Re: [PEDA] Protell99SE (SP6) missing diagonal pads off gerbers (sometimes) - bug?
At 09:19 PM 2/5/2002 +, Steve Wiseman wrote: > > Elsewhere I described an alternate method of doing a virtual short, that > > is, a jumper footprint that appears as open to DRC but is actually shorted > > in plot. This alternative involves placing a track, as part of the VS > > footprint, on an otherwise unused mech layer. > >I used to do this, and still do sometimes for jumper links. However, it's >extra steps at photoplot time, and extra steps = extra opportunities for >mistakes. Since, by the time a board this complex goes out, I've normally >been working 20-hour days for a week, the simpler I can make things, the >longer the PCB shop will let me sleep before phoning for clarification :) It is one extra step, which does not need to be repeated. This is one great feature of the CAM Manager: you can set up individual parameters for each plot if you want, and then all [enabled] plots will be generated at once. Usually we don't need to do this, but making such a shunt is a case. I also use this feature to generate formal drawings, merging a different mech layer. Remember, if you *do* forget to short the part, it is not a big disaster, if you have made the parts properly. You might even do both: a virtual short and a shunt. That is, take your current virtual shorts and add mech layer track to short them. If we had layer associations it would help. (Top is associated with Top Overlay, so when you flip the board, the overlay flips with it. That doesn't happen with the mech layers, which is a Protel deficiency. Tango DOS had top and bottom assembly layers in addition to the legend layers, they flipped with the part) Thus one should make a top layer shunt and a bottom layer shunt, and they should not be flipped in design. Protel should, in general, fix the photoplot routines so that WYSIWYG, without *any* deviation except the unavoidable one of roundoff error. There is little reason for aperture matching in times when the plotters can handle D-codes to D999. I'd make aperture matching an option that defaults to zero. *Maybe* I would accept minimum aperture matches that represent only the minimum difference resulting from unit shifts (mm-mil). But I think not. By the way, it's pretty obvious why the rotated pads did not plot. The plot routine quite properly does not draw pads or any other primitive with a zero aperture unless zero is the actual size of the primitive. The programmer trapped it out, it would lead to lockup. [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] Protell99SE (SP6) missing diagonal pads off gerbers (sometimes) - bug?
On Tue, 5 Feb 2002, Abd ul-Rahman Lomax wrote: > Looking at Mr. Wiseman's files, I discover that there is indeed a zero > aperture in the RS-274X list. Wondering what the source of this file might > be, I looked through the PCB file and found two fiducials with arcs with > zero width, used apparently to keep tracks out. (These arcs should have the > keepout attribute, but they don't.) it's not clear that keepout is useful here, and, since using keepout for features other than board edge has been seen to irritate the autorouter, I tend to not use it. I'm prepared to be convinced otherwise, but at the moment, simple copper does fine. > Editing the arc to 1.5 mils draw causes the pads in question to be drawn > correctly. Deleting the arc also causes the pads to be drawn. this is the giveaway, isn't it... > It appears that there may be a minimum match width, not too surprising. I > don't have time to check further today, but the match routines could be old > enough that they allow a 1 mil variation no matter what. 1 thou, on a board where I'm using 4 thou track and gap, just won't do. 2 thou boards are coming my way soon, by the look of things. Time for Protel to get this fixed, and maybe generate a patch / SP? > The virtual shorts being used here depend on very precise photoplotting, I generally boost the long axis of the shunts by a thou before plotting, to be safe. However, I do not expect (or see) any problems plotting at this size. The whole board's 4-thou track & gap - two thou overlap across a 6 thou feature is enormous. > Elsewhere I described an alternate method of doing a virtual short, that > is, a jumper footprint that appears as open to DRC but is actually shorted > in plot. This alternative involves placing a track, as part of the VS > footprint, on an otherwise unused mech layer. I used to do this, and still do sometimes for jumper links. However, it's extra steps at photoplot time, and extra steps = extra opportunities for mistakes. Since, by the time a board this complex goes out, I've normally been working 20-hour days for a week, the simpler I can make things, the longer the PCB shop will let me sleep before phoning for clarification :) > There are several bugs here, interacting. When a zero aperture is assigned > to draw the pads, they are not drawn, they are missing. The pads themselves > are not completely drawn even when the aperture is correct, though this may > be harmless in this case. The zero-aperture arc, however, is drawn. I > placed a zero-width track and it is also drawn correctly, the problem is > just in the pad-drawing routine. > > Aperture match is not exact even if match is set to 0. I think that summarises concisely and accurately - I thank you all for your time & effort - this list continues to be amazingly useful! Steve * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] Protell99SE (SP6) missing diagonal pads off gerbers (sometimes) - bug?
