Re: [PEDA] [dxp] Control Thermal Reliefs by Area
At 06:48 PM 1/8/2004, Dom Bragge wrote: Further to this (somewhat harking back to the old days - process tends to improve over time) there is quite a deal of XY expansion in the copper planes, especially during wave soldering, which can lead to cracks forming at the knee (where a copper plane turns 90degrees & continues down the hole). This is more prevalent in plane to hole connections than when compared to a small track (or multiple small tracks i.e. thermal relief) are used. Yes a thermal relief also allows mechanical strain relief in this situation. I'm a bit skeptical about this as applied to inner plane connections (which is what we've been discussing, not external copper pours, which I'm not considering). If the hole is expanding, it would seem to me just as likely -- or more likely -- that a narrow track would crack than a solid connection. I.e., the hole expands, but the surrounding prepreg is cooler and does not expand as much, stressing the narrow track at the knee. Because copper is such a good conductor of heat, a broader connection, not thermally relieved, would, I'd think, cause the prepreg to heat up and expand more, thus reducing stress. Just my thoughts, not backed by any kind of serious study in this case. Has a study been done comparing thermally relieved vias vs. solid connection vias going to inner planes? Many times myths have become enshrined as standard practice simply because it seemed to be right to someone. The reality might be different. As mentioned, of course, from a noise perspective, solid connection of vias to power planes is generally better. As a minor benefit, the gerber files are smaller also :-) * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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/[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] [dxp] Control Thermal Reliefs by Area
Hamid A. Wasti wrote: One off topic question: Why would you ever want a via to connect to a power plane with a thermal relief? The thermal relief is to allow you to heat up the pins of an IC as you solder them in a through hole pad that is connected to a plane. Further to this (somewhat harking back to the old days - process tends to improve over time) there is quite a deal of XY expansion in the copper planes, especially during wave soldering, which can lead to cracks forming at the knee (where a copper plane turns 90degrees & continues down the hole). This is more prevalent in plane to hole connections than when compared to a small track (or multiple small tracks i.e. thermal relief) are used. Yes a thermal relief also allows mechanical strain relief in this situation. Of course, we all want less inductance in those vias & so there comes the trade off... -- Regards, Dom VK2JNA Dom Bragge, CID MIEEE | Silverbrook Research PL, PO Box 207 Snr PCB Layout Engr| Balmain NSW 2041, AUSTRALIA Ph +61-2-9818-6633xt163| [EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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/[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] [dxp] Control Thermal Reliefs by Area
At 01:58 AM 1/8/2004, JaMi Smith wrote: ... and while I too had never before investigateed the full list allowed by the slider, right there at the bottom is what I am looking for This is an example of why I consider it quite useful when I make a public mistake. I'm not entirely dim, at least not yet, and when I err, often there are others who have similarly overlooked something, and exposing it helps all of us. (I had been aware of the additional scope possibilities in the past, I had used them, I just didn't see them when I looked into it while writing my post) * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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/[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] [dxp] Control Thermal Reliefs by Area
At 01:58 AM 1/8/2004, JaMi Smith wrote: It would have been nice to be able to just "select" a single via, as it appears that you can do with pads. There are at least four ways, one of which you noted. As you mentioned, one can create a via different in diameter or hole size (better the former), and then use via specification scope. One can use the net to affect all vias on that particular net. (But one should probably have all vias set for direct connect anyway. That ought to be the Protel default. A situation would be rare where the best solution is to thermal-relieve a via.) One can use a free pad instead of a via; that way one can name the little beastie, and one can create as many varieties as you like. And one can define a region which is tight around the via. Back to the Area question, the "Region" seems to be the answer. "Footprint" won't work with a BGA, since most vias related to a BGA are actually free vias, which are part of the fanout, and not the "Footprint". If the fanout is part of the library part, they should be affected by Footprint scope. If not, there might be some combination scope (i.e., Footprint = X and Via Specification). But, really, one ought to direct-connect all vias, I can't think of a reason not to do it. Now the only question is can I do this in DXP? I'd be astonished if it couldn't be. But it is not clear to me how to do it. The question really should be asked on the DXP list, but I think Mr. Smith, if I recall correctly, may have burned his bridges there For me, the matter of interest is that it is not easy to figure out how