# Adequate decoupling / noise reduction for two accelerometers?

This is my first PCB, so please forgive some of my ignorance! I'd like to mount two accelerometers (ADXL193: +/- 250g), orthogonally, on the same PCB, and have a question about noise.

The current design is to have 5 strands of a ribbon cable soldered to the PCB, shown below: 5V, GND, X_OUT_1, NC, X_OUT_2. The "NC" is connected to GND on the DAQ board, but has no connection on the accel PCB, intended to reduce noise between the signal lines. They are single-ended, collected simultaneously.

• C1 and C2 are 0.1uF and 1uF ceramic capacitors, respectively, intended to decouple noise from the power supply.
• ribbon cables to these PCBs from the DAQ board will be up to 16 inches long, and could have ferrite cores along the ribbon cables

Questions:

• Should this combination of the ground plane/capacitors effectively reduce noise?
• If I want to use a radio on the DAQ, will it take a lot more decoupling?

I appreciate any help! I plan to make this design freely available after having it made and tested.

RECENT EDITS:

• swapped the power plane on the top of the board for a ground plane that's tied to the bottom
• added larger keepouts (top + bottom) around the drill holes for #4-40 socket cap screw head
• moved the self-test pins onto the 0.1" grid. unfortunately doing so removed 2 other labels from the board...

Images:

• If you are going to be hand soldering these, it will be less work if you increase the separation on the copper pour, and increase the length of the pads on the IC footprints. Since the package is a Leadless Chip Carrier the iron tip will not reach. If the pad is long enough then the solder will flow into the joint after a good amount of flux is added. – Phil Mar 28 '12 at 0:17
• You didn't ask but this is necessary (since as far as I can tell the output is voltage) - are you implementing an anti-aliasing filter on the DAQ-side or did you forget about it? It would make sense to put it on the DAQ side of the ribbon so you can change the sampling rate without changing the sensor board, but I just wanted to make sure you had considered it. – AngryEE Mar 28 '12 at 16:57
• @Phil I designed these with plans for reflow soldering, though I do have enough room on the PCB for them to be hand soldered. This would be a nice change for them to be more usable... Thanks for the idea! – Joel Mar 28 '12 at 19:46
• @AngryEE Thanks! I'm planning on a simple low-pass filter (series resistor + capacitor to ground) on the DAQ-side of the ribbon, before connecting to a designated ADC and then on to something like an Arduino Mega. – Joel Mar 28 '12 at 19:50

The datasheet describes device as very well noise immune one with ratiometric (to power supply) output from DC to 400Hz. So to read DC "ratio" well, try use 2+2+2=6 wire "drive" "sense" cable for 2 devices. At DC you are affected by ohmic, galvanic, thermoelectic forces, but not the radio.

-- Drive --->--*-----+----------------------------+
-- Sense ---<--/     |                            |
|                            |
-- Sense ---<----Device (of DC half bridge type),Device--->---Sense--
|                            |
-- Sense ---<--\     |                            |
-- Ground --<--*-----+----------------------------+


All 3 sense wires should meet ratiometric input of ADC, say top goes to positive reference input of ADC, middle into positive input, bottom sense goes into 2 pins: negative reference (of balanced input) and negative pin of input.

Edit: Other thought. If there is movement on flexible cable, think about "triboelectricity". If cable friction, hit, vibration is an issue, then read specs about correct impedance of load. If this is high impedance, then add differential "line drivers" with current loop output and match a type of ADC to be "current ADC". Or better add small ADCs on board itself.

Since the ADXL193 operates by tracks the plate motions using 400KHz excitation, it is sensitive to impulse noise at this fundamental and harmonic. Since DC-DC switchers often cross this range, you need to beware. AD suggests 50 ohm series +/or ferrite bead and Cap up 4.7uF A spectrum analyzer would be most useful to measure system noise and DC filter requirements. Otherwise, you need to make some assumptions on input noise and supression level. The chip would mix the V+ noise with the clock (400KHz) and pass thru intermod products within 400Hz LPF. Consider what noise output is tolerable in terms of g levels and mV and worst case V+ ripple and thus attenuation required.

.... they suggest 50ohm (47R) and 4.7uF and compute impedance of this cap and attenuation. Your design uses 0.1uF which is 4 ohms @ 400KHz so very little attenuation. even with line inductance. YOu should include R and/or Ferrite bead and caps...///.... I recall in the early days of Air Bag sensors (similar) that got false triggered by automotive battery chargers with high frequencer pulsers for lead acid rejuvenation in a ski resort. It was of suffient radiated levels to trigger Air Bag collision sensors in parking lots. (poof) So design layout for noise suppression with large ferrite beads, resitor and caps. THey can left out if the application is quiet.

• I considered the recommendations on the datasheet when I included the 0.1uF and 1.0uF caps, but decided against additional ferrite beads thinking (hoping) noise levels would be low. The first set of boards is coming this week... so as you suggested, I will need to measure the system noise and evaluate the setup. Thanks! – Joel Apr 11 '12 at 13:43