I was working to complete a KiCad footprint for an ON Semi 3.3V regulator, NCP117DT33T5G, in the DPAK package. I had four different sources, all of which should have been reliable, and I was not overly happy with any of them. So, I did this:
I created a FabLayer with the actual physical dimensions of the part. Most of the dimensions are exactly the middle of the tolerances, only a couple of the dimensions are slightly rounded a couple of thousands (with 20-40 thou tolerance range).
Do note that the project measures in inch units and this particular footprint is adapted to be well suited to an inch grid.
You probably want to remove the thermal relief from pin 2 of your DPAK, so it connects to the surrounding copper.
I would probably also make that pad a bit wider(East and West sides) and longer (North side), but I don’t know how big the copper tab under that component really is.
The exposed copper is now smaller than your DPAK and this will mean that the body will rest on the soldermask. This will also lift pins 1 and 3 a bit. I’m not sure, but I think it is common to make the exposed copper for pad Nr 2 big enough to fit the whole component in.
For components with such big pads it is common to make the solder paste mask a lot smaller than the pads itself, because else you have much to much solder on those big pads. Pin 2 only needs a very thin layer of solder, it does not have to “envelop” the component pins such as the other pads.
I have seen other data sheets specify a much smaller solder paste pad. This device did not have a recommendation in the device specific data sheet. However, it does have a recommendation to:
*For additional information on our Pb−Free strategy and soldering
details, please download the ON Semiconductor Soldering and
Mounting Techniques Reference Manual, SOLDERRM/D.
I have fixed the screen captures. The Fablayer capture shows the size of the metal tab under the component; it’s the mostly square polygon.
How are you planning to assemble this board? Will it be done by machine or by hand? If by machine, will it be wave solder or reflow? If by hand, will you be using a soldering iron and wire solder, reflow using solder paste and hot air, or reflow using solder paste in an oven or on a hot plate? All these things are factors when laying out a board.
I’m a hobbyist. I solder through-hole parts with a soldering iron and wire solder, and SMT components with solder paste and a handheld hot air soldering station. With the hot air wand I can heat up a ground or power plane fast enough that I don’t need thermals, but without them my normal soldering iron doesn’t put out enough heat to get a good joint.
The fun part of hand-soldering with solder paste and a hot air wand is that the surface tension of the solder will cause components like capacitors, resistors, and small transistors to align themselves. But you have to get the solder paste applied properly and evenly. A solder stencil is a great help for this. Be wary of the so-called “hand solder” SMT pads in the KiCad libraries; I find excessively long pads will sometimes cause devices to shift far enough that only one end makes contact.
You are more then welcome to create all of them for yourself to examine; simply PM me for the sources.
The entire point of the post is that one can compare “Serving Suggestions”, of Land Pattern Data across more then one data sheet, to the actual dimensions of the physical part when drawn also in KiCad on a differying layer.
Sorry you did not like the idea.
I thought it was pretty cool and decided to share.