Author Topic: The Living PCB Design Thread  (Read 178928 times)

0 Members and 1 Guest are viewing this topic.

Offline jmdaly

  • Posts: 43
  • Location: Ottawa, Canada
Re: The Living PCB Design Thread
« Reply #750 on: Tue, 05 June 2018, 08:29:18 »
I do have the ground planes set up, as per the tutorial. However I did end up with more large red areas which I assume are 'missing ground planes' than he has in the tutorial, which I was not sure what to do with.

Those red areas you see show that you have ground plane on one side of the board, but not the other. The trick to getting the ground plane over to the other side is to do via stitching. I followed https://forum.kicad.info/t/protip-nicer-via-stitching/1103 to do my via stitching.

Offline evn

  • Posts: 10
Re: The Living PCB Design Thread
« Reply #751 on: Tue, 05 June 2018, 12:02:26 »
Those red areas you see show that you have ground plane on one side of the board, but not the other. The trick to getting the ground plane over to the other side is to do via stitching. I followed https://forum.kicad.info/t/protip-nicer-via-stitching/1103 to do my via stitching.

Thanks! That actually worked out great https://i.imgur.com/qB1Fjyp.png

Offline jmdaly

  • Posts: 43
  • Location: Ottawa, Canada
Re: The Living PCB Design Thread
« Reply #752 on: Tue, 05 June 2018, 12:06:58 »
Those red areas you see show that you have ground plane on one side of the board, but not the other. The trick to getting the ground plane over to the other side is to do via stitching. I followed https://forum.kicad.info/t/protip-nicer-via-stitching/1103 to do my via stitching.

Thanks! That actually worked out great https://i.imgur.com/qB1Fjyp.png

Great, I'm glad it helped!

Offline evn

  • Posts: 10
Re: The Living PCB Design Thread
« Reply #753 on: Tue, 05 June 2018, 16:40:22 »
Okay I think this design is about ready to be scrutinised. Would someone be willing to have a look over my kicad files and point out any mistakes/errors? They're available here.

Offline hanya

  • Posts: 93
  • Location: Japan
Re: The Living PCB Design Thread
« Reply #754 on: Tue, 05 June 2018, 19:14:58 »
Okay I think this design is about ready to be scrutinised. Would someone be willing to have a look over my kicad files and point out any mistakes/errors? They're available here.
Hi,
- It is hard to solder through hole diodes under the switches. But it is OK if your switch having hole which allows you to put a diode on the case of the switch.
- In your design rules, you have 0.6 mm via dia and 0.4 mm via drill. This means 0.1 mm annular ring of via. I suppose you to make larger annular ring to match the design rule of the PCB manufacturer which you have choosen.
- If you want to make reference of some parts clear, place references away from pads and vias.
PFU HHKB JP, Sanwa MA-TB38 trackball

Online dead_pixel_design

  • Posts: 561
  • Location: Portland, OR
  • IIIV is not a Roman Numeral. Positive Vibes.
Re: The Living PCB Design Thread
« Reply #755 on: Wed, 06 June 2018, 02:55:50 »
Okay I think this design is about ready to be scrutinised. Would someone be willing to have a look over my kicad files and point out any mistakes/errors? They're available here.

I would recommend not running USB through vias where you can help it, and avoid 'T' junctions for your traces, you don't want hard 90deg angles.

Offline evn

  • Posts: 10
Re: The Living PCB Design Thread
« Reply #756 on: Wed, 06 June 2018, 07:23:55 »

I would recommend not running USB through vias where you can help it, and avoid 'T' junctions for your traces, you don't want hard 90deg angles.

I should be able to change the traces to avoid vias from the USB and remove 90deg angles without too much hassle. Thanks for your input! Do you know if wiring these 3 pads on the USB like this is okay? It isn't in the tut to do it, I just did it to get rid of an unconnected pads error.

