Re: gEDA-user: no pins in JUMPER10
On Thu, 9 Nov 2006 15:00:19 -0500 "John Luciani" <[EMAIL PROTECTED]> graced us with this prophetic message: [snip] > I did not add Y for crystal since I have never seen a schematic that > used that convention (I also have not seen a lot of Spice schematics ;-) I'll chime in here real quick. Background: I work as a PC assembly reworker at a contract electronics manufacturer. I don't deal with the schematics directly but I do deal with the PCBs and I've seen crystals indicated via the silk screen on the PCB as either Xn or Yn, mostly depending on what the customer wanted when they designer their circuit. Further, I've also seen RPn for a Resister Pack, which is equivalent to a resistor network. And Dn, LDn, and LEDn for LEDs. And TVn for Transient Voltage Suppressors (Transorbs?). > I have also seen SPKR for speaker and piezoelectronic buzzers as well as > PB for just piezoelectronic buzzers. I did not add these since there is > probably something better. I've also seen PBn indicate a Push Button switch (momentary tactile type, generally). > > (* jcl *) > > -- > http://www.luciani.org > > > ___ > geda-user mailing list > geda-user@moria.seul.org > http://www.seul.org/cgi-bin/mailman/listinfo/geda-user Essentially, what this all means is that the really common parts have defacto standard designators, but parts that aren't used quite as much will have some variations. Hope this helps some. Rick. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: no pins in JUMPER10
On 11/9/06, joeft <[EMAIL PROTECTED]> wrote: I would suggest that "Y" be used for crystals rather than "X", which might prevent collisions when someone uses their netlist for SPICE simulations that have subcircuits. Some lesser used prefixes I've seen: F Fuse and some two letter prefixes (if you can deal with more than one letter prefixes...) TP Test point FB Ferrite bead RN Resistor Network Thanks Joe. I don't know how I forgot Fuse or TP (which I use all the time). I added Fuse, Testpoint, Ferrite Bead and Resistor Network to the Wiki entry that Carlos created. I did not add Y for crystal since I have never seen a schematic that used that convention (I also have not seen a lot of Spice schematics ;-) I have also seen SPKR for speaker and piezoelectronic buzzers as well as PB for just piezoelectronic buzzers. I did not add these since there is probably something better. (* jcl *) -- 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: no pins in JUMPER10
On 11/9/06, Carlos Nieves Ónega <[EMAIL PROTECTED]> wrote: El mié, 08-11-2006 a las 08:14 -0500, John Luciani escribió: [snip] > Below are the refdes conventions that I use (that I have > seen on *many* schematics). > > I may have missed a few since this is BC (before Cappuccino). > > (* jcl *) > > Substitute an integer value for > > value component type > - > R Resistor > L Inductor > C Capacitor > > B Battery > J Connector > P Connector (usually plugs that mate with J) > K Relay > S Switch > T Transformer > > D Diode > Q Transistor > U IC > X Crystal Added to the wiki: http://geda.seul.org/wiki/geda:master_attributes_list#refdes Thanks, Carlos Carlos, Thanks for adding these. (* jcl *) -- 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: no pins in JUMPER10
I would suggest that "Y" be used for crystals rather than "X", which might prevent collisions when someone uses their netlist for SPICE simulations that have subcircuits. Some lesser used prefixes I've seen: F Fuse and some two letter prefixes (if you can deal with more than one letter prefixes...) TP Test point FB Ferrite bead RN Resistor Network Joe T Carlos Nieves Ónega wrote: El mié, 08-11-2006 a las 08:14 -0500, John Luciani escribió: [snip] Below are the refdes conventions that I use (that I have seen on *many* schematics). I may have missed a few since this is BC (before Cappuccino). (* jcl *) Substitute an integer value for value component type - R Resistor L Inductor C Capacitor B Battery J Connector P Connector (usually plugs that mate with J) K Relay S Switch T Transformer D Diode Q Transistor U IC X Crystal Added to the wiki: http://geda.seul.org/wiki/geda:master_attributes_list#refdes Thanks, Carlos ___ 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: no pins in JUMPER10
