HOWTO

Create a component footprint with an irregular pad shapes

From the Altium's SUPPORTcenter :

Component footprints with irregular pad shapes can be created using any of the design objects available in the library editor, but be aware that the software automatically creates solder and paste masks based on the shape of the pad objects. If Pad objects are used to build an irregular pad shape then the matching irregular mask shape will be generated correctly. However, building the irregular pad shape from other objects such as fills, solid region(s), line (tracks) or arcs would require solder and paste masks to be defined manually by placement of suitably enlarged or contracted objects on the solder mask and paste mask layers.

The following is an example of creating an irregular pad using a pad and a solid region:

Create a new component and place a pad:

• Open up a PCB library, create a new component footprint and from the menu select Place » Pad.
  As the pad is floating on the cursor before placement press the Tab key to define the pad properties. The pad dialog will be displayed, choose top layer for Layer under Properties section. Click Ok and then place the Pad. Right click or press ESC to exit pad placement mode.

Create the irregular pad shape using a solid region:

• To create an irregular pad shape using a solid region, select Place » Solid Region and assign it to the top layer. Use this to place a polygonal-shaped object to represent a copper region on the PCB board.
  
  After selecting this command, the mouse shape changes to a cross-hair. Click to define each of the vertices of the region. Click the right mouse button to finish drawing the polygon shape.

Note: When placed on a signal layer the positive region becomes an area of solid copper that can be used to provide shielding or to carry large currents. Positive regions can be combined with track or arc segments and can be connected to a net.

Next, it's necessary to define any required solder and paste masks by placing objects on the solder mask and paste mask layers

• Enable the Top Solder and Paste masks layers by pressing shortcut key “L” to display Board Layers and Colors dialog. Check the Show boxes for the Top Solder and Top Paste layers.
   
• Select the Solid Region on the top layer and copy it.  During the copy process, the cursor will change to a crosshair for the selection of a reference point. This is a coordinate relative to the selected object(s) and is used to accurately position the selection when using the paste command. Simply position the cursor as required and click or press ENTER - the selection will be copied to the clipboard.
   
• Make the Top Paste layer active, and from the menu select Edit » Paste special.  The Paste Special dialog will appear - choose the option Paste on current layer. Position the region and align it with the region on the top layer.
   
• Switch to the Top Solder layer, and follow the same process to copy the region to that layer.  There should now be 3 regions, on the Top, Top Paste and Top Solder layers.
   
• Save the library.

Once the footprint is used, and nets are assigned to the pad, the fills will need to get their net information updated. The most appropriate way to do this is to use the Update Free Primitives From Component Pads... command from the Design » Netlist menu. This should look at each pad's net and the tracks, fills, etc connecting to the pad and then it assigns the pad's net to the connected tracks or fills.