QFN CAD Libraries

In previous posts (here and here), I've talked about QFN layout issues and solder stencil openings. Here is an example of a the library that follows the component manufacturer's and our recommendations.

Qfn_copper_layer_1 First step is the copper layer. In this case, the copper layer is solid and covers the full area of the pad under the part.

 

 

Qfn_solder_mask_layer_2Next is the solder-mask area (inverted). Note that the solder mask leaves the  entire center copper pad area unmasked. I've seen a few boards where the designer tried to solve the problem by reducing the solderable area by reducing the center opening size in the solder-mask. What that will tend to do is just make the part less stable and cause it to tilt to one side or the other, almost ensuring a non-functional board.

Qfn_solder_paste_stencil_layer_good_1Last is the solder paste layer. This is pretty much a best case example. The solder paste stencil will have a series of small openings in the center, each about the same size as the signal pads on the outside edge of the chip. This gives about 50% paste coverage in the center and will result in even solder distribution and a finished part with a reliable mechanical and electrical connection all around.

If your part libray doesn't look like this, consult with the part manufacture layout guidelines first, but you will likely need to modify the component library before sending the board out for fab and assembly. Some QFN parts require a custom copper pad layout in the center too so you may need to adjust that part of the library as well.

Duane Benson
Paste well, my son

QFN solder paste stencil guidelines

To better illustrate the proper way to make your solder paste stencil for QFN parts, as I discussed in the post just before this one, I went to the back room and took a couple of photos of good and bad.

Qfn_float This is essentially what happens with too wide an opening for the center pad on the QFN. The part high-centers and never gets the opportunity to contact the signal pads. In some case, the part will cock a little sideways and contact some of the signal pads but not all.

Qfn_stencil_full_open_aperture_moddedThis is what a worst-case stencil would look like. Note how much surface area that the center pad has compared to the row of side cut-outs. Actual size for this part is 5 x 5 mm. By default, we typically reduce the size of such cut-outs already, but in a case like this, it is difficult to reduce it enough and still get even paste distribution. The proper option is to segment to solder stencil area.

Qfn_stencil_four_cut_outsThis is one example of a recommended practice. We would actually suggest even a little less coverage. The basic idea is that you distribute a lower quantity of solder over a broader area. You reduce your chances of high-centering and other problems associated with large paste areas, such as outgassing and spattering.

Just make sure that the openings match your copper layer underneath the stencil openings. Some parts require that the copper pad be segmented also. Be sure that your stencil openings only fall above the copper and not over any solder-mask or bare-board sections.

Qfn_stencil_lots_of_small_cut_outsThis is a pretty good example of how to do it properly. This will give good solder distribution with little chance of high-centering or outgassing problems.

Dfn_stencil_cut_outs_1 It works for DFN packages also.

 

 

 

Duane Benson

QFN float be bad

At a recent tradeshow, I received a sample part in a 3 x 3 mm QFN package. While I haven't tried yet, I'm pretty sure that, like a water bug, the part is light enough to float on a water surface due to not having enough weight to break the surface tension. But, that's not what I'm talking about.

In the middle of the part, like with many/most QFN packaged parts, is a metal contact pad. It may be there for grounding or heat conduction, depending on the specific part. The float that I'm talking about happens when we lay too much solder paste on the pcb for that center pad.

To a small extent, the height of the solder paste blop is proportional to the aperture in the solder stencil - bigger opening = taller blop. With most parts, that isn't a problem because either all of the pads are big enough so that that ratio doesn't have a first order impact, or because all of the pads are the same size and will be equally impacted.

With the QFN center pad being a much larger opening in the stencil than the signal pad openings, and the signal pad openings being in the 10 - 20 mil or less range, this blop height to width ratio begins to have a first order impact.

Acording to Amkor, the signal pads should have a standoff height of 2 - 3 mils. If too much solder is deposited in the center, the part can very easily float up beyond that height and prevent the signal contacts from contacting. To help prevent this, Amkor recommends smaller multiple openings in the stencil area for the center pad - approximately 50 - 80% pasted coverage.

Take a look at page 3 of an Amkor app note and page 5 of a Freescale app note for examples of how to cut down on the excess solder for better placement reliability. We strongly recommend that you follow these guidelines or similar guidelines published by your part manufacturer.

Duane Benson
I won't float your boat

Via in pad?

In general, we would recommend against placing vias in any pads that will receive solder during the assembly process. A couple of undesirable events can happen depending on the method used during board fab.

If your vias are left open, solder will tend to wick down into the via hole. The larger the diameter, the worse the wicking problem can be. You might end up without enough solder left to secure the component. You might even see a solder bump on the bottom side of the board, which could interfere with other components or lead to shorts.

If your vias are capped or partially filled, the caps might pop off due to thermal expansion or out-gassing. Internal air bubble can migrate up, leading to voids in your solder joint.

In a perfect world, we'd like to never see a via in pad. However, the real-world is saying otherwise. Manufacturers of QFN parts are starting to recommend vias in the heat-slug pad for improved thermal conductivity. High frequency designs benefit from the shortest possible routing, which may indicate via in pad. Super fine pitch BGAs may not leave any other options.

This not very helpful, but somewhat humorous thread from 2004 on the SMTnet message forum illustrates common opinion on the process. If you need to place vias in the solder area, we would recommend that you use as small a diameter as the design will allow and follow the component manufacturer's guidelines for placement and via capping or filling.

References:

We'll be watching this issue closely and pass on more hints and tips as we find them.

Duane Benson
Via le pcb assembly