to do it in DXP. Maybe I should read the manual, a cursory scan did not pick up the needed information. I'm pretty sure that the procedure would be to define a Query that selects the objects in question. That I can do with Vias generically, which would solve the present problem. However, some of the possible scopes in 99SE seem to be missing in DXP, in the Query Builder (under Edit). There may well be some way to manually create them, but, again, this is already a fair amount of work compared to the few keystrokes required in 99SE. But the query in the Rule Wizard (Advanced/Start with a blank Query) has even fewer scope options than the already reduced set in Query Builder. I've suggested in the past that there be a user panel to provide suggestions and guidance to Protel as they chart the future of the software, and I know the matter was under consideration. The Query technique is a great idea, conceptually. But I don't think it was necessary to kill the old functionality in order to implement the idea, and a user panel would almost certainly have recommended keeping it, at least as an option, or would have otherwise ensured that (1) full functionality and efficiency was maintained, and (2) retraining was made relatively painless. The situation *should* have been as the salesperson claimed, and I see no reason why that could not have been done. It could still be done, not all the horses have left the barn. The user panel should be chosen by users; its function would be advisory; Protel would necessarily retain, however, veto power over nominations to the panel, though I doubt that users would recommend members for the panel who would necessitate vetos. (Veto would properly be exercised where there was a concern regarding non-disclosure; being a hard critic of Protel would not necessarily disqualify one, and, in fact, listening to the hardest critics can be very useful. But if a critic was so angry that non-disclosure or advisory process were threatened, yes, exclusion would be appropriate.) I do have ideas as to how users could *all* be represented on the panel if they so choose Imagine what it would be like if the company could communicate with its users as if they were a single customer. There are those who think this would be hard on the company, but, personally, I prefer to have intelligent customers who know what they want and who are also amenable to suggestions. They are much easier to please than a faceless crowd. * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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/[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] [dxp] Control Thermal Reliefs by Area
JaMi Smith wrote: the ability to apply the rule directly to a single via, which appears to be the one thing that is not in the list, although I guess that I could make a seperate via-specification that had a very very slightly different sized pad, and place it where I wanted the my "no-connect" via. That is the simplest solution to the problem. The via specifications allow you to select on a large number of parameters. You can vary the via diameter by 0.1 mil for the no-connect rule. One off topic question: Why would you ever want a via to connect to a power plane with a thermal relief? The thermal relief is to allow you to heat up the pins of an IC as you solder them in a through hole pad that is connected to a plane. By the time your via goes through a trace to connect to a surface mount pad, you are already far enough removed from the plane that you do not need a thermal relief. Now the only question is can I do this in DXP? My first reaction is to respond with "Fat chance" But since I don't know DXP well enough, I will instead respond with: "Good luck" Hamid * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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/[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] [dxp] Control Thermal Reliefs by Area
Abd and Hamid Ok, Protel 99 SE, I had a little trouble following all of that at first, but actually got in there and started playing around with the scope of the rule for Power Plane Connect Style, and while I too had never before investigateed the full list allowed by the slider, right there at the bottom is what I am looking for, which is "Region", and while it takes a little bit of work to set it up, that is just what I was looking for. This also appears to possibly be the answer to the "No Connect" situation I inquired about in a parallel post, since I can set up special rule for "no-connect", although the one thing that I was looking for there in the "scope", was the ability to apply the rule directly to a single via, which appears to be the one thing that is not in the list, although I guess that I could make a seperate via-specification that had a very very slightly different sized pad, and place it where I wanted the my "no-connect" via. It would have been nice to be able to just "select" a single via, as it appears that you can do with pads. Back to the Area question, the "Region" seems to be the answer. "Footprint" won't work with a BGA, since most vias related to a BGA are actually free vias, which are part of the fanout, and not the "Footprint". Now the only question is can I do this in DXP? Thanks, JaMi - Original Message - From: "Abd ulRahman Lomax" <[EMAIL PROTECTED]> To: "Protel EDA Forum" <[EMAIL PROTECTED]> Sent: Wednesday, January 07, 2004 8:25 PM Subject: Re: [PEDA] [dxp] Control Thermal Reliefs by