Re: [PEDA] 45 degree pad problem !
Abd, please see below. - Original Message - From: Abd ulRahman Lomax [EMAIL PROTECTED] To: Protel EDA Forum [EMAIL PROTECTED] Cc: JaMi Smith [EMAIL PROTECTED] Sent: Monday, October 21, 2002 2:17 PM Subject: Re: [PEDA] 45 degree pad problem ! The best way to learn is to make mistakes. To learn big, make big mistakes. (Of course that isn't the whole story!) Unfortunately for some, this appears to be the only way that they can ever learn anything , but then there are others that just figure it out ahead of time : ) Actually, I find that a rather odd statement coming from someone who claims to have attended Throop Polytechnic. At 12:29 PM 10/16/2002 -0700, JaMi Smith wrote: Even if it is done at gerber time, it may make a difference in how Protel defines the pad to the gerber file based upon whether it is encountered as part of the design or part of a component, either of which should be different than a fill which it will most certainly draw. There are a couple of misconceptions here. Protel does not understand RS-274X rotations. It has been recommended that this be fixed! Fills are normally created by using a flash. I.e., Protel treats a fill, which is always rectangular, as if it were a rectangular pad. It creates an aperture for it. However, because Protel can't rotate this, it must draw rotated non-circular pads. The point I am making is that Protel may in fact be handling things such as a component in a draw it (or define the fill) once and repeat it fashion, and may in fact try and rotate what it has drawn itself by simply recalculating each previously drawn fill segment, as opposed to encountering the object to be drawn in its final rotated state and attempting to draw it from scratch at that point. There are obviously numerous different ways that any of the different kinds of objects could be handled bu Protel, and unless we ask the original programmer or look at the source we will never really know for sure, and cetainly not well enough to be dogmatic. The point is that we know that something is amuck, but we don't quite know what it is and where it is, and my suggestions simply point out a few other possible ways to possibly skirt the problem, if in fact the problem is possibly only in one area, which it may not be. It really depends on how the code handles all of these different things, and where the problem lies in the code. The alternativites that I suggested would excercise any of these internal differences (if they did in fact happen to exist), and may or may not be a workaround, but that will never be known until they are tried. I do not recall how to control the draw width If I remember correctly, the fills may be done with the D10 aperature, but I cannot remember why I remember it that way (may just be another neural failure). You can build up pads with fine draws if you really need them, as part of the library part, I've done this for critical RF parts. Yes, it's a pain As to whether or not it is necessary for a particular design, that's an RF engineering decision that is outside my realm. I'm told that it might be important in some cases. Yes, some of these little things really do matter. What I really want to know is what was the radius of the rounding of the corners of the pads to begin with, and whether or not any of the other suggestions offered in this thread were tried by Daniel and whether any of them worked. Daniel, what's the status. JaMi Smith * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:proteledaforum;techservinc.com * * To leave this list visit: * http://www.techservinc.com/protelusers/leave.html * * Contact the list manager: * mailto:ForumAdministrator;TechServInc.com * * Forum Guidelines Rules: * http://www.techservinc.com/protelusers/forumrules.html * * Browse or Search previous postings: * http://www.mail-archive.com/proteledaforum;techservinc.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] 45 degree pad problem !
That's how the life goes... --- Abd ulRahman Lomax [EMAIL PROTECTED] wrote: The best way to learn is to make mistakes. To learn big, make big mistakes. __ Do you Yahoo!? Y! Web Hosting - Let the expert host your web site http://webhosting.yahoo.com/ * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:proteledaforum;techservinc.com * * To leave this list visit: * http://www.techservinc.com/protelusers/leave.html * * Contact the list manager: * mailto:ForumAdministrator;TechServInc.com * * Forum Guidelines Rules: * http://www.techservinc.com/protelusers/forumrules.html * * Browse or Search previous postings: * http://www.mail-archive.com/proteledaforum;techservinc.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] 45 degree pad problem !
