Can we design the teensy alternative for keyboards?

[flabbergast]

Cumulative capacitive loading on USB power lines should not exceed 10 µF. That is the limit of the USB specs. If I understand it correctly we are now at 2*2.2 + 3*0.1 = 4.7 µF. So there is still space to increase the capacitors but not more than about 2 times.

I didn't want to increase the capacitance but the voltage rating (i.e. trade 2.2uF 6V for 2.2uF 10V or more).
{I think the limit is there to limit the inrush of current when first powered up, which could drop the voltage on VBUS more than allowed. I'm pretty sure there are ways to limit that; for instance Arduino Uno has w 47uF caps around the regulator I think. But I think we should stick with 2.2uF anyway; maybe we could go 4.7uF on the VBUS if we really wanted.}

[vvp]

Yes, it is about inrush current. It cannot be more than what a 10 µF capacitor in parallel with a 44 Ω resistor consumes.

[matt3o]

I agree with flabbergast that the board should be first of all easy to work with from a custom-builder standpoint.

Apart from that is there anything you need from me to keep the board development going?

[mohitgarg]

I'm still waiting on a consensus regarding dimensions, peninsula, switch mounting holes or not, USB connector. Once we decide we can begin recreating the board

[matt3o]

- dimensions: 38x20 (including peninsula AND usb port) would be the max size. the smaller the better considering that we need to place the PCB on some headers under two switches.
- usb connector micro-usb (unless usb-c is physically better, meaning it has some features that let us make the board within our constrains)
- if mid-mounting the connector would let us stay 3.4mm thicknes I would explore the feasibility (on a small peninsula as in pomk's design). If it wouldn't be possible to stay between the plate and the PCB, then I wouldn't bother and I would use a standard USB port
- peninsula: we don't need a pronounced peninsula, but I would make it stick anyway few mm (also considering that USB port already sticks 1mm as far as I understand)
- mounting holes for the switches would let us fix the PCB anywhere between two switches in hand wired keyboards. I believe that would be a nice touch. I don't think we need to support all switch orientations, though (you use this option only in handwired keyboards, so it really doesn't matter how you place the switches). I would only support upside down position (LED up) with LED holes and ALPS+MX. All this ONLY IF we can keep the board within specifics with enough pads
- would be nice have both pad holes and castellated PCB but not strictly needed

Regarding voltage/capacitance/vbus/ohm/etc... I trust flabbergast and the more tech savvy people. Do what is best trying to keep the cost as low as possible. If you have any question don't hesitate to ask.

[flabbergast]

We should decide on something. I think the schematics Mohit and pomk is "correct", the point now is the layout / "mechanical" design. I'll try to list the features which "cost" PCB space, and give them some order. The other things should be achievable without affecting other things too much (e.g. castellated pads).

(A) mid-mounted micro if <= 3.4mm thick
(B) peninsula
(C) 2.54mm spaced pads
(D) USB-C
(E) switch+LED-mounting pads+holes
(F) OSH Park's design rules (this affects how tight can we route)

I feel like it's not going to be easy to have all of these things. The biggest constraint is (E) (which will basically dictate where the MCU can be; pomk's vs mohit's design), then (C), (D), (F).

I think we should do a "vote" or whatever, to decide what should we try, and which features you guys feel like they're more important.

My "weights": for me the most important things are (C) and (F); (B) is preferred; (A) and (D) don't mind either way; (E) would be nice but only if we can keep (F) and (C).

About (F): the use case I am thinking of is people who want to make a small run of boards for themselves. Of course Chinese fabs are OK (and generally have less tight requirements), but it is relatively expensive to have gold immersed PCBs with them in small quantities. I would not care about this if our boards would be available more-less "continuously", i.e. not just, say, one MD run or something like that.

[matt3o]

I do not feel (F) is so important. I'm afraid it's too limiting and the plan is to find retailers willing to stock the controller (MK.com maybe, hopefully others). We could also suggest manufacturers able to produce our design.

On everything else I agree with flabbergast.

