Re: gEDA-user: single-sided boards
On Thu, Mar 5, 2009 at 5:25 AM, David SMITH wrote: > On Tue, Mar 03, 2009 at 07:05:05PM +, Kai-Martin Knaak wrote: >> On Tue, 03 Mar 2009 16:47:28 +, David SMITH wrote: >> >> > From a user's point-of-view, it makes life much easier because they no >> > longer have the hassle of generating Gerbers (e.g. getting the correct >> > version of RS274, putting in the right number of decimal places, >> > including a readme file to indicate which layer is which, etc...) >> >> There are no such options in the gerber export dialog of pcb. > > Maybe not, but it's there in other packages, though, so this info still > needs to be communicated to the fab somehow (as it doesn't go in the > Gerber file itself), or you rely on them making correct assumptions. > > Just looking at the FAQs on many of the PCB fab websites, it is clear > that people make all types of mistakes generating Gerbers (layer order > wrong, drill file mistakes, etc...). Being able to put this process > in the hands of the "professionals" who are doing it all the time just > means that errors are likely to be eliminated. I would rather submit boards in the gerber format that is common to all vendors rather than rely on "professionals" to properly translate multiple CAD formats to their process. The PCB gerber plots work well. I have done 30 - 40 designs and have not had an issue. I always check the gerber plots with gerbv to confirm the plots. I set the PCB color scheme and the gerbv color scheme to the same values for easier comparison. I would rather do the panelization and plots myself, with scripts, rather than rely on the vendor. It is easier for me to check the resulting plots. (* jcl *) -- You can't create open hardware with closed EDA tools. http://www.luciani.org ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: single-sided boards
David SMITH wrote: > On Tue, Mar 03, 2009 at 07:05:05PM +, Kai-Martin Knaak wrote: >> On Tue, 03 Mar 2009 16:47:28 +, David SMITH wrote: >> >>> From a user's point-of-view, it makes life much easier because they no >>> longer have the hassle of generating Gerbers (e.g. getting the correct >>> version of RS274, putting in the right number of decimal places, >>> including a readme file to indicate which layer is which, etc...) >> There are no such options in the gerber export dialog of pcb. > > Maybe not, but it's there in other packages, though, so this info still > needs to be communicated to the fab somehow (as it doesn't go in the > Gerber file itself), or you rely on them making correct assumptions. FAB houses have lots of experience in dealing with the confusing and broken output from a whole slew of EDA tools. Note that some of this information is in fact there. For example, the leading/trailing zero bit and # of digits is *supposed* to go in the headers (at least for the drill files) but some tools give you flexibility to go outside of the specs and also generate garbage headers. > > Just looking at the FAQs on many of the PCB fab websites, it is clear > that people make all types of mistakes generating Gerbers (layer order > wrong, drill file mistakes, etc...). Being able to put this process > in the hands of the "professionals" who are doing it all the time just > means that errors are likely to be eliminated. > but now they need to deal with countless versions of countless different tools. And while it is not a big deal for pcb, it becomes a big deal if they are having to buy high dollar EDA tools and there is plenty of room for a "professional" to screw up generation of gerbers. Actually, I cringe at the idea of someone else generating gerbers for a board of mine without me reviewing the result with something like gerbv. There is a newer file format available that is supposed to address many of the shortcomings of the now-ancient RS274-X but the information I've been given by the one or two vendors I asked is that they still prefer RS274-X and haven't had a solid migration to the newer format(s). -Dan ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: single-sided boards
On Tue, Mar 03, 2009 at 07:05:05PM +, Kai-Martin Knaak wrote: > On Tue, 03 Mar 2009 16:47:28 +, David SMITH wrote: > > > From a user's point-of-view, it makes life much easier because they no > > longer have the hassle of generating Gerbers (e.g. getting the correct > > version of RS274, putting in the right number of decimal places, > > including a readme file to indicate which layer is which, etc...) > > There are no such options in the gerber export dialog of pcb. Maybe not, but it's there in other packages, though, so this info still needs to be communicated to the fab somehow (as it doesn't go in the Gerber file itself), or you rely on them making correct assumptions. Just looking at the FAQs on many of the PCB fab websites, it is clear that people make all types of mistakes generating Gerbers (layer order wrong, drill file mistakes, etc...). Being able to put this process in the hands of the "professionals" who are doing it all the time just means that errors are likely to be eliminated. -- David SmithWork Email: dave.sm...@st.com STMicroelectronics Home Email: david.sm...@ds-electronics.co.uk Bristol, England GPG Key: 0xF13192F2 ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: single-sided boards