Hi,
- It is hard to solder through hole diodes under the switches. But it is OK if your switch having hole which allows you to put a diode on the case of the switch.
- In your design rules, you have 0.6 mm via dia and 0.4 mm via drill. This means 0.1 mm annular ring of via. I suppose you to make larger annular ring to match the design rule of the PCB manufacturer which you have choosen.
- If you want to make reference of some parts clear, place references away from pads and vias.

- In the tutorial I followed he mentions that this diode placement only works for SMD diodes, so I'm gonna get SMD ones for this. That should be okay as I think the SMD diodes go on the other side, right?
- I haven't even looked into PCB manufacters yet, I'm going to do that now. Thanks for your help!

Online dead_pixel_design

  • Posts: 561
  • Location: Portland, OR
  • IIIV is not a Roman Numeral. Positive Vibes.
Re: The Living PCB Design Thread
« Reply #757 on: Wed, 06 June 2018, 15:43:38 »
Running the ground trace like that isn't a problem, but might be redundant since those pads will connect through the layers and ground.

SMD will be fine, no issues there, the diodes and switches are on different sides of the board so if you use SMD you won't run into problems.

The cheapest place I have found for getting a PCB printed was at https://jlcpcb.com/quote, but my pcb shape and size were normalish, I don't know how your PCB shape will affect costs.

Offline _ODIN_

  • Posts: 284
  • Location: Europe
Re: The Living PCB Design Thread
« Reply #758 on: Wed, 13 June 2018, 15:02:20 »
Do you know a good online shop located in Europe to by the components, like diodes and the controller, from?

« Last Edit: Tue, 19 June 2018, 16:21:43 by _ODIN_ »

Offline Croktopus

  • Posts: 3
Re: The Living PCB Design Thread
« Reply #759 on: Fri, 22 June 2018, 06:41:05 »
Hey, does anyone have an SMK 2nd gen footprint on hand? I sent out a couple PMs to people selling SMK boards and haven't heard back yet, so I figured I'd ask here

Offline Tech22

  • Posts: 4
Re: The Living PCB Design Thread
« Reply #760 on: Fri, 22 June 2018, 13:43:59 »
Hello. I want to use this type c pro micro controller with a custom pcb found at https://tinyurl.com/yby9bd42

How would I go about making the PCB to work with that? I am also confused on how I bridge each switch with the traces etc. I am using KiCad and my layout can be found at https://tinyurl.com/y9b6oftl

Thank you.
« Last Edit: Fri, 22 June 2018, 13:45:39 by Tech22 »

Offline MandrewDavis

  • Posts: 441
  • Location: Fl
  • Chasin' That Neon Rainbow
Re: The Living PCB Design Thread
« Reply #761 on: Fri, 22 June 2018, 17:29:24 »
Hey, does anyone have an SMK 2nd gen footprint on hand? I sent out a couple PMs to people selling SMK boards and haven't heard back yet, so I figured I'd ask here

I don't know if all 2nd gen SMK switches have the same pin spacing, but Scott who runs www.lfkeyboards.com was cool enough to post all his keyboard footprints on GitHub.
I've come to view humanity as predominantly monkey business.

My Classifieds Thread

Offline Croktopus

  • Posts: 3
Re: The Living PCB Design Thread
« Reply #762 on: Sat, 23 June 2018, 03:55:55 »
thank you so much mandrew!

Offline MandrewDavis

  • Posts: 441
  • Location: Fl
  • Chasin' That Neon Rainbow
Re: The Living PCB Design Thread
« Reply #763 on: Mon, 25 June 2018, 09:49:25 »
First of all, thank you for everyone who checked my schematic and gave me advice on my last project, it ended up working out great.

Currently, I am trying to create an AEK compatible PCB for the KBDFans KBD66 based on Hasu's Alps64 project. Due to a deficiency of pins, I placed solder jumpers so there is choice between having the reset LED or split-backspace and a third key to the right of the spacebar (neither of which I will use). Can anyone tell me if this is alright since I am about to send this out for fabrication.

