Re: gEDA-user: Still confused on using PCB to make footprints
DJ Delorie wrote: However, if PCB can find your footprints in the library window, try using the new importer (File-Import Schematics). I've not tried that yet. Any chance it will work with flattened hierarchic named schematics with repeated subschematics? John ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Still confused on using PCB to make footprints
I've not tried that yet. Any chance it will work with flattened hierarchic named schematics with repeated subschematics? It supports whatever gnetlist supports. It just doesn't use gsch2pcb to do the merge. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Still confused on using PCB to make footprints
On Thu, 27 May 2010 10:03:27 -0700, Mike Bushroe wrote: Could someone explain to me how to create a footprint in PCB with pins and assign names/numbers to them? Karel Kullhavy compiled a comprehensive howto here: http://ronja.twibright.com/guidelines/footprints.php There is a link to the howto in the geda wiki: http://geda.seul.org/wiki/geda:pcb_tips#how_do_i_draw_a_new_footprint ---)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+kmkop=get ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
gEDA-user: Still confused on using PCB to make footprints
I was trying to make footprints for the screw terminals I am using in my current project. They are on 5 mm spacing, not inches, so I was hesitant to start with a different footprint and try to change it for fear of getting the units mixed up and creating a mess. So I switched PCB to mm with 0.5mm grid spacing. I had no trouble laying out a silkscreen outline, and little trouble adding vias for the three through holes. But then I could not figure out how to change the vias to pins to assign them numbers and or names. And I am still confused on how to make sure that the pins in a footprint I make will match up with the correct nets from the schematic symbol pins. I looked through every drop down menu several times, and checked the key mapping info. I am sure that there is a tutorial somewhere that helps with this, but the only ones I have read seem to skip over the pin creation and naming, and verifying that they associate with the correct pins on the symbol. Could someone explain to me how to create a footprint in PCB with pins and assign names/numbers to them? And what information is needed to get gscht2pcb to correctly assign nets to pads? Is there any way to test a symbol - gsch2pcb - footprint translation without making a whole schematic? And is there a better tutorial on making footprints with PCB for gschem symbols that I should have been reading instead (and if so, where can I find it)? I managed to gerrymander a 2 row header perl script in inches into making the mm spaced single row of holes for the screw terminals using Luciani's perl scripts, but I was doubtful until they finally worked. Mike ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Still confused on using PCB to make footprints
Could someone explain to me how to create a footprint in PCB with pins and assign names/numbers to them? And what information is needed to get gscht2pcb to correctly assign nets to pads? http://www.delorie.com/pcb/docs/gs/ The second Your first board has that. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Still confused on using PCB to make footprints
Thanks DJ. The first part of that looks familiar. I guess I never read down far enough to get the footprint creation. I now realize that my problem was that the menu did not indicate that converting the buffer to an element converted vias to pins. I had no idea at all how the pin numbers were assigned. Is there a way to change the pin numbers if you create the vias in the wrong order? Or do you have to cut the element back to the buffer, break the element back to pieces, and manually move the vias around to get the pin numbers in the right places? And also how do you add names to the pins? I know that the gschem symbols have a pin number, a pin sequence number, and a pin label (John Doty is probably snarling already at how heavy this makes the symbols :)). Which governs the association of symbol pin to footprint pin? The pin number, or the pin name/label? And what does the pin sequence number do? Does adding a pin label override the pin numbers if they disagree? Hopefully at this point, most of these questions are for future learning. I _think_ I have the schematics ready to populate the board. The last big hold out, and what was going to be my first plea for help, was CONN8 finding the RJ45 footprint, then not finding it. In the process of documenting all the relevant files, I found that my RJ45.fp footprint was actually the html code for the page that gave the link to the footprint file! It found the file, but failed to make a footprint of it. Now that I have that solved, I should be able to get all elements to load tonight. Mike ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Still confused on using PCB to make footprints
Is there a way to change the pin numbers if you create the vias in the wrong order? The easiest way is to use a text editor. And also how do you add names to the pins? gsch2pcb and pcb's File-Import do that automatically, based on the pin names in the schematic. Which governs the association of symbol pin to footprint pin? The pin number, or the pin name/label? Pin number. And what does the pin sequence number do? It determines the order in which the pins are printed in the netlist. Not really useful for PCB, but useful for simulation models. Does adding a pin label override the pin numbers if they disagree? No. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Still confused on using PCB to make footprints
