Applies to Altium Designer versions: 15.1, 16.0, 16.1 and 17.0
The Region dialog
This dialog allows you to specify the properties of a Region object. A Region, also known as a Solid Region, is a polygonal-shaped primitive object that can be placed on any layer. It can be configured to be positive (for example, placed as a copper region) or negative (for example, placed as a polygon pour cutout). By placing it as a negative on the multi-layer, it can be placed as a board cutout. It can also be used to define a cavity - used to accommodate a component that is 'embedded' within the board. In the latter instance, the region used to define the cavity is placed as part of the component footprint definition in the PCB Library Editor, and on a suitable mechanical layer.
For information on how a placed region object can be modified graphically, directly in the workspace, see Graphical Editing.
The Region dialog can be accessed prior to entering placement mode, from the PCB Editor – Defaults page of the Preferences dialog. This allows the default properties for the region object to be changed, which will be applied when placing subsequent regions.
During placement, the dialog can be accessed by pressing the Tab key.
While attributes can be modified during placement, 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.
After placement, thedialog can be accessed in the following ways:
Double-clicking on a placed region object.
Placing the cursor over a region object, right-clicking and choosing Properties from the context menu.
Using the Edit»Change command and clicking once over a placed region object.
Region dialog - Graphical tab.
Use the dialog's Graphical tab to modify graphical properties of the region object.
Locked - enable this option to protect the region from being edited graphically.
If attempting to graphically modify an object that has its Locked property enabled, a dialog will appear asking for confirmation to proceed with the edit. If the Protect Locked Objects option is enabled on the PCB Editor – General page of the Preferences dialog, and the Locked option for that design object is enabled as well, then that object cannot be selected or graphically edited. Double click on the locked object directly and disable the Locked property, or disable the Protect Locked Objects option, to graphically edit the object.
Keepout - this option is only available when Kind is set to Copper. Enable it to define the region as a keepout. A keepout object is used on a signal layer to create a layer-specific keepout. Layer-specific keepouts are not included during output generation.
Kind - Choose the function of the region:
Copper - this kind of region is a solid, positive area, that can be placed on any design layer, such as a signal (copper) layer.
Polygon Cutout - this kind of region functions as a polygon cutout, defining a negative, or no-copper area, within a polygon. Repour the polygon after placing a Cutout.
Board Cutout - this kind of region functions as a board cutout, defining a negative area, or hole, within the board shape.
Cavity Definition - this kind of region is used to define an embedded cavity, within which a component will reside 'inside the board'. A region of this kind can only be placed on a suitable mechanical layer and must completely enclose the 3D body of the component, with sufficient clearance on each side. Check with the fabricator to find out how much clearance is required.
Note that the Cavity Definition kind is only available when placing a region within the PCB Library Editor.
Layer - this field is only available when Kind is set to either Copper, Polygon Cutout, or Cavity Definition. Use it to specify the layer on which the region is placed. For a Copper region and Polygon Cutout, all defined (and enabled) layers for the active board design will be listed in the drop-down list. For a Cavity Definition, only enabled mechanical layers will be listed.
Net - this field is only available when Kind is set to Copper. Use it to choose a net for the region. All nets for the active board design will be listed in the drop-down list.
Outline Vertices Tab
Region dialog - Outline Vertices tab.
Use the dialog's Outline Vertices tab to modify the individual vertices of the currently selected region object. You can modify the locations of existing vertices, add new vertices, or remove them as required. Arc connections between vertex points can be defined, and support is also provided for exporting vertex information to, and importing from, a CSV-formatted file. You also can adjust the position of the region object by globally applying delta-x/delta-y values to all vertex points.
Vertices Grid - the main region of the tab lists all of the vertex points currently defined for the region, in terms of:
Index - the assigned index of the vertex (non-editable).
X - the X (horizontal) coordinate for the vertex. Click to edit.
Y - the Y (vertical) coordinate for the vertex. Click to edit.