Also, anyone have Alps64 parts on hand and can do the SMD work? Otherwise, I'll just buy a cheapo 858D.
I've come to view humanity as predominantly monkey business.

My Classifieds Thread

Offline Croktopus

  • Posts: 3
Re: The Living PCB Design Thread
« Reply #764 on: Fri, 29 June 2018, 02:34:19 »
id really like to add a volume wheel of some sort (like a knob from a car stereo, or a rolling design, or whatever really), but i have no idea how. has anyone here done something like that before?

Offline senso

  • Posts: 45
  • Location: Portugal
Re: The Living PCB Design Thread
« Reply #765 on: Mon, 02 July 2018, 04:25:21 »
Hardware wise, an encoder is what you want, lots of styles to choose from.

Offline Nixon

  • Posts: 15
Re: The Living PCB Design Thread
« Reply #766 on: Thu, 26 July 2018, 03:16:21 »
Designing a 39 key board using the new Kailh Chocs, similar to the Planck but 10 keys wide instead of 12. First complex design in Eagle so I thought I'd better upload it here to see if anyone can spot something I've done wrong. I know I've wasted space by mounting the Arduino Pro Micro behind and not underneath the keys, but wanted a pen tray so got space in the case and it made laying traces a whole lot easier. Will add mounting holes and a ground plane but just want to check that my progress so far is all good.

Edit: Here's the parts library for Eagle with the Kailh Choc in: https://github.com/skullydazed/clueboard_eagle
« Last Edit: Thu, 26 July 2018, 03:18:11 by Nixon »

Offline marhalloweenvt

  • Posts: 11
  • Location: Viet Nam
Re: The Living PCB Design Thread
« Reply #767 on: Thu, 26 July 2018, 05:16:32 »
Designing a 39 key board using the new Kailh Chocs, similar to the Planck but 10 keys wide instead of 12. First complex design in Eagle so I thought I'd better upload it here to see if anyone can spot something I've done wrong. I know I've wasted space by mounting the Arduino Pro Micro behind and not underneath the keys, but wanted a pen tray so got space in the case and it made laying traces a whole lot easier. Will add mounting holes and a ground plane but just want to check that my progress so far is all good.

Edit: Here's the parts library for Eagle with the Kailh Choc in: https://github.com/skullydazed/clueboard_eagle

So far, your work is still good. But i think you should put column pins in 1 side and row pins in other side of pro micro for easy to debug if there would be errors.

Offline MandrewDavis

  • Posts: 441
  • Location: Fl
  • Chasin' That Neon Rainbow
Re: The Living PCB Design Thread
« Reply #768 on: Wed, 08 August 2018, 15:28:55 »
I am a bit confused by everyone grouping the capacitors off to the side. I have been looking at the Teensy 2.0 schematic and TalkingTree's GH80-3000 PCB for reference. When using the ATmega32u4, do I need a 1μF capacitor on both the UVCC and VBUS lines? Also, does it matter whether I be put the 22Ω resistors for the D+ and D- lines near the MCU or USB port?  I've read the capacitor on pin 42 (AREF) is optional.

Done with this PCB so this is what I have (minus the ground plane).



I've come to view humanity as predominantly monkey business.

My Classifieds Thread

Offline bpiphany

  • Posts: 1012
  • Location: Stockholm, Sweden
  • bpiph is a special type of crazy. //mkawa
Re: The Living PCB Design Thread
« Reply #769 on: Fri, 10 August 2018, 09:10:27 »
Aref is optional altogether if you're not doing analog readings. I believe you should leave it unconnected if not used.

You need a 1uF cap on Ucap.

It's recommended to put the 22Ω resistors close to the pins.

It's recommended to have one 100nF cap close to each VCC pin, it's probably also advisable to have some bulkier capacitances close to the chip, as well as a big bulk capacitor over the VCC to GND pins. You should keep the total capacitance below 10uF to comply with the USB spec.

Decoupling is a complicated subject, and you are most probably better off overkilling it.