El mié, 08-11-2006 a las 08:14 -0500, John Luciani escribió: [snip] > Below are the refdes conventions that I use (that I have > seen on *many* schematics). > > I may have missed a few since this is BC (before Cappuccino). > > (* jcl *) > > Substitute an integer value for > > value component type > - > R Resistor > L Inductor > C Capacitor > > B Battery > J Connector > P Connector (usually plugs that mate with J) > K Relay > S Switch > T Transformer > > D Diode > Q Transistor > U IC > X Crystal Added to the wiki: http://geda.seul.org/wiki/geda:master_attributes_list#refdes Thanks, Carlos ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: no pins in JUMPER10
On 11/9/06, Giorgenes Gelatti <[EMAIL PROTECTED]> wrote: by "all these things" i mean gschem and pcb. But do not worry, it's just the complaining of a newbie user. :) I mean, if it's mandatory to have things named "J", "R", why none of gschem, gsch2pcb or pcb said me so? I agree that gsch2pcb or PCB should report the fact that the nets in the netlist are not going to be connected in the layout. It's still weird for me, but i'm sure there is some reason for that, I just don't know it yet. Developer resources to add input checking. (* jcl *) -- 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: no pins in JUMPER10
by "all these things" i mean gschem and pcb. But do not worry, it's just the complaining of a newbie user. :) I mean, if it's mandatory to have things named "J", "R", why none of gschem, gsch2pcb or pcb said me so? It's still weird for me, but i'm sure there is some reason for that, I just don't know it yet. Well, I'll try to finish my work now. Thank you very much guys, for you time and patience. 2006/11/8, John Luciani <[EMAIL PROTECTED]>: On 11/8/06, Giorgenes Gelatti <[EMAIL PROTECTED]> wrote: > I've changed the refdes as you said and it worked. > Thank you. > > You know, I`m new to electronics, geda and such. > But it seems too tricky for me. > I just wonder why are all these things necessary. I am not sure what you mean by "all these things". Your first problem occured because the gsch2pcb script places all of the components on top of each other. It would be nice if the script spaced the components out but you now know how to deal with that issue. Your second problem occured because you were not familiar with the reference designator syntax that PCB requires. If you follow the outline I posted you should be OK. You now should be able to proceed with your layout. Here are a couple of things to be careful of --- 1. Verify that the footprints you choose meet the manufacturer's package specification for the components you are using. Usually each component datasheet contains a recommended footprint. 2. Set the DRC rules to match the PCB vendor that you plan on using and run the DRC *frequently* as you are doing your board. It is much easier to fix the errors as you go than to end up with a huge list (which can be quite discouraging). 3. Always check the Gerber files prior to sending them to the PCB vendor. I use gerbv to do this. (* jcl *) -- http://www.luciani.org ___ 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: no pins in JUMPER10
On 11/8/06, Giorgenes Gelatti <[EMAIL PROTECTED]> wrote: I've changed the refdes as you said and it worked. Thank you. You know, I`m new to electronics, geda and such. But it seems too tricky for me. I just wonder why are all these things necessary. I am not sure what you mean by "all these things". Your first problem occured because the gsch2pcb script places all of the components on top of each other. It would be nice if the script spaced the components out but you now know how to deal with that issue. Your second problem occured because you were not familiar with the reference designator syntax that PCB requires. If you follow the outline I posted you should be OK. You now should be able to proceed with your layout. Here are a couple of things to be careful of --- 1. Verify that the footprints you choose meet the manufacturer's package specification for the components you are using. Usually each component datasheet contains a recommended footprint. 2. Set the DRC rules to match the PCB vendor that you plan on using and run the DRC *frequently* as you are doing your board. It is much easier to fix the errors as you go than to end up with a huge list (which can be quite discouraging). 3. Always check the Gerber files prior to sending them to the PCB vendor. I use gerbv to do this. (* jcl *) -- 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: no pins in JUMPER10
