voltage drop on STRATIX FPGA supply planes

Power planes have a finite resistance per square, and logic frequently slurps up a lot of current. One of the joys of mixed signal design is trying to stop digital supply current from returning through the ground connections used to define an analog ground.

-- Bill Sloman, Nijmegen

I've had this issue in recent designs too. Currents are higher, voltages are lower (1.0, 0.9V, etc), supply tolerances are tighter (3% instead of

5% now for some parts) but copper doesn't seem conduct any better :(

About the only thing that's improving is the DC/DC converter; some parts have a reference precision better than 1% now. Transient response is also better due to faster switching frequencies and cheap, large, low ESR caps.

The Cu in the BGA is thin. I don't know its sheet resistance, but it's probably greater than the (roughly) 1mohm / square of the inner layers of your PCB. At 20 or 30 amperes, you don't need many squares to get a voltage drop that puts you outside the supply voltage tolerance of the FPGA.

In my last "high power" FPGA design, we ended up with a plane on an inner (1/2 oz) layer in parallel with a fill on an outer (1oz) layer for the core supply. The layout guy hated doing it, but it gave adequate results.

It might also be possible to use smaller vias in your BGA fanout to reduce the "swiss cheese" effect on your planes, but I haven't tried that in an actual design.

I've noticed that some PC motherboard manufacturers are advertising 2oz copper as a feature, so it's not just FPGA folk that are feeling the pain.

Regards, Allan

Another thing I've been doing is to boost the nominal voltage slightly.

(Contrived) example: Requirement is 0.9V +/- 3% (i.e. +/- 27mV) at the die.

I budget +/- 1% (+/- 9mV) for the transient response. I budget +/- 1% (+/- 9mV) for the initial tolerance.

This leaves +/- 1% (+/- 9mV) for the voltage drop. However, the voltage drop is only in the -ve direction. If I change the feedback resistors to move the nominal voltage up by +1% (+ 9mV), I can allow for a voltage drop of 0 to -2% (0 to -18mV).

Of course, one can use remote sense on the DC/DC converter to get feedback to eliminate the voltage drop. My experience has been that the degradation of the transient response (due to having a more phase shift in the feedback) isn't worth it. YMMV.

Regards, Allan

How much current are you expecting in the core?

What do mean by "30mV voltage drop across the BGA itself" ? Does that mean PCB plane drop, or rather BGA balls to chip internal voltage?

The chip vendors should give us one remote-sense feedback/measurement ball.

John

I do that, namely go 50 mV or so high out of my switchers, anticipating copper losses.

I think the tight voltage specs on these FPGAs is part of the overall speed budget. If you're not pushing the clock rate/timing/temperature margins, it's not as critical. I also like to power-supply margin test working units, just to see how much wiggle room we have. Usually it's a lot.

John

es

ts.

.

If you have an old version .dxf file [with scale] of your PCB plane and identify current magnitudes and injection points, tell me the two cutout diameters to test; I could compare the effect of the 'swiss cheese' on the voltage drop across the plane. Actually do 3D voltage plots showing NO HOLES, Small Holes, Large Holes, and Delta Voltage comparisons.

I created a PCB Layout Tool that quantifies the Ground Plane Noise distributed across a PCB caused by currents from digital logic.

Provide an email address that accepts .zip and I can send small example images of results in .zip attachment. approx 72kB

[The purpose for creating the tool was to confirm parts placement and efficacy of plane cuts to keep GND noise below 1/4 LSB of the 24 bit ADC on the same PCB as the microcontroller. I simply got tired of 'shooting from the hip', worrying if the cut(s) is enough, and answering questions with, "In my opinion,..." Plus, wanted this PCB layout 'right' the first time.]

Colin

I'm not surprised at the numbers you are quoting. Personnally I would be more worried by the dynamic current variation and the effects that that the resistance and the parasitic inductance can have. If your decoupling isn't good enough ,and your power plane forms part of that, the effect of getting it wrong is far harder to debug than a static voltage issue.

Going back to the static losses using parallel planes is a good option as mentioned elsewhere. You can also go for heavier weights of copperin your power planes but that tends to restrict you track and gap you can use. This also related to the abilities of the manufacturer of your PCB and sometimes the price you pay for a PCB. There are also speciality PCB techniques like bonding busbars to the PCB to reduce the resistive loss but usually it's better to use a point of load technique and localise the high current areas. You can see examples of that technique in our extrene Merrick family of boards which are aimed at the HPC marketplace. Our recently annouced Merrick3

g/merrick-3/ uses 6 12A circuits just in PCIe card format for the core voltage. Internal distribution is by 12V rail in this case. Our new revision of our Merrick1 board will take this further and there are 20 POL regulators just for the core voltage.

One easy thing to do is to set you power supply on the higher end of the input specification at light load. Tolerance of your power supply is important if you use this method. Then even after losses hopefully your FPGA die is still receiving voltage within spec.

Many FPGAs will still operate out of spec although may not meet timing spec. Sometimes this can be used to solve a particular power issue but use with care.

John Adair Enterpo> Guys

You can probably already take your pick.....if you sacrifice the immediate local signal functions.

RL

I can sense an I/O bank supply voltage by just pulling an output up, but core voltage is harder to get at. I could swipe one ball out of, say, ten paralleled ones, I guess, if I were sure they were really paralleled.

Are core voltages segmented on most FPGAs, or are all the Vcc_core balls connected to one power net?

John

(snip, someone wrote)

(snip)

As far as I know, you aren't supposed to do that. Even if they are paralleled internally, there might be enough voltage drop across the internal connection to cause problems.

My choice would be to run a wire out from one of the power balls and measure the voltage on that wire. You could even use a power supply with a remote sense, such that it would adjust its output to get the right voltage on the sense line. Maybe even sense lines for both Vcc and ground.

If you don't have remote sense on the power supply, just use them as a remote voltage measurment.

-- glen

Probably not a good idea. You'll be leaving one corner of the power mesh sagging. A sense to the pad might not be a bad idea, though. ...if you can control the regulator.

Paralleled.

I should have probably have clarified the POL approach for a single FPGA. Some of the regulators we use are capable of being used in tandem so you might use 2 or 4 of them together. They do need to be tied together to avoid issues caused by large differences. This does avoid all of the current being delivered in a small contact area which can reduce losses and is sort of similar to the approach taken by most FPGAs themselves. It's also worth pointing out that there are always differences between individual FPGA power balls but they are small and FPGAs do cope with that. Sometimes part of the effect is more current gets dragged through an individual "good" ball causing more volts drop and crudely self regulating.

If we are looking at losses don't forget the vias. We recently did a

50A circuit on our Broaddown3 board and to keep losses reasonable we put something like 30 vias between the regulators arms and the internal plane. This is more extreme than most people will need to think about and you can argue about which size of via to use as there are some trades here in numbner of vias versus size. In some boards like our Merrick1 where we used a brick dc/dc, instead of an on-board regulator approach, we can have 50A going though a single hole / leg. It does help a lot having the leg to carry current but still means a lot of current in a local board area to handle.

Something to consider are copper filled vias when dc loss is important. They are a specalist technique also used to reduce via losses but do come at a cost and tend to limit the number of PCB manufacturers you can use.

John Adair Enterpo> On Sun, 08 Jan 2012 10:48:37 -0800, John Larkin

sh

you can