EMC discussion
in [FPGA]
|
From: glen herrmannsfeldt on 25 Mar 2010 19:29 Symon <symon_brewer(a)hotmail.com> wrote: > On 3/25/2010 6:13 PM, Kolja Sulimma wrote: (snip) >> Well, how do you create a low inductance path to the next capacitor? >> You do not necessarily need a full plane, but making sure there is a >> low inductance path quickly gets very cumbersome. > You use copper pours and puddles around the IC to link its bypass > capacitors. >> A power plane is as good a reference for a signal as a ground plane >> and the PCB stack needs to be symmetric anyway. So what is the >> disadvantage of having a power plane as layer 2 when there is >> a gnd in layer N-2? > 1) The stack up does not need to be symmetrical wrt to planes and signal > layers. However, you should make the substrates symmetrical. I have made > several boards that aren't plane symmetrical. Talk to your PCB vendor. > (Some of these boards were about 12x8 inches and didn't warp.) > 2) When a signal trace passes from layer 1 to layer N-1, its reference > plane has now changed. If this signal has a fast rise time, you have to > use a bypass capacitor nearby, with its attendant inductance, and via > inductance. With two ground planes, a regular via is enough. As I understand it, that mostly isn't true. For a reasonably plane there is enough capacitance around to get the signal across from one to the other. > 3) You make an interesting point when you say that a power plane is as > good as a ground plane as a reference. This is true. The problem comes > that you now have two references in your system, and they will have some > small noise voltage between them. You can reduce this to a small amount > of noise with capacitors, but for each power plane, you have to do this. > With multiple ground planes, they are all bonded together with the > ground vias in your board. Note that a single wire has inductance, and a single plane has capacitance. Even without another plane nearby, the capacitance of a ground plane isn't so bad. With another plane nearby, though, it is somewhat higher. At the higher frequencies, it is the plane capacitance that you see. At lower, but still plenty high frequencies, the actual bypass capacitors become more important. >> Putting a GND plane there instead will waste more space with >> no gain (as you still need to route the power signals somewhere) >> and putting no plane in that layer will result in a bent board. > Indeed, you need to put the powers somewhere. I recommend routing them > all on a couple of dedicated layers away from signal traces. On an FPGA > with at least 1.2V, 1.8V, 2.5V and 3.3V rails, which of these are you > suggesting will be on a plane? All of them? > (Again, the bent board thing is a fallacy, I have found.) >> Also, adjacent power planes provide multi GHz decoupling that is next >> to impossible to achieve with soldered capacitors. > We've been here before. It has a small amount of capacitance, which > doesn't help you because the multi-GHz can't get up the vias and balls > into the dice. Think of it this way, the reason a soldered capacitor > doesn't give you multi-GHz is the fact that you have to connect to it. > Actually in the ceramic of the cap is multi-GHz. It's the same with > connecting your chips to a adjacent-plane-made capacitor. Pin inductance is significant, and there isn't anything you can do about that on the board. Getting a reasonably low impedance to the pin is the best you can do, and that is still worth doing. > Of course, what this arrangement does also provide is the possibility of > multi-GHz resonances in your power planes. Lovely. Using a ground plane > where ever a reference plane is needed makes the SI design very simple > indeed. There was a question on a different post about the relative importance of noise on the ground vs. power pins. -- glen
From: Symon on 25 Mar 2010 21:26 On 3/25/2010 11:29 PM, glen herrmannsfeldt wrote: >> inductance. With two ground planes, a regular via is enough. > > As I understand it, that mostly isn't true. For a reasonably plane > there is enough capacitance around to get the signal across from > one to the other. > Enough? Care to fill in any numbers? :-) > > Note that a single wire has inductance, and a single plane has > capacitance. Even without another plane nearby, the capacitance > of a ground plane isn't so bad. With another plane nearby, though, > it is somewhat higher. At the higher frequencies, it is the plane > capacitance that you see. At lower, but still plenty high frequencies, > the actual bypass capacitors become more important. > A single plane, like one hand clapping, has a capacitance to the inside of a hollow infinite conducting sphere. As such, it is as much use here as a chocolate teapot. Everything has the same capacitance to the aether. The planet earth has a capacitance of nearly a millifarad. Perhaps I should connect my 3.3V supply to that? > > Pin inductance is significant, and there isn't anything you can do > about that on the board. Getting a reasonably low impedance to > the pin is the best you can do, and that is still worth doing. > No it isn't worth doing. I posted a spice cct showing that about a month ago. Please try it out yourself. >> Of course, what this arrangement does also provide is the possibility of >> multi-GHz resonances in your power planes. Lovely. Using a ground plane >> where ever a reference plane is needed makes the SI design very simple >> indeed. > > There was a question on a different post about the relative > importance of noise on the ground vs. power pins. > > -- glen Glen, I beg your pardon, but I wonder, do you design circuit boards for a living? I'd love to see one! :-) Cheers, Syms.