I've changed the refdes as you said and it worked. Thank you. You know, I`m new to electronics, geda and such. But it seems too tricky for me. I just wonder why are all these things necessary. 2006/11/8, John Luciani <[EMAIL PROTECTED]>: On 11/8/06, John Luciani <[EMAIL PROTECTED]> wrote: > > Substitute an integer value for This should be Substitute a cardinal number for (* jcl *) -- http://www.luciani.org ___ 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: no pins in JUMPER10
On 11/8/06, John Luciani <[EMAIL PROTECTED]> wrote: Substitute an integer value for This should be Substitute a cardinal number for (* jcl *) -- 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: no pins in JUMPER10
On 11/8/06, Giorgenes Gelatti <[EMAIL PROTECTED]> wrote: there is goes.. thank you I changed the refdes value of "pinbar" to "J1" and the value of "serial" to "J2" and the netlist loads. Below are the refdes conventions that I use (that I have seen on *many* schematics). I may have missed a few since this is BC (before Cappuccino). (* jcl *) Substitute an integer value for value component type - R Resistor L Inductor C Capacitor B Battery J Connector P Connector (usually plugs that mate with J) K Relay S Switch T Transformer D Diode Q Transistor U IC X Crystal -- 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: no pins in JUMPER10
there is goes.. thank you 2006/11/7, John Luciani <[EMAIL PROTECTED]>: On 11/7/06, Giorgenes Gelatti <[EMAIL PROTECTED]> wrote: > sure. > And I did the "disperse all elements" too. > > 2006/11/7, Dan McMahill <[EMAIL PROTECTED]>: > > Giorgenes Gelatti wrote: > > > > > > 2006/11/6, John Luciani <[EMAIL PROTECTED]>: > > > > > >> On 11/6/06, Giorgenes Gelatti <[EMAIL PROTECTED]> wrote: > > >> > I got a simpler circuit that is not working. > > >> > I have snap turned on, but can't see a way of making it works :( > > >> > > > >> > > >> What specifically isn't working? > > >> > > >> the netlist produced --- > > >> > > >> unnamed_net9serial-2 pinbar-9 > > >> unnamed_net8serial-1 pinbar-10 > > >> unnamed_net7serial-4 pinbar-7 > > >> unnamed_net6serial-6 pinbar-5 > > >> unnamed_net5serial-8 pinbar-3 > > >> unnamed_net4serial-3 pinbar-8 > > >> unnamed_net3serial-5 pinbar-6 > > >> unnamed_net2serial-7 pinbar-4 > > >> unnamed_net1serial-9 pinbar-2 > > >> > > >> which is all of the connections. I do not have the same set of > > >> footprints so I > > >> did not check out a PCB file. > > >> > > >> (* jcl *) > > > > > In pcb the components are not connected. :-( Attach the PCB file and the netlist file. (* jcl *) -- http://www.luciani.org ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user db2bar.net Description: Binary data db2bar.pcb Description: Binary data ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: no pins in JUMPER10
On 11/7/06, Giorgenes Gelatti <[EMAIL PROTECTED]> wrote: sure. And I did the "disperse all elements" too. 2006/11/7, Dan McMahill <[EMAIL PROTECTED]>: > Giorgenes Gelatti wrote: > > > > 2006/11/6, John Luciani <[EMAIL PROTECTED]>: > > > >> On 11/6/06, Giorgenes Gelatti <[EMAIL PROTECTED]> wrote: > >> > I got a simpler circuit that is not working. > >> > I have snap turned on, but can't see a way of making it works :( > >> > > >> > >> What specifically isn't working? > >> > >> the netlist produced --- > >> > >> unnamed_net9serial-2 pinbar-9 > >> unnamed_net8serial-1 pinbar-10 > >> unnamed_net7serial-4 pinbar-7 > >> unnamed_net6serial-6 pinbar-5 > >> unnamed_net5serial-8 pinbar-3 > >> unnamed_net4serial-3 pinbar-8 > >> unnamed_net3serial-5 pinbar-6 > >> unnamed_net2serial-7 pinbar-4 > >> unnamed_net1serial-9 pinbar-2 > >> > >> which is all of the connections. I do not have the same set of > >> footprints so I > >> did not check out a PCB file. > >> > >> (* jcl *) > > > In pcb the components are not connected. :-( Attach the PCB file and the netlist file. (* jcl *) -- 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: no pins in JUMPER10
