Re: [PEDA] Gerber woes
Warning Unable to process data: multipart/mixed;boundary==_NextPart_000_0003_01C28709.AAB8FA20
Re: [PEDA] Gerber woes
Kulajew, I never use polygon pads and therefore I am not an expert but I can tell you that there are reported problems with polygon pad rotations (P99SE I assume). Abd-ul Rahman is the expert on this topic as I recall. Solution, do not use rotated polygon pads, possibly don't use polygon pads period. Hey Abd-ul Rahman, are you out there today? Kulajew needs your expertise on this topic! Sincerely, Brad Velander. Lead PCB Designer Norsat International Inc. Microwave Products Tel (604) 292-9089 (direct line) Fax (604) 292-9010 email: [EMAIL PROTECTED] http://www.norsat.com Check out our fall promotion at www.norsat.com. Limited quantities. Sale ends December 24, 2002. Contact your Account Manager or call 1-800-NII-4LNB or email [EMAIL PROTECTED] -Original Message- From: Kulajew Waldemar [mailto:waldemar.kulajew;kuebler.com] Sent: Friday, November 08, 2002 6:25 AM To: ProtelForum (E-Mail) Subject: [PEDA] Gerber woes Hello all. Is there any GerberGURU out there? I got a call from my board house just some minutes ago. They tells me the extended gerber file I send them is buggy. There seam to be an octagonal pad showing up rotated with 22,5 degrees. That, naturally, causes shorts to the surrounding Polygon. In fact it seams to be in the extended gerber file itself. Caused by the line %ADD34P,0.063X8X0*% in the header,. So here is my question: has anybody out there heard about a similar behavior? And is there a workaround? Yes I know one: do not use octagnal pads. ;-) But is there an other? Just wanted to push up the traffic on PEDA-forum before I jump into my weekend. ;-) Any advice appreciate when I comme back to fight with the Problems on Monday morning. Cheers, Waldemar * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:proteledaforum;techservinc.com * * To leave this list visit: * http://www.techservinc.com/protelusers/leave.html * * Contact the list manager: * mailto:ForumAdministrator;TechServInc.com * * Forum Guidelines Rules: * http://www.techservinc.com/protelusers/forumrules.html * * Browse or Search previous postings: * http://www.mail-archive.com/proteledaforum;techservinc.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] Gerber woes
This is a well known Protel bug. Octagonal pads are off by 22.5 degrees of rotation in Gerber files. The choices are: 1) Don't use octagonal pads 2) Have your board house fix your Gerber files by rotating all octagonal pads 22.5 degrees. 3) Do the fix yourself using a Gerber editor. John Williams - Original Message - From: Kulajew Waldemar [EMAIL PROTECTED] To: ProtelForum (E-Mail) [EMAIL PROTECTED] Sent: Friday, November 08, 2002 6:24 AM Subject: [PEDA] Gerber woes Hello all. Is there any GerberGURU out there? I got a call from my board house just some minutes ago. They tells me the extended gerber file I send them is buggy. There seam to be an octagonal pad showing up rotated with 22,5 degrees. That, naturally, causes shorts to the surrounding Polygon. In fact it seams to be in the extended gerber file itself. Caused by the line %ADD34P,0.063X8X0*% in the header,. So here is my question: has anybody out there heard about a similar behavior? And is there a workaround? Yes I know one: do not use octagnal pads. ;-) But is there an other? Just wanted to push up the traffic on PEDA-forum before I jump into my weekend. ;-) Any advice appreciate when I comme back to fight with the Problems on Monday morning. Cheers, Waldemar * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:proteledaforum;techservinc.com * * To leave this list visit: * http://www.techservinc.com/protelusers/leave.html * * Contact the list manager: * mailto:ForumAdministrator;TechServInc.com * * Forum Guidelines Rules: * http://www.techservinc.com/protelusers/forumrules.html * * Browse or Search previous postings: * http://www.mail-archive.com/proteledaforum;techservinc.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] Gerber woes
I got caught out on this myself, so I downloaded a gerber spec from the web somewhere. Specifically, the line means: %ADAperture description D34Name of the aperture P, It's a regular polygon 0.063X Size of the polygon 8X It's has 8 sides 0 NOT rotated *% End of description The printout I have suggests that for no rotation, do not use the rotation parameter. IMHO it sounds like the manufacturer's interpretation of the gerber data is not correct. Kiernan F Quoting Kulajew Waldemar [EMAIL PROTECTED]: Hello all. Is there any GerberGURU out there? I got a call from my board house just some minutes ago. They tells me the extended gerber file I send them is buggy. There seam to be an octagonal pad showing up rotated with 22,5 degrees. That, naturally, causes shorts to the surrounding Polygon. In fact it seams to be in the extended gerber file itself. Caused by the line %ADD34P,0.063X8X0*% in the header,. So here is my question: has anybody out there heard about a similar behavior? And is there a workaround? Yes I know one: do not use octagnal pads. ;-) But is there an other? Just wanted to push up the traffic on PEDA-forum before I jump into my weekend. ;-) Any advice appreciate when I comme back to fight with the Problems on Monday morning. Cheers, Waldemar * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:proteledaforum;techservinc.com * * To leave this list visit: * http://www.techservinc.com/protelusers/leave.html * * Contact the list manager: * mailto:ForumAdministrator;TechServInc.com * * Forum Guidelines Rules: * http://www.techservinc.com/protelusers/forumrules.html * * Browse or Search previous postings: * http://www.mail-archive.com/proteledaforum;techservinc.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] Gerber woes
At 04:51 PM 11/8/2002 +, [EMAIL PROTECTED] wrote: The printout I have suggests that for no rotation, do not use the rotation parameter. IMHO it sounds like the manufacturer's interpretation of the gerber data is not correct. Based on my recollection: That is the same error that Protel made, probably based on the same incorrect assumption. If you download the complete RS-274X specification, you will discover that zero rotation means that a point of the polygon is on the y-axis. This might have been a bad decision on the part of those who wrote the spec, since 99% of the uses of this shape (as an octagon) would have the flats orthagonal to the x and y axes. The manufacturer is following the specification as carefully intepreted without making the assumption that zero rotation for an octagon gives you the same thing as a non-rotated square but with the corners chamfered. I do understand why they made the decision, though. For polygons with an odd number of vertices, normal-to-the-flats would be weird. At the very least, the specification should have been much more explicit! * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:proteledaforum;techservinc.com * * To leave this list visit: * http://www.techservinc.com/protelusers/leave.html * * Contact the list manager: * mailto:ForumAdministrator;TechServInc.com * * Forum Guidelines Rules: * http://www.techservinc.com/protelusers/forumrules.html * * Browse or Search previous postings: * http://www.mail-archive.com/proteledaforum;techservinc.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
