#pcbtips

When following LowPowerLabs' excellent stencil tutorial, I had trouble with the step for shrinking the pads. Viewmate is unavailable on Linux, and it seems an unnecessary complication for a competent program such as Eagle. After a bit of poking around, here's the easy way and repeatable way to make your stencil layer.

Step 1: Open Files Open up your circuit in Eagle, and head over to the board layout.

Step 2: Layers Open up the layer's menu, hit "none", and select only Top and tCream. tCream is a layer that specifies which area is supposed to get solder paste. Coincidentally, that's the exact layer of interest for a stencil. Notice how the cream layer very nicely overlays your pads. The default is to make them the same size, which is a good guess, but we need to fix it.

Step 3: Run DRC Open up the DRC menu. For the uninitiated, this is the Design Rule Check, which helps make sure your board meets the specifications of your PCB manufacturer. If you have a fab's DRC file, go ahead and load it. If you don't It's good advice to get it from their web site.

Now, head over to the "masks" tab. It will look something like this:

See that line that says "Cream"? That's what we're looking for.

Step 4: Fiddle Keeping with Eagle's user interface principles, the options here are a bit confusing at first. But don't worry! The term "mask" refers to a layer that blocks something else. In this case, the "mask" is a layer that keeps solder paste off of the pad. Play around with them for a few to see how they interact. This is also a easy and visual to learn about masks, which are mentioned a lot in Eagle (stop mask, keep out mask, etc.), So what do these mean exactly? The Max column is the most that the pad gets shrunk down, which doesn't do anything on its own. The Min column is the least that it will get shrunk. Adjust Min and hit apply, and you'll see every pad's cream layer shrink by a bit. Now, for the percentage. At this point, you can probably guess: It shrinks the cream layer down by X% of the pad's size, while shrinking at least Min, and not going more than Max.

Step 5: Replicating the tutorial So, to match the tutorial's settings, where he suggests "5-6 mil", we'd put 5mil in the Min and Max column, and leave % at whatever. Give it a whirl!

Uh oh. This particular board doesn't like his. The TSSOP footprint and the 0603 surface mount parts look great. If that's all you have, you're probably done here; but this board uses some tiny parts. Look at that MLF footprint in the center, the crystal footprint on the top, and the 4x0402 array on the right. That doesn't look promising at all. In my case at least, further tweaking is needed.

So, let's tweak the options a bit more precisely: The problem is the pads that are giving me problems are ~9mil wide, and we're cutting 8 out, leaving 1 mil for paste. Judging by the values int he tutorial, we're looking for a cut of around 20%. Here's what that looks like:

However, that doesn't look so great either. We still haven't taken enough from the tiny pads, and the big ones are now way too small.

Let's try this again, this time let's cap the Max at 5 mils so they don't over-shrinkthe large pads. And lastly, to make sure we get a good cut of the small ones, and set the min to about 2mil.

Perfect!