1. Home
  2. Electronics Design
  3. Micro and ADC

Micro and ADC

Hi,

I am assigned to layout a mixed signal printed circuit board for the first time. The main chips on the board are as follows

  1. Microprocessor: MSP430F5438AIPZ ; just one on the board

  1. Analog to Digital Converter: ADS1298IPAG; four on the board

  2. Multiplexer : ADG732BSUZ

The size of the board is approximately : 4.5 inches Long adn 3.5 inches wide

I started looking into application notes to design the PCB and found that I need to follow rules inorder to get this PCB done. But application notes do not mention issues related with four on board ADCs.

  1. I am looking for a Layer Stack up scheme that can help in

a. keeping the noise low b. low EMC

  1. I need your views about the following layout stack up

Eight Layer Board: Layer1 : Slow Analog Signal ( Only Analog Chips) {Top Layer) Layer2: Analog Ground Plane Layer3: Power Plane Layer4: Analog Signal Routing Layer5: Digital Ground Plane Layer6: Digital Signal Routing Layer7: Analog Ground Plane Layer8: Digital Fast Signals ( Only Digital Chips) { Bottom Layer }

For example, the clock line will go from bottom layer through via and appear next to the ADC's clock pin and will be routed on the Layer 6. So, it will stay between the two Analog Plane Layers. Any comments!

  1. I also read that tight coupling between the layer can also keep the crosstalk to a minimum. The formula 1 / 1+ ( D/H )^2 . Where

D is the distance between the two traces H is the height of the trace above the circuit board.

Is this true? If yes, than does it mean that I have to keep the width of the prepeg in mind? Should I ask the board manufacturer to use the thinnest prepeg he can use.

  1. The system will run on 16 to 20MHz clock and 16 bits will be used from the 24 bit ADC. The gain on the board is 50. So, according to the following application note

formatting link

How can I use this appllication note to design my PCB?

  1. The box for this circuit in made up of plastic and it will be non shieled.

I think that you guys might say that the frequency is too low for this kind of stack up plane. But this is my first board and I want it to be perfect.

jess

Reply to
jsscshaw88
Loading thread data ...

time. The main chips on the board are as follows

need to follow rules inorder to get this PCB done. But application notes do not mention issues related with four on board ADCs.

That will be hard to enforce in real life. Like, can you route all the "fast digitals" on one layer.

I'd vote for a single ground plane on layer 2 of, probably, a 4 or 6 layer board. Maybe

1 sigs 2 gnd 3 power pours 4 sigs

The ADC inputs are differential, so small ground loops aren't an issue. Just keep the nasty digitals away from any analog stuff.

Does the box have to be plastic? That may cause EMI problems.

--

John Larkin         Highland Technology, Inc 

jlarkin at highlandtechnology dot com 
http://www.highlandtechnology.com 

Precision electronic instrumentation 
Picosecond-resolution Digital Delay and Pulse generators 
Custom laser drivers and controllers 
Photonics and fiberoptic TTL data links 
VME thermocouple, LVDT, synchro   acquisition and simulation
Reply to
John Larkin

Hi,

I am thinking about keeping the Digital Signals on the Bottom Layer and on Layer6 and through vias will be connected to the ADC's Digital pins. The vias will be very close to the ADC's digital pins. The ADCs are on the top layer.

I can not change the box, it will be a plastic.

jess

Reply to
jsscshaw88

time. The main chips on the board are as follows

need to follow rules inorder to get this PCB done. But application notes do not mention issues related with four on board ADCs.

I'd put this design on a 2 layer board. Just optimize parts & pins so you can route most signals on the top layer and keep the bottom layer as a mostly solid ground plane.

Placing the parts in a way you don't need vias is the key to a good PCB layout.

--
Failure does not prove something is impossible, failure simply 
indicates you are not using the right tools... 
nico@nctdevpuntnl (punt=.) 
--------------------------------------------------------------
Reply to
Nico Coesel

Draw a line across the board. Label one side of it "quiet", and the other side "noisy". Place your ADCs and the multiplexer so they straddle the line, with the digital pins on the noisy side and the analog pins on the quiet side (pay attention to digital vs. analog grounds, while you're at it). Place any power-supply filtering or regeneration at the border, too.

Ideally the line will stay straight, but if it must have curves or kinks, let it.

Keep all the digital nets on the "noisy" side, and all the analog nets on the "quiet" side.

Don't bother with special layers for different signals -- horizontal separation is better than vertical separation.

If you have a sophisticated-enough board layout package, you can enforce this electronically. Otherwise, you'll have some hand work to do.

Then wait for Joerg to chime in on this thread, and do whatever he says.

--
My liberal friends think I'm a conservative kook. 
My conservative friends think I'm a liberal kook. 
Why am I not happy that they have found common ground? 

Tim Wescott, Communications, Control, Circuits & Software 
http://www.wescottdesign.com
Reply to
Tim Wescott

Incredible. You must be a 4PCB shareholder. A 4-layer design would be no brainer. With careful layout, this could be done on 2-layer board.

Put the routing on the outer layers and leave ground and power planes inside; so you would be able to troubleshoot the board.

Vladimir Vassilevsky DSP and Mixed Signal Consultant

formatting link

Reply to
Vladimir Vassilevsky

.
f

le

,

Gufaw..

All good advice otherwise. I was going to add that looking at the signal flow on the schematic can help with the pcb. (provided the schematic's not a rat's nest.)

ttdesign.com- Hide quoted text -

Reply to
George Herold

snipped-for-privacy@gmail.com schrieb:

Hello,

you will get heavy problems in routing the digital signals on one layer only, I would recommend at least two layers, one for horizontal traces and one for vertical. If there are only short and few traces, one layer is possible.

Bye

Reply to
Uwe Hercksen

That makes good sense, but what exactly do you mean by that last statement, Tim? Where should the grounds go?

To the OP: A four layer PCB should be enough. Signals on top and bottom, one full ground plane and power distribution inside. Don't cut up your ground plane, keep the area of loops carrying substantial currents small and keep nodes having large fast voltage swings small too. Keep sensitive tracks away from noisy ones. I they have to get close, put them on different layers.

Keep in mind that copper is no superconductor and that traces have inductance too. A trace carrying large currents or fast- changing signals does not have the same potential throughout.

Don't use components, logic or amplifiers, much faster than they need to be. Keep impedance of sensitive nodes as low as you can get away with. (Those are circuit design issues, which I suppose are not in your hands.)

Jeroen Belleman

Reply to
Jeroen Belleman

Hi,

So, it means that the PCB will be fine in both cases. It does not matter if I go with Four Layer board or with 8 layer board with the layer stack scheme that I mentioned in my original post.

jess

Reply to
jsscshaw88

Well, if "does not matter" includes a quadrupled cost.

Suit yourself...

Tim

-- Deep Friar: a very philosophical monk. Website:

formatting link

Reply to
Tim Williams

ElectronDepot website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.