Minimal Arduino Eagle PCB

For my second attempt at an Eagle PCB design I am doing my version of a minimal Arduino, a miniscuino :smiley: I will be accessing the IO pins via the two 14 pin headers running down either side of the 328 and using a two pin screw connector for the 9 volt power connection. The FTDI connection will just be via the VIN and GND pins of the LH header and the reset, TX and RX pins when required. I was not sure about providing a heat sink facility for the LM7805. I am just wondering if anyone can see any problems with my proposed circuit and layout.
Thanks Pedro.

Standalone Arduino Copy2.brd (84.3 KB)

Standalone Arduino Copy2.sch (321 KB)

Saw this a couple days ago, forgot to comment: 1. Add 0.1uF cap from Aref to Gnd. 2. Move Crystal & 22pF caps closer to the chip. 3. Reverse polarity diode? May save your butt sometime. Can leave off, but put pads in for it. 4. Connect open header pins to something; +5, Gnd? 5. Electrolytic caps for the regulator, vs ceramic disc 6. Lay the regulator down so you can bolt it to the board for cooling. 7. Reset (DTR) cap connects to wrong side of reset resistor to do anything. 8. Extra set of pads for +9, Gnd in case you want to break out for another device.

Thanks CR. Yes I was looking at what I had posted here last night and saw that I had used ceramic caps in the schematic but had full intentions of using Electrolytic caps (honest :) ) but thanks for pointing that out Also I saw on a YouTube video series RPC Electronics has a good Eagle intro ) and in it he used a 7805 device that that lay it down against the board so thanks again I will modify that too. Nice pickup on the incorrectly placed cap on the reset resistor and cap between AREF and Gnd. I assume that moving the crystal / caps closer is because the caps should always be as close to the chip as possible? Connecting the open header pins to 5v / Gnd presumably is just a case of they may as well be used for something that could come in handy and the same thing with extra pins for the 9 volts in? I suppose the diode just goes on the 9V in to the 7805? I will amend the files and repost them. At least with me making some mistakes I get to learn how to update the board from the schematic etc so it’s all good. Thanks again for the use of your Eagle eye, Pedro.

I reworked my PCB and incorporated the suggested improvements along with fixing my cock ups. I did not add an additional 9 volt access point seeing as the present one is a screw terminal type which can be easily tapped into if required. Just wondering how it looks now,
thanks Pedro.

Conn Edit Standalone Arduino Copy2.brd (99.1 KB)

Conn Edit Standalone Arduino Copy2.sch (756 KB)

I would add a 1N4148 diode in parallal with the resistor (cathode to +5V), to prevent the reset pin going above 5V and putting the chip in programming mode. This diode was added in the Uno R3.

Whether you want ceramic or electrolytic caps on the 5V regulator depends on the regulator. Check its datasheet for the recommended values and types.

I would NOT lay the 7805 down, instead I would place it upright and with its flange side in line with one edge of the board, so that you can attach a heatsink if necessary. Bolting the regulatior to the PCB will have very little cooling effect unless you have a large area of copper under and around the regulator.

EDIT: also, I suggest you rework your PCB design to use a ground plane. If you want to lay the 7805 down, then put the ground plane on the top side of the board, then it can also help cool the 7805. Or have the main ground plain on the underside, and a smaller one on the top side around the 7805.

Thank you for your suggestions dc42

He already had the ground planes DC42.
Pedro, swap the position of the 22pf caps - don’t have the crystal to cap lines crossed.

Your whole 9V connector/diode/caps layout arrangement is kind of awkward, that could be done better. Rotate the connector 180 degrees, move the diode up, move the caps to the right.
On the schematic, Edit:Net Classes. Make the default trace width at least 10 mil, drill 12 mil, clearance 10 mil. Power trace, 15 is okay, I would go wider, like 24, drill 26, clearance 10 mil.

I agree with reset diode in parallel with reset resistor - anode to reset pin, cathode to +5.
Add a power on LED? From +5. You have room.

