RE: [kicad-users] prototype PCBs
Hi, I use them often. Yes, very good. Also, look at www.Olimex.com for simple double sided. Bob Kondner -Original Message- From: kicad-users@yahoogroups.com [mailto:[EMAIL PROTECTED] On Behalf Of betalayout Sent: Thursday, October 25, 2007 9:34 AM To: kicad-users@yahoogroups.com Subject: [kicad-users] prototype PCBs Has anyone used the PCB-pool.com service before? Excellent prices for prototypes, no minimum quantity, anything from 1 to 6 layers - no tooling costs Fully industrial quality, ideal for hobbyists, small businesses etc. Happy routing! Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-devel Yahoo! Groups Links
RE: [kicad-users] Re: composite layers and negative plots
Hi, That RS-274-X spec has more holes than Swiss Cheese. For example: If you start a Poly Fill and use a ARC I guess the ARC becomes part of the the poly edge, correct? Doing so results in a polygon with circular voids. This is a huge area for Interpretation Errors in gerber processors. Now add to the fact that these polygons could be in clear or dark areas of a single layer and the multiple layers COULD be combined. Good luck finding 2 gerber processors that render this to the same film image. Chance are about 5% that you get a call from the PCB vendor. Chances are 95% that you get back a bad PCB. Worse yet the location for finding errors in circular voids is in an internal plane. Shorts in a plane are like an unforgivable sin, nothing can save you. After many years of doing PCB designs and the writing of a gerber reader (MUCH more difficult than writing gerbers) my suggestion is Keep It Simple (KISS Solution). The generation of gerbers and their resulting rendering to film must be ABSOLUTLY PERFECT. We live and die by this level of perfection. To achieve this level of perfection think of a gerber as a vector driven bitmap. No Aperture Macros and no Polygons need to apply. Even if 99% of the code in the industry reads and processes PERFECTLY that 1% is a reason NOT to use them. We need ROCK SOLID routines for flattening a higher level structure of shapes. The output is a set of scan lines that paints the required image. I write in Delphi, I can easily generate .dlls, and the resulting scan lines could convert directly to KISS generation of gerbers. I have a simple gerber reader that is used to read from LOTS of different apps. It took years learning what liberties every app programmer could take with gerber generation. Lets NOT to the same thing in DRIVING film plotters. Summary: We live or die with gerber generation. If we even need to talk to a fab house about gerber processing we are dead meat. I would love to see a solution got this gerber generation issue. Thanks, Bob Kondner _ From: kicad-users@yahoogroups.com [mailto:[EMAIL PROTECTED] On Behalf Of Geoff Harland Sent: Friday, September 21, 2007 12:06 AM To: Kicad Users Subject: [kicad-users] Re: composite layers and negative plots Hi Ben, I have a copy of the RS274X specification, and this states that the G36 and G37 commands are actually used to turn on Polygon Area Fill and turn off Polygon Area Fill (respectively). There are other commands which can be used to change the polarity of a Gerber file's contents (i.e. whether any draw and stroke commands which follow are dark or clear, or positive or negative in nature), but the G36 and G37 commands are used in conjunction with a set of vertexes whose associated region is to be entirely filled. The related specification specifically states: ... G36 and G37 provide a more efficient means of filling closed polygons than stroke fill. When these codes are used, the filled area is defined simply by its closed outline. Stroke fill is an inefficient method of filling a polygon. ... I haven't studied the relevant (source) code (for KiCad) in depth, but I am still picking that the G36 and G37 commands have deliberately been used because it is far easier to depict poured copper areas within Gerber files by using those commands rather than by using stroked fills instead. It probably would be possible to make changes to the relevant source code so that users subsequently had the option of generating Gerber files using the G36 and G37 commands (the existing