Re: [PEDA] Gerber generation bug?
Re: [PEDA] Gerber generation bug?
On Thu, 13 June 2002, "Watnoski, Michael" wrote > > Greetings, > > I recently found a problem while generating Gerber files from > Protel. When the Gerbers are generated without the 'Use Software Arcs' box > checked, parts of polygon copper pours become complete arcs where they > outline some pads. This is not a problem on the board design. These arcs > short to adjacent polygons and tracks. It seems to work OK when the box is > checked. I verified the Gerber files using Lavenier ViewMaster and LPKF > BoardMaster and they look the same. I have not checked the ASCII output of > the Gerber file yet, but I suspect that the angles of the included arc are > not generated properly. Has anyone else seen this problem? > > Michael Watnoski > Dear Protel Experts, As well as Mr. Watnoski I found out the same bug in the very beginning when I obtained Protel99 and after many experiments relised that: In Gerber files generated with Protel 99SE CAM Manager the following strange things are observed: 1. When using format 274-D: Pads with rectangular and oblong shapes with rotation angle different from 0 deg are reverted to 0 deg. This doesnt happen in 274-X. 2. Both 274-D and 274-X: 2.1. The same as above happens with area fills. 2.2. Arcs with angle less than 90 deg are converted into their complementaries i.e. if an arc has an angle 20 deg, in Gerber file it appears with angle 360-20=340 deg. The start-, end point and centre remain the same. This doesnt happen with software arcs ON because arcs are exploded down to straight line segments. But this isnt the right solution can you imagine how large will become the Gerber file with 2000 arcs in it? Above mentioned problems do not depend on the resolution (number of decimals) as well as on the measure system (metric or inch). In addition they dont occur with Protel 98. This is definitely bug in the CAM server itself because the same Gerbers imported back into Protel PCB and into third party software (CAM350, CAMTASTIC, PCGERBER etc. etc.) look exactly the same. If anybody has an idea about the solution I would appreciate his advice. Regards Emil Strezov [EMAIL PROTECTED] __ Get your FREE personalized e-mail at http://www.canada.com * Tracking #: CFD478F26FB0584081FF8CEB9B76FB4CC4E19D10 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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 generation bug?
Better yet, don't import your Gerbers back into Protel at all . Use a 3rd party viewer like Lavenir (Viewmate) or Camtastic, both are free and do a great job at catching all these little gerber generating bugs and/or user errors . Best Regards, Matt Tudor, MSEE http://www.gigahertzelectronics.com - Original Message - From: "Jon Elson" <[EMAIL PROTECTED]> To: "Protel EDA Forum" <[EMAIL PROTECTED]> Sent: Friday, June 14, 2002 2:58 PM Subject: Re: [PEDA] Gerber generation bug? > "Watnoski, Michael" wrote: > > > Greetings All, > > > > I am generating the Gerbers at 2.4 imp. The problem does not seem > > to be a round off type, rather the arc portion of the poured polygon around > > a pad continues for a full 360 degrees. I did not have to import the > > Gerbers back to Protel. > > No, I didn't mean to import Gerbers into protel for work on the PCB, but > to see whether Protel displays the incorrect info IN PROTEL. This would make > it a lot more meaningful to the Altium support people, if the error can be > demonstrated completely within Protel. I always check my Gerber files > by importing back into Protel, and catch a number of common mistakes > in setting up apertures, hole sizes, board outline and plot legends, etc. > I do this mostly because it is the fastest way to check the Gerbers. > > Jon > > > > * Tracking #: 8A2612DAEB9E8045B6B5ED837D393DC97FDEEDC4 > * > * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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 generation bug?