sure. And I did the "disperse all elements" too. 2006/11/7, Dan McMahill <[EMAIL PROTECTED]>: Giorgenes Gelatti wrote: > > 2006/11/6, John Luciani <[EMAIL PROTECTED]>: > >> On 11/6/06, Giorgenes Gelatti <[EMAIL PROTECTED]> wrote: >> > I got a simpler circuit that is not working. >> > I have snap turned on, but can't see a way of making it works :( >> > >> >> What specifically isn't working? >> >> the netlist produced --- >> >> unnamed_net9serial-2 pinbar-9 >> unnamed_net8serial-1 pinbar-10 >> unnamed_net7serial-4 pinbar-7 >> unnamed_net6serial-6 pinbar-5 >> unnamed_net5serial-8 pinbar-3 >> unnamed_net4serial-3 pinbar-8 >> unnamed_net3serial-5 pinbar-6 >> unnamed_net2serial-7 pinbar-4 >> unnamed_net1serial-9 pinbar-2 >> >> which is all of the connections. I do not have the same set of >> footprints so I >> did not check out a PCB file. >> >> (* jcl *) > In pcb the components are not connected. :-( Did you open the .pcb file and then load the netlist and then press 'o' (optimize rats)? -Dan ___ 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: no pins in JUMPER10
Giorgenes Gelatti wrote: 2006/11/6, John Luciani <[EMAIL PROTECTED]>: On 11/6/06, Giorgenes Gelatti <[EMAIL PROTECTED]> wrote: > I got a simpler circuit that is not working. > I have snap turned on, but can't see a way of making it works :( > What specifically isn't working? the netlist produced --- unnamed_net9serial-2 pinbar-9 unnamed_net8serial-1 pinbar-10 unnamed_net7serial-4 pinbar-7 unnamed_net6serial-6 pinbar-5 unnamed_net5serial-8 pinbar-3 unnamed_net4serial-3 pinbar-8 unnamed_net3serial-5 pinbar-6 unnamed_net2serial-7 pinbar-4 unnamed_net1serial-9 pinbar-2 which is all of the connections. I do not have the same set of footprints so I did not check out a PCB file. (* jcl *) > In pcb the components are not connected. :-( Did you open the .pcb file and then load the netlist and then press 'o' (optimize rats)? -Dan ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: no pins in JUMPER10
In pcb the components are not connected. :-( 2006/11/6, John Luciani <[EMAIL PROTECTED]>: On 11/6/06, Giorgenes Gelatti <[EMAIL PROTECTED]> wrote: > I got a simpler circuit that is not working. > I have snap turned on, but can't see a way of making it works :( > What specifically isn't working? the netlist produced --- unnamed_net9serial-2 pinbar-9 unnamed_net8serial-1 pinbar-10 unnamed_net7serial-4 pinbar-7 unnamed_net6serial-6 pinbar-5 unnamed_net5serial-8 pinbar-3 unnamed_net4serial-3 pinbar-8 unnamed_net3serial-5 pinbar-6 unnamed_net2serial-7 pinbar-4 unnamed_net1serial-9 pinbar-2 which is all of the connections. I do not have the same set of footprints so I did not check out a PCB file. (* jcl *) -- http://www.luciani.org ___ 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: no pins in JUMPER10
On 11/6/06, Giorgenes Gelatti <[EMAIL PROTECTED]> wrote: I got a simpler circuit that is not working. I have snap turned on, but can't see a way of making it works :( What specifically isn't working? the netlist produced --- unnamed_net9serial-2 pinbar-9 unnamed_net8serial-1 pinbar-10 unnamed_net7serial-4 pinbar-7 unnamed_net6serial-6 pinbar-5 unnamed_net5serial-8 pinbar-3 unnamed_net4serial-3 pinbar-8 unnamed_net3serial-5 pinbar-6 unnamed_net2serial-7 pinbar-4 unnamed_net1serial-9 pinbar-2 which is all of the connections. I do not have the same set of footprints so I did not check out a PCB file. (* jcl *) -- 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: no pins in JUMPER10
