EE/PCB layout experts, got a question on trace sizes for you.

I'm having one hell of a time routing traces on a board I've been trying to route for a week now. The board is 15.05" x 3.02 inches, has the following components:

384 x 0805 resistors ~24 x 0805 capacitors 24 x 52QFP IC's 24 x 32x32mm LED matrix boards (24 PTH pins each) =576 PTH holes 1 x 16pin Header

Needless to say, the board is packed. I tried using SO-16 resistor networks to cut down on the number of resistors, but due to the closer spacing, this actually made routing more difficult.

Due to costs, I'm trying to keep this board a 2 layer board, but am finding it extremely hard. I tried to manually route the layout, but found that to be extremely hard to do, so I went with an autorouter (, java based router). After much trial and error, I was able to route the board, however I had to use the following numbers for my layout:

Signal traces: 0.1mm (~4mil) traces/0.2mm (~8mil) spacing 5V power traces: 0.2mm(~8mil) traces/0.2mm spacing Smallest hole:0.2mm

I used a Trace Width Calculator to come up with the numbers above given a max load of 1A possible, but not sure if those numbers will work.

My question is, given the following datasheet information regarding the LED matrix displays, and the LED drivers, will those widths be enough, or do I need to go larger to be safe?

LED Matrix forward Current: 20mA @ 2.3V (reverse voltage: 5v)

Driver Row Sink current: 16mA @5v Driver Row Source Current: -70mA @5v Driver COM(common) Sink Current: 350mA @5v Driver COM Source Current: -60mA @5v

I can post the datasheets if necessary.


Yow! That does sound packed. Why not go to 0603 resistors/caps? That will free up some routing space.

You will probably lower your costs by going to a 4-layer board and increasing trace/space to 6mil/6mil design rules and 12mil holes. You are going to pay a premium for 4 mil traces and 8 mil holes, possibly more than going to a 4-layer board. At least investigate the option!

It also doesn't make much sense to have 4 mil traces and 8 mil spaces. Board houses will use the same number for both, so you could go with 4mil/4mil design rules for the same price and get better routing density.

8mil traces for 350mA should be fine. Traces carry more current than you think. Of course, the bigger the better! You may want to route those traces by hand at 12mil just to see if you can get away with it.

-- The Gadget Shield: accelerometer, RGB LED, IR transmit/receive, speaker, microphone, light sensor, potentiometer, pushbuttons

Thanks for the quick reply. yeah, I thought about 0603, and will probably go to that size to free up as much space as I can. I’ve also considered (as well as to facilitate possible replacement of bad LED Matrix boards) using SMD headers to free up the space occupied on the bottom layer by all the holes.

4 Layer was also an option, however at least for the first prototype, I’d like to try and save as much in terms of cost as I can, as the house I’m going with ( charges nearly double for 4 layers (57.81/board with 190.35$ setup fee for 1 board) vs 54.98 for 1 board with a one time 98$ setup fee. 150$ for 1 board vs 250 is a huge difference (given if the design works, then it would be much cheaper to mass produce off the same design.

to give you an idea of the space constraints, here is the board image (ignore the 4 caps off to the botttom right, I haven’t placed those yet.

I’m going to try to reroute again with .2mm traces (according to your post the .2 should be fine for the power requirements as well) and then hand route the traces that don’t work (I ended up having to manually route about 12 traces the first time.) The benefit for me of having the autorouter batch it is speed, as well as reducing the # of vias used (when I first ran it, I started with 532 Vias, it was able to cut down that number to 432)

I wish the matrix’s were a little larger, or had integrated resistors…this would make things much easier!

Edit: having so many damn resistors is going to suck hand soldering, as that board won’t fit in my toaster oven =(
Edit2: Just checked, you’re right about the premium cost. a 4 layer board with larger drills/traces is cheaper, but only by about 40$, $213 for 4 layer vs $150 for 2 layer with smaller traces. the per board price is around the same, it’s the setup/tooling costs that are changing. I’m going to give it a shot at routing again on 2 layers, but if it’s a hassle I’ll have to switch to 4 layers.

Actually it looks like you have more room than I thought. One thing working against you is how close the QFN's are to each other. Is that necessary? You need to leave space around them to break out traces to get to other places. I'd suggest spacing them out a bit more. Given how much space there is I doubt going to 0603 components will help all that much. But move the components farther away from the PTH holes as you are essentially blocking off all routing in that area.

Thinking about your problem again, it's not going to be 5V that is as much of a concern as is GND. If you have 24 LED matrix boards each drawing 350mA then the ground return path is carrying 8.4A !!! You need to think carefully about how you're going to carry that back to the power supply.

-- The Ruggeduino: compatible with Arduino UNO, 24V operation, all I/O's fused and protected

RuggedCircuits: Thinking about your problem again, it's not going to be 5V that is as much of a concern as is GND. If you have 24 LED matrix boards each drawing 350mA then the ground return path is carrying 8.4A !!! You need to think carefully about how you're going to carry that back to the power supply.

I'm putting top and bottom ground polys on the board, and these get fed back through the 8x2 connector to a control board that has it's own ground plane that connects directly to the battery terminals used to power the the display, so I'm somewhat sure that this should not be an issue (tested to work using an arduino uno with the battery) Also, the 350mA is continuous, however each line is only driven for a split second (scrolling text, along with PWM brightness control). In testing with a multimeter and 3 separate panels connected to an arduino, the panels are drawing around 250mA with a standard line of text moving across them.

I'll admit I'm not a power expert, but it seems to work as designed so far.

Unfortunately, Holtek does not supply layout or design guidelines with their chip, so I'm going with the same guidelines Atmel puts, and that is to put parts close to the chip. As for the spacing, I could space the bottom ones out slightly further, I positioned them closer to the inside to allow more space to route out around them. If I go with SMD headers, that'll free up some space on the bottom potentially due to to the lack of holes.

I've been using Pcbcart and reckon they are great (can send native Altium files which I like), however I may use itead for the next job as they are a lot cheaper for prototypes. (just noticed the board size though, no good for itead)

One other thing, many board houses have a restriction on the board's aspect ratio, 15x3 is pretty narrow, have you checked that?


^^ I've used them before for small boards (~3 sq inches) and they were good, but for larger prototypes it was faster to use . However, for something this size, is too expensive (2.50/sq inch), so I'm going with pcbcart again. using the online quote tool, it accepted my measurements, so it should be ok, and I'll probably order 2 or 3 copies as a start.

I've successfully gotten the traces up to 8 mil for signal, and 12mil for power, might go slightly larger on the power, but this should be fine. I had to hand route 12 traces, but thats not bad vs. the 1500 or so that it started off with. Going to have to do some tweaking to it.

RuggedCircuits, I took your idea btw, and spaced the bottom TQFP ic's further apart, this helped me in the end to route larger traces. They're now aligned so that the left or right row of pins is directly below the opposite side in the top row (Top right pins align with bottom left pins, etc)