Parent page: PCB Objects
A Board Region is a user-defined area of a PCB that can have a unique layer stack assigned to it. A board can be split into multiple regions by segmenting its single default region, as defined by the board shape outline, with each region assigned an individual layer stack arrangement. The layer stackups can be configured to cater for both rigid and flexible regions of the board, facilitating rigid-flex PCB design.
Board Regions can only be implemented in the PCB Editor with the View mode set to Board Planning Mode (View » Board Planning Mode – press the 1 shortcut).
The region sections are defined by placing Split Lines (Design » Define Split Line), which segment the board outline shape. A single board region (for example, that of a newly-created board) is split into two regions by placing a Split Line.
Board Regions are defined by placing Split Lines:
Board Regions are the areas between the Split Lines, and are assigned a default region name.
When a new board is created it will have a single region, and this region will be assigned the default layer stack, named
Board layer stack. When the board shape is split into multiple regions, each new region is also assigned this default main layer stack. Each board region is also given a default name, with the original region named
Default Layer Stack Region, and subsequent regions named using the format
Layer Stack Region n.
Within a board layout, Board Regions are defined by the positioning of Split Lines. The Split Line can be graphically edited by manipulating the nodes at the end of each line using a select and drag method.
To edit a Board Region by moving a Split Line:
To redefine a Board Region by removing a Split Line:
The following methods of non-graphical editing are available:
A Board Region's properties can be accessed and edited from the Board Region dialog, which is opened by double-clicking on the region. Note that the PCB editor should be in the Board Planning Mode view – View » Board Planning Mode (shortcut 1).
To give a region a more meaningful name, update the Name field in the Board Region dialog. Similarly, to assign the required layer stack to the selected region, select the appropriate layer setup from the Layer stack list. Note that one board region must have the 3D Locked option enabled to define the physical ground reference for the 3D display mode.
Click OK to accept the new setting and close the dialog.
The PCB panel allows you to browse the current PCB design using various filter modes to determine which object types or design elements are listed, highlighted or selected. It also has editing modes for certain object types or design elements that provide you with specific controls on the panel for editing procedures.
Set the PCB panel browsing mode (top drop-down list) to Layer Stack Regions. The panel shows:
To edit the properties and elements of a selected Board Region:
The PCB Inspector panel enables the designer to interrogate and edit the properties of one or more design objects in the active document. Used in conjunction with appropriate filtering - by using the PCB Filter panel, or the Find Similar Objects dialog - the panel can be used to make changes to multiple objects of the same kind, from one convenient location.
The PCB List panel allows the designer to display design objects from one or more documents in tabular format, enabling quick inspection and modification of object attributes. Used in conjunction with appropriate filtering - by using the PCB Filter panel, or the Find Similar Objects dialog - it enables the display of just those objects falling under the scope of the active filter – allowing the designer to target and edit multiple design objects with greater accuracy and efficiency.
Valid students can get their very own 6-month Altium Designer Student License for FREE! Just fill out the form below to request your Student License today.