At 11:13 AM 7/13/2006, Didier Fabbro wrote: >for "label attached" i want to say that a net with an assigned name is >connected to the pad >yes this is the air gap...i see the same thing with a gerber viewer >solder mask expansion is different just circular shape >power plane connect show air gap and you can deduct conductor width >gerbers aren't differents with gerber viewer like GCpreview
Okay, the gerbers show the pad as being clear from the plane. Just to be sure, the blowout clearance flash, the circular aperture which creates the plane clearance, should be larger than the *hole* in diameter by twice the plane clearance. (which also might be incorrect, by the way, it might be a special rule for the voltage, but in the end, if there is clearance on the gerbers, there should be clearance on the board). *Therefore* the problem is either a short *somewhere else* or a photoplot or manufacturing defect. If the manufacturer, for example, used the wrong aperture to photoplot the pads, there you go. Now, this raises one possibility. Protel 99SE, as I recall, had a problem with rotated thermal reliefs. They don't plot properly, they should never be used. But there should be no thermal relief involved here. There is something odd about what you wrote. It implies that the solder plane expansion looks different from the power plane connect A power plane expansion, to keep the pad from contacting the plane, will look exactly the same as a solder mask expansion, the only difference, possibly, would be the clearance. It would seem from the above that the power plane relief is *not* a circular flash. (Normally, Protel, as I recall, will plot circular clearances for non-connected holes, no matter what shape is used for the pad. If one were, for example, to merge the pads back into the photoplot, on the theory that having pads on the inner plane layers makes for better mechanical strength (maybe it does, but it also makes more opportunity for shorts), this could cause a short. What if the fabricator did this, and the pad was not round? Or was too large? Remember, the plane clearance is calculated from the *hole* size, not from the pad size. Protel assumes, for inner plane generation, that there is no pad if there is no connection. You also mentioned that "you can deduct conductor width." I do not understand what this means here. What conductor width? There has been no conductor mentioned that is in the power plane, which is supposedly where the short is taking place. Power planes, including split planes, are no generated with "conductors" having a width. Rather, any line primitives placed on that layer are anti-copper, the "conductor" is what is left after being cut away with whatever is plotted. Thermal reliefs appear to have conductors, but what is actually plotted is the clearance, not the conducting spokes of the relief. And this pad supposedly is not connected, and therefore shouldn't have any thermal relief, it should have complete clearance. (But, also, thermal reliefs should never be used to connect what are essentially vias, not used to solder component pins, to inner planes, they should always be direct-connect, i.e., nothing is plotted at the hole location at all, so it connects fully to the plane.) I know English is difficult for you, but it would be useful if you write as much as you can, there is no harm if you say more than the minimum, and it might reveal something about the situation. Explain what you mean when you write something like "the conductor width." what conductor, what width, where is is, why is it important, etc. You know, in trying to describe what you are doing more fully, you might actually come to realize what the problem is, problem-solving often works like that. (You are certainly doing better in English than I would do in French, or, indeed, in any other language!) ____________________________________________________________ You are subscribed to the PEDA discussion forum To Post messages: mailto:[email protected] Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/[email protected] Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/[email protected]
