On 10:56 AM 29/06/2001 +0100, Jason Morgan said:
>Methinks I've found a bug in Protel, can someone confirm?
>
>We want SMT top layer pads with no solder pasted, i.e. no hole in the paste
>mask.
>
>So under pad, paste mask expansion we put -3mm (pads are 1mm wide x 2mm
>tall).
-0.5mm should be enough (but see below), in your case, as the expansion is
applied all around the edge; a negative expansion is an inwards expansion
(if that makes sense) so only need be half the minimum dimension of the
pad. That said Protel should be smart enough to ignore zero (or negative)
sized apertures. (I seem to recall an old bug in which negative apts could
get into the apt list - maybe I recall incorrectly).
>In pcb and when importing Gerber to check the data, the solder paste mask
>shows no
>paste - CORRECT.
Yep - I tired your test and this is what I see as well.
>However, our PCB house says that there are apertures 5.000mil x 0.000mil
>(Yes ZERO).
I do not get this (P99SE SP6). There are no apts with a zero dimension in
the gerbers I am getting. I did try to replicate your situation as best I
understood it. *But* if I tried a paste mask expansion of -0.5mm, just
enough to close the paste mask, I did see a apt in the file with a 0
dimension. making the expansion -0.51mm removed the apt from the gerbers
files.
So, what I can see is that there is a bug in that Protel does not remove
from the apt list apts with a zero dimension. I assume that there is a
mils to mm conversion round-off error that then gets truncated in the
conversion to the specified gerber apt format. Or something like
that. The gerber write code should filter from the gerber files any post
gerber-formatted apts with a zero dimension.
Rule: specify an expansion slightly over that required to just close over
the pad.
It is interesting that even with the zero-dimensioned apt in the apt list
the draft code does not seem to be used. Making the expansion -0.49mm does
add a flash to the paste mask gerber file.
Now why you see the odd apt in the files when you specify a larger than
necessary negative expansion makes me wonder if there is not something else
up with your file (or there is a mis-print in your email, but I doubt
that). Have you any further info?
>Oddly enough, 5mil is the gap between the two pads (being used for solder
>blob jumper).
>
>It seems that the Gerber aperture generator is messing up.
>
>We have an external Gerber viewer and this confirms the same, in fact
>showing the erroneous apertures
>as odd shaped rectangles, just as the PCB house found.
>
>Jason Morgan - Development Engineer
>CITEL Technologies Ltd.
Any chance of sending the file (zipped and as small as possible) direct
(not to the list) to allow another eye to study. This does sound odd and I
am always very worried about gerber issues - I was there in the early
Protel windows versions with many gerber bugs, the emotional scars have
never quite left me.
I must say, Jason, that you seem to have no end of trouble with Protel. I
feel for you. From memory you have had file corruptions, enormous
(ridiculous!) edit times for some boards, and now this.
I wonder if Premier are giving you the support you deserve?
Bye for now,
Ian Wilson
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
*
* To leave this list visit:
* http://www.techservinc.com/protelusers/leave.html
* - or email -
* mailto:[EMAIL PROTECTED]?body=leave%20proteledaforum
*
* Contact the list manager:
* mailto:[EMAIL PROTECTED]
*
* Browse or Search previous postings:
* http://www.mail-archive.com/[email protected]
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