I got a simpler circuit that is not working. I have snap turned on, but can't see a way of making it works :( 2006/11/6, John Luciani <[EMAIL PROTECTED]>: On 11/6/06, Giorgenes Gelatti <[EMAIL PROTECTED]> wrote: > I didn't put footprints in some components becouse I didn't get any > error about that. They seem to have a default footprint already. > Is it a problem to leave the default footprints? The schematic you posted, programmer.sch, did not have footprints for the components for max1, max2, trans1, uc1 (there may be others). Select the component, right-click and go to the edit menu. The only attribute that is set is refdes. (* jcl *) -- http://www.luciani.org ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user db2bar.sch Description: Binary data ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: no pins in JUMPER10
On 11/6/06, Giorgenes Gelatti <[EMAIL PROTECTED]> wrote: I didn't put footprints in some components becouse I didn't get any error about that. They seem to have a default footprint already. Is it a problem to leave the default footprints? The schematic you posted, programmer.sch, did not have footprints for the components for max1, max2, trans1, uc1 (there may be others). Select the component, right-click and go to the edit menu. The only attribute that is set is refdes. (* jcl *) -- 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: no pins in JUMPER10
I didn't put footprints in some components becouse I didn't get any error about that. They seem to have a default footprint already. Is it a problem to leave the default footprints? 2006/11/6, John Luciani <[EMAIL PROTECTED]>: On 11/5/06, Giorgenes Gelatti <[EMAIL PROTECTED]> wrote: > i'm sending my project. it's very simple. > Thank you. One big problem is that a number of your components do not footprints. For example --- max1, max2, trans1, uc1. The majority of your connections go to these devices. You need to pick the appropriate footprints for the devices that you are using. (* jcl *) -- http://www.luciani.org ___ 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: no pins in JUMPER10
On 11/5/06, Giorgenes Gelatti <[EMAIL PROTECTED]> wrote: i'm sending my project. it's very simple. Thank you. One big problem is that a number of your components do not footprints. For example --- max1, max2, trans1, uc1. The majority of your connections go to these devices. You need to pick the appropriate footprints for the devices that you are using. (* jcl *) -- 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: no pins in JUMPER10
On 11/5/06, Giorgenes Gelatti <[EMAIL PROTECTED]> wrote: I got it working in the example, but it still doesn't work in my project. :( How can I check for errors, like the "on grid" stuff you said? The active end of each symbol pin should be a different color. You should also have a grid of dots. Verify that each active end is on a dot. It is probably easier to view the netlist. The netlist will show you all of the pin connections. You can then quickly isolate the pins that aren't connected. You may want to break your schematic into small pieces and get each piece working separately. After you get all the pieces working merge them. (* jcl *) -- 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: no pins in JUMPER10
i'm sending my project. it's very simple. Thank you. 2006/11/5, Giorgenes Gelatti <[EMAIL PROTECTED]>: I got it working in the example, but it still doesn't work in my project. :( How can I check for errors, like the "on grid" stuff you said? Thank you. 2006/11/5, Giorgenes Gelatti <[EMAIL PROTECTED]>: > I did what you said and got it working now. > Thank you very much. > I just wonder whether it is a bug or a feature :) > > Tks. > > 2006/11/5, John Luciani <[EMAIL PROTECTED]>: > > On 11/5/06, Giorgenes Gelatti <[EMAIL PROTECTED]> wrote: > > > yes, I did. > > > But it doesn't work for me. > > > I've just realized I'm getting warnings when I load the net list: > > > > > > 2: Warning! net "unnamed_net10" is shorted to net "unnamed_net1" > > > 3: Warning! net "unnamed_net10" is shorted to net "unnamed_net1" > > > 4: Warning! net "unnamed_net9" is shorted to net "unnamed_net5" > > > 5: Warning! net "unnamed_net9" is shorted to net "unnamed_net5" > > > 6: Warning! net "unnamed_net8" is shorted to net "unnamed_net2" > > > 7: Warning! net "unnamed_net8" is shorted to net "unnamed_net2" > > > 8: Warning! net "unnamed_net7" is shorted to net "unnamed_net3" > > > 9: Warning! net "unnamed_net7" is