From: Symon on 25 Mar 2010 21:27 On 3/25/2010 8:26 PM, Thomas Entner wrote: > Thank you everyone for the comments, it is an very interesting > reading. I already got a lot of input for a new PCB-design, from > which we will do some variants to check which EMC-solution works best. > Looks like we need more variants than originally planned... > > Thomas Hi Thomas, Will you post back with the results of your testing? Thanks, Syms.
From: John_H on 25 Mar 2010 22:33 On Mar 25, 7:29 pm, glen herrmannsfeldt <g...(a)ugcs.caltech.edu> wrote: > > 2) When a signal trace passes from layer 1 to layer N-1, its reference > > plane has now changed. If this signal has a fast rise time, you have to > > use a bypass capacitor nearby, with its attendant inductance, and via > > inductance. With two ground planes, a regular via is enough. > > As I understand it, that mostly isn't true. For a reasonably plane > there is enough capacitance around to get the signal across from > one to the other. Not only no but hail no. The only way for the current to get from one side of the board to the other is through capacitors. The distributed capacitance within two very close planes as measured in units of picofarads per square inch is relatively miserable. There are exotic materials where an extremely thin prepreg with copper that's applied differently than normal so the "smooth" rolled sides face each other rather than the rough side. I don't know anyone that's used those materials. Move two planes many mils apart and the capacitance drops off. Have more than one plane between start and finish of the signal and you have multiple capacitors in series. That's a bad thing, right? Capacitors in series show significantly lower overall capacitance when compared to the individual caps. > Note that a single wire has inductance, and a single plane has > capacitance. Even without another plane nearby, the capacitance > of a ground plane isn't so bad. I'm sincerely wondering where you get your levels of magnitude for reference. Can you provide a picofarad per square inch value for the capacitance of a plane to earth ground? I know fully about self inductance but never in my days of electromagnetics graduate work was the concept of self-capacitance of a plane considered in my admittedly fading recollection. Capacitance needs two bodies. I can only assume the other body is earth ground in your description. For EMI and for crosstalk, the loop formed by the currents - forward and return - determine how much signal is "shared."
From: glen herrmannsfeldt on 26 Mar 2010 01:42
John_H <newsgroup(a)johnhandwork.com> wrote: (snip) > I'm sincerely wondering where you get your levels of magnitude for > reference. Can you provide a picofarad per square inch value for the > capacitance of a plane to earth ground? I know fully about self > inductance but never in my days of electromagnetics graduate work was > the concept of self-capacitance of a plane considered in my admittedly > fading recollection. Capacitance needs two bodies. I can only assume > the other body is earth ground in your description. It comes out easily if you do electrodynamics in CGS (gaussian) units. The unit of capacitance is the centimeter and, without trying too hard, you find that it is the capacitance of a sphere of the specified radius. Concider a concentric sphere capacitor in the limit that the outer sphere radius goes to infinity. The conversion factor to SI units is 4*pi*e0, or about 1.1 pF/cm. As with inductance, you can also do it though potential energy. 0.5*C*V**2 is the energy in a capacitor, which is equal to the energy in the electric field integrated over all space. (For ordinary capacitors, most of the energy is inside.) 0.5*C*V**2=0.5*epsilon*the integral over all space of E**2*dv (E is electric field, v is volume). > For EMI and for crosstalk, the loop formed by the currents - forward > and return - determine how much signal is "shared." Yes, including the effect of any capacitors in the circuit. -- glen |