SparkFun Forums 

Where electronics enthusiasts find answers.

Questions relating to designing PCBs
By ajk48n
Hi everyone,

I'm designing an LED clock using an Arduino, 74HC595s for the control, and ULN2803s for grounding the LEDs.

I've got everything working on a breadboard, designed on a schematic and a first version laid out on a pcb in Eagle. I've never designed a pcb before, so I'm sure there's lots of little errors.

The main question I have is related to decoupling capacitors and a ground plane. I was having trouble finding out online if the capacitors should have their own pathway to the 74HC595s, or if they could both simply be connected to the ground plane.

I haven't put the ground plane in in this version, and any suggestions overall are much appreciated.

Thanks for any help

By Omgitskillah
Hi ajk48n,
I took a look at your PCB specifically to see what you did with the decoupling capacitors.
An easy to remember rule of thumb while laying down decoupling capacitors is to always put them as close as possible to the pin they feed power to. Then when laying the power trace, let the line go first into the capacitor then to the power pin. Therefore, you should remove the trace that seems to avoid the capacitor. The trace may render the capacitor useless.
The capacitors can share the same ground plain with everything else. Remember that all grounds should always be tied together.

All the best!
By InactiveUser001
Well done on your first attempt, some comments below:

For U2, U3 and the leftmost one - can the pads change to fingers/ovals like the ULH1 IC ? running tracks between them as round pads can lead to shorts, its far better to have a greater gap between the pads.

Whats with the loops for the vcc connection between C1 and pin16, C2, C3 ??

If the blue connections from S3 to R22, R26 to S1 are bought onto the red side you can flood more copper under there.
DItto from ULH pin 1, ULH2 pin 1, ULH3 pin 1, most of the LED connections. If your having a double sided board, you can get more copper groundplane on it by maximising the use of the top layer for tracks. (assuming this will be a manufactured board with plated holes).

Where you cannot get groundplane, make the gnd tracks thicker.

How are you going to mount this board? I see no mounting holes and tracks in the corners where they would go.

The top red track on R20 could jump over the blue track by moving R20 left a bit.

It's generally better to have all LED's oriented in the same direction, makes life easier when assembling and viewing from underneath. Its not as if the tracking would be harder.

Make the 5v track thicker.

you have some leds underneath the arduino board, are these all supposed to be fitted on the other side of the board?
I'm sure they could all fit in a nicer line or 2 rows up top.

Given the distance between the power pins of each IC pair, you may be better with a separate decoupling cap next to the top row of IC's vcc pin.

Silkscreen Ident: Identify the functions of the switches. add a name and version.

next to C2 is an arduino mounting hole, if you intend using these, move tracks well away from them - consider the fixings (screws/pillars etc.) you will use.

make sure that you run a DRC check before finishing.
make sure that you review the gerbers in gcprevue before sending them off.

I'm not sure on the board size but under 10cm square and you can get it made very cheaply.

If it was me,. I'd be putting all those leds in a long line with the resistors all vertical in a row, it looks like there is room for it (or at least an alternating dual row).

But keep it up, enjoy laying out a pcb - its a good skill to learn.