Re: [PEDA] Gerber problem
Don, Sorry, finally got to your own post seeing you discovered the problem, was what I answered. Bob Wolfe - Original Message - From: "Don Mayfield" <[EMAIL PROTECTED]> To: "Protel EDA Forum" <[EMAIL PROTECTED]> Sent: Monday, December 09, 2002 10:40 PM Subject: [PEDA] Gerber problem > Dear All, > > I have a problem generating gerber files for my 5 layer board. I get a > whole lot of 0 mil holes > reported when I look at the gerber files however there are none on the > board apart from surface > mount parts which don't usually get reported. Strange thing is that when > I change something > the holes reported as 0 mil move around the board. Anyone seen this? > More importantly, anyone > know what causes it? Any help would be greatly appreciated. > > Cheers, > > -- > Don Mayfield > Anglo-Australian Observatory > 167 Vimiera Rd > Eastwood > NSW 2122 > Australia > Ph. 61-2-9372-4836 > Fax. 61-2-9372-4880 > > > > * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] Gerber problem
Don, I did not read all responses, but like the ones I did read is it gerber or drill data that is giving info. If gerber the other item that I don't think was mentioned is the fact that using symbols for drill dwg, there are only 12 or 16 of those symbols default, and when you run the GERBER output for the drill legend ALL holes sizes beyond the 12/16 you have available will be added up and show as Zero as size. Same for alphabet at 26. So that could be it too. But the other data like NC Drill File will be correct, but the two of course will not match now. Bob Wolfe - Original Message - From: "Don Mayfield" <[EMAIL PROTECTED]> To: "Protel EDA Forum" <[EMAIL PROTECTED]> Sent: Monday, December 09, 2002 10:40 PM Subject: [PEDA] Gerber problem > Dear All, > > I have a problem generating gerber files for my 5 layer board. I get a > whole lot of 0 mil holes > reported when I look at the gerber files however there are none on the > board apart from surface > mount parts which don't usually get reported. Strange thing is that when > I change something > the holes reported as 0 mil move around the board. Anyone seen this? > More importantly, anyone > know what causes it? Any help would be greatly appreciated. > > Cheers, > > -- > Don Mayfield > Anglo-Australian Observatory > 167 Vimiera Rd > Eastwood > NSW 2122 > Australia > Ph. 61-2-9372-4836 > Fax. 61-2-9372-4880 > > > > * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] Gerber problem
Hi All, The problem turned out to be an old one - the number of holes sizes was greater than 15. More than 15 will work if one changes the legend to use characters instead of symbols. I usually reduce the number of holes sizes used on a board and so never actually encountered the problem until now. Thanks to all who offered help, Don. Brad Velander wrote: Don, as Brian had suggested, it would be very helpful if you could describe how you are having these 0 mil holes reported to you. You say that you can't see anything when looking at the Gerbers, not unexpected, how would you see something that is non existent? Do these 0 mil holes appear in your .DRR report? Are they in the .txt drill file? If they appear in these files then it sounds like Steve had the right idea. I have never heard of such a thing but have seen lots of 0mil arcs in Gerber generated by Protel. Seems they are generated when using the arc routing tools. 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: Don Mayfield [mailto:[EMAIL PROTECTED]] Sent: Monday, December 09, 2002 7:41 PM To: Protel EDA Forum Subject: [PEDA] Gerber problem Dear All, I have a problem generating gerber files for my 5 layer board. I get a whole lot of 0 mil holes reported when I look at the gerber files however there are none on the board apart from surface mount parts which don't usually get reported. Strange thing is that when I change something the holes reported as 0 mil move around the board. Anyone seen this? More importantly, anyone know what causes it? Any help would be greatly appreciated. Cheers, -- Don Mayfield -- Don Mayfield Anglo-Australian Observatory 167 Vimiera Rd Eastwood NSW 2122 Australia Ph. 61-2-9372-4836 Fax. 61-2-9372-4880 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] Gerber problem
