All,
After reading and contributing to a few interesting threads recently about PCBs for FPGA designs, I thought I'd post about the technology I've been using for the past 3-4 years. My job involves getting a lot of high density circuitry into a small space, and so awhile back I decided to use microvias (laser drilled vias) to pack more stuff onto my boards. The surprising thing was that the boards worked out cheaper for my application than if I hadn't used this method.
I'll explain why, but you might first want to download the picture at
My stackup is ten layers, like this:-
1) signal 2) signal 3) ground 4) signal 5) signal 6) ground 7) signal 8) signal 9) ground10) signal
There are laser drilled microvias between layers 1 and 2. The only other vias are through vias, i.e. from layer 1 through all layers to layer 10. This means there's still only one mechanical drilling process during manufacture. What you can see in the picture you downloaded is how to route out all but four of the signal pins on banks 2 and 3 of a V2PRO in a FG676 package without using any through vias, just microvias between the two layers, blue and light green. The track and gap distance is 4mils or 100um. With this technology you can go 8 rows deep on a 1mm pitch BGA without using through vias.
In no particular order, here are the advantages.
It's no problem at all to put microvias in a pad. The microvia is just a
2mil deep pit that fills with solder, unlike a through via which must be plugged to stop the solder wicking away.You can use fewer signal layers because the signal paths out from the FPGA aren't baulked by through vias.
You can use fewer (or no) power layers because it's possible to fit a lot of bypass caps on the back side of the board from the FPGA, with through vias direct from these to the FPGA power balls. (In the picture you can see the ground (green) balls and Vcco (yellow) balls. By the time this board went out, there were two through vias for each power ball.) With a conventional board, the through vias don't leave space on the backside to fit (m)any caps.
You get to have a decent ground plane(s) for your BGA devices, not one turned into Swiss cheese by a myriad through vias. Bye-bye ground bounce.
You gain board area all over the back side of the board simply because there's less space used by the vias from the topside.
Compared to a through via, the SI of a microvia is much better. After all, it's only 1/30th the length of a through via.
The components can be closer together, reducing SI issues.
I always follow some rules when routing FPGAs this way. Like these:-
Draw lines from the four corner balls to the very centre of the part. Don't let any layer 1 or 2 traces cross these lines, it always seems to screw things up.
Be prepared to put much more effort into the PCB. This doesn't work well unless you're prepared to sit down with the layout person and swap pins on the FPGA as you route things up to align with other components on the board. For diff pairs be prepared to swap Ps and Ns. You can fix up the inversion inside the FPGA.
The upshot is, for a lot of my applications this saves me 4-6 layers over a conventional board. (For others, it simply makes the job possible!) This more than compensates for the cost of using the laser vias. Also, I don't want to hear about warpage! Although the stack looks asymetrical wrt ground planes, the stack up *is* symmetrical wrt cores and prepreg layers. I've had no problems whatsoever with warpage on 1.6 mm boards of up to 8x6 inches.
I'm by no means saying this is the best solution for every board, but it worked really well for me. It's certainly worth asking the PCB fab house about the cost, yield etc.
Best, Syms.
p.s. I'm glad I'll have microvias when I come to route up this bugger.:-