Arc Angle - the angle of an arc that is drawn to connect this vertex point to the next. By default, connections are straight line edges, with this field remaining blank. Click to edit then enter an arc angle as required. Entry of a positive value will result in an arc drawn counter-clockwise. To draw a clockwise arc, enter a negative value.
Straight line edges are used to connect one vertex point to the next. If you would rather have an arc connection, simply enter a value for the required Arc Angle. Entry is made in the field associated to the source vertex point, with the arc being from this vertex to the subsequent vertex below in the list.
Multi-cell selection and editing is also supported (within the same column) using standard Ctrl+click, Shift+click, and click&drag techniques. To edit multiple selected cells, use the Edit command from a menu. The focused cells in the selection (distinguished by a dotted cell outline) will be in "in-place" editing mode. Type the required value then press Enter (or click away). All cells in the selection will be updated to have that same value.
Add - click this button to add a new vertex point. The new vertex will be added below the currently focused vertex entry (as distinguished by a dotted outline around a cell in its row) and will initially have the same X,Y coordinates as the focused entry.
Do not be concerned if the new vertex is inadvertently added at the wrong position in the overall list of vertex points. You can use the Move Up and Move Down commands on a menu to adjust as necessary.
Remove - click this button to remove the currently selected vertex entries in the list. This command will be unavailable if there are only two vertices present for the region then click Remove.
To remove multiple vertices, simply select them as required using standard multi-select features (Ctrl+click, Shift+click, drag-select) then click Remove.
Menu - click this button to access a pop-up menu containing the following commands:
Edit - right-click on a coordinate cell (X or Y) for a vertex, or its associated Arc Angle cell, and use this command to edit the value in that cell. Alternatively, click directly on the cell.
Multi-cell selection and editing also is supported (within the same column) using the Edit command. The focused cells in the selection (distinguished by a dotted cell outline) will then be in "in-place" editing mode. Type the required value then press Enter (or click away). All cells in the selection will be updated to have that same value.
Add - use this command to add a new vertex point. The new vertex will be added below the currently focused vertex entry (as distinguished by a dotted outline around a cell in its row) and will initially have the same coordinates as the focused entry.
Remove - use this command to remove the currently selected vertex entries in the list. This command will be unavailable if there are only two vertices present for the region.
Copy - use this command to copy the content of the selected cells in the list to the clipboard (alternatively use Ctrl+C).
Paste - use this command to paste the content of the clipboard into the list, starting at the selected cell (alternatively use Ctrl+V).
Export to CSV - use this command to export all vertices to a CSV-formatted file (*.csv). The full list will be exported. There is no need to select anything prior to launching this command. Use the subsequent Export Outline Vertices dialog to determine where and under what name the file is to be saved.
Import from CSV - use this command to import vertices from a CSV-formatted file (*.csv). Use the resulting Import Outline Vertices dialog to browse to and open the required CSV file. The contents of the file will completely overwrite existing vertices in the Outline Vertices tab.
The vertices can be modified as required externally in your chosen spreadsheet editor. Once modified, import the new vertex information using this command.
Select All - use this command to quickly select the entire grid contents of the list.
Select Column - use this command to quickly select the entire column in which the currently focused cell resides.
Move Up - use this command to move the selected vertex upward in the list.
Move Down - use this command to move the selected vertex downward in the list.
Move By XY - use this command to move the entire region object within te workspace. The Move By dialog will appear in which you can enter the increment value to be applied to each vertex point X and Y coordinates.
Using the Select Column and Select All commands, in conjunction with the Copy command, you can also quickly take vertex information into an external editor, and then use the Paste command to bring modified information back in.
All of the above Menu commands are also available from the right-click context menu associated to the main list region.
Quickly change the units of measurement currently used in the dialog between metric (mm) and imperial (mil) using the Ctrl+Q shortcut. This affects the dialog only and does not change the actual measurement unit employed for the board, as determined by the Measurement Unit setting in the Board Options dialog (Design » Board Options).