Thermal Vias 4

[rgraceati]

I am using a voltage regulator in an LLP-16 package from National Semi. Application Note AN-1187 recommends using "Thermal Vias" placed directly in the pad. The instructions from the AP note are below and are very confusing to me. I need help with the vocabulary. Can anyone hep me understand the terms "barrel plating", "plug the via" and "tented with solder mask" in the below paragraph?

Thanks

AP-Note AN-1187 excerpt

"An array of vias with a 1.27 mm pitch is shown in Figure 6. The via diameter should be 0.2 mm to 0.33 mm with 1oz. copper via barrel plating. It is important to plug the via to avoid any solder wicking inside the via during the soldering process. The thermal vias can be tented with solder mask on the top surface of the PCB. The solder mask diameter should be at least 75 microns (or 3 mils) larger than

 

[Comcokid]

Copper conducts heat very well. Under surface mount power devices, a grid of closely spaced via holes (in this case 1.27mm center-to-center) is generally placed to conduct the heat from under the device to the ground plane on the opposite side of the board.

In standard PC board manufacturing, a plating process is used to plate the thru holes for components and vias. A PC board manufacturer will start with a board that has a 1/2 or 1 oz copper thickness and plate it. This both plates the holes and thickens the etch copper to the final desired thickness. For this via, they are indicating the plating process should add the equivalent of 1 oz thickness to whatever base thickness is used.

A part that has a ground tab directly attached to the board will have a CAD PCB footprint that supresses the solder mask under the device and has a opening for solder paste in the stencil. In the reflow solder process, the solder will attach the part. However, you don't want the vias to allow solder to wick through them onto the opposite side of the board. This might pull too much solder and leave voids under the part. The voids will impare the thermal transfer from the ground tab to the PCB. To avoid this, the vias on the opposite side of the board will be "tented" - that is covered by solder mask so only a minor amount of solder will flow into the via but not out the opposite side. In some high-end applications, epoxy or some other material may be used to fill or "plug" the via.

 

[Skogsgurra]

Exactly. Very well described. PLS for you.

Gunnar Englund

http://www.gke.org

 

[rgraceati]

Thanks for the explanation. This helps alot.

 

[LionelHutz]

They are saying to cover the via's with the solder mask on the top side of the board with is usually the component side, as opposed to the back side of the board. They also say to tent the via's so that solder does not wick inside the via, which also seems to support this.

The last line probably completes as saying the mask should be 3 mils larger than the via??

When you do this you need the via's to connect to a plane on the opposide side of the board. An internal ground plane doesn't dissipate heat very well.