Through Hole SMDs

This section is about how to use 0603 SMDs as through hole components and even vias. This means, instead of placing SMDs flat on your PCB, you connect one side to the top layer, and the other to the bottom. This makes hand assembly much easier, but it is not the ‘normal’ way of doing things to say the least. I start with listing the downsides, but if you already know you don’t want this, you can skip ahead to Scratch Milling Jigs.

The Downsides of Through Hole SMDs

The big downside is you probably won’t be able to get a professional PCB board made in this style. Actually I don’t know that as I’ve never tried, but it requires either drilling overlapping holes, or punching out rectangles – not standard practice. Second it is unproven – there may be issues with things like heat or durability. I have noticed problems if too much flux gets in the hole – the solder seals things and the flux boils, causing a mini geyser. So there are unknowns. Lastly, it requires more thinking when designing, and some fudging in KiCad. I like to think of this as more options, but it is another dimension to keep track of when placing things.

The Positives of Through Hole SMDs

The best thing about vertical SMDs is hand assembly is much easier and less error prone. A professional board with solder resist will be easier to use a solder mask and reflow, but you still have to precisely place all the components vs drop them in a hole. Of course if you have a pick and place machine that step is easy too, but then again, if you have a pick and place machine, why are you even reading this ;).

Another positive is it allows you to think in three dimensions when designing. There are many cases where this simplifies design – caps connecting to ground, a pull up resistor to a connection pin, a trace that has to dip under other lines etc. With DIY boards you don’t have plating on connector holes, so your connector traces will have to terminate on the bottom of the board — it’s surprising how often you can accommodate this with through hole SMDs. Where you normally need a via or two, you often can just cleverly have components do double duty as a ‘smart via’.

Also remember not all components need to be through hole – a voltage divider works well with one resistor coming through from ground, and the second flat on the top to power. Ultimately it reminds you experimental circuit boards allow you to try weird things, and you should try them.

KiCad Considerations

The one certainty is you will need to get comfortable designing your own footprints. The first issue is the square peg in a round hole problem. SMDs are rectangular, and drills are round. Drilling a hole the diameter of the largest side isn’t terrible for the more square capacitors, but the extra space is problematic for flatter SMDs. I find drilling two overlapping holes works best – you can dial it close enough that it grips the component, and there isn’t so much extra space that it becomes hard to connect solder all around. Create test drills in Fusion360 or even with KiCad footprints, and record what works. Don’t forget to record the style of bit you use, as that can make a difference at these tolerances.

The drills and spacing I find works is, for flat SMD resistors 0.7mm drill and 0.35mm spacing between holes (I always center on the holes, and then use positive and negative X for the offsets, so -0.175 and +0.175).

For the taller capacitors, I use slightly larger holes (0.9 mm drill), and space them 0.4 mm apart (0.2 mm on each side of center). Of course these may change depending on the measurements of your brand of components, always important to test.

After the holes, there are two pads, one on the top as pin 1 and one on the bottom as pin 2. The pad shapes can be anything you like, I have experimented with shapes for ease of solder-ability, but settled on plain pads for now. For directional components like diodes, you may need to make a second set of footprints with pin 2 on top and pin 1 on the bottom, to give you more flexibility during layout.

The last caveat when using KiCad is that non plated through holes are very hard to connect properly. The best way to deal with this is make a duplicate set of your footprints, and remove the holes. Then you can wire all your traces with this set, and they will connect to pads as normal (pads are the red areas in the images above). Once this is complete, you can use find and replace to change to the pads with holes. If you name things carefully, this is a very simple step, and it is easy to go back and forth between working and export. It would be trivial to make a script for this as well.

For assembly, if your holes are the right size, you can simply lay the board flat, drop the components in the holes, and dab solder on them. Adding a little solder to the ends before putting them in the hole makes the final soldering easier, but that takes practice to get the right amount. Once all components are in and soldered on one side, simply flip the board and solder the other side. If you make a mistake, heating things up and using a ‘solder sucker’ can usually get the component out, or even just push it all the way through if using an air gun.

I’m still adjusting this process every board I do, I’ll update again if things change for the better (or worse!).

Next: Scratch Milling Jigs