At 08:21 AM 2/5/2002 +0100, Edi Im Hof wrote: >Just a quick shot, you said the pads are drawn with an aperture of a >quarter of the smallest dimension of the pad. In this case this would be >1.25mil. Have you tried to gerber with a 0.01mil resolution? Is such an >aperture in the gerber file? If yes, is this aperture actually used? This is literally on the right track. Looking at Mr. Wiseman's files, I discover that there is indeed a zero aperture in the RS-274X list. Wondering what the source of this file might be, I looked through the PCB file and found two fiducials with arcs with zero width, used apparently to keep tracks out. (These arcs should have the keepout attribute, but they don't.) It appears that Protel is creating the 0.0 aperture and then assigning it to the tracks used to draw the rotated pads. Editing the arc to 1.5 mils draw causes the pads in question to be drawn correctly. Deleting the arc also causes the pads to be drawn. The match width in the aperture setup is set to .00013 mm, which is the default. Changing the match width to 0 does not fix the problem, however. It appears that there may be a minimum match width, not too surprising. I don't have time to check further today, but the match routines could be old enough that they allow a 1 mil variation no matter what. The virtual shorts being used here depend on very precise photoplotting, photoplot roundoff can cause difficulties. Normally one creates the pads to be integral values in the system being used for plot (that's one problem here). Further, rotating the pad causes it to be drawn, introducing other possible errors. Elsewhere I described an alternate method of doing a virtual short, that is, a jumper footprint that appears as open to DRC but is actually shorted in plot. This alternative involves placing a track, as part of the VS footprint, on an otherwise unused mech layer. In the photoplot setups, the layer on which one wants the short plotted has a separate photoplot setup that merges the appropriate mech layer. This is a tad less simple to set up than the virtual short component, but I expect it to be more reliable. There are several bugs here, interacting. When a zero aperture is assigned to draw the pads, they are not drawn, they are missing. The pads themselves are not completely drawn even when the aperture is correct, though this may be harmless in this case. The zero-aperture arc, however, is drawn. I placed a zero-width track and it is also drawn correctly, the problem is just in the pad-drawing routine. Aperture match is not exact even if match is set to 0. [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] Protell99SE (SP6) missing diagonal pads off gerbers (sometimes) - bug?
At 18:09 04.02.02 -0500, you wrote: >At 09:30 PM 2/4/2002 +, Steve Wiseman wrote: > >>I'm not sure if you import & check your gerbers, looking for features that >>have been rendered wrongly... It's not something I'm prepared to do. (this >>board reports as 20,000 tracks, 4019 pads, and I'm looking for a defect 8 >>thou by 6 - it's quicker to have it etched & assembled than to go through >>looking for weird problems) > >That's a very small pad, this could be related to the problem. There are a >number of things I can think of, but I can't take the time to speculate, >I'd rather look at files. Just a quick shot, you said the pads are drawn with an aperture of a quarter of the smallest dimension of the pad. In this case this would be 1.25mil. Have you tried to gerber with a 0.01mil resolution? Is such an aperture in the gerber file? If yes, is this aperture actually used? Edi Im Hof >[EMAIL PROTECTED] >Abdulrahman Lomax >Easthampton, Massachusetts USA + IH electronic+ Phone: ++41 52 320 90 00 + + Edi Im Hof + Fax: ++41 52 320 90 04 + + Doernlerstrasse 1, Sulz + URL: http://www.ihe.ch + + CH-8544 Rickenbach-Attikon + E-Mail: [EMAIL PROTECTED] + + Switzerland + + * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] Protell99SE (SP6) missing diagonal pads off gerbers (sometimes) - bug?
On Mon, 4 Feb 2002, Jon Elson wrote: > I think there is a report bugs email address or link on their web site. Yeah, I just couldn't get to www.protel.com this morning... Ho hum... > Well, I DO check them this way. I certainly DON'T check EVERY track > and pad, just look for wierd stuff, like 1" square pads or tracks that > don't end on a pad (good guess there is SUPPOSED to be a pad there, > and it was not in the aperture list). Oh, I certainly run the gerbers through the viewer, to catch as many things as I can - things like plane mishaps, proper tenting on vias, but spotting open-ended tracks seems a bit hopeful. If I could run the error-checker over the gerbers, to check for continuity, that'd be great, but that's not (yet) an option. Steve * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] Protell99SE (SP6) missing diagonal pads off gerbers (sometimes) - bug?
