ADC design help

[mechknoll]

So I had a board printed from Oshpark for a 24-bit ADC,TI ads1255.  I am powering it with a 9V battery.  Now there is one obvious mistake... both the TPS7133 and TPS7148 have their enable tied high when they should tied to ground.  I have another board I am going to solder up tomorrow, but I could really use another set of eyes.

Thank you!

[free_electron]

Wow. What a mess ! Clean up you schematic !
This thing is full of mistakes. Look at pin 5 of the chip top,eft. That wire coming from the bottom is not connected. There is no dot at the t junction !

There are more like that.

Or are you overlaping wires and pins ?

Yikes. You are.. I see you do the same around the connectors.
I also see dots where there are not supposed to be any...
I also see parts that do not have a designator... Just a *

This is a recipy for disaster... Learn how to draw clean schematics. You are just asking for faulty boards.

[dannyf]

You are just asking for faulty boards.

That's the crowd sourcing way of engineering.

[CarlG]

Hi,

With 2% tolerance the output voltage of the TPS7148 might be below min supply for the ADC. And why use a 4.8V regulator when the recommended supply is 5V? Something leads me to think you want to use a USB supply here...which can be down, what is it, 3.8V? And even if you have 5V in, the PSRR at 5Vin/4.8V out is basically none. Use 9V or 12V in, 5V out instead.

U1 does not seem to have any supply connected.

Noise from the ADC digital supply will couple through the TPS7133 and affect the ADC performance.

Wouldn't it be wise to have a GND connection (or 2-4 of them) in P3?

BR,
Carl

[mechknoll]

Ok thanks guys for the honesty.  I need that if I ever hope to become a better engineer.  I replaced the 4V8 LDO with a 5V0 LDO... So thats fix 1.   I can run a patch wire to the 3V3 and power it directly from 9V battery so no noise from the 5V rail makes its way to the 3V3.  The ADS1255 is connected to the 4V8.  I cleaned the schematic a bit.  Still some mess around P3 and P4.  Thanks guys

[mechknoll]

Also, the headers P3 and P4 are for an arduino nano.

[CarlG]

Hi, the schematic looks better now, but it can still be cleaned up a bit. E g the placement of C8 is miserable. Messy schematics have a strong tendency to go along with stupid misses like the missing ref supply before. Or connecting the Vref supply to a single pin net...  So get it right.  Including defining all refdes. NC crosses (or similar) on deliberately open pins is also recommended.

You get credit for the protection diodes   Using schottky diodes instead might be considered.

Connect U1 sleep pin to its supply pin (optionally via a pull up R) - but that was your intention of course

Depending on your board (2 or 4 layer?) and layout , you might need a small cap at U1 supply pin as well.

If you're going into this business, you might start adding a pull-down/pull-up resistor on enable pins right now. In real life, i.e. in production tests the manufacturer wants to be able to disable anythin that can be disabled. While your at it, you could add a pullup on the reset and PDWN pins as well.

Regarding the noise coupling, the noise that couples through IC3 will couple through IC1 as well...what you need is a ferrite bead. The question then is where  to put it. With a 4-layer board, I'd put it between IC3 output (with a minimum cap) and the decoupling caps for ADS1255, make a local plane for DVDD.

A series resistor on the oscillator output is generally needed to trim the drive level of the crystal. Sometimes a parallel R across XIN/XOUT is a good feature, but sometimes it's included on the chip.

BR,
Carl

[mechknoll]

Carl, thanks I really appreciate your comments!  It is a 4 layer board.  i feel like a numskull having it printed already.    Looks like its time for a ton of patch wires! 

[daqq]

Hi,

The Analog iCoupler isolators can generate a fair bit of noise. For the actual layout, please read:

http://www.analog.com/static/imported-files/application_notes/AN-1109.pdf

What are you going to measure? Won't the leakage current of the diodes (several uA) be an issue?

The REF192 is connected to a +4V8 net. I can't find it anywhere else on the schematic.

Just a minor point: Why are you designing the board with more than one size of caps? 0402 for the crystal ones, others 0805?

[mechknoll]

The 4V8 is a typo from the original schematic.  It is connected to 5V rail.  I am trying to measure a differential voltage from a high end accelerometer.  Yea the leakage on the diodes could pose a problem...  Should I just leave them out?  The accelerometer should not be providing a signal larger than 1V diff... but that being said it will most likely be dropped and be subject to several g's!!!

[CarlG]

Then use discrete N-channel JFETs type J11 or equivalent instead. Connect source and drain to form a diode from the gate. Add series resistors to limit the current.