[PEDA] Excellon Drill Files
Re: [PEDA] Excellon Drill Files
Hi Michael The drl-fire is binary it doesn't match with all viewers. Is the txt not over the gerber? Then you must play with the settings in gerber generating. In Gerber-Setup-Advanced you have options to relativ or absolute coordinats. Try it. Regards Wolfgang Geier * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] Excellon Drill Files
Watnoski, Michael wrote: Hi All, I have been trying to import Protel drill files into a Gerber viewer (ViewMate) for checking. The .drl file has not been able to be read properly, regardless of the settings used for generation. The .txt file displays, but not in the proper locations. It does not appear to be scaling issue relating to the selection of imperial or metric, or zero suppression.. Does anyone have any suggestions? The .drl file is a binary EIA format that almost no-one uses now. Most board shops will want the ASCII .txt file. The drill file is always generated using screen coordinates - if you have a hole at 1000, 1000 on the screen, it will be at 1000, 1000 in the drill file. When generating Gerbers, there is an option to Center plots on film which is checked by default - if that is checked, the coordinates in the Gerber files will be adjusted to place the board in the center of the plotter film. This will, of course, cause the drill file to not align with the Gerbers. Uncheck Center plots on film, regenerate the Gerbers, and everything should line up. -- Peter Bennett TRIUMF 4004 Wesbrook Mall, Vancouver, BC, Canada GPS and NMEA info and programs: http://vancouver-webpages.com/peter/index.html * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] Excellon Drill Files
Have you moved the origin of the PCB? I have found often run into disconnect between the gerber output and the drill output origin if the origin was changed using the EditOrigin Command. There is a reset command (EditOriginReset). Try resetting the origin and outputing all new files. The .txt file is probably the file you will want to use. Anthony W. -Original Message- From: Watnoski, Michael [mailto:[EMAIL PROTECTED]] Sent: Wednesday, November 14, 2001 11:13 AM To: '[EMAIL PROTECTED]' Subject: [PEDA] Excellon Drill Files Importance: High Hi All, I have been trying to import Protel drill files into a Gerber viewer (ViewMate) for checking. The .drl file has not been able to be read properly, regardless of the settings used for generation. The .txt file displays, but not in the proper locations. It does not appear to be scaling issue relating to the selection of imperial or metric, or zero suppression.. Does anyone have any suggestions? Michael This message was scanned for viruses on behalf of The Black Decker Corporation. * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] Excellon Drill Files
Re: [PEDA] Excellon Drill Files
Watnoski, Michael wrote: Hi Wolfgang, The problem is not merely an offset, but it is not the same size. It also appears not to be exactly the same, though it seems to have a similar pattern. Michael IIRC I had a problem with a co-worker's job, where he was working in metric - I think the drill file was not scaled correctly. Try setting Protel to work in inches, then regenerate both Gerber and drill files (and make sure you don't have Center board on film checked when generating the Gerbers) If the size is out by a factor of 10, you may have the wrong numeric format selected in the Gerber viewer when you are importing the Gerbers or the drill file. -- Peter Bennett TRIUMF 4004 Wesbrook Mall, Vancouver, BC, Canada GPS and NMEA info and programs: http://vancouver-webpages.com/peter/index.html * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] Excellon Drill Files
Michael, your problem is probably a combination of the things that others have already mentioned. The location misalignment is probably due to the plot center function in the advanced gerber tab of the cam server. I always use the absolute origin for both gerbers and drill generation. You could use the relative origin if you choose but just use it for both drills and gerber. Besides that there are also the other factors effecting drill generation. The first is your data format, 2.3, 2.4, 2.5. This sets the number of digits (2) and the number of decimal places (3 - 5), if your scaling is off by a factor of 10 or 100 then this is the culprit. The other function is the leading or trailing zero suppression, it can give some wild results in the drill output when you reader is not configured similarily. In short, you must have the same origin point used for gerber and drill generation, you must have the same formats selected between Protel and the gerber viewer for correct drill alignment and scaling. That's the gist of your problem. It really doesn't matter what formats you use as long as the viewer is configured correctly to import the data that you formatted when generating the gerbers or drills. Sincerely, Brad Velander. Lead PCB Designer Norsat International Inc. #300 - 4401 Still Creek Drive, Burnaby, B.C., Canada, V5C 6G9. Tel (604) 292-9089 (direct line) Fax (604) 292-9010 Website: www.norsat.com -Original Message- From: Watnoski, Michael [mailto:[EMAIL PROTECTED]] Sent: Wednesday, November 14, 2001 8:46 AM To: 'Protel EDA Forum' Subject: Re: [PEDA] Excellon Drill Files Importance: High Hi Wolfgang, The problem is not merely an offset, but it is not the same size. It also appears not to be exactly the same, though it seems to have a similar pattern. Michael * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] Excellon Drill Files