shorted to net "unnamed_net3" > > > 10: Warning! net "unnamed_net6" is shorted to net "unnamed_net4" > > > 11: Warning! net "unnamed_net6" is shorted to net "unnamed_net4" > > > 12: Warning! net "unnamed_net5" is shorted to net "unnamed_net9" > > > 13: Warning! net "unnamed_net4" is shorted to net "unnamed_net6" > > > 14: Warning! net "unnamed_net3" is shorted to net "unnamed_net7" > > > 15: Warning! net "unnamed_net2" is shorted to net "unnamed_net8" > > > 16: Warning! net "unnamed_net1" is shorted to net "unnamed_net10" > > > > I left out a step in my sequence --- > > > > Before pressing "O" I moved the connectors so that they were not > > on top of each other. If I open PCB, load the netlist, and press "O" (without > > moving one of the connectors) I get the same 16 warnings that you do. > > > > The reason you get the warnings is that with one connector on top of the other > > the pins are connecting incorrectly. > > > > Rather than moving all of your footprints you could use the command > > Select -> Disperse all elements. > > > > Sorry about the mixup. After making this mistake (a few times) I now > > instinctively move the components and forgot to mention it. > > > > (* jcl *) > > > > > > -- > > http://www.luciani.org > > > > > > ___ > > geda-user mailing list > > geda-user@moria.seul.org > > http://www.seul.org/cgi-bin/mailman/listinfo/geda-user > > > programmer.sch Description: Binary data ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: no pins in JUMPER10
On 11/5/06, Giorgenes Gelatti <[EMAIL PROTECTED]> wrote: I did what you said and got it working now. Thank you very much. I just wonder whether it is a bug or a feature :) Non-catastrophic infelicity ;-) (* jcl *) --- 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: no pins in JUMPER10
I got it working in the example, but it still doesn't work in my project. :( How can I check for errors, like the "on grid" stuff you said? Thank you. 2006/11/5, Giorgenes Gelatti <[EMAIL PROTECTED]>: I did what you said and got it working now. Thank you very much. I just wonder whether it is a bug or a feature :) Tks. 2006/11/5, John Luciani <[EMAIL PROTECTED]>: > On 11/5/06, Giorgenes Gelatti <[EMAIL PROTECTED]> wrote: > > yes, I did. > > But it doesn't work for me. > > I've just realized I'm getting warnings when I load the net list: > > > > 2: Warning! net "unnamed_net10" is shorted to net "unnamed_net1" > > 3: Warning! net "unnamed_net10" is shorted to net "unnamed_net1" > > 4: Warning! net "unnamed_net9" is shorted to net "unnamed_net5" > > 5: Warning! net "unnamed_net9" is shorted to net "unnamed_net5" > > 6: Warning! net "unnamed_net8" is shorted to net "unnamed_net2" > > 7: Warning! net "unnamed_net8" is shorted to net "unnamed_net2" > > 8: Warning! net "unnamed_net7" is shorted to net "unnamed_net3" > > 9: Warning! net "unnamed_net7" is shorted to net "unnamed_net3" > > 10: Warning! net "unnamed_net6" is shorted to net "unnamed_net4" > > 11: Warning! net "unnamed_net6" is shorted to net "unnamed_net4" > > 12: Warning! net "unnamed_net5" is shorted to net "unnamed_net9" > > 13: Warning! net "unnamed_net4" is shorted to net "unnamed_net6" > > 14: Warning! net "unnamed_net3" is shorted to net "unnamed_net7" > > 15: Warning! net "unnamed_net2" is shorted to net "unnamed_net8" > > 16: Warning! net "unnamed_net1" is shorted to net "unnamed_net10" > > I left out a step in my sequence --- > > Before pressing "O" I moved the connectors so that they were not > on top of each other. If I open PCB, load the netlist, and press "O" (without > moving one of the connectors) I get the same 16 warnings that you do. > > The reason you get the warnings is that with one connector on top of the other > the pins are connecting incorrectly. > > Rather than moving all of your footprints you could use the command > Select -> Disperse all elements. > > Sorry about the mixup. After making this mistake (a few times) I now > instinctively move the components and forgot to mention it. > > (* jcl *) > > > -- > http://www.luciani.org > > > ___ > 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: no pins in JUMPER10
