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
gEDA-user: gschem: How to overwrite invisible attributes?
Hello, there exists symbols with net attributes which are not visible/accessible when symbol is inserted in a schematic, for example net=Vcc:14 Problem: I am using many different positive supply voltages, i.e. 5V and 3.3V. I want that this symbol has 3.3V supply, but I have no Vcc defined (or maybe Vcc is defined to be +5V). Can I simple add a new attribute to the symbol to overwrite the invisible/hidden net=Vcc:14 for pin 14 with something like net= +3.3V:14 ? I think that I have read that this overwriting of attributes shall work -- but I can't find it again. Best regards Stefan Salewski ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: gschem: How to overwrite invisible attributes?
On Sun, Mar 30, 2008 at 2:41 PM, Stefan Salewski [EMAIL PROTECTED] wrote: Hello, there exists symbols with net attributes which are not visible/accessible when symbol is inserted in a schematic, for example net=Vcc:14 Problem: I am using many different positive supply voltages, i.e. 5V and 3.3V. I want that this symbol has 3.3V supply, but I have no Vcc defined (or maybe Vcc is defined to be +5V). Can I simple add a new attribute to the symbol to overwrite the invisible/hidden net=Vcc:14 for pin 14 with something like net= +3.3V:14 ? I think that I have read that this overwriting of attributes shall work -- but I can't find it again. Why not just remove the hidden nets from the symbols? With mulitple values of Vcc (or GND) the hidden nets create a lot of hidden problems. (* jcl *) P.S. I have a script that removes the hidden nets and generates appropriate power symbols. -- 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: gschem: How to overwrite invisible attributes?
Why not just remove the hidden nets from the symbols? With mulitple values of Vcc (or GND) the hidden nets create a lot of hidden problems. Indeed, for symbols created by myself I do not use net attributes for power supply. I prefer to use visible power pins or to divide larger symbols into one separate power symbol. But there are some existing gschem-symbols with these net-attributes... OK, maybe I should make a local copy and remove the hidden nets. Best regards Stefan Salewski ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Asking questions, obtaining answers ...
The idea is twofold: 1. Create a web-based support bulletin board. This would be a lot like the e-mail list, except that you wouldn't need to subscribe or read your e-mail. 2. Put a link into each program's help menu item which would open a browser up on the support bulletin board page. My thought: In principle, a great idea. Indeed, lots of commercial software products include stuff like this. For us, however, it may represent a lot of maintainence work. We're a small project with a finite number of developers whose time is already streched between family, work, other activities, and gEDA. However, maintaining a BBS means administering the box or finding hosting. Next, somebody must diligently watch the BBS and remove spam, flames, and off-topic junk. Oh, and answer questions too. Hm I'm sorry that sounds so negative. Is there a way to make the support site self-service, like the wiki? After all, we already link to the wiki from within gschem. Stuart On Sun, 30 Mar 2008, Peter Clifton wrote: Hi guys, I just came across this blog post from an Inkscape developer: http://bryceharrington.org/drupal/inkscape-answers ??Bryce is also a Canonical employee, so there may be some Launchpad bias, but I think the idea is neat. We could similarly provide a more direct link to human help from gschem and other gEDA tools, from the help menu. I realise we currently have links to the wiki / FAQ, but feel there is a high barrier to entry for a new user to sign up to a mailing list for an answer to what might be a simple question, even if they can't find the answer in the FAQ. I'm very keen that we should encourage new users to join the gEDA community, and think this may be a good way to get them thinking more about gEDA as something they aren't alone in using. Any thoughts? -- 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 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: 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: Asking questions, obtaining answers ...
