Re: gEDA-user: question about how to get pads on my circuit board for power and gnd...
Ed Hartnett wrote: So it looks like I am missing an m4 footprint called SIP2N. I will took a look at gedasymbols, but it was not there. Can you email it? The attribute footprint=SIP2N was brought by the connector symbol in the default. However, the default lib of PCB does not include a footprint with this name. (Oh my. Most symbols omit footprint attributes. And one of the few that does, presents an invalid value...) I attached a version of the schematics with the footprint attributes changed to HEADER2_1. This should be included in your PCB install. -- Search for HEADER2_1.fp. For reference I also attached a PCB with components as placed by import schematics from the file menu of PCB. ---)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 - not happy with moderation of geda-user mailinglist gndcon.pcb Description: application/pcb-layout gndcon.sch Description: application/geda-schematic ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: question about how to get pads on my circuit board for power and gnd...
Wow, thanks for all the great information guys!! I am starting to work through all the info you provided; I'll send an update when I have tried out some of your suggestions and studied the example. Thanks again! Ed ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: question about how to get pads on my circuit board for power and gnd...
Howdy Kai-Martin! Thanks for the answers and especially the example! I am looking at it closely. You have a bunch of gnd symbols around the place. When you create your netlist, these are not going to be on it, correct? Because you have these pins connected to grn symbols without a footprint, you will have to add the traces to the correct pins in pcb. Is this correct? Or am I missing something? On Sat, Jul 9, 2011 at 7:23 AM, Kai-Martin Knaak [1]k...@lilalaser.de wrote: Ed Hartnett wrote: Do I add a connector on gschem yes. and use it instead of then GND/5V symbols? no. You add just one connector and connect it with the gnd-symbol. Then you connect the gnd symbol wherever you need GND potential. Or do I associate a footprint of HEADER2_1 with each of them? Or with one of them? The footprint should be associated with the connector symbol. See the attached example. Although I used symbols and footprints from the default library of gschem and PCB, I'd recommend to also look at [2]gedasymbols.org . (@Ales: Yes, I am working on the beginners lib. Progress is slow though. See my recent activity at gedasymbols) ---)kaimartin(--- -- Kai-Martin Knaak Email: [3]k...@familieknaak.de not happy with moderation of geda.user ___ geda-user mailing list [4]geda-user@moria.seul.org [5]http://www.seul.org/cgi-bin/mailman/listinfo/geda-user References 1. mailto:k...@lilalaser.de 2. http://gedasymbols.org/ 3. mailto:k...@familieknaak.de 4. mailto:geda-user@moria.seul.org 5. 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: question about how to get pads on my circuit board for power and gnd...
Howdy Kai-Marten! I ran your example through gsch2pcb and got the following output: = Using the m4 processor for pcb footprints CONN2: can't find PCB element for footprint SIP2N (value=unknown) So device CONN2 will not be in the layout. CONN1: can't find PCB element for footprint SIP2N (value=unknown) So device CONN1 will not be in the layout. -- Done processing. Work performed: 1 file elements and 2 m4 elements added to gndcon.pcb. 2 elements could not be found. So gndcon.pcb is incomplete. So it looks like I am missing an m4 footprint called SIP2N. I will took a look at gedasymbols, but it was not there. Can you email it? Thanks! Ed ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: question about how to get pads on my circuit board for power and gnd...
Ed Hartnett wrote: You have a bunch of gnd symbols around the place. When you create your netlist, these are not going to be on it, correct? The netlist does not contain symbols or footprints anyway -- just pins and nets :-) The gnd symbols make sure, a particular pin is connected to the gnd net. Because you have these pins connected to grn symbols without a footprint, you will have to add the traces to the correct pins in pcb. Is this correct? yes. BTW, you may try the new import_schematic feature of PCB. This creates the netlist on the fly and imports it into the layout with much less hassle than the traditional gsch2pcb work flow. ---)kaimartin(--- -- Kai-Martin Knaak Email: k...@familieknaak.de http://pool.sks-keyservers.net:11371/pks/lookup?search=0x6C0B9F53 not happy with moderation of geda-user ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: question about how to get pads on my circuit board for power and gnd...
