Component footprints are created in the PCB Library editor and placed in the PCB editor. Components are available for placement in the following ways:
- Choose Home | Place| Component from the main menus of the PCB editor.
- Select the component in the Libraries panel (View | System| Libraries), right-click then select Place <ComponentName>.
PCB component footprints are automatically placed when the design is transferred from the schematic editor to the PCB editor. This is called Design Synchronization, which is a process to detect and resolve the differences between the schematic and the PCB.
The process used to locate the required component footprint will depend on the method chosen to perform placement. Once the required footprint has been chosen for placement and is floating on the cursor:
- Press Tab to edit the properties of the component in the Inspector panel before it is placed.
- Press Spacebar to rotate the component counterclockwise (Shift+Spacebar for clockwise). The default rotation step is 90 degrees. To change this setting, use the Rotation Step value in the PCB Editor - General page of the System Preferences.
- If the component is being rotated, the Designator and Comment strings can be configured to hold their orientation or to rotate with the footprint. This behavior is controlled by the Autoposition setting for these strings in the Inspector panel.
- Press the L shortcut to flip the component to the bottom side of the board. Do not use the X or Y keys as this will mirror the part but not change its layer.
Placing From the Libraries Panel
With the part selected in the Libraries panel, placement of the component can be made in the following ways:
- Right-click then select Place <ComponentName> from the context menu.
- Double-click on the selected component. The component will appear floating in the design space. Place the component in the desired location then click to place.
- Click and hold the component's name in the Components panel then drag the component to the desired location and click to place it. This is a 'single shot' placement technique, meaning only a single instance of the chosen component can be placed. The other methods allow multiple instances to be placed.
Only components that have linked models can be placed in a design. Such components are distinguished with the
![](/documentation/sites/default/files/wiki_attachments/301766/Pnl_Libraries_Icon_HasModel.webp)
icon in the component list in the
Libraries panel.
The
Components panel also includes the category selection and
Search features to narrow down the list of the community components. Refer to the
Libraries panel page for more information.
Graphical Editing
Graphical component editing is limited to moving, rotating, and flipping. When a component is selected in the design space, it is highlighted in the current selection color as shown in the image below. To graphically manipulate a selected component:
- Press Delete to remove the selected component from the design.
- Click, hold, and drag to move the selected component. The cursor will jump to the component reference point, or the nearest pad center if the Smart Component Snap option is enabled on the PCB Editor - General page of the System Preferences.
- While a component is moving on the cursor press the Spacebar to rotate it (Shift+Spacebar to rotate in the other direction).
- While a component is moving on the cursor press the L key to flip it to the other side of the board.
If the Protect Locked Objects option is enabled on the PCB Editor - General page of the System Preferences and the Locked option for that design object is enabled as well, that object cannot be selected or graphically edited.
Component Selection
When you click and select a component, the selection bounding box appears. Traditionally, the default bounding box behavior has been to use the smallest rectangle that encloses all of the primitives in that component, excluding the designator and comment strings.
Explode Component to Free Primitives
When you right-click in the PCB editor's design space, the Component Actions commands appear. Among those commands is the Explode Component to Free Primitives command which is used to convert a Component object back to its original set of primitives.
After launching the command, the cursor will change to a cross-hair and you will enter component explode mode. Position the cursor over the component you wish to explode then click or press Enter. A confirmation dialog will appear - click Yes to proceed. An exploded component is no longer a component, so the designator and comment will be removed and the component will revert to the various primitives from which it was made.
Explode is a one-way process; there is no command to regroup an exploded component.
Continue converting further components to their free primitives or right-click or press Esc to exit component explode mode.
Explode has no effect on the footprint model stored in the applicable source component, only on the converted instance(s) of the component(s) placed on the PCB document.
To clear the selection of (or de-select) the object, use the Esc key.