At the risk of being accused a Canonical / Launchpad fan-boy, if this were an idea we wanted to implement, I'd take a fair bit of convincing that we didn't just want to use Launchpad answers... On Sun, 2008-03-30 at 17:55 -0400, Stuart Brorson wrote: The idea is twofold: 1. Create a web-based support bulletin board. This would be a lot like the e-mail list, except that you wouldn't need to subscribe or read your e-mail. Launchpad answers does require a launchpad account, and reading your email is a good way to know the question has had a response. Ok, there is still some barrier to entry. 2. Put a link into each program's help menu item which would open a browser up on the support bulletin board page. Thats the basic idea. My thought: In principle, a great idea. Indeed, lots of commercial software products include stuff like this. For us, however, it may represent a lot of maintainence work. We're a small project with a finite number of developers whose time is already streched between family, work, other activities, and gEDA. However, maintaining a BBS means administering the box or finding hosting. Next, somebody must diligently watch the BBS and remove spam, flames, and off-topic junk. Oh, and answer questions too. Using an existing service does take away the pain of writing / maintaining the web-app code. Hm I'm sorry that sounds so negative. Is there a way to make the support site self-service, like the wiki? After all, we already link to the wiki from within gschem. For many projects I've come across, there are good users out there who will monitor the the answers pages and help those in need of help. If it worked, the community has a good opportunity to grow around this. If not, it would be at least some of the pain you describe. The primary concern I had that if it were to turn out the idea doesn't work, we've deployed n copies of gEDA irrevocably with a given web-address in it. We could, I guess, use a re-direct page on one of our servers, so if the idea didn't fly we could replace the page with Sorry, answers facility closed, please see the geda-user mailing list. The web-access logs a redirect page may provide interesting statistics on the size of our user-base (without needing to make gEDA evil and phone home). We can probably bet many users will click the menu item even if they don't end up asking a question. -- 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 geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Asking questions, obtaining answers ...
At the risk of being accused a Canonical / Launchpad fan-boy, if this were an idea we wanted to implement, I'd take a fair bit of convincing that we didn't just want to use Launchpad answers... H. OK, I just looked into Launchpad. Looks intriguing. For many projects I've come across, there are good users out there who will monitor the the answers pages and help those in need of help. Folks already do that on the e-mail list. Therefore, folks will also do it on Launchpad. I agree. If it worked, the community has a good opportunity to grow around this. I like it.. I'll continue reading up on Launch pad. You may be convincing me. Stuart ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Asking questions, obtaining answers ...
FWIW, somebody already signed gEDA up for a Launchpad acct: https://launchpad.net/geda Therefore, it's probably a simple matter of activating the answers: thingie and embedding a link into each app. Stuart On Sun, 30 Mar 2008, Peter Clifton wrote: At the risk of being accused a Canonical / Launchpad fan-boy, if this were an idea we wanted to implement, I'd take a fair bit of convincing that we didn't just want to use Launchpad answers... On Sun, 2008-03-30 at 17:55 -0400, Stuart Brorson wrote: The idea is twofold: 1. Create a web-based support bulletin board. This would be a lot like the e-mail list, except that you wouldn't need to subscribe or read your e-mail. Launchpad answers does require a launchpad account, and reading your email is a good way to know the question has had a response. Ok, there is still some barrier to entry. 2. Put a link into each program's help menu item which would open a browser up on the support bulletin board page. Thats the basic idea. My thought: In principle, a great idea. Indeed, lots of commercial software products include stuff like this. For us, however, it may represent a lot of maintainence work. We're a small project with a finite number of developers whose time is already streched between family, work, other activities, and gEDA. However, maintaining a BBS means administering the box or finding hosting. Next, somebody must diligently watch the BBS and remove spam, flames, and off-topic junk. Oh, and answer questions too. Using an existing service does take away the pain of writing / maintaining the web-app code. Hm I'm sorry that sounds so negative. Is there a way to make the support site self-service, like the wiki? After all, we already link to the wiki from within gschem. For many projects I've come across, there are good users out there who will monitor the the answers pages and help those in need of help. If it worked, the community has a good opportunity to grow around this. If not, it would be at least some of the pain you describe. The primary concern I had that if it were to turn out the idea doesn't work, we've deployed n copies of gEDA irrevocably with a given web-address in it. We could, I guess, use a re-direct page on one of our servers, so if the idea didn't fly we could replace the page with Sorry, answers facility closed, please see the geda-user mailing list. The web-access logs a redirect page may provide interesting statistics on the size of our user-base (without needing to make gEDA evil and phone home). We can probably bet many users will click the menu item even if they don't end up asking a question. -- 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 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: Asking questions, obtaining answers ...
