BGA on 2 layer PCB

[lawrence11]

In order to save cost on a prototype, I am going 2 layers board .

Most sections have been done on 2 layers and carefully selected ribbon wire strategies but now it comes down to the BGA, all my other component are QFP and every signal is well references and currrent loops on discontinuities are 1mm or less,

Board is all digital, running at about 160 Mhz 2ns rise time, My traces are very short etc, a bit longer than 1/6th but not much. When I dont run a trace over ground I run a jumper wire on the bottom plane that has a grounded via on the jumpr ends, this wire  has ground underneath it  and top and bottom tracks (wires) cross themselves at 45 degrees or 90 degrees, depending on opportunities, as you can imagine the board required much effort etc to keep all short and tight etc.

However, once they come to the BGA region, there is simply not enough room to to use the bottom layer as a pure ground plane, and I dont feel like having jumper wires underneath the BGA for signal. There was gonna be a jumper strategy/flat cable, for the Power region in the middle of the BGA, I was gonna make it as less inductance as possible  , however this is not elegant.



So I was thinking that maybe I can solve my board flex issue and my elegance issue by having made a very small 2 layer board that will accompany my main board and provide the necessary connections for the BGA power and HOPEFULLY also provide a ground plane to any signal that may be routed from the bottom layer? Is a ground plane discontinuity of about 1-3 mm really that bad? underneath the BGA, or am I worrying too much?

[Howardlong]

For initial prototyping BGA, I have had success with Proto Advantage breakouts, using parts over 200MHz such as the NXP LPC4370. Not sure if they have one for your device pitch.

To check continuity of all pins after reflowing, you can use your multimeter’s diode and continuity test to check the protection diodes and any intentional internal and unintentional external shorts. You can also peek visually down the rows and columns with your microscope, adjusting the focus appropriately, but the diode test is a pretty good one, and can easily be done in a five minutes once you get into the swing of it.

[lawrence11]

Hello, I wont be using breakout board.

I will solderng the BGA on the main board and a complement PCB for power plane emulation, that will be soldered with many wires to stitch the power planes together.

This will also add rigidity.

[lawrence11]

In order to save cost on a prototype, I am going 2 layers board .

Most sections have been done on 2 layers and carefully selected ribbon wire strategies but now it comes down to the BGA, all my other component are QFP and every signal is well references and currrent loops on discontinuities are 1mm or less,

Board is all digital, running at about 160 Mhz 2ns rise time, My traces are very short etc, a bit longer than 1/6th but not much. When I dont run a trace over ground I run a jumper wire on the bottom plane that has a grounded via on the jumpr ends, this wire  has ground underneath it  and top and bottom tracks (wires) cross themselves at 45 degrees or 90 degrees, depending on opportunities, as you can imagine the board required much effort etc to keep all short and tight etc.

However, once they come to the BGA region, there is simply not enough room to to use the bottom layer as a pure ground plane, and I dont feel like having jumper wires underneath the BGA for signal. There was gonna be a jumper strategy/flat cable, for the Power region in the middle of the BGA, I was gonna make it as less inductance as possible  , however this is not elegant.



So I was thinking that maybe I can solve my board flex issue and my elegance issue by having made a very small 2 layer board that will accompany my main board and provide the necessary connections for the BGA power and HOPEFULLY also provide a ground plane to any signal that may be routed from the bottom layer? Is a ground plane discontinuity of about 1-3 mm really that bad? underneath the BGA, or am I worrying too much?

[ebastler]

In order to save cost on a prototype, I am going 2 layers board .

That implies that you intend to move to 4 layers for production units. If that's the case, how significant will the learnings and test results from the 2 layer prototype be? The final production design may behave quite differently, and having to revise it (late in your design process) may introduce errors. Wouldn't it be advisable to get your prototype as close to the final design as possible?

It seems to me that you are aiming to save money in the wrong place. You may easily pay more than the saved amount by requiring an additional prototype iteration, or many times more if you end up with a bad production batch. (Not to mention labor hours...)

[lawrence11]

It will be finished project, that stays a prototype.

There will be no iteration.

It will be either elegant or ugly.

[ehughes]

In order to save cost on a prototype, I am going 2 layers board .

Just as a reality check,  if you spent more than a couple hours planning for a double stack of  2-layer boards then you have already eliminated the possibility of a cost reduction.