Steve Wiseman wrote: > On Mon, 4 Feb 2002, Jon Elson wrote: > > You should open a new PCB file, and import the gerbers to it. Then, take a > > look > > at the pads in question. > > Just done it - and no, no pads. It's definitely a problem within Protel, > (but easier to visualise in a gerber viewer which can display pads & > tracks in different colours). > > > If so, it may be easier to get Altium to take a look at the problem, > > too - if it can be demonstrated all within Protel. > > Hmm. I don't even know who to report bugs to at Protel / Altium, or if > it's worth the effort. I think there is a report bugs email address or link on their web site. As for whether it is worth it, I just don't know. Exotic bugs that are really hard to reproduce don't seem to get much attention. Straightforward, easy to reproduce bugs that cause the gerbers to not match the screen in a severe way SHOULD get attention there, but I don't know. My experience has been pretty much the same. > > I have been using this technique to check Protel output, and haven't had > > a problem that wen't undetected by Protel. (Except for the giant aperture > > definitions in 274X, which my PCB vendor can't handle.) > > I'm not sure if you import & check your gerbers, looking for features that > have been rendered wrongly... It's not something I'm prepared to do. (this > board reports as 20,000 tracks, 4019 pads, and I'm looking for a defect 8 > thou by 6 - it's quicker to have it etched & assembled than to go through > looking for weird problems) Well, I DO check them this way. I certainly DON'T check EVERY track and pad, just look for wierd stuff, like 1" square pads or tracks that don't end on a pad (good guess there is SUPPOSED to be a pad there, and it was not in the aperture list). Jon * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] Protell99SE (SP6) missing diagonal pads off gerbers (sometimes) - bug?
Steve If you wish send a sample this way. Ian Capps - Original Message - From: "Steve Wiseman" <[EMAIL PROTECTED]> To: "Protel EDA Forum" <[EMAIL PROTECTED]> Sent: Tuesday, February 05, 2002 3:27 AM Subject: Re: [PEDA] Protell99SE (SP6) missing diagonal pads off gerbers (sometimes) - bug? > > > Now, to the present problem. Here is what I suggest. Create a board file > > with just one of the pads in question. Plot it. Copy the gerber code into a > > mail to the list. Describe the pad's characteristics fully, also anything > > which might be relevant from the gerber setups. > > Unfortunately, neither my simple test board nor a copy & paste of the > offending pads into a test pcb exhibits the fault. (and, naturally, the > pcb in question is sensitive...). I'll keep trying to generate a test case > that fails, but I've not managed to provoke it yet. It's notable that it's > only the shunts that fail to plot - I've got some rotated capacitors that > worked fine. > > Ah - an update. Copy & paste failed, but cut & paste worked. I've now got > a small PCB that shows the behaviour. Any takers for a .pcb and .GBL? > > Steve > * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] Protell99SE (SP6) missing diagonal pads off gerbers (sometimes) - bug?
On Mon, 4 Feb 2002, Abd ul-Rahman Lomax wrote: > That's a very small pad, this could be related to the problem. indeed, but being very small isn't a crime... I guess it could be that the pad needs to be rendered with a 1.5 thou track, which might get rounded down to zero (although there's no zero-width lines visible in Viewmate, which generally gets them right). > There are a number of things I can think of, but I can't take the time > to speculate, I'd rather look at files. They left here 5 hours ago (or so), are they lost in transit? Steve * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] Protell99SE (SP6) missing diagonal pads off gerbers (sometimes) - bug?
At 09:30 PM 2/4/2002 +, Steve Wiseman wrote: >I'm not sure if you import & check your gerbers, looking for features that >have been rendered wrongly... It's not something I'm prepared to do. (this >board reports as 20,000 tracks, 4019 pads, and I'm looking for a defect 8 >thou by 6 - it's quicker to have it etched & assembled than to go through >looking for weird problems) That's a very small pad, this could be related to the problem. There are a number of things I can think of, but I can't take the time to speculate, I'd rather look at files. [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] Protell99SE (SP6) missing diagonal pads off gerbers (sometimes) - bug?
In US, [EMAIL PROTECTED] works, I think, or 1-800-544-4186. I've gotten pretty good responses the 2 or 3 times I've contacted them in the last few months. (You're mileage may vary!) > -Original Message- > From: Steve Wiseman [mailto:[EMAIL PROTECTED]]On Behalf Of Steve Wiseman > Sent: Monday, February 04, 2002 1:31 PM > > If so, it may be easier to get Altium to take a look at the problem, > > too - if it can be demonstrated all within Protel. > > Hmm. I don't even know who to report bugs to at Protel / Altium, or if > it's worth the effort. * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] Protell99SE (SP6) missing diagonal pads off gerbers (sometimes) - bug?
On Mon, 4 Feb 2002, Jon Elson wrote: > You should open a new PCB file, and import the gerbers to it. Then, take a > look > at the pads in question. Just done it - and no, no pads. It's definitely a problem within Protel, (but easier to visualise in a gerber viewer which can display pads & tracks in different colours). > If so, it may be easier to get Altium to take a look at the problem, > too - if it can be demonstrated all within Protel. Hmm. I don't even know who to report bugs to at Protel / Altium, or if it's worth the effort. > I have been using this technique to check Protel output, and haven't had > a problem that wen't undetected by Protel. (Except for the giant aperture > definitions in 274X, which my PCB vendor can't handle.) I'm not sure if you import & check your gerbers, looking for features that have been rendered wrongly... It's not something I'm prepared to do. (this board reports as 20,000 tracks, 4019 pads, and I'm looking for a defect 8 thou by 6 - it's quicker to have it etched & assembled than to go through looking for weird problems) (I may also chase the "generate software arcs gives straight lines" issue, which caught me out a while back - the PCB shop swore blind I had thousands of sub-thou gaps - oddly all where teardropping had placed arcs... I just turned off "use software arcs" and all was well, so I let it slip. I'm really not a good software tester...) Steve * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] Protell99SE (SP6) missing diagonal pads off gerbers (sometimes) - bug?
> From: "Steve Wiseman" <[EMAIL PROTECTED]> > > > > Ah - an update. Copy & paste failed, but cut & paste worked. I've now got > > a small PCB that shows the behaviour. Any takers for a .pcb and .GBL? > > You should open a new PCB file, and import the gerbers to it. Then, take a look at the pads in question. It may be useful to know if there is something in the Gerber files that Protel can display. If so, it may be easier to get Altium to take a look at the problem, too - if it can be demonstrated all within Protel. I have been using this technique to check Protel output, and haven't had a problem that wen't undetected by Protel. (Except for the giant aperture definitions in 274X, which my PCB vendor can't handle.) Jon * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] Protell99SE (SP6) missing diagonal pads off gerbers (sometimes) - bug?
>Ah - an update. Copy & paste failed, but cut & paste worked. I've now got >a small PCB that shows the behaviour. Any takers for a .pcb and .GBL? > >Steve I'd be very interested in taking a look at this if you don't mind sending 'em to me. I use shunts all the time. Thanks, Frank Frank Gilley Dell-Star Technologies (918) 838-1973 Phone (918) 838-8814 Fax [EMAIL PROTECTED] http://www.dellstar.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 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] Protell99SE (SP6) missing diagonal pads off gerbers (sometimes) - bug?
On Mon, 4 Feb 2002, Sean James wrote: > I have parts on a few of my boards that are rotated at 45 degrees. If I use > round pads, they photoplot OK. When I tried rectangualr pads, they were > "drawn" with a spiral pattern that looked like a rectangular pad. If you can > live with round pads on your parts, then use them. (BTW - Accel didn't have > this problem, if I remember). This is indeed the case - it's ugly but not the problem I'm suffering. I don't get pads, either drawn or flashed. I get nothing, which conducts rather worse :( An interesting update on my sample board - when I pasted in the sample section from the broken board, all the previously perfect pads vanished, without any changes being made, so it's not necessarily something odd about my library part, more something screwy going on internally. This might be a pain to track down. Steve * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] Protell99SE (SP6) missing diagonal pads off gerbers (sometimes) - bug?
At 05:27 PM 2/4/2002 +, Steve Wiseman wrote: >Ah - an update. Copy & paste failed, but cut & paste worked. I've now got >a small PCB that shows the behaviour. Any takers for a .pcb and .GBL? Sure [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] Protell99SE (SP6) missing diagonal pads off gerbers (sometimes) - bug?
