Re: gEDA-user: gschem vs. PCB diode pin numbering
On Sat, Aug 27, 2011 at 08:37:59PM -0600, John Doty wrote: On Aug 27, 2011, at 8:12 PM, Dan McMahill wrote: This problem goes beyond diodes and transistors. For example, the old 10H series of ECL parts came both in DIP packages as well as PLCC packages. Some of the parts though, would be in a 16 pin DIP or a 20 pin PLCC and so the pin numbers didn't agree between the two packages. Yep. I recently got bit by this with the LT1078 opamp (different pinouts in DIP8 and SO8). I've used the LT1013 (since 1993 or so) which has the same feature. Linear Technology originally (early 90s) claimed that this was because they had to rotate the die when fitting it into the SO8 package. I distincly remember having to create a special symbol under OrCAD to have the right pinout for this device. Gabriel ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: gschem vs. PCB diode pin numbering
On Fri, 26 Aug 2011 11:34:04 +0200 Kovacs Levente leventel...@gmail.com wrote: When you use a light symbol, a script finds a pinmap, and constructs a heavy symbol. Say for example if you have a SOT23 diode with A1A2K pinout you'll get a symbol with name like 'diode-SOT23-A1A2K.sym' this symbol is then copied to the project's symbol directory, and the original symbol name in the schematic is replaced by the name of the newly created symbol. The script will add other information as well like footprint name, etc. With this, you don't have to mess with your symbols nor with your footprints, and everything works quite well for me. Of course, everything is makefile driven... etc. The pinmap and symbol names are coming from a database. Nice! That sounds very slick. Have you shared your code for this pin-mapping tool? Regards, Colin ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: gschem vs. PCB diode pin numbering
On Mon, 29 Aug 2011 10:28:11 -0700 Colin D Bennett co...@gibibit.com wrote: Nice! That sounds very slick. Have you shared your code for this pin-mapping tool? What I do is I share my git repositories... http://git.logonex.eu/?p=utils4geda.git;a=tree;f=scripts4geda;h=e2d27439fbed3df645cfc65248ef690dd32956f4;hb=HEAD The magic is done by light2heavy.pl and gen_heavy_sym.pl, but you need other scripts as well. You should look at dbsym_update.pl as well, which calls other scripts. You can examine my makefile system too. http://git.logonex.eu/?p=utils4geda.git;a=tree;f=pskel;h=4acca5f5b50d8943656cbd9a4faf46726a0e804f;hb=ce4516e8a351b54818abfaacb215d7864b6d1b43 Makefile.sch is the one for schematics. Levente -- Levente Kovacs http://levente.logonex.eu ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: gschem vs. PCB diode pin numbering
On Mon, 29 Aug 2011 22:28:22 +0200 Levente Kovacs leventel...@gmail.com wrote: On Mon, 29 Aug 2011 10:28:11 -0700 Colin D Bennett co...@gibibit.com wrote: Nice! That sounds very slick. Have you shared your code for this pin-mapping tool? What I do is I share my git repositories... http://git.logonex.eu/?p=utils4geda.git;a=tree;f=scripts4geda;h=e2d27439fbed3df645cfc65248ef690dd32956f4;hb=HEAD The magic is done by light2heavy.pl and gen_heavy_sym.pl, but you need other scripts as well. You should look at dbsym_update.pl as well, which calls other scripts. You can examine my makefile system too. http://git.logonex.eu/?p=utils4geda.git;a=tree;f=pskel;h=4acca5f5b50d8943656cbd9a4faf46726a0e804f;hb=ce4516e8a351b54818abfaacb215d7864b6d1b43 Makefile.sch is the one for schematics. Bfff... this was an old commit... this one is head. http://git.logonex.eu/?p=utils4geda.git;a=tree;f=pskel;h=e4a14b5b812f2b235f875a959ad3967cdb4bb471;hb=b8920019ddd79ce76d9644689fe847be9332bfa9 Levente -- Levente Kovacs http://levente.logonex.eu ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: gschem vs. PCB diode pin numbering
On 08/27/2011 10:37 PM, John Doty wrote: On Aug 27, 2011, at 8:12 PM, Dan McMahill wrote: This problem goes beyond diodes and transistors. For example, the old 10H series of ECL parts came both in DIP packages as well as PLCC packages. Some of the parts though, would be in a 16 pin DIP or a 20 pin PLCC and so the pin numbers didn't agree between the two packages. Yep. I recently got bit by this with the LT1078 opamp (different pinouts in DIP8 and SO8). You could (ab)use the slotting functionality to account for different packages - just remember which package goes with which slot number. I'm guessing (though I haven't checked) that slots must be assigned a number, and not a string. If it were a string, that would make it quite a bit more versatile for this usage. -Ethan ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: gschem vs. PCB diode pin numbering
