How to create a pad with three PTH holes?

[dean]

I'm trying to create a library entry for a large 3Pin PTH Phoenix Connector needed for a project. The part no is PC 5/3-GSF-7,62.

I can't find a way to design the three large pads that each will contain three PTH holes for each pin. ( Each pin in this connector is like a large fasten tab with three legs presumably because of the large current capability of this connector. 

If i place three separate pads per pin then i guess the schematic package will need three separate connections for each pin and this is messy at best as it will become a 9pin connector!!

Any ideas??

[Anonymous]

Hello Dean, This is a common problem and luckily has a common solution.

What is typically done is to create a package with as many PHYSICAL pads as needed, in your case you create 9 PTH at the appropriate locations.

Then, you create a symbol with the correct number of LOGICAL pins, in your case a 3 pin connector symbol.

Finally, when you go to create the device (joining the package and symbol) when you click on the connect button to specify how the pads and pins are connected. You can use the "Append" button to make more than one physical pad connect to the same logical pin.

So first, you select the first pad and the first pin and click "connect", then you can click the second pad and click "append" and now both PTH will be connected to the same pin on the schematic. Repeat as needed for as many pads as you need connected. Take note also of the symbol shown in the list of connections, you can click that little symbol to select between "all" or "any" which determines the requirements when connecting traces. Any indicates that a trace can connect to any one pad, while All requires a trace to connect to all of the pads on the same net. For high current applications like this you may want to use "All" while for say, a shielded connector with 6 shield connections you may desire to connect to only one.

[dean]

Many Thanks Nicholas54, I did not see the significance of the append button in the connection box! One final question, the three connected pads per pin will probably overlap each other due to the large pad required especially as two of the three connected pads per pin are on a very small pitch. Will this cause DRC errors or will the software see that they are now connected on the same net?

[jorge_garcia]

Hi dean,

Thank you for your participation, if memory serves you won't get a copper violation however if the drills of these pads are too close you will still generate a DRC violation.

If you do get a copper violation, this will not stop the board from generating gerbers our producing any other form of manufacturing output. Remember that you can always approve DRC errors.

Let me know if there's anything else you need.

Best Regards,