Re: PCB Layout for BGAs

By "normal" vias I mean through-hole, without plugging or tenting - the cheap ones. And by "normal" track widths and spacing, I mean the perhaps 6 mil - cheap sizes that any pcb manufacturer can make without extra charge. Basically, at 0.8 mm BGA we didn't need to do anything special or consider it an especially high-density card. It was still an effort to route, as there are a lot of connections in a small area. But it didn't need extra cost for the pcb.

If you are already congested at 6 layers on the board, then you will might have to go for beyond that. The first step is to talk to your pcb and board manufacturers about via-in-pad, using tented or plugged vias. If you can put the vias on the pads themselves, without causing voids or blowouts during soldering, you can save a /lot/ of space. Next step beyond that is microvias from outer layers to layers 2 and 5. We had to do that for the 0.65 mm package BGA.

I'm afraid I don't remember the sizes used - I was not directly involved in the layout and routing. (I've done fine-pitched BGA layout, but it's probably 15 years since I did a pcb design myself.)

Is it the routing you see as a problem for 0.65 mm pitch, or the cost of boards with high density features, or the production of them? We have found that while the 0.65 mm pitch parts were harder for the layout and a little more expensive for the boards, parts in these packages can be a lot easier to get hold of. The choice of 0.65 mm or 0.8 mm was forced by component availability, rather than as a preference by our layout folk. (Our production people have no qualms about mounting small pitch BGAs.)

Mechanical drilling has a lot bigger tolerances than laser drilling, so you do need to have extra space between the via hole and tracks on the internal layers to account for the inaccuracies. Some manufacturers will give you tighter specifications - in particular, some use lasers for 0.2 mm holes. (And some, on the other hand, use mechanical drills and charge extra for 0.2 mm holes due to extra breakage of the small drill bits.)

That's always the big problem these days. I'm afraid I can't give much advice there (at least, nothing that you won't already have thought of yourself) - we are all in the same boat.

I've not done this for real, but I did a bit of playing around with PCB routing such BGA FPGAs. I was trying to see if it was feasible to use them on cheap PCB processes with basic soldering (I never actually made any boards to test it). One of the limitations of cheap processes is the tolerances can be quite slack: eg 6mil track width/spacing, which makes doing the BGA escapes hard.

An interesting (to me) observation was that you may be able to make PCB routing easier by choosing your pinout wisely - eg don't route signals from inner or adjacent balls where you don't need them. That means it wasn't such a headache to have more pins because you can ignore many of them. For some of them, it was fine to short adjacent pins to (safe) power rails if it wasn't possible to separate them.

Another observation was that it might be fine to have a net route through unused pins if they're all high impedance in the FPGA config. I'd not do this for fast signals, but maybe OK for slow/static ones.

Not ideal, but a couple of tricks where FPGAs offer a little bit more PCB routing flexibility compared with off the shelf parts.

Theo

On 2023-01-09 snipped-for-privacy@gmail.com wrote in comp.arch.fpga:

Digikey has a number of FPGAs in QFP100/144 in stock. Efinix, Microchip, Lattice, Xilinx. Nothing that suits your needs?

Okay, QFP144 is too large, that severily limits the QFP options, but Lattice does have a QFP100: ICE40HX1K-VQ100. But this one may not have enough logic for you, its the smallest in the series.

Just four or eight multipliers, and many more on-chip goodies:

That should be enough to fit a via between the 0.8mm-BGA pads - that's what we do regulary. If you want blocking caps underneath the BGA, you will probably require plugged/plated vias. You will have to look at the pinout and do the fanout routing to see how many layers you need.

Talk to your PCB manufacturer about the details before doing the final layout - there is some fine tuning (eg. drill size, annular ring, spacing) where different PCB manufacturers have different preferences regarding which rules will yield good results - when doing do, 0.8mm BGA should be possible at modest PCB costs.

cu Michael

We have used Lattice MachXO2 in TQFP100 in the past - not sure if these fit your needs.

Okay, this sounds like the MXO2 might be two sizes to small for you.

cu Michael

The reason you can parts in high-density packages, but not low-density packages, is that there are lots of people such as yourself who are so reluctant to use the small pitch devices. (This is not criticism - you have solid reasons for preferring larger pitch devices, as do many others.) Big manufacturers often prefer smaller pitch and higher density, as it can lead to lower overall costs for their products, even if design is more costly and the pcbs are more expensive.

There have been component supply issues for several years now, with only gradual improvement in many areas. But there is a general pattern of somewhat higher availability in smaller pitch parts.

The board stackup, routing and bypassing recommendations from FPGA manufacturers are basically bollocks. I believe it is primarily a matter of being able to fob off complaints and support requests by saying "Did you follow our layout application notes, impossible though they may be? If not, it's not /our/ fault that you have problems."

OK, that's a bit of an exaggeration, but you can ignore the suggestions of 16 layers with 8 different power planes and a dozen different capacitor sizes mounted directly below the device.

Yes, there are complications for BGA layouts. And I'm afraid you are going to have to do some research, some learning, and some discussions with both PCB manufacturers (or their proxies) and board builders.

For the same pitch of BGA, there can be different sized balls, and different sized pads on the underside of the BGA device which will affect the shape of the ball after soldering. Pad size on the pcb has different options. You have a key decision between solder mask defined and non-solder mask defined pads, which affects mechanical strength, thermal stability, solder paste masks, routeability, and manufacturing requirements. And BGA soldering has different requirements in production than non-BGA devices.

I have no doubt that this is something you can master quite quickly - it's not /that/ hard. But it's not something you can learn just by a thread on a newsgroup.