[vvp]

Ok, I did not post my vote because I doubt I'll ever use the board. I'm interested only in contoured cases with LCD and that means it is just easier to home etch controller PCB and hand wire the switches (instead of complete "bird nest" this controller board would lead to).
But for a flat keyboard my preferences would be (in the order of importance):
1) through-hole mid mount USB micro connector so that it can fit between plate and the PCB and I do not need to rip off the USB connector
2) mounting holes (two in the middle are enough)
3) no peninsula (USB connector more or less aligned with the board edge)
4) 2.54 mm pads (but I can go also with 2 mm pads or (in the worst case) 1.27 mm pads)
5) get all ports available on pads (internal pads anywhere inside (if we cannot fit them around edges) are OK)
6) 38.1 × 17.78 mm dimensions are ok; I could go also with 38.1 × 20.32 mm
7) SWD related pins near to each other
8) Features needed to have it mountable below two switches are the least important since if I would build a flat keyboard then I would want it column staggered and I doubt I would like an USB connector sticking to the side. But if they can be added so that the spring hole is shared as with a mounting hole then why not. I would not bother with trying to connect the switch pads to anything. This can be done with separate wires. I would not care about switch diodes too. As for as LED diode support - at most make unconnected pads for them. No Alps support for me.
9) As for as fab rules. I do not care. I would buy this as a finished product.

[matt3o]

I did some digging on the mid-mount USB.

The connector is 2.94mm. The height of the exceeding part of the connector should be 1.52mm + 1.60mm of the PCB should place us at 3.12mm. So technically we could use that... by a whisker (3.50mm being our roof). I guess the soldering job must be spotless, though. Also one might want to add some insulation, even though it's just panel ground.

reference http://www.molex.com/pdm_docs/sd/476420001_sd.pdf

[matt3o]

we haven't dropped the ball, have we?

[Matt_]

I was wondering the same, then I realized I didn't even comment on your last message about requirements. So:

+++ C (2.54 mm spacing for pads) is the most important, because 2.54 mm headers are cheap, ubiquitous and easy to solder. It makes little sense to design a controller for everyone to use if they have trouble getting headers easily.
++ B (peninsula), I can do without because of the way I'll use the board, but it makes sense when you consider most custom board designs and won't add much to the overall cost (board surface).
+ A (mid-mounted USB connector) would be nice to have a lower profile controller, but not essential, micro USB is not that tall anyway.

- D (USB-C), there are pros and cons, if it drives the price too high and makes the board bigger, we can forget it; otherwise, it has its advantages over micro USB so why not, but I don't think it's essential.
-- E (switch+LED-mounting pads+holes), I'm afraid it will make routing on the board much more convoluted, or we'll lose too much space and/or locations for pads.
--- F (OSH Park's design rules), does that mean that the fab used for this controller can reliably make boards with thinner traces/spacing than OSH Park?

I suppose most people will buy the board already assembled, and that those who want to build their own variant can rework it in KiCad if they need to, so I don't think we should focus too much on OSH compatibility. But is it safe to go with traces/spacing smaller than 6 mil anyway?

Most importantly, I think we can't please everyone. So let's choose what make sense for most people and forget about marginal uses so that we can get something going soon-ish. If the controller works, as long as the whole thing is open source, people will be able to make variations that suit more specific needs anyway.

[mohitgarg]

Just been very busy with work since I got to India. I'll have some free time later this week and will redesign the board keeping in mind all the suggestions. I believe we should be able to,
- Mid-mounted connector
- Peninsula (
- 2.54mm spaced pads
- USB-C
- OSH Park's design rules - Current board is using specs which are fine by OSHPark and comfortable for all Chinese fabs.
- Two mount holes
- Get all ports available on pads
- Dimensions, 38.1*18.1
- SWD related pins and bat-power related pins near to each other

Will try to fit as well,
- Switch mounting holes - won't be able to fit LEDs and PCB guide pins, just basic MX/Alps in one orientation.

[matt3o]

thank you mohitgarg. looking forward to seeing the new version.

just wanted to add that usb-c is totally not needed and that the switch/led pins don't need to be routed. they are just raw "sockets" that would be later hand wired.

[flabbergast]

sorry guys, very busy at work.

[matt3o]

thank you guys. just let me know if there's anything I can do to help.

[matt3o]

I'm available at paying for the development of the board if I need to

[pomk]

Very busy at work. I'd have time today, but seeing how mohitgarg already said he'd do it, I'd rather not as it would take up at least an entire day and parallel efforts are quite unnecessary at this point.

[mohitgarg]

Had a look at a bunch of USB Type-C connectors, most sit around 2.2mm above the PCB, to use the controller between the plate and the PCB, we'd have to use a PCB of 1.2mm thickness.

