Re: gEDA-user: Thermals on Pads
On Sun, 2011-01-30 at 12:54 -0700, asom...@gmail.com wrote: > When I design surface mount boards I make extensive use of planes, and > it is a severe annoyance that I can't automatically connect those > planes to component pads. The standard solutions to this problem seem > to be either: What is wrong with a track segment which you "join" to the polygon with the "j" hotkey? (Were you aware of that one?) When it comes to auto-thermal'ing pads, one has a lot of possible choices of trace thickness, orientation etc.. and it is not obvious whether an auto-thermal would be an easy thing to do. IMO, what we "want" is an auto-join based on connectivity. (Lets presume we can mark the plane as "belonging" to the GND net.. draw a trace which connects to a pad which belongs to that net and it should quite probably join up (by default). NB: Sometimes one deliberately routes a track belonging to the same "net" separately - 4 terminal current sensing springs to mind, where big polygons might make up the power traces. -- Peter Clifton Electrical Engineering Division, Engineering Department, University of Cambridge, 9, JJ Thomson Avenue, Cambridge CB3 0FA Tel: +44 (0)7729 980173 - (No signal in the lab!) Tel: +44 (0)1223 748328 - (Shared lab phone, ask for me) signature.asc Description: This is a digitally signed message part ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Thermals on Pads
On Mon, 2011-01-31 at 13:09 -0700, asom...@gmail.com wrote: > The IPC- table of contents shows that "Thermal Relief in Conductor > Planes" gets only one tenth of a page. I can't imagine any detailed > information in that space. It's sister document, IPC-2221, can be > found for free at > http://www.victronics.cl/Inf_tecnica/Notas%20de%20aplicacion/PCBs/IPC-2221(L).pdf (You're not supposed to though.. IPC charge for their standards!) Thanks to those who've quoted me text from their copies of the standards.. I've the info I was looking for. Basically they suggest web width be about 60% of the minimum acceptable land diameter for the part.. DIVIDED by the number of webs in use. They also stipulate how the webs should SHRINK if you make the pad bigger than the minimum allowable size, and give a limit for the total width of web over all planes. What they don't say is how to calculate the clearance (obviously important for thermal conductivity to the plane), nor whether there is any special relationship between clearance and web width. (Implied not, since they provide explicit guidelines for web width). Clearly attributes are the way forward - let the user fiddle.. but I would also like to see it possible for a thermal to be recognised as "default" in some way.. and scale with other geometry. Perhaps this is me just making things more complex than necessary. The good old-fashioned +,x thermals with no rounding are the nicest in my opinion ;) I'm told by an industry source that some fab's (high end ones perhaps?), don't always produce an exact 1:1 match between the design geometry you send them and what they produce. THEY will know how to do thermals in a way which suits THEIR soldering process, so they may modify things in their own CAD software. Conveying the _intent_ of the design is what you need to do. For the cheap (or DIY) end of the fab market we often serve - I think we should assume that we get what our design files ask for, even if it is silly! For my money, Fully parametrised thermals will basically boil down to arbitrary polygons built up from things we can teach PCB how to do.. such as webs. I want to see support for arbitrary web count, web geometry and web positioning.. (How this works for square.. I don't know). Ideally, square pads would connect coming in at the corner of the square pad, or employ a tear-drop for extra robustness against drill breakout. Since this could get complex quickly - I wonder if we ought to at this stage start doing these by reference.. include the thermal design ONCE, and reference it by name on pads which use it. Best wishes, -- Peter Clifton Electrical Engineering Division, Engineering Department, University of Cambridge, 9, JJ Thomson Avenue, Cambridge CB3 0FA Tel: +44 (0)7729 980173 - (No signal in the lab!) Tel: +44 (0)1223 748328 - (Shared lab phone, ask for me) signature.asc Description: This is a digitally signed message part ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Thermals on Pads
