# PCB Layout Help (with schematics!) - Split ground plane or not?

Obligatory "not an EE, just a ChemE trying to make some pressure readings for science"!

Schematic attached, along with my current layout. It's a 6-channel pressure sensor using MPX4115AP sensors and an AD7606-6 simultaneous sampling ADC. The ADC is overkill, probably, but I happen to have about a dozen laying around. It communicates to the host via SPI.

Each pressure sensor has bypass caps and an RC filter on the output to remove any fluctuations that occur due to high-frequency pressure disturbances in my system.

The whole board is powered by a single LM-1117 5V regulator in an SOT-223-4 package. The upper-left corner of the board acts as a heat sink. With the exception of the two pours in the upper-left (+5V and the regulator input capacitor), all the other pours on the top layer are ground. The entire back layer is +5V.

I've been reading a lot about how to properly lay out a ground plane to separate analog and digital portions of an ADC system. This design uses a star ground point at pins 2 and 3 of the ADC. The ground plane under the ADC itself goes off and runs under all the sensors, while the ground plane under J2 and all the digital pins is split off, only tied together at the star ground point.

I have a few questions. Am I overthinking this? Do I really need to separate the ground planes when everything runs off a single supply? I'm already using maximum oversampling on the ADC since I have plenty of time to take measurements (around once per second, later averaged to a 5-second reading). The measurements don't need to be ultra precise, either.

If separate ground planes are recommended, should I separate the power plane as well? I've read that one uses separate ground planes when the analog and digital circuitry are operated from different supplies, but I'm not doing that, hence my 1st question about split ground planes.

• Just want to say, for a non-EE, that layout looks fairly good, at least at first glance! Jun 15 '18 at 0:41
• @Felthry Thanks! It's not my first PCB, but it's my first time using such a powerful ADC. Jun 15 '18 at 0:44
• This is a frequently asked question. Don't split ground. Also, if at all possible, dedicate one side of the board entirely to GND (put a completely solid GND plane on one side of the board or the other. This is much more important than having a solid VCC. Keep lots of space around analog signals. Do those two things and you shouldn't have much problem. If you flood the other layer with GND in the otherwise unused spaces, make sure you use lots of vias to tie the chunks of copper to the plane. Jun 15 '18 at 4:29
• If you can't make a completely solid ground plane, at least try to keep it mostly solid, and use it only for short traces that don't split it up too bad. Jun 15 '18 at 4:32
• I would say that unless you are an expert in analog or RF design, or have one nearby to help you, you should always avoid splitting ground planes. In general, the purpose of the ground plane is to provide a low impedance return path for all AC and DC currents. Splitting it NEVER reduces the impedance. It only increases it. If you use a split to fence GND current out of an area where you don't want current, you have created potential for radiated emissions and increased the voltage gradient on some portion of the GND plane when current is flowing. Jun 20 '18 at 16:13

Replying as one nonEE who did his share of circuits to another nonEE...

First of all you have a clean schematic and a clean layout, so chances are things will just work as they are already. This is the benefit of overthinking the design in the right way.

Now, for the questions per-se:

## Are you overthinking it?

That depends what is your definition of "ultra-precise" is and how good your design is without overthinking.

A simple calculation with numbers from the sensor and ADC tells us that $$\frac{1 kPa}{46mV} * \frac{2*5V}{2^{15}} \approx 2.3 \frac{Pa}{LSB}$$ your highest achievable theoretical precision is 2.3 Pascal per each bit of output. I assume that's way too accurate and we don't really need that.

Now we go and look at the noise from the sensor. Figure 1 shows that we have little less than 20mV peak-to-peak of noise, witch translates to about 0.4 kPa. Lets assume this is too much of an error for you and we need to remove it.

This is broadband noise that starts at 500 Hz and goes well beyond Nyquist threhold. From the plot at p. 19 of the ADC datasheet you can see that oversampling will not really help with this noise. But a simple RC filter will bring the noise down to several mV. Alas! You have a filter, just the wrong one. If you look at the application note you will the see the recommended values of the filter (650 Ohm, 0.33 uF). And since the ADC datasheet clearly states we do not need a buffer before it we can just use the simple RC filter you already got.