Offline AresTheGod

  • Posts: 96
  • Location: Paris, France
Re: The Living PCB Design Thread
« Reply #770 on: Sat, 11 August 2018, 17:19:56 »
First time using KiCad, but I'd like to create an on-board per keys RGB TKL pcb with multiple layouts available with USB Type C connector. I've read loads of thing about how to design PCB but almost none of them mention how to add per keys RGB. So far, the closest thing I've seen to what I'd like to do would be this https://easyeda.com/IBNobody/Matias_RGB_TKL_copy-2d2fab1805ff4c39b05c490e5ca4c47c?authenticate=force# . However, it doesn't meet every one of my requirements. I'm also not sure which controller I should use as I've seen people talking about a lot of different controllers such as the ATmega32u4 and the Teensy++ 2.0 .
Here's what I've done so far since I don't really understand which/where should I put the RBG led in here 201864-0
« Last Edit: Sat, 11 August 2018, 17:21:27 by AresTheGod »

Online ErgoMacros

  • Posts: 164
  • Location: SF Bay Area
Re: The Living PCB Design Thread
« Reply #771 on: Sat, 11 August 2018, 18:30:55 »
Hi,
I can't help with the RGB LEDs (sorry), but in terms of what micro controller board to use
start with your input/output pin requirements.

These will be something like:
  x = number of columns
  y = number of rows
  l  = number of indicator LEDs (caps lock, numb lock...)
  u = number of pins to talk to your RGB array

So you might need something like:
   17
+  6
+  0 or 3? Not sure about this count
+  3 or whatever you want
----
  29 or so available pins on your controller, minimum

Teensy++ 2.0 has lots (37!)
Pro Micro has 18.

You can get away with fewer by either adding hardware (chips) for things like multiplexing (http://www.openmusiclabs.com/learning/digital/input-scanning-matrix/shift-brigade/index.html) or creating more complex matrixes.

Your 17 x  6 keyboard, minus 11 blank key slots = 91 keys. A 10 x 10 matrix will cover 100 keys so if you wanted to create a "complex" matrix 20 pins would do (instead of 17+6 = 23)
Today's quote: '...“but then the customer successfully broke that.”

Offline AresTheGod

  • Posts: 96
  • Location: Paris, France
Re: The Living PCB Design Thread
« Reply #772 on: Sun, 12 August 2018, 03:59:30 »
So if I understood what you're saying, the pros of having a "complex" matrix would be to use fewer pins and the cons would be the "complex" part? Are the pros worth the cons? And the "complex" matrix would look like that? 201898-0

Online ErgoMacros

  • Posts: 164
  • Location: SF Bay Area
Re: The Living PCB Design Thread
« Reply #773 on: Sun, 12 August 2018, 13:34:16 »
Yes, exactly.
The pros of fewer pins are
* cheaper processor. . If you're producing millions of keyboards, and the larger (more pins) processor costs $1 more, it's probably worth it to design for the cheaper processor.
* for 1 keyboard the price difference is negligible.
* if the real estate on the PCB were very limited for some reason, having a physically smaller processor (fewer pins) could help.

The cons of fewer pins are
* not every key on keyboard row 0 would go to the same processor pin. So every time you wanted to know which 2 pins went to key you'd have to do a mental translation between the physical location and the microprocessor pins.
* The advantage of more pins is that the matrix is laid out just as you first posted. Each key maps to the same pins as it's neighbors.
This makes the keymap simpler, easier to "grok" as you change the key assignments.

Today's quote: '...“but then the customer successfully broke that.”

Offline AresTheGod

  • Posts: 96
  • Location: Paris, France
Re: The Living PCB Design Thread
« Reply #774 on: Sun, 12 August 2018, 14:08:21 »
Ok I see, thank you!
But by the way, since we’re using a Teensy controller, why not using the lastest? I saw a Teensy 3.6 somewhere and it had even more pins that the Teensy 2.0++. Would it also be overkill for a keyboard and be more expensive that it should be? Because it seems that nobody is using these newer version of Teensy.