-
- News
- Books
Featured Books
- smt007 Magazine
Latest Issues
Current IssueIPC APEX EXPO 2024 Pre-show
This month’s issue devotes its pages to a comprehensive preview of the IPC APEX EXPO 2024 event. Whether your role is technical or business, if you're new-to-the-industry or seasoned veteran, you'll find value throughout this program.
Boost Your Sales
Every part of your business can be evaluated as a process, including your sales funnel. Optimizing your selling process requires a coordinated effort between marketing and sales. In this issue, industry experts in marketing and sales offer their best advice on how to boost your sales efforts.
The Cost of Rework
In this issue, we investigate rework's current state of the art. What are the root causes and how are they resolved? What is the financial impact of rework, and is it possible to eliminate it entirely without sacrificing your yields?
- Articles
- Columns
Search Console
- Links
- Events
||| MENU - smt007 Magazine
QFN Layout Guidelines
December 31, 1969 |Estimated reading time: 4 minutes
By Duane Benson, Screaming Circuits
While quad flatpack, no leads (QFN) and dual flatpack, no leads (DFN) packaged parts are becoming more common in new component releases, they aren't getting easier to use. Their form-factor advantages are clear they allow smaller geometries, better grounding, and improved thermal properties over other types of surface mount packages. Most QFNs have a center metal pad on the underside of the part, typically for grounding or heat conduction. It's this center metal pad that makes this form factor so difficult to use.
QFN FloatI recently received a sample part in a 3- × 3-mm QFN package. While I haven't tried it, I'm pretty sure that, like a water bug, the part is light enough to float on the surface of the water because it doesn't have enough weight to break the surface tension. But, that's not the "float" to which I'm referring. The middle of the part has a metal contact pad like most QFN packaged parts. It may be there for grounding or heat conduction, depending on the part specifics. This float happens when there is too much solder paste on the PCB for that center pad. To a small extent, the height of the solder paste deposit is proportional to the aperture in the solder stencil opening (bigger opening = taller deposit). With most parts, that isn't a problem because all of the pads are big enough so that that ratio doesn't have a first-order impact, or all of the pads are the same size and will be impacted equally. Because the QFN center pad has a larger opening in the stencil than the signal pad openings, and the signal pad openings are in the 1020-mil or less range, this deposit height-to-width ratio will have a first-order impact.
When the opening for the center pad on the QFN is too large, the solder paste deposit in the center will be taller than the deposits on the small signal pin pads. The part high-centers and never has the opportunity to contact the signal pads. In some cases, the part will tilt sideways and contact some of the signal pads, but not all of them.
Solder Paste StencilTypically, the signal pads should have a standoff height of 23 mils after assembly. If too much solder is deposited in the center, the part can float up beyond that height and prevent the signal contacts from connecting. To prevent this, the solder stencil opening should be broken into a series of smaller openings, and should cover between 50 to 75% of the pad area.
This means that when you layout your PCB, you must look at the solder paste layer for your QFN components. If the solder paste layer in the computer-aided design (CAD) package part library follows the copper pad pattern or the soldermask opening, you may need to customize the CAD package part library to avoid trouble. To better illustrate the proper way to make your solder paste stencil for QFN parts, I examined images of good and bad solder paste stencil practices. In the worst-case stencil image, the actual size for this part was 7 × 7 mm. However, the center pad has much more surface area than the row of side cutouts. With most SMT components, it is standard procedure to reduce the size of the paste cutout area in the stencil. In this case, it is difficult to reduce it enough and still obtain even paste distribution. The best option is to segment the solder stencil area.
By simply reducing the paste opening aperture and providing one smaller opening without segmenting it, you may end up with a part that is still too high in the middle to ensure good contact on the signal pads. The part also may be unstable and likely will tilt. With leaded solder, a single 50% sized opening may work because of the wicking properties of lead-based solder. Since lead-free solder does not wick as well, this technique is very unlikely to work in a RoHS-compliant process. In both cases, the most consistently reliable method is to segment the stencil pattern.
This is an example of recommended practice. 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. This will give good solder distribution, with little chance of high-centering or outgassing problems. When you reduce or segment the solder paste stencil pattern, do not do the same with the soldermask. Assembly works best with an even distribution of solder, and masking part of the pad area will work against good assembly.
Specialized Copper PadsSome parts, especially high-frequency parts, require a segmented copper pad under the QFN. If this is the case, it is important to segment the solder paste stencil to match the custom pad. It is a fairly common practice to use a standard full-size square opening and hope that surface tension will distribute the solder in the correct places. While that may happen, the chances against it are high. For best reliability and buildability, make sure that the openings match your copper layer underneath the stencil openings. Be sure that your stencil openings only fall above the copper and not over any soldermask or bare-board sections.
ConclusionThe QFN form factor delivers a number of advantages over other SMT package form factors. It is generally a smaller part and, with the center pad, offers better grounding and thermal properties. However, these advantages are partially offset by layout and assembly difficulties. By following a few guidelines, you can use the parts with confidence. Check the layout guidelines in the component applications notes. Segment your solder stencil opening for the center pad. Make a custom component library for your CAD package if you need to, then design away. SMT
Duane Benson, marketing manager, Screaming Circuits, may be contacted at (866) 784-5887; e-mail: dbenson@screamingcircuits.com.