way), or otherwise by using stroked fills instead. That said, while I can't speak for any of the other developers, my personal attitude is that I would rather spend the limited amount of time that I have available (for improving KiCad) in implementing various other improvements. While that attitude might seem harsh or unreasonable, I am also of the view that PCB manufacturers *should* be able to cope with any Gerber files whose contents are fully compliant with the RS274X specification. If you, or anybody else, can provide proof that any Gerber files created by KiCad are *not* fully compliant with that specification, then I would be fully prepared to look at the relevant source code, and make any changes which would be necessary to make those files fully compliant. But as I don't have unlimited time available for making improvements to KiCad, I am not of an inclination to make any changes for the benefit of any PCB manufacturers who are not capable of dealing with any Gerber files which they *should* be capable of dealing with. Given the circumstances, my advice would be to advise the PCB manufacturer concerned that other PCB manufacturers are capable of dealing with Gerber files which incorporate G36 and G37 commands, so unless they are able to prove that there are any genuine problems with the contents of any Gerber files which you have
RE: [kicad-users] Re: composite layers and negative plots
Geoff, Thank you for the comments. Yes, I did suggest rather radical surgery in the quest for PERFECT GERBERS. PERFECT GERBERS is asking for a lot but that is what we need. The problem with using Aperture Macros is that it implies a tremendous software task. How can KiCAD verify design rules on planes if the aperture info in KiCAD is not EXACTLY THE SAME as the patterns in the photo plotter? I don't think this can be done. :-( Radical? Maybe but do we intend to detect and flag Cutoff or Missing Spokes in planes? If so they we already did all the hard work with thermals so drawing them with simple shapes should be easy. If we don't completely error check plane rendering then KiCAD plane generation is very weak. To draw a thermal all we need is a center CIRCLE for the inside PAD, the region outline drawn with arcs and lines, and spokes. Verify of spoke to region outlines, other spokes, drills or other nets is easy. Now we have perfect circular plane voids and full error checking without Aperture Macros. Maybe I missed something? Also, the circular void as line segments issue needs a resolution. Do we chop an arc into segments until we get some max error? Maybe .01mm? A big pad is going to give a lot of segments. I would suggest simply using arcs. The ARC commands are very solid, they are pretty well defined and have been there since -D. I can accept the idea of using ARCs to draw the outline of a region, this will give perfect arcs limited only by the photo plotter resolution. One could then use -X polygons to fill in the main body of the region just as scan lines can be used. I found -X Poly operation rather consistent though scan lines are less complex. Summary: Just Say No to Aperture Macros Outline copper regions with Lines and Arcs. I am open to ideas. Thanks, Bob Kondner -Original Message- From: kicad-users@yahoogroups.com [mailto:[EMAIL PROTECTED] On Behalf Of gharlandau Sent: Friday, September 21, 2007 1:02 PM To: kicad-users@yahoogroups.com Subject: [kicad-users] Re: composite layers and negative plots I fully agree that there are many aspects of the RS274X specification that leave a lot to be desired, but I'm still not convinced of the merits of totally forsaking the use of Aperture Macros and Polygon commands. The copy of the RS274X standard which I have (an Acrobat file which I downloaded from a website some years ago) makes no specific reference to being able to use Arc commands in conjunction with Polygon commands, so I concur that it would be desirable to avoid using that combination. And I also think that it would be highly desirable to avoid incorporating different layers within the same Gerber file (re using both dark and clear polarities). But I think that totally avoiding the use of Aperture Macros could be taking things too far. As long as the