Component

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>.

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:

1. Press Tab to edit the properties of the component in the Inspector panel before it is placed.
2. 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.
3. 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. 
4. 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  icon in the component list in the Libraries panel.

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.

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.

Continue converting further components to their free primitives or right-click or press Esc to exit component explode mode.

All Component object properties are available for editing in the Inspector panel when a placed component is selected in the design space.

Location 

Use the options to configure the X/Y coordinates and the rotation of the component.

Properties

• Layer - sets the layer on which the component is placed. Components can be assigned to the Top layer or Bottom layer. Use the drop-down to select a different layer. Changing the layer status swaps all of the component primitives to each layer's respective opposite layer. For example, moving a Top layer component to the Bottom layer means single layer pages are swapped from the Top to the Bottom layer, primitives on the Top Overlay are reassigned to the Bottom Overlay, and primitives on a paired mechanical layer are swapped to the other mechanical layer in that pair. The orientation of the component will be flipped along the X-axis and the component overlay text will read from the bottom. 

• Designator - the designator is used to uniquely identify each placed part to distinguish it from all other parts placed in all the PCB documents in the project. It is an alphanumeric string of up to 255 characters. Each component must have a unique Designator string. Toggle the eye icon to show/hide the designator. Click Designator to open the Parameter mode of the Inspector panel to configure the designator.

  

  The designator is automatically placed when the parent component part object is placed. It is not a design object that you can directly place.

• Comment  - the comment of the component is used to add additional information to a placed object. It is an alphanumeric string of up to 255 characters. Toggle the eye icon to show/hide the comment. Click Comment to open the Parameter mode of the Inspector panel to configure the comment.

  

• Description - enter the desired description.
• Type - select one of the following component types for the component footprint here. The available types are:
  • Standard - these components possess standard electrical properties, are always synchronized between the schematic and PCB (the footprint, pins/pads, and net assignments must all match), and are included in the BOM. An example is a standard electrical component, such as a resistor.
  • Mechanical - these components do not have electrical properties, are not synchronized (you must manually place them in both editors), and are included in the BOM. An example is a heatsink.
  • Graphical - these components do not have electrical properties, are not synchronized (you must manually place them in both editors), and are not included in the BOM. An example is a company logo.
  • Net Tie (in BOM) - these components are used to short two or more different nets together. They are always synchronized between the schematic and PCB (the footprint, pins/pads, and net assignments must all match), and are included in the BOM. They differ from a Standard component in that connectivity created by copper within the footprint is not checked - it is this copper that allows the nets to be shorted. Note: enable the Verify Shorting Copper option in the Design Rule Checker dialog to verify that there is no unconnected copper within the component.
  • Net Tie - these components are used to short two or more different nets together. They are always synchronized between the schematic and PCB (the footprint, pins/pads, and net assignments must all match), and are not included in the BOM. They differ from a Standard component in that connectivity created by copper within the footprint is not checked - it is this copper that allows the nets to be shorted. Note: enable the Verify Shorting Copper option in the Design Rule Checker dialog to verify that there is no unconnected copper in the component.
  • Standard (No BOM) - these components possess standard electrical properties, are always synchronized between the schematic and PCB (the footprint, pins/pads, and net assignments must all match), and are not included in the BOM. An example is a testpoint component that you wish to exclude from the BOM.
  • Jumper - these components are used to include wire links in a PCB design, for example, on a single-sided PCB that cannot be fully routed on one layer. For this component type, the component footprint and pins are synchronized between the schematic and PCB but the net assignments are not, and the component is included in the BOM. As well as selecting this option at the component level, both of the pads in the component must have their JumperID set to the same non-zero value. Jumper type components do not need to be wired on the schematic; they only need to be included on the schematic if they are required in the BOM. If they are not required in the BOM, they can be placed directly in the PCB where the Component Type is set, the JumperIDs are set, and the Nets manually assigned for the pads. 
• Height - a height field for the component, this field was used before the introduction of the 3D Body object, which provides a superior method of defining the component height.
• 3D Body Opacity - enter the desired opacity percentage or use the slider bar.
• Primitives - click the associated lock icon to lock/unlock. After editing, the component primitives should be re-locked.
• Strings - click the associated lock icon to lock/unlock.

Swapping Options

• Enable Pin Swapping - check to allow the pin swapping function.
• Enable Part Swapping - check to allow the part swapping function (e.g., four parts of a 74 series IC).

Schematic Reference Information 

• Designator - the designator of the schematic component to which this PCB component has been matched.
• Hierarchical Path - displays where, in the hierarchical structure of the schematic, this component can be found.
• Channel Offset - when a design is first transferred from schematic to PCB, each component on each schematic sheet is given a unique channel offset.

The Component Actions on the right-click menu of a PCB document includes commands that allow you to further configure a component. The key commands are described below.

Fanout Component

The Fanout Component command opens the Fanout Options dialog in which you can specify fanout and escape routing options. Typical fanout behavior is for used inner pads to first be fanned out using the traditional dog-bone (a short route with a via on the end) to access another layer, and then from the via, they are escape-routed out just beyond the edge of the device, working through the available routing layers until all pads have been escape-routed. Ultimately, this makes routing connections to them much easier.

Manage 3D Bodies

This command opens the Component Body Manager dialog in which you can manage the 3D bodies for components interactively. It provides a central console with which to quickly modify 3D Body attributes.

Configure Pin/Part Swapping

This command opens the Configure Pin Swapping dialog in which you can configure swap settings for the pins and subparts of each component on the board. Use the dialog to enable or disable pin/part swapping and assign or change swap groups.