re virtual short 'cracks' the final resolution (after several 'final' resolutions) was do not use centroid origin, use pin 1 origin ** most important ** design the part so that the pad centers fall on an integer 1 mil grid then gerber 2.3-2.5 works great, no cracks (i had pushed the pads centers off by .005 mil and that caused the roundoff error, *sometimes*) Dennis Saputelli Abd ulRahman Lomax wrote: > > At 01:00 PM 6/14/2002 -0700, Dennis Saputelli wrote: > >i can see the submil cracks in my defective virtual shorts quite easily > >in CAMtastic > > > >i would agree that it is a better tool for looking at gerbers than > >protel > > Just to note, Mr. Saputelli's problem with virtual shorts was due, as I > recall, to roundoff error in the gerber generation. The cracks would *also* > have been visible, I expect, in gerber reimported to Protel. My point about > Protel being better in the submil region is that the display routines are > more accurate, even if the gerber generation is a tad shaky at times. > > The Protel *database* has a substantially finer resolution than what > CAMtastic stores, I think, and the display routines are pretty good (though > they will sometimes show pixel cracks where none exist, but those cracks do > not widen upon zooming in, and sometimes they even disappear at some zoom > levels. * Tracking #: B85D0906364B5948B3E88FE909EE6C04A1922B32 * -- ___ www.integratedcontrolsinc.comIntegrated Controls, Inc. tel: 415-647-04802851 21st Street fax: 415-647-3003San Francisco, CA 94110 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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 generation bug?
At 01:00 PM 6/14/2002 -0700, Dennis Saputelli wrote: >i can see the submil cracks in my defective virtual shorts quite easily >in CAMtastic > >i would agree that it is a better tool for looking at gerbers than >protel Just to note, Mr. Saputelli's problem with virtual shorts was due, as I recall, to roundoff error in the gerber generation. The cracks would *also* have been visible, I expect, in gerber reimported to Protel. My point about Protel being better in the submil region is that the display routines are more accurate, even if the gerber generation is a tad shaky at times. The Protel *database* has a substantially finer resolution than what CAMtastic stores, I think, and the display routines are pretty good (though they will sometimes show pixel cracks where none exist, but those cracks do not widen upon zooming in, and sometimes they even disappear at some zoom levels. * Tracking #: 9B6F3A185E8E7048AB780FCCD728F97049C52796 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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 generation bug?
- Original Message - From: "Abd ulRahman Lomax" <[EMAIL PROTECTED]> To: "Protel EDA Forum" <[EMAIL PROTECTED]> Sent: Friday, June 14, 2002 2:28 PM Subject: Re: [PEDA] Gerber generation bug? [snip] > > Mr. Elson's question about protel import was a good one, however. If Protel > imports the gerber and the arcs are correct, we probably have a case of > differing interpretations of the gerber code. This seems like the most likely explination to me too. I've been generated thermal relief's on my power planes for a very long time and I've become accustom to GCPrevue just not display them. But if I read the power plane back into Protel, there they (thermal relief's) are. I've never tried this with Camtastic. Jeff Stout [snip] * Tracking #: 540A22AB95FC424184B82AE23C675D060EE99C26 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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 generation bug?
Abd ulRahman Lomax wrote: > Actually, Protel import, while the information would be valuable, is *not* > the best check of file accuracy. CAMtastic is much, much better for this. > If RS-274X output is used, it is almost one-button to bring all the gerbers > into CAMtastic, and only a few seconds more to bring in the *drill* > information. > > > I always check my Gerber files > >by importing back into Protel, and catch a number of common mistakes > >in setting up apertures, hole sizes, board outline and plot legends, etc. > >I do this mostly because it is the fastest way to check the Gerbers. > > Unfortunately, it does not really check the gerbers, because Protel made > mistakes in gerber implementation, and Protel might well repeat these > mistakes in the other direction. The most famous one is the incorrect > implementation of octagonal pads. (I forget if this one looks okay on > import.) An independent gerber viewer, particularly the kind of CAM program > that a fabricator might be using, is much better. > > There is one problem with CAMtastic, however. The resolution is limited. > Not a problem until one is working with pretty small dimensions, however. > If one really needs high accuracy, in the submil region, I'd be sure to > verify the viewer. Protel does better on this, it does not break down until > the microinch region. Yes, I know there are risks in all this, but I often DO view things with just a couple pads filling the whole screen, and then sometimes measure the gaps between planes and pads. All I can say is I haven't gotten in trouble with this. If the board maker finds something and refers it back to me, I can always see it on the imported Gerbers, and then fix whatever it might be and regenerate. So, I've never experienced a flaw that could not be detected by careful examination of the imported gerber files just using Protel. I've gotten to the point that my board fab rarely has anything to squawk about, and errors are generally present in the schematic or schematic library information, too. I do not use octagon pads, which seem to be a holdover from the optical aperture wheel on the original Gerber photoplotter, to prevent diagonal lines from having faded edges. I guess some tight zig-zag BGA grids might benefit from these pads, though. Jon * Tracking #: BCF741E35AF7824D997BDEFB858CD7C3FA2C0E18 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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 generation bug?
