I’ve been working on this schematic for the past few weeks, and I compared it to the given schematic for the G80 TH board.
I ordered some boards, and very unfortunately, nothing happened when I plugged it in.
Could you folks look over my schematic, and tell me if I missed something?
Impossible to read that.
Can you post the Eagle files somewhere and then we can have a look for you.
Some things to check in the meantime.
Is the 3.3V supply good with the USB plugged in?
What does it draw current wise when you plug it in?
@ adam8797 -
Are you aware of the following?
G80 TH
The module only needs 3.3V to operate, even if a USB cable is being used.
A external 3.3V power supply is required to power the board.
See:
https://www.ghielectronics.com/catalog/product/552
See:
Overview
@ adam8797 - the basics, measure 3.3V, reset, mode pin, check crystal…
Welcome to the community.
Sorry for the delay, I was barred for 8 hours as this is my first post.
As soon as I posted, I noticed that the forum down-scaled my image, but couldn’t edit.
Here’s the link to the Dropbox folder containing the .sch and .brd files.
As for 3.3V, there is a regulator onboard (U4 - MIC5219-3.3V), and it was working.
I’ve pulled Reset high.
I’m pretty sure that I have both clocks right.
So have you checked oscillations on xtals with an oscilloscope? Noise on power rails with o’scope?
How did you solder this?
Did any of your boards you mention work, or have you only built one?
Did you check orientation of G80 is correct?
@ Brett - I haven’t been able to get it on my scope yet. I’ll try that tomorrow and report back.
I’m 99.9% sure I have the G80 oriented the correct way. There are two circles, and only one looks like it was purposely put there. I used that one.
I soldered the first board with a combination of iron and hot air rework. I’ve been trying to make my own paste stencils, but its rough going. I’m trying to get the stencil right before I solder a second board.
Did you use the autorouter on this?
I think your fault with with the layout is with the crystals and the way you have laid them out on the board. These should be as close to the processor as you can get them and no other lines running under them. Check with a scope to be sure.
Your power rails are also way too thin.
Your decoupling CAPS should be as close to the processor power pins as you can get them. C1 to C 7 are all lined up and doing nothing. They should be located next to the processor.
There is no good ground path for the design as your ground lines are too thin. You ideally want a ground plane to give a good ground path return.
Your USB D+ and D- should be run as a differential path and a short run as possible. Try and avoid vias on these if you can. You can run longer but you need to run them in parallel and keep away from other lines as best you can.
I suggest beefing up the power rails to 40 mil (1mm) and just neck these down near the processor pins.
PS… If the CPU was aligned wrong, it will draw excessive power and get pretty hit quickly.
Yes, I did use the AutoRouter for a good portion, but I did most of the power by hand.
Thanks for the feedback. That’s the kind of good information that’s difficult to find on doc sheets.
Its called experience :whistle:
And there is a lot of that in this forum! 
@ njbuch - I’ve always been told that experience is just another name for a long string of mistakes ;D
In an interesting turn of events, I soldered a second board up, and it was actually recognized by the computer!
All I see right now is a “GHI Bootloader Interface”. I haven’t been able to make it do anything else yet, but I’m working on it.
And I just flashed the first program! It worked.
Thanks to everyone for your help. It seems to have just been a bad solder job on my part.
But special thanks to @ Dave McLaughlin for that valuable information. I’ll be sure to reference it when I eventually design Rev B.
@ adam8797 - I read Dave’s comments as saying their might be some unpleasant surprises with the current design.
@ Mike - Oh I understand, and I will be taking that into consideration during redesign. This was my first prototype, and I’ll be expecting some odd behavior.
Correct. The long and different length lines on the crystal and the decoupling caps not being close to the processor is often a failure point. It all seems to work well until and then it suddenly stops. At least for now you can get your coding done but it may give issues once the software is running and currents are fluctuating.
A good friend of mine used to design the boards without any decoupling and we had all sorts of issues with freezing etc. I kept screaming at him, decoupling, decoupling and the next revision and all boards since then have worked perfectly.
On you other board that is not working, check for pins not properly soldered or shorted. That is the most likely culprit.