Parent Page: PCB Objects
A polygon pour is a group design object - that is, it is made up of simpler primitive objects. Polygon pours are used to create a solid or hatched (lattice) area on a PCB layer, using either Region objects, or a combination of Track and Arc objects. Also referred to as copper pours, polygon pours are similar to a region, except that they can fill irregularly shaped areas of a board as they automatically pour around existing objects, connecting only to objects on the same net as the polygon pour.
On a signal layer, you can place a solid polygon pour to define an area for carrying large power supply currents, or as a ground-connected area for providing electro-magnetic shielding. Hatched polygon pours are commonly used for ground purposes in analog designs.
Polygon Pours can only be placed in the PCB Editor. You can place them directly, or create them from selected primitives. To place a polygon:
After launching the command, the Polygon Pour dialog will open:
As well as interactively placing a polygon, they can also be created from a set of existing track and arc objects that define a closed shape. To define a polygon from an existing closed shape:
The polygon will be created with its Fill Mode set to Outline. Note that the original selected primitives are not removed, and the new polygon is poured inside the selected objects. The selected objects can now be deleted or moved to another layer (via the Inspector panel). Double-click to repour the new polygon as solid or hatched. Note that the edge of the new polygon will lie along the centerline of the selected objects that were used to create it.
As the Create Polygon from Selected Objects algorithm uses the centerline of the selected objects, it requires that the end and start locations of touching objects are exactly co-incident (at the same location). If this is not the case a Confirm dialog will appear, giving the location where the algorithm failed, and also providing the opportunity to instruct the algorithm to attempt to define the polygon from the edges of the objects instead. As long as the selected objects overlap slightly this option should create a polygon, with the edge of the polygon tracing the outer edge of the selected objects.
There are a number of commands available to graphically modify a polygon.
Polygons contain to points, or "handles" with which to edit the shape of the polygon.
An existing polygon can be re-shaped by moving these handles, or vertices, located at each corner, or at the center of each edge.
To modify the polygon shape:
To create a cutout, or hole inside a polygon you place a polygon pour cutout on top of the existing polygon. To do this:
An existing polygon can be sliced into 2 smaller polygons, to do this:
As these are now 2 independent polygons, each can be edited and repoured as required.
The following methods of non-graphical editing are available:
Dialog page: Polygon Pour
This method of editing uses the following dialog to modify the properties of a polygon pour object.
The Polygon Pour 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 polygon pour object to be changed, which will be applied when placing subsequent polygon pours.
During placement, the dialog can be accessed by pressing the Tab key.
After placement, the dialog can be accessed in one of the following ways:
The polygon pour placement engine can construct polygons from either: solid regions, or from a combination of tracks and arcs. To help you decide which of these to use, consider the following:
Remove any areas of copper that are less than the specified area. This option is area-based only, it does not consider if that island is connected to a pad or via. Note that all small unconnected areas of copper are always removed if the Remove Dead Copper option is enabled.
In a region-based polygon circular holes are approximated by a series of straight edges, reducing this value will result in a larger number of straight edges being used to give a better approximation of an arc.
Use this to remove narrow slithers of copper. Note that when this option has a larger value there will be a greater number of tight locations where the polygon cannot pour. The value should not be smaller than the narrowest track width that the fabricator can support, as a guide it can be set to be the same as the narrowest track width used on the board.
The Net Options includes a drop down with the following 3 options:
Remove Dead Copper - if this option is enabled any area of polygon that does not include at least one connection to another net object (such as a pad or via) is automatically removed. Note that if your polygon does not enclose any pads on the assigned net, then it is all dead copper and will all be removed. In this situation the outline of the polygon is still shown to indicate that a polygon exists in this location.
To perform design tasks within a polygon, such as repositioning a component or moving routing, the polygon can be Shelved. Shelving a polygon does not remove it from the design, it is simply hidden from display and the DRC and net connectivity analysis engines.
If you have changed the design within a polygon, once it has been restored it will need to be repoured to clear any violations created by the design changes. To repour polygons:
An 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, the panel can be used to make changes to multiple objects of the same kind, from one convenient location.
A 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, 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.