Schematic & Board review please..

Projects General Guidance
1

Hey gang-

I am attempting to whip up some minor PCB's to be fab'd, and would appreciate some reviews before sending them out.

It been roughly a year since I even worked in Eagle..(so definitely some ring rust)..

There are also some 'firsts' for me here.. as I have never worked with screw terminals before.. nor through holes parts before (everything I have ever done in the past has been all SMT stuff)

Summary of project.
This is really just a 'motherboard' type of PCB.. meaning that it (more or less) have some power regulation, a few passives, and some female headers for a NANO and a DFPlayer audio board to 'plug into'.

There will be screw terminals around the board to easily connect:
Battery source
Main power (latching) switch
Trigger button
Speaker
Neopixel Ring #1
Neopixel Ring #2

Similar to this Nano Screw terminal board: (but with voltage regulation and room for another audio board)

1000×810 154 KB

Questions:

SCREW TERMINALS:
I have never used screw terminal components before..
Is the 'double' line the 'front'? (where the user would insert the wires?)
I read that the square pad is normally to the 'left' side when facing you.. and is mostly used for the V+ (but that can be used as whatever in your design)

I believe I chose the SCREWTERMINAL-3.5MM part.. instead of the 5MM variant.... what is normally used when people add these to their projects? Is there a preferred size? (and why?)

VOLTAGE REGULATOR:
ROHM Semiconductor: BA50DD0T (Fixed, +5v/2A)

Datasheet:
https://www.mouser.com/datasheet/2/348/baxxdd0-e-208708.pdf

This is the chosen part for regulation... however reviewing the datasheet, I'm not sure how its supposed to be wired up? I 'think' the diagram I am supposed to follow only has a 22uF cap on the output? (thats it)..

I added another 22uF cap on the INPUT as well...... bad move? Overkill? Not needed? (Remove it?)

MAIN POWER TERMINAL:
One of the terminals is intended for a latching switch to be connected to it.. so it can toggle the main power the project.
I'm not sure if in the schematic that is the correct way to do this? I was really struggling on how to join the nets/lines in the schematic.. but not sure if that maters as long as its routed correctly in the board design??

You'll see in the board file I added some poly fills for ground planes.. but moved/chopped it away form the BATTERY TERMINAL... so the MAIN POWER TERMINAL will break/connect GROUND. Is that the proper way to add in a 'main power' switch? On the GND line? Or should it go on the VIN line? (or doesnt that matter?)

THROUGH HOLE PARTS:
I have never really used through hole parts.,. so when picking a capacitor... how do I know I have the right 'size' (footprint?) I mean the schematic symbol is fine/universal... but the board footprint/symbol is what I'm concerned about.

I used a NANO component for its footprint... but it also seems to have the ISP header broken out in the middle of the board.
Not great.. but that wont really be connected to anything in the end.. since the nano will be plugged into 2 female header rows..

Is this fine? Or should I replace with 2 female header rows?

I also added some extra pads to be able to tap some power sources (+3.3v, +5v, VIN..etc)
As well as another set of pads for battery connection. (noted on the schematic)

In order to NOT have an GOUND connection when the switch is off.. I made some odd shaped poly fill ground planes.. (I have only ever made full size ground planes before.. so not sure if this logic is sound.. of if this practice/approach is no good?)

I'm hoping there isnt too much wrong.. as I'd like to get these sent out today.. and start the process.

Schematic: (right click and view image to see it at full size)

1108×761 133 KB

Board:

430×725 160 KB

And EAGLE file(s): (.sch & .brd) for review in real-time:

http://dmstudios.net/misc/schematic_check/Rocketeer_motherboard_no-diode_AR.brd

http://dmstudios.net/misc/schematic_check/Rocketeer_motherboard_no-diode_AR.sch

Thanks for the eyes & the time guys!