On 8/23/2011 8:47 PM, Matthew Lewis wrote: I was double checking a pcb layout today and I discovered a rather nasty gotcha. It seems that gschem and PCB don't agree on which end of a diode should be pin 1. Gschem views pin 1 as the anode and PCB considers pin 1 to be the cathode. It doesn't prevent you from laying out a board correctly, but it does cause the silkscreen polarity to be printed backwards (for the SOD devices at least). It gets worse that this. The basic problem with a generic symbol like a diode or a transistor is that physically it may come in many different packages. So on one package, the cathode may be pin 1 and on a different package the cathode may be pin 2. But wait, it gets worse... Some packages, SOT-23 for example, sometimes have their physical pins numbered differently by different vendors. This problem goes beyond diodes and transistors. For example, the old 10H series of ECL parts came both in DIP packages as well as PLCC packages. Some of the parts though, would be in a 16 pin DIP or a 20 pin PLCC and so the pin numbers didn't agree between the two packages. There are multiple ways to solve this problem but the approach I use (on the rare occasion that I actually have time to do something like this) is I created a transistor symbol which is really just a template. The pins are numbered @b@, @c@, and @e@. Then I have an ASCII file that has a line for each complete vendor part number. By complete I mean the part number including package codes. On this line in the ASCII file, I call out the template name, the footprint name, and the mapping from symbol pin to package pin. Then I have a smallish awk program which creates all the different symbols with the footprints filled in and the pin outs are all correct. In my schematic, I don't instantiate an NPN, I instantiate a MMBT3904L or instead of just a MAX882, I'd use MAX882CPA (DIP8) or MAX882CSA (SO8). This has solved this issue for me. I've also noticed that gschem searches the older m4 library first ahead of the new pcblib. Is there a way to get PCB to use the newlib first? The reason I ask is because I swapped the pins on the diodes to match gschem in the newlib, but the change had no effect since the older m4 lib is being used when you import a schematic. You have to go back and manually replace the footprints if you want newlib. FWIW, the m4 generated library that ships with pcb has more and often times better footprints than the newlib one which ships with pcb. For example all of the surface mount resistors and capacitors and quite a number of surface mount IC packages. -Dan ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: gschem vs. PCB diode pin numbering
On Aug 27, 2011, at 8:12 PM, Dan McMahill wrote: This problem goes beyond diodes and transistors. For example, the old 10H series of ECL parts came both in DIP packages as well as PLCC packages. Some of the parts though, would be in a 16 pin DIP or a 20 pin PLCC and so the pin numbers didn't agree between the two packages. Yep. I recently got bit by this with the LT1078 opamp (different pinouts in DIP8 and SO8). John Doty Noqsi Aerospace, Ltd. http://www.noqsi.com/ j...@noqsi.com ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: gschem vs. PCB diode pin numbering
On Thu, 25 Aug 2011 14:21:26 -0700 Colin D Bennett co...@gibibit.com wrote: Do you really want to delete and re-add each of your dozens of transistors in gschem when you change the transistor to one with a different pinout? If you use a logically-pinned symbol, you can easily change the pinout by just editing the footprint attributes (gattrib, gschem property editor, export/import to/from spreadsheet, etc.). I don't want it. Conversation regarding TO-92 transistor package pinouts: http://thread.gmane.org/gmane.comp.cad.geda.user/37190/focus=37197 Well, I always say I won't get into the logical/physical pinning debate, but I always do. :-) For me, using logical pins on the schematic symbols such as transistors and diodes (*especially* diodes in IC packages like SOT-23) is the only way that makes sense ... at least until proper pin mapping is implemented. Let me go into details. My work flow is as follows. There are two libraries. One with heavy, another with light symbols. If you use heavy symbols, there's nothing to say. Everything is static. When you use a light symbol, a script finds a pinmap, and constructs a heavy symbol. Say for example if you have a SOT23 diode with A1A2K pinout you'll get a symbol with name like 'diode-SOT23-A1A2K.sym' this symbol is then copied to the project's symbol directory, and the original symbol name in the schematic is replaced by the name of the newly created symbol. The script will add other information as well like footprint name, etc. With this, you don't have to mess with your symbols nor with your footprints, and everything works quite well for me. Of course, everything is makefile driven... etc. The pinmap and symbol names are coming from a database. Levente -- Kovacs Levente leventel...@gmail.com Voice: +36705071002 ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: gschem vs. PCB diode pin numbering