On Sat, 9 Jul 2011 05:19:01 -0600 Ed Hartnett edwardjameshartn...@gmail.com wrote: On Mon, Jul 4, 2011 at 7:46 AM, DJ Delorie d...@delorie.com wrote: I am trying to make my first PCB and I have selected a super-simple circuit to start with, a 555 astable circuit. It's a single-sided board, and I'm going to etch it myself - something I've always wanted to try. But what footprints do I use for the GND and VCC connections? I guess I would just like these to be two pads on the PCB. Is there a way to tell gschem this? Or do I just manually make that change in the pcb program? Usually, you would add one two-pin connector, or two one-pin connectors, for the power connection. There are a range of footprints available for this - if you just want to solder wires to it, HEADER2_1 is sufficient - it's just two pins on 0.1 centers. Would this be done in gschem? Or in pcb? In gschem I have a symbol for gnd, and there is no footprint associated with it. There is another symbol for +5 V. Do I add a connector on gschem and use it instead of then GND/5V symbols? Or do I associate a footprint of HEADER2_1 with each of them? Or with one of them? I think Kai-Martin probably answered this pretty thoroughly, but I'll comment that, like you, I once wanted to add two plain old surface mount pads to which I could solder my power/ground supply wires. You correctly noted that GND/+5V symbols don't have a footprint associated. These “power rail” symbols, like the input/output pin symbols (input-2.sym, etc.), are schematic conveniences only. You could remove them and instead connect all nodes with actual net lines instead, but that is often very messy. The power rail and I/O pin make schematics cleaner. What you want is to use is either (1) use connector2-1.sym, and then assign it a 2-pin footprint like “JUMPER2” (2-pin SIP, 100 mil pitch through-hole header). Then connect pin 1 of the connector to your ground net and pin 2 to your power net (or vice-versa). If you want surface-mount pads, you can assign the connector component a 2-pin SMD footprint like “RESC4532M”. or if you want to be able to separately place the power and ground connections on the PCB layout: (2) insert two one-pin symbols (e.g., terminal-1.sym connector1-2.sym, but note that these are “heavy” symbols and you need to change the footprint unless you want the default though-hole pin footprint). Connect one symbol to your ground net and one to your power rail net. Assign the appropriate footprint--for a through-hole footprint, use “JUMPER1”, “CONNECTOR 1 1”, or “SIP1N”; for a surface-mount footprint, use a test-pad symbol or other single-pad SMD footprint (look on gedasymbols.org; AFAIK the default pcb footprint library doesn't have any single-pad SMD footprints). Tip: If you use a 2-pin through-hole JUMPER2 footprint, you can solder a 2-pin header from a ubiquitous single-row breakaway header (100 mil) and then have a detachable power supply connection. I have found the low-cost Molex KK-100 series kit (see [1] below) invaluable for all sorts of connections like this. With a bit of practice, you will be able to quickly made a wide variety of cables from 1 to 10+ pins. I use bits of ribbon cable to make most signal connectors because it's very convenient and looks tidy when you're done. Regards, Colin References [1] Molex KK-100 Connector Kit With premium crimp tool (I highly recommend this option): Molex Part #: 76650-0009 Mouser link: http://www.mouser.com/ProductDetail/Molex/76650-0009/?qs=sGAEpiMZZMtsLRyDR9nM1%2ffCLkgKsWdRr36mItq8jVo%3d With basic crimp tool: Molex Part #: 76650-0007 Mouser link: http://www.mouser.com/ProductDetail/Molex/76650-0007/?qs=sGAEpiMZZMtsLRyDR9nM1%2ffCLkgKsWdRSyrCqTUdKBE%3d ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: question about how to get pads on my circuit board for power and gnd...
On Mon, Jul 4, 2011 at 7:46 AM, DJ Delorie [1]d...@delorie.com wrote: I am trying to make my first PCB and I have selected a super-simple circuit to start with, a 555 astable circuit. It's a single-sided board, and I'm going to etch it myself - something I've always wanted to try. But what footprints do I use for the GND and VCC connections? I guess I would just like these to be two pads on the PCB. Is there a way to tell gschem this? Or do I just manually make that change in the pcb program? Usually, you would add one two-pin connector, or two one-pin connectors, for the power connection. There are a range of footprints available for this - if you just want to solder wires to it, HEADER2_1 is sufficient - it's just two pins on 0.1 centers. Would this be done in gschem? Or in pcb? In gschem I have a symbol for gnd, and there is no footprint associated with it. There is another symbol for +5 V. Do I add a connector on gschem and use it instead of then GND/5V symbols? Or do I associate a footprint of HEADER2_1 with each of them? Or with one of them? Thanks for answering beginner questions! Ed References 1. mailto:d...@delorie.com ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: question about how to get pads on my circuit board for power and gnd...
Ed Hartnett wrote: Do I add a connector on gschem yes. and use it instead of then GND/5V symbols? no. You add just one connector and connect it with the gnd-symbol. Then you connect the gnd symbol wherever you need GND potential. Or do I associate a footprint of HEADER2_1 with each of them? Or with one of them? The footprint should be associated with the connector symbol. See the attached example. Although I used symbols and footprints from the default library of gschem and PCB, I'd recommend to also look at gedasymbols.org . (@Ales: Yes, I am working on the beginners lib. Progress is slow though. See my recent activity at gedasymbols) ---)kaimartin(--- -- Kai-Martin Knaak Email: k...@familieknaak.de not happy with moderation of geda.user gndcon.sch Description: application/geda-schematic ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: question about how to get pads on my circuit board for power and gnd...
I am trying to make my first PCB and I have selected a super-simple circuit to start with, a 555 astable circuit. It's a single-sided board, and I'm going to etch it myself - something I've always wanted to try. But what footprints do I use for the GND and VCC connections? I guess I would just like these to be two pads on the PCB. Is there a way to tell gschem this? Or do I just manually make that change in the pcb program? Usually, you would add one two-pin connector, or two one-pin connectors, for the power connection. There are a range of footprints available for this - if you just want to solder wires to it, HEADER2_1 is sufficient - it's just two pins on 0.1 centers. Creating footprints isn't that hard - adding a one-pin pad for soldering or test points is a suitable beginner's exercise. See http://www.delorie.com/pcb/docs/gs/ for a tutorial. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