But here comes a problem. The sensors output is ratiometric. That is, it depends on the power supply voltage. (Take notice that all the reference voltages at the sensors' datasheet are given at a supply voltage of 5.1 V.) But the ADC has an internal, stable, reference voltage (that adds its own DC bias to your measurement). So now we go and look at your power.

The combined maximum current consumption of the sensor and ADC is $6 * 0.1 mA + 27 mA \approx 28 mA$ and under those condition up to about 60dB of input noise from DC to 10kHz is filtered. So we can assume that under normal conditions the power supply noise will be much less than 1mV.

## Do I really need ground separation?

At this point we can say that if you only need an accuracy of 0.5 kPa you can even remove the RC filters and not worry about a thing.

But if you need something better than this is the time to start thinking about things such as ground and power separation.

## Do I really...? Should I....? What about power...?

To answer all your other questions, lets assume you do need ground separation.

First of all, in your current design, your ground is not separated. By using a single tie point in the layout you might have avoided some nasty ground loops (that act as antenna and pick up whatever noise there is), but you could have achieved simpler (and usually better) results if you'd just flood fill the entire bottom side with ground.

In case of a flood fill with no islands and no narrow bridges everything is good. Also, if you must do a fill at the bottom layer it is usually better if it is the ground in case the insulation scrapes off and the conductor touches whatever is below it. Since there is usually some chassis, and chassis are usually at ground potential... you get the picture.

This is not always good since it creates a parasitic capacitance between the ground and other traces. Sometimes it can be used for good, sometimes its a problem.

This is actually why I personally never do less than 4 layers on projects where I can afford the extra cost, because in that case the inner layers become grounds and powers and there are almost no problems with ground loops.

Now, if you want to do a proper ground separation then you need to have a net with a name different to "GND" in your schematic. I usually use "DGND" and "AGND", other people call it other things. Then you find out what frequencies you want to filter so they won't reach the analog ground (this is usually the clock frequency of your digital stuff), you you build an RLC (not RC) filter and connect the grounds using the induction of the filter, not the capacitance.

For this to have any meaning each ground zone/area must have its own, filtered, power supply(LDO).

## Some remarks on the current design

To get the best layout look at the datasheets for both the ADC and the LDO. Towards the end they have layout recommendations with reasoning. It's really helpful to learn from that. Their layout solves many problems you might not even encounter but it, usually, will not create new one without someone warning you about it.

BTW, you're wasting half the range of your ADC because its bipolar and your design is not.

## Many designs ago, on a PCB far away...

If we assume that you do not need something extreme accuracy-wise, I would just take a Cypress PSoC5 developement board. It costs about \$10, and it has everything you need for this project on a single chip. Including a USB connection to the PC with drivers. Oh, and the multi-channel ADC project is just one of the existing demo projects for the CPU.

Am I over-answering this? Even if so I Hope I could help.

• Excellent, excellent answer. Many things here that I hadn't considered yet, and will end up incorporating in the final design! I'll likely redesign the PCB and post a followup to get some last bits of advice before having it fabricated. I know the AD7606-6 is overkill, but I'm using one in another project where I DO need bipolar inputs, and I happen to have about a dozen extra chips and software already written for them. Jun 15 '18 at 16:10
• If this is going to be in a lab and collecting data I would just buy some DAQ system, their range of USB and PCI should cover all your small lab needs (and PXI for the big labs). They have excellent hardware and software, used in many industrial projects. And their stuff just works. Unless your goal is to build something yourself. Aug 19 '18 at 0:39

I wanted to add this as a comment but fell short of reputations.

Seeing your layout, I noticed that the silkscreen markings of resistors, capacitors and diodes are over the pads. This will be trouble when you solder components. Usually a good PCB fabricator will observe this and remove overlapping portions of silk. But still, I suggest you edit footprint so that silk is not overlapping the pads.

• I'll certainly do that before I have it fabbed, I just wanted to get this question answered before I finished up the details. Jun 15 '18 at 16:09