Re: gEDA-user: new components
Hi, I have a bunch of symbols here: http://logonex.eu/git/?p=svn.git;a=tree;f=gschem-sym;h=a684be6d0dc98a94e7d8ea092972e18f4a9cdce4;hb=90743ea21068a0c473ce71da1fd457353310ccf4 and a bunch of footprints here: ttp://logonex.eu/git/?p=svn.git;a=tree;f=levalib;h=f13a688b8f588acff7f081ac95999259bb0c01d2;hb=90743ea21068a0c473ce71da1fd457353310ccf4 feel free to pick anything you want. On Tue, 2 Feb 2010 08:32:51 -0500 Chris Cole cle...@gmail.com wrote: Hey all, I'm new to the gEDA community (and fairly new to electronics in general), and I have a pretty simple question for the gurus. I was working on converting a PIC project schematic into gschem when I realized that none of the Microchip IC's I was using were in the component library. What's the standard procedure for this? Is it easier to mooch off an existing part or to create your own? Thanks, Chris -- Levente Kovacs http://logonex.eu ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: new components
Christian Riggenbach wrote: I normaly use a Makefile to generate the symbols out of the ASCII-files. It is relatively straightforward to generate a big list of the pins, describe them and then split this list to the logical symbols. I'd like to see an example of that, if your project is open. Or, just some snippets from it would be good too. John ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: new components
On Tue, 2010-02-02 at 15:55 -0800, Ben Jackson wrote: On Tue, Feb 02, 2010 at 06:11:44PM -0500, resea...@ottomaneng.com wrote: I'm also creating symbols for an FPGA and a DSP which naturally has alot of pins. I've once heard of using multiple files for the symbols so you For a really simple example look at http://ad7gd.net/xc9536/ where I split the power and IO. Very interesting. I am contemplating my first BGA design with gEDA tools (AT91SAM9G45, Atmel ARM9). The part is a 18 x18 =324 ball device with row designators marked as A-V (missing I,O,Q,S,...). The Pin designators are labels K16, R2, G7, .. with the Alpha first, followed with the number. I tried to put in a pin label like this, but encountered problems with the online tool at (http://vivara.net/cgi-bin/djboxsym.cgi). Has anyone been making BGA parts with multiple symbol files? If so, what do I need to look out for as I go down the development path? (Will multiple symbols process as multiple items on the BOM?, Will the netlister correctly pickup the different symbols. Can Alpha-number designators be used at all? Thanks in advance Mike The symbols are also at http://gedasymbols.org/user/ben_jackson/ I could upload an Altera EP2C8 set of symbols if that would help. One symbol per IO bank, power, and config, iirc. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: new components
On Fri, Feb 05, 2010 at 03:33:25PM -0600, Mike Crowe wrote: tools (AT91SAM9G45, Atmel ARM9). The part is a 18 x18 =324 ball device ... Has anyone been making BGA parts with multiple symbol files? I've used PQ208 with one symbol per bank, one for general power (not IO-bank specific) and one for config and strap pins. All you have to do is give them the same refdes and it's all one part as far as the tools are concerned (actually I think you can suffix a lower case letter if you like and it will be ignored, eg U1a, U1b, but I didn't do that). Can Alpha-number designators be used at all? I think so. Like others I wrote my own boxsym program so I don't know if DJ's is trying to enforce numeric pins. Here's an example of a BGA on gedasymbols: http://www.gedasymbols.org/user/darrell_harmon/symbols/xilinx/index.html They have alphanumeric pin names. -- Ben Jackson AD7GD b...@ben.com http://www.ben.com/ ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: new components
Am Freitag 05 Februar 2010 22.33:25 schrieb Mike Crowe: Has anyone been making BGA parts with multiple symbol files? Yes, apparently ;) If so, what do I need to look out for as I go down the development path? Simply use the same designator for all parts, perhaps such with a special number. Will multiple symbols process as multiple items on the BOM?, Will the netlister correctly pickup the different symbols. Can Alpha-number designators be used at all? No problems here, I used a part with about ten symbols, but you have to keep track of the used pins and ref-deses. It is also important, that the splitted symbols have the same set of attributes (at least the footprint and ref-des), strange things can happen otherways. I normaly use a Makefile to generate the symbols out of the ASCII-files. It is relatively straightforward to generate a big list of the pins, describe them and then split this list to the logical symbols. All you have to do then is make. -- mit freundlichem Gruss Christian Riggenbach ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: new components