I did what you said and got it working now. Thank you very much. I just wonder whether it is a bug or a feature :) Tks. 2006/11/5, John Luciani <[EMAIL PROTECTED]>: On 11/5/06, Giorgenes Gelatti <[EMAIL PROTECTED]> wrote: > yes, I did. > But it doesn't work for me. > I've just realized I'm getting warnings when I load the net list: > > 2: Warning! net "unnamed_net10" is shorted to net "unnamed_net1" > 3: Warning! net "unnamed_net10" is shorted to net "unnamed_net1" > 4: Warning! net "unnamed_net9" is shorted to net "unnamed_net5" > 5: Warning! net "unnamed_net9" is shorted to net "unnamed_net5" > 6: Warning! net "unnamed_net8" is shorted to net "unnamed_net2" > 7: Warning! net "unnamed_net8" is shorted to net "unnamed_net2" > 8: Warning! net "unnamed_net7" is shorted to net "unnamed_net3" > 9: Warning! net "unnamed_net7" is shorted to net "unnamed_net3" > 10: Warning! net "unnamed_net6" is shorted to net "unnamed_net4" > 11: Warning! net "unnamed_net6" is shorted to net "unnamed_net4" > 12: Warning! net "unnamed_net5" is shorted to net "unnamed_net9" > 13: Warning! net "unnamed_net4" is shorted to net "unnamed_net6" > 14: Warning! net "unnamed_net3" is shorted to net "unnamed_net7" > 15: Warning! net "unnamed_net2" is shorted to net "unnamed_net8" > 16: Warning! net "unnamed_net1" is shorted to net "unnamed_net10" I left out a step in my sequence --- Before pressing "O" I moved the connectors so that they were not on top of each other. If I open PCB, load the netlist, and press "O" (without moving one of the connectors) I get the same 16 warnings that you do. The reason you get the warnings is that with one connector on top of the other the pins are connecting incorrectly. Rather than moving all of your footprints you could use the command Select -> Disperse all elements. Sorry about the mixup. After making this mistake (a few times) I now instinctively move the components and forgot to mention it. (* jcl *) -- http://www.luciani.org ___ 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: no pins in JUMPER10
On 11/5/06, Giorgenes Gelatti <[EMAIL PROTECTED]> wrote: yes, I did. But it doesn't work for me. I've just realized I'm getting warnings when I load the net list: 2: Warning! net "unnamed_net10" is shorted to net "unnamed_net1" 3: Warning! net "unnamed_net10" is shorted to net "unnamed_net1" 4: Warning! net "unnamed_net9" is shorted to net "unnamed_net5" 5: Warning! net "unnamed_net9" is shorted to net "unnamed_net5" 6: Warning! net "unnamed_net8" is shorted to net "unnamed_net2" 7: Warning! net "unnamed_net8" is shorted to net "unnamed_net2" 8: Warning! net "unnamed_net7" is shorted to net "unnamed_net3" 9: Warning! net "unnamed_net7" is shorted to net "unnamed_net3" 10: Warning! net "unnamed_net6" is shorted to net "unnamed_net4" 11: Warning! net "unnamed_net6" is shorted to net "unnamed_net4" 12: Warning! net "unnamed_net5" is shorted to net "unnamed_net9" 13: Warning! net "unnamed_net4" is shorted to net "unnamed_net6" 14: Warning! net "unnamed_net3" is shorted to net "unnamed_net7" 15: Warning! net "unnamed_net2" is shorted to net "unnamed_net8" 16: Warning! net "unnamed_net1" is shorted to net "unnamed_net10" I left out a step in my sequence --- Before pressing "O" I moved the connectors so that they were not on top of each other. If I open PCB, load the netlist, and press "O" (without moving one of the connectors) I get the same 16 warnings that you do. The reason you get the warnings is that with one connector on top of the other the pins are connecting incorrectly. Rather than moving all of your footprints you could use the command Select -> Disperse all elements. Sorry about the mixup. After making this mistake (a few times) I now instinctively move the components and forgot to mention it. (* jcl *) -- 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: no pins in JUMPER10
