Help needed; Check of PCB and some other questions

[TvK]

Hi all, first post, don’t know if correct topic,
For these kinds of questions, I would have usually asked a professor of mine but Corona is a bummer and he is not able to respond, your help would be greatly appreciated. I am quite a novice in electronics design and finally mustered up the courage to ask these (probably) dumb questions.

I’m currently working on a sensor system for my bachelor’s degree project. It is basically a bunch of IR-LEDS and sensors in a beam-break configuration (similar PCB is other side of beam break) you'll find further explanation of my project and setup further down.
I have designed a PCB (View attachment PCB_SZ-001a.pdf) to eliminate wiring mistakes in my project but have a few
questions.
- Are the pcb traces of the sensor (BLUE) far enough apart (~1.1mm) to avoid interference/crosstalk from adjacent traces. (considering they are all V high and have very short V drops (drop < 1mS)
- Does anyone have experience with larger PCB’s (1050mm long) and what are the problems it brings with it.
- I assume the powerbank will put out a relative steady voltage and I this circuit does not overload by it. Is that too naïve? If so, what are the problems/solutions for it?
- Does anyone see anything very wrong with my circuit (crucial components missing, dumb wiring, etc)

Setup explanation of sensor system.
-5V Powerbank drives 11 LEDs, they blink at 56kHz (generated by a BJT (2N2222) circuit from an Arduino)
- LEDs are config. in 4 parallel strips (2L-3L-3L-3L) to optimize voltage and amp used (80 amps used)
-10 sensors are driven directly from a 5V Arduino pin, all parallel. They all have their own analog pin back to the arduino. (further away from PCB, pads connected to blue traces are connected to wires). The sensors are active high, when something drops through the IR-beam, the sensor does not see any light and drops in voltage.

I have included data sheets of LEDView attachment WP7113F3C-8988.pdfand SensorView attachment PCB_SZ-001a.pdf. I hope some of you sees a challenge in helping me and is willing to donate some time to improve my knowledge and help me with this project.

Regards,
TvK

 

[BradtheRad]

Your image is a long, thin pcb. Detail is visible by enlarging it.

Did you intend for your sensor data sheet to be a duplicate of your pcb?

Is each sensor supposed to detect light from a particular led a few feet away?
Are the led's narrow beam? Are the sensors narrow beam?

 

[TvK]

Appologies,
tssp40.pdf is sensor datasheet.
Indeed, each sensor is paired with a LED, 6ish feet away.
Sensor and LED are not narrow beam, however, the sensors are only able to see one LED through a small hole in the casing.
I tested this and it works.

 

[BradtheRad]

I can see why all led's and sensors must point 90 degrees from two flat PCB's facing each other.

The length of your narrow circuit board (1050 mm) converts to 3.44 feet. Do you intend to make it yourself? Or have it made by a service?
It's a risk because something that long & thin can break in transport.
The board is able to bend in one direction but only so far. And it cannot bend in every direction which force can be applied.

Did you consider making a number of short module boards... even though it causes increased work in setup and connecting?
You could mount them on a long wooden plank. Anyway even if you have everything on one long board, it's a good idea to fasten it to a long plank.

 

[TvK]

I will bend te sensors so they line up with the leds and face the same direction.

I plan to have the PCB made by a service, it breaking in transport is a valid point, i will look into that.
thought about making modules but was worried more connectors might mess up the PMW signal or te sensor signal, is dat valid or injust?

Should i be worried about crosstalk or the length of the traces?

Fastening it to a plank was indeed my idea, als to keep it stable.

Thanks for all your help so far!

 

[FvM]

To assess cross talk and voltage drop, we need to refer to the presently unknown circuit to estimate voltages, currents and net suceptibility.

Maximum PCB length is in the range of 500 to 600 mm for most manufacturers. I would strongly suggest to divide the board.

 

[TvK]

LED driver: 5V - 80 mA (4 parallel series: I supply per series: 20mA) on PCB this is 'powerb.'
Sensor driver: 5V - 7mA (10 parallel units: I supply per Unit: 0.7mA)
Sensor output (High): 5V - 0.5mA (not sure, could not find on datasheet) (these are the BLUE wires on SZ-001a.pdf)
Sensor output (Low): 100mV - 0.5mA (this is expected for around 0.7ms)

I dont know anything of net suceptibility, where can i calculate/find this?

 

[BradtheRad]

Should i be worried about crosstalk or the length of the traces?

It sounds as though you have 50kHz pulses running through tracks separated by 1 mm, for a few feet of length. There is a certain amount of inductance between the tracks. Have you tested that it works?

