PCB_Cmd-PlaceEmbeddedBoardPlaceEmbeddedBoard_AD

Applied Parameters: None

Summary

This command is used to place an Embedded Board Array object onto the active document. An Embbeded Board Array allows you to create a PCB panel (representing the physical board from which the PCB is to be manufactured) as part of your PCB design project. This is also known as panelization. You can use this panel to hold an array of PCBs. This command links the panel to the original PCB design files, stepping it out the specified number of times. You cannot edit the PCBs directly from the board array, only through their original files.

Multiple embedded board arrays can be placed and each can reference a different PCB file. By spacing out the boards in each array and then overlaying, rotating and flipping the different embedded arrays, any panelization arrangement can be created. This can be used to reduce manufacturing costs by maximizing the number of PCBs per panel of PCB material.

Access

This command can be accessed from the PCB Editor by:

• Choosing the Place » Embedded Board Array/Panelize command from the main menus.
• Right-clicking in the workspace then choosing the Place » Embedded Board Array/Panelize command from the context menu.

Use

After launching the command, the cursor will change to a cross-hair with an empty array boundary floating on it and you will enter embedded board array placement mode. Placement is made as follows:

1. The location of the cross-hair decides the lower-left corner of the board array. Position this corner of the array at the required location then click or press Enter to place the array.
2. Continue placing additional arrays or right-click or press Esc to exit placement mode.

Additional actions that can be performed during placement are:

• Press the Spacebar to rotate the array counterclockwise. Rotation is in increments of 90°.
• Press the L key to flip the array to the other side of the board.

Verification of Layer Stack Compatibility

When building a panel, it is important that you ensure the layer stackup for each referenced child board is compatible with the stackup for the parent board onto which the panels are placed. When you choose the reference PCB design for the embedded board array being placed, the software will compare the layer stacks of that board with that of the active PCB into which you are placing the array. The result of this comparison will be presented in the Embedded Board Array mode of the Properties panel:

• If the layer stacks are compatible, the following text will be displayed: Child and Parent PCB Design Layer Stacks are Compatible.
• If the layer stacks are not compatible, the following text will be displayed: Child and Parent PCB Design Layer Stacks are NOT Compatible.

You have the choice to manually resolve the discrepency at a later stage; a reminder will be generated if you attempt to generate fabrication output. Alternatively, you can get the software to automatically attempt to resolve layer stack compatibility issues. The automatic layer stack synchronization process will attempt to:

• Ensure that all required child board layer stack ordered layers exist in the parent board (the PCB file containing the embedded board array).
• Modify the parent board layer stack in an attempt to achieve synchronization; a child board is never modified.
• Make only additive or layer type modifications to the parent board; layers are never removed.

Tips

1. If a placed array does not yet reference a PCB document, there will be a green rectangular bounding box with the text No source at its center along with a small cross to mark the lower-left corner of the array.
2. While attributes can be modified during placement (Tab to open the Properties panel), 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.
3. After placement, properties of an embedded board array are accessed through the Properties panel. If the panel is visible, select the array to load the panel with its properties. Otherwise, double-click the placed array to open the panel.

Applied Parameters: Mode=Viewport

Summary

This command is used to place a Design View object onto the active document. A design view is a graphic snapshot of any rectangular-shaped region of the current board or another board. It can be placed anywhere in the workspace and scaled to any size.

Access

This command is accessed from the PCB Editor by:

• Choosing the Place » Design View command from the main menus.
• Right-clicking in the workspace then choosing Place » Design View from the context menu.

Use

After launching the command, a design view will appear attached to the cursor. Position the design view in a suitable location then click or press Enter to place it.

Additional actions that can be performed during placement while the design view is still floating on the cursor and before the design view is anchored are:

• Press the Tab key to pause the placement to access the Design View mode of the Properties panel from where its properties can be changed on-the-fly. Click the workspace pause button overlay ( ) to resume placement.
• Press the Alt key to constrain the direction of movement to the horizontal or vertical axis depending on the initial direction of movement. 

 After placement of the design view, you can define the display of desired layers by performing the following steps:

1. With the Design View selected in the workspace, open the Properties panel by double-clicking or right-clicking then choosing Properties from the context menu.
2. Use the Define button in the Properties panel to interactively define the area of interest.
3. In the Layers section of the Properties panel, click (toggle) the  icon to enable the display of the desired layers. When enabled in the Properties panel, the desired layer(s) will display the  icon.