value of each parameter (for each primitive that is used within an Aperture Macro) is explicitly defined, and no algebraic substitutions are required in that regard, I would regard the usage of Aperture Macros as acceptable (assuming that no attempt is being made to push the limits of the RS274X specification at the time). A really extreme view of Gerber files is that they should *never* incorporate *any* Arc commands either, least some PCB manufacturers not be able to cope with them. Would you advocate that as well? I have not really looked at the source code for generating Gerber files so far, but when I get a chance, I will take a look and see if there are any aspects where improvements could be made to at least reduce (and preferably totally eliminate) the possibility of Gerber files' contents ever being misinterpreted. In that regard, I would regard it as preferable to use an Aperture Macro (incorporating a type 21 / centered line primitive) to define an aperture for a pad having a rectangular shape on a non-orthogonal angle, rather than using a Polygon command, and there could well be various other aspects which could also be improved. And maybe something else which should be considered at some stage is providing the feature of generating (sets of) ODB++ files from PCB files. While I am not currently an expert on such files, it is still my understanding that they don't suffer from the shortcomings that afflict Gerber files (due to the shortcomings of the RS274X standard). However it is also my understanding that many PCB manufacturers are not yet equipped to handle such files, and I gather that some of them haven't even heard of such files. But doubtless any PCB manufacturers who actually can cope with such files would still prefer to receive them whenever that is possible. Regards, Geoff Harland. Robert Kondner wrote: Hi, That RS-274-X spec has more holes than Swiss Cheese. For example: If you start a Poly Fill and use a ARC I guess the ARC becomes part of the the poly edge, correct? Doing so results in a polygon with circular voids
RE: [kicad-users] Re: Orcad EDIF to KICAD
Thanks, I will look into that. Problem with a parser is you need somewhere to put the data. Some vendors of translation products have their own format but that is just another level of conversion. EDIF is just an exchange syntax, you still need to understand each and every format. I have been looking at higher level structures where schematic symbol, routing and decal pin assignment and purchasing info can all be stored. Plus it needs to be in a structure which is easily searched and synchronized over the web. The only useful approach I see is to read am EDIF and immediately populate this higher level structure. I pretty much have that for PCB Decal and purchasing info. I now need the schematic side of things. Anyone interested can contact me off line. [EMAIL PROTECTED] Bob -Original Message- From: kicad-users@yahoogroups.com [mailto:[EMAIL PROTECTED] On Behalf Of Frank Bennett Sent: Sunday, September 16, 2007 10:01 PM To: kicad-users@yahoogroups.com Subject: [kicad-users] Re: Orcad EDIF to KICAD --- In kicad-users@yahoogroups.com, Robert Kondner [EMAIL PROTECTED] wrote: Hi, I put a schematic with its EDIF output. http://www.kondner.com/files/ps10.zip There usetobe, might still be there, in the gEDA distribution source code, and doc, an EDIF to Sue converter: gEDA/mmi_pd_040526/edif2sue1.2.12 I think I even saw the Sue schematic editor source in the public domain somewhere I started an EDIF parser once but I lost interest, an example file might be good enough to get started. I found you can usually get pretty close without a spec. Instead of dealing with EDIF you might consider a netlist translator from OrCad to KiCAD like the one I just submitted for PCB123 to KiCad: http://sourceforge.net/tracker/index.php?func=detailaid=1794790group_id=14 5591atid=762479 Most Netlists are human readable, ASCII with a simple syntax. One good feature of KiCad is it's open source and the whole database is ASCII which make the KiCad end of any translation easier. cheers, Frank Bennett I have a copy of the spec, yes that is what I paid. Come on, what is a month of your time worth? That's cheap :-) If you can do this I will help pay for it and your time. Contact me at: [EMAIL PROTECTED] You might want to look at www.aapcb.com. I wrote all their internal code and I licensed it to them. I want to do for SCH to PCB what I did for PCB to Assembly. I like the idea of KiCAD but the required features and library structures does not make it possible to use KiCAD. Do you use Delphi? Thanks, Bob Kondner -Original Message- From: kicad-users@yahoogroups.com [mailto:[EMAIL PROTECTED] On Behalf Of Bob_xyz Sent: Sunday, September 16, 2007 6:46 PM To: kicad-users@yahoogroups.com Subject: [kicad-users] Re: Orcad .OLB to KICAD --- In kicad-users@yahoogroups.com, Robert Kondner rkondner@ wrote: Hi, For a sample EDIF export an OrCAD schematic or library. Unfortunately, I have no access to a system running OrCAD. You will need the EDIF 2.0.0 documents they cost a couple hundred dollars. I just found the spec - OUCH, it's US$372. That's a bit more than I was planning to spend on this effort. I'll have to see if I can get access to a copy without buying one. With a few example files, though, it should be possible to figure out the basics from the files themselves. The descriptions and examples that I've seen indicate that EDIF is a fairly straightforward format. If noone in this group is able to post a few EDIF files, I'll try to get someone over on the OrCADexchange Yahoo group to post some. If you really want to do this keep in touch, I have plans on doing the same at some point in the near future. Will do. Regards, Bob Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-devel Yahoo! Groups Links Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-devel Yahoo! Groups Links
RE: [kicad-users] Re: Orcad .OLB to KICAD
You can export OrCAD to EDIF, which is not only text but well documented. Bob Kondner -Original Message- From: kicad-users@yahoogroups.com [mailto:[EMAIL PROTECTED] On Behalf Of Bob_xyz Sent: Sunday, September 16, 2007 10:58 AM To: kicad-users@yahoogroups.com Subject: [kicad-users] Re: Orcad .OLB to KICAD --- In kicad-users@yahoogroups.com, [EMAIL PROTECTED] wrote: On 14 Sep 2007 at 14:12, stephen_alexander_1 wrote: David, Apologies if this is a resend, the original reply seems to have disappeared. Did you ever get a solution to this problem? I have an OrCAD olb file which I downloaded from ST Microelectronics, which I would like to convert for use with KiCAD. If you managed to get a solution for this, I would apreciate the info. Thanks, No, I more or less gave up. Does OrCAD have the capability to export to text files? Or might there be a utility program around that could do the binary-to-ASCII extraction? I've never been able to make any sense of the .olb file format. If they can be converted to plain text, though, automated translation to another EDA program's format should be possible. Alternately, is there any documentation available that describes the details of the .olb file format? Regards, Bob Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-devel Yahoo! Groups Links
RE: [kicad-users] Re: Orcad .OLB to KICAD
Hi, For a sample EDIF export an OrCAD schematic or library. You will need the EDIF 2.0.0 documents they cost a couple hundred dollars. If you really want to do this keep in touch, I have plans on doing the same at some point in the near future. Bob Kondner [EMAIL PROTECTED] -Original Message- From: kicad-users@yahoogroups.com [mailto:[EMAIL PROTECTED] On Behalf Of Bob_xyz Sent: Sunday, September 16, 2007 5:17 PM To: kicad-users@yahoogroups.com Subject: [kicad-users] Re: Orcad .OLB to KICAD --- In kicad-users@yahoogroups.com, Robert Kondner [EMAIL PROTECTED] wrote: You can export OrCAD to EDIF, which is not only text but well documented. That's terrific. If someone could post an example EDIF file or two, I'd like to take a crack at writing a utility to do the conversion automatically. I do have a different target CAD system in mind. Once the basics are in place, though, I wouldn't expect it to be too difficult to adapt the program so that it can output kikad-format files as well. I do need to review the kikad and EDIF formats but I'm fairly sure that this would be quite possible to do. Regards, Bob Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-devel Yahoo! Groups Links
