Electronic – SDRAM issue – LPC1788

That's a lousy stackup. Your cores should be 0.2 mm and the balance of your thickness should be in the prepreg between layers 3 and 4 (Inner 1 and Inner 2).

The reason for this is that, for any signal on a trace, there needs to be a return current path on the plane right under it. The return current in the plane will try to minimize inductance (i.e. loop area), which means it will try to follow under the signal trace. If the signal trace is distant from the plane, it will look to other traces to find a return path. This is electromagnetics you're fighting.

Further, by having inner layers at different distances from their reference planes (remember, all supply rails look like grounds at AC!) compared to the outer layer distances, you create an impedance change every time you swap layers (though this can be counteracted with trace width changes, though I found it worth the trouble only once), and you significantly increase the potential for crosstalk and other interference.

Another thing you need to check is the materials used: there are over 20 different materials that call themselves "FR-4", for example. The stuff I usually use is called 370-HR. It behaves quite well with high-speed 100-500 MHz signals.

Regarding the clock line, IIRC on my last SDRAM design I had the clock set up so its edge happened last (its trace was longest by 1 cm), after all the address and data lines stabilized. So, yes, retarding the clock is worth trying. I didn't need any impedance control on the SDRAM lines.

Your termination resistors should be placed as close to the line drivers as possible. If they're not within about 0.5 cm, they can cause reflections themselves, resulting in overshoot and ringing. IMHO, 3 cm trace length is awful short to need termination resistors (I use them starting around 6-10 cm); have you tried just taking them out?

Another thing to check are your planes: Do you have signal traces crossing plane cuts? This is a huge no-no, because it forces the return current to take a long route around the cut.

Finally, edge rate is a huge problem in these designs. A lot of chips have needlessly short rise and fall times, and reducing clock frequency has no effect on this. These fast edges are great for creating reflections. This is what your 22 ohm terminator resistors are trying to fix: they slow down the edges. Though, if you're really pushing it, a tool like Mentor Graphics' HyperLynx can be used to find the optimal termination design.

Some books I can recommend to you that cover all this and a lot more, and we swear by them at work:

• Signal Integrity Simplified by Eric Bogatin
• Electromagnetic Compatibility Engineering by Henry Ott

These books cover EMI reduction, shielding design, PCB stackup, impedance control, power supply decoupling, and a lot more. Further, Mr. Ott teaches seminars on this topic (comes with a free copy of his book).

For 2, start with settings from an iMX31 demo board. Then modify them as required for your part (speed and size mainly). In particular you probably have the wrong number of wait states on read.