The Part represents the actual physical electronic component.
A Part is an electrical design primitive. It is a schematic symbol that represents an electronic device, such as a resistor, a switch, an operational amplifier, a voltage regulator, etc. Parts are stored within components in schematic component libraries. Note that each component can contain one or more parts. Along with a symbolic representation of the component, the part also includes links to models, such as the PCB footprint, and also parameters that are used to document details such as component parameters and supplier information. How the model links and parameters are added to the part depends on the type of library storage being used.
The terms Part and Component are both used to describe the symbol that represents the actual electronic device. The term Part is used because some components contain multiple parts. For example, a quad Op Amp component contains four separate Op Amps, or a resistor network can contain eight independent resistors. For these types of devices, you can create a separate schematic symbol to represent each Part during the component definition and place each of these parts independently. The terms Part and Component are used interchangeably on this page unless a multi-part component is being discussed.
Parts are available for placement in both the schematic and schematic library editors.
In the schematic editor, click Place » Part.
Right-click in the design space then choose Place » Part from the context menu.
From the Components panel, right-click on a component and select Place <ComponentName>.
Dragging and dropping a component from the Components panel.
Select the Place button in the Details pane of the Components panel, or by using the Enter hotkey.
From the SCH Library panel when in the schematic library editor, select a component, then click Place.
Placement from the Components Panel
In the schematic editor, the part selection and placement process may be done from the Components panel.
The panel displays the contents of the currently selected library. Use the drop-down next to the library name to choose another library.
Use the mask field below the currently selected library field to filter the list and speed the searching process or scroll and select the required part.
Click Place, double-click, or click and drag to place the selected component onto the active schematic sheet. While the part is floating on the cursor, it can be rotated (press Spacebar), mirrored along an axis (press X or Y), or edited (press Tab) before placement.
The columns shown in the list of components in the currently selected library can be reorganized (click and drag) or reconfigured (right-click, then choose Select Columns).
Searching for a Component
The non-Workspace library menu options provide you the ability to set preferences, perform searches, and migrate database and file-based library content. To access these options, select the library menu button at the top right of the Components panel.
Select File-based Libraries Preferences to open the Available File-based Libraries dialog, where you may view controls to add or remove libraries, install libraries, and specify library search paths.
The current listing of database and file-based library components may be filtered by entering a search phase in the Components panel Search field. To access more advanced search capabilities for component libraries, select the File-based Libraries Search option from the panel’s menu (top right), which opens the File-based Libraries Search dialog. The dialog offers flexible search options including query-based filter constraints, and the ability to search through all available database and file-based libraries or those within a specified path.
The default search Scope is to search for Components in the Available File-based Libraries.
Alternatively, the dialog also supports searching through Libraries on path stored in folders on a drive. To do this, enable the Libraries on path option then configure the Path options as required.
The Filters use "AND" and, therefore, it is better to start with a simple filter and if there are many results, use the Refine last search mode to search within the results.
Query search results are presented in the File-based Libraries Search dialog when selecting Helper.
Placing from the Schematic Library Editor
A Part also can be placed directly from a library that is open in the schematic library editor from the SCH Library panel. Note that:
Clicking the Place button in the panel will place the selected part (component) in the last active schematic sheet.
While the part is floating on the cursor, it can be rotated (press Spacebar), mirrored along an axis (press X or Y), or edited (press Tab) before placement. The action can also be performed while dragging the object. Rotation is in increments of 90°.
While attributes can be modified during placement (Tab to access the Properties panel), keep in mind that these will become the default settings for further placement unless the Permanent option on the Schematic – Defaults page of the Preferences dialog is enabled. When this option is enabled, changes made will affect only the object being placed and subsequent objects placed during the same placement session.
Graphical editing for a part is limited to moving, rotating, and mirroring. When a part is selected in the design space, a dashed selection box will appear around it. To graphically manipulate a selected component:
Press Delete to remove the selected part from the design.
Click and hold to move the selected part. The cursor will jump to the nearest electrical hotspot (the wiring end of the nearest pin).
Press the Spacebar to rotate the arc counterclockwise or Shift+Spacebar for clockwise rotation. The action can also be performed while dragging the object. Rotation is in increments of 90°.
While a part is moving on the cursor, press the X or Y key to mirror it along that axis.