RE: [kicad-users] Re: Orcad .OLB to KICAD
Hi, I put a schematic with its EDIF output. http://www.kondner.com/files/ps10.zip I have a copy of the spec, yes that is what I paid. Come on, what is a month of your time worth? That's cheap :-) If you can do this I will help pay for it and your time. Contact me at: [EMAIL PROTECTED] You might want to look at www.aapcb.com. I wrote all their internal code and I licensed it to them. I want to do for SCH to PCB what I did for PCB to Assembly. I like the idea of KiCAD but the required features and library structures does not make it possible to use KiCAD. Do you use Delphi? Thanks, Bob Kondner -Original Message- From: kicad-users@yahoogroups.com [mailto:[EMAIL PROTECTED] On Behalf Of Bob_xyz Sent: Sunday, September 16, 2007 6:46 PM To: kicad-users@yahoogroups.com Subject: [kicad-users] Re: Orcad .OLB to KICAD --- In kicad-users@yahoogroups.com, Robert Kondner [EMAIL PROTECTED] wrote: Hi, For a sample EDIF export an OrCAD schematic or library. Unfortunately, I have no access to a system running OrCAD. You will need the EDIF 2.0.0 documents they cost a couple hundred dollars. I just found the spec - OUCH, it's US$372. That's a bit more than I was planning to spend on this effort. I'll have to see if I can get access to a copy without buying one. With a few example files, though, it should be possible to figure out the basics from the files themselves. The descriptions and examples that I've seen indicate that EDIF is a fairly straightforward format. If noone in this group is able to post a few EDIF files, I'll try to get someone over on the OrCADexchange Yahoo group to post some. If you really want to do this keep in touch, I have plans on doing the same at some point in the near future. Will do. Regards, Bob Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-devel Yahoo! Groups Links
RE: [kicad-users] Re: pcbnew 2007-07-09 crash
Hi, What I do is call out the un-plated holes at a slightly different size. I then tell the fab house All hole at xxx are non-plated. For example I have a lot of 0.125 files. The holes to be un-plated I make 0.126 size. Bob Kondner -Original Message- From: kicad-users@yahoogroups.com [mailto:[EMAIL PROTECTED] On Behalf Of Pedro Martín Sent: Sunday, September 09, 2007 4:58 PM To: kicad-users@yahoogroups.com Subject: Re: [kicad-users] Re: pcbnew 2007-07-09 crash Hi, It is not possible with Gerbers. We do it in 2 ways: 1. with the technical layers, pointing the holes we do not want to be plated. 2. with a readme file expaining the same things. Some manufacturers don't accept neither of them, example Pcbexpress. Pedro. 2. When making holes in the board that you don't want to be plated, What method do you use to give the board manufacturer a list of the holes that you don't want plated? Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-devel Yahoo! Groups Links
RE: [kicad-users] free-ecb-at91
I have a Rough gerber to .pdf I wrote. It does not process CLEAR layers and someday I need to add round endcaps. But, if it helps, you can download it at: http://kondner.com/files/gerb2pdf.zip Bob Kondner -Original Message- From: kicad-users@yahoogroups.com [mailto:[EMAIL PROTECTED] On Behalf Of John Griessen Sent: Monday, August 06, 2007 9:28 PM To: kicad-users@yahoogroups.com Subject: Re: [kicad-users] free-ecb-at91 Hristo Antonov wrote: Hi 2 all i have a plan to export the AT91 Linux embedded computer (http://wiki.emqbit.com/free-ecb-at91) to Kicad file format as main embedded platform for our firm The gEDA team is also working on this task . ;) But that effort is stalled at seeing a RS-274X gerber file of the existing layout... Any one with the free-ecb-at91 project have RS-274X or postscript output of the board layout I can look over to see what I could reuse in a gschem/pcb schematic and layout? Thanks, John Griessen, a gEDA user/contributor Ecosensory Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-devel Yahoo! Groups Links
RE: [kicad-users] free-ecb-at91