So without adding the parts, you could have something like this, easily a single sided board also if you wanted, as seen with the ground planes turned off.

Conn Edit Standalone Arduino Copy2.brd (97.5 KB)

Conn Edit Standalone Arduino Copy2.sch (756 KB)

Thanks that looks really good CR.

When I look at mine compared to yours it's like comparing a bowl of spaghetti to a few well placed pieces of fine Italian fettuccine :D That being said, I am learning so much from the Crossroads School of Electronic Design. I thank you yet again,

Pedro.

That's where experience & practice come into play. It gets easier the more you do it.

I did not like to ignore your and dc42’s suggestion regarding the diode on the reset line and also the power LED so this is what I came up with. I am just wondering does it look anything like fettuccine or just a can of Campbell’s spaghetti

Crossroads Edit1 Standalone Arduino.sch (838 KB)

Crossroads Edit1 Standalone Arduino.brd (107 KB)

Parts look good.
You do not need to put in ground traces - the ground planes take of those connections.
If you move the ground plane layers to just outside of the board dimensions, and “ripup” them so they show like this picture, the next step would be click "ratsnest"button (Tools:Ratsnest), then the ground connections would all get made on the layers, and a + appears across the pad so you can see its connected.

I have been trying to move the ground plane just outside the dimension border but the dotted lines keep getting deformed. I tried highlighting them and moving them outwards by "grabbing " them in the centre but I am obviously not doing it correctly. Also I keep somehow selecting the dimension layer instead of the dotted ground plane line. Tearing my hair out doesn't seem to be helping.

Delete the ground polygon & re-add it, is simpler sometimes.

I deleted the ground planes and re did them outside the dimension layer but when I try to rip them up nothing seems to happen. At one stage I did briefly see a message down in the bottom left corner that think said “calculate short test airwires” but before I knew it was gone. You have got to be quick sometimes.

EDIT - In frustration I manually ripped up all the ground traces then hit ratsnest and this is what I have now. How did I go. It seems to be the same as your photo after you did it ‘properly’ I live in hope :smiley:
If miraculously I have managed to get this ground trace problem sorted out, how do I prevent it happening again. Is it a matter of initially drawing the ground polygons outside the dimension layer before hitting ratsnest because I really do not want to have to go through that again :smiley:

Crossroads Edit1 Standalone Arduino.brd (104 KB)

Crossroads Edit1 Standalone Arduino.sch (838 KB)

CrossRoads: He already had the ground planes DC42.

I don't see any ground planes in the board layout I downloaded (the one attached to reply #3).

The dashed line around the board edge is the polygon(s) that are the ground plane. Clicking Ratsnest would make the layers visible, but makes the signal traces a little harder to see. I draw the polygons just outside of the board edge so they can be ripped up to make the traces easier to see. Having them right on the dimension line makes them difficult to manipulate.

"initially drawing the ground polygons outside the dimension layer before hitting ratsnest" Exactly. I don't manually route much stuff, I tihnk Eagle does a pretty good job. After it's done, I'll do some cleanup, make sure there are no really long traces with odd routing, sometimes do a little tweaking to get all the ground pins connected, and to fix right angle corners.

That's great CR.

So just to clarify, the last version that I posted appears to be all OK and doesn't require any further tweaking if I decide to get some boards made in the near future?

Thanks Pedro.

I believe so.

I have one small suggestion regarding the board layout you attached to reply #13. The trace between the regulator output and the microcontroller Vcc and AVcc pins could be routed underneath the chip. Then it can be on the blue side of the board like most of the other traces, and it won't disrupt the main ground plane that I believe you have on the red side.

In fact, with a little extra effort, all the remaining red traces could be rerouted on the blue side, giving you an unbroken ground plane (unbroken by traces that is).

The silk screen for one of the resistors doesn't line up with the resistor itself.

CrossRoads:
I believe so.

Excellent 8) Thanks so much and have a good day

Thanks dc42 I will have a look at that.