Display Your Know How: Footprints

Paste pattern is related to reflow. We would use the manufacturer's data sheet recommendation and have our assembly shop review.

The pad can be tied into a copper shape for heat dissipation if required. This can be determined by calculating the thermal resistance.

Every Contract Manufacturer (CM) I have ever worked with wants option B. I believe this was originally born out of the fact that squeegee blades on solder paste screening equipment wasn't always a steel blade. It was sometimes a flexible blade and it would deform down into the larger stencil opening of option A and scoop some of the paste back out of the aperture, leaving you with less paste on the pad then intended. Since most squeegee blades tend to be steel now, I'm not sure that this is much of a concern.

The current reason to use option B in my opinion is to control the amount of paste deposited so you keep all the paste migrating to the intended pad. Option A has the risk of applying too much paste and having solder balls form and going elsewhere on the design during reflow. Our entire library is done based on option B and trying to maintain a minimum of 60% pad coverage which I believe is an IPC requirement. CM's still prefer option B as well.

There is no simple answer to this question. B is going to be a better option for most requirements but the split shown will only give about 30% paste coverage. Using fewer larger tiles would increase the percentage.

Using too much paste risks the device "floating" on the pad which may cause solder balls and/or the remaining pins to be lifted away from their pads resulting in opens. Using too little paste may cause the joint starvation and reduce power and thermal transfer.

Don't trust data sheets for paste. In my experience they rarely match real-world requirements. Ask your manufacturer for guidelines and work with them for the best compromise.

Both of these footprints will work however none of them are optimal. For SMD components your better off using rounded or concave rectangles for the pads. The main reason pertains to the stencil. Laser's cant create square corners. With standard rectangular footprints the paste cant fill the corners due to the way the paste stencil is made.

Best Regards.

Good points eDAve, thank you for your contributions to the discussion! 

We reviewed this paste footprint and agree that yes the total area of paste looks a bit lower than the 50 -60% target for Thermal pads. Therefore we have created the following option C based on this larger area target. Let us know if you would agree with this and any further experience or thoughts on this option: