Re: gEDA-user: PGA 100 footprint
On 02/12/2011 06:33 PM, Kai-Martin Knaak wrote: Sounds like a lot of work. Yes, sounds like scriptable work. I've already done one connector as you described. Now I'd like to do the next with a script. The way I generate rows of pads with DJ's http://www.gedasymbols.org/user/dj_delorie/tools/dilpad.html tool. The code for dil pads is right there in gedasymbols.org. I need to look at it is all... JG ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: PGA 100 footprint
On 2/12/2011 4:33 PM, Kai-Martin Knaak wrote: John Griessen wrote: How would one generate rows of pads on both component and solder side? If the pads are the same size, shape and position on both sides you can do this in a text editor by copying the pads, and pasting twice. You then change the flags for the second set of pads for the second side. You can either increment the pad numbers as well, if the connector is bifurcated. Phil ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: PGA 100 footprint
John Griessen wrote: > How would one generate rows of pads on both component and solder side? > > For old fashioned edge connectors... I'd use the PCB GUI: 1) Set the grid to a multiple of the distance of the fingers. 2) Draw track segment with appropriate width on the first layer 3) copy-paste to yield a row of tracks 4) copy the whole row to buffer 5) paste the row somewhere. 6) select the second layer 7) do [m] on all segments of the second row to move them to the second layer 8) move the second row to the same place as the first row 9) Go over all segments with [n] and enter the correct pad number 10) draw the silk 11) copy everything to paste buffer 12) do convert_to_element 13) paste the component somewhere 14) go over all pads with [q] to make them square 15) save 16) run my convenience script set_pinnumber.awk to set the pin numbers to the same value as the pin names. 17) copy component to buffer 18) save_buffer_as from the buffer menu 19) upload to gedasymbols.org Sounds like a lot of work. But it is straight forward. ---<)kaimartin(>--- -- Kai-Martin Knaak Email: k...@familieknaak.de Öffentlicher PGP-Schlüssel: http://pool.sks-keyservers.net:11371/pks/lookup?search=0x6C0B9F53 ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: PGA 100 footprint
On 02/12/2011 02:35 PM, Darrell Harmon wrote: It would be possible to add a PGA mode to footgen, but How would one generate rows of pads on both component and solder side? For old fashioned edge connectors... JG ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: PGA 100 footprint
On Sat, Feb 12, 2011 at 12:49 PM, Phil Taylor wrote: > On Feb 12, 2011, at 10:37 AM, Oliver King-Smith wrote: > >> Does anyone have a PGA100 foot >> If I layout the footprint would folks recommend using PCB or is there a >> better way to do this style of footprint? > > Use a script, a spreadsheet or a text editor or a combination of these based > on what comes easy to you. > > Phil http://dlharmon.com/geda/footgen.html To make a PGA instead of a BGA: add these immediately after the def bga(attrlist): line drill = findattr(attrlist, "drill") paddia = findattr(attrlist, "paddia") polyclear = findattr(attrlist, "polyclear") maskclear = findattr(attrlist, "maskclear") change bgaelt = bgaelt + ball(x, y, balldia, polyclear, maskclear, ballname(col,row)) to bgaelt = bgaelt + pin(x,y,paddia,drill,ballname(col,row),polyclear,maskclear) You will need to define drill, paddia, polyclear and maskclear in addition to the usual BGA parameters. It would be possible to add a PGA mode to footgen, but I don't want a patch as they are relatively rare. Darrell Harmon ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: PGA 100 footprint
On Feb 12, 2011, at 10:37 AM, Oliver King-Smith wrote: > Does anyone have a PGA100 foot > If I layout the footprint would folks recommend using PCB or is there a > better way to do this style of footprint? Use a script, a spreadsheet or a text editor or a combination of these based on what comes easy to you. Phil ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
gEDA-user: PGA 100 footprint
Does anyone have a PGA100 footprint made already? I think the footprints are pretty standardized, but in case they are not, this is the socket I am using: [1]http://www.mouser.com/ProductDetail/Mill-Max/510-93-100-13-062001/?q s=kJUkXSjFC7zF7XgyqhSPcw%3d%3d If I layout the footprint would folks recommend using PCB or is there a better way to do this style of footprint? Oliver References 1. http://www.mouser.com/ProductDetail/Mill-Max/510-93-100-13-062001/?qs=kJUkXSjFC7zF7XgyqhSPcw%3d%3d ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
