SO-8FL Package Footprint Eagle PCB

Question

I am making a PCB with a component that is of the package SO-8FL. The component is n-channel MOSFET NVMFS4C03N by ON Semiconductor and the datasheet is here.

I started to make the package in Eagle, but got stuck and didn't feel comfortable. It's a bit more complex than other packages. I've searched many libraries that are available for download, and have not found any that include the SO-8FL package.

I need to integrate this into my PCB schematic and board design in Eagle. Please point me in the right direction.

Answer 1

Right, so that one was quite a challenge! You can download the library I made here. Note, this solder layout is for reflow soldering. If you want to do this by hand, I suggest making the pads a bit longer so you can get a solder tip on them.

The two things that made this part a bit trickier were the (very) non-standard solder pad (drain), and the multiple pads for a single pin (source). More instructively, here's the steps to make it (Eagle 8.3):

1. Create a new library. (Control Panel -> File -> New -> Library)

2. Copy a generic N-MOSFET symbol from the built in library into the new library. This has the schematic symbol and the pin names (G, D, S).

3. Start a new package.

4. The 4 pins are easy. Just place a single SMD pad at the origin; type "info" and click on then edit it to the correct dimensions given in "Recommend soldering footprint" on page 6 of the datasheet. Type "grid", and set it to "1.27 mm" - you can then just copy the pad across as the pin pitch is 1.27 mm (0.05 in for our Imperial masters).

5. For the drain solder pad, initially just place an SMD pad somewhere under where you want the pad to be. This will act as the anchor to connect to when you layout the board. Now, select "Polygon" and roughly draw the shape you need on the "Top" layer. Then, type "info" and edit each edge to the correct start/stop points. I usually draw out the part on a piece of paper, and then you can calculate the dimensions relative to your origin.

6. Once in place, copy your polygon (not including the SMD pad) twice. Change the layer for one of them to "tStop" and the other to "tCream". This opens a hole in the soldermask and sets a solder paste stencil hole respectively. This is important as the polygon is not a pad, so these are not placed by default.

7. Add the package outline on the layer "tPlace" using the wire tool. Add the text ">NAME" on the layer "tName" with the text tool.

8. Start a new device. Add the symbol from part 2 and then hit "New" on the package box to the right; add the package from steps 4-7. Hit "Connect" and then associate the pins with the correct pads. If you want to have the same pin on multiple pads, use the "Append" button in the dialog.

I can add some more info if needed, but that should definitely get you started as an example. You could do as @T2JSplode suggested, but I prefer a single pad to be a single entity, not a piecewise construction.

Answer 2

Since the main body of the pad is just a rectangle with "wings", the simplest thing to do is make a 4.56 x 4.02 pad, and add 0.495x0.905 pads on the sides, and 0.75x0.51 pads (based on minimum dimension G) at the top. 4 pads at the bottom are standard.