GH60 Keyboard Project

[komar007]

How hard would it be to add a USB port onto this (to plug in a number pad)?

Very easy because all you need is to wire another port to the incoming port to make a primitive USB hub.

One thing is there must be some place for this additional connector and it can't interfere with the poker case (so it has to be recessed).
Second thing is the user has to drill a hole in the case.
And thirdly, atmega32u4 doesn't support USB Host, so you can't make a USB hub. We'd need a dedicated IC for that. BTW, you can't make a hub by just splitting wires;). Though possible from protocol's perspective, it won't work at least because plug/unplug detection can't work (pull ups/pull downs will be messed up).

[damorgue]

Though possible from protocol's perspective, it won't work at least because plug/unplug detection can't work (pull ups/pull downs will be messed up).

Ok, didn't know that. I knew that the protocol supported it because I have done so in the past, but I guess I was lucky then and that these are more complicated circumstances.

I suppose one could remove the plasic casing from a proper USB hub and mod it in there instead.

[komar007]

You actually did that?
I didn't know it was possible in practice at all...
Anyway, I think we shouldn't do too much, I mean one more cable on the desk isn't so bad.

[jdcarpe]

I think that we should stick to a USB Mini B connector. Since that's what is used for the Poker, Pure, HHKB, Rosewill, QFR, Leopold, etc.

[komar007]

Ok, what do you think about this one? http://www.digikey.com/product-detail/en/UX60SC-MB-5ST(80)/H11671DKR-ND/2004588
It's $.63@100pcs
It seems it will fit, but I'll check that.

[jdcarpe]

Looks good to me. Can we get those mounted to the PCB by the fab, or will we need to do final assembly to add these connectors? Some people may not be comfortable with the soldering SMD. Maybe whoever distributes the PCBs will be willing to solder all the USB connectors.

[komar007]

Well, I chose smd so that we can get the cheapest assembly, but have no experience in that matter...
In the worst case we can find a few people (me included) to actually solder the whole thing before shipping if assembly is too expensive.

It would be good if someone who's had experience working with fabhouses shared some of it with us.
I've also checked the prices of a local pcb manufacturer and it seems we can get down to $20@60pcbs. Not sure I calculated this correctly, and I don't know if they have gold-plating.

[Bim Gao]

Very interested

[TheProfosist]

I prefer type B too, but it won't fit to the slot in the poker case...

wait your using the poker case now? I thought this was going to have a custom case. Also arnt pokers hard to get or has that been cleared up? Additionally the DOX revsion that ive been helping on requires a poker case as well and there are already a few PCB designs and firmware and even a plate though my exact layoutis being worked out at this time.

I think that we should stick to a USB Mini B connector. Since that's what is used for the Poker, Pure, HHKB, Rosewill, QFR, Leopold, etc.

MicroB is much more durable than minib

Well, I chose smd so that we can get the cheapest assembly, but have no experience in that matter...
In the worst case we can find a few people (me included) to actually solder the whole thing before shipping if assembly is too expensive.

It would be good if someone who's had experience working with fabhouses shared some of it with us.
I've also checked the prices of a local pcb manufacturer and it seems we can get down to $20@60pcbs. Not sure I calculated this correctly, and I don't know if they have gold-plating.

Are the PCB's going top be finished like the phantom? The reason i ask is the DOX ones not done as nicely because were ordering in much smaller numbers.

[IvanIvanovich]

No idea how plausible it is and if anyone else would be on board with it, but speaking of finishing... can we get the pcb done in white?

[bpiphany]

So, I sort of stopped reading on page 4 or so... I just cut down what I am working on for the next round of full size "Phantoms". It's got a bunch of layout options, perhaps a bit ever the top for this project. I think that the arrow layout on the bottom right would be nifty on a small board like this though. See this pdf for layouts http://geekhack.org/index.php?action=dlattach;topic=34392.0;attach=1997



With overlapping switch footprints the solder pads end up far apart enough to be possible to drill. There is no actual need to rotate footprints because of that. The center holes on the other hand starts to overlap. I don't know how eager the manufacturers are to do drill holes that overlap. I bet it depends on the amount of overlap and the drill sizes. The problem is if the drill drifts into the first hole. This has the possibility of both messing up the PCB as well as snapping the drill bit. Routing is fine though. So I set the overlapping holes up as slot holes, which are routed. Drilling a larger hole overlapping a smaller hole may not be as dangerous since the larger drill will have less tendencies to jump into the first hole. But that situation doesn't arise too frequently for us.