Another issue is that the sensor wires appear unshielded. They're exposed to unknown electrical noise (including ambient 60 cycle hum). This can create false readings, unless you include precautions such as shielding, filtering, pull-up resistors or diodes, etc.

 

[FvM]

Most sensitive net is open drain sensor output with 30 k internal pull-up. Should possibly use additional external pull-up.

Power traces are unnecessarily small, also why not use a continuous or hatched ground plane for the sensors? It could also effectively shield the sensor output nets.

 

[KlausST]

Hi,

I agree FvM. A GND plane shold give some benefit.
Maybe add some capacitors for supply voltage stabilisation.
And maybe add GROUNDed tracks between the signal lines to suppress capacitive coupling. Use a via every couple of centimeter to the GND plane.
I´d also use wider tracks. I see no need for them to be that narrow.


Klaus

 

[TvK]

It sounds as though you have 50kHz pulses running through tracks separated by 1 mm, for a few feet of length. There is a certain amount of inductance between the tracks. Have you tested that it works?

The 56kHz signal drives the LEDS, these traces are seperated by at least 2.5mm. The sensorOUT wires are seperated by 1mm (5V, low amp).
I could not test anything because i did not order the pcb. I wanted to ask these questions before spending a lot of money which i dont really have. I did however build a small setup as a proof of concept with 2 LEDS and 2 Sensors. It all worked perfectly.

This can create false readings, unless you include precautions such as shielding, filtering, pull-up resistors or diodes, etc.

I have already implemented a filter at the Arduino side of the sensor read-out. Is that wat you mean or am i missing a point?

- - - Updated - - -

Awesome, will look into placing a GND plane (hatched i think, with my minimal research so far).

Will try to figure out the capacitors, however, supply voltage is already regulated from the source. (Again am i missing your point?)

GND tracks between SensorOUT wires: does the spacing between these wires need to be larger then or can i just drop them in between the sensorOUT wires as i spaced them now? (1mm gap)

Ill increase the size of the power trace, what mm2 should i think about?

Thank you all for helping, you're teaching me more atm than my professors ever could.

 

[KlausST]

Hi,

Will try to figure out the capacitors, however, supply voltage is already regulated from the source. (Again am i missing your point?)

your traces on your PCB will introduce some resistance (mainly depend on width, length and thickness) and impedance (almost independent of thickness and width)..
Thus - even if the power supply gives a clean ouput - it may be noisy at the end of the traces. You may compensate this a lot by installing capacitors close at the load.
Maybe 100nF ceramics. You are free to increase the value.

GND tracks between SensorOUT wires: does the spacing between these wires need to be larger then or can i just drop them in between the sensorOUT wires as i spaced them now? (1mm gap)

1mm will be is sufficient.

Ill increase the size of the power trace, what mm2 should i think about?

For those with higher current you may calculate the voltage drop.
For those with lower current I see no need to go below 0.6mm... but technically and for the signals even 0.2mm should work. Maybe the thicker traces give some benfit with mechanical force. (when bending the long PCBs)

Klaus

 

[BradtheRad]

I have already implemented a filter at the Arduino side of the sensor read-out. Is that wat you mean or am i missing a point?

Then what you installed may be sufficient. The source of noise isn't much different from the buzzing that comes through an amplifier when the microphone lacks a ground connection. Inside is a high-impedance wire acting like an antenna.

Looking at your sensor data sheet, there's a schematic showing a 33k resistor between the sensor and supply rail. In that sense it's a pull-up resistor. Probably it can do the job of preventing noise and interference on the signal wire.

 

[TvK]

Hi all,
Thanks for all the help. These are my further actions:
- I'll increase the size of the power traces
- Add GND plane and wires between sensor wires
- Include connectors for capacitors. When the PCB arrrives, ill measure the power at the end of the traces and then decide wether the capacitors are needed.

Probably it can do the job of preventing noise and interference on the signal wire.

Just to be sure, if this statement eliminates one of my 'further actions', could you let me know?

Finally, i will split the boards. Turns out, the service which said they could manufacture my boards, cant do it. i'll make 3 smaller board and connect them on a plank.

If you're reminded of something i probably forgot or that could be of use to me or projects like these, please let me know.
I hope to remember to post the outcome of this project

 

[wwfeldman]

in post #4 BradtheRad suggested making modules of the sensors so the PWB in not so long and narrow

i agree
you can connect the modules with twisted pair wire, which will significantly reduce the crosstalk and interference issues.
it will also make it easier to align transmitters with receivers, since you'll be able to adjust one pair at a time
without effecting the alignment of any other pair.

put about 10 cm of service loop in the connecting cables to ease positioning and alignment.