Capturing the Schematic

Applies to Altium Designer version: 24

Placing from the Components Panel onto the Schematic

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.

To open the Components panel, click the Panels button button at the bottom right of the application window and select Components from the menu.

The panel’s Categories pane (or the drop-down menu in the panel's compact mode) lists available Workspace library components under the All category entry. When the panel is in its normal mode, click the Categories list icon or the « icon to collapse or expand the display of the list. The structure of categories reflects component types currently defined on the connected Workspace (use the Data Management – Component Types page of the Preferences dialog for viewing and managing Component Types).

The Components panel being used to browse components stored in a Workspace.
The Components panel being used to browse components stored in a Workspace.

To place a component from the panel, you can:

  • Click the Place button in the Component Details pane – the cursor automatically moves to be within the bounds of the schematic sheet and the component appears floating on the cursor; position it and click to place. After placing a component, another instance of the same component will appear on the cursor; right-click to drop out of placement mode.

    Components panel, placing from component details pane

  • Right-click on the component and select Place from the context menu. The component appears floating on the cursor; position it and click to place. Note that if the panel is floating over the design space, it will fade to allow you to see the schematic and place the component. After placing a component, another instance of the same component will appear on the cursor; right-click to drop out of placement mode.
  • Click, Hold&Drag – click and drag the component from the grid region of the panel onto a schematic sheet. This mode requires that the cursor is held down; the component is placed when the cursor is released. Using this technique only one component is placed. After placing the component, you are free to select another component or another command.

Placement Tips

While the component is floating on the cursor, you can:

  • Press Spacebar to rotate it counterclockwise in 90º increments.
  • Press X to flip it along the X-axis; press Y to flip it along the Y-axis.
  • Press Tab to display the Properties panel and edit the properties of an object prior to placement. The values entered become the defaults. If the designator has the same prefix, it will be auto-incremented.
  • During component placement, the software will automatically pan if you touch the window edge. Autopanning is configured in the Schematic – Graphical Editing page of the Preferences dialog. If you accidentally pan beyond where you want, while the component is floating on the cursor you can:
    • Ctrl+Mouse Wheel to zoom out and in again, or
    • Right-Click, Hold&Drag to slide the schematic around, or
    • Ctrl+PgDn to display the entire sheet again.
  • If the Components panel is floating over the schematic sheet when you place a part, it will automatically become transparent whenever the cursor+component gets close to it. The transparency of floating panels is configured in the System – Transparency page of the Preferences dialog. Alternatively, all floating panels can be hidden/displayed at any time (while running a command or not) by pressing the F4 shortcut.

Learn more about Schematic Placement & Editing Techniques

Working with the Properties panel during Placement

During object placement, if you press Tab the editing process will pause and the interactive Properties panel in its appropriate mode will open. The default behavior is for the most commonly edited field to be highlighted, ready for editing. Because the editing process is paused, you can use the cursor (or press Tab on the keyboard) to move to another field in the panel.

When you have finished editing, click the Pause button ( Pause button) as shown in the image below to return to object placement. Alternatively, press Enter to finish object editing and return to object placement.

Editing is paused when you press Tab during placement – click the Pause icon on the screen to return to placing the component.
Editing is paused when you press Tab during placement – click the Pause icon on the screen to return to placing the component.


Placing the Multivibrator Parts

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

You can proceed to find and place the components. Note that the collapsible sections below include tips on editing during placement, which is more efficient than editing after placement. If you choose to leave the editing until after the components are placed, click to select the component and edit it in the Properties panel.

All the components have been placed, ready for wiring.
All the components have been placed, ready for wiring.

Editing in the Properties Panel

One of the powerful features of the Properties panel is that it supports editing multiple selected objects at the same time.

  • If all objects share a property, that property will be available for editing.
  • If all objects share the same property value, that value will be displayed.
  • If objects share the same property but have different values, it will display an asterisk (*).
  • The value entered or option chosen is applied to all selected objects.

Use the Properties panel to edit the properties of multiple selected objects. The selected components are rotated to force their strings to the default locations.
Use the Properties panel to edit the properties of multiple selected objects. The selected components are rotated to force their strings to the default locations.

You have now placed all the components. Note that the components shown in the image above are spaced so that there is plenty of room to wire to each component pin. This is important because you cannot place a wire across the bottom of a pin to get to a pin beyond it. If you do, both pins will connect to the wire. If you need to move a component, click and hold on the body of the component then drag the mouse to reposition it.

