This dialog is displayed when the Properties option is chosen with an Area Item selected. It shows and allows you to modify the restrictions for the selected Area Item.
Shortcuts
Default Keys: I or Alt+Enter
Default Menu: Edit
Command: Properties
Locating this option
Available from: Edit menu > Properties option
Available from: Context menu > Properties option
Available from: Shortcut key > I
Using Areas
Areas are used to Keep In or Keep Out PCB layout design item types such as Tracks, Vias, Testpoints and Components. Use Insert Area to see how to add an area.
You can use an option within Design Rule Check to find any items that disobey these Keep In**Keep Out** Rules.
Using the Area Properties Dialog
Name
An area in a design can have an optional unique name. You can then refer to this name. For example, you can post process a named area. You can also name areas in footprints and symbols. Named areas can be referred to in Spacing and other rules
The box is checked if the name is visible. Note that it will only be visible on screen if the ‘Item Name’ attribute is also set to displayed in the Colours Dialog.
Design Extents
An area can be marked as defining the design extents. All such marked areas which not within a symbol, define the extents when the View Extents command is used.
Keep In/Out
As well as explicitly assigning Keep In/Out restrictions directly on the area, you can also define Area Rules which are applied in addition to these restrictions.
Use the drop down lists to change the restriction applicable to the category of layout item. There are three restriction categories.
Keep In means that this category of item should only be allowed to placed in this area (or other areas with the same restriction).
Keep Out means that this category of item should not be allowed to placed into this area.
Keep Exclusive means Keep Out, except for tracks or Vias on tracks which originate from a pad in the area. This rule type is only available for Tracks, Vias or Micro-vias
Note: explicit Keep Out Areas take priority over any matching Component Place Rules. Whereas, explicit Keep In Areas are overridden by any matching Keep In rules.
When using Keep Out for Components you can use the If Higher Than box to apply a height restriction to keep out components greater than the supplied height. Within a footprint, if the area is also marked as a Body, then this defines the component body to be at the height above the board. This allows other, lower components to be placed underneath.
Note: if no units are added to the end of the height value, it will use the units of the design when used.
Note: the keep out of Component Pads does not include Mounting Holes, Component Vias or Die Pads or Micro-via, these are defined items.
Unrestricted means that this area has no constriction on the placement of items of this category.
If your design contains Micro-via spans, then an additional control will appear next to the Via control for Micro-vias. Vias and Micro-vias are handled completely separately for Keep In or Out areas.
Copper Keep Out
Check this box if it is an error to have any copper item in this area. This includes pads and text, but not tracks, vias and component vias which are checked separately. The check does not apply to items in the same footprint.
Drill Keep Out
Check this box if it is an error to have drill hole in this area. Only the actual hole is checked, not the surrounding pad. THis check does not apply to holes in the same footprint.
Set All Keep Out/in
This button provides a quick way to set all the Keep In/Out options on the dialog.
Power Planes
Copper Pour Avoid
Check this box if poured copper is not allowed inside the area. Use this to prevent copper from being poured under components.
Power Plane Avoid
Check this box to create a void in any power plane which crosses this area.
Alternative Thermal Gap
Check this box to create a shape which will be used as the thermal gap for a pad on a power plane or poured copper plane. If the centre of a pad is within the area, and a thermal pad is required, this shape is used instead of the gap defined in the Thermal Rules.
Board Cutout
Check this box to create a cutout in any surrounding board outline. A board cutout must be on the Through Board layer. This area will be treated as a board cutout for all checking and drawing purposes. There is an optional plated flag. Plated and non-plated cutout areas can be processed separately.
Override Within Area
Use in Area Based Styles, Spacings and Rules
Use this check box to specify that the area can be used to override the spacings, default styles and rules used within it. For example use it on areas within a BGA component to allow tracks to be thinner and placed closer together to be able to break out of the tight pad pattern.
The spacings are overridden by matching the areas name to the area name specified in the Match Pair Spacing Rules.
The default track and via styles are overridden by matching the area name to the area names defined in the design technology Net Styles entries. There are Options which determine how the track style change should take place.
This override checkbox also needs to be checked to allow Differential Pair Gaps by area.
See the Rules By Area help page for more information on using areas this way.
The rules are overridden by matching the area name to the area names defined in the design technology area based rule entries.
Only check this box on named areas that need different styles, spacings or rules to the rest of the board, as it will slow down some interactive operations if too many areas need to be checked when adding tracks and vias.
Use in Footprint Rules
Use this check box to indicate that the area name can be used in Footprints Rules to restrict a rule so it only applies to components positioned within this area of the side of the PCB board specified by the remainder of the rule.
Component
These controls are only available for an area in a footprint. They define the limits of the component body and the required clearance around the component. The visibility of these areas can be controlled on the layer class.
Placement Clearance
An area nominated to be a Placement Clearance area, defines the area required around the component. For example, you may require a space along the sides of the component to allow for the jaws of a placement machine. The body area of another component cannot overlap with this Clearance area. Clearance areas may overlap as long as the body areas are legal.
Body
The component body is the shape of the actual component and is used to determine if something (such as a testpoint) is underneath the component.
Check this box to specify the area as a Body. This area (or areas) is used in the automatic placement of components and for checking the component to component spacing. The rules are applied such that neither a body, nor a Placement Clearance area, of another component may overlap a body. Also, Body areas must be at least the Component to Component spacing apart.
Body Height
Use the Body Height: box to specify the height of the component body. This height will be used in checking against component keep out areas. Note: if no units are added to the end of the height value, it will use the units of the design when used.
Note that if no Body or Clearance areas are defined, the bounding box of any documentation (e.g. silkscreen) shapes is used.
Model Placement
An area marked as a Model Placement area is used for aligning STEP models when using the Output STEP File option or displaying it in the 3D Viewer. The relative height and width of the area is used to determine the correct orientation of the STEP model with respect to the overall height and width of the footprint.
Rules
The rules pane will display any specific rules associated with the selected Area.
Related Topics
Insert Area | Design Rule Check | Spacings, Styles and Rules By Area | Technology - Area | Technology - Layer Class | Technology - Testpoint Rules | Technology - Spacing Rules | Technology - CAM Plots