Re: gEDA-user: Request for comments
andrewm wrote: I have same numbered the pins on the switch as they are electrically connected inside. I often use the pins on those switches as jumpers to get wires out of tight spots and thought that giving them the same number would allow the nets to look connected. Steven Michalske wrote: From my experimentation, PCB wants the net connected to both of the pins and will not treat it as a jumper... I find this as a minor bug, would you care to verify and make an example schematic to submit a bug/feature request for us? Steve, Sure I can do a bug/feature request on this (after I read up how too). Just want to make sure that it is something wrong or something people want. Should the two pins same-named be treated as a single entity so they can be used like a jumper or should the connection have to be made manually in the schematic and the pins be named differently. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Request for comments
On Sep 11, 2007, at 2:49 PM, andrewm wrote: Steve, Sure I can do a bug/feature request on this (after I read up how too). Just want to make sure that it is something wrong or something people want. Should the two pins same-named be treated as a single entity so they can be used like a jumper or should the connection have to be made manually in the schematic and the pins be named differently. My feeling is that if pins are numbered the same then they are electrically connected in the part. an example is the 4 mounting pins on a SMA to PCB jack the 4 outer pins are electrically equal, you can attach to any of them they are the same net PCB wanted all 4 pins connected... but electrically only one needs connection. Some discussion could be put into this. do we want sub pins for the net of pins so on a SMA example the center conductor would be pin 1 the 4 mounting pins would be pins 2.1, 2.2, 2.3, 2.4 so if the net specified connect to pin 2 it would make a electrical connection to any of the pins and be done if you specified that it was pin 2.1 it would connect to that sub pin. if you specified 2.* it would require connection on all sub pins. this would provide for the most options in how to handle internally connected pins with the same numbering. thoughts gang? Steve ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Request for comments
Steven Michalske wrote: On Sep 11, 2007, at 2:49 PM, andrewm wrote: Steve, Sure I can do a bug/feature request on this (after I read up how too). Just want to make sure that it is something wrong or something people want. Should the two pins same-named be treated as a single entity so they can be used like a jumper or should the connection have to be made manually in the schematic and the pins be named differently. My feeling is that if pins are numbered the same then they are electrically connected in the part. True. an example is the 4 mounting pins on a SMA to PCB jack the 4 outer pins are electrically equal, you can attach to any of them they are the same net PCB wanted all 4 pins connected... but electrically only one needs connection. Not true. I would never use this type of connector and only connect one ground pin. Add in the parasitic inductance of the pins and then see if they are electrically equal. Some discussion could be put into this. do we want sub pins for the net of pins so on a SMA example the center conductor would be pin 1 the 4 mounting pins would be pins 2.1, 2.2, 2.3, 2.4 I don't see the necessity of this. When I build parts with multiple pins all of which I want connected I give them different numbers. There may be other types of examples where this is needed but I've never hit one. thoughts from Joe T. so if the net specified connect to pin 2 it would make a electrical connection to any of the pins and be done if you specified that it was pin 2.1 it would connect to that sub pin. if you specified 2.* it would require connection on all sub pins. this would provide for the most options in how to handle internally connected pins with the same numbering. thoughts gang? Steve ___ 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: Request for comments
First, this is debate mode not argument mode.. Sorry, bad example At DC they are the same :-P 2GHz not so much.. I want my ground plane! DB9 mounting tabs, that's better, I saw a SMA connector in my head as common enough for people to relate to with out firing up some drawing app :-P On Sep 11, 2007, at 4:26 PM, joeft wrote: PCB wanted all 4 pins connected... but electrically only one needs connection. Not true. I would never use this type of connector and only connect one ground pin. Add in the parasitic inductance of the pins and then see if they are electrically equal. Some discussion could be put into this. do we want sub pins for the net of pins so on a SMA example the center conductor would be pin 1 the 4 mounting pins would be pins 2.1, 2.2, 2.3, 2.4 I don't see the necessity of this. When I build parts with multiple pins all of which I want connected I give them different numbers. There may be other types of examples where this is needed but I've never hit one. The SMA connector, do you have all four pins labeled separately, I wouldn't or would I pins 1,2,3,4,5 ? pin=2.* would define in the symbol to attach all pins to the net Steve ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Request for comments
On Sep 7, 2007, at 9:16 PM, andrewm wrote: I have same numbered the pins on the switch as they are electrically connected inside. I often use the pins on those switches as jumpers to get wires out of tight spots and thought that giving them the same number would allow the nets to look connected. From my experimentation, PCB wants the net connected to both of the pins and will not treat it as a jumper... I find this as a minor bug, would you care to verify and make an example schematic to submit a bug/feature request for us? Steve ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
gEDA-user: Request for comments
Howdy all, I have just uploaded my first footprints I have made to the geda symbols site http://www.gedasymbols.org/user/andrew_mccubbin/ If some of the in crowd can have a look at them and comment if I am doing things the right way. Hopefully before DJ links them to the front page and they escape to the real world. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Request for comments
If some of the in crowd can have a look at them and comment if I am doing things the right way. Hopefully before DJ links them to the front page and they escape to the real world. Too late; the link is automatic :-) ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Request for comments
On Sat, Sep 08, 2007 at 12:04:26PM +1000, andrewm wrote: http://www.gedasymbols.org/user/andrew_mccubbin/ Looking only at CTS-252-switch in detail: PCB will not clip the silkscreen over the copper, and some fabs will go ahead and print it right over the pads. Interesting quirk I see with PCB is that you have some same-numbered, overlapping pad/pins and they are in the same net (via 'find') but your same-numbered non-overlapping pins are not. I'm not sure how that would play out in a real layout. Your soldermask clearance is about 1.5mil. That's smaller than the printing tolerances of most fabs. On the other hand, if you grow all the soldermasks to some minimum after layout, starting small is fine. -- Ben Jackson AD7GD [EMAIL PROTECTED] 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: Request for comments
Your soldermask clearance is about 1.5mil. That's smaller than the printing tolerances of most fabs. Hmm, it's exactly the tolerance of the fabs I use. But pcb also has a MinMaskGap() action specifically designed to grow masks to meet fab tolerances :-) ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Request for comments
andrewm [EMAIL PROTECTED] writes: If some of the in crowd can have a look at them and comment if I am doing things the right way. DJ Delorie wrote: Quick note: you shouldn't draw silk over pins or pads. Some fab houses won't remove it, resulting in ink on top of your exposed copper. Ah - OK - didn't realise not all fabs removed the silkscreen over pads. Will fix that up. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Request for comments
Ben Jackson wrote: Looking only at CTS-252-switch in detail: PCB will not clip the silkscreen over the copper, and some fabs will go ahead and print it right over the pads. Interesting quirk I see with PCB is that you have some same-numbered, overlapping pad/pins and they are in the same net (via 'find') but your same-numbered non-overlapping pins are not. I'm not sure how that would play out in a real layout. Your soldermask clearance is about 1.5mil. That's smaller than the printing tolerances of most fabs. On the other hand, if you grow all the soldermasks to some minimum after layout, starting small is fine. Thanks for comment. I did the 1.5mil clearance as that was the smallest of the common fabs I looked at on the internet and some of them said they automatically increase solder mask clearances if smaller than they recomended. I have same numbered the pins on the switch as they are electrically connected inside. I often use the pins on those switches as jumpers to get wires out of tight spots and thought that giving them the same number would allow the nets to look connected. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