On Sun, 30 Mar 2008 17:55:46 -0400, Stuart Brorson wrote: For us, however, it may represent a lot of maintainence work. We're a small project with a finite number of developers whose time is already streched between family, work, other activities, and gEDA. The idea is to expand the community and broaden the pool of potential aides. The project might profit from more users like me -- I wouldn't call myself a developer, but gladly answer usage questions on the mailing list... However,maintaining a BBS means administering the box or finding hosting. I could install a message board on one of my webspaces. Shared hosting has become pretty cheap these days. However, I don't like a separate www forum for users, if only because of all the maintenance issues you mentioned. How about a slight modification of the idea: Put a link to a web based email form in the help menu. The email address would be hard wired to the user mailing list. No changes to the existing infra structure. ---(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
Re: gEDA-user: Asking questions, obtaining answers ...
On Sun, 2008-03-30 at 18:54 -0400, Stuart Brorson wrote: FWIW, somebody already signed gEDA up for a Launchpad acct: Peter B and I keep it up to date. It was originally registered by one of the gEDA users, but we (the gEDA developers) staged a coup. The reason we cared, was that Launchpad provides a very neat mechanism for translators to work in a less technical manner, allowing wider contribution. One of my TODO tasks is to merge and resolve any conflicts from the changed translations in Launchpad and git. We have already gained some support for Turkish, IIRC. Therefore, it's probably a simple matter of activating the answers: thingie and embedding a link into each app. Yep.. just wanted to get a feel for whether people liked the idea or not - both users and developers. -- 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 geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Asking questions, obtaining answers ...
On Sun, 2008-03-30 at 22:56 +, Kai-Martin Knaak wrote: On Sun, 30 Mar 2008 17:55:46 -0400, Stuart Brorson wrote: How about a slight modification of the idea: Put a link to a web based email form in the help menu. The email address would be hard wired to the user mailing list. No changes to the existing infra structure. Does the right thing happen the first time a user emails that address without being signed up to the mailing list? (Having signed up before my first posting, I don't know the answer myself). The main benefit of an answers database type system, is that users can see existing questions before asking. If they are new signups to the email list, they WILL ask the same questions over and over. Try this: https://answers.launchpad.net/inkscape/+addquestion Type in the box, Bitmap output antialiasing settings (as an example I've tested). User will see their question may already have been answered - before they are allowed to proceed asking a new one. The searches for existing answers work without a launchpad account, but you can't use the: URL: https://answers.launchpad.net/inkscape/+addquestion Try: https://answers.launchpad.net/inkscape/] 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 geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Asking questions, obtaining answers ...
FWIW, somebody already signed gEDA up for a Launchpad acct: Peter B and I keep it up to date. It was originally registered by one of the gEDA users, but we (the gEDA developers) staged a coup. The reason we cared, was that Launchpad provides a very neat mechanism for translators to work in a less technical manner, allowing wider contribution. I just signed up as a developer Peter B approved me. Thanks! Therefore, it's probably a simple matter of activating the answers: thingie and embedding a link into each app. Yep.. just wanted to get a feel for whether people liked the idea or not - both users and developers. I think it's a great idea! To me, it seems much more newbie friendly than the e-mail list. Kinda like Ubuntu vs. my old SuSE box. Welcome to the new face of Linux... Stuart ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Asking questions, obtaining answers ...
