gEDA-user: Hello, Bills missing transistors and Attribute questions
Hi Everyone Thanks so much for looking! My names Mark and I am from Malaysia. Im a newbie and recent convert to the world of gEDA and have been really struggling trying to understand it all! I must have put in about 2 solid weeks of reading most of the gschem documentation. Slowly slowly I am figuring it out! I think one of the big problems is more that I am from a mechanical background and have little to non experience with EDA. Having said that, I really like the interface of gschem and hope to be able to get to use it well! Anyhows I am writing in to you all with the hope that some kind souls could help with a few things... The first thing is that when one looks thru Bill Wilson's really helpful gsch2pcb_Tutorial, there is a link to a library of transistor symbols and elements that Bill created. The URL is in the Custom File Elements section of the document: http://www.geda.seul.org/docs/current/tutorials/gsch2pcb/gsch2pcb-libs-20040110.tar.gz Unfortunately it leads to an object not found page. Would anyone have a copy of this library? This library is of particular interest to me as Bill discusses the problems of correlating all the various TO92 pin outs in gschem with PCB. My next question is about the Symbol Attributes. Lets say I wish to make a symbol for a BC550 transistor. As I would be using this particular device a lot, I would like to make this symbol as correctly as I can. So, if I have a BC550 NPN GENERAL PURPOSE TRANSISTOR, what are the preferred values to give: Device=? Description=? My guess is that: Device=NPN TRANSISTOR Description= BC550 NPN GENERAL PURPOSE TRANSISTOR Would this be correct or would you suggest some other values? My next problem is with the pins. I think what is most important is that the pin numbers of the symbol pins match the physical pin numbers of the particular transistor when placed inside the PCB. Difficult with TO92 as there are lots of em ;) As you know... these small package transistors have specific manufacturer numbered legs. In the case of my BC550, I have a Leg #1 (Collector), Leg #2 (Base) and Leg #3(Emitter). Does it matter say if pinseq=1 is where transistor Leg #2 goes? Can we attach any Leg # to any pinseq#? On the subject of pinnumber, what would a better approach be? Should I use values of 1, 2 and 3? Or would it be smarter to use values of E, B and C for my transistor symbol? On the subject of pintype for transistors, what should I be using? pas? I am uncertain how open collector and emmiter fit into the picture here. As I might wish to one day run spice... I would really appreciate some info on what values I should be setting for the E, B C legs on my transistors. For pinlabel, would it be correct to say that I do not need to include this attribute unless I am connecting a particular transistor leg to another schematic somewhere else? Or do I need to include this attribute. If so.. what would I label them for the E, B C legs on my transistors? Well guys... thank so much for your time going thru this. Really appreciate it! Regards Mark Be a better friend, newshound, and know-it-all with Yahoo! Mobile. Try it now. http://mobile.yahoo.com/;_ylt=Ahu06i62sR8HDtDypao8Wcj9tAcJ ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Hello, Bills missing transistors and Attribute questions
On Sun, 2008-03-30 at 04:01 -0700, Mark wrote: My names Mark and I am from Malaysia. Im a newbie and recent convert to the world of gEDA and have been really struggling trying to understand it all! Hello, and welcome... The first thing is that when one looks thru Bill Wilson's really helpful gsch2pcb_Tutorial, there is a link to a library of transistor symbols and elements that Bill created. The URL is in the Custom File Elements section of the document: http://www.geda.seul.org/docs/current/tutorials/gsch2pcb/gsch2pcb-libs-20040110.tar.gz Unfortunately it leads to an object not found page. Would anyone have a copy of this library? I don't unfortunately, perhaps someone else will be able to help though. So, if I have a BC550 NPN GENERAL PURPOSE TRANSISTOR, what are the preferred values to give: Device=? Description=? My guess is that: Device=NPN TRANSISTOR Description= BC550 NPN GENERAL PURPOSE TRANSISTOR Would this be correct or would you suggest some other values? Those sounds good to me. As a general rule though, these are for your benefit. This said, SPICE or gnucap backends may attach meaning to the Device= attribute. In the existing symbols, see mostly: device=NPN_TRANSISTOR There is also device=SPICE-NPN (Note its device not Device, similarly description). Also might be of interest, is the attribute: documentation= If you set the attribute to a URL, then you can access that URL in a web-browser from the menu Hierarchy-Documentation when you have a pacticular component selected. My