Just so we all understand each other, I'll review the assumptions that should apply here. *Boards can be made with mixed copper thicknesses. This is no big deal. *Only the power and ground planes "need" 2 oz copper, though this might be overkill. *Even if 2 oz cu is used for power distribution, the signal layers should still be sized for fine pitch, 1 oz or less (unless we are talking about some heavy duty power signals, in which case the fine pitch concept does not apply anyway). *If you do design with mixed layer thicknesses, warpage is a problem if the stackup is asymmetric. *If the thicker layers are the two middle layers or the two outer layers, as an example, then the board is symmetric and the board is not more prone to warp than a board without mixed thicknesses. The tendency to warp is not a cliff edge effect, which is to say that a small amount of deviation from perfectly symmetric means only a small amount of warp tendency, a lot means a lot. *Multilayer boards can have an even or odd number of layers, but the actual board is built by laminating thin, double sided boards together with prepreg in between. An odd layer count simply makes one of these single sided. Go for an even layer number and the "extra" layer is almost free. *As a matter of wisdom, the stackup should be designed so that the thicker layers are paired on the same double sided component. Layer pairs with the same cu thickness on both sides is ordinary. Ask for a different weight on each side and the fabricator sees dollar signs floating in the air. *Also be aware that fabricators might add copper to layers in open areas to keep the board the same nominal height over the entire surface. These floating pieces of copper can be a constant impedance or stray coupling issue, so be sure to specify where this should not be done. One thing I recommend for any engineer involved in multilayer design is a tour of a PWB fabricator. This is usually just a matter of a phone call and a few well spent hours. See the steps with your own eyes, ask about all the points just made and any others you can think of, and design your boards to fit the process. Ask what space and trace their particular process supports without a big kink in the cost curve. There are process variations that might apply. It's that or wonder why the price of different designs keeps jumping around, and problems like yield, warpage, or worse keep happening. OK, experts, time to add your 2 cents. Orin Laney On Thu, 19 Jul 2007 06:33:35 -0400 (EDT) Stuart Brorson <sdb@xxxxxxxxxx> writes: > Andrew, > > Thanks for your answer. Your points make sense. The point is that > 2 > oz Cu is inappropriate for fine-pitch boards, particularly for large > boards where the final feature size might vary over the > board's surface due to non-uniform etch rates. Right? > > Is there a rule of thumb, like trace/space = 10/10 => OK for 2oz Cu, > but 5/5 => not OK? A similar rule for 1oz Cu? > > Cheers, > > Stuart > > > > On Wed, 18 Jul 2007, Andrew W. Riley III wrote: > > > Stuart, > > > > I do not see board warpage being a factor unless there are extreme > > differences in copper layers of the PCB, or the fab house is not > reputable. > > > > Coming from the layout side, I have only had complaints from fab > houses WRT > > tolerances and extended reliability at 2oz routing layers. At > that time it > > was the customer's request and I was able to talk them down with > facts > > supplied or easily researched and sometimes a conference call that > included > > an engineer specialized in signal integrity with reliable > simulation tools. > > > > In an attempt to make this reply short, my experience has been > that > > increasing copper weight was not a favorable consideration in > those designs. > > Having the backup of an experienced and proven signal integrity > expert on > > call was a factor. > > > > Sometimes you gotta bite the bullet and let the powers that be > know it's not > > gonna be free. > > > > Cheers! > > Drew ------------------------------------------------------------------ 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