On May 27, 2010, at 2:13 PM, DJ Delorie wrote: And what does the pin sequence number do? It determines the order in which the pins are printed in the netlist. Not really useful for PCB, but useful for simulation models. Also needed for slotting. John Doty Noqsi Aerospace, Ltd. http://www.noqsi.com/ j...@noqsi.com ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Still confused on using PCB to make footprints
Thanks and DJ and John. Now I finally begin to feel comfortable with creating footprints in PCB. But I am still finding another problem with getting the whole pile to translate. I have made or downloaded several custom symbols and footprints. But not matter how many times I insert a gafrc into /gaf or /myproject, it still fails to help gsch2pcb find the custom footprints. For awhile, I was getting an error message saying possible unbalanced parenthesis, but that has gone away, even though I have not changed the parenthesis in either gafrc file. Only the project file seems to actually register when I use the double verbose mode, but even though the element-library is correctly mentioned, it is not searched when looking for footprints. Here is the gafrc in the /gaf directory: (component-library /media/TOSHIBA/gaf/symbols) (element-library /media/TOSHIBA/gaf/footprints) (element-library /media/TOSHIBA/gaf/packages) And here is the one from the project directory (component-library /media/TOSHIBA/gaf/symbols) (element-library /media/TOSHIBA/gaf/footprints) (element-library /media/TOSHIBA/gaf/packages) These are currently setup to run off my USB drive so that I can work off a KNOPPIX disk at work that has gschem and pcb, but the same files ar eon my home drive, with /media/TOSHIBA replaced with /home/mike. The project file is: component-library /media/TOSHIBA/gaf/symbols element-library /media/TOSHIBA/gaf/packages schematics ATMega164P_motherboard.sch ROV_2010_analog.sch ROV_2010_power.sch ROV_2010_Hydraulics.sch ROV_2010_I2C.sch ROV_2010_subprocesser.sch ROV_2010_camera.sch output -name ROV-2010_motherboard When processed, the verbose output is : Loading schematic [/media/TOSHIBA/gaf/ROV_2010/motherboard/ATMega164P_motherboard.sch] Loading schematic [/media/TOSHIBA/gaf/ROV_2010/motherboard/ROV_2010_analog.sch] Loading schematic [/media/TOSHIBA/gaf/ROV_2010/motherboard/ROV_2010_power.sch] Loading schematic [/media/TOSHIBA/gaf/ROV_2010/motherboard/ROV_2010_Hydraulics.sch] Loading schematic [/media/TOSHIBA/gaf/ROV_2010/motherboard/ROV_2010_I2C.sch] Loading schematic [/media/TOSHIBA/gaf/ROV_2010/motherboard/ROV_2010_subprocesser.sch] Loading schematic [/media/TOSHIBA/gaf/ROV_2010/motherboard/ROV_2010_camera.sch] Loading schematic [/media/TOSHIBA/gaf/ROV_2010/motherboard/ATMega164P_motherboard.sch] Loading schematic [/media/TOSHIBA/gaf/ROV_2010/motherboard/ROV_2010_analog.sch] Loading schematic [/media/TOSHIBA/gaf/ROV_2010/motherboard/ROV_2010_power.sch] Loading schematic [/media/TOSHIBA/gaf/ROV_2010/motherboard/ROV_2010_Hydraulics.sch] Loading schematic [/media/TOSHIBA/gaf/ROV_2010/motherboard/ROV_2010_I2C.sch] Loading schematic [/media/TOSHIBA/gaf/ROV_2010/motherboard/ROV_2010_subprocesser.sch] Loading schematic [/media/TOSHIBA/gaf/ROV_2010/motherboard/ROV_2010_camera.sch] Using the m4 processor for pcb footprints Loading schematic [/media/TOSHIBA/gaf/ROV_2010/motherboard/ATMega164P_motherboard.sch] Loading schematic [/media/TOSHIBA/gaf/ROV_2010/motherboard/ROV_2010_analog.sch] Loading schematic [/media/TOSHIBA/gaf/ROV_2010/motherboard/ROV_2010_power.sch] Loading schematic [/media/TOSHIBA/gaf/ROV_2010/motherboard/ROV_2010_Hydraulics.sch] Loading schematic [/media/TOSHIBA/gaf/ROV_2010/motherboard/ROV_2010_I2C.sch] Loading schematic [/media/TOSHIBA/gaf/ROV_2010/motherboard/ROV_2010_subprocesser.sch] Loading schematic [/media/TOSHIBA/gaf/ROV_2010/motherboard/ROV_2010_camera.sch] Reading project file: project component-library /media/TOSHIBA/gaf/symbols element-library /media/TOSHIBA/gaf/packages schematics ATMega164P_motherboard.sch ROV_2010_analog.sch ROV_2010_power.sch ROV_2010_Hydraulics.sch ROV_2010_I2C.sch ROV_2010_subprocesser.sch ROV_2010_camera.sch output -name ROV-2010_motherboard Processing PCBLIBPATH=/usr/share/pcb/pcblib-newlib:/usr/share/pcb/newlib Adding /usr/share/pcb/pcblib-newlib to the newlib search path Adding /usr/share/pcb/newlib to the newlib search path Running command: gnetlist -g pcbpins -o ATMega164P_motherboard.cmd ATMega164P_motherboard.sch ROV_2010_analog.sch ROV_2010_power.sch ROV_2010_Hydraulics.sch ROV_2010_I2C.sch ROV_2010_subprocesser.sch ROV_2010_camera.sch Running command: gnetlist -g PCB -o ATMega164P_motherboard.net ATMega164P_motherboard.sch ROV_2010_analog.sch ROV_2010_power.sch ROV_2010_Hydraulics.sch ROV_2010_I2C.sch ROV_2010_subprocesser.sch ROV_2010_camera.sch Default m4-pcbdir: /usr/share/pcb/m4 gnet-gsch2pcb-tmp.scm override file: (define m4-pcbdir /usr/share/pcb/m4) (define gsch2pcb:use-m4 #t) Running command: gnetlist -g gsch2pcb -o ATMega164P_motherboard.pcb -m gnet-gsch2pcb-tmp.scm
Re: gEDA-user: Still confused on using PCB to make footprints
Here's one of my project files (for gsch2pcb): -- laminator.prj -- m4-pcbdir /envy/dj/geda/share/pcb/m4 elements-dir /envy/dj/geda/gedasymbols/www/user/dj_delorie/footprints elements-dir ./footprints schematics laminator.sch output-name laminator -- -- However, if PCB can find your footprints in the library window, try using the new importer (File-Import Schematics). If you have more than one toplevel *.sch you'll need to read the docs on the Import() action to see how to add the names, but it uses PCB's internal library path instead of gsc2pcb's paths. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