designators are labels K16, R2, G7, .. with the Alpha first, followed with the number. I tried to put in a pin label like this, but encountered problems with the online tool at Yeah, djboxsym assumes pins are numbered, as it sorts them and checks for missing ones when it dumps the stats at the end. It does allow a trailing letter, but I don't remember why I added that. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: new components
Mark Rages wrote: You are invited to use the interactive djboxsym editor on my website: http://vivara.net/cgi-bin/djboxsym.cgi I believe it is the easiest I maed a version of this to suit my style, (smaller compact box symbols), jgboxsym See http://www.gedasymbols.org/user/john_griessen/ JG ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: new components
resea...@ottomaneng.com wrote: I'm also creating symbols for an FPGA and a DSP which naturally has alot of pins. Any pointers to how to deal with large pin count symbols Give this a look: http://www.gedasymbols.org/user/john_griessen http://www.gedasymbols.org/user/john_griessen/tools/jgbanksym JG ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
gEDA-user: new components
Hey all, I'm new to the gEDA community (and fairly new to electronics in general), and I have a pretty simple question for the gurus. I was working on converting a PIC project schematic into gschem when I realized that none of the Microchip IC's I was using were in the component library. What's the standard procedure for this? Is it easier to mooch off an existing part or to create your own? Thanks, Chris ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: new components
Hi Chris, Welcome to the free world! If you've not already found it, a good place to start is here: http://geda.seul.org/wiki/geda:gsch2pcb_tutorial then have a good read of: http://geda.seul.org/wiki/geda:gschem_symbol_creation and http://geda.seul.org/wiki/geda:transistor_guide Then have a look at this bit of the FAQ here: http://geda.seul.org/wiki/geda:faq-gschem#gschem_symbols I only suggest doing it that way round because otherwise you may get distracted by the rest of the FAQ ... and when it comes to PCB footprints, I'd recommend you read this first: http://www.brorson.com/gEDA/land_patterns_20070818.odf or http://www.brorson.com/gEDA/land_patterns_20070818.pdf from: http://www.brorson.com/gEDA/ and then go back to: FAQs Quick Reference http://geda.seul.org/wiki/ :) Cheers, Andy. Signality Solutions t: +44 (0) 5601 720 580 m: +44 (0) 7796 538 192 skype: andyfierman www.signality.co.uk On 2 February 2010 13:32, Chris Cole cle...@gmail.com wrote: Hey all, I'm new to the gEDA community (and fairly new to electronics in general), and I have a pretty simple question for the gurus. I was working on converting a PIC project schematic into gschem when I realized that none of the Microchip IC's I was using were in the component library. What's the standard procedure for this? Is it easier to mooch off an existing part or to create your own? Thanks, Chris ___ 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: new components
I find it best(*) in the long run to crank out my own symbols. For things like the PIC, I use a modified version of DJ's djboxsym. I also have a couple of little generator scripts for other parts. -dave * By best, I mean best way to get symbols that match my personal taste. On Feb 2, 2010, at 5:32 AM, Chris Cole wrote: Hey all, I'm new to the gEDA community (and fairly new to electronics in general), and I have a pretty simple question for the gurus. I was working on converting a PIC project schematic into gschem when I realized that none of the Microchip IC's I was using were in the component library. What's the standard procedure for this? Is it easier to mooch off an existing part or to create your own? Thanks, Chris ___ 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: new components