yes, I did. But it doesn't work for me. I've just realized I'm getting warnings when I load the net list: 2: Warning! net "unnamed_net10" is shorted to net "unnamed_net1" 3: Warning! net "unnamed_net10" is shorted to net "unnamed_net1" 4: Warning! net "unnamed_net9" is shorted to net "unnamed_net5" 5: Warning! net "unnamed_net9" is shorted to net "unnamed_net5" 6: Warning! net "unnamed_net8" is shorted to net "unnamed_net2" 7: Warning! net "unnamed_net8" is shorted to net "unnamed_net2" 8: Warning! net "unnamed_net7" is shorted to net "unnamed_net3" 9: Warning! net "unnamed_net7" is shorted to net "unnamed_net3" 10: Warning! net "unnamed_net6" is shorted to net "unnamed_net4" 11: Warning! net "unnamed_net6" is shorted to net "unnamed_net4" 12: Warning! net "unnamed_net5" is shorted to net "unnamed_net9" 13: Warning! net "unnamed_net4" is shorted to net "unnamed_net6" 14: Warning! net "unnamed_net3" is shorted to net "unnamed_net7" 15: Warning! net "unnamed_net2" is shorted to net "unnamed_net8" 16: Warning! net "unnamed_net1" is shorted to net "unnamed_net10" That may be a hint of the problem. Thank you very much. 2006/11/3, John Luciani <[EMAIL PROTECTED]>: On 11/3/06, Giorgenes Gelatti <[EMAIL PROTECTED]> wrote: > What do you mean "on grid"? gschem has a grid set at 100 gschem-units. For a connection to be made pins have to have the active end on the grid. Your schematic is on grid. Did you load the netlist file prior to running the optimize command? Your schematic, PCB and netlist file look correct and they worked for me. I did the following: 1. File->Load Layout 2. File->Load netlist File 3. Pressed the 'O' key (optimize rats nest). (* jcl *) -- http://www.luciani.org ___ 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: no pins in JUMPER10
On 11/3/06, Giorgenes Gelatti <[EMAIL PROTECTED]> wrote: What do you mean "on grid"? gschem has a grid set at 100 gschem-units. For a connection to be made pins have to have the active end on the grid. Your schematic is on grid. Did you load the netlist file prior to running the optimize command? Your schematic, PCB and netlist file look correct and they worked for me. I did the following: 1. File->Load Layout 2. File->Load netlist File 3. Pressed the 'O' key (optimize rats nest). (* jcl *) -- 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: no pins in JUMPER10
What do you mean "on grid"? I don't get that. I'm sending a very simple example. Exporting it to PCB will get no connections between the connectors. Thank you. 2006/11/3, John Luciani <[EMAIL PROTECTED]>: On 11/3/06, Giorgenes Gelatti <[EMAIL PROTECTED]> wrote: > Hi there, > > I've made an schematic with a "pin bar" that has "JUMPER10" as footprint. > But when I export it to PCB none of the pins on it get connected. > The rest of my circuit is ok, but the "JUMPER10" components goes > disconnected in PCB. > In the schematic are the connection ends of the pin bars on grid? Are the pin numbers consistent between the schematic symbol and the PCB footprint? You may want to post a *small* schematic and pcb file that demonstrates the problem. For the schematic make sure you use embedded symbols. (* jcl *) -- http://www.luciani.org ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user jumper.sch Description: Binary data jump Description: Binary data jmp.pcb Description: Binary data jmp.net Description: Binary data ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: no pins in JUMPER10
On 11/3/06, Giorgenes Gelatti <[EMAIL PROTECTED]> wrote: Hi there, I've made an schematic with a "pin bar" that has "JUMPER10" as footprint. But when I export it to PCB none of the pins on it get connected. The rest of my circuit is ok, but the "JUMPER10" components goes disconnected in PCB. In the schematic are the connection ends of the pin bars on grid? Are the pin numbers consistent between the schematic symbol and the PCB footprint? You may want to post a *small* schematic and pcb file that demonstrates the problem. For the schematic make sure you use embedded symbols. (* jcl *) -- http://www.luciani.org ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
gEDA-user: no pins in JUMPER10
Hi there, I've made an schematic with a "pin bar" that has "JUMPER10" as footprint. But when I export it to PCB none of the pins on it get connected. The rest of my circuit is ok, but the "JUMPER10" components goes disconnected in PCB. Any advice? Thank you guys. []'s ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
