Andrew

The rotation is almost certainly as you describe and one can only assume 
that 0 is upright (+) and 45 is a cross (X). I can understand why GCPREVU 
and others might not like the inside and outside diameters to be equal, but 
in any event, a directly embedded pad (via?) shouldnt need any pad on the 
gerber output for the plane layer at all, it only needs a plated through 
hole, so that bit is probably a gerber generation bug.

In your new version below, D193 looks healthy and D194 looks sick still. 
What you should do is find a line which says D194* further down the gerber 
file (ie some use of the D194 aperture) and then look at some of the X,Y 
coordinates that follow it, then locate the offending pads (vias) on the pcb 
and work backwards. It might be a rule conflict or simply a corrupted 
database object eg. a via assigned to an invalid layer pair etc.


Doug



>That's very helpful. Let me pitch this to you...
>
>I'd say the 0 width cross hair means, as you say, a direct connection
>(merge) into the plane. I'd say 45 degree rotation determines whether
>the cross-hair is + (90 degrees) or X (45 degrees).
>
>I think the reason this doesn't work is that the inside and outside
>diameters overlap, and the cross hair is zero.
>
>Owing to repeated re-generation of Gerbers (and some tweaking in
>between) I know have a file with the following two aperature macros:
>
>%AMTHD193*
>7,0,0,2.800,2.300,0.250,45*
>%
>%ADD193THD193*%
>%AMTHD194*
>7,0,0,2.016,2.016,0.000,45*
>%
>
>So D193 works (it's 2.8-2.3 = 0.5mm), but D194 doesn't work because the
>line is 0mm thick with 0mm crosshair.
>
>I think I understand now why the aperatures aren't being read by GCPREVU
>and my board house. So, what is Protel doing? Have I set up two
>contradictory rules - if so, why does it appear ok in the PCB editor,
>and why do Gerbers imported into Protel appear ok?


_________________________________________________________________
Join the world s largest e-mail service with MSN Hotmail. 
http://www.hotmail.com


* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
*
* To leave this list visit:
* http://www.techservinc.com/protelusers/leave.html
*
* Contact the list manager:
* mailto:[EMAIL PROTECTED]
*
* Forum Guidelines Rules:
* http://www.techservinc.com/protelusers/forumrules.html
*
* Browse or Search previous postings:
* http://www.mail-archive.com/proteledaforum@techservinc.com
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

Reply via email to