On Thu, 05 Mar 2009 10:30:29 +0300, Ineiev wrote: > It now contains --merge-drills option to output all drills into single > "unplated" file; probably this can be useful for producing > "single-sided" boards. I'd prefer an option "single sided". This should produce gerbers suitable to send to the fab for production as a single sided layout. ---<(kaimartin)>--- ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: single-sided boards
On 3/3/09, Kai-Martin Knaak wrote: > On Tue, 03 Mar 2009 16:47:28 +, David SMITH wrote: > >> From a user's point-of-view, it makes life much easier because they no >> longer have the hassle of generating Gerbers (e.g. getting the correct >> version of RS274, putting in the right number of decimal places, >> including a readme file to indicate which layer is which, etc...) > > There are no such options in the gerber export dialog of pcb. There are some feature requests, though. BTW, I've just updated the patch series 2156903 at http://sourceforge.net/tracker/index.php?func=detail&aid=2156903&group_id=73743&atid=538813 It now contains --merge-drills option to output all drills into single "unplated" file; probably this can be useful for producing "single-sided" boards. Regards, Ineiev ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: single-sided boards
On Tue, 03 Mar 2009 16:47:28 +, David SMITH wrote: > From a user's point-of-view, it makes life much easier because they no > longer have the hassle of generating Gerbers (e.g. getting the correct > version of RS274, putting in the right number of decimal places, > including a readme file to indicate which layer is which, etc...) There are no such options in the gerber export dialog of pcb. With the fabs I used, a README wasn't necessary, because the file names are explicit enough for them to figured out their meaning. I just zipped all of the files and sent the package to the fab. PCBs came out as expected :-) ---<(kaimartin)>--- -- Kai-Martin Knaak tel: +49-511-762-2895 Universität Hannover, Inst. für Quantenoptik fax: +49-511-762-2211 Welfengarten 1, 30167 Hannover http://www.iqo.uni-hannover.de GPG key:http://pgp.mit.edu:11371/pks/lookup?search=Knaak+kmk&op=get ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: single-sided boards
On Tue, Mar 03, 2009 at 11:37:35AM +0300, Ineiev wrote: > On 3/2/09, David SMITH wrote: > > If I may make a suggestion - "solve" the layer handling problem which > > prevents PCB's data files from being taken directly by companies like > > www.pcb-pool.com. (I think it's something to do with the fact that > > the file doesn't contain any info to define the meaning of each layer > > (e.g. top copper, bottom copper, etc.) > > What layer handling problem do you speak of? > > The top and bottom copper layers _are_ marked in PCB files; and other > copper layers are ordered as well. > > As I understand, PCB files are not taken directly because PCB users > send to the manufacturers Gerber files rather than force them to > install the program on their machines. I'm afraid that I don't remember much more than I've already told you. Some PCB manufacturers (e.g. pcb-pool) will take native files as well as just Gerbers. I guess that the manufacturer either has a copy of that tool installed locally, or they've developed an automated conversion script. >From a user's point-of-view, it makes life much easier because they no longer have the hassle of generating Gerbers (e.g. getting the correct version of RS274, putting in the right number of decimal places, including a readme file to indicate which layer is which, etc...) In my case, I just send them my application's native file. For someone who makes one PCB every year or so, it means that I don't have to worry about making sure that the Gerber generation settings are correct, and if there's a problem (e.g. layers are in the wrong order, etc.) it's definitely their mistake, not mine :-). I guess it's one way in which manufacturers can gain competitive advantage by making their customers' lives easier. I remember at some point suggesting that pcb-pool should support 'pcb' files natively, and they said that it wasn't currently possible because some necessary information was missing from the file format. I thought that they said it was the layer definition information, but ICBW. This was a few years ago, so things might have changed since. If only the PCB manufacturing industry could standardise on a new, open format that solves Gerber's shortcomings. It does seem to be rather silly that we're still using a file format that was defined in the days when memory was so expensive that they did away with the decimal points... -- David SmithWork Email: dave.sm...@st.com STMicroelectronics Home Email: david.sm...@ds-electronics.co.uk Bristol, England GPG Key: 0xF13192F2 ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: single-sided boards
On 3/2/09, David SMITH wrote: > If I may make a suggestion - "solve" the layer handling problem which > prevents PCB's data files from being taken directly by companies like > www.pcb-pool.com. (I think it's something to do with the fact that > the file doesn't contain any info to define the meaning of each layer > (e.g. top copper, bottom copper, etc.) What layer handling problem do you speak of? The top and bottom copper layers _are_ marked in PCB files; and other copper layers are ordered as well. As I understand, PCB files are not taken directly because PCB users send to the manufacturers Gerber files rather than force them to install the program on their machines. Regards, Ineiev ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: single-sided boards