2

Suggest you add:

  • series resistors in the data line going to the pixel rings.
  • 100nF Decoupling on Vin and several on 5v
  • decoupling at all power terminals.
  • difficult to tell if the GND is going where it should.
  • seems like the routing is weaving between the two layers more than needs to be.
  • maybe diode in the Vin line for reverse protection.
  • beef up the width on 5v traces.
  • vias bigger.
  • vias between GND plains.
  • thermo vias under regulator.
  • Nano pads could be bigger.
  • how about some mounting holes?
3

Nice suggestions..

Let me ask a few questions.. and add a few comments..

  • Series resistors for DI lines.. (good idea, I'll add them)
  • Some 100nF decoupling caps..at all pads & terminals (will do)
  • Beef up the width on 5v traces. - (How much bigger should the be? they are .5 width currently I believe!)
  • how about some mounting holes? - (another good idea!, I need to find out where/how these are to be mounted)

** difficult to tell if the GND is going where it should. - I'm sure what you mean here? (I also provided the .brd file if needed)

** vias bigger. - (why?.. I am compliant with the fab house design rules.. no errors. Is there another angle to understand here?)

** thermo vias under regulator... (can you expand on this? I have never added a 'thermo via' before? Where does one find this part? In Eagle?)

  • Nano pads could be bigger - (bigger than the default Nano EAGLE part?.. why?).. and should these be changed out the female header components I have there?

** maybe diode in the Vin line for reverse protection... I actually had one in there (you can still see the two conjunctions in the wires by the regulator).. but I removed it, because of the voltage drop. I am trying to allowed a wider range or battery sources to be used.. (roughly +6v - +7.4v packs).. if I add a diode.. +6 packs wont be an option any more....right? (I struggle with this.. as I always like to have reverse polarity protection)

The over all size of the board is only (roughly) 1.5in. x 3in.... do you still think all the decoupling is needed? I'll still be adding the cap to the Neopixel terminals as well as the resistor too.

Thanks for the time & eyes LarryD (appreciate it)

4

xl97:
Nice suggestions..

Let me ask a few questions.. and add a few comments..

  • Series resistors for DI lines.. (good idea, I'll add them)
  • Some 100nF decoupling caps..at all pads & terminals (will do)
  • Beef up the width on 5v traces. - (How much bigger should the be? they are .5 width currently I believe!)
    I like these to be big, 50mil is okay, 75mil is better.
  • how about some mounting holes? - (another good idea!, I need to find out where/how these are to be mounted)

** difficult to tell if the GND is going where it should. - I'm sure what you mean here? (I also provided the .brd file if needed)
I don't use Eagle.

** vias bigger. - (why?.. I am compliant with the fab house design rules.. no errors. Is there another angle to understand here?)
Bigger vias bigger holes, 50mils is reasonable 60 is better IMO.
Bigger holes, more copper from one side to the other.

** thermo vias under regulator... (can you expand on this? I have never added a 'thermo via' before? Where does one find this part? In Eagle?)
Same as a regular via ~60mil but you place a matrix under a component (ex TO220) to carry the heat from one side to the other side for heat dissipation.
Make these 'Tented' so you can fill with solder.

  • Nano pads could be bigger - (bigger than the default Nano EAGLE part?.. why?).. and should these be changed out the female header components I have there?
    If no trace are going between the pads, make the pads large for easier soldering. 80mil would be great, but what's reasonable :wink:

** maybe diode in the Vin line for reverse protection... I actually had one in there (you can still see the two conjunctions in the wires by the regulator).. but I removed it, because of the voltage drop. I am trying to allowed a wider range or battery sources to be used.. (roughly +6v - +7.4v packs).. if I add a diode.. +6 packs wont be an option any more....right? (I struggle with this.. as I always like to have reverse polarity protection)
The diode could be a Schottky, .2V.
Maybe put the option for having it there.

The over all size of the board is only (roughly) 1.5in. x 3in.... do you still think all the decoupling is needed?
Always always always use decoupling, if things are tight, use 1206 SMD .1uF.
Oh, I should have said ALWAYS.

I'll still be adding the cap to the Neopixel terminals as well as the resistor too.

Thanks for the time & eyes LarryD (appreciate it)