Author Topic: The Living PCB Design Thread  (Read 198342 times)

0 Members and 2 Guests are viewing this topic.

Offline jmdaly

  • Posts: 44
  • 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: 44
  • 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: 96
  • 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

Offline dead_pixel_design

  • Posts: 586
  • 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!

Offline dead_pixel_design

  • Posts: 586
  • 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: 450
  • Location: Valhalla
  • Figth for honor!
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: 13
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 »

Online MandrewDavis

  • Posts: 450
  • 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: 13
Re: The Living PCB Design Thread
« Reply #762 on: Sat, 23 June 2018, 03:55:55 »
thank you so much mandrew!

Online MandrewDavis

  • Posts: 450
  • 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: 13
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: 47
  • 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: 19
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: 17
  • 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.

Online MandrewDavis

  • Posts: 450
  • 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: 1015
  • 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 »

Offline ErgoMacros

  • Posts: 199
  • 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

Offline ErgoMacros

  • Posts: 199
  • 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.

Online MandrewDavis

  • Posts: 450
  • Location: Fl
  • Chasin' That Neon Rainbow
Re: The Living PCB Design Thread
« Reply #775 on: Sat, 18 August 2018, 22:00:36 »
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.

Thank you once again for such a detailed response. I do have the 1uF capacitor on UCAP and will remove the on AREF, but other than than does everything look good? When you say VCC, does that only include just the pins 14 and 34 or the UVCC, VBUS and AVCC pins too?
I've come to view humanity as predominantly monkey business.

My Classifieds Thread

Offline hanya

  • Posts: 96
  • Location: Japan
Re: The Living PCB Design Thread
« Reply #776 on: Sun, 19 August 2018, 00:49:18 »
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.
Not so many people designs full size keyboard which requires many pins. If you design such PCB, you can put MCU on your board directly. No need to put external board.
If you use RGB LED contains own controller such as SK6812, its V_HIGH is 3.4V on 5V circuit. Teensy 3.6 works on 3.3V and it might not work with the LED. Most of them might work well even with 3.3V but some might not work.
Not only the price of the board but components on your circuit is also important to choose target MCU. You can use level converter between 5V and 3V system if you really needed.
PFU HHKB JP, Sanwa MA-TB38 trackball

Offline _ODIN_

  • Posts: 450
  • Location: Valhalla
  • Figth for honor!
Re: The Living PCB Design Thread
« Reply #777 on: Sun, 26 August 2018, 08:34:55 »
hello guys, do you know where to get the kicad footprint of this component? http://www.kailhswitch.com/uploads/201815927/PG151101S11.pdf


Offline bpiphany

  • Posts: 1015
  • Location: Stockholm, Sweden
  • bpiph is a special type of crazy. //mkawa
Re: The Living PCB Design Thread
« Reply #778 on: Tue, 28 August 2018, 06:03:36 »
Thank you once again for such a detailed response. I do have the 1uF capacitor on UCAP and will remove the on AREF, but other than than does everything look good? When you say VCC, does that only include just the pins 14 and 34 or the UVCC, VBUS and AVCC pins too?

Slow response, but the answer improved from it I believe =) When you are doing a simple design powered through USB with 5V IO everything VCC is the same. There are some different scenarios in the chapter " USB Module Powering Options" in the datasheet http://ww1.microchip.com/downloads/en/DeviceDoc/doc7799.pdf

Offline CameronBanna

  • Posts: 5
  • Location: San Diego, California
Re: The Living PCB Design Thread
« Reply #779 on: Tue, 04 September 2018, 00:27:09 »
hello guys, do you know where to get the kicad footprint of this component? http://www.kailhswitch.com/uploads/201815927/PG151101S11.pdf

If you google search "kailh socket kicad" you can find quite a few.
Heres one for example. https://github.com/daprice/keyswitches.pretty

Online MandrewDavis

  • Posts: 450
  • Location: Fl
  • Chasin' That Neon Rainbow
Re: The Living PCB Design Thread
« Reply #780 on: Wed, 05 September 2018, 21:56:28 »
Thank you once again for such a detailed response. I do have the 1μF capacitor on UCAP and will remove the on AREF, but other than than does everything look good? When you say VCC, does that only include just the pins 14 and 34 or the UVCC, VBUS and AVCC pins too?