The best way to learn is to make mistakes. To learn big, make big mistakes. (Of course that isn't the whole story!) At 12:29 PM 10/16/2002 -0700, JaMi Smith wrote: Even if it is done at gerber time, it may make a difference in how Protel defines the pad to the gerber file based upon whether it is encountered as part of the design or part of a component, either of which should be different than a fill which it will most certainly draw. There are a couple of misconceptions here. Protel does not understand RS-274X rotations. It has been recommended that this be fixed! Fills are normally created by using a flash. I.e., Protel treats a fill, which is always rectangular, as if it were a rectangular pad. It creates an aperture for it. However, because Protel can't rotate this, it must draw rotated non-circular pads. I do not recall how to control the draw width You can build up pads with fine draws if you really need them, as part of the library part, I've done this for critical RF parts. Yes, it's a pain As to whether or not it is necessary for a particular design, that's an RF engineering decision that is outside my realm. I'm told that it might be important in some cases. 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 www.lomaxdesign.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:proteledaforum;techservinc.com * * To leave this list visit: * http://www.techservinc.com/protelusers/leave.html * * Contact the list manager: * mailto:ForumAdministrator;TechServInc.com * * Forum Guidelines Rules: * http://www.techservinc.com/protelusers/forumrules.html * * Browse or Search previous postings: * http://www.mail-archive.com/proteledaforum;techservinc.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] 45 degree pad problem !
Morning All: I have placed some rectangular pads on a 45 degree angle to accomodate a microstrip design. The problem is that when I generate gerbers, these pads on an angle have rounded corners. This changes copper layout enough to be a problem for my RF design. I am wondering if there is a setting in the gerber generation properties that can be changed to correct this problem. Anyone have a solution ? Thanks, Daniel Webster 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 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] 45 degree pad problem !
Daniel, I am assuming that you are placing the pad in the design, and then made it rectangular and changed its rotation. Have you tried making the rectangular pad as a component, and then placing it and rotating it, or alternatly, rotating the pad within the component itself. Yet another approach would be placing a Fill, and then rotating it, either directly in the design, or once again within a component. JaMi Smith - Original Message - From: Daniel Webster [EMAIL PROTECTED] To: 'Protel EDA Forum' [EMAIL PROTECTED] Sent: Wednesday, October 16, 2002 10:41 AM Subject: Re: [PEDA] 45 degree pad problem ! Morning All: I have placed some rectangular pads on a 45 degree angle to accomodate a microstrip design. The problem is that when I generate gerbers, these pads on an angle have rounded corners. This changes copper layout enough to be a problem for my RF design. I am wondering if there is a setting in the gerber generation properties that can be changed to correct this problem. Anyone have a solution ? Thanks, Daniel Webster 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 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] 45 degree pad problem !
Daniel, I don't believe there is any fix for this problem. One Work-around that 'doesn't' work is to place a fill of the appropriate size and shape over the pad because when Gerbered the fill also gets drawn instead of flashed. I have usually found that the draw was with such a small aperture that it didn't round the corners very much. How much is yours being rounded, what size is the pad, what size aperture is used in the drawn Gerber? I would expect the pad is being drawn with an aperture of 10mil or less, then that is only a 5 mil radius. Is your engineer being too paranoid, our engineers have never worried about such minute details even at 35 - 40GHz? 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 Norsat's Microwave Products Division has now achieved ISO 9001:2000 certification -Original Message- From: Daniel Webster [mailto:[EMAIL PROTECTED]] Sent: Wednesday, October 16, 2002 10:42 AM To: 'Protel EDA Forum' Subject: Re: [PEDA] 45 degree pad problem ! Morning All: I have placed some rectangular pads on a 45 degree angle to accomodate a microstrip design. The problem is that when I generate gerbers, these pads on an angle have rounded corners. This changes copper layout enough to be a problem for my RF design. I am wondering if there is a setting in the gerber generation properties that can be changed to correct this problem. Anyone have a solution ? Thanks, Daniel Webster 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 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] 45 degree pad problem !
Jami, doesn't matter how you do it, Protel draws rotated pads or fills when gerbered. 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 Norsat's Microwave Products Division has now achieved ISO 9001:2000 certification -Original Message- From: JaMi Smith [mailto:[EMAIL PROTECTED]] Sent: Wednesday, October 16, 2002 11:14 AM To: Protel EDA Forum Cc: JaMi Smith Subject: Re: [PEDA] 45 degree pad problem ! Daniel, I am assuming that you are placing the pad in the design, and then made it rectangular and changed its rotation. Have you tried making the rectangular pad as a component, and then placing it and rotating it, or alternatly, rotating the pad within the component itself. Yet another approach would be placing a Fill, and then rotating it, either directly in the design, or once again within a component. JaMi Smith * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] 45 degree pad problem !