Don, as Brian had suggested, it would be very helpful if you could describe how you are having these 0 mil holes reported to you. You say that you can't see anything when looking at the Gerbers, not unexpected, how would you see something that is non existent? Do these 0 mil holes appear in your .DRR report? Are they in the .txt drill file? If they appear in these files then it sounds like Steve had the right idea. I have never heard of such a thing but have seen lots of 0mil arcs in Gerber generated by Protel. Seems they are generated when using the arc routing tools. 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: Don Mayfield [mailto:[EMAIL PROTECTED]] > Sent: Monday, December 09, 2002 7:41 PM > To: Protel EDA Forum > Subject: [PEDA] Gerber problem > > > Dear All, > > I have a problem generating gerber files for my 5 layer > board. I get a > whole lot of 0 mil holes > reported when I look at the gerber files however there are > none on the > board apart from surface > mount parts which don't usually get reported. Strange thing > is that when > I change something > the holes reported as 0 mil move around the board. Anyone seen this? > More importantly, anyone > know what causes it? Any help would be greatly appreciated. > > Cheers, > > -- > Don Mayfield * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] Gerber problem
Don off to the side of your design place a pad , change it 0 mils, select it then globally select all the same, then delete them all if then at once, regenerate gerber files Mike - Original Message - From: Don Mayfield <[EMAIL PROTECTED]> To: Protel EDA Forum <[EMAIL PROTECTED]> Sent: Monday, December 09, 2002 10:40 PM Subject: [PEDA] Gerber problem > Dear All, > > I have a problem generating gerber files for my 5 layer board. I get a > whole lot of 0 mil holes > reported when I look at the gerber files however there are none on the > board apart from surface > mount parts which don't usually get reported. Strange thing is that when > I change something > the holes reported as 0 mil move around the board. Anyone seen this? > More importantly, anyone > know what causes it? Any help would be greatly appreciated. > > Cheers, > > -- > Don Mayfield > Anglo-Australian Observatory > 167 Vimiera Rd > Eastwood > NSW 2122 > Australia > Ph. 61-2-9372-4836 > Fax. 61-2-9372-4880 > > > * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] Gerber problem
In a message dated 12/9/2002 10:49:23 PM Eastern Standard Time, [EMAIL PROTECTED] writes: > I have a problem generating gerber files for my 5 layer board. I get a > whole lot of 0 mil holes > reported when I look at the gerber files however there are none on the > board apart from surface > mount parts which don't usually get reported. Strange thing is that when > I change something > the holes reported as 0 mil move around the board. Anyone seen this? > More importantly, anyone > know what causes it? Any help would be greatly appreciated. > > It sounds like you might have some pads set to Multilayer with a 0 mil hole diameter. I believe it's the layer selection, not the hole diameter, which determines whether or not the pad shows up in the drill file. Steve Hendrix * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] Gerber problem
Is it the Drill Report that's telling you about the holes? Or the DRC? What does the Hole Size Editor Tool list as holes? Anything odd? Can you locate a zero sized hole on the board from data in the Text Drill File? One thing to try is to select all zero holes and attempt a global change to, say, 100mil; that can help you to visualize what's going on. (Of course, you'll have to deselect SMD pads and other "good" zero-holes.) It may be that you somehow wound up with zero diameter holes on a mechanical or drill drawing or keepout layer. I think the drill generator will output data for any holes on all layers, whether they are visible or not. Make sure All Used Layers are turned on for display. Try to repair the database using the tool under the green "down arrow" in the upper left of the toolbar area. You have to close the .ddb before you can repair it. Good luck * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
[PEDA] Gerber problem
Dear All, I have a problem generating gerber files for my 5 layer board. I get a whole lot of 0 mil holes reported when I look at the gerber files however there are none on the board apart from surface mount parts which don't usually get reported. Strange thing is that when I change something the holes reported as 0 mil move around the board. Anyone seen this? More importantly, anyone know what causes it? Any help would be greatly appreciated. Cheers, -- Don Mayfield Anglo-Australian Observatory 167 Vimiera Rd Eastwood NSW 2122 Australia Ph. 61-2-9372-4836 Fax. 61-2-9372-4880 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
