There have been a lot of good comments given by all. I would like to add a few more points: 1. It has been established that routing single ended signal under copper fill can cause signal integrity problems on the single ended signal or half wave resonances on the copper patch. But there seems to be a belief that it is ok for differential signals to go under copper fill areas. We know that it is bad to route signals across a plane cut. It is not as severe a problem if a differential pair is routed across a plane cut, *as long as the cut is small compared to the signal rise time*. But if the cut is wide compared to the signal rise-time, reflections will occur due to impedance mismatches. The same is true with copper fills. If the fill is large compared to the signal rise time, even differential signals will have reflections when they are routed under the copper fill. 2. A few people mentioned that these copper patches should be made small to avoid resonances under these patches, which may cause emi problems (or even signal integrity problems if the resonance is coupled onto sensitive analog circuits nearby). This is true. But another point to watch out for is that these patches should be placed with adequate spacing from each other. Otherwise, at high enough frequency, the wave energy will couple from one patch onto the next patch and propagate down the board. This defeats the purpose of keeping the patches small. What I would do is to space the patches (or dots) with 4 times the dielectric height. If the top layer dielectric is 5 mils thick, then the patch spacing should be 20 mils apart. This ensures that the patches are better coupled to the plane layer below than to the adjacent patch. 3. I would not recommend adding vias to tie these patches/dots to ground. If you have a board running at 3Gbps, one tenth of the wavelength of the 5th harmonic is about 80 mils in FR4. I would make the patches in the size between 60 to 80 mils diameter. This would require the fab house to place hundreds or thousands of patches. Adding that many vias to a board not only increases the cost of the board but also increases the chance of power planes shorting out if a via is drilled off center and the power plane antipad is not large enough. In some cases, the short does not occur immediately. But due to small cracks in FR4 and moisture content in the material as electrolyte, copper atoms can migrate through the crack to cause shorts later on. This is simply not a good idea. 4. Some mentioned about using the copper fill as a shield for electromagnetic waves. This will work only if the fill is designed as a faraday cage with vias closely stitched and no part of the circuit penetrates the cage unless careful filtering is done on the circuits that penetrate the cage. Otherwise, it will not work. 5. Some also mentioned that the copper fill can be used to terminate electromagnetic waves to reduce emi emission. This idea rarely works. We know that a signal on a transmissionline can be terminated by a matched impedance load. A copper fill with vias tied to ground has an impedance varying with frequency. This is a resonating structure at best. EMI emissions from digital circuits occur at multiple frequencies, and these frequencies can drift with temperature and / or change due to manufacturing tolerances of discrete components (capacitors). Using a resonating structure for impedance matching at multiple frequencies that may drift with temperature is a task that few have even attempted. And even fewer have succeeded. 6. Another person suggested using the copper fill to add parasitic capacitance to lower the impedance of the board. This can work only if this fill is placed near the circuit of interest. At low frequency, the whole board behaves as a capacitor. This copper fill may help, but so do discrete capacitors. At high frequency, the board behaves as a resonating structure, adding capacitance a quarter wavelength away only creates more reflections and/or shifts the resonance frequency of another circuit. Adding copper fill randomly can create problems in some cases. George George Tang LSI Logic ------------------------------------------------------------------ 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 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