Modular MEGAphone: Prototyping castellated modules

 In the last post, I described a concept for the modules for the MEGAphone based on the following approach:

B. Half-Round Castellated Pins

C. Key Pins & Varied Module Dimensions.

D. Carrier Board Cut-Outs for Reduced Height / Reverse Component Mounting

E. Carrier Board Cut-Outs for Ease of Removal

F. Bridges for Power and Ground Thermal Relief

I'm going to add to that:

G. Image Registration Reference Markers

The reason here, is to make it easier to check if a device has been tampered with, by making it possible for someone to make an image registration-based blink comparator, to quickly and easily check of the glitter polish has been tampered with. I'm not going to implement that right now, but I want to make it easy to do.

Let's start with making a footprint in KiCad for a simple version of the carrier board half of this interface.  This requires the surface-mount pads for the pins, and the cut-outs for the ease of removal, and the cut-out to allow for reverse-side components on the modules, as well as the image reference markers.

So let's start with measuring the size of the hooks on the end of an IC puller I have here, so that we can size the cut-outs at the ends. The hooks are only about 3mm wide and  2mm deep, so it looks like 4mm x 4mm should be big enough. These should stick out far enough, so that the hook can be got into place, but still have enough of the cutout beneath the module for the hooks to grab onto.  The edges of the module will restrain the IC puller when used, but won't restrain a screwdriver or other improvised tool, if one is used. Therefore, the cut-outs for the ends should not be contiguous with the cut-out for the module components.

Let's take a look at what this looks like for the 2x5 format:

We have the 2 rows of 5 pads in the middle, where the module will sit on top.  Then above and below that, we have the A1,A2 and B1,B2 jumper pairs: These are for putting the jumpers on that connect the module to the possible large and heat sucking GND and VCC planes of the carrier board -- and vice-versa, cutting and removing the jumpers disconnects the module from those planes, and thus making it much easier to desolder or resolder, because none of the pins are going to be massive heat-sinks.

Back to the missing pin 2: This is what allows the user to know which way around the module should go: You can't rotate it or flip it, and still have the missing pad line up with the missing pad on the module half, that looks like this:

I've included exclusion zones for everything except for tracks on the rear side, except for the area marked in the middle that corresponds to the cut-out in the carrier board. The pry zones should have exclusion zones for everything, including tracks, so that using hard tools there can't mess up the function of the module.  I've not got those quite right here, which I'll have to fix, but hopefully you get the idea.

On the front side, there is no exclusion zone, because those physical problems don't apply there.

On the rear side of the module, we can see the pry zones, where no components should be placed, because a user may be using a hard tool against that surface to try to lift the board off.

Any components on the rear side should go in that square in the middle.

Now, for a symbol for the module, I've gone with this, so that those power and ground plane isolation jumpers are explicit:

For modules, a regular 10 pin symbol can be used for now, so I haven't made an explicit symbol just yet.

As I discussed in the previous post, I'd like for different modules that are not electrically compatible with one another, that they shouldn't fit. To do that, we can most easily remove different pins, or combinations of pins.  For removing only a single pin, there are only two choices: a corner, or a pin next to a corner. Removing a middle pin won't work, as then the module could be flipped vertically. So we can have a "minus pin 1" and a "minus pin 2" version.  If we want more variants, then we need to remove two pins, with "minus pins 1,2", "minus pins 1,3", "minus pins 1,4", "minus pins 1,7", "minus pins 1,8" and "minus pins 1,9" are the only options that maintain resistance to Murphy's Law. That would give us 8 total variants. 

I'll get to those, but first, I wanted to make a 20 pin version, with narrow and wide variants, depending on the space required on the module:

At this point, I have enough done that I can design up some simple test PCBs for fabrication, so that I can see whether they really are easy to solder and desolder etc.

For that, I'll make a 100x100mm carrier board (US$5 for 5 pieces from PCBWay and friends) with places for various modules, on both sides of the board, as well as simple examples of the modules, with hole-throughs that go to each pin, so that I can easily verify that the connections have been made. I'm not going to worry about the various missing-pin combinations, as that's less relevant right now.

Here's the test carrier board, with six of these footprints, spread over both sides, with every pin broken out to some standard 0.1" headers for ease of testing:

Looking at this, I'm slightly concerned that I have the inter-pad spacing a bit tight, and that they will be prone to bridging. I know that 0.1" pin headers are super easy to solder, so I should be able to reduce the pad heights to match that ratio of pad to space. They were 2mm, so only just over 0.5mm between them. I've now reduced them to 1.75mm, so that they now have just over 0.75mm between them, which feels a lot better:

Now for the test modules. I decided to add them as snap-offs on the PCB, as this should be cheaper than submitting 4 different PCB orders. I've not done this before, nor worked with PCBWay for castellated edge connectors. So let's see if they complain about my design :)

Actually, it occurred to me that it might be cheaper to do it in two parts, since the modules are forced to be 4 layer in this arrangement, even though they are just simple adaptors right now. But maybe I'll leave them all together, as it will still confirm that PCBWay can do this with 4-layer boards. In which case I should ideally put GND and power layers in them, with thermal relief connections to the pins, so that the thermal issues from that for soldering are reproduced.  Once I get the review feedback from PCBWay (I submitted it in the middle of the night), I'll make a decision on it, as I'll be pleasantly surprised if they accept it first time around.

As expected, I got some feedback from PCBWay, who pointed me at this resource. 

Basically I need to make my tabs wider (2mm+), with rounded ends, as well as the gap between the boards (1.6mm+), and I can then put drill holes (diameter > 0.45mm) along the edge, to make it easier to break them off.  Here is how the connections work now:

So let's see how PCBway goes with that. It passed, but the price is pretty high for five pieces, due to the castellations, and the 6 different designs on the panel. I'll live with that for now, as my priority right now is testing the module design.

Hopefully, it will work when it arrives...