Slow response, but the answer improved from it I believe =) When you are doing a simple design powered through USB with 5V IO everything VCC is the same. There are some different scenarios in the chapter " USB Module Powering Options" in the datasheet http://ww1.microchip.com/downloads/en/DeviceDoc/doc7799.pdf

Thanks, must have missed all that when looking through the 32u4 files, added a 1μF capacitor to VBUS. I'll have this off to fab once I get the USB port measurements coordinated with the case.
I've come to view humanity as predominantly monkey business.

My Classifieds Thread

Online Moosewing

  • Posts: 3
Re: The Living PCB Design Thread
« Reply #781 on: Wed, 12 September 2018, 15:34:52 »
Hoping to order a prototype within the next few days, but I'd like to run it by someone first.

Schematic and BOM:



I know it's bad practice but I didn't put the switch matrix in the schematic because it was constantly changing up until the end and I didn't want to bother editing the schematic after every little change. I'll be better about this in the future, I promise.

Full board pics:



This PCB is going to be used for a few different projects involving Omron B3G-S and KPT switches. The outermost pins in these switches are connected internally, so it's easy to go row2col and keep it (mostly) on one layer. I originally had it wired col2row until I opened up my FK-555 and noticed this pattern on its PCB.

MCU pics:



I only just realized as I was making this post that I forgot to connect the bottom left VCC pin to the rest of the VCC pins. That aside, I have a few questions.
Does it matter which VCC pin is connected to the USB port since they're all connected anyway? I have mine connected to uVCC but a lot of boards I've seen have it connected to VBUS.
I have a ground plane on each layer, connected together by the mounting holes. Are those enough, or should I add some via stitches elsewhere?
How should I go about connecting the isolated copper islands under the MCU and by C1 and C4/R3? I have a via on each section just to mark and identify which ones need to be connected, but beyond that I'm not sure. And of course, if anything else needs to be changed, I'm all ears.
« Last Edit: Thu, 13 September 2018, 17:59:50 by Moosewing »

Offline RealLaugh

  • Posts: 139
  • Location: Germany
Re: The Living PCB Design Thread
« Reply #782 on: Fri, 14 September 2018, 00:38:47 »
it might be the software you're using but I don't see the 2 other pins (2 and 4) on the quartz going to GND?

More
Hoping to order a prototype within the next few days, but I'd like to run it by someone first.

Schematic and BOM:
Show Image

Show Image


I know it's bad practice but I didn't put the switch matrix in the schematic because it was constantly changing up until the end and I didn't want to bother editing the schematic after every little change. I'll be better about this in the future, I promise.

Full board pics:
Show Image

Show Image


This PCB is going to be used for a few different projects involving Omron B3G-S and KPT switches. The outermost pins in these switches are connected internally, so it's easy to go row2col and keep it (mostly) on one layer. I originally had it wired col2row until I opened up my FK-555 and noticed this pattern on its PCB.

MCU pics:
Show Image

Show Image


I only just realized as I was making this post that I forgot to connect the bottom left VCC pin to the rest of the VCC pins. That aside, I have a few questions.
Does it matter which VCC pin is connected to the USB port since they're all connected anyway? I have mine connected to uVCC but a lot of boards I've seen have it connected to VBUS.
I have a ground plane on each layer, connected together by the mounting holes. Are those enough, or should I add some via stitches elsewhere?
How should I go about connecting the isolated copper islands under the MCU and by C1 and C4/R3? I have a via on each section just to mark and identify which ones need to be connected, but beyond that I'm not sure. And of course, if anything else needs to be changed, I'm all ears.

