Bob and others, Planes do act as caps.... especially at frequencies where the normal decoupling caps already behave like inductors. There's no way to do proper power supply decoupling above let's say 200MHz with traditional caps. Lower the distance between power and ground. I know, lot fo people are using caps in the picofarad range for very high speed decoupling. With a distance between power and ground of about 100um you can save all this caps. You still need low and medium frequency decoupling caps in the uF and nF range. A final trick is to mix the base material between power and ground with some kind of ferrite. The ferrite will not come apparent at low frequnecies, but at higher frequencies the losses in the ferrite rise dramatically and destroy all of the RF energy. Great method, but it isn't cheap. BTW, you always need resistance to remove energy. I.e. it's the ESR of the decoupling caps that makes EMI disappear. So using NPO caps is no good for decoupling. Z5U is just bad enough. Decoupling is a science (and probably religion) of it's own. regards, Peter Marek Peter Marek MarekMicro GmbH General Director Phone + 49 - 9661 - 908-210 Fax + 49 - 9661 - 908-100 E-Mail [log in to unmask] -----Ursprungliche Nachricht----- Von: Bob Landman [SMTP:[log in to unmask]] Gesendet am: Freitag, 23. Juli 1999 02:50 An: [log in to unmask] Betreff: Re: [DC] Stackup assignment for pcb boards. Jack, Brooks wrote recently about planes acting as caps - they do not. If you do the math you will see why. 0.1uF takes a LOT of parallel copper separated by that much glass-epoxy (distance reduced the capacitance). In a 0.1uF the separation is the oxide layer on the aluminum foil. Much as we don't like them, every single power pin MUST be bypassed by 0.1uF caps - if a large chip like a BGA or PLCC has say 4 power pins - bypass them ALL or pay the piper. Bypass is a misnomer - what they mostly do is stiffen the power rail and act as small local power sources until the power supply inches away can replace the charge in the caps. Bob Landman H&L ----- Original Message ----- From: Jack Olson <[log in to unmask]> To: <[log in to unmask]> Sent: July 22, 1999 4:51 PM Subject: Re: [DC] Stackup assignment for pcb boards. >From my experience: 1) If a designer can get away with using ? ounce copper he should, because it is easier to etch and control trace widths. The only reason to use thicker copper on internal layers would be so that the same trace width can handle more current. Internal traces need way more copper to handle the same thermal rise than external traces, but if current isn't an issue I don't think there is a reason for one ounce. 2) A small dielectric thickness between power and ground will increase capacitance, so in effect the planes coupled together act as one big cap. Maybe some decoupling caps can be removed? 3) I only specify material thicknesses for impedance controlled boards. For example, we do lots of 100 ohm differential pairs that need 5mil or 6mil cores, but the rest we don't exactly care about. Don't constrain the vendor without a reason, in my opinion. Jack -----Original Message----- From: Eileen Ong [R&D] [mailto:[log in to unmask]] Sent: Wednesday, July 21, 1999 1:57 AM Subject: Stackup assignment for pcb boards. I have seen different specification given to pcb house for pcb fabrication. What is the guidelines regarding the thickness of copper for different layers for best performance and cost effective. 1) For example for a 2/4 layer pcb,examples of some of the spec. are : 2 layer pcb : a) FR4 material with 1/2 oz copper b) FR4 material with 1oz copper 4 layer pcb : c) FR4 material with 1oz copper in all layers d) 1/2oz copper clad FR4 plate up 1oz, inner layer use 1oz Any differences between a) & b) or c) & d) ? 2) I have read from "somewhere" that it is better to use smallest distance spacing between power & ground plane in the inner layer for lowest power impedance. What is this smallest distance ? 3) How about core and prepreg, do you'll usually specify their thickness also ? Thanks in advance for all contributions given. Best Regards, EILEEN ONG (R&D Dept.) Paradise Innovations (Asia) Pte Ltd Email : mailto:[log in to unmask] Web: http://www.paradisemmp.com