- Original Message - From: Brad Velander [EMAIL PROTECTED] To: 'Protel EDA Forum' [EMAIL PROTECTED] Sent: Wednesday, October 16, 2002 11:32 AM Subject: Re: [PEDA] 45 degree pad problem ! Jami, doesn't matter how you do it, Protel draws rotated pads or fills when gerbered. 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 Norsat's Microwave Products Division has now achieved ISO 9001:2000 certification -Original Message- From: JaMi Smith [mailto:[EMAIL PROTECTED]] Sent: Wednesday, October 16, 2002 11:14 AM To: Protel EDA Forum Cc: JaMi Smith Subject: Re: [PEDA] 45 degree pad problem ! Daniel, I am assuming that you are placing the pad in the design, and then made it rectangular and changed its rotation. Have you tried making the rectangular pad as a component, and then placing it and rotating it, or alternatly, rotating the pad within the component itself. Yet another approach would be placing a Fill, and then rotating it, either directly in the design, or once again within a component. JaMi Smith * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] 45 degree pad problem !
Oops . . . I'll try again with a message this time . . . anyway, it's Wenesday, and my brain only functions on Tuesdays and Thursdays. I just thought that it might make a difference in how it is handled based on where it is encountered, and also if it was a fill verses a pad. Even if it is done at gerber time, it may make a difference in how Protel defines the pad to the gerber file based upon whether it is encountered as part of the design or part of a component, either of which should be different than a fill which it will most certainly draw. Other than that it sounds like it is being drawn with the wrong size aperature, possibly too large. Oh well, thats all I can think of on a Wenesday . . . Thanks, JaMi - Original Message - From: Brad Velander [EMAIL PROTECTED] To: 'Protel EDA Forum' [EMAIL PROTECTED] Sent: Wednesday, October 16, 2002 11:32 AM Subject: Re: [PEDA] 45 degree pad problem ! Jami, doesn't matter how you do it, Protel draws rotated pads or fills when gerbered. 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 Norsat's Microwave Products Division has now achieved ISO 9001:2000 certification -Original Message- From: JaMi Smith [mailto:[EMAIL PROTECTED]] Sent: Wednesday, October 16, 2002 11:14 AM To: Protel EDA Forum Cc: JaMi Smith Subject: Re: [PEDA] 45 degree pad problem ! Daniel, I am assuming that you are placing the pad in the design, and then made it rectangular and changed its rotation. Have you tried making the rectangular pad as a component, and then placing it and rotating it, or alternatly, rotating the pad within the component itself. Yet another approach would be placing a Fill, and then rotating it, either directly in the design, or once again within a component. JaMi Smith * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] 45 degree pad problem !
On 11:31 AM 16/10/2002 -0700, Brad Velander said: Daniel, I don't believe there is any fix for this problem. One Work-around that 'doesn't' work is to place a fill of the appropriate size and shape over the pad because when Gerbered the fill also gets drawn instead of flashed. I have usually found that the draw was with such a small aperture that it didn't round the corners very much. How much is yours being rounded, what size is the pad, what size aperture is used in the drawn Gerber? I would expect the pad is being drawn with an aperture of 10mil or less, then that is only a 5 mil radius. Is your engineer being too paranoid, our engineers have never worried about such minute details even at 35 - 40GHz? Brad, I think there may be a sort of fix. One fix is to ensure there is a smaller aperture in your design. Add in a 2mil string somewhere (on a mech layer) to force inclusion of a 2-mill apt and it should paint the corners with this smaller apt. At least this was how you could improve things way back in the Autotrax days (by including a small apt in the apt file) - the current pad and fill drawing code may well be similar. I haven't tested this to confirm the old behavior. In general Protel will flash what it can, but some things will be drawn, and I believe with the smallest available apt - but I could be wrong. A nice option would be to allow the pad and fill drawing code to request an apt, size set by the user, if only larger ones are used elsewhere in the design. So you could control the maximum radii of corners. If I was really fussed about repeatable boards, I would run a track on the outside of my fill to make sure that *all* plotted versions looked the same. Nothing was left to chance. It would mean all rotated fills had, controlled, rounded corners. A pain with rotated pads if there are lots of them. Bye for now, Ian * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