So I was thinking that maybe I can solve my board flex issue and my elegance issue by having made a very small 2 layer board that will accompany my main board and provide the necessary connections for the BGA power and HOPEFULLY also provide a ground plane to any signal that may be routed from the bottom layer? Is a ground plane discontinuity of about 1-3 mm really that bad? underneath the BGA, or am I worrying too much?

This is an extremely bad idea for your return currents.    You want you reference plane to be 1 pre-preg layer (4-8mils depending on materials) from your signal if you care about Z-Control,  EMC, etc.   

Your time is much more expensive than the cost adder for a 4-layer board at this point.

[lawrence11]

Dont mix myths with what is really possible.

1 pre-preg layer? I am using .8mm pcb material, so the plane is at best .8mm away.

I hope this will be enough. My spacing between is 4x distance of trace, the jumper wires are even closer to the ground.

There wont be significant propagation delay variation and my current loops will be tiny.

I will keep traces short at 40mm and this will be modeled as a capacitor.

[asmi]

Board is all digital, running at about 160 Mhz 2ns rise time

Something doesn't add up here. 160 MHz equals to 6.25 ns period. If we assume fall time equals to rise time, we get 6.25 - 2 * 2ns = 2.25 ns / 2 (assuming 50% duty) = 1.125 ns of "sustained" level. This is not good signal to begin with.

So I was thinking that maybe I can solve my board flex issue and my elegance issue by having made a very small 2 layer board that will accompany my main board and provide the necessary connections for the BGA power and HOPEFULLY also provide a ground plane to any signal that may be routed from the bottom layer? Is a ground plane discontinuity of about 1-3 mm really that bad? underneath the BGA, or am I worrying too much?

Yes, it is very important to have unbroken reference plane. When it comes to SI, there is no such thing as "just a little bit". You can use thinner traces in BGA breakout regions, but broken ref plane is an absolute "no-no". "Ground under jumper wire" is just

Bottom line is - you're trying to find savings in the worst possible place. Physical layout is a "make or break" when it comes to high-speed circuits, and the purpose of the prototype is to find out if your layout is good enough or not. Besides 4 layer boards are very cheap nowadays, so odds are you're going to spend more money doing multiple layouts and manual assembly and jump-wiring stuff. We're talking about ~30-40$ of savings - that's about 30 minutes' worth of earning for good engineer. Think about how much additional time you're going to spend botching together these 2 layer "prototypes", and then think again if you're saving money, or wasting much more instead.

[lawrence11]

http://www.ti.com/lit/ds/symlink/tfp401a.pdf

1.9 ns

How can it be an absolute nono when a via, is only considered bad at about 1+ Gbps before you start needing grounded via strategy around that via. That via is like what, 1mm... 1/3 of my GAP.

Basicly, a via should be made with grounded vias once you hit 150mhz according to what you are saying?

[asmi]

1 pre-preg layer? I am using .8mm pcb material, so the plane is at best .8mm away.

Forget about SI with that kind of "reference plane". You will need 1mm+ wide traces to get anywhere near required impedance. 0.2 mm wide trace over ref plane 0.8 mm apart will give you ~120 Ohm impedance. That will destroy what's left of your signal integrity - which is already very bad with 2ns rise.

[lawrence11]

I thought this only applied when track was considered transmission line.

and at 1/5.7th lenght  rise time I could get away with that and do as I wished.

Ringing is basicly the impulse response, and the parameters of that response are based on inductance, capacitance, trace lenght.

[lawrence11]

I thought this only applied when track was considered transmission line.

and at 1/5.7th lenght  rise time I could get away with that and do as I wished.

Ringing is basicly the impulse response, and the parameters of that response are based on inductance, capacitance, trace lenght.

But I get you the the dielectric thickness.

this Is a major issue, It might mean its impossible if the return current is all spread out since the field is far away.

Cant have a super flimsy board now can I.

This makes it difficult now, I`m a bit pissed.

[asmi]

I thought this only applied when track was considered transmission line.

and at 1/5.7th lenght  rise time I could get away with that and do as I wished.

Ringing is basicly the impulse response, and the parameters of that response are based on inductance, capacitance, trace lenght.

I suspect your problem will be impedance, not ringing. Will run some sims later if I won't forget.
Also you're going to have ~1.5 Gbps HDMI traces on this board. They will probably go off-board. These traces are required (by HDMI spec) to have 50/100 Ohm impedance.

