4.2V in my 3V3?!

[mftkoehler]

Board layout

Screen Shot 2013-11-07 at 6.51.46 AM.png (212.55 KiB) Viewed 399 times

Hey all.

I'm trying to build an alarm clock for my world-traveling, fairly deaf father. I've done a mashup of several Adafruit designs with my own to produce the attached board. The clock is powered from USB since they're ubiquitous in the US and Europe. The basic design uses an ATMega 328 to take output from a ChronoDot and displays it on one of the Adafruit 1.2" 7-segment displays using a rotary encoder to interact with the user. I've also incorporated an iPhone charger, a light sensor to dim the display and a buzzer for an alarm, but found that my father doesn't hear the frequencies that a piezo buzzer can produce well. So I added sound, inspired by the wave shield design. MicroSD for input, run it through a DAC and amplify. The microSD of course requires 3V3 and level shifting, so I put that in as well. This has now become the source of my issue. I've had boards made at OSHPark, soldered them up and done some basic testing. 5V works fine, my iPhone charges, BUT 3V3 is not 3.3V, it's 4.2!

Here's my troubleshooting so far:

1. replaced the 3V3 regulator: no change
2. soldered a R220 between my 3V3 test point and ground to give it a load: no change
3. checked the traces on my board under magnification to make sure I hadn't solder bridged between my two voltages at the voltage regulator
4. checked the spot near the 5V decoupling capacitor (C7) at the 3V3 regulator to see that it is in fact physically separate from the 3V3 output right next to it. It's under solder mask, but appears to be OK.

Now I'm at a loss. Am I missing something obvious?

Thanks in advance,

Mike

[zener]

Am I missing something obvious?

Yes. Your regulator footprint is wrong. Vout and GND are swapped.

http://www.st.com/web/en/resource/techn ... 000544.pdf

[mftkoehler]

Aaaargh! Thanks very much for finding this. It has been tormenting me for days. Hello, green wire!

Mike

[mftkoehler]

Screen Shot 2013-11-07 at 1.34.49 PM.png (17.53 KiB) Viewed 368 times

I just went back and looked at my .brd file again and I don't see that I've swapped the pads. I've mounted this rotated 180 degrees, so +5V comes in on the left, 3V3 is in the middle, and ground is on the right. That's what I have...

Mike

[zener]

Sorry! Are you measuring the 4.2V right at the regulator from pin 2 to pin 1 ?

[Renate]

As long as you are playing with the regulator, measure the voltage of the 3.3 V with the regulator out.
Still 4.2 V, huh?

I'll bet the 5 V is feeding an input on a 3.3 V device and the protection diode is routing the 5 V into the 3.3 V with a drop of 0.7 V.

[zener]

That is exactly what I was thinking, and the next test I was going to suggest. However I only see two 3.3 devices, an SD socket and a 74VHC125. The data sheet for that says specifically that the inputs can accept voltages higher than Vcc. However, it doesn't say what would happen in that case. An equivalent input circuit was shown, and there were no clamping diodes on it. But yes, I would remove the regulator, and if the voltage is still there, then start cutting lines free until the source is tracked down.

[mftkoehler]

Thanks so much for all your help. I found the error last night, prompted by Zener's question of whether I had measured the voltage directly at the 3V3 regulator. As it happened, I hadn't, and I found that both ground and output were at 4.2V! WTF? I took one of my unpopulated boards and started checking for ground continuity, and found that everything was connected to my ground plane except the 3V3 regulator and test point. When I went back to the schematic, I found the problem. I hadn't ever connected the net at the regulator to ground. I green wired in a connection, and everything works now! (Well, I see 3.3V. I'm not claiming victory on all the stuff on the board yet, but at least I can load in the bootloader and check.)

Thanks again!

Mike

[adafruit_support_mike]

Now that your main problem is solved, I have a secondary question:

I saw that your design calls for TL072 dual op amps. Are those actually working for you in a 5v single-supply setup?

As I remember them, TL07/8* op amps require the input to be about 3v higher than the negative rail and can only deliver output to within about 1.5v of either the high or low rails. They were designed in the era of +/-15v split supplies, and had plenty of swing to send signals to +/-10v circuits. What you have looks to be equivalent to +/-2.5v, which seems awfully tight.