Update Free Primitives

Save a copy of your Design before using Update Free Primitives From Component Pads !

Design > Netlist  > Update Free Primitives from Component Pads

Component footprints with irregular pad shapes can be created using any of the design objects available in the library editor.

You should be aware that the tool automatically creates solder and paste mask features based on the shape of the pad objects.

If Pad Objects are used to build irregular land patterns then the matching irregular mask shapes will be also be generated.  

Building irregular pad shapes from objects such as fills, solid region(s), line (tracks) or arcs will require solder and paste masks to be defined manually by placement of appropriately constructed objects on the solder mask and paste mask layers.

Example:

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 cross hair 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 easiest  way to do this is to use the Update Free Primitives From Component Pads... command from the Design » Netlist menu. 

Gotcha's: 

Let's say you have a shield outline or some other free primitives in your PCB. Any net that the free primitives happens to be touching will be inherited and the results may not be what you had hoped for.