Vias in Symbol

You could:

Use the Multiple Drill option in the Pad Designer, specify the Drill Size, the array count, and the edge to edge clearance for the "drills", specify the Pad details for the layers to put the drills between, Top, Bottom and Default Inner for "all". This will be one pin in the schematic and "n" (30) drills in the board

Add a copper shape for the pad in the Symbol Editor, add a Surface Mount pad within it for the connect point, use Layout>Connections, double-click to add a Via, "Done" that, and then copy that Via to form the required connections - the via should be a through, set the Parameters for the via with a "Modify Design Padstack" if your default via differs from the required via. Add Copper Shapes / Keepouts for the "other" layers if you need specific "contact" or "isolation". Set the Via Property Dyn_Thermal_Conn_Type of "Full Contact" for "solid" connections to the shape(s). You may get Via / Shape DRCs in the Symbol Editor but these will clear when a netlist is loaded into a board using these components.

To answer your questions.

The multi Drill option is used in a pad when more than one drill hole is needed. "Typical use is for a regulator tab" to remove heat to a plane.

In a multi drill pad "There are no thermal vias" It is simply one pad with holes in it.

Net connectivity is based on pin info in Allegro. So if the pin has a net name of ground and that particular pin has a multi drill padstack attached to it then it "Will connect to a ground plane or shape or any net that is named ground"

In a thermal pad there is no reason to tent the holes, that dont make sense to me. I can see dong that in vias but in this particular instance no tenting is needed.

Lastly over on the schematic side your multi drill padstack that is really only "1 Pin on a pcb footprint" can be represented as 1 pin in the schematic symbol.

Scott 

Thank you Scott

Some manufacturers such as TI recommends tenting thermal vias from the componet side to prevent voiding formulation (www.ti.com/lit/an/slma002g/slma002g.pdf‎). Or in Via in Pad Guidelines (PDF) - Screaming Circuits.

How can you make this selective soldermask over thermal pad when multi drill option is used?

Thanks

 I took a look at that app note, in the app note they talk about tenting the drill holes as a means to stop wicking of the solder paste, but if you are using 13Mil holes then tenting will be a challenge as the hole is so small. A better solution is to have the holes plated shut for small holes.

There is a dis advantage to haveing mask "Tented holes" under the bonding pad of a power part. Having mask there "Tented holes" means when the solderpaste is applied it will also cover the mask, this can lead to problems when the part goes through a reflow oven in that the solder paste will dam under the part in certain areas. The biggest issue with doing this is you are reducing heat transfer from the part.

With the multi drill pad option you can either have a solder mask built into the pad or not. If not you will have to use a shape on the soldermask layer to achieve your desired results. In other words place a Shape of the desired size to represent the mask for the pad then if you need mask over the holes add a circular shape "Void" over each hole on the mask layer.

Believe that should work. 

Scott