thanks Gisbert,
that was the info i was seeking and it sounds like it would have caught
this error
actually there was a tiny connection path, the voiding track or fill
covered most but not all of the via
so the remaining connection was probably not able to be etched, but i
wonder if the program would still see it as a valid connection ?
Dennis Saputelli
_______________________________________________________________________
Integrated Controls, Inc. Tel: 415-647-0480 EXT 107
2851 21st Street Fax: 415-647-3003
San Francisco, CA 94110 www.integratedcontrolsinc.com
[EMAIL PROTECTED] wrote:
I don't know your particular design, but P2004 flags an error if you cover
plane connections with polygons or fills, or split plane intersections.
A real improvement compared tp 99SE!
Mit freundlichem Gruß
Kind regards
Gisbert Auge
N.A.T. GmbH
www.nateurope.com
i think maybe i asked this before but did not get an answer ...
i recently made a mistake (first one ever)
i 'improved' a working design on a rev spin by slightly increasing power
plane voids under 1.4GHz signal traces and input filters
i did not catch that the void (primitives on power planes) intersected a
tiny via tagged on the side of an 0603 resistor and thus spoiled the gnd
connection to the resistor (actually a tiny bit appeared to connect but
was probably not fabricate-able)
as is well known the 99SE DRC does not flag this other than a
generalized warning to which i am now well immune since i always have
primitives on all planes
upon explaining this to my associate he was amazed that such an
important DRC function was missing from protel since he said that PADs
has had that for many many years including something about 'amount of
copper connection' which part i did not quite catch **
so the question is, does DXP/Protel 2004 finally address this critical
need ?
ds
**
a bit more blather along the sames lines ...
on this same board there is an area where i have ground 'cuts'
(not 'splits', but rather traces on the planes to localize circulating
currents)
i noticed (in time in this case) that there was an area which had very
limited plane continuity remaining after the late addition of a mounting
hole near a 'cut' in the plane
so even if protel had a negative continuity plane check, this would have
passed but would have been a crappy situation
the PADs 'minimum amount of copper' DRC implied by my friend would have
flagged such a situation
does Protel 2004 address this ? or are there plans to ?
would this also apply to the situation of a rounded track end just
barely grazing the edge of a pad which passes protel continuity but
would probably fab as a break?
_______________________________________________________________________
Integrated Controls, Inc. Tel: 415-647-0480 EXT 107
2851 21st Street Fax: 415-647-3003
San Francisco, CA 94110 www.integratedcontrolsinc.com
Brad Velander wrote:
Leo,
Yes I have seen this issue as well, wrecked a board or two over
the years. It is some bug that seems to be particular to specific detailed
geometries in a poured polygon area. I am assuming that you have a polygon
where this shows up, it has always been such on my designs. It may effect
planes under certain circumstances but I have never seen it there because I
barely ever use true planes.
The only fix that I have found is to tweak the polygon outline
slightly in the area effected. Move the polygon vertices by some small
amount and then repour. It seems to usually occur near a vertice for the
polygon outline or where you have a vertice for a cutout or clearance area
(watch for small tight acute angles on the polygon pour outline, cutout or
just how the polygon has poured with the clearance rule). So moving the
polygon or a cutout vertice just slightly (+/-5mils - +/- 50mils) seems to
fix it. You may have to try a couple of different vertice moves until the
Gerber comes out correct. Another option is to vary the clearance (even as
little as +/-1 mil) for that polygon as well so that the actual poured
polygon edges have been moved slightly.
Sincerely,
Brad Velander
Senior PCB Designer
Northern Airborne Technology
#14 - 1925 Kirschner Road,
Kelowna, BC, V1Y 4N7.
tel (250) 763-2329 ext. 225
fax (250) 762-3374
-----Original Message-----
From: Leo Potjewijd [mailto:[EMAIL PROTECTED]
Sent: Monday, September 19, 2005 5:31 AM
To: [email protected]
Subject: [PEDA] arcs in Gerber go the wrong way
On the PCB (P99SE) all my arcs look great, even on the print preview.
But in the Gerber files some, not all, are wrong: the start and end in
the
right places, but go the wrong way around. So a 90 degree turn ends up as
a
270 degree turn with another center and shorts stuff......
It happened once before, but the fab house detected and reported that
error
so they could correct it in time.
Like now, I could not identify the source of the problem and have no clue
whatsoever....
I checked the PCB at ASCII level but could not find any indications what
went wrong (a 'good' one looks exactly the same as a 'wrong' one). I even
generated the Gerbers from that copy: no luck.
Inside the Gerbers I am at a loss: I cannot identify arcs, let alone the
right and wrong ones.
Has anyone seen this before and found a solution or workaround?
Checking the 'software arcs' box is not an option: that messes up the
already tight clearances (had a close shave with that one, too).....
Leo Potjewijd
hardware designer
Integrated Engineering B.V.
[EMAIL PROTECTED]
+31 20 4620700
____________________________________________________________
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]