Online Moosewing

  • Posts: 3
Re: The Living PCB Design Thread
« Reply #783 on: Fri, 14 September 2018, 10:31:10 »
it might be the software you're using but I don't see the 2 other pins (2 and 4) on the quartz going to GND?

2 and 4 are connected together, and then 2 is connected to the ground plane. I'll go ahead and connect it manually to the ground pads on the capacitors though.

Offline online

  • Posts: 124
Re: The Living PCB Design Thread
« Reply #784 on: Wed, 19 September 2018, 10:18:59 »
Hi everyone,

I'm trying to design a pcb with atmega32u4 by following the pcb design guide on github. Got some pcbs made.
Soldered 4-5 of them but all have the same problem.
When it connected to PC (Windows 10), it recognised as 32u4 and detected by Atmel flip as well. However, after it plugged in for around 15mins, it disconnected by itself. It continue failed to be recognized after I reconnect it.

It happened with or without firmware flashed-in. I checked all pins are not shorted.

I set all trace to width to 6.30mil(0.16mm) and realised the VCC trace width is too thin after I sent the file to the manufacturer, could this be the problem?

Here is the schematic and PCB. Please help. :(
203917-0
203919-1
« Last Edit: Wed, 19 September 2018, 14:43:44 by online »

Offline tedfs3

  • Posts: 18
    • No Mercy Given
Re: The Living PCB Design Thread
« Reply #785 on: Sun, 23 September 2018, 19:50:24 »
Has anyone done up KiCad footprints and symbols for Kailh BOX switches or do the MX footprints suffice ? I'm not entirely clear if the nubs on the switch need to sit ON the PCB or if they sit down IN the PCB.

Offline senso

  • Posts: 47
  • Location: Portugal
Re: The Living PCB Design Thread
« Reply #786 on: Tue, 25 September 2018, 05:38:53 »
Hi everyone,

I'm trying to design a pcb with atmega32u4 by following the pcb design guide on github. Got some pcbs made.
Soldered 4-5 of them but all have the same problem.
When it connected to PC (Windows 10), it recognised as 32u4 and detected by Atmel flip as well. However, after it plugged in for around 15mins, it disconnected by itself. It continue failed to be recognized after I reconnect it.

It happened with or without firmware flashed-in. I checked all pins are not shorted.

I set all trace to width to 6.30mil(0.16mm) and realised the VCC trace width is too thin after I sent the file to the manufacturer, could this be the problem?

Here is the schematic and PCB. Please help. :(
(Attachment Link)
(Attachment Link)

Your decoupling caps are in a nice row, miles away from the micro-controller.

Traces are too thin as you said.

No ground plane, ground is horrible as well, and it seems like your bypass caps ground is not connected to anything

Offline bpiphany

  • Posts: 1015
  • Location: Stockholm, Sweden
  • bpiph is a special type of crazy. //mkawa
Re: The Living PCB Design Thread
« Reply #787 on: Tue, 25 September 2018, 07:53:38 »
and it seems like your bypass caps ground is not connected to anything

Good spotted, I didn't catch that. Which also would mean the oscillator caps are not connected to GND either. The oscillator circuit layout in whole is questionable as well I'd say.

It's hard not to sound harsh about it, but did you read up anything at all on circuit design?

Online Findecanor

  • Posts: 3958
  • Location: Stockholm, Sweden
  • On the outside looking in
Re: The Living PCB Design Thread
« Reply #788 on: Tue, 25 September 2018, 14:13:41 »
(Attachment Link)
BTW. I see quite a few junctions between rows and columns in that matrix. (I suppose you would have spotted and corrected those yourself by now, but anyway...)
Smoking is assault. I defend myself.
Daily driver: Phantom (Lubed Cherry MX Clear, Lasered Cherry PBT keycaps with Row A. Plastic "Frankencase". Custom firmware, Swedish layout)