A selected Part
When a component is rotated, its text strings are automatically repositioned to suit the new orientation. This behavior can be disabled if required. To do this, edit the string then clear the Autoposition checkbox in the Parameters Properties panel. Note that manually positioned text strings are denoted by a dot. These dots can be hidden if required by clearing the Mark Manual Parameters option on the Schematic – Graphical Editing page of the Preferences dialog.
If attempting to graphically modify an object that has its Locked property enabled, a dialog will appear asking for confirmation to proceed with the edit. If the Protect Locked Objects option is enabled on the Schematic – Graphical Editing page of the Preferences dialog and the Locked option for that design object is enabled as well, then that object cannot be selected or graphically edited. Double-click on the locked object directly and disable the Locked property or disable the Protect Locked Objects option to graphically edit the object.
Working Between the Schematic Component and the PCB Component
The software includes tools to help work between the component on the schematic and that same component on the PCB. These tools include Cross Probing, Cross Selection, and Selecting the PCB Components from the schematic.
As the name implies, Cross Probe allows you to click on a component in one editor and jump to that component in the other editor. To Cross Probe:
Click Cross Probe located on the schematic or PCB editor menu on the Tools menu.
When you click the component in the schematic editor, it will be centered and zoomed in the PCB editor. The zoom level is set on the System – Navigation page of the Preferences dialog.
The default behavior is to remain in the same editor, ready to cross probe another component. To switch to the other editor as you Cross Probe, hold the Ctrl key.
Cross Select Mode
Cross Select Mode selects the same component in the other editor. Note that it does not zoom and center. Cross Selection is either on or off. Click Tools » Cross Select Mode to toggle the mode on/off. Select multiple components by holding the Shift key as you click to select.
Selecting the PCB Components
This feature allows you to select multiple schematic components in a specific order, then place those same components in the PCB editor in the same order. To use this feature:
Select the components on the schematic one by one (hold Shift as you click to select multiple components).
Switch to the PCB editor then press the I, C shortcut to launch the Reposition Selected Components command. The Reposition Selected Components command is also available on the right-click menu after pressing the I shortcut.
If attempting to graphically modify an object that has its Locked property enabled, a dialog will appear asking for confirmation to proceed with the edit. If the Protect Locked Objects option is enabled on the Schematic – Graphical Editing page of the Preferences dialog, and the Locked option for that design object is enabled as well, then that object cannot be selected or graphically edited. Click the locked object to select it then disable the Locked property in the List panel or disable the Protect Locked Objects option to graphically edit the object.
This method of editing uses the associated Component dialog and the Properties panel mode to modify the properties of a part object.
The Component dialog (the first image) and the Component mode of the Properties panel (the second image)
After placement, the Component dialog can be accessed by:
Double-clicking on the placed component object.
Placing the cursor over the component object, right-clicking then choosing Properties from the context menu.
During placement, the Component mode of the Properties panel can be accessed by pressing the Tab key. Once the component is placed, all options appear.
After placement, the Component mode of the Properties panel can be accessed in one of the following ways:
If the Properties panel is already active, by selecting the component object.
After selecting the component object, select the Properties panel from the Panels button in the bottom right section of the design space or select View » Panels » Properties from the main menus.
If the Double Click Runs Interactive Properties option is disabled enabled (default) on the Schematic – Graphical Editing page of the Preferences dialog, when the primitive is double-clicked or you right-click on a selected primitive then choose Properties, the Properties panel will open. When the Double Click Runs Interactive Properties option is disabled, the dialog will open.
While the options are the same in the dialog and the panel, the order and placement of the options may differ slightly.
If a component used in a design (or managed schematic sheet) has been deleted, this will be indicated at the bottom of the General tab in the Properties panel by the associated icon.
If a selected component sourced from the connected Altium 365 Workspace has any health issues, an indication of this will be presented by the (for errors) or (for fatal errors) icon next to the component's revision status. The number at the right of the icon indicates the number of found issues. Click the down arrow at the right of the number to see the short descriptions of the issues.
Editing Multiple Objects
The Properties panel supports multiple object editing, where the property settings that are identical in all currently selected objects may be modified. When multiples of the same object type are selected manually, via the Find Similar Objects dialog or through a Filter or List panel, a Properties panel field entry that is not shown as an asterisk (*) may be edited for all selected objects.
A List panel allows you to display design objects from one or more documents in tabular format enabling quick inspection and modification of object attributes. Used in conjunction with appropriate filtering – by using the applicable Filter panel, or the Find Similar Objects dialog – it enables the display of just those objects falling under the scope of the active filter – allowing you to target and edit multiple design objects with greater accuracy and efficiency.