On Tue, 2010-02-02 at 08:32 -0500, Chris Cole wrote: realized that none of the Microchip IC's I was using were in the component library. What's the standard procedure for this? Is it easier to mooch off an existing part or to create your own? If there is no symbol at www.gedasymbols.org I would suggest making a new one, maybe with tragesym. http://www.geda.seul.org/wiki/geda:tragesym_tutorial Please note, you do not need a spreadsheet program, a plain editor works fine. On Tue, 2010-02-02 at 14:35 +, Andy Fierman wrote: then have a good read of: http://geda.seul.org/wiki/geda:gschem_symbol_creation gEDA/gaf Symbol Creation Document by: Ales V. Hvezda / July 6th, 2004 Well, old documents may be fine. But people may think: Documentation is from 2004, so there seems not much progress in the last 6 years. At least this is not very good promotion. We may include DJ's fine, more recent tutorial in the list: http://www.delorie.com/pcb/docs/gs/gs.html Maybe we should have something like Getting Started at gpleda.org, with a few links to the most basic beginners documentation? ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: new components
http://www.delorie.com/pcb/docs/gs/gs.html That's in the pcb source tree now, too. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: new components
On Tue, Feb 2, 2010 at 7:32 AM, Chris Cole cle...@gmail.com wrote: Hey all, I'm new to the gEDA community (and fairly new to electronics in general), and I have a pretty simple question for the gurus. I was working on converting a PIC project schematic into gschem when I realized that none of the Microchip IC's I was using were in the component library. What's the standard procedure for this? Is it easier to mooch off an existing part or to create your own? Thanks, Chris You are invited to use the interactive djboxsym editor on my website: http://vivara.net/cgi-bin/djboxsym.cgi I believe it is the easiest way to get a basic symbol for something like a microprocessor. Regards, Mark markra...@gmail -- Mark Rages, Engineer Midwest Telecine LLC markra...@midwesttelecine.com ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: new components
On Tue, 2010-02-02 at 11:53 -0600, Mark Rages wrote: On Tue, Feb 2, 2010 at 7:32 AM, Chris Cole cle...@gmail.com wrote: Hey all, I'm new to the gEDA community (and fairly new to electronics in general), and I have a pretty simple question for the gurus. I was working on converting a PIC project schematic into gschem when I realized that none of the Microchip IC's I was using were in the component library. What's the standard procedure for this? Is it easier to mooch off an existing part or to create your own? Thanks, Chris You are invited to use the interactive djboxsym editor on my website: http://vivara.net/cgi-bin/djboxsym.cgi I believe it is the easiest way to get a basic symbol for something like a microprocessor. That is neat. You might consider modifying your CGI to return the mime-type: application/x-geda-symbol That should make it show up with an icon when offering a download on a gEDA installed system, (and possibly) open directly in gschem - depending on your web-browser. Best wishes, Peter C. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: new components
On Tue, 2010-02-02 at 18:17 +, Peter Clifton wrote: application/x-djboxsym or something like that. application/x-geda-djboxsym Would fit our upstream pattern better. Unfortunately, since djboxsym isn't shipped with gEDA sources (it could be if DJ wanted though), it would have to grow its own mime-type registration support. (One could steal the appropriate scripts from gEDA or PCB). ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: new components
I'm also creating symbols for an FPGA and a DSP which naturally has alot of pins. I've once heard of using multiple files for the symbols so you can move each freely (one for power, another for I/O, etc). This isn't covered in the symbol creation tutorial. Any pointers to how to deal with large pin count symbols (tragesym is great for initial symbol creation but i cant seem to make enough space between the blocks of pins). Omer Osman ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: new components
On Tue, Feb 02, 2010 at 06:11:44PM -0500, resea...@ottomaneng.com wrote: I'm also creating symbols for an FPGA and a DSP which naturally has alot of pins. I've once heard of using multiple files for the symbols so you For a really simple example look at http://ad7gd.net/xc9536/ where I split the power and IO. The symbols are also at http://gedasymbols.org/user/ben_jackson/ I could upload an Altera EP2C8 set of symbols if that would help. One symbol per IO bank, power, and config, iirc. -- Ben Jackson AD7GD b...@ben.com http://www.ben.com/ ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
