Assigning multiple pads to one pin

I think you should think about the symbol from the perspective of the footprint. What I mean is if your footprint contains 6 pads then your symbol will have 6 pins. This way when you put the symbol down on the schematic you will have a 1 to 1 electrical representation of the footprint from the perspective of a schematic netlist.

You could possibly draw the symbol the way the footprint looks. I typically avoid naming pins by name such as cathode / anode etc but go with simple naming such as 1234 for the names and 1234 for the pin numbers.

Main thing would be have symbols and footprints that match so a reliable netlest can be generated without packaging errors or pin numbering errors.

Thanks Scott

 After a few hours of intense pdf readings i have found a solution. For unconnected pins the answer is quite simple... in the Part Editor select Options-> Part Properties-> New. The name of the new property has to be NC (not connected) and the value the pads numbers separeted with comma. In my example pad 5 was unconnected so ex: Name : NC   Value: 5 (if you have multiple pads then it would be 5,6,7.....)

Assignin one anode pin to 4 different pads was a little difficult. In the part editor place down as many pins as you need in my example 4. Name them differently. After that Part Properties-> New. The name of the new property now is PACK_SHORT. The Value has the following syntax. (pin1,pin2,pin3...) where pin1, pin2,pin3 are the names of the pins you want to be connected together. Now theses pins are all connected together we just have to hide them. View->Package. After that Edit->Properties. You have to check the pins names you dont want to appear in the symbol. Ignore them. You are done. I've tried this method is works perfectly. 

Hope this will help someone else who is also strugeling with it...

Thanks Szabi