On Sat, Feb 28, 2009 at 02:21:23PM -0500, Stuart Brorson wrote: > > How often does the need for single-sided boards arise? > > The question about single-sided boards is interesting, but the > answer depends upon how you intend to fabricate your boards. > > If you're sending the boards to a PCB manufacturer, then the raw > material they use is fiberglass clad with copper on both sides. In > this case, it's senseless to ask for a single-sided board to save > costs -- they start with a double-sided board in any case. However, some of them do provide a cheaper, single-sided service - even the low-volume "panellising" companies - for example, www.pcb-pool.com. If they are starting from double-sided stock, then they can save on the production of an artwork - just expose the "component" side fully (or not at all, depending on whether their photoresist requires a positive or a negative exposure). They can also save on through-hole plating. When I've used their single-sided service before, I just sent them my whole data file (yes, I know, I'm a sinner - I use a commercial PCB design package), and asked them to do just the bottom copper layer. > I agree that it tends to trip up newbies. However, there's one Gerber > file per (metal) layer, so you can always discard the back side file > without any problems. That's what I was going to say :-) > Finally, one of the projects slated for work under the Linux Fund's > PCB project is to update PCB's handling of layers. Things like the > ability to easily deal with single sided boards from inside of PCB > are part of the work to be funded by the Linux Fund. I'll just remind > everybody that they can make this work happen sooner by making a > donation! If I may make a suggestion - "solve" the layer handling problem which prevents PCB's data files from being taken directly by companies like www.pcb-pool.com. (I think it's something to do with the fact that the file doesn't contain any info to define the meaning of each layer (e.g. top copper, bottom copper, etc.) Gerber is such a vile format; it's time it was consigned to the scrapheap :-) -- David SmithWork Email: dave.sm...@st.com STMicroelectronics Home Email: david.sm...@ds-electronics.co.uk Bristol, England GPG Key: 0xF13192F2 ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: single-sided boards
Single sided boards do not have plated holes, so pad diameter for pins must be greater, usually two to three times the drill size. Some footprints have very small pads which will be too weak if used for single sided board. If pins are arranged in rows then oval pads may be a solution. > Design for two-sided, but with all the traces on the solder side. > When you dump your gerbers, delete the component side one and rename > the plated-holes one to unplated-holes. Voila! A single sided board. > > It's all just names when you're doing single sided. There's no such > thing as a single sided board - just a double sided board with nothing > on one side. > Wojciech Kazubski ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: single-sided boards
On Feb 28, 2009, at 11:21 AM, Stuart Brorson wrote: > Hi -- > >> How often does the need for single-sided boards arise? > > The question about single-sided boards is interesting, but the > answer depends upon how you intend to fabricate your boards. > > If you're sending the boards to a PCB manufacturer, then the raw > material they use is fiberglass clad with copper on both sides. In > this case, it's senseless to ask for a single-sided board to save > costs -- they start with a double-sided board in any case. To be fair, this is true when making few boards. AKA less than a LOT Your PCB manufacture would order single sided stock if you were making say 10,000 boards plus. Or if you were dealing with a manufacture that dealt a lot with single sided boards. TV manufactures and boom box makers use these tricks, but they also do things like use FR2 http://en.wikipedia.org/wiki/FR-2 The quick turn PCB houses online, usually don't run single sided for small jobs, as they panelize your board with others, that are most likely double sided. > > > If you're making the PCBs at home, starting with single-sided > fiberglass from e.g. Radio Shack, then it's totally sensible to make > single sided boards. In this case, just throw away the back side > Gerber file. > >> this kind of >> cosmetics with gerber files is an additional error-prone manual step. >> Has it been considered to make this an option that is supported by >> pcb? > > I agree that it tends to trip up newbies. However, there's one Gerber > file per (metal) layer, so you can always discard the back side file > without any problems. > > More to the point: the Gerber, and the related drill file > formats are pretty stupid. They don't carry any top-level > information about your design. A particular Gerber file knows only > about its own layer, and knows nothing about any other layer. The > Gerber files have no concept of "stack-up" (i.e. what order the layers > are supposed to be stacked in). The drill file only contains > information about what drill diameters to use, and where to put the > holes. The remaining information, like stack-up, plated > vs. non-plated holes, how thick your copper layer should be, how thick > your FR-4 should be, desired manufacturing tolerances, etc., are all > told to your PCB manufacturer using "fab notes" (i.e. a > human-readable text file) and a "fab drawing" (a drawing of the board, > stack-up, and other graphical info). > > Finally, one of the projects slated for work under the Linux Fund's > PCB project is to update PCB's handling of layers. Things like the > ability to easily deal with single sided boards from inside of PCB > are part of the work to be funded by the Linux Fund. I'll just remind > everybody that they can make this work happen sooner by making a > donation! > > http://www.linuxfund.org/projects/pcb/ Thanks for the reminder, I just chipped in some. > > > HTH, > > Stuart > > > ___ > 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: single-sided boards