I would suggest using the smaller ATmega32u2 controller. The TQFP packages that are easy to solder by hand are quite a lot larger than the QFN packages the chips on the different Teensy boards use. The ATmega32u2 TQFP32 chip is the same size as the ATmega32u4 QFN44 chip. The 32u2 has a bit fewer pins. There are 20 easily available IO-pins. Then there is the HWB pin which needs to be tied to ground to enter the bootloader at reset. It can be used as an IO-pin but that requires a two button reset procedure (or something similar, software bootloader jumping is fine as well as long as the firmware doesn't hang up). In extreme need of IO-pins the reset pin can be configured as an ordinary IO-pin as well. The downsides to doing this should be pretty obvious...

An 8 by 9 matrix should be enough for a board like this, adding 3 IO-pins for LEDs that sums up to the 20 convenient IO-pins available. A 5 by 14 matrix would probably be much more convenient when laying out traces in this case. With 2 LED lines that still fit the 21 actually usable IO-pins.

PCB mount stabilizer holes can make a mess to any layout =P Especially the ones for the ISO enter overlaps with just about anything ANSI... I think it can still be managed though. In the very worst case they can be made only as 1mm pilot holes. This makes it easy to center a drill to enlarge the holes needed for each individual board. That wouldn't really be recommended for higher volumes though...

Edit: The reset pin may actually be a 23rd IO-pin. I find the datasheet a bit confusing on that... Also, I realized that a 7 by 10 matrix is going to be sweet =D

[komar007]

Hi bpiphany,
thanks for your input.
I can see that your Phantom board has even longer slots than we have here, and I have a question.
With such long holes, isn't there a problem with mounting pcb-mount switches? I'm going to ask a pcbfab if they can drill or mill holes so close to each other, because a few overlapping holes would mount the switch more firmly, I suppose. Not sure if this is possible at all, so we may end up doing slots anyway.

As for rotating switches, I hope this is not a problem, and thanks to this we have support for pcb-mount pins in all switches but capslock.

Also, I see that in the design you attached, many solder pads are covered by slots, but I can't see the same in the Phantom pcb photos, it seems that they fit just fine. I currently have one such situation (capslock also) and I'm worried that this will be hard to solder and really fragile. And we have to remember that this will be soldered by the unexperienced.

I've put all the project files on github, so you can all see where we are: https://github.com/komar007/ghkb

[bpiphany]

The center hole slots cuts into the solder pads. The two CapsLock footprints on the Phantom are made that way, as well as the Spacebar footprints. The Filco Spacebar footprints are made the same way. That is where I got the idea from. I haven't seen the Phantoms IRL yet of course =P But the ErgoDox has these slots as well. They do look a bit funny, the router bit has only pushed the through plating into the hole a bit, while the glassfiber is gone =)

I haven't made any this long slots before, and I think I would skip the PCB mount holes on the bottom row to get some more material. It would require some more care to get the switches straight while soldering, but that isn't too hard. Put the switch in, solder one pad, put a cap on, re-melt the solder while aligning the key. And presto, a straight key =)

There is also a Poker mount slot there on the right side that takes some more material away.. The FR-4 material is really tough, the center hole slots will not substantially weaken the solder pads. The PCB may be a bit more flexy on the bottom row from taking this much away though.

Edit: I think that mounting slot on the bottom right is a bit misplaced actually...

[Tenkey]

What software are you guys using to draw the layouts?

[dirge]

think they use kicad

[bpiphany]

Yes, KiCAD it is =)

koomar007, your Cherry footprints  are not according to the specs. I don't know if you have measured the terminals on the switches yourself and they will actually fit (there is some play with Cherry specs), but they are way smaller than specified.

Do you have any switch located on some integer coordinate?.. You seem to have a 19mm spacing between keys, the standard is 0.75" = 19.05mm. That is not a big difference, but over 14 spaces still ~0.7mm.

The USB port on the Poker is not centered between the two switches.

Have you taken your measurements of the Poker yourself? or do you have access to the "real" ones? I don't know if they did it in mm to start with or whatever. I would be interested in knowing the exact locations for mounting holes if you've got them =)

Also, I don't have the build of KiCAD with the "standard" libraries. I always collect all the footprints and components I use for a project directly in the working directory. It makes it a lot easier to share files..

[komar007]

If you mean the size of pads, they may be wrong, but I'll play with them in the end. As for the positions of everything, I used cherry's webpage (http://www.cherrycorp.com/english/switches/key/mx.htm), I hope this part is correct.

Well, I knew there would be problems with kicad files. I'll try to make them shareable.