next problem is with the pins. I think what is most important is that the pin numbers of the symbol pins match the physical pin numbers of the particular transistor when placed inside the PCB. Difficult with TO92 as there are lots of em ;) Yes, a common problem. Also, rather surprisingly I can't find a TO92 package in PCB. My suggestion would be (if you're targeting PCB for board design), to find the right footprint in PCB and match your pinnumbers in your specific symbol. Al Davis or Start Brorson may be able to answer more about the requirements for using gnucap or some SPICE variant to simulate your design. You might take a look at: http://www.brorson.com/gEDA/ http://www.brorson.com/gEDA/SPICE/ As you know... these small package transistors have specific manufacturer numbered legs. In the case of my BC550, I have a Leg #1 (Collector), Leg #2 (Base) and Leg #3(Emitter). Does it matter say if pinseq=1 is where transistor Leg #2 goes? Can we attach any Leg # to any pinseq#? pinseq defines the output ordering for the spice backend. (And allows us to reference specific pins which might have different pinnumbers when using slotted components (e.g. one opamp symbol for all opamps in a chip with 2 or 4 inside). For SPICE, the order you _need_ pinseq incrementing is: collector (pinseq=1), base (pinseq=2) , emitter (pinseq=3). If you were modelling a transistor in an IC design, you could also hook up to the silicon substrate of the transistor with pinseq=4. On the subject of pinnumber, what would a better approach be? Should I use values of 1, 2 and 3? Or would it be smarter to use values of E, B and C for my transistor symbol? You can do either, so long as the pin names in PCB match the pinnumber in gschem. pinnumber also works with letters - it just means that you'd be making specific PCB footprints for all the TO92 pinout variants you want to use. On the subject of pintype for transistors, what should I be using? pas? I am uncertain how open collector and emmiter fit into the picture here. As I might wish to one day run spice... I would really appreciate some info on what values I should be setting for the E, B C legs on my transistors. pas sounds good to me, but its probably not generally appropriate. Those values are only used by the design rule checker, and appear to be much more geared to digital logic - where there are clear power, input, output pins etc.. The purpose would be to check (for example) there aren't two outputs connected together, or inputs which aren't driven. For pinlabel, would it be correct to say that I do not need to include this attribute unless I am connecting a particular transistor leg to another schematic somewhere else? Or do I need to include this attribute. If so.. what would I label them for the E, B C legs on my transistors? I'd add it if it improves clarity. I generally use them to show the signal names of signals on more complex chips. Eg. IRQ D0 A12, etc.. Well guys... thank so much for your time going thru this. Really appreciate it! No problem, we hope you enjoy using gEDA - any further queries, just ask here. Best wishes, -- Peter Clifton Electrical Engineering Division, Engineering Department, University of Cambridge, 9, JJ Thomson Avenue, Cambridge CB3 0FA Tel: +44 (0)7729 980173 - (No signal in the lab!) ___ geda-user mailing list
Re: gEDA-user: Hello, Bills missing transistors and Attribute questions
On Sun, 30 Mar 2008 12:57:56 +0100, Peter Clifton wrote: On the subject of pinnumber, what would a better approach be? Should I use values of 1, 2 and 3? Or would it be smarter to use values of E, B and C for my transistor symbol? You can do either, so long as the pin names in PCB match the pinnumber in gschem. pinnumber also works with letters - it just means that you'd be making specific PCB footprints for all the TO92 pinout variants you want to use. You might want to take a look at my TO92 footprints in gedasymbols.org They were made to fit FETs (TO92_GDS.fp) or ordinary transistors: http://www.gedasymbols.org/user/kai_martin_knaak/footprints/generic/TO92_ECB.fp http://www.gedasymbols.org/user/kai_martin_knaak/footprints/generic/TO92_GDS.fp I just included these footprints in my current project. Bit they have not yet been produced in an actual pcb. So you should double check for errors. ---(kaimartin)--- PS: Leventes TO92 footprint looks like TO18 to me http://www.gedasymbols.org/user/levente_kovacs/footprints/TO92.fp -- Kai-Martin Knaak http://lilalaser.de/blog ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Hello, Bills missing transistors and Attribute questions
On Sun, 30 Mar 2008 23:49:38 +0100, Peter Clifton wrote: Bug report: The graphic for the GDS variant still shows ECB against it. Just did a cvs commit for a fix. ---(kaimartin)--- -- Kai-Martin Knaak http://lilalaser.de/blog ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
