Hey guys, I’m looking to use an LPC3180 which only comes in a BGA320 package. The following image shows the package dimensions, pulled right from the datasheet.
My question is whether or not creating a dev board around this package is even possible using BatchPCB.
http://www.onstagedancetheater.com/new/untitled.PNG
Sorry for the large image…
-Nate
You are going to have a very hard (basically impossible) time getting the signals out with 20 mil vias. You can make the footprint easily with 8 mil clearances, but you are only going to be able to get to the inner and outer rows of balls - the middle signals will be lost. Even with round minimum-sized lands you will only have around 0.45mm of diagonal space between them. You’re looking at microvias at that point.
Basically, it’s going to be a lot cheaper to buy an EK than build any small quantity of these.
Hmm, so you’re suggesting I buy an eval board / dev board rather than wasting my time creating one.
The only issue is where do I get one for the LPC3180?
I may have to decide to go with a different chip altogether then.
Ever used an ARM9 before? Any suggestions? I have a feeling that the response to that will depend on its use… Check the thread about the Super MP3 Player in the Projects forum.
Thank you for you input!
I just did my first BGA board and, while I’m hardly an expert at this point, I did learn a few things along the way. From what you’ve described, I’d say you have one thing going in your favor and one against. The one thing in your favor is the fact that there are only four pads deep. The one I did was a 10x10 matrix (100 pins - AVR Mega640 in the CBGA package). The thing working against you is the pitch - 0.5mm is about as small as you can get. I haven’t checked what size pad is needed for a 0.5mm part but for the Mega640 it was half. Given the 0.8mm pitch of the Mega640, that was 0.4mm. If that holds true with the 0.5mm part (ie: 2.5mm) then you are looking at a 0.5mm space between adjacent pads. This works out to 19.68 mils. That is enough for a single trace with 6 mil trace / spacing between pads. Unfortunately, that won’t get you there with BatchPCB but there are others that can handle this (check [PCBFabExpress among others). With 6 mil trace / spacing you should be able to route the outer perimeter of pins straight out and the next inner perimeter between the pads of the outer perimeter. As for the two inner perimeters, you can head in the opposite direction - towards the center of the chip. Since I have not done this, I could be completely off base here, however, at first glance it looks like the obstacles you are facing are less severe than what I had (since I had no “empty” inner portion of the chip to work with).
Good luck,
Dave
[Edit] Ack - I just rechecked my math (never post on a Sunday after watching NCAA games and consuming too many brews). You only have 2.5mm between pads, or 9.8 mils. With a space/trace/space between pads, this works out to less than 4 mils - doable, but expensive with most board shops. Sorry - my bad.
Dave](http://www.pcbfabexpress.com)
No problem on the maths, I fell into a similar trap when I first did them.
I think I’m going to switch my design to use an EP9315 from cirrus logic. It’s got more features that I’m looking for built into the chip which leaves more board space for potential routing issues, and will bring overall cost down as the board should be smaller. There is also a dev board with many nice features thats already available, and Olimex is in the process of finishing one up. It’s also a little less fine of a pitch which should help with routing when designing the final board, theres about 20.4724409 mils between pads, but a more complex pad pattern.
That’s a little more manageable, no?
Also, do you have any suggestions about the routing process itself, ie which signals where?
-Nate](ImageShack - Best place for all of your image hosting and image sharing needs)
Ohh!
If i use the nominal values specified, 1.27mm pitch, .75mm max ball diameter:
1.27mm - 2 * (.75mm / 2) = .52mm = 20.4724409 mils
If i fudge the pad size from .75 to .7, that gets me 22.4409449 mils, which means I can run one trace between each row/column of balls (7 mil traces/spaces, which is the smallest batchpcb bot will allow).
Do I have to use the max diameter of the ball for the size of the pad, or I guess the real question is how big should I make the pads?
Edit
I found an apnote by altera which said that for a solder mask defined pad with a 1.27mm pitch and .75mm ball diameter, that I should use a .60mm diameter pad. For a non solder mask defined pad, I should use an even smaller .51mm pad.
http://www.altera.com/literature/an/an114.pdf
Unless you really want/have to build a board, this one appears to be well-supported and affordable:
http://www.phytec.com/products/sbc/ARM- … C3180.html
I don’t have any experience with the vendor, but Keil supports the board.
If you can just as easily use the Altera part, go for it. Keep in mind soldering BGAs, while not too difficult, becomes harder as they get bigger and can be very difficult to diagnose when things aren’t right (unless you have access to an X-ray machine.
Good luck!
Thanks for your support!
I’ve got one final question about utilization of layers for a 4 layer board; Should I make the bottom layer a ground layer, the next layer a signal layer, the next layer another signal layer, and finally, the top layer a power layer?
What is the best way to approach this?
You should have it like this for a four layer board:
Top signal
Gnd
Power
Bottom signal
This gives maximum capacitance for the ground and power layers, and minimum inductance for connections to the ground layer.
Leon
