[PEDA] pb short-circuit beetwen pad and internal plane with protel 99se

[Abd ul-Rahman Lomax]

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!)