At 08:33 AM 11/14/01 -0800, Peter Bennett wrote: The drill file is always generated using screen coordinates - if you have a hole at 1000, 1000 on the screen, it will be at 1000, 1000 in the drill file. No, it is optionally set at absolute coordinates or what Mr. Bennett described, which is relative coordinates. Same for the gerbers When generating Gerbers, there is an option to Center plots on film which is checked by default - if that is checked, the coordinates in the Gerber files will be adjusted to place the board in the center of the plotter film. This will, of course, cause the drill file to not align with the Gerbers. Uncheck Center plots on film, regenerate the Gerbers, and everything should line up. Assuming that both outputs are set to the same coordinate system. Center plots on film should *not* be the default. Photoplotters will center the output anyway, but centering really screws up every coordinate. Frankly, I'd get rid of the feature, but, certainly, I would not have it be the default. More attention could be paid to this area of the program [EMAIL PROTECTED] Abdulrahman Lomax Easthampton, Massachusetts USA * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] Excellon Drill Files
Re: [PEDA] Excellon Drill Files
Watnoski, Michael wrote: Thanks for all your attempts. I still have the problem with the .drl file . I may not have explained it clearly. The origin and zero suppression were set correctly, as was the data format. The holes appear to be the right size, they are usually just placed in the lower left hand corner of the design. Some of the holes are in approximately the right relative position, though many are not. I would hope that the output format from protel would be an industry standard so that a conversion would not be necessary to use a common viewer. I usually prefer to check the outputs with a viewer from a nonrelated vendor for a confidence check. My .txt drill files use trailing zero suppression - if yours are the same format (and I don't recall anyplace in Protel to set the drill format), and the Gerber viewer is expecting leading zero suppression, this would put most holes down in the bottom left of the workspace - only holes requiring three digits after the decimal would be where they belong. (my Gerber files use leading zero suppression. A coordinate of 01.500 would come out as 1500 in Gerbers, and 015 in the drill file...) -- Peter Bennett TRIUMF 4004 Wesbrook Mall, Vancouver, BC, Canada GPS and NMEA info and programs: http://vancouver-webpages.com/peter/index.html * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] Excellon Drill Files
Michael, well you have got me. I have seen what you are describing many times with many different CAD packages and every single time it is one of the configuration formats for the drill data (or the gerber data). To check which is wrong I usually do a measurment in the CAM tool to see which is right, gerber or drill. Short of what has been suggested by myself or others, I am at a loss. Yes, I too always check Gerber usuing an independant CAm tool. Sometimes two CAM tools before I am satisfied. I am sure there is a configuration problem because I have no problem with my Protel Gerber or Drill output. One thing to remember, is the problem always the same even though you had changed settings? Are your Gerbers going to the directory that you expected outside of the database? Check you file dates and times to make sure you are seeing the latest Gerbers when you are changing things. I hate the way the external directory is set within the Protel menu and not in the actual CAM file where it would be saved with the file. Many times I am chasing problems which don't seem to change just because the files are going somewhere other then where I expected them to go. Sincerely, Brad Velander. Lead PCB Designer Norsat International Inc. #300 - 4401 Still Creek Drive, Burnaby, B.C., Canada, V5C 6G9. Tel (604) 292-9089 (direct line) Fax (604) 292-9010 Website: www.norsat.com -Original Message- From: Watnoski, Michael [mailto:[EMAIL PROTECTED]] Sent: Wednesday, November 14, 2001 12:27 PM To: 'Protel EDA Forum' Subject: Re: [PEDA] Excellon Drill Files Importance: High Thanks for all your attempts. I still have the problem with the .drl file . I may not have explained it clearly. The origin and zero suppression were set correctly, as was the data format. The holes appear to be the right size, they are usually just placed in the lower left hand corner of the design. Some of the holes are in approximately the right relative position, though many are not. I would hope that the output format from protel would be an industry standard so that a conversion would not be necessary to use a common viewer. I usually prefer to check the outputs with a viewer from a nonrelated vendor for a confidence check. Michael * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] Excellon Drill Files
At 01:21 PM 11/14/01 -0800, Peter Bennett wrote: My .txt drill files use trailing zero suppression - if yours are the same format (and I don't recall anyplace in Protel to set the drill format), and the Gerber viewer is expecting leading zero suppression, this would put most holes down in the bottom left of the workspace - only holes requiring three digits after the decimal would be where they belong. The setting is part of the CAM Outputs for... setup for drill files, likewise it is a gerber option. When I want a drill file to be easy for a human to read, I set it for no zero suppression. [EMAIL PROTECTED] Abdulrahman Lomax Easthampton, Massachusetts USA * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