I do a lot of embedded power supply stuff and can configure battery pack. If someone needs a battery/charger/power supply rolled into this let me know. I think a generic small processor would be useful. Bob Kondner -Original Message- From: kicad-users@yahoogroups.com [mailto:[EMAIL PROTECTED] On Behalf Of Lisandro Damián Nicanor Pérez Meyer Sent: Wednesday, August 01, 2007 10:02 AM To: kicad-users@yahoogroups.com Subject: Re: [kicad-users] free-ecb-at91 El Miércoles 01 Agosto 2007, Hristo Antonov escribió: Hi 2 all i have a plan to export the AT91 Linux embedded computer (http://wiki.emqbit.com/free-ecb-at91) to Kicad file format as main embedded platform for our firm . The project is GPL and all the documentation will be free . I think that this is good way for Kicad to grow , cause at this point Kicad is professional CAD system and blinkin led and battery chargers should be left in the past. If someone wants to help or use the project feel free to write ! I think , that in 2-3 months we might have working board. The gEDA team is also working on this task . ;) Greeat!!! I and a couple of friends are suposed to do exactly that, with an additional CAN interface!!! As we are all Linux users, we decided to use kicad! Please, keep in touch!! -- The irony is that Bill Gates claims to be making a stable operating system and Linus Torvalds claims to be trying to take over the world. -- seen on the net Lisandro Damián Nicanor Pérez Meyer http://perezmeyer.com.ar/ #bblug irc.freenode.net Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-devel Yahoo! Groups Links
RE: [kicad-users] Re: [EE]Less Expensive PCB Layout Programs
Hi, From my experience first improvement in EDA CAD would be web libraries which include purchasing info. After/As I design a schematic I need to finish 3 tasks: 1. Design the PCB 2. Purchase the parts 3. Assemble the PCB Do I want to maintain a World Class library here in my shop? No, I only want to use it. But it needs to deal with the above 3 issues. Does the lib need to have 100% of all my parts? Not at a projects start but after I finish I should have 100% of the parts in my own local version of the library. I did the code for aapcb.com so I know the assembly business well. Anyone interested in the web library thing let me know. Bob Kondner _ From: kicad-users@yahoogroups.com [mailto:[EMAIL PROTECTED] On Behalf Of Tobias Gogolin Sent: Friday, July 27, 2007 3:21 PM To: Microcontroller discussion list - Public. Cc: kicad-users@yahoogroups.com Subject: [kicad-users] Re: [EE]Less Expensive PCB Layout Programs Actually I don't know how it would be seen If I was to suggest to sidetrack this thread a bit (OK hijack it ;) Like to the subject line 'defining the perfect EDA CAD of the future' And I wonder how many of you know _parametric modeling_ in the mechanical CAD world? So I've been thinking EDA isn't showing enough tendencies for parametric modeling, or is it? To get ones mind around it, lets say in a parametric environment the memory area could be modified in depth and width by 2 parameters which would results in all the component and netlist changes that the program could figure out by itself... Sounds easy no? OK also functional blocks should be possible to be defined, duplicated and wired based on parameters... Component specifications (parametric values) could be automated by Formulas and looked up from lists of available components In _parametric modeling_ keyword is the capture of the design intention, and the elimination of repetitive operations. Is there any EDA tool that shows tendencies toward this direction? --- Bob Axtell [EMAIL PROTECTED] wrote: A while ago, folks were talking about less expensive PCB layout programs. Anybody remember the links? I need: up to 8 layers, 13 x 13 max, and it must generate RS274X. Does NOT have to have or autoroute. Sounds like KiCad would do the job - for free: http://www.lis.inpg.fr/realise_au_lis/kicad/ Cheerful regards, -- Tobias Gogolin cel. (646) 124 32 82 skype: moontogo messenger: [EMAIL PROTECTED] You develop an open source motor controller at http://groups.yahoo.com/group/GoBox
RE: [kicad-users] mounting holes