On Sun, 2008-03-30 at 19:31 -0400, Stuart Brorson wrote: FWIW, somebody already signed gEDA up for a Launchpad acct: Peter B and I keep it up to date. It was originally registered by one of the gEDA users, but we (the gEDA developers) staged a coup. The reason we cared, was that Launchpad provides a very neat mechanism for translators to work in a less technical manner, allowing wider contribution. I just signed up as a developer Peter B approved me. Thanks! Therefore, it's probably a simple matter of activating the answers: thingie and embedding a link into each app. Yep.. just wanted to get a feel for whether people liked the idea or not - both users and developers. I think it's a great idea! To me, it seems much more newbie friendly than the e-mail list. Kinda like Ubuntu vs. my old SuSE box. Welcome to the new face of Linux... In the spirit of SPAM, I've just signed up the gEDA administrators group to be an answer contact - so we get emailed if anyone asks a question. If people in this group don't like that idea, or the traffic grows too much, we can perhaps probably create another group for geda-questions or similar. NB.. AFAIK the answers app doesn't need switching on.. just no one has used it yet. I'll keep any eye myself, as its not good for our image if people do use it and questions go unanswered. 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 geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
gEDA-user: Silk text disappears when making a component
Hello all, I have a component, and wanted to add a warning text to the silkscreen layer. I broke the component down, added the text and copied everything to the buffer. All well till now. I can even past it back to the board. But when I press 'Convert buffer into element', the text disappears. What am I doing wrong here? PCB version is 20080202, GTK GUI. John ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Silk text disappears when making a component
But when I press 'Convert buffer into element', the text disappears. What am I doing wrong here? Elements don't have a way of storing additional silkscreen text, sorry. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Asking questions, obtaining answers ...
On Mon, 31 Mar 2008 00:31:07 +0100, Peter Clifton wrote: How about a slight modification of the idea: Put a link to a web based email form in the help menu. The email address would be hard wired to the user mailing list. No changes to the existing infra structure. Does the right thing happen the first time a user emails that address without being signed up to the mailing list? (Having signed up before my first posting, I don't know the answer myself). You get an email to confirm, that your email is valid. IMHO, this is the right thing. The main benefit of an answers database type system, is that users can see existing questions before asking. This already works with the current set-up. Type geda launchpad in a google window ;-) I'll admit that the launchpad solution is much more organized. If they are new signups to the email list, they WILL ask the same questions over and over. Well, isn't this the reason there are two mailing lists user- and developer- ? They just happen to look the same because there are not so many non developer users registered to the list. Try this: https://answers.launchpad.net/inkscape/+addquestion I get To continue, you must log in to Launchpad. plus a registration form. After giving away my email address to yet another potential source of spam I can type my question. Looks sleek :-) My main concern is, that somebody will have to watch the launchpad thingy and answer all the newbie questions. Until there is a user base comparable with inkscape, this has to be done by developers and long time users. Is it realistic to do this kind of service in addition to the mailing lists, the wiki and the official manuals? ---(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
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
Re: gEDA-user: Asking questions, obtaining answers ...
My main concern is, that somebody will have to watch the launchpad thingy and answer all the newbie questions. Until there is a user base comparable with inkscape, this has to be done by developers and long time users. Is it realistic to do this kind of service in addition to the mailing lists, the wiki and the official manuals? [] I guess if my goal were to be achieved through the use of Answers, allowing more users to make first contact, then yes - there could be more work involved. If it were to become too much work, the stock response could resort to being ask on the geda-user mailing list. Actually, I'll probably just do a cut and paste job from the wiki for most questions on launchpad. I can also provide a link to the appropriate answer on the wiki. IMO, it's not a hassle at all. On the contrary -- it lowers the barrier to getting newbie questions answered, which is good for everybody. Thanks, Peter, for getting this set up! Stuart ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
gEDA-user: trailing -
After I edit a file with pcb and save, I get a backup with a - (dash) added to the name. Is this deliberate? Wouldn't a ~ (tilde) be more appropriate? ---(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
Re: gEDA-user: Silk text disappears when making a component
On Sun, 30 Mar 2008 20:30:58 -0400 DJ Delorie [EMAIL PROTECTED] wrote: Elements don't have a way of storing additional silkscreen text, sorry. Thanks for the fast reply, DJ. I have a footprint for RJ45, but it can be used for connector with top or bottom contacts. I wanted to make two footprints each with an appropiate text, as I probably won't remember after making a board. I'll put the text on the board manually. Cheers John ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Silk text disappears when making a component
Elements do have silkscreen, though. I suppose you could use that to mark the top of the element with something. PCB could, in theory, explode any silk text into individual elementlines. Ugly but possible, with some coding. Or we could have someone add ElementText() to the file format ;-) ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