Hi -- > How often does the need for single-sided boards arise? The question about single-sided boards is interesting, but the answer depends upon how you intend to fabricate your boards. If you're sending the boards to a PCB manufacturer, then the raw material they use is fiberglass clad with copper on both sides. In this case, it's senseless to ask for a single-sided board to save costs -- they start with a double-sided board in any case. If you're making the PCBs at home, starting with single-sided fiberglass from e.g. Radio Shack, then it's totally sensible to make single sided boards. In this case, just throw away the back side Gerber file. > this kind of > cosmetics with gerber files is an additional error-prone manual step. > Has it been considered to make this an option that is supported by pcb? I agree that it tends to trip up newbies. However, there's one Gerber file per (metal) layer, so you can always discard the back side file without any problems. More to the point: the Gerber, and the related drill file formats are pretty stupid. They don't carry any top-level information about your design. A particular Gerber file knows only about its own layer, and knows nothing about any other layer. The Gerber files have no concept of "stack-up" (i.e. what order the layers are supposed to be stacked in). The drill file only contains information about what drill diameters to use, and where to put the holes. The remaining information, like stack-up, plated vs. non-plated holes, how thick your copper layer should be, how thick your FR-4 should be, desired manufacturing tolerances, etc., are all told to your PCB manufacturer using "fab notes" (i.e. a human-readable text file) and a "fab drawing" (a drawing of the board, stack-up, and other graphical info). Finally, one of the projects slated for work under the Linux Fund's PCB project is to update PCB's handling of layers. Things like the ability to easily deal with single sided boards from inside of PCB are part of the work to be funded by the Linux Fund. I'll just remind everybody that they can make this work happen sooner by making a donation! http://www.linuxfund.org/projects/pcb/ HTH, Stuart ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: single-sided boards
On Sat, 28 Feb 2009 18:58:44 +0100, Juergen Harms wrote: > Nice to know that this is normal and works. This seems to be a frequently asked question. I added a slightly edited version of DJs answer to the pcb-faq, err, pcb-tips in the wiki: http://geda.seul.org/wiki/geda:pcb_tips#how_do_i_produce_gerbers_for_a_single_sided_board > How often does the need for single-sided boards arise? this kind of > cosmetics with gerber files is an additional error-prone manual step. Ack. An option "single sided output" for gerber export would be nice. ---<(kaimartin)>--- -- Kai-Martin Knaak http://lilalaser.de/blog ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: single-sided boards
Thanks - that corresponds to the "ugly" solution I had considered. Nice to know that this is normal and works. I have already some unplated mounting holes, I will have to merge the plated file into the unplated one. How often does the need for single-sided boards arise? this kind of cosmetics with gerber files is an additional error-prone manual step. Has it been considered to make this an option that is supported by pcb? ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: single-sided boards
Design for two-sided, but with all the traces on the solder side. When you dump your gerbers, delete the component side one and rename the plated-holes one to unplated-holes. Voila! A single sided board. It's all just names when you're doing single sided. There's no such thing as a single sided board - just a double sided board with nothing on one side. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
gEDA-user: single-sided boards
How do I poceed to make a single sided board (copper only on wiring side, no plated holes), but nevertheless use my footprint library which is made for multiple layers (that defines copper plated-holes and pins with copper pads on both sides)? If I naively use my library and create a single-sided board, looking at the files exported to gerber, I end up with a component side which has all the copper pads, and with a long list in the plated-drill.cnc file, which is not really what I want. I am looking for a way - using my standard footprint library - to produce gerber files which do not have plated holes, and which have no copper on the component side. Can I control this in pcb - or is there an (ugly) way to achieve this playing around with the gerber files? Or is my intention a false desire for economy - should I better keep the pads on the component side and the plated holes? (considering that a pcb with solder sipping into the plated holes might represent a more reliable result?) ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
