Board and schematic review (ATTiny85)

[PCBAlex]

Hi, I was hoping to get some feedback with a board I am designing. Its basic function is to control a 9g rc servo motor when it detects a change in the photointerupter. It has two modes of operation controlled by a switch. The brain box of this guy is the ATTiny85. There is a ground pour only on the top side of the board.

View attachment PAO Rev2.pdf

Here is what I need help with:

1) I tried to add ESD protection to the external pins based on what information I could find online but I am not sure I am properly implementing things.
2) Have I added too many or too few Bulk capacitors and are their values appropriate?
3) Any tips to improve the board layout or routing?
4) Any other tips, comment, or resources in general you can provide would be appreciated.

Please keep in mind you are talking to someone who has no electrical engineering background. I am a caveman trying to learn how to get into a new hobby.

Thanks in advance

 

[BigBoss]

-You schematic is not standard, everything seems up side down..
-PCB is not appropriate for high current application.Don't hesitate to use larger tracks ( or copper pour is better)
-Protect MOS against overshoots at Gate ( a series resistor) and Drain-Source ( A fast parallel and reverse tied diode )
-Decoupling capacitors are always tied to Loads or Sources.
-A diode pair that is reverse connected to GND and VDD will protect your uC against ESD.( if you meant to say)

 

[KlausST]

Hi,

Currently you have the GND plane on the component side. This cuts the GND plane into pieces.
I'd move the GND plane to the bottom side and move as many as possible bottom traces to the top side.

Klaus

 

[Relayer]

Hello PCBAlex,
Is your circuit intended to see some reasonable current passing through the MOSFET?
If so, you need to widen any tracks associated with the Source and Drain of the device.
Pin 3 of JP2 to the Drain, and from the Source to R3 and ground. And from the junction
of the Source and R3 to N$17.
Regards,
Relayer

 

[BigBoss]

Draw you schematic in comprehensive manner and use that configuration for high current carrier tracks.
This is an example only and you should adapt it into your requirements.Because TO-220 is a large and heavy package and if the tracks are poorly tied, it may ***** the connections.
Consider the currents and voltages too..

 

[PCB Designers]

Hi, I was hoping to get some feedback with a board I am designing. Its basic function is to control a 9g rc servo motor when it detects a change in the photointerupter. It has two modes of operation controlled by a switch. The brain box of this guy is the ATTiny85. There is a ground pour only on the top side of the board.

View attachment 141115

Here is what I need help with:

1) I tried to add ESD protection to the external pins based on what information I could find online but I am not sure I am properly implementing things.
2) Have I added too many or too few Bulk capacitors and are their values appropriate?
3) Any tips to improve the board layout or routing?
4) Any other tips, comment, or resources in general you can provide would be appreciated.

Please keep in mind you are talking to someone who has no electrical engineering background. I am a caveman trying to learn how to get into a new hobby.

Thanks in advance

Have you done with your SCH and LAYOUT ?

I can help you, please don't consider it a paid job.

Regards,
Maqbool

 

[BrunoARG]

Hi Alex,

First of all, it's a good practice (and pretty necessary) to have a topology standard to draw schematics circuits, and it does exist:

-Higher potentials up, lower, down. Just like the water falls, from top to bottom. You put all GND in the upper part of each circuit section, it should be down, as it's the common 0V, the lower voltage you have in the PCB. Negative potentials (voltages) should go beyond GNDs.

-Input left, outputs right. Just like reading, the inputs (audio jacks, control signals connectors, sensors, etc) should go at the very left, and the outputs (motors, LEDS, speakers, relays, lamps, etc) at right.

It's much more easier to understand what kind of use has each part of the circuit with that topology.

-Put "legible" names to the important nets of the circuits: not N$12. You (and whoever that will read the circuit) should understand what important signals are in the circuit and where they are. For example, "Audio_input_stereo" and "Power_audio_output" should help to understand a circuit.

A quick rule: Read the circuit and imagine: "Will I still understand this circuit after 1 year now?" If the answer is no, then you should make some more annotations and corrections.


And the tracks width become important at high currents, they do have resistance and a poor power dissipation, and trust me they will blow up (even being capable to damage other parts of the circuit as the copper litteraly separate from the board). There are easy to use charts that tells you what is the minimum width you can use at X current, not even a calculation is required.

 

[KlausST]

Hi,

-Input left, outputs right. Just like reading,

I agree with: Inputs left, outputs right

But mind that different countries use different reading direction....

And I agree with the rest of the post.

Klaus

 

[Mattylad]

All the above.

Schematic:
If something goes down to ground then it should show it goes "down" to ground. Up to supply etc.
Try to get your labels (component name, value etc.) all reading left to right so the reader does not have to look sideways etc.
Also get them the same size, CR1+CR2 are huge compared to others.

Rotate J1 90 to the right.
Also rotate VR1 so the labels are readable left-right, in fact the whole symbol would be better if the IN was on the left edge, the OUT on the right edge and GND on the bottom edge.
And connect the +12vs so that J1 feeds into VR1, there is no point having the 12v, add a text label if you want to identify the voltage.
MOS1 is a different scale to the other symbols, consider making it smaller.

The LED's, if you have a line through them you can rotate them 180 and not realize it, diodes are best with no lines through them.
R9 has 22 inside the symbol.

But heck, good try - its still readable.

The PCB:
C3 should be right next to the input pin of the regulator with thicker tracks.
C4 by the output pin (I cannot even find C4???)
You have no protection on your input, no reverse polarity diode nor fusing?
What is "power" ?

C5 & C6 +pins connect to R3 and SS2 Mode pins (+5v). On your schematic this is not the same net for IC1 pin 6 to C6 (not shown as electrolytic) and R8? Thier placement is nowhere near where they should be (wherever that is - but its not where they are now).

Either your labels are not next to the components they belong to, or you have some serious misplacement issues, take CR1 for instance, its next to P1? (is that JP1) yet the schematic shows it as connected to JP2.
I'm going to stop here as it clearly does not match the schematic for me - you need to ensure that it does.

What software are you using?
Either way, welcome into the hobby, please dont take this as bad criticism but helpful criticism (is that actually a thing?).
Enjoy the hobby, learn more, do more, enjoy it more. (Beer helps).