The IPC- table of contents shows that "Thermal Relief in Conductor Planes" gets only one tenth of a page. I can't imagine any detailed information in that space. It's sister document, IPC-2221, can be found for free at http://www.victronics.cl/Inf_tecnica/Notas%20de%20aplicacion/PCBs/IPC-2221(L).pdf . IPC-2221 has a section on thermal relief, but without any useful details. On Sun, Jan 30, 2011 at 2:20 PM, Peter Clifton wrote: > On Sun, 2011-01-30 at 20:39 +, Peter Clifton wrote: >> I've been looking at some brokenness with our normal thermal shape >> generation recently, so if I get a chance I could look at your patch - >> and possibly work from it. > > The only reference to geometry I've found so far is: > > http://www.pcbwizards.com/Glossary20.htm > > And IPC-. (Which I don't have a copy of). > > Anyone have access to a copy? > > -- > Peter Clifton > > Electrical Engineering Division, > Engineering Department, > University of Cambridge, > 9, JJ Thomson Avenue, > Cambridge > CB3 0FA > > Tel: +44 (0)7729 980173 - (No signal in the lab!) > Tel: +44 (0)1223 748328 - (Shared lab phone, ask for me) > > > > ___ > geda-user mailing list > geda-user@moria.seul.org > http://www.seul.org/cgi-bin/mailman/listinfo/geda-user > > ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Thermals on Pads
Hi, > -Original Message- > From: geda-user-boun...@moria.seul.org > [mailto:geda-user-boun...@moria.seul.org] On Behalf Of rickman > Sent: Monday, January 31, 2011 5:11 PM > To: gEDA user mailing list > Subject: Re: gEDA-user: Thermals on Pads > > On 1/31/2011 10:33 AM, Martin Kupec wrote: > > On Sun, Jan 30, 2011 at 11:13:27PM -0500, rickman wrote: > >> On 1/30/2011 4:47 PM, Martin Kupec wrote: > >>> On Sun, Jan 30, 2011 at 04:37:17PM -0500, rickman wrote: > >>>> What geometry problems do you have? There are plenty of > references > >>>> in regard to thermals. I don't recall seeing any other than > >>>> bridges that span a uniform gap around the pad. The > only variation I can recall is > >>>> the number and rotation angle of the pattern. But > most, if not all > >>>> that I have seen use four bars either along the x and y > axes or at > >>>> 45 degree angles. I think there are even some built in commands > >>>> for this in the RS-274X Gerber file spec. > >>>> > >>>> Or am I missing something? > >>> We already do support bridges with rounded corners. And > what we do > >>> not support is anything suitable for TSOP package pads(long thin > >>> pads near to each other). > >>> > >>> But the big problem with you current implementations is > the size of > >>> the bridges. The size is somewhat magicaly calculated > from the size > >>> of pin and from the size of clerance. But this is > neighter working > >>> nor probably right. > >>> > >>> With big clerance the shape becomes completly bogus(at > least for the > >>> rounded versions). > >> That surprises me that the bridge width would be calculated rather > >> than specified. What's the idea behind that? Isn't it a simple > >> matter to let the designer pick the dimensions both for > the width of > >> the bridge and the width of the clearance? > > I would not argue against it. > > > > So shall we change the code in a way, that older files gets current > > calculation and newer ones has thermal specification in file? > > > > This opens discussion how/what to specify. > > > > Martin Kupec > > Is there a way to support both compatibly? If the data is to > be specified, it will need to be stored in the design file. > If that info is there, use it, if the info is not present let > the software determine the values be used? I would think the > only issue is determining a file format that would allow the > info to be optional yet compatible with existing formats > without the info. > > Rick > > Maybe use attributes here ? Just my EUR 0.02 Kind regards, Bert Timmerman. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Thermals on Pads
On 1/31/2011 10:33 AM, Martin Kupec wrote: On Sun, Jan 30, 2011 at 11:13:27PM -0500, rickman wrote: On 1/30/2011 4:47 PM, Martin Kupec wrote: On Sun, Jan 30, 2011 at 04:37:17PM -0500, rickman wrote: What geometry problems do you have? There are plenty of references in regard to thermals. I don't recall seeing any other than bridges that span a uniform gap around the pad. The only variation I can recall is the number and rotation angle of the pattern. But most, if not all that I have seen use four bars either along the x and y axes or at 45 degree angles. I think there are even some built in commands for this in the RS-274X Gerber file spec. Or am I missing something? We already do support bridges with rounded corners. And what we do not support is anything suitable for TSOP package pads(long thin pads near to each