They drill the board, run it through an electrode-less process that leaves a VERY THIN layer of copper in the hole. Then they electroplate the entire board with thicker copper which builds up a thicker layer of copper. This way ALL holes are plated through. If you need holes which ARE NOT plated through they have to take the finished boards and re-drill the holes. It is always better to accept holes as plated through is you can. Bob Kondner -Original Message- From: kicad-users@yahoogroups.com [mailto:[EMAIL PROTECTED] On Behalf Of Chris Albertson Sent: Monday, June 25, 2007 1:35 PM To: kicad-users@yahoogroups.com Subject: Re: [kicad-users] mounting holes --- Pedro Martin [EMAIL PROTECTED] wrote: Be careful with metallization, there are pcb providers that will metallize the hole. So it can be avoided? I thought that because of the process all holes got plated. I admit I don't know how they plate the holes. How do they plate the hole? Chris Albertson Home: 310-376-1029 [EMAIL PROTECTED] Office: 310-336-5189 [EMAIL PROTECTED] Choose the right car based on your needs. Check out Yahoo! Autos new Car Finder tool. http://autos.yahoo.com/carfinder/ Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-devel Yahoo! Groups Links
RE: [kicad-users] mounting holes
When the board come out of the plating process there is copper all over the surfaces and edges. It is one big copper coated piece at that point. Later it is etched and trimmed off. Bob Kondner -Original Message- From: kicad-users@yahoogroups.com [mailto:[EMAIL PROTECTED] On Behalf Of John Luckey Sent: Monday, June 25, 2007 4:46 PM To: kicad-users@yahoogroups.com Subject: RE: [kicad-users] mounting holes At that point there is copper foil on both sides, and the board is still part of a larger panel. Later in the process the board is cut, or routed from the panel. -Original Message- From: kicad-users@yahoogroups.com [mailto:[EMAIL PROTECTED] On Behalf Of Chris Albertson Sent: Monday, June 25, 2007 1:39 PM To: kicad-users@yahoogroups.com Subject: RE: [kicad-users] mounting holes --- Robert Kondner [EMAIL PROTECTED] wrote: They drill the board, run it through an electrode-less process that leaves a VERY THIN layer of copper in the hole. Why does the copper only plate out inside the holes and not on the board's edges or on the face of the board? Chris Albertson Home: 310-376-1029 [EMAIL PROTECTED] Office: 310-336-5189 [EMAIL PROTECTED] Ready for the edge of your seat? Check out tonight's top picks on Yahoo! TV. http://tv.yahoo.com/ Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-devel Yahoo! Groups Links Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-devel Yahoo! Groups Links
RE: [kicad-users] Re: IPC Netlist
These are basic scripts for running under PADs. If anyone is really interested in IPC Netisits and Gerber to Netlist processing let me know. I am writing some CAD Tools in this area. I wrote all the tools at www.aapcb.com and I have quite a good array of component models. Bob Kondner -Original Message- From: kicad-users@yahoogroups.com [mailto:[EMAIL PROTECTED] On Behalf Of yajeed2000 Sent: Thursday, May 31, 2007 9:04 AM To: kicad-users@yahoogroups.com Subject: [kicad-users] Re: IPC Netlist Hi, I've found another useful link. http://www.capecad.com/htm/programs.htm Hope it's of use to someone. David. --- In kicad-users@yahoogroups.com, yajeed2000 [EMAIL PROTECTED] wrote: Hi, I don't know much about IPC netlists, but on googling around I found this link http://www.pcbstandards.com/forums/archive/index.php/f-84.html This lists a .BAS file (contained in a zip archive) that seemingly converts a PADS netlist into a IPC netlist. It won't solve your problem now, but it might spark some ideas off for creating a script or conversion utility. Regards, David. --- In kicad-users@yahoogroups.com, apluscw apluscw@ wrote: I am pleased to say we are having our rather large, KiCad designed control board being looked at for production. The board house is asking for an IPC netlist. That is not an (obvious) option from KiCad. Can anyone please tell me how to get to an IPC netlist from a KiCad schematic? Thank you, a+ Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-devel Yahoo! Groups Links
RE: [kicad-users] Re: Resolution of zones