Abd ulRahman Lomax wrote: > No one has come forward with a similar report. At this point, I will > underline one of my first comments: it would be useful to see the Gerber > output code. I described in my last post in this thread a means of > obtaining a test PCB file that could be shared, and the gerber code itself, > which would be only one or a few lines, could be included in a post. I can state that at one time, when I used a low resolution Gerber format to generate a Gerber file with a poured copper fill, that it would cause shorts to the signal tracks. It was pretty obvious it was a resolution problem, and regenerating the Gerber files with a higher resolution (2.4 instead of 2.3) fixed the problem. I believe this was WITH software arcs, not without, so it now appears that it is totally unrelated to the problem currently being discussed. It is pretty obvious that generating the plot with insufficient resolution and software arcs could lead to track endpoints being misplaced due to rounding error, and so is not a clear 'bug', although a nice note during Gerber generation that coordinates are being rounded to lower resolution might be nice. (This message would probably come out during ALL Gerber generations, however, so might be meaningless.) Jon * Tracking #: 7EAD9569EB7DA6428B768E1BB27BFCF881381B15 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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 generation bug?
i can see the submil cracks in my defective virtual shorts quite easily in CAMtastic i would agree that it is a better tool for looking at gerbers than protel Dennis Saputelli Abd ulRahman Lomax wrote: > >> There is one problem with CAMtastic, however. The resolution is limited. > Not a problem until one is working with pretty small dimensions, however. > If one really needs high accuracy, in the submil region, I'd be sure to > verify the viewer. Protel does better on this, it does not break down until > the microinch region. * Tracking #: 5CAE931B5911F845B8630E9D04425D01A5EE4850 * -- ___ www.integratedcontrolsinc.comIntegrated Controls, Inc. tel: 415-647-04802851 21st Street fax: 415-647-3003San Francisco, CA 94110 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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 generation bug?
At 01:58 PM 6/14/2002 -0500, Jon Elson wrote: >No, I didn't mean to import Gerbers into protel for work on the PCB, but >to see whether Protel displays the incorrect info IN PROTEL. This would make >it a lot more meaningful to the Altium support people, if the error can be >demonstrated completely within Protel. Actually, Protel import, while the information would be valuable, is *not* the best check of file accuracy. CAMtastic is much, much better for this. If RS-274X output is used, it is almost one-button to bring all the gerbers into CAMtastic, and only a few seconds more to bring in the *drill* information. Yes, the CAMtastic user interface is a bit of a pain to learn, if you want to use it to edit gerber, but for inspecting the boards one pretty much only needs to know how to enable layers and to zoom in and out (the + and - keys, which also recenter on the cursor, so it is very quick to move in and out and around). > I always check my Gerber files >by importing back into Protel, and catch a number of common mistakes >in setting up apertures, hole sizes, board outline and plot legends, etc. >I do this mostly because it is the fastest way to check the Gerbers. Unfortunately, it does not really check the gerbers, because Protel made mistakes in gerber implementation, and Protel might well repeat these mistakes in the other direction. The most famous one is the incorrect implementation of octagonal pads. (I forget if this one looks okay on import.) An independent gerber viewer, particularly the kind of CAM program that a fabricator might be using, is much better. There is one problem with CAMtastic, however. The resolution is limited. Not a problem until one is working with pretty small dimensions, however. If one really needs high accuracy, in the submil region, I'd be sure to verify the viewer. Protel does better on this, it does not break down until the microinch region. * Tracking #: E574454C74DA054CBDD9DBD68340556BDE654F17 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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 generation bug?