19.05 mm you say...  I was pretty sure it's 19mm spot on:/, but this should be easily fixable if necessary.
As for positions, I measured the Poker and that's basically what I got.
The pcb starts at (0.5, 0.5)mm so if you subtract that from positions of things, you should get the coordinates with respect to the pcb of the Poker.
EDIT: sorry, that's if you move everything to the edges of the document first.
I'll have to print this layout and try to fit it to poker to check if it's correct.

[bpiphany]

Well, it all depends on how they actually designed the Poker.. They may well have used 19mm. I just had a look at my scans and measured the spacing to right in between 19mm and 0.75" =D

Using relative coordinates is no problem as long as it is easy to find some place to start =) Space sets the relative origin to the current pointer location.

Your Cherry footprints looked correct except for the solder pad sizes. Overall I think it looks pretty good.

[komar007]

That's good, because I thought something else was wrong too.
The pads are different than specs, that's for sure and now I remember actually making that change.
The drills are 1mm, I'll drill such holes and check if that's enough. If it is, maybe I'll leave it like that. Or maybe larger will be better. That's for hand soldering...

Should I put ALL the libs in the repo? Also stuff like R, C, etc?

[bpiphany]

You can put it all there or just copy paste the parts you are actually using into your own components and footprint files. Or I could just find out how to install the standard libraries I guess =P

[komar007]

I fixed schematic, it should be OK now.
The pcb should work fine, I think kicad saves all the footprints inside the .brd file.

[bpiphany]

Yes, the brd file contains all the info =) I installed the standard libraries, and rebuilt KiCAD from scratch as well.. The only thing missing then was the Cherry switch components in the matrix schematic file. And they still seem to be missing. If I got this git thing correct, and have actually updated =P

[komar007]

The cherry switch should be in mx1a-simple.lib in lib directory.

[komar007]

Ok, so here's a demo of what I have so far.

What we still need is connections between the matrix and atmega and various dimension bug fixing.
I'm not sure about ground pours. Maybe I should pour the whole area with ground, maybe the other side with VCC to form additional bypass cap.
Or maybe nothing.

[bpiphany]

I don't really know actually. I guess the danger is that you may introduce a very strong "coupling" to GND if you pour the zones out everywhere. Could increase rise and sink times for the signals I suppose. It doesn't seem to be much of a problem on previous designs though.

[komar007]

I know why the USB connector is centered between the switches in my design, and not in the Poker. Because the Poker has all the switches moved a bit. They're not exactly centered with respect to the pcb. I think I'll leave mine centered, that is, 18.5mm from the left edge.

[bpiphany]

I know why the USB connector is centered between the switches in the Poker and not in my design. Because the Poker has all the switches moved a bit. They're not exactly centered with respect to the pcb. I think I'll leave mine centered.

I don't know if you lost a "not" there, but the USB connector is not centered on the Poker. It is closer to the '~' key than the '1' key. If the switches aren't centered it would look very strange...

[komar007]

Sorry, fixed my post.


EDIT: if you put the pcb on the poker in such a way that the space between pcb and case is the same on the right as on the left, you can see, that the usb connector is moved 0.5mm to the left with respect to the slot in the case. Our design won't have that flaw;)

[bpiphany]

Looks like you are correct that the switches aren't completely centered, funky.. But still, check if the keys are centered in the case. If so, you still want to keep the USB port off-center to have it centered in the hole in the case..

[__red__]

The drills are 1mm, I'll drill such holes and check if that's enough. If it is, maybe I'll leave it like that. Or maybe larger will be better. That's for hand soldering...

The hole dimensions are specified in the datasheet so no need to guess:
1.5 (+-) 0.05 (Pads)
1.7 (+-) 0.05 (Fixing pins)
1 (+-) 0.1 (LED or diodes)
4 (+-) 0.1 (Center Hole)

[komar007]

I know, but I thought it would be easier to solder the switches by hand if they fit tight instead of falling out of the board.

[bpiphany]

PCB mount switches hang on to the PCB pretty well with the extra pegs. They are tightly fitted, and also align the switch properly. Through holes for soldering should be a bit bigger than the leads, or so I've heard at least. Makes some sense probably, if nothing else it will be extremely hard to de-solder a lead that fits tightly into its hole.

[komar007]

Okay, I think I'm convinced enough to enlarge them;)

[Caaaarrrt]

This looks awesome. I'm quite interested.

[dirge]

How are things going with this one?  Worried that it's gone a little quiet ;p

[damorgue]

What is the pcb looking like atm? Is the position of the controller final? Will it fit imsto's new aluminium cases?

