It is an inductor where the datasheet asks for 2 long pads but with only the ends of the pads being exposed for soldering to.
The question was - How to do this ?
If you look at the footprint information supplied:
You can see from this footprint that the shaded area (which is solder resist) effectively separates the 2 long pads into 4 smaller exposed pads where each pair are joined together under the resist.
This can easily be achieved in CADSTAR by adding 4 pads and connecting them together using component copper, I shall show you how.
First figure out from the drawing how big the 4 pads need to be and add 4 rectangular pads so that the left 2 are pads 1 and 3, the right 2 are pads 2 and 4 as follows.
(The reason for this is that the inductor symbol has only 2 terminals so you can identify them as pads 1 and 2.)
That will provide you with the required 2 large copper pads but with 4 exposed areas, however as far as your netlist goes pads 1 and 2 are connected to your circuit, pads 3 and 4 are not and you will get component copper to pad errors.
To prevent these errors and connect pads 1 and 3 together with the copper, in the copper properties enter the pad numbers (identifiers) for both pads.
What this will do is electrically connect them together, so in the part you only need to allocate pin 1 and 2, then when connecting to pin 1 - pin 3 is connected via the copper (Max pins = 2).
You can only connect 2 pads together like this so if you are wanting to connect more than 2 together you simply use more pieces of component copper and daisy chain them together etc.
So you will end up (once you have added the outlines etc) with a component footprint that looks like:
For similar components - perhaps where the datasheet calls for a pad shape not supported by CADSTAR, you can create the shape with component copper and attach it to a pad that covers as much of it as you can, 99 out of 100 time this is more than adequate for the component.
Any problems - post a comment.
When creating the symbol it must have only 2 terminals, using 4 will enable you to add 4 nets to it in the schematic and in the PCB it will need to be only 2 - 4 will produce an error.