Quick question: in footprint names like QFN-32-1EP_5x5mm_Pitch0.5mm, what does the “1EP” stand for? A bit of searching turned up that “EP” stands for “Exposed Pad” (i. e. a thermal pad), but what does the “1” mean?
The one stands for the number of pads. Yes there are special footprints that have more than one such exposed pads.
5 Likes
These are the power and RF parts that have a central pad between the usual perimeter pads. Most of these parts have a single pad beneath the package.
The larger ones sometimes subdivide the pad into four with mask for solder paste, for better levelling
1 Like
Would that be considered 4EP, or is it still 1EP since it’s physically one pad?
Take a look at the DFN-44-1EP_5x8.9mm_Pitch0.4mm
1EP power pad, actually 16 sub-pads overlapping and each with their own solder paste aperture
2 Likes
Atleast for myself. Subdividing for solder paste purposes is generally 1 continuos pad (the edges touch or overlap) just with a reduction in the paste apetures.
Weird RF packages can have multiple pads that need to be tied to different things. This i would consider more than 1
2 Likes
That’s also my understanding.
In addition: subdividing paste does not need to subdivide copper. I generally would suggest to use one large copper pad and multiple small paste pads on top of it. (The paste pads do not even need a pin number.)
This way you can be sure you have the correct size for the copper pad. Otherwise you need to trust in your math skills.
2 Likes
Unless the component manufacturer recommends otherwise, there should be as many copper pads on the PCB as there are exposed pads on the component package.
If the area of an exposed pad is less than 25mm2 then one stencil aperture is sufficient. If the area of the pad is 25mm2 or larger then the stencil area should be divided into smaller apertures such that the individual aperture areas are less than 25mm2. Apertures can be rectangular or circular and while 25mm2 is generally the maximum aperture size it is permissible to have a larger number of smaller apertures. For instance if 4 apertures results in aperture areas that are less than 25mm2 it would still be permissible to increase the number of apertures. The total area of all apertures should be 50% to 70% of the area of the exposed pad, in some cases as high as 80%, depending on stencil thickness.
There are several reasons for dividing a stencil aperture into smaller apertures. It reduces scooping, where the squeegee deforms into the aperture opening and scoops out some of the solder paste. It helps prevent tearing of the solder paste which occurs with larger apertures. It provides better paste release. And it helps reduce voids by providing channels for outgassing which occurs during reflow.
Never assume that a footprint in any library is correct for the component you intend to use with it. Always check them for compliance with both general guidelines and component manufacturer recommendations. Two components in the same package can sometimes require different footprints.
3 Likes