[dirge]

I'd like to throw in a request for an alps version, I wanted to try and take it on myself but just haven't got the ability if I'm honest.

[komar007]

Hi,
I know you may be thinking the project is stalled, but it's not;)
Sorry for not updating you, but I had some other projects too. I'll try to finalize the pcb soon.

What is the pcb looking like atm? Is the position of the controller final? Will it fit imsto's new aluminium cases?

The position is not final. I have to make sure the controller won't get in the way with the poker case, because it has some strengthening horizontal bars.
Not sure about imsto's cases though, I only have the original plastic case, but if it's the same mould, it should be fine.

I'd like to throw in a request for an alps version, I wanted to try and take it on myself but just haven't got the ability if I'm honest.

Please find some trustworthy datasheets with footprints for the alps switches and I'll see if it's possible to integrate them to the current design. If not, we can do an alps-only version next time.

[dirge]

Matias said the datasheets would be ready early September, soon as I see them I'll pass them on.

[TheProfosist]

Hows the work coming along? Also just so you know the bottom of imsto's poker case it completely flat.

[komar007]

Just a quick update:
I got back to the board today and I'm currently fixing alignment problems and positions of crucial parts. I've done the horizontal part, in a while I'll fix the vertical positions.
I also fixed one bug (two switches missing for short right shifts) and corrected the usb socket placement. Also the controller needed a bit of moving things around, because it could get in the way with horizontal bars in the plastic case (not a problem in imsto's case though).

I've also searched for some manufacturers and decided we have two ways to go about the production:
1. PCB and assembly separately
   pros: full control, we see the boards before they're assembled, but I'm not sure this really matters
   cons: we have to buy parts ourselves, make sure to get proper supported reels, or we'll pay more for technicians' work
             someone has to receive the boards, inspect them, send to manufacturer along with the parts, etc
             it's necessary to make sure the boards are compatible with the assembly company (panels or not, dimensions)
2. Full service company - I've found one locally, but obviously there are more all around the world
   pros: we don't care for anything, they buy the parts for us, make pcbs, stencils, pick-and-place and reflow, we get a ready product
   cons: probably we don't get to see if the board is ok before assembly of all of them, unless we ask and probably pay for a prototype


One obvious thing is that I need a prototype before making any real quantity orders and it would be good to have the prototype done by the same company that will later produce the final product. However, if you want to order just one, these companies are much more expensive than those that do single prototypes.


So I think after the pcb is done, I'll order a prototype anywhere just to see if I didn't make mistakes, especially as for component placement and alignment and later we'll have to assume that the final manufacturer won't produce a very different board.


I'm not sure exactly when I'll end the pcb, but if you're interested in an exclusive (well, kind of) pre-production prototype, drop me a PM.

[nebo]

Too many things have popped up in the last month that I want D: . If any help is needed with programming the controller I could pitch in when needed.

[komar007]

I will need some help eventually, but mostly with the GUI, firmware itself doesn't need much work. Or maybe it will, if so I'll talk to you!
Someone who knows Java/Swing will be very helpful too if we want it to be multiplatform.

[nebo]

Never really used Java but I co C# for a living and they're close enough I could pick it up fairly quickly.

[komar007]

Good. Java is not the only option.
C++/Python/Ruby/etc + Qt/GTK will be ok too.

[metalliqaz]

ugh Java = sad face

[komar007]

Here's what I have so far:


EDIT: I'm putting a link, no thumbnail. Just in case.
https://www.dropbox.com/s/yx6f5gr57m5gxc2/kb.png

Electrically speaking, it's missing a reset switch, and that should be it.


I've been measuring and measuring the distances between screw holes both in the case and poker pcb and this is all wrong. I can't measure it reliably so I have a question.


Could someone measure the relative positions of screw holes, put them on a drawing and post them for reference?
It seems I won't manage to do it, maybe my ruler and calipers are all wrong, I don't know.


I need help!

[TheProfosist]

Are we 100% just going with 1.5 1 1.5 7 1.5 1 1.5 bottom row the reason I ask is that that really limits what can be put on that keyboard for keycaps. Also do you think that I could get a blank layout of the GH60 do that I can start messing around with what my layout could potentially be?

[mkawa]

there's an issue with the attachment komar was trying to upload in his previous post. i'm working on it. unfortunately the only advice i can give right now is to attempt to make it smaller, komar and re-upload.

SDF(&*#)W(*%*)(#W$# smf *grumble*

[SmallFry]

Just a thought...totally off what you guys were currently talking about, but if you want a controller other than the Teensy I can fire up my AIKON controller project again.