other). But the big problem with you current implementations is the size of the bridges. The size is somewhat magicaly calculated from the size of pin and from the size of clerance. But this is neighter working nor probably right. With big clerance the shape becomes completly bogus(at least for the rounded versions). That surprises me that the bridge width would be calculated rather than specified. What's the idea behind that? Isn't it a simple matter to let the designer pick the dimensions both for the width of the bridge and the width of the clearance? I would not argue against it. So shall we change the code in a way, that older files gets current calculation and newer ones has thermal specification in file? This opens discussion how/what to specify. Martin Kupec Is there a way to support both compatibly? If the data is to be specified, it will need to be stored in the design file. If that info is there, use it, if the info is not present let the software determine the values be used? I would think the only issue is determining a file format that would allow the info to be optional yet compatible with existing formats without the info. Rick ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Thermals on Pads
On Sun, Jan 30, 2011 at 11:13:27PM -0500, rickman wrote: > On 1/30/2011 4:47 PM, Martin Kupec wrote: > > On Sun, Jan 30, 2011 at 04:37:17PM -0500, rickman wrote: > >> What geometry problems do you have? There are plenty of references in > >> regard to thermals. I don't recall seeing any other than bridges that > >> span a uniform gap around the pad. The only variation I can recall is > >> the number and rotation angle of the pattern. But most, if not all > >> that I have seen use four bars either along the x and y axes or at 45 > >> degree angles. I think there are even some built in commands for this > >> in the RS-274X Gerber file spec. > >> > >> Or am I missing something? > > We already do support bridges with rounded corners. And what we > > do not support is anything suitable for TSOP package pads(long thin pads > > near to each other). > > > > But the big problem with you current implementations is the size of the > > bridges. The size is somewhat magicaly calculated from the size of pin > > and from the size of clerance. But this is neighter working nor probably > > right. > > > > With big clerance the shape becomes completly bogus(at least for the > > rounded versions). > > That surprises me that the bridge width would be calculated rather than > specified. What's the idea behind that? Isn't it a simple matter to > let the designer pick the dimensions both for the width of the bridge > and the width of the clearance? I would not argue against it. So shall we change the code in a way, that older files gets current calculation and newer ones has thermal specification in file? This opens discussion how/what to specify. Martin Kupec ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Thermals on Pads
On 1/30/2011 4:47 PM, Martin Kupec wrote: On Sun, Jan 30, 2011 at 04:37:17PM -0500, rickman wrote: What geometry problems do you have? There are plenty of references in regard to thermals. I don't recall seeing any other than bridges that span a uniform gap around the pad. The only variation I can recall is the number and rotation angle of the pattern. But most, if not all that I have seen use four bars either along the x and y axes or at 45 degree angles. I think there are even some built in commands for this in the RS-274X Gerber file spec. Or am I missing something? We already do support bridges with rounded corners. And what we do not support is anything suitable for TSOP package pads(long thin pads near to each other). But the big problem with you current implementations is the size of the bridges. The size is somewhat magicaly calculated from the size of pin and from the size of clerance. But this is neighter working nor probably right. With big clerance the shape becomes completly bogus(at least for the rounded versions). That surprises me that the bridge width would be calculated rather than specified. What's the idea behind that? Isn't it a simple matter to let the designer pick the dimensions both for the width of the bridge and the width of the clearance? Rick ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Thermals on Pads