Component Positioning Tips

  • To reposition any object, place the cursor directly over the object, click and hold the left mouse button, drag the object to a new position then release the mouse button. Movement is constrained to the current snap grid, which is displayed on the Status Bar. Press the G shortcut at any time to cycle through the current snap grid settings. Remember that it is important to position components on a coarse grid, such as 50 or 100mil.
  • Once a component has been placed on the schematic, the software will attempt to maintain connectivity (keep the wires attached) if the component is moved. This connective-aware movement is referred to as dragging. To move the component without maintaining connectivity, hold Ctrl as you click and drag the component. To switch the default behavior from dragging to moving, disable the Always Drag option in the Schematic – Graphical Editing page of the Preferences dialog.
  • You can also re-position a group of selected schematic objects using the arrow keys on the keyboard. Select the objects then press an arrow key while holding down the Ctrl key. Hold Shift as well to move objects by 10 times the current snap grid.
  • The grid can also be temporarily set to the minimum 10mil value while moving an object with the mouse; hold Ctrl to do this. Use this feature when positioning text.
  • The grids you cycle through when you press the G shortcut are defined in the Schematic – Grids page of the Preferences dialog (Tools » Preferences). The Units controls on the Schematic – General page of the Preferences dialog are used to select the measurement units; select either Mils or Millimeters. Note that Altium Designer components are designed using an imperial grid; if you change to a metric grid, the component pins will no longer fall onto a standard grid. Because of this, it is recommended to use Mils for Units unless you plan on only using your own components.

Wiring up the Circuit

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 animation shown below.

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

The Active Bar

The tools most commonly used in each editor are available on the Active Bar, which is displayed at the top of the editing window.

Place a Net Label, using the Active Bar

The buttons on the Active Bar are either single-function or multi-function. Multi-function buttons are indicated by a small white triangle in their bottom-right corner. Click and hold anywhere on a multi-function button for one second or right-click it – a menu will appear listing other available commands. The last-used command will become the default for that button location.

Wiring Tips

  • Use the Ctrl+W shortcut to launch the Place » Wire command.
  • Left-click or press Enter to anchor the wire at the cursor position.
  • Press Backspace to remove the last anchor point.
  • Press Spacebar to toggle the direction of the corner. You can observe this in the animation shown above toward the end when the connector is being wired.
  • Press Shift+Spacebar to cycle through the wiring corner modes. Available modes include: 90, 45, Any Angle, and Autowire (place orthogonal wire segments between the click points).
  • Right-click or press Esc to exit wire placement mode.
  • Click, Hold&Drag to drag the component together with any connected wires; Ctrl+Click, Hold&Drag to move a placed component.
  • Whenever a wire crosses the connection point of a component or is terminated on another wire, a junction will automatically be created.
  • A wire that crosses the end of a pin will connect to that pin even if you delete the junction. Check that your wired circuit looks like the figure shown before proceeding.
  • Wiring cross-overs can be displayed as a small arch if preferred. Enable the Display Cross-Overs option in the Schematic – General page of the Preferences dialog.

Nets and Net Labels

Each set of component pins that you have connected to each other now form 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.
Net Labels have been added to the 12V and GND nets, completing the schematic.

Net Labels, Ports, and Power Ports

  • As well as giving a net a name, Net Labels are also used to create connectivity between two separate points on the same schematic sheet.
  • Ports are used to create connectivity between two separate points on different sheets. Off Sheet Connectors can also be used to do this.
  • Power Ports are used to create connectivity between points on all sheets; for this single sheet design, Net Labels or Power Ports could have been used.
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

Project-specific settings are configured in the Project Options dialog shown below (Project » Project Options). The project options include the error checking parameters, a connectivity matrix, class generation settings, the Comparator setup, Engineering Change Order (ECO) generation, output paths and connectivity options, Multi-Channel naming formats, and project-level Parameters.

Project outputs, such as assembly outputs, fabrication outputs, and reports can be set up from the File and Reports menus. These settings are also stored in the Project file so they are always available for this project. An alternate approach is to use an OutputJob file to configure the outputs, with the advantage that an OutputJob can be copied from one project to the next. See Preparing Your Design for Manufacture to learn more about configuring the outputs.

Dynamic Compilation

The Unified Data Model (UDM) is available from the moment a project is opened and should not require additional compilation, which saves time with increased speed of compilation and persistent listings of nets and components in the Navigator panel. The design connectivity model is incrementally updated after each user operation. This means that manual project compilation is not necessary to see the contents of the Navigator panel, run the Bill of Materials (BOM), or perform an Electronic Rules Check (ERC). Manual compilation is not needed for:

  • Navigator and Projects panels
  • ActiveBOM
  • Cross-probing
  • Net color highlighting
  • Pin swapping
  • Component cross reference

Checking the Electrical Properties of Your Schematic

Schematic diagrams are more than just simple drawings – they contain electrical connectivity information about the circuit. You can use this connectivity awareness to verify your design. When you compile a project (Project » Validate PCB Project), the software checks for logical, electrical, and drafting errors between the UDM and compiler settings. Any violations that are detected will display in the Messages panel.