On Wed, 24 Aug 2011 08:21:17 -0400 Ethan Swint eswint.r...@verizon.net wrote: I've defined my own symbols and footprints to use 'A' and 'K' instead of 1 and 2. I don't think it's a good idea. Instead, I use my own library, where pin numbers are consistent. In addition I have my perl scripts which can add pin numbers to symbols according to pinmap files. Levente -- Kovacs Levente leventel...@gmail.com Voice: +36705071002 ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: gschem vs. PCB diode pin numbering - anode/cathode definition
On 08/24/2011 01:15 PM, Colin D Bennett wrote: On Wed, 24 Aug 2011 08:21:17 -0400 Ethan Swinteswint.r...@verizon.net wrote: On 08/23/2011 08:47 PM, Matthew Lewis wrote: I was double checking a pcb layout today and I discovered a rather nasty gotcha. It seems that gschem and PCB don't agree on which end of a diode should be pin 1. Gschem views pin 1 as the anode and PCB considers pin 1 to be the cathode. It doesn't prevent you from laying out a board correctly, but it does cause the silkscreen polarity to be printed backwards (for the SOD devices at least). I've defined my own symbols and footprints to use 'A' and 'K' instead of 1 and 2. That's a good idea. Anything you can do to error-proof yourself is a Good Thing. However, I refuse to use “anode” and “cathode” for diode symbols, since these terms refer to electron flow and are _incorrect_ when the diode is reverse-biased (most obvious for common Zener diode circuits). I understand that it is electrical convention to name diode terminal anode and cathode, but I reject it as a confusing and ambiguous naming convention. Yes, it's not quite correct, but it is a widely held convention, unlike numbering the pins 1 and 2 (or 3 or 4). For my diode symbols and footprints, I choose to name the terminals “P” and “N“ (for the p-type doped side and the n-type doped side). If you use P and N, Schottky diodes are now in error. ;) ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: gschem vs. PCB diode pin numbering
Kovacs Levente wrote: On Wed, 24 Aug 2011 08:21:17 -0400 Ethan Swint eswint.r...@verizon.net wrote: I've defined my own symbols and footprints to use 'A' and 'K' instead of 1 and 2. I don't think it's a good idea. Why not? ---)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 ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: gschem vs. PCB diode pin numbering - anode/cathode definition
On Thu, 25 Aug 2011 08:28:46 -0400 Ethan Swint eswint.r...@verizon.net wrote: On 08/24/2011 01:15 PM, Colin D Bennett wrote: On Wed, 24 Aug 2011 08:21:17 -0400 Ethan Swinteswint.r...@verizon.net wrote: On 08/23/2011 08:47 PM, Matthew Lewis wrote: I was double checking a pcb layout today and I discovered a rather nasty gotcha. It seems that gschem and PCB don't agree on which end of a diode should be pin 1. Gschem views pin 1 as the anode and PCB considers pin 1 to be the cathode. It doesn't prevent you from laying out a board correctly, but it does cause the silkscreen polarity to be printed backwards (for the SOD devices at least). I've defined my own symbols and footprints to use 'A' and 'K' instead of 1 and 2. That's a good idea. Anything you can do to error-proof yourself is a Good Thing. However, I refuse to use “anode” and “cathode” for diode symbols, since these terms refer to electron flow and are _incorrect_ when the diode is reverse-biased (most obvious for common Zener diode circuits). I understand that it is electrical convention to name diode terminal anode and cathode, but I reject it as a confusing and ambiguous naming convention. Yes, it's not quite correct, but it is a widely held convention, unlike numbering the pins 1 and 2 (or 3 or 4). For my diode symbols and footprints, I choose to name the terminals “P” and “N“ (for the p-type doped side and the n-type doped side). If you use P and N, Schottky diodes are now in error. ;) I am not an expert by any means, for in the 25 years I've dabbled in electronics, including a formal course in high school, it's always been K to designate the cathode (in addition to what the overall symbol implies, of course), regardless of the type of diode or the true direction of current flow. New users, and those not on this list, are not going to be aware of this thread, and are going to expect the anode/cathode convention to hold - anything else unnecessarily complicates things, and could potentially lead to much bigger problems (i.e. an apparent unreliability of gEDA or PCB). Why change what works for most electronics folks? -- There are some things in life worth obsessing over. Most things aren't, and when you learn that, life improves. http://digitalaudioconcepts.com Vanessa Ezekowitz vanessaezekow...@gmail.com ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: gschem vs. PCB diode pin numbering