I did not write what Mr. Watnoski attributed to me. Rather it was written by Mr. Elson in response to my own post. I did not think that the problem had anything to do with resolution, Mr. Watnoski was quite explicit in his first post that it was an arc rotation extent problem. The arc is correct on the PCB but is not correct in the gerber, as seen by several viewers. Mr. Elson's question about protel import was a good one, however. If Protel imports the gerber and the arcs are correct, we probably have a case of differing interpretations of the gerber code. It would likewise be interesting to see what CAMtastic shows. (CAMtastic is really an independent program even though it is now sold by Altium/Protel.) No one has come forward with a similar report. At this point, I will underline one of my first comments: it would be useful to see the Gerber output code. I described in my last post in this thread a means of obtaining a test PCB file that could be shared, and the gerber code itself, which would be only one or a few lines, could be included in a post. If we have a test pcb, a small file which shows the problem for Mr. Watnoski, it will be possible to verify the issue, or the converse, to show that the file plots properly for the rest of us. That file could be sent to me personally as an attachment, I could put it up on the protel-users filespace. *Don't try to send attachments to the list.* Bad Feng Shui. (For a long time, the list would forward attachments. Eventually, Techserv figured out that this put a huge burden on the mail server when someone attached a couple of megabyte file to a post, which then was copied to a thousand list members, plus it was poor security -- viruses and all -- and bad policy in general and turned the option off.) A possible workaround is to use software arcs, that is, check the box and allow Protel to generate the arcs as a proliferation of line segments. The only practical difference is the size of the gerber files, which will not be exhorbitantly larger with software arcs unless there are a *lot* of arcs If the problem still exists with software arcs, we have a bug or trashed installation on a whole different level At 02:49 PM 6/14/2002 -0400, Watnoski, Michael wrote: >Greetings All, > > I am generating the Gerbers at 2.4 imp. The problem does not seem >to be a round off type, rather the arc portion of the poured polygon around >a pad continues for a full 360 degrees. I did not have to import the >Gerbers back to Protel. I checked them with several independent viewers. I >ran the Gerber generation several times while swapping from software arcs >and back. The problem only exists when 'Use Software Arcs' in not checked. > >Michael Watnoski > > >Abd ulRahman Lomax wrote: >One thing he should try is to regenerate the Greber files at the highest >numeric resolution (2.5). Roundoff errors could cause the described >problem if the arcs were small. He doesn't mention whether importing >the gerber files back into Protel shows the problem, or doesn't. >That might be useful info. > >Jon > > >* Tracking #: FFDE52F5867D3849AFE575C2EAB3D9620BCD8CAF >* > > * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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 generation bug?
"Watnoski, Michael" wrote: > Greetings All, > > I am generating the Gerbers at 2.4 imp. The problem does not seem > to be a round off type, rather the arc portion of the poured polygon around > a pad continues for a full 360 degrees. I did not have to import the > Gerbers back to Protel. No, I didn't mean to import Gerbers into protel for work on the PCB, but to see whether Protel displays the incorrect info IN PROTEL. This would make it a lot more meaningful to the Altium support people, if the error can be demonstrated completely within Protel. I always check my Gerber files by importing back into Protel, and catch a number of common mistakes in setting up apertures, hole sizes, board outline and plot legends, etc. I do this mostly because it is the fastest way to check the Gerbers. Jon * Tracking #: 8A2612DAEB9E8045B6B5ED837D393DC97FDEEDC4 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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 generation bug?
Re: [PEDA] Gerber generation bug?