On Sun, 2011-01-30 at 16:37 -0500, rickman wrote: > > > What geometry problems do you have? There are plenty of references > in > regard to thermals. I don't recall seeing any other than bridges > that > span a uniform gap around the pad. The only variation I can recall > is > the number and rotation angle of the pattern. But most, if not all > that I have seen use four bars either along the x and y axes or at 45 > degree angles. I think there are even some built in commands for > this > in the RS-274X Gerber file spec. Firstly, the general shape is not so much the problem, but dimensions of the shape. Second - PCB calculates what it thinks the thermal finger width should be, but actually calculates the geometry wrong - so the thermal you see is not what the calculation PCB does suggests it should be This is evident at certain clearance sizes, where the thermal cutouts start to overlap and cause polygon problems. At some geometries, the general shape is wrong - we need to restrict some of the dimensioning to keep the thermal shape valid, or add routines for a different thermal shape in these cases. > -- Peter Clifton Electrical Engineering Division, Engineering Department, University of Cambridge, 9, JJ Thomson Avenue, Cambridge CB3 0FA Tel: +44 (0)7729 980173 - (No signal in the lab!) Tel: +44 (0)1223 748328 - (Shared lab phone, ask for me) signature.asc Description: This is a digitally signed message part ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Thermals on Pads
On Sun, Jan 30, 2011 at 04:37:17PM -0500, rickman wrote: > What geometry problems do you have? There are plenty of references in > regard to thermals. I don't recall seeing any other than bridges that > span a uniform gap around the pad. The only variation I can recall is > the number and rotation angle of the pattern. But most, if not all > that I have seen use four bars either along the x and y axes or at 45 > degree angles. I think there are even some built in commands for this > in the RS-274X Gerber file spec. > > Or am I missing something? We already do support bridges with rounded corners. And what we do not support is anything suitable for TSOP package pads(long thin pads near to each other). But the big problem with you current implementations is the size of the bridges. The size is somewhat magicaly calculated from the size of pin and from the size of clerance. But this is neighter working nor probably right. With big clerance the shape becomes completly bogus(at least for the rounded versions). Martin Kupec ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Thermals on Pads
On 1/30/2011 3:39 PM, Peter Clifton wrote: On Sun, 2011-01-30 at 21:12 +0100, Martin Kupec wrote: On Sun, Jan 30, 2011 at 12:54:23PM -0700, asom...@gmail.com wrote: I'm a novice to the pcb code base, and I couldn't find much developer documentation, but I am willing to try to add this feature. I need a little help though: the pcb code base is too large for me to grok all at once. Could someone please tell me where to start? What would I have to modify to allow this? Actualy, there already is a patch. It can be found here: https://bugs.launchpad.net/pcb/+bug/699495 This patch has some issues as mentioned in the bug report, but it should be usable. I am willing to fix and extend the patch, but I do have exams period(or how is the english word for it) :-( I should be on that issue in few weeks(like 2-3). I've been looking at some brokenness with our normal thermal shape generation recently, so if I get a chance I could look at your patch - and possibly work from it. The main problem I have is not code, but deciding what such geometry needs to look like it and how to specify it. Whatever we decide we have to live with, as we can't go changing geometry on users with existing boards. That is the problem I'm hitting now. Harry's clipper branch (a long time ago) without comment, changed the thermal generation formulas in (IMO, a retrograde way). I can't change it back (or fix the geometry calculation) for fear of possibly breaking all the users who have made boards since then. What geometry problems do you have? There are plenty of references in regard to thermals. I don't recall seeing any other than bridges that span a uniform gap around the pad. The only variation I can recall is the number and rotation angle of the pattern. But most, if not all that I have seen use four bars either along the x and y axes or at 45 degree angles. I think there are even some built in commands for this in the RS-274X Gerber file spec. Or am I missing something? Rick ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Thermals on Pads
