So here are pictures of my current layout. Thanks in advance for any helpfull comment.
So the first problem I see isn't with the power stuff, but with your DDR memory. You seem to be routing the pins "just to hook them up" -- this isn't a 100 kHz i2C bus on an Arduino board where you can get away with that -- this is a 266 MHz DDR memory bus. You can't use right-angle traces (they cause huge impedance changes), you have to keep trace spacing consistent (as much as possible), and the DDR CLK signals are a differential pair -- they need to be routed as such. Trace lengths need to be matched. Solid ground references need to be poured under the traces.
Two-layer boards are feasible, but only if you put the DDR memory on the bottom of the board, right under the i.MX233. Download the design files from Olimex for their Olinuxino Micro to see how they do it. I'm pretty sure they were inspired by the TuxRail board, which also has similar routing. Without putting the DDR memory under the chip, you're never going to get the trace lengths matched close enough for signal timing.
If you want to keep components on a single side, you'll have to go to a four-layer board. Trust me -- I've tried routing a two-layer single-sided i.MX233 board, and they've never worked. Four-layer boards make routing much better.
You also have major power issues. You just need to pay attention to what you're doing a little more, use planes better, and switch to smaller caps. First of all, use the largest traces you can fit for all power connections -- especially that inductor. You have a polygon pour on your top (red) layer, but look at it -- it's useless. None of the important components are connected to it because you've got traces and components that block it. I had to look at it for a while to figure out what it was even connected to -- ground. Typically, on two-layer boards, I do ground on the bottom and VDD on the top layer. I put my decoupling capacitors right next to the power supply pins, and then drop a via to ground.
You need to get those caps way closer to the pins -- and use wide traces if you need to carry power (say, the 1.2V supply rail that you're routing under the chip). For capacitor sizes, I recommend 0402 for the 100n, 0603 for the mid-sized (1-5.6uF), and 0805 for the big guys (33+ uF). The DC/DC converter pins will need one of each of those. The i.MX reference design also has a 10n, but I've always safely ignored that one. Linear regular output pins just need the mid-sized one and the 100n -- I use 4.7u for the mid-size cap because I have a few reels of them laying around. Power input pins just need the 100n. In all cases, prioritize their placement in ascending order -- for the DC/DC converter outputs, the 100n should be closest, followed by the mid-sized cap, followed by the large reservoir cap.
Your board is also just really sparsely placed and routed. There's huge gaps of hundreds of mils between components. You just need to squeeze everything in -- that'll help a lot.
For an example of a layout that works, here's a picture of one of my i.MX233 layouts:
Full disclosure, this board is obviously a work in progress and hasn't been tested, but it's in line with how a board like this should be routed. The layer stack-up I'm using is 3.3V on the top (orange) layer, 2.5V on the second (purple) layer, GND on the third layer (solid power plane -- no routing -- not shown), and 2.5V on the bottom (blue) layer. Do you see now nicely all the caps fit in together? Except for the 1.2V and 1.8V supplies (which only have a few connections), all the voltage nets are routed on planes and polygon pours. Here's a picture with those polygons shown:
Notice how few dead areas there are? That takes thoughtful, careful component placement and routing.
I don't want to get into a tools discussion -- because, at the end of the day, the best tool is the one that you know how to use. Having said that, I've never used KiCAD much, and although I'm a big fan of open-source software, until their experimental follow-me and push routing get integrated into the program, I don't think it's a useful tool to routing a board like this. It doesn't have any built-in support for length tuning, and routing is painfully slow to do. If you want to stick to KiCAD, you'll most likely have to export your board to FreeRouting.net, and do the routing there. Yuck.
Luckily, as a university student, I have access to Altium -- so I was able to route this whole board by hand in about an hour :-) If you have access to a professional PCB editor, you should definitely take time to learn it. And if you ever get a job doing PCB design for a company, don't let your boss be a cheapskate -- make him or her get you a copy of a real PCB editor (Altium, Orcad, PADS, etc).
Hi
If i may ask you one more time for help.
Here is my current ram routing. All traces are between 13mm and 15.5mm long. I've matched groups more precisely when I could. Do you think it should work?
By the way I've started to devellop a length matching tool for kicad (and joined the devellopement team):
http://www.youtube.com/watch?v=UdQ-2EnWNkw
(of course it is very earlu stage).
Also I'm starting to wonder about trace inpedance. Do you think it is important. Also when I do the calculation whith the specification of my pcb manufacturer I get a result very far from 50ohm, and 50 ohm would require very large traces. But i'm unsure whether I should use 0.18mm (layer 1) or 0.018mm (croper foil) in the calculation. My current track width is 0.2.
My stack-up is 3.3v/groung/2.5v/ground.
Thank's in advance for your kindness! :smileyhappy:
Pierre.
I've just seen a picture of olinuxino micro. They don't seem to have done any global length matching. There are very short traces (like clk) and very long ones.
Therefore I guess my length matching should clearly be good enough.
EDIT: I just read your second message that indicates you connected BATT and DCDC_BATTERY together. That's your problem. Lift the chip, cut your trace, re-solder, and your board should work. Good luck! /EDIT
Since you're not using a battery, did you leave the BATT and DCDC_BATTERY pins disconnected? If they're connected together, your board will not boot. I recently ran a board that uses the IMX233 (in the LQFP package), and doesn't have battery support. You may want to cross-check your schematic with mine to make sure you've got everything in order. Here's the schematic of the power block of my design:
