PlaceComponent

Applied Parameters: None

Summary

This command is used to place a PCB 2D/3D Component model from any of the Available Libraries onto the current document. A PCB 2D/3D Component model is the representation of a physical device on a PCB. It includes a 2D footprint (with such items as pads for connecting to the pins of a device, a physical outline of the package, and device mounting features), and any 3D information (through the association of one or more 3D Bodies).

Access

This command can be accessed from the PCB Editor by:

• Choosing the Place » Component command from the main menus.
• Clicking the  button on the Wiring toolbar.

Use

After launching the command, the Place Component dialog will appear. Use the dialog to choose the required PCB 2D/3D Component model. Two placement methods are supported:

• Footprint - search for a PCB 2D/3D Component model. You can enter the name for the model directly, or search for the required model across all available libraries (*.PcbLib and *.IntLib) using the Browse Libraries dialog.
• Component - search for a schematic component and then use the PCB 2D/3D Component model linked to that component (or choose the model if multiple are defined). You can enter the logical symbol name for the schematic component directly or search for the required schematic component across all available libraries (*.SchLib and *.IntLib) using the Browse Libraries dialog.

Once the required 2D/3D Component model has been chosen, set the appropriate designator and any comment text. Proceed with placement as follows:

1. Click OK - you will return to the PCB document and an outline of the component will be floating on the cursor.
2. Position the component and click or press Enter to place it.
3. Continue placing further instances of the same component or right-click or press Esc to exit.
4. The Place Component dialog will reappear. Either browse for a different component to place or click Cancel to exit component placement mode.

Additional actions that can be performed during placement while the component is still floating on the cursor are:

• Press the Tab key to access the Component dialog, from where properties for the component can be changed on-the-fly.
• Press the Alt key to constrain the direction of movement to the horizontal or vertical axis depending on the initial direction of movement.
• Press the Spacebar to rotate the component counter-clockwise or Shift+Spacebar for clockwise rotation. Rotation is in accordance with the value for the Rotation Step as defined on the PCB Editor – General page of the Preferences dialog.
• Press the L key to flip the component to the other side of the board.
• Press the X or Y keys to mirror the component along the X-axis or Y-axis, respectively (on the same side of the board).

Tips

1. An alternate method of component placement is to use the Libraries panel. The panel offers advanced search functions and the ability to drag and drop a component from the panel directly onto the active PCB document. If the Place button in the panel is clicked, the Place Component dialog will appear loaded with the selected footprint in the panel. Placement proceeds as if using the Place Component command.
2. The designator is auto-incremented as you place further instances of the same component footprint type. It is therefore advisable to set the designator to that which is required before commencing placement of the first instance.
3. While attributes can be modified during placement (Tab to bring up associated properties dialog), keep in mind that these will become the default settings for further placement unless the Permanent option on the PCB Editor – 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.

Applied Parameters: RepositionSelected=True

Summary

This command is used to reposition a number of selected components sequentially in the order that you selected them.

Access

This command is accessed from the PCB Editor by using the Tools » Component Placement » Reposition Selected Components command from the main menus.

Use

First, ensure that all components to be repositioned are selected in the design workspace. As the command works sequentially, select components progressively using the Shift+click selection approach.

After launching the command, the cursor will change to a cross-hair with the first selected component attached to it. Proceed with repositioning as follows:

1. Position the first component at the required new location in the workspace and click or press Enter to effect placement.
2. Reposition each subsequent component in the selection as required, clicking or pressing Enter to effect placement each time.
3. Once all components in the original selection have been repositioned, you will exit placement mode. All components will remain selected.

Additional actions that can be performed during placement – while a component is still floating on the cursor – are:

• Press the Tab key to access the Component dialog from where properties for the component can be changed on-the-fly.
• Press the Alt key to constrain the direction of movement to the horizontal or vertical axis, depending on the initial direction of movement.
• Press the Spacebar to rotate the component anti-clockwise or Shift+Spacebar for clockwise rotation. Rotation is in accordance with the value for the Rotation Step as defined on the PCB Editor – General page of the Preferences dialog.
• Press the L key to flip the component to the other side of the board.
• Press the X or Y keys to mirror the component along the X-axis or Y-axis, respectively (on the same side of the board).
• Right-click or press Esc to exit placement mode at any time. The current component on the cursor, and all subsequent components in the sequence, will retain their original positions on the board.

Tips

1. The ability to reposition a component in this way can also be enabled as part of the Cross Select feature. Simply enabling the Reposition selected component in PCB option, in the Cross Select Mode region of the System - Navigation page of the Preferences dialog. Then, with Cross Selection enabled, selecting a component on the schematic will select that component on the PCB, and attach it to the cursor ready to be relocated.
2. While attributes can be modified during placement (Tab to bring up associated properties dialog), keep in mind that these will become the default settings for further placement unless the Permanent option on the PCB Editor – 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.