Insert areas in to the design using Polygon, Rectangle or Circle interactive insert options.
Areas can be used in many ways where a specific portion of the design needs to be identified. You can define rules which only apply within the area. You can also restrict a plot to an area. Within a symbol, they can define the extents of a component body.
Shortcuts
Toolbar: 
polygon
Default Keys: None
Default Menu: Insert
Commands: Insert Area Polygon
Toolbar: 
rectangle
Default Keys: None
Default Menu: Insert
Commands: Insert Area Rectangle
Toolbar: 
circle
Default Keys: None
Default Menu: Insert
Commands: Insert Area Circle
Toolbar: 
ellipse
Default Keys: None
Default Menu: Insert
Commands: Insert Area Ellipse
Using Areas
In a PCB layout, areas can be are used to Keep In or Keep Out design item types such as Tracks, Vias, Testpoints, Components and Component Pads. Once added, use Properties to change the area usage.
You can use an option within Design Rule Check (DRC) to find any items that disobey these Keep In**Keep Out** Rules.
In a Schematic design, you can define Area Attribute Rules.
How To Use Insert Area
- On the Toolbar, select Insert Area Icon. This will insert a Polygon shaped area by default (the default icon can be changed as required), or;
- From the Insert menu select Insert Area. You may then select from one of the following:
You then define the area shape within the board area. This is the basis of your Keep In or Keep Out areas. The Properties of the area must now be amended to determine which item(s) are to be either kept into this area or kept outside of this area.
Designating An Area To Be Keep In or Keep Out
Whilst adding the area shape you can right click to use the Out option from the shortcut menu. Alternatively you can use properties using the following procedure:
Select any segment of the area if it is a Rectangle or Polygon, or the complete Circle/Ellipse. Then select Properties by:
- On the Edit menu, select Properties, or (and these are the much preferred method):
- Select the shape and Right mouse click. Select Properties from the shortcut menu, or;
- Select the shape and click the Properties shortcut key.
The Properties dialog opens. Select the Area tab
In the Keep In/Out dialog, you can defined Tracks, Vias, Testpoints, Components, Component Pads, as either:
Unrestricted meaning there is no restriction on whether the item is inside or outside the area.
Keep In meaning the item will be kept within the area during processes which use it.
Keep Out means the item will be kept outside the area during processes which use it.
You can also designate an area as a Copper Keepout area, this is used by DRC to check that copper items are not within the area. Similarly Drill Keepout areas can be checked for drill holes.
You can also designate it as a Copper Pour or Power Plane Avoid area, this enables you to define voids in any poured copper or power planes which cross the area.
Board Cutout Areas
An area can be defined as a Board Cutout. For rule checking purposes, this area is part of the board outline. You can define this cutout as Plated or not plated. Plated and not plated cutouts can be post processed separately as they may be cut at different stages of manufacture. For example, you may want to plate one set of cutouts and not another set, or stamp out one set and drill another. A Board Cutout area through the whole board is on the Through Board layer. If buried or blind Layer Spans are defined in the design, board cutout areas can be placed on these spans to create Board Cavities.
Processes Which Use Keep In/Out Areas
The Keep In/Out areas are used by the following:
- Auto place - Keep Out of Components only
- Auto routing - Keep Out of tracks and vias only
- DRC - Keep In and Out of tracks, vias, testpoints, drills, components and component pads. Board Cutouts are checked as part of the board outline.
- Copper Pour - Copper Pour Avoid areas will form voids in any poured copper
- Post Process - Power Plane Avoid areas will form voids in the copper on a power plane. As power planes are usually plotted in negative, the area would be plotted as a filled shape. Board Cutouts are plotted as part of the board outline.
Override Within Area
Check the Use in Area Based Styles, Spacings and Rules 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 Net Class to Net Class 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.
The rules are overridden by matching the area name to the area names defined in the design technology area based rule entries.
See the Styles By Area help page for more information on using areas this way.
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.
Placement Body and Clearance Areas For PCB Footprints
When creating Footprints for use in PCB layout, you can also specify that an area is a Body Area. This is done by selecting the check box on the Area Properties dialog within the Footprint editor.
This body area is used by the component pushing when moving components interactively during the design process. It is used as the component boundary from which the component to component spacing is set. If this area does not exist then the component bounding box is used. The component body area is also used by the Auto Placement tool.
When using the Design Rules Check, the placement area will be used to check the component to component spacing.
Using Areas For Plotting
A named area can be used within the plotting option to define an area that should be plotted. Perhaps you require four locations to be plotted equally in each of the four corners of the plot paper. By using four named areas, you can achieve this.
Other Areas In PCB Footprints
A powerful feature of areas is that they can be defined within a footprint. This means that you will always have Keep Out areas correctly positioned under the component. Copper Pour/Plane Avoid areas will ensure that you can prevent copper flooding under the component. Add areas around a BGA footprint that override the spacings and styles used within it to help getting out of tight pad patterns. Finally, you can designate an area as a Board Cutout which is useful for defining a slot in the board. As this slot is part of the footprint it will always be positioned correctly relative to the component. Note that you can also create a slot as part of a pad style.
Related Topics
Out | Board Cavities | Insert Polygon | Insert Rectangle | Insert Circle | Insert Ellipse | Properties - Areas | Design Rule Check | Pour Copper | Spacings, Styles and Rules By Area | Split Power Planes | Define Pad Style