I have a 529 pin BGA with 0.8mm pitch. SMD pads for the BGA are 0.4mm, vias are also 0.4mm with 0.2mm drill. Using these rules, a via fits nicely between 4 BGA pads.

I have plugged/plated vias in order to put 0402/0201 capacitors underneath the BGA, but if you can place the capacitors outside the BGA area, normal vias should do.

OK, if you do not order the PCBs yourself, you have to forward this through your CM. You will probably have to prepare a sample design (just the BGA area with fanout), produce gerbers, and have them ask for feedback. Same about the layer stackup if you need controlled impedances.

cu Michael

A great many boards are built into products. It's not just on cell phones or other consumer gadgets that saving space is important. If the device you are making can be smaller, then it uses less material (plastic, aluminium, whatever), weighs less, can go in a smaller box, costs less to deliver, smaller storage space, etc. For most people who only see one part of a system, it can be surprising how these things add up in the complete price of many products. Shave off a percent or two of the price at each step, and it all adds up (actually, it all /multiplies/ up!) to lower cost overall even if the board is more expensive. Of course you have to be dealing with large quantities (bigger numbers than anything we make) for these things to be important

- but it's the big buyers that buy most of the parts!

Even if we just stick to the pcb itself, pcbs cost per square centimetre. Using smaller packages can mean higher cost per unit area, but can also mean lower total area if the package size is the driving factor (rather than mechanics, connectors, etc.). Reduced total area can lead to more boards per panel for part placement and soldering, and lower manufacturing costs.

Fair enough. Certainly you want to look at all the information you can here - you just have to be aware that some of it will be conflicting, and some of it will be overkill. I read somewhere (a long time ago, and I've forgotten the details) of someone who initially made their design following application notes for bypass capacitors. Then to save costs, they depopulated about 90% of these capacitors, basically at random. There were no measurable differences in signal integrity, EMC results, or any functionality.

Yes.

BGA balls are attached to circular pads on the underside of the BGA package, and the size of these pads can be different for different packages with the same pitch. In general, you get the mechanically strongest bond when the pads on the pcb (or the opening in the solder mask, for solder mask defined pads) is the same size. But that does not mean you /always/ want them to be the same as there are other factors in the trade-offs, and it's quite rare that mechanical strength is critical. (If you are gluing on a large heatsink, without screws, and then mounting the board upside down in a high vibration environment, you'll have different requirements from a "normal" usage.)

That's the unfortunate reality these days. Find out what you can get hold of, check if it looks good enough, then buy the stock. There's no point in finding out that vendor X has good layout and manufacturing information, or vendor Y has good toolchains, if you can only get parts from vendor Z. (This is not news to you, of course - I'm just sympathising.)

Trace width in the BGA area is 0.11mm (for data lines).

That is the minimum given by our PCB manufacturer - small via pads allow for bigger traces where needed (power traces, despite using a 8-layer PCB).

That is the area where you can fine tune after discussion with your PCB manufacturer. Some may like a bigger annular ring, some may prefer smaller ring and more pad-to-trace clearance.

I would expect pick & place to be easier for the 0.8mm BGA than the TQFP. Cost increase will probably happen at the PCB level (small annular ring, or more expensive surface finish - TQFP may work with HASL, BGA needs a flatter finish. However, ENIG is not that expensive nowadays.)

cu Michael

Yes, BGAs can often be easier to place than TQFP's - you have a bigger pitch, and they "float" to the correct place even if there is a slight placement error.

On the other hand, you need better control of the soldering parameters, and they are harder if you have a board that has awkward heat flow - many high components nearby, or big thermal masses. And it is harder to check connectivity and good quality soldering.

A good production facility will have tools to help here. They will do the first boards with temperature probes between the balls, and X-Ray to check the quality of the soldering. Make sure you have a production house that is not scared to give you feedback - many far eastern places will just do their best with what you give them, and never tell you how to improve your layout.

Re-work is, obviously, far more difficult with BGAs.

The 0.8 mm 256-ball T20 isn't bad...

We considered a T8 for a simpler application, but its 0.5 mm ball pitch looked nasty.

The efinix tool chain looks like it was developed in someone's garage, which is actually praise. It's free and simple and just works without

The BGAVIAs are 12.5 mil OD with 8 mil drills. The other vias on the board STANDARDVIA and POWERVIA are bigger.

I have seen vias with no annullar ring, just a trace falling into a hole, but the PCB houses don't like that.

Filled via-in-pad would be cool but that's complex and expensive. As is buried vias.

We use US suppliers for production boards, and they seem to think this

Another project used a 484 ball Zynq and we used almost every ball. Lots of different power pours too. That took 10 layers. Another recent board has a 400-ball ZYNQ with a few unused PS pins and fits on 8 layers.

The ZYNQ has analog inputs but, crazily, they are all differential so they make you ground a perfectly good i/o pin for every analog input that you want.

$150! That's in the noise, and an eval board is good anyhow.

Yeah, we have a lot of aerospace customers and avoid Chinese parts.

I don't know. My PCB guy decides stuff like that. I'd guess that he wanted it to pass some design rule check, or maybe he started metric. The board houses haven't complained as far as I know.

You should do your own thing and check with whoever will make your boards.

IF you contact a "Good" board shop, they should be able to give you their specification to make the board.

They may have several levels (of cost) with different requirements.

If you board shop is NOT giving you a promise that the boards theya have built will be "successful", then I would not touch them.

Yes, capabilities do vary a lot, so I always like to talk with my CMs about what shops they use for the sort of class board we are working on, and check with the shop on their requirements.

We also keep a general idea of capabilities, so if one shop is a bit better on one spec, we might try not fully using that so other shops are likely able to handle it.