On Thu, 25 Aug 2011 14:03:35 +0200 Kai-Martin Knaak kn...@iqo.uni-hannover.de wrote: Why not? Pinnumbers are numbers in the first place. Former versions of netlisters/PCB got confused by non-digital pinnumbers. With this approach you have to have a SOT23 footprint with 1,2,3 pinout, A,K,NC pinout, A1,A2,K pinout, B,C,E pinout etc. Sooner or later, your library will contain duplicated data. What if you discover that you want to modify the shape of the SOT23.fp footprint? You have to modify all of them. Yuk. I think a footprint must have only *one* pinout, that is a standard pinout of the package. Have an intermediate layer (scripts, database, pinmaps, etc.) that do the heavy lifting for you. Levente -- Levente Kovacs http://levente.logonex.eu ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: gschem vs. PCB diode pin numbering - anode/cathode definition
On Thu, 25 Aug 2011 08:28:46 -0400 Ethan Swint eswint.r...@verizon.net wrote: On 08/24/2011 01:15 PM, Colin D Bennett wrote: I understand that it is electrical convention to name diode terminal anode and cathode, but I reject it as a confusing and ambiguous naming convention. Yes, it's not quite correct, but it is a widely held convention, unlike numbering the pins 1 and 2 (or 3 or 4). Agreed that A and K certainly avoids ambiguity, as compared to numbering diode pins simply 1 and 2. It is 100% superior as it does convey the required information. For my diode symbols and footprints, I choose to name the terminals “P” and “N“ (for the p-type doped side and the n-type doped side). If you use P and N, Schottky diodes are now in error. ;) Good point. The moral of the story is: at least name the pins in a way that communicates the pin's function in a clear way. I will have to make my peace with the fact that there is no 100% technically correct way to do so... at least we can avoid errors caused by arbitrarily naming pins 1 and 2. Regards, Colin ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: gschem vs. PCB diode pin numbering
On Thu, 25 Aug 2011 22:41:28 +0200 Levente Kovacs leventel...@gmail.com wrote: On Thu, 25 Aug 2011 14:03:35 +0200 Kai-Martin Knaak kn...@iqo.uni-hannover.de wrote: Why not? Pinnumbers are numbers in the first place. Former versions of netlisters/PCB got confused by non-digital pinnumbers. Who cares? There's no reason to restrict ourselves from doing it right when the tools support it now. With this approach you have to have a SOT23 footprint with 1,2,3 pinout, A,K,NC pinout, A1,A2,K pinout, B,C,E pinout etc. Sooner or later, your library will contain duplicated data. What if you discover that you want to modify the shape of the SOT23.fp footprint? You have to modify all of them. Yuk. I won't get into it too much here; the logical vs. physical pinnumber assignment has been discussed in much detail before. http://thread.gmane.org/gmane.comp.cad.geda.user/32149/focus=37188 I think a footprint must have only *one* pinout, that is a standard pinout of the package. Have an intermediate layer (scripts, database, pinmaps, etc.) that do the heavy lifting for you. Maybe in an ideal world (when pin mapping orthogonal to the schematic and layout is introduced), but for now, the only two ways to handle transistors etc. properly is to either (1) create separate symbols for each pinout, where pinnumber is assigned numerically according to package pin number (1, 2, 3). For instance, you would need symbols NPN-EBC, NPN-BCE, etc., and potentially different symbols for packages with a fourth “tab” pin such as SOT-223-4 http://www.onsemi.com/pub/Collateral/NSS40300MZ4.PDF; or (2) create separate footprints for each pinout, using logical pinnumbers B, C, E, and footprints that assign these to appropriate package pins; then you only need two BJT symbols “NPN.sym” and “PNP.sym” that use these logical pins; this supports packages with a fourth “tab” pin without cluttering the schematic, and allows such details as pinout to be deferred until after basic schematic drawing. Do you really want to delete and re-add each of your dozens of transistors in gschem when you change the transistor to one with a different pinout? If you use a logically-pinned symbol, you can easily change the pinout by just editing the footprint attributes (gattrib, gschem property editor, export/import to/from spreadsheet, etc.). Conversation regarding TO-92 transistor package pinouts: http://thread.gmane.org/gmane.comp.cad.geda.user/37190/focus=37197 Well, I always say I won't get into the logical/physical pinning debate, but I always do. :-) For me, using logical pins on the schematic symbols such as transistors and diodes (*especially* diodes in IC packages like SOT-23) is the only way that makes sense ... at least until proper pin mapping is implemented. Regards, Colin ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: gschem vs. PCB diode pin numbering
Matthew Lewis wrote: but the change had no effect since the older m4 lib is being used when you import a schematic. You have to go back and manually replace the footprints if you want newlib. This is why I habitually move the m4 lib out of the way, so gnetlist does not find it even if it tries. Users have been struggling with this m4 persistency at least since 2005. ---)kaimartin(--- -- Kai-Martin Knaak Email: k...@familieknaak.de http://pool.sks-keyservers.net:11371/pks