On Sun, 2011-01-30 at 20:39 +, Peter Clifton wrote: > I've been looking at some brokenness with our normal thermal shape > generation recently, so if I get a chance I could look at your patch - > and possibly work from it. The only reference to geometry I've found so far is: http://www.pcbwizards.com/Glossary20.htm And IPC-. (Which I don't have a copy of). Anyone have access to a copy? -- Peter Clifton Electrical Engineering Division, Engineering Department, University of Cambridge, 9, JJ Thomson Avenue, Cambridge CB3 0FA Tel: +44 (0)7729 980173 - (No signal in the lab!) Tel: +44 (0)1223 748328 - (Shared lab phone, ask for me) signature.asc Description: This is a digitally signed message part ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Thermals on Pads
> The main problem I have is not code, but deciding what such geometry > needs to look like it and how to specify it. Whatever we decide we have > to live with, as we can't go changing geometry on users with existing > boards. I think it would be acceptable to change geometry on the community if it happens at the same time as a new version of the PCB file format. That way PCB files in old file formats could have the old geometry (legacy mode), and newly created ones could have new geometry. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Thermals on Pads
On Sun, 2011-01-30 at 21:12 +0100, Martin Kupec wrote: > On Sun, Jan 30, 2011 at 12:54:23PM -0700, asom...@gmail.com wrote: > > I'm a novice to the pcb code base, and I couldn't find much developer > > documentation, but I am willing to try to add this feature. I need a > > little help though: the pcb code base is too large for me to grok all > > at once. Could someone please tell me where to start? What would I > > have to modify to allow this? > > Actualy, there already is a patch. > It can be found here: https://bugs.launchpad.net/pcb/+bug/699495 > > This patch has some issues as mentioned in the bug report, but it should > be usable. > > I am willing to fix and extend the patch, but I do have exams period(or > how is the english word for it) :-( > I should be on that issue in few weeks(like 2-3). I've been looking at some brokenness with our normal thermal shape generation recently, so if I get a chance I could look at your patch - and possibly work from it. The main problem I have is not code, but deciding what such geometry needs to look like it and how to specify it. Whatever we decide we have to live with, as we can't go changing geometry on users with existing boards. That is the problem I'm hitting now. Harry's clipper branch (a long time ago) without comment, changed the thermal generation formulas in (IMO, a retrograde way). I can't change it back (or fix the geometry calculation) for fear of possibly breaking all the users who have made boards since then. -- Peter Clifton Electrical Engineering Division, Engineering Department, University of Cambridge, 9, JJ Thomson Avenue, Cambridge CB3 0FA Tel: +44 (0)7729 980173 - (No signal in the lab!) Tel: +44 (0)1223 748328 - (Shared lab phone, ask for me) signature.asc Description: This is a digitally signed message part ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Thermals on Pads
On Sun, Jan 30, 2011 at 12:54:23PM -0700, asom...@gmail.com wrote: > I'm a novice to the pcb code base, and I couldn't find much developer > documentation, but I am willing to try to add this feature. I need a > little help though: the pcb code base is too large for me to grok all > at once. Could someone please tell me where to start? What would I > have to modify to allow this? Actualy, there already is a patch. It can be found here: https://bugs.launchpad.net/pcb/+bug/699495 This patch has some issues as mentioned in the bug report, but it should be usable. I am willing to fix and extend the patch, but I do have exams period(or how is the english word for it) :-( I should be on that issue in few weeks(like 2-3). Martin Kupec ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
gEDA-user: Thermals on Pads
When I design surface mount boards I make extensive use of planes, and it is a severe annoyance that I can't automatically connect those planes to component pads. The standard solutions to this problem seem to be either: 1) Use a solid plane. But that makes soldering difficult. 2) Draw a very small solid rectangle to connect your pad to the plane. That works, but it's labor intensive. I'm a novice to the pcb code base, and I couldn't find much developer documentation, but I am willing to try to add this feature. I need a little help though: the pcb code base is too large for me to grok all at once. Could someone please tell me where to start? What would I have to modify to allow this? -Alan ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