Hi, When creating this kind of gerber Kicad needs to outline the poly area with lines and arcs. PADs does this and it makes for very nice planes. Maybe Kicad does it on the gerbers by not the screen? I don't know, I have just started looking at these kind of software issues. Bob Kondner _ From: kicad-users@yahoogroups.com [mailto:[EMAIL PROTECTED] On Behalf Of bartvanderlaan Sent: Thursday, May 24, 2007 3:55 PM To: kicad-users@yahoogroups.com Subject: [kicad-users] Re: Resolution of zones Sorry, the links did not work properly, these should: picture1 http://www.xs4all.nl/~monique4/TentLabs/pcbzoneissue1.jpg picture2 http://www.xs4all.nl/~monique4/TentLabs/pcbzoneissue1.jpg Thanks! Bart
RE: [kicad-users] BOMS and other reports
Hi, I wrote a good sized application for a start up on Colorado, they do proto type assembly and this app is used to manage BOM info and feed pick and place equipment. See: www.aapcb.com Download BOM Builder at www.indexdesigns.com/files/bbsetup4.zip (22MB) It might be to much of a pain for most circuit designers to use but it is really good if you want to control all aspects of assembly. Someone needs to setup jobs, with automated links to schematic and PCB design tools it because very easy. Be sure to read the manual! Bob Kondner -Original Message- From: kicad-users@yahoogroups.com [mailto:[EMAIL PROTECTED] On Behalf Of Chris Bartram Sent: Tuesday, May 01, 2007 12:46 PM To: kicad-users@yahoogroups.com Subject: [kicad-users] BOMS and other reports I've been using Kicad in my work for the last year, and I find that my copy of Protel gets less and less use! One aspect of Kicad which could be usefully improved would be to add an option for reports which allows the generation of report data in some form of spreadsheet format. The majority of my clients require BOMs to be presented in this way, and I'd find the ability to write direct to an OASIS (or even an Excel!) spreadsheet file very useful. Or have I missed something?? Best wishes Chris Bartram Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-devel Yahoo! Groups Links
RE: [kicad-users] Pick Place Data
Hi, I am new on the KiCAD list but I wrote all the code for Advanced Assembly (aapcb.com) so I know pick and place data real well. Here are some ideas on what you really need from KiCAD, IM/HO 1. If you can supply a rotation that's nice but they will never match machine rotations It took a lot of code to adjust for different CAD tools. Some spin CW others CCW and this will vary on top vs bottom. 2. Supply Digikey numbers if possible. If there is a question about the part size and shape (we call that the Package) then the assembly folks can look it up and not waste time playing phone tag with you. 3. A Good BOM in machine readable form. Spread sheets are ok but people type stuff into the cells and they create errors. I have seen notes about parts in the cell with the refDes. How can code read refdes from fields with text notes in the field. 4. Use consistent footprint names that have some info about the part. I even see some files where the users has ReTyped the footprint names. That is a disaster since we process rotations based on footprint names. Re-naming then messes up this tracking logic. 5. Put all parts in the BOM. All Parts, even if they are not stuffed. People do us a Favor and leave the no stuffs off the BOM. When the job hits inspection we don't know if it was a dropped part or a no stuff. Give the complete BOM and then provide a list of RefDes to not stuff. 6. Keep RefDes simple. RN101 C23 are ok. +5V and J27_A are NOT ok. Remember allthis text gets feed down into automated equipment with their own syntax requirements. A lot of sorting is required. Keep It Simple. 7. Be sure there is some small mark in the gerbers at the 0,0 component reference point. Have some text in the silk or copper that identifies this point. 8. Use something like a 1mm RND for fiducial points and make sure the solder mask is backed off by 1mm. Getting mask near the fiducial makes it visually difficult to align with. 9. Use a DIAMOND (square rotated by 45 degrees) as a fiducial, those are best. Bob Kondner _ From: [EMAIL PROTECTED] [mailto:[EMAIL PROTECTED] On Behalf Of Mark Webster Sent: Friday, April 13, 2007 9:31 AM To: [EMAIL PROTECTED] Subject: [kicad-users] Pick Place Data Hello, A quick question, does anyone know if KiCAD can produce pick place data? If so, what is the position based on? Is it the anchor point of the module? Thanks in advance. MarkW
