Guideline 3: Treat an exposed heatsinking pad (if required) as a separate and unique terminal pad having the ultimate number in the terminal sequence. Create the pad with slightly smaller dimensions (say, 0.1 mm in length and width) than the corresponding area of the package's exposed heatsink flag.
Specialized SOIC and QFN power packages have an exposed heatsinking flag that allows for the direct flow of heat from the bottom of the IC die to the PCB. For this to be effective, the PCB must have a corresponding exposed pad area with through-hole vias to sink the heat to a larger plane of copper (either on the bottom of the PCB and/or in interior layers of a multilayer PCB). Being an irregular shape, the exposed pad will need to be created as a polygon.
Take care to choose a line width narrow enough to produce the detail, but not so narrow that the figure eats up large amounts of CAM tool-processing time. (Remember, the polygon will be filled by drawing-in the interior using lines the same width as used to draw the polygon itself.) Some liberties may be taken to simplify small, complex features of the exposed pad, and care must be taken to maintain a minimum clearance with the perimeter pads of at least 0.2 mm.
Before you continue, don't forget to delete the temporary reference line from the top copper. Designing the top copper for this pad isn't difficult, but the design of the corresponding solder-mask-stop layer and solder stencil layer for the exposed pad is somewhat tricky.
Top Solder-Mask Stop: After completing the top copper layer, the next logical step is to create the top solder-mask-stop layer's artwork. The solder mask covers the areas of the board where you don't want solder to adhere. Therefore, the soldermask stop comprises the apertures within the solder mask where the copper will be exposed for soldering.
There are two scenarios for the relationship between the copper pads and the solder-mask stop: The mask-stop aperture may be less than or equal to the corresponding copper pad's dimensions, or the mask stop may be greater than those dimensions.
In the first scenario, the pad is considered to be solder-mask-defined (SMD). That means the mask defines the solderable area of copper, since it overlaps it. This is advantageous in prototyping because it creates a trace that's doubly affixed to the PCB substrate and is therefore less likely to delaminate under the abuses of multiple desoldering and resoldering. It also supplies added protection against solder bridging and other shorts in the prototype.
In production designs, though, SMD pads for small terminals are undesirable. This is because the solder-mask edge on top of the copper pad creates a stress point in the solder joint that may crack when subjected to long-term temperature cycling. For this reason, in the production design, the stop-mask apertures should be larger than the pad dimensions to produce an open periphery of about 0.065 mm around the copper pad. This scenario is called non-solder-mask-defined pads (NSMD).
Guideline 4: Use SMD pads for finepitch leads when prototyping, and change them to NSMD pads when going to production.
In this PCB prototyping example, the SMD technique should be used. The easiest way to do this is to set the soldermask-stop apertures equal to the copper pad dimensions. If the PCB-layout software you're using automatically generates the stop masks, set its maximum size limit equal to the pad itself (that is, no growth in dimensions). It's also easy to create copper rectangles slightly smaller than the pads by zooming in and setting the resolution to finest. Then, draw the apertures on the top-stop layer while viewing and tracing inside the outline of the top-copper pads.
Once you've created the different pad rectangles, simply copy and paste them inside the pads. The large exposed pad polygon can be copied/cut and pasted as a whole entity into the top-stop layer. Figure 4 shows a zoomed-in view of one of the corners of the footprint with the top-copper and top-stop layers active in the PCB-layout software. Note that the rectangular pad has a top-stop opening (shown as yellow) that's slightly smaller than the pad (shown as gray), making this a solder-mask-defined pad.
Solder Stencil: The next step is to create the artwork that defines the solder-stencil layer. This stencil is used in a screenprinting process to precisely apply the solder paste to the pads on the PCB. The stencil is placed in intimate contact with the PCB surface; the pattern of holes should perfectly align with the pattern of copper. Then a rigid squeegee is used to force the solder paste through the stencil and onto the PCB. Even in a completely manual process, several boards per minute can be "printed" with solder paste, readying the boards for component placement.
Two factors determine the amount of solder paste applied to an area on the board—the area of the openings in the stencil, and the thickness of the stencil. Laser-cut, stainless-steel stencils for a prototype PCB can be obtained at the same time as the PCB. They're also available via Internet-based companies. A common thickness for such stencils is 6 mils (0.006 in.), which is sufficiently rugged to withstand indefinite use in a manual process. We'll assume this thickness as you design your stencil artwork layer. |