Area > At 10:26 PM 1/7/2004, Hamid A. Wasti wrote: > >Abd ul-Rahman Lomax wrote: > >>In 99SE, this would be controlled by a Design Rule, and the choices for > >>scope are Board, Footprint, Component/Class, Net/Class, Pad Class and > >>Specification. I'm a little surprised not to see "via" there > > > >Look harder. It is there and always has been. It is located just below > >"Pad Specification" > > duh. as is the rest, i.e., Via Specification, Footprint-Pad, and Region. I > overlooked the slider > > >>Now, in DXP, it seems to be a little more complicated. > > > >I looked and could not come up with a way to do it, so I gave up after > >wasting an hour. So much for the claim by the Protel sales person that if > >you are an experienced user of 99SE, there is absolutely no learning curve > >to be just as productive in DXP. > > I'd say that was puffery. > > > A learning curve is involved only if you chose to take advantage of > > additional powerful features. Would you call that a blatant lie, an > > ignoramus telling the truth as he knew it, or in our politically correct > > world a poor victim of capitalist society merely taking liberties with > > the truth in order to earn enough commission to feed his family? > > I'd say somewhere between the second and the last, it can be hard to tell > the difference (though I don't know if Protel salespeople get commissions). > It is not entirely false, i.e., much of the basic functionality is the > same, but enough functions have changed in some way to cause delay as one > figures out how to do it in DXP. How much impact this has on productivity, > I can't personally say, because I haven't pushed a job through DXP yet. But > it will have an impact in the short term, I have no doubt. > > In real life, I'd ask the question on the DXP list, not here, if I wanted > to get the fastest and best answers. > > >What I was specifically trying to do in DXP was to have all vias connect > >to the planes without thermal reliefs. > > Well, I defined a via specification scope direct-connect rule in 99SE > (unchecking all the specifications so that it applied to all vias), then I > imported the board to DXP. I did get a rule with the same name, but the > scope did not mention vias... just All. > > And I don't see via or pad scopes in DXP Power Plane Connection Style > rules. What am I missing? > > (In 99SE, to reiterate, one may, for example, give free pads a PadName and > then use Free-PadName in the scope, allowing one to control connection > style and other characteristics like Solder Mask Expansion, pad-by-pad > simply by editing the pad name. Or one could have one size of via that is, > say, tented, and one size that is not.) > > The DXP way, as I understand it, would be to create a Query that selects > the objects to be affected by the rule. I can create a Query that selects > Vias with the Build Query command, but I don't see how to connect this with > the Rule, the "Query Builder" button in t
Re: [PEDA] [dxp] Control Thermal Reliefs by Area
AbdulRahman Lomax wrote: And I'm not thrilled that the rule from the 99SE file did not survive import. What one needs to be more scared about, if that is indeed the case, is that it did not survive import and did not generate a warning. I experienced power objects quietly disappearing on the one transfer I did of a 4 sheet schematic from 99SE to DXP -- my sole experience moving anything into DXP. If you import a board with 1000+ components, 3000+ vias, 100+ rules, almost 20 split planes, you can not possibly check everything and make sure everything came across perfectly. All it takes is one ignored item to make the board unusable. The cost of bare boards, the cost of having them assembled and tested, the cost of your time, the cost of schedule delays... add them all up and the $8K new price for DXP is lost in the noise. Did I mention that Protel sales person told me that they have a very reliable import utility with which you could import any 99SE design into DXP and just continue on after you manually handled the split planes? Hamid * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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/[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] [dxp] Control Thermal Reliefs by Area
At 10:26 PM 1/7/2004, Hamid A. Wasti wrote: Abd ul-Rahman Lomax wrote: In 99SE, this would be controlled by a Design Rule, and the choices for scope are Board, Footprint, Component/Class, Net/Class, Pad Class and Specification. I'm a little surprised not to see "via" there Look harder. It is there and always has been. It is located just below "Pad Specification" duh. as is the rest, i.e., Via Specification, Footprint-Pad, and Region. I overlooked the slider Now, in DXP, it seems to be a little more complicated. I looked and could not come up with a way to do it, so I gave up after wasting an hour. So much for the claim by the Protel sales person that if you are an experienced user of 99SE, there is absolutely no learning curve to be just as productive in DXP. I'd say that was puffery. A learning curve is involved only if you chose to take advantage of additional powerful features. Would you call that a blatant lie, an ignoramus telling the truth as he knew it, or in our politically correct world a poor victim of capitalist society merely taking liberties with the truth in order to earn enough commission to feed his family? I'd say somewhere between the second and the last, it can be hard to tell the difference (though I don't know if Protel salespeople get commissions). It is not entirely false, i.e., much of the basic functionality is the same, but enough functions have changed in some way to cause delay as one figures out how to do it in DXP. How much impact this has on productivity, I can't personally say, because I haven't pushed a job through DXP yet. But it will have an impact in the short term, I have no doubt. In real life, I'd ask the question on the DXP list, not here, if I wanted to get the fastest and best answers. What I was specifically trying to do in DXP was to have all vias connect to the planes without thermal reliefs. Well, I defined a via specification scope direct-connect rule in 99SE (unchecking all the specifications so that it applied to all vias), then I imported the board to DXP. I did get a rule with the same name, but the scope did not mention vias... just All. And I don't see via or pad scopes in DXP Power Plane Connection Style rules. What am I missing? (In 99SE, to reiterate, one may, for example, give free pads a PadName and then use Free-PadName in the scope, allowing one to control connection style and other characteristics like Solder Mask Expansion, pad-by-pad simply by editing the pad name. Or one could have one size of via that is, say, tented, and one size that is not.) The DXP way, as I understand it, would be to create a Query that selects the objects to be affected by the rule. I can create a Query that selects Vias with the Build Query command, but I don't see how to connect this with the Rule, the "Query Builder" button in the Rule window does pop up a query dialog, but the required options (Via, for example) are not there There has got to be a way. If I were trying to get a job out, having managed to get it designed in DXP and now I'm just trying to finish the details, I'd be fairly upset! (And, as I said, I'd ask on the DXP list. But my own motive here is to explore a bit what it is like to move to DXP as an old hand with 99SE, to find the rough edges.) And I'm not thrilled that the rule from the 99SE file did not survive import. (But maybe it did and I'm just not understanding what I'm seeing) * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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/[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] [dxp] Control Thermal Reliefs by Area
Abd ul-Rahman Lomax wrote: At 02:14 PM 1/7/2004, you wrote: Is there a way to define whether or not connections to Planes get a Thermal Relief, and if so, what type, by the area of the Board in which they occur? In 99SE, this would be controlled by a Design Rule, and the choices for scope are Board, Footprint, Component/Class, Net/Class, Pad Class and Specification. I'm a little surprised not to see "via" there Look harder. It is there and always has been. It is located just below "Pad Specification" But, no, there was no region scope. Yes there is, 3 items below "Via Specification" Are you talking about DesignRules->Manufacturing->PowerPlaneConnection rules or something else? Now, in DXP, it seems to be a little more complicated. I looked and could not come up with a way to do it, so I gave up after wasting an hour. So much for the claim by the Protel sales person that if you are an experienced user of 99SE, there is absolutely no learning curve to be just as productive in DXP. A learning curve is involved only if you chose to take advantage of additional powerful features. Would you call that a blatant lie, an ignoramus telling the truth as he knew it, or in our politically correct world a poor victim of capitalist society merely taking liberties with the truth in order to earn enough commission to feed his family? What I was specifically trying to do in DXP was to have all vias connect to the planes without thermal reliefs. Hamid * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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/[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] [dxp] Control Thermal Reliefs by Area
At 02:14 PM 1/7/2004, you wrote: Is there a way to define whether or not connections to Planes get a Thermal Relief, and if so, what type, by the area of the Board in which they occur? In 99SE, this would be controlled by a Design Rule, and the choices for scope are Board, Footprint, Component/Class, Net/Class, Pad Class and Specification. I'm a little surprised not to see "via" there But, no, there was no region scope. I am thinking specifically about the area under a BGA, where I may not want Thermal Reliefs, or possibly may want a mixture. Can this be controlled to physical Dimensions with Rooms? This is a DXP question, but staying with 99SE for a moment, why would you want to do this? If the pads in question are part of a footprint, footprint scope would cover it. Now, in DXP, it seems to be a little more complicated. I'm still a DXP newbie, and it is in looking at matters like this that I am dismayed; I have to learn quite a bit to use DXP, this is pretty well known. Scope in DXP is defined by Query, and that I do not find nearly as simple as the old way. Powerful, probably Perhaps someone will explain how to do, for example, a footprint scope rule for power plane connections in DXP. The queries given in the query wizard don't include such an option as far as I can see. * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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/[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