I have parts on a few of my boards that are rotated at 45 degrees. If I use round pads, they photoplot OK. When I tried rectangualr pads, they were "drawn" with a spiral pattern that looked like a rectangular pad. If you can live with round pads on your parts, then use them. (BTW - Accel didn't have this problem, if I remember). Sean James PCB Designer Telecast Fiber Systems, Inc. 102 Grove Street Worcester, MA 01605 (TEL) 508.754.4858 x33 (FAX) 413.541.6170 - Original Message - From: "Steve Wiseman" <[EMAIL PROTECTED]> To: "Protel EDA Forum" <[EMAIL PROTECTED]> Sent: Monday, February 04, 2002 12:27 PM Subject: Re: [PEDA] Protell99SE (SP6) missing diagonal pads off gerbers (sometimes) - bug? > > > Now, to the present problem. Here is what I suggest. Create a board file > > with just one of the pads in question. Plot it. Copy the gerber code into a > > mail to the list. Describe the pad's characteristics fully, also anything > > which might be relevant from the gerber setups. > > Unfortunately, neither my simple test board nor a copy & paste of the > offending pads into a test pcb exhibits the fault. (and, naturally, the > pcb in question is sensitive...). I'll keep trying to generate a test case > that fails, but I've not managed to provoke it yet. It's notable that it's > only the shunts that fail to plot - I've got some rotated capacitors that > worked fine. > > Ah - an update. Copy & paste failed, but cut & paste worked. I've now got > a small PCB that shows the behaviour. Any takers for a .pcb and .GBL? > > Steve > > > * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] Protell99SE (SP6) missing diagonal pads off gerbers (sometimes) - bug?
> Now, to the present problem. Here is what I suggest. Create a board file > with just one of the pads in question. Plot it. Copy the gerber code into a > mail to the list. Describe the pad's characteristics fully, also anything > which might be relevant from the gerber setups. Unfortunately, neither my simple test board nor a copy & paste of the offending pads into a test pcb exhibits the fault. (and, naturally, the pcb in question is sensitive...). I'll keep trying to generate a test case that fails, but I've not managed to provoke it yet. It's notable that it's only the shunts that fail to plot - I've got some rotated capacitors that worked fine. Ah - an update. Copy & paste failed, but cut & paste worked. I've now got a small PCB that shows the behaviour. Any takers for a .pcb and .GBL? Steve * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] Protell99SE (SP6) missing diagonal pads off gerbers (sometimes) - bug?
At 03:26 PM 2/4/2002 +, Steve Wiseman wrote: >All is well, except that, when placed at angles >like 45 degrees, they don't get plotted on the gerbers. (neither the >copper nor the holes in the solder resist.) Viewmate and my PCB shop >agree... Protel draws rectangular pads when they are rotated. They could do better, in general the Protel implementation of RS-274X ... is less than the best. The pad appears to be drawn with an aperture which is one-fourth the smallest dimension of the pad. This makes a rounded rectangle. It is, however, a significant deviation from display, a violation of the general rule that the gerber should match display (and DRC). Normally, however, this difference will not cause board failure (but it could). All forms of gerber will support accurate drawing, it is rather shameful, I'd say, that the ways in which Protel falls down have not been fixed after all these years. We could start with octagons, which are flat out incorrect. Protel does not, in the Knowledge Base, seem to recognize how badly things are broken. It is true that *most* PCBs do not contain conditions which show plot problems, that's the only reason that the existing situation has been tolerable. One Knowledge Base item recognizes, for example, that rotated octagons are plotted as circles; it suggests a work-around of rotating the individual pads to rotation 0. Which, of course, produces an octagon which is rotated 22.5 degrees according to RS-274X, but it appears that fabricators know not to follow the standard! The big problem with this work-around is that the pad edges are no longer where they were in the PCB file, and the difference could be significant. We can hope for better with Phoenix. It's about time that Protel generates true and correct RS-274X code. Yes, this will require different routines than are used for RS-274D, but along the way positive/negative plane merges and the like would become possible. And rotated flashes, I think, though RS-274X itself is frustratingly obtuse. Nevertheless, Protel owns CAMtastic and *better* get it right! (CAMtastic also has problems, it does not seem to handle submil features properly.) Now, to the present problem. Here is what I suggest. Create a board file with just one of the pads in question. Plot it. Copy the gerber code into a mail to the list. Describe the pad's characteristics fully, also anything which might be relevant from the gerber setups. Since rotated pads *do* plot for me, we need to look for something specific about *these* pads. [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] Protell99SE (SP6) missing diagonal pads off gerbers (sometimes) - bug?
On Mon, 4 Feb 2002, Andrew Ircha wrote: > I assume that Viewmate is some kind of Gerber viewing package. Yep, from Lavenir - seems to be well behaved, and is free (but won't save in demo mode). > It might be helpful to tell us how many of these shunts you have on the > board. 30, of which 9 were diagonal... > If there's a lot we might have to think of something clever, if > there's only a few we could come up with a hack. It's not a lot, and your 45 degree hack seems sane. It's just a pain that this all happens after all the error checking, so boards that I expect to come back working need an embarassing number of patch wires. A test board I've just built doesn't exhibit this problem, so It's not a trivial bug :( It's noticeable that Protel draws off-axis pads using track rather than pad, so I guess it's possible that weird bits of code are getting called, but I can't provoke it in a trivial test board. Steve * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
