Criticism on pcb routing and advice re pull up resistors

Does it look ok?
It’s an arduino shield for a motorcycle dyno.
Three inputs:

Ambient temperature - tmp36, analog pin 2.

Roller rpm pickup (“wheel” label) - 1gt101dc hall sensor, digital pin 2.

Ignition pickup (lightning label) - coax wrapped around ignition hv cable, shield grounded to pcb, digital pin 3.

All the 10k pull ups to keep the unused pins high for noise suppression - needed? Use internal pull ups instead?

my favorite part is that diode that connect the ground plane to the ground plane.

Lol, looks like fritzing screwed up the ground plane. Thanks, glad I decided to get more eyes on the design, I allways overlook something obvious and stupid.

Pullups, I would just go with the internal. Less traces hanging in the breeze to act as antennas.
Or, set them as outputs and write them high or low.
See these App notes also.

Atmel9108 Microcontroller in a Harsh Environment.pdf (139 KB)

atmel-AVR042-avr-hardware-design-considerations_application-note 7-2013.pdf (758 KB)

AtmelAVR4013 picoPower.pdf (92.4 KB)

It seems that’s not the only ground plane issue you’ve got.
Pins 2 and 3 of the bc547 are shorted to GND, 100k resistor too.

Yep, you’re right. And the 100pf cap. I’ve managed to somehow disconnect the trace between the cap and 100k to ++ . Too much coffee I guess.
Hopefully fixed now.

According to your parts overlay, the collector of the BC547 is connected to the ground plane, and the emitter is connected to the 555 trigger pin. (You need to flip the component overlay for that, or you'll end up fitting the transistor the wrong way around.)

Considering the off-board connections, I think I'd probably use more than just the single 0.1uF decoupling capacitor that's on pin 8 of the 555, too. It wouldn't hurt to add something a little more substantial across the power pins of the Hall-effect sensor, perhaps 1uF to 10uF. Not absolutely necessary, but I'd do it, to avoid potential problems. It would smoothe things out a bit over the whole board. I'd put an 0.1uF cap directly across the TMP36 power pins too, as recommended on the datasheet. You can't really have too much decoupling, (within reason), but it's very easy to have too little.

Just below 1N4148 there are 4 lines that can be made into one. As mentioned earlier, you do not need antennas. .

The "ignition" input is something of an unknown. If you get really good coupling to the ignition lead, you could easily get 1000V coming in there. The protection circuitry needs to be as close as possible to the input. Don't let it hop over other wires getting to your protection diode. If it wants to make problems then it can bypass your protection.

Think of your circuit like a medieval castle. It has layers of protection. Keep the unknowns outside the walls and control what comes through the gates. Then the inside of your castle can work without fear of being damaged.

Have you got a schematic to go with the PCB, so we can do a proper check.

Thanks, Tom… :slight_smile:

Thanks for all the advice!

  • fixed the bc547 orientation.
  • removed all the separate power trace “antennas”.
  • 100nf on the tmp36.
  • 1uf on the hall sensor.
  • moved the diode, cap and 100k close to the connection point, move the transistor to?

With more than the 100nf on the 555, do you mean more caps with different values in parallel?


adegnes: With more than the 100nf on the 555, do you mean more caps with different values in parallel?

I've read up on decoupling, and am pretty sure that's what you mean. Any advice on sizes and how many? 1uf electrolyte parallel with the 100nf ceramic? Maybe even a third bigger one?

Looks like you have room for: 10uf, 1uf and .1uf

I usually use one .1uf ceramic per VCC pin. As close to the pin as you can get.


What he ^ said. :)


adegnes: Better?

If you swapped the positions of the two 1K resistors over and used pins 6 and 7 on the Arduino, you'd have a lot less doglegs in the traces.

I'll throw in a 10uf to then. Using pin 6 and 7 would tidy it up a bit, but I need the interupts on pin 2 and 3, thanks for the advice anyway.

Great videos, thanks!

Should move the 555 to get more room.
100nf on the reset pin a good idea to?

Also, I’ve basically copied the design from this site

(Picture attached.)

but I’ve left out the part where the ignition signal enters the board on the top layer and is transmitted by capacitive coupling to the bottom layer. Instead I increased the cap value from 22 to 100pf(seemed logic, but what do I know).

SP1 ignition sense.gif

Heres a version with capacitive coupling of the ignition signal between the board layers before it enters the circuit.
I also moved stuff around a bit.
What do you think?