Thanks for the link to an easily readable data sheet.
A high on pin 3 overrides the output generated by pin 4, so to Gnd. pin 4 the OP needs to alter his PCB so pad 3 is connected to Vcc instead of Gnd.
Because pin 3 is Gnd instead of Vcc
Mouser and Digikey are good sources for datasheets of elements they have. I used alldatasheet only few times to find datasheet of inaccessible (old) elements.
You are wrong. Check it once more.
Pin 3 set to VCC enables the driver but OP needs to have driver disabled so pin 3 should be connected to GND as he did it.
Since 90s we use (in most of our products) ICs that are MAX485 functional equivalents (+ some extra features we need).
Do you know what the difference between a bypass cap and a decoupling cap is, and do I need both?
My take is that is two different words for essentially the same thing. Don’t worry about that! 
What do you mean by stiffer ground connection? Currently, I have a 0.75mm clearance, I didn’t want to make the clearance too small.
I just had a look at the board I am working on. My clearance is 0.5 mm and that is quite large=conservative for low voltages (voltages under 24V for example). I do not know much about your design, but the large clearance means that the rows of pins for a DIP cause a slit in the ground. In a very critical design this would reduce the effectiveness of your ground plane.
I like big clearance, but even 0.35 mm should not be a problem to work with for low voltages.
I cannot be certain, but I suspect that because your board is mostly through hole (not SMT) that the ICs are older and none of the signals or switching is VERY fast. FWIW any time a forum member is doing a new design and buying the components, I strongly recommend going with surface mount. It is not difficult (and is easier in some ways) so long as you are not using tiny lead pitch devices such as 0.5 mm or smaller. Of course if you have the through hole parts already, you might as well use them. I do that also.
Anyway I think it is unlikely that those slits I observe and mention above are likely to cause problems. That would seem like a more critical design than most of what I think is discussed on this forum.
I’m using 5V and 15V in my board. And I’m using THT because I’ve never hand soldered SMT before, I also have all the components already. I’ll probably reduce the clearance to 0.4 or 0.5mm
See this one:
#11/36
Older ICs but manufactured recently can be much faster than maximum times specified in their datasheets simply because competition forces cheaper production (die shrinking).
We ran into this problem 15 years ago when some our device designed in 90s refused to work when made with recently bought (the same type and manufacturer) serial EEPROM.
Since many years I have to use 0.2mm for whole PCB. As there are some places at PCB with 0.2mm clearance than for zones I use little bigger - 0.25mm. In designs I made this year I had to use 0.18mm whole PCB clearance. It is because of 0.4mm raster QFN element. Datasheets specifies 0.22m pads so distance between them is 0.18mm.
Around 1990 I switched from THT to THT at top and 1206 R and C at bottom and few years later to all SMD with 0805 as typical size and shortly to 0603. 25 years later 0603 is all the time the basic size for me. There is not problem with soldering them.
I have no argument with that for professional boards. Mainly I am discussing boards that I assemble by hand in my home lab. Before starting with KiCad I did many boards with ExpressPCB, and many of those had no solder mask.
I was sort of a chief engineer at a power supply manufacturer during 1981-1998. I was responsible for the first boards that used SMT, and yes I had us start with 1206’s and SOT23’s. The board assembly replaced a previous design which used 1/8 Watt leaded resistors all standing on end. But these days I am completely comfortable soldering 0603s; I use a somewhat small 0805 footprint for those 0603s.
0805_Top_Small.kicad_mod (1.5 KB)
Great effort!
I’ve designed an Arduino 328 for a project. The only issue I had that really had me scratching my head was the reset circuit. I ended up using the exact design Arduino use and no more troubles after that.
You don’t look like you are using the UART for uploading code…which is fine as I’m guessing you’ll preprogram the Atmega.
I would stress too much about the decoupling caps. I use 100nF for them if I think it’s going to be an issue.
If a ground current has to flow from somwhere left of your controller to somewhere right of it, it now must flow around it. If there ground fill was connected between the pins it could flow straight under it. That would give smaller loop area and thus lower EMI.
2 Likes
On a double sided board, I would always use a copper fill on the front. In most cases a copper fill for +5V on the bottom. Vias don’t cost extra, so you can stich a plane back together when it got separated.
For your first board, the routing and parts placement look very good!
Nick
I appreciate everyone’s feedback so far! This is the LED array I plan on using. It consists of 57 WS2812E-V5 LEDs. There is a ground pour on the back and I am using vias to connect the ground of each LED to the ground layer. If I could get some feedback that’d be great.
LED_v5 Schematic.pdf (193.0 KB)
I have never designed anything like that so I’m not sure about what I am saying.
As it is digital transmission between LEDs shouldn’t there be some capacitors?
I don’t know the current. May be it would be better to have 5V fill zone at top to reduce voltage drop at tracks.
I know that for a lot of these types of LEDs, capacitors are typically used. The datasheet for this LED is in a different language, but there’s a schematic and it doesn’t show capacitors.
WS2812E-V5.pdf (779.7 KB)
I found a datasheet in English for WS2812B-V5 which seems to be similar to what I’m using (WS2812E-V5), and the datasheet says
“The peripheral circuit don’t need to add filter capacitor”
WS2812B-V5_V1.0_EN.pdf (640.2 KB)
I could be wrong, but it seems that for these LEDs, you don’t need capacitors. They may already be built in, I’m not too sure.
The max current draw is going to be about 2A. Having a 5V fill on top wouldn’t be a bad idea, I may add that.
Yes, sounds like a good idea and could also help with heat dissipation. Or at least some more direct connections like between D37 and D38 or between D7 and D18 would be probably good. The current goes a really roundabout way otherwise. But adding a fill is probably the simplest solution.
I would move the crystal and associated caps closer to the CPU. You might also consider a guard ring around the crystal and caps. Here is one reference.
Regarding your original design, I wouldn’t put electrolytic capacitors on the underside of the board. I don’t know how you intent to store or mount the boards, but it looks really awkward. For simple decoupling, I’d probably use small ceramic smd capacitors instead, which also have a lower ESR. If you really need large capacitance, there’s enough free space at the top side of the board.
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.