Hi, I've thought for years that there ought to be some kind of fairly standard crosstalk coupon that the PCB mfg can test similar to the widely-used impedance coupons. Every time I've brought it up, it seem that the expertise on the production floor at the PCB mfg doesn't quite exist. Is anybody regularly doing this? -Eric Lee Ritchey wrote: Istvan, I agree with your approach. Good fabricators expect things to work this way. Lee [Original Message] From: Istvan Nagy <buenos@xxxxxxxxxxx>[1] To: <codymiller@xxxxxxxxxx>[2]; <si-list@xxxxxxxxxxxxx>[3] Date: 12/10/2008 10:42:49 AM Subject: [SI-LIST] Re: Designing PCB Stackups hi most of the people advices to not to specify exact material types, leave this decision for the production people, based oneveryday actual pricing and stock info. this way its cheapest to manufacture, and the lead times are shortest. this is typical in the industry. i dont advice this, because: crosstalk. if a production technician adjusts layer thicknesses (chosing a different material) they can make the original impedance values on the board, requested by the designer company, but the crosstalk levels will change. this is something what a PCB manufacturer and any of their employees can not understand, just a HW design engineer or a signal integrity engineer. we had a processorboard, where the manufacturer changed a dielectric layer from 50um to 75um, then the impedances were correct, but the crosstalk levels (simulated) increased by aroud 50%. what i would do, is to chose a pcb manufacturer, send a rough stackup, ask if its ok for them or advice another stackup. then fix the materials, and use those forever for that board, in its lifetime. managers and purchasing people wouldnt like it, but thats the only way to have not just controleld impedance, but controlled crosstalk levels as well. a common misunderstanding in the industry, is that a lot of people specify trace-to-trace clearances based on the trace width. (like d>2*w). it should be specified based on the dielectric thickness (like d>2*h). if you understand this, then its quite obvious why is it bad if the manufacturer specifies/changes the thicknesses during production. the best is if you calculate the impedances (you need a good field solver, like Polar-si8000 or MMTL...), and check the resulting trace widths and dielectric thicknesses, tosee if you can get good noise imunity and good circuit density on your board. the first methos worked well 15 years ago when people had 2 controlledimpedance traces on a PCB, and it was easy to maintain proper distance to other traces. if you check a DIMM memory module (you are from Micron, wright?), its full of controlled impedance traces, closely spaced because of the density. regards, Istvan Nagy Concurrent Technologies Plc, UK --- Links --- 1 mailto:buenos@xxxxxxxxxxx 2 mailto:codymiller@xxxxxxxxxx 3 mailto:si-list@xxxxxxxxxxxxx ------------------------------------------------------------------ To unsubscribe from si-list: si-list-request@xxxxxxxxxxxxx with 'unsubscribe' in the Subject field or to administer your membership from a web page, go to: //www.freelists.org/webpage/si-list For help: si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field List technical documents are available at: http://www.si-list.net List archives are viewable at: //www.freelists.org/archives/si-list or at our remote archives: http://groups.yahoo.com/group/si-list/messages Old (prior to June 6, 2001) list archives are viewable at: http://www.qsl.net/wb6tpu