It basically looks OK. One thing is the No Vector Font errors on that “Scaru” text. Text in the signal layers needs to be in a vector font. Select the text and change the type to VECTOR. Also, there are two SCARUS on top of each other on the blue layer. Delete one of them. Or put the text on the silk screens, not in etch.
Seeds design rule file says 12 mil min drill size, their web site says .3mm (11.8 mil). That’s causing the drill size errors.
Other than those, it looks like it might fly. The clearance and overlap errors seem to be due to the drilling into polygons, etc.
Not bad for a first run with Eagle. It’s been a long time (and a lot of versions) since I tinkered with it, but I don’t remember it being the most intuitive program
Comments:
1 ) The text on the top silk-screen is off the board - it will be cut off
2 ) Not sure if it was your intent or not, but the 4 emitters are not centered on the PCB - they’re shifted to the right quite a bit
3 ) No via’s for the thermal pads? Or maybe they’re in the design and you just didn’t export/create the NC-Drill file?
And change the name of the E$5 net to something meaningful…
I would also do the wiring to the left hand leds the same as the right hand ones (connections to the LED power pins) Run the connections vertically and don’t come into the LEDs via those little nubs. That tiny gap between the power etches and the LED pads is not a good thing.
Also, bring the etch into that E$5 pad in at an angle. It is currently forming a very acute angle with the hexagonal pad… that is known as an acid trap. Also, if you can, try to avoid right angle turns in an etch. Not as important these days, but it is good form.
Sweet, BTW can traces intersect? I'm asking because I was thinking about making a monster 7135 board, but I'm not sure how I could do it without the traces intersecting.
I’m not sure what you mean by intersect, to be honest. That board you just posted would fail miserably. You’ve got pin 2 and pin 3 tied together (at a minimum, I stopped looking after seeing that). That’s why you have two layers and vias. When you need one net to cross over another net, you drop a via and continue the trace on the opposite layer - thus running “Under” or “Over” the other net.
Ok, another question. How exactly do I connect a pad to a via? So far I have gotten this far.
I just need to connect all of the right pins together, since I can't have the wires (I think you call them etches) cross this means I have to route them through a via to get them on the other side of the PCB. But I can't figure out how to get the wires to connect electrically to the vias.
The placement looks better.
You need to widen the traces to the Out pin and the Gnd pin/tab. This will be carrying about 6A and those traces are going to be a bottleneck. Go as wide as you can.
Only traces that carry the same node can cross on the same side of the PCB. There is only one layer of copper on each side.
For example, you cannot cross a Gnd trace with a Vcc trace on the same side of the PCB. I’m not sure if that is the question you are asking.
When you do add vias add plenty each time to transfer a trace to the other side (2-3 per Amp is a minimum).
Place the vias where you want them (I would do them along the E10/E14/E18 row and manually rout an etch/trace from the third row pins to the nearest via on the red layer. Connect the row of vias on the blue layer.
You can have Eagle automatically drop in vias and switch to the next layer using the center mouse button. Run the trace to where you want to switch layers, left click to end the trace, middle click will then drop in a via and switch layers.
BTW, use fatter traces. .024” works well with SO8, etc surface mount pads. And I would replace all those zig-zags with a single trace. You can tell Eagle to do corners at other than 90 degrees.