PlaceEmbeddedBoard

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 that the PCB is to be manufactured from) 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 is accessed from the PCB Editor by choosing the Place » Embedded Board Array/Panelize command, from the main menus.

Use

After launching the command, the Embedded Board Array dialog will appear. Use this dialog to choose the reference PCB document, and configure the array as required. After clicking OK, the cursor will change to a cross-hair and you will enter embedded board array placement mode. Placement is made as follows:

• 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 and click, or press Enter, to place the array.
• The Embedded Board Array dialog reappears. Configure another array to place, with the same or different reference PCB, or click Cancel, or press Esc, to exit placement mode.

Additional actions that can be performed during placement are:

• Press the Spacebar to rotate the array anti-clockwise. Rotation is anti-clockwise and in steps 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 dialog:

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

Continuing to place the array will cause a warning dialog to appear. You have the choice to manually resolve the discrepency at a later stage, whereby 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 acheive 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'll only be a small cross presented in the workspace, to mark the lower-left corner of the array boundary. This cross appears in the color of the layer on which the array resides.
2. Control the display of embedded board array objects in the workspace, using the Show Embedded Board Arrays option, on the Show/Hide tab of the View Configurations dialog.
3. While attributes can be modified during placement (in the associated properties dialog), bear 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: 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.

Use

After launching the command, the Design View dialog will appear. Use this dialog to configure the view as required. You can create a view of an area of the current board, or of a different, referenced board. The region for the view can be defined interactively in the workspace, or textually in the dialog - by submitting a width, height and location of the lower-left corner of the image. You can determine the scale of the view, and also which layers are to be displayed within it.

Once the area has been defined, click OK to place the design view in the workspace.

Additional actions that can be performed during placement are:

• Press the X or Y keys to mirror the view along the X-axis or Y-axis respectively.
• Press the L key to flip the view to the other side of the board.
• Press the Tab key to access the Design View dialog, from where properties for the view can be changed on-the-fly.

Tips

1. Control the display of design view objects in the workspace, using the Show Design Views option, on the Show/Hide tab of the View Configurations dialog.
2. While attributes can be modified during placement (in the associated properties dialog), bear 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.