[Brutte]

I have never routed a BGA pcb.
The footprint looks like a uC and that does not seem like a 160MHz signals. What 160MHz signals would you like to feed into that uC? SDRAM @ 160MHz?

15x15-9=216, seems like TFBGA216 with 0.8mm pitch.
Out of those 7x7 internal square is just VCC/GND and some supplies so you have to worry only about 176 balls there. Of course 14*4 =56 are easily faned out, the remaining 120 would have to fit into 56 spaces in between perimeter balls. If you are able to fit two traces in between two balls then that job seems easy. What I can suggest is:
- count the IOs/balls that you must fan out. If you can leave some external ball unused then just use the real estate to fan-out more traces underneath and cover that with soldermask. No solderpaste. If you leave 10 IOs of those 216 hanging here or there - nothing bad happens. Unless it is a boot pin or something equally essential.
- you can also hardwire IO to VCC or GND to spare some room with fanning out (just do not mess up the IO configuration)
- also you can hardwire two/three IOs if you do not need those at the same time.

Of course this is a hack. Iff you go for volume (>10k) it is worth considering.

Mind I do not believe in the supremacy of GND over Vcc.
IMHO same currents, same electrons, same ripple. Just direction opposite.
GND does not deserve better treatment than VCC.

[Mattylad]

BGA on a 2 layer board?

Ha, ha, ha...... good luck with that.

[T3sl4co1l]

False economy. 4-layer boards are hardly more expensive than 2, and vastly cheaper compared to the heroic effort you're considering (and I guess, have already mostly done(!)).  Same goes for any cost/savings on using/avoiding BGAs or such (as the case may be).

Tim

[ehughes]

Dont mix myths with what is really possible.

1 pre-preg layer? I am using .8mm pcb material, so the plane is at best .8mm away

I am not sure what myth you are referring to.    A 4-layer PCB should have reference planes on layers 2 and 3 so they are just below your transmission lines.      A standard 4 layer will only have 1 or 2 sheets of 2112 between layers 1-2 and 3-4.

A 4 layer board is what you want.    Look up any presentation by Rick Hartley.  He teaches it well.     In your stackup,. Your high speed return currents are going to flow everywhere execept the plane on your daughter card.

Solve your mechanical issues with proper supports, not a daughter card.  The psuedo 4 layer design is the worst of all world's when it comes to SI, ease of assembly and cost.

[lawrence11]

Well I guess 4 layers is the best answer then. But you guys talk like its a 30$ difference, its more like a 200$ difference.

Its not really about BGA problem tho, they component had a tqfp package, but the layout was gonna be more messy.

The problem is bad ground plane, its too high above.

So I watched the Rick Hartley, I really liked it, but he mentions .2mm for 300mhz signal

what if I had 150 mhz signal on a .4mm pcb??

My board could be .4mm thick and about 3" x 3"

But honestly tho, you guys exagerate so much, its all about "your perspective" about black magic, I'm sure I could make this work even on a 2 layer board if I do everything perfect, but do I feel like doing that now since it will be so flimsy?

You guys cannot even imagine how whacked out crazy I can be when it comes to 2 layer boards, theres always a solution.

[lawrence11]

Ok yeah it took like 100 hours to figure it out, but I still did it.

I could switch to 4 layers if I wanted to.

[ebastler]

Well I guess 4 layers is the best answer then. But you guys talk like its a 30$ difference, its more like a 200$ difference.

That number seems high. What board size and quantity are you looking at, and who are you ordering from?

[krho]

@lawrence11: 160x100mm 10pcs 120US$ + whatever the postage is to Canada

[lawrence11]

Okok

4 layers is what I gonna do.

Anyways I dont like the tone of you naysayers, It can be done I tell ya .

The price gone down last I checked.

[xaxaxa]

pcbshopper quotes $65 cad including dhl shipping for a 10cm x 10cm 4 layer board at easyeda, and $83 cad at elecrow. In china it's $40 cad everywhere. Still a bit more expensive than the $20 for a 2 layer board, but for me imo just not needing to solder any jumper wires is worth it.

[mikeselectricstuff]

For a 1-off, the additional time to do it on 2L will far outweigh the additional cost of a 4L PCB, even if you don't value your time very much
At 160MHz you really need a decent ground plane for decoupling, so you may spend time doing 2L only to find it doesn't work reliably.