[matt3o]

micro usb is just fine

[Muirium]

Exactly. It's not great, it's just fine.

[mohitgarg]

Exactly. It's not great, it's just fine.

Know a source for a USB Type C that fits our requirements?

[pomk]

This is the best I've found in the height aspect: http://www.digikey.fi/product-detail/en ... ND/5246072

But even this sits good 2 mm higher than the pcb, making it at least 0,1mm too tall.

[flabbergast]

I think it's quite fine to go with 1.2mm thick PCB, or even 1mm. The thing will be small, and that thickness is plenty. Source: I've had 1.2mm batch of these. {I actually also have a 0.5mm thick this one - and that one flexes slightly when some amount of force is applied.}

[matt3o]

I think it's quite fine to go with 1.2mm thick PCB, or even 1mm. The thing will be small, and that thickness is plenty. Source: I've had 1.2mm batch of these. {I actually also have a 0.5mm thick this one - and that one flexes slightly when some amount of force is applied.}

is 1.2mm strong enough if you use the on board USB port? I mean if you place the board to the top side of the keyboard and connect the cable directly.

also, with 1.2mm can we still place the board flush over another PCB? Don't the USB pins stick out?

[pomk]

the one I posted sits 1,1mm below the pcb surface. Some others around 1mm.

[vvp]

1.2 mm PCB will be about 2.3 times mechanically weaker than 1.58 mm PCB (because force needed to flex depends on third power of thickness).

But it does not matter if the metal pins on which the USB connector holds are even weaker than the PCB. Whether it is so will depend on the peninsula size/shape.

If there would not be any peninsula and if it would not be a mid mount connector then I say 1.2 mm is enough. I had one 1 mm thick PCB and it was strong enough. But there was no fancy peninsula and no mid mount connector. Only a simple through hole pin headers. But in our situation, I do not know. If somebody has a CAD with FEM analyses then he can run a simulation for our peninsula shape.

[mohitgarg]

Can't comment on the shape of the peninsula right now, but there's no USB C top-mount connector that will fit, as they are all around 3.2mm in height. Mid mount will be our only choice.

[matt3o]

considering this is a DIYer's product I don't feel we really really absolutely need usb-c. just my 2c

[pomk]

1.2 mm PCB will be about 2.3 times mechanically weaker than 1.58 mm PCB (because force needed to flex depends on third power of thickness).

But it does not matter if the metal pins on which the USB connector holds are even weaker than the PCB. Whether it is so will depend on the peninsula size/shape.

If there would not be any peninsula and if it would not be a mid mount connector then I say 1.2 mm is enough. I had one 1 mm thick PCB and it was strong enough. But there was no fancy peninsula and no mid mount connector. Only a simple through hole pin headers. But in our situation, I do not know. If somebody has a CAD with FEM analyses then he can run a simulation for our peninsula shape.

In case someone plans to calculate this, the wrenching strength for the receptacle (according to the usb type c standard) is defined so that the receptacle has to be able to withstand moment of 2Nm to 3,5Nm depending on the direction of the force. It's better described here: https://doc.xdevs.com/doc/Standards/USB ... 20test.pdf

Id' also like to mention that these mid mount connectors are used in many mobile phones and with pcb heights typically less than 1,6mm without major issues. The fact that they sit so high compared to mid mount micro usb connectors gives a clue to the 'designed' pcb thickness. For the connectors to be flush with the pcb bottom (which is usually how you want them to be when using mid mount connectors), the pcb thickness for the currently available mid mount type c connectors seems to be designed to be either 1mm or 1,2mm depending on the manufacturer.

I would not worry about the pcb strength as long as the peninsula has 45 degree chamfers on both sides.

[bpiphany]

My God, you're on page 12 already.. I haven't read it all.

All I have to say is that QFN's are a bitch to solder at home. At least quickly and reliable. There may be people with more assembly skills than me out there, but I tend to get a lot of solder bridges, or unconnected pads, always requiring hands on touching up. And that is no fun at all, not even seeing the pads and all.. 0402s and other fine pitched things are ok, they are at least accessible. I have a hard time believing anyone will want to be home-assembling something like this for the masses. Factory assembled is another story of course.

Long long time ago I made this It never made it into any project. I put it aside because of the QFN. That one was intended to fit between two rows of switches.


I had some better experiences with the firefly

Then just days ago I shot myself in the foot trying them QFNs again =P