents. When you need detailed control, you can selectively configure the comparator using the individual comparison settings.

1. Right-click the project entry in the Projects panel and select the Project Options command from the context menu to open the Project Options dialog, then select the Error Reporting tab of the dialog.

   

2. Scroll through the list of error checks and note that they are clustered in groups. Each group can be collapsed if required.

3. Click on the Report Mode setting for any check and note the options available.

4. Select the Connection Matrix tab of the Project Options dialog.

5. Your circuit contains only passive pins. Look down the row labels to find the Passive Pin row. Look across the column labels to find Unconnected. The square where these entries intersect indicates the error condition when a passive pin is found to be unconnected in the schematic. The default setting is green () indicating that no report will be generated.

   

6. Change the default settings so that the connection matrix detects unconnected passive pins. Click on this intersection box until it turns orange () so that an error will be generated for unconnected passive pins when the project is validated. You will purposely create an instance of this violation later in the tutorial.

   

7. Select the Class Generation tab of the Project Options dialog.

8. For a simple, single-sheet design such as this, there is no need to generate a component class. Clear the Component Classes checkbox for the project's schematic document.

   

9. Click OK to apply changes and close the Project Options dialog.

10. Save the project locally by right-clicking its entry in the Projects panel and selecting Save from the context menu.

You are now ready to validate the project and check for any errors.

Validating the Project

Main page: Validating Your Design Project

Validation of a project checks for drafting and electrical rules errors in the design documents, and details all warnings and errors in the Messages panel. You have set up the check settings in the Error Checking and Connection Matrix tabs of the Project Options dialog, so you are now ready to check the design.

1. To validate the Multivibrator project, right-click its entry in the Projects panel and select Validate PCB Project Multivibrator.PrjPcb from the context menu.

   

2. All validation warnings and errors are displayed in the Messages panel. The panel will only open automatically if there are errors detected (not when there are only warnings). To open it manually, click the  button at the bottom right of the design space and select Messages from the menu.

3. If your circuit is drawn correctly, the Messages panel should not contain any errors, only the message Compile successful, no errors found. If there are errors, work through each one, checking your circuit, and ensuring that all wiring and connections are correct.

   

You will now deliberately introduce an error into the circuit and validate the project again.

1. Click in the middle of the wire that connects P1 to the emitters of Q1 and Q2 (the wire of net GND). Small, square editing handles will appear at each vertex of the wire and the selected color will display as a dotted line along the wire to indicate that it is selected. Press the Delete key to delete the wire.

   

2. Validate the project again (select Validate PCB Project Multivibrator.PrjPcb from the right-click menu of the project entry in the Projects panel). The Messages panel will display error messages indicating you have unconnected pins in your circuit.

   

   • The Messages panel is divided horizontally into two regions as shown in the image above. The upper region lists all messages, which can be saved, copied, cross probed to, or cleared via the right-click menu. The lower region details the warning/error currently selected in the upper region of the panel.

   • When you double-click on an error or warning in either region of the Messages panel, the schematic view pans and zooms to the violating object.

   • When you hover the cursor over the violating object (not the wiggly line), a message describing the violation condition will appear.

Before you finish this section of the tutorial, fix violations in the schematic.

1. Undo the delete action (Ctrl+Z) to restore the deleted wire.

2. Validate the project again to check that there are no longer any violations. The Messages panel should show no violations.

3. Save the project to the Workspace. To do this, click the Save to Server control next to the project entry in the Projects panel, confirm that the Multivibrator.PrjPcb and Multivibrator.SchDoc files are checked in the Save to Server dialog that opens, enter a meaningful comment into the Comment field (e.g., Schematic is created and validated), then click the OK button.

Configuring the Bill of Materials

Main page: BOM Management with ActiveBOM

Ultimately, every component used in a design must have detailed supply chain information. Rather than requiring that this information be added to each design component or added as a post-process in an Excel spreadsheet, you can add it at any point through the design cycle in an ActiveBOM document (*.BomDoc).