Go Down

Topic: Arduino compatible board for energy monitoring (Read 1 time) previous topic - next topic

Bouha

Hey everyone,
This project is based on the Open Energy Monitor designs (http://openenergymonitor.org/). It is an ATMega with Uno bootloader, an RFM12B radio module, a space for a WIZ820IO (Wiznet W5200 ethernet chip) + jacks for four clamps current sensors and one AC AC voltage adapter.
Power supply is on the board (same AC AC voltage sensor)

This is my first PCB with a microcontroller on board so I am a little nervous to send it to be fabbed (especially that it's all SMD).

Would be great if you could have a look at my schematics and board files and give me some feedback.
Thanks
www.optimalabs.de

CrossRoads

I don't see any decoupling caps(100nF) on the power pins for the various devices.

I see a diode on the FTDI power interface - if someone plugs in a 5V USB/Serial adapter, that will put 4.3V on the VCC line, could be a problem with the rest of the board appearing to run at 3.3v based on the power header.  Most 3.3V devices only want 3.6 to 3.8V Absolute max.

Standard anymore is a diode across the reset pullup resistor to dissipate any spikes to the Vcc pin and  not put the uC into high voltage reset state.
I've posted the Atmel Application Note on that a few times.

Your ICSP header is in a non-standard location. Could be a problem for some shields.

Rx & Tx need to be swapped on the FTDI header.

What is the Aref solder jumper for?

Are there top & bottom layer ground planes? Hard to tell from the drawing.

Move the signal names away from IC3, can't read what they are.

Overall, I'd  say Good start.
Designing & building electrical circuits for over 25 years.  Screw Shield for Mega/Due/Uno,  Bobuino with ATMega1284P, & other '328P & '1284P creations & offerings at  my website.

Bouha

Thanks for your quick and helpful comments Crossroads :)

Quote
I don't see any decoupling caps(100nF) on the power pins for the various devices.


I didn't know about this practice, could you please tell me more about it? or suggest reading? and I just put it on the Vin pin of a device? or between VCC and GND?

Quote
I see a diode on the FTDI power interface - if someone plugs in a 5V USB/Serial adapter, that will put 4.3V on the VCC line, could be a problem with the rest of the board appearing to run at 3.3v based on the power header.  Most 3.3V devices only want 3.6 to 3.8V Absolute max.


You are right, those 4.3V go to the Regulator Vin. Was that wrong?

Quote
Standard anymore is a diode across the reset pullup resistor to dissipate any spikes to the Vcc pin and  not put the uC into high voltage reset state.
I've posted the Atmel Application Note on that a few times.


I'll do that.

Quote
Your ICSP header is in a non-standard location. Could be a problem for some shields.


You're right, but I'm afraid I can't put it where it should, at least in this design.

Quote
Rx & Tx need to be swapped on the FTDI header.


I'm a little confused here: I thought the FTDI's RX goes to arduino TX and vice versa. Is it wrong?

Quote
What is the Aref solder jumper for?


I was not sure if I must set my AnalogReference to external and connect it to VCC so I offered myself that possibility later.

Quote
Are there top & bottom layer ground planes? Hard to tell from the drawing.


Bottom plane is, but not the top. Do you advise to create a GND polygon on the top too?

Quote
Move the signal names away from IC3, can't read what they are.


Will do, sorry :D

Quote
Overall, I'd  say Good start.


Thank you sir ;)
www.optimalabs.de

pito

75ohm resistors with the LEDs? What are the LEDs intendeded for? Are those the laser diodes driving a 150km long fiber optics? :)

Bouha

Wrong values of course :D

I just copy pasted the closest resistor that had the same size.
www.optimalabs.de

CrossRoads

Quote

I don't see any decoupling caps(100nF) on the power pins for the various devices.

I didn't know about this practice, could you please tell me more about it? or suggest reading? and I just put it on the Vin pin of a device? or between VCC and GND?

Not sure where I'd find something. Best way I can describe is the 0.1uF provide local pockets of energy for each chip as they switch internally so they are not starved for power. Go from the power pin on each device (Vcc, Vdd +5, 3.3, whatever it is called) to Gnd.


Quote

I see a diode on the FTDI power interface - if someone plugs in a 5V USB/Serial adapter, that will put 4.3V on the VCC line, could be a problem with the rest of the board appearing to run at 3.3v based on the power header.  Most 3.3V devices only want 3.6 to 3.8V Absolute max.

You are right, those 4.3V go to the Regulator Vin. Was that wrong?

That would be fine - can't tell from your schematic as it is not labelled. There are many unlabelled signals, having names on everything really helps in analyzing.

Quote

Rx & Tx need to be swapped on the FTDI header.

I'm a little confused here: I thought the FTDI's RX goes to arduino TX and vice versa. Is it wrong?

No, I was confused by names that look like RXI_TX and TXO_RX.
If the actual signal names are RX and TX, then you are fine.
CTS needs to connect to GND, that's an input to the FTDI chip, Clear To Send.

Quote

What is the Aref solder jumper for?

I was not sure if I must set my AnalogReference to external and connect it to VCC so I offered myself that possibility later.

Ok, so just pads then? Or connected to something? Signal names again.

Quote

Are there top & bottom layer ground planes? Hard to tell from the drawing.

Bottom plane is, but not the top. Do you advise to create a GND polygon on the top too?

Yes I do. Add some vias and Name them GND to connect the two layers.
Be sure to Name the layers GND as well.
Designing & building electrical circuits for over 25 years.  Screw Shield for Mega/Due/Uno,  Bobuino with ATMega1284P, & other '328P & '1284P creations & offerings at  my website.

pito

#6
Aug 12, 2012, 11:11 am Last Edit: Aug 12, 2012, 01:41 pm by pito Reason: 1
..decoupling capacitors - as crossroads said - good electronics practise tells you each active component (where you do fast switching, or you handle larger currents/voltages, or the circuits with high amplification, or high frequency circuits...) shall get its own decoupling capacitor. The reason is the wires coming to the component have some resistance/impedance, so they create a "dynamic drops" in voltage while the component works (you can see that on a fast oscilloscope). Moreover, when several active components are located on the same wire, these voltage/current drops are passed to all other components hanging on that wire, thus the "noise" from one component is passed to all other components via their power railes and grounding loops - we say the devices are coupled then - and you need to decouple them in order they work properly. To eliminate these drops, the decoupling capacitors are used (as the current reservoirs - the same principle as the water dams). For best performance however, the capacitor values and types have to be chosen carefuly, and also the point of their connection is important - but basicaly, the capacitor has to be connected as close as possible to the particular device with as short as possible wires (a few mm).
For further reading - google ie. "analog devices decoupling" :)

Go Up