Offline N9vem

  • Posts: 1
  • Location: Hungary
Re: The Living PCB Design Thread
« Reply #789 on: Fri, 05 October 2018, 17:16:41 »
Hi!
Are there someone who designed a pcb for RAFI RS 76 C switches? Can hall effect switches be compatible with QMK? I'm only briefly run trough the rafi schematics and I'm not good enough / I don't have time enough to design a pcb for 76 C switches yet, but its one of my further goals. Does somebody encountered Marquardt Two Fingers Typewriter switches, is it worth the time to design a pcb for them (for those great doubleshot keycaps)?
Thanks!

Offline LifeZ

  • Posts: 655
  • LifeZone
Re: The Living PCB Design Thread
« Reply #790 on: Thu, 18 October 2018, 20:02:49 »
Hello guys,  ;D
I am going to study artwork.
It is not easy because there is no knowledge about electronics.
I use Altium.
I just want to follow various things.

Offline online

  • Posts: 124
Re: The Living PCB Design Thread
« Reply #791 on: Sun, 21 October 2018, 07:11:37 »
Hi everyone,

I'm trying to design a pcb with atmega32u4 by following the pcb design guide on github. Got some pcbs made.
Soldered 4-5 of them but all have the same problem.
When it connected to PC (Windows 10), it recognised as 32u4 and detected by Atmel flip as well. However, after it plugged in for around 15mins, it disconnected by itself. It continue failed to be recognized after I reconnect it.

It happened with or without firmware flashed-in. I checked all pins are not shorted.

I set all trace to width to 6.30mil(0.16mm) and realised the VCC trace width is too thin after I sent the file to the manufacturer, could this be the problem?

Here is the schematic and PCB. Please help. :(
(Attachment Link)
(Attachment Link)

Your decoupling caps are in a nice row, miles away from the micro-controller.

Traces are too thin as you said.

No ground plane, ground is horrible as well, and it seems like your bypass caps ground is not connected to anything

Thanks for your help. I've re-designed another test board based on your suggestion and it works! :)

and it seems like your bypass caps ground is not connected to anything

Good spotted, I didn't catch that. Which also would mean the oscillator caps are not connected to GND either. The oscillator circuit layout in whole is questionable as well I'd say.

It's hard not to sound harsh about it, but did you read up anything at all on circuit design?

I'm a total noob when it comes to circuit design, I read ruiqimao keyboard pcb design guide and also bits of info from everywhere.
atm, I'm just copying people's design and modify the layout to fit my need, didn't realise it's not as straightforward as I wish to be.

Didn't know the decoupling caps need to be placed near the IC.  :-\

PCB layer is filled with ground plane, is this a correct way to ground oscillator?


Here is another test board which is working, but any suggestion on improvement will be appreciated.
205871-0
205873-1

Offline bpiphany

  • Posts: 1015
  • Location: Stockholm, Sweden
  • bpiph is a special type of crazy. //mkawa
Re: The Living PCB Design Thread
« Reply #792 on: Tue, 23 October 2018, 09:51:53 »
That looks a lot better =)

I would rotate the controller 180° to route the USB lines shorter. Everything else should be equally easy to route that way. There is no reason not to move C4 closer to its VCC pin. You could move C3,7,8 closer to the chip as well.

I never used an external pull-up resistor on the reset pin, and I never had any problems without one. I would just drop R1 completely.

I would rotate C6 to have its axis pointing towards the controller (like the other caps and resistors), but that's just personal preference.

Offline marhalloweenvt

  • Posts: 17
  • Location: Viet Nam
Re: The Living PCB Design Thread
« Reply #793 on: Tue, 23 October 2018, 22:42:15 »
Hello,

I am designing my PCB with Kicad. Could you guys please give me some advices/tips in how to route track? For now, my tracks on pcb are a mesh. I just want to make them as beautiful as you guys did.
I am very appreciated with every single advice/tip you guys can give me.