Abd ulRahman Lomax wrote: > At 10:06 AM 6/13/2002 -0400, Watnoski, Michael wrote: > >When the Gerbers are generated without the 'Use Software Arcs' box > >checked, parts of polygon copper pours become complete arcs where they > >outline some pads. This is not a problem on the board design. These arcs > >short to adjacent polygons and tracks. It seems to work OK when the box is > >checked. I verified the Gerber files using Lavenier ViewMaster and LPKF > >BoardMaster and they look the same. I have not checked the ASCII output of > >the Gerber file yet, but I suspect that the angles of the included arc are > >not generated properly. Has anyone else seen this problem? > > It will be good to see the answer to Mr. Watnoski's question before going > much further; I usually check the box out of long-standing habit (Tango did > not even have a gerber arc output option, so all arcs were "software arcs.") > > There may be some problems with variants on RS-274X, as one speculation, > sometimes the standard is a bit unclear, it used to be positively ambiguous > on the matter of polygonal pads, which is why Protel's octagon plotting is > so defective. > > By all means, I would look at the output code, probably by exploding the > polygon on a copy of the board file, deleting everything on the board but > the relevant arc, and generating gerber, comparing the Protel arc > parameters with those in the gerber. One thing he should try is to regenerate the Greber files at the highest numeric resolution (2.5). Roundoff errors could cause the described problem if the arcs were small. He doesn't mention whether importing the gerber files back into Protel shows the problem, or doesn't. That might be useful info. Jon * Tracking #: 18435314E4A14544AA35BAD9887EE3A051424D20 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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 generation bug?
At 10:06 AM 6/13/2002 -0400, Watnoski, Michael wrote: >When the Gerbers are generated without the 'Use Software Arcs' box >checked, parts of polygon copper pours become complete arcs where they >outline some pads. This is not a problem on the board design. These arcs >short to adjacent polygons and tracks. It seems to work OK when the box is >checked. I verified the Gerber files using Lavenier ViewMaster and LPKF >BoardMaster and they look the same. I have not checked the ASCII output of >the Gerber file yet, but I suspect that the angles of the included arc are >not generated properly. Has anyone else seen this problem? It will be good to see the answer to Mr. Watnoski's question before going much further; I usually check the box out of long-standing habit (Tango did not even have a gerber arc output option, so all arcs were "software arcs.") There may be some problems with variants on RS-274X, as one speculation, sometimes the standard is a bit unclear, it used to be positively ambiguous on the matter of polygonal pads, which is why Protel's octagon plotting is so defective. By all means, I would look at the output code, probably by exploding the polygon on a copy of the board file, deleting everything on the board but the relevant arc, and generating gerber, comparing the Protel arc parameters with those in the gerber. The RS-274X standard is at: http://www.maniabarco.com/transdown/rs274xrevd_e.pdf Abd ul-Rahman Lomax LOMAX DESIGN ASSOCIATES PCB design, consulting, and training Protel EDA license resales Easthampton, Massachusetts, USA (413) 527-3881, efax (419) 730-4777 [EMAIL PROTECTED] * Tracking #: 604CB06782BA634EACE8C1C68843AB771FDEAB1F * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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 generation bug?
Michael, well this news won't help you out but I never use 'Use Software Arcs' and certainly don't see your problem. Sorry but figured I could probably tell you that you seem to be barking up the wrong tree unless it is something specific to your database. I am relatively sure that many others also don't use 'Use Software Arcs' judging by other discussions here in the recent past. SO I am sure that you are chasing some other fault, just seems to be the fault of the 'Use Software Arcs' feature right now. 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 Visit us at Booth 2G2-09 at CommunicAsia 2002 in Singapore June 18-21. > -Original Message- > From: Watnoski, Michael [mailto:[EMAIL PROTECTED]] > Sent: Thursday, June 13, 2002 7:06 AM > To: '[EMAIL PROTECTED]' > Subject: [PEDA] Gerber generation bug? > > > Greetings, > > I recently found a problem while generating Gerber files from > Protel. When the Gerbers are generated without the 'Use > Software Arcs' box > checked, parts of polygon copper pours become complete arcs where they > outline some pads. This is not a problem on the board > design. These arcs > short to adjacent polygons and tracks. It seems to work OK > when the box is > checked. I verified the Gerber files using Lavenier > ViewMaster and LPKF > BoardMaster and they look the same. I have not checked the > ASCII output of > the Gerber file yet, but I suspect that the angles of the > included arc are > not generated properly. Has anyone else seen this problem? > > Michael Watnoski > * Tracking #: AA32238FA696134A8DCE9F2CC85C2CEEF05A58B0 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