Setting up the Error Reporting

Dialog page: Error Reporting

The Error Reporting tab in the Project Options dialog is used to set up a large range of drafting and component configuration 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.

Configure the Error Reporting tab to detect for design errors when the project is compiled.
Configure the Error Reporting tab to detect for design errors when the project is compiled.

Setting Up the Connection Matrix

Dialog page: Connection Matrix

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 compiled.

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; continue to click to move to the next check-level. Set the matrix so that Unconnected – Passive Pin generates an Error, as shown in the image below.

The Connection Matrix tab defines what electrical conditions are checked for on the schematic; note that the Unconnected – Passive Pin setting is being changed.
The Connection Matrix tab defines what electrical conditions are checked for on the schematic; note that the Unconnected – Passive Pin setting is being changed.

Configuring the Class Generation

Dialog page: Class Generation

The Class Generation tab in 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). By default, the software will generate Component classes and Rooms for each schematic sheet, and Net Classes for each bus in the design. For a simple, single-sheet design such as this, there is no need to generate a component class or a room. Ensure that the Component Classes checkbox is cleared; doing this will also disable the creation of a room for that component class.

Note that this tab of the dialog also includes options for User-Defined Classes.

The Class Generation tab is used to configure what classes and rooms are automatically created for the design.
The Class Generation tab is used to configure what classes and rooms are automatically created for the design.

Setting Up the Comparator

Dialog page: Comparator

The Comparator tab in the Project Options dialog sets which differences between files will be reported or ignored when a project is compiled. Generally, the only time you will need to change settings in this tab is when you add extra detail to the PCB, such as design rules, and do not want those settings removed during design synchronization. If you need more detailed control, you can selectively control the comparator using the individual comparison settings.

For this tutorial, it is sufficient to confirm that the Ignore Rules Defined in PCB Only option is enabled as shown in the image below.

The Comparator tab is used to configure exactly what differences the comparison engine will check for.
The Comparator tab is used to configure exactly what differences the comparison engine will check for.

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

Verifying the Project to Check for Errors

Main page: Verifying 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 rules in the Error Checking and Connection Matrix tabs of the Project Options dialog, so you are now ready to check the design.

To verify the project and check for errors, select Project » Validate PCB Project Multivibrator.PrjPcb from the main menus.

Use the Messages panel to locate and resolve design warnings and errors; double-click on a warning/error to cross probe to that object.
Use the Messages panel to locate and resolve design warnings and errors; double-click on a warning/error to cross probe to that object.

When you double-click on an error in the Messages panel:

  • The schematic zooms to present the object in error. The Zoom Precision is set by the upper slider in the Highlight Methods section of the System – Navigation page of the Preferences dialog.
  • The entire schematic fades except for the object in error. The amount that the schematic fades is controlled by the Dimming level, set by the lower slider in the Highlight Methods section of the System – Navigation page of the Preferences dialog. Click anywhere on the schematic to clear the dimming.

    Preferences dialog, setting the zoom level when you double-click on an error in the Messages panel

  • To clear all messages from the Messages panel, right-click in the panel and select Clear All.

Configuring the Bill of Materials

Main page: BOM Management with ActiveBOM

Ultimately, every part used in the 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 (*.BomDoc).

ActiveBOM is the component management editor included in Altium Designer, which is used to:

  • Configure the component information so that it is BOM-ready, including adding additional non-PCB component BOM items, such as the bare board, glue, mounting hardware, and so on.
  • Add additional columns, such as a line number column, to suit the requirements of the assembly house.
  • Map each design component to a real-world manufacturer part.
  • Verify the supply chain availability and price for each part, for a defined number of manufactured units.
  • Calculate the cost to build for the defined number of manufactured units.

ActiveBOM is used to map each design component to a real-world part.
ActiveBOM is used to map each design component to a real-world part.

This ability to inject supply chain details directly into the BOM changes the role of the BOM document in the PCB project. No longer a simple output file, ActiveBOM raises the component management process to sit alongside the schematic capture and PCB design processes, where ActiveBOM's BomDoc becomes the source of all Bill Of Materials data for the PCB project for all BOM-type outputs. ActiveBOM is the recommended approach to BOM management.
ActiveBOM queries the supply chain in real-time, using the Part Providers enabled in the settings of your connected Workspace. Because data is updated in real-time, the availability of the parts used in this tutorial will change over time. The list of available suppliers also changes over time. For these reasons, the results you get may be different from the results shown and described in this tutorial.

Schematic capture is now complete. It's time to set up the design constraints!

If the Constraint Manager is not available (you can quickly check if the Constraint Manager is available by opening the Design main menu of the Schematic editor and checking for the Constraint Manager command), go to the Creating and Configuring the PCB Document page.

Note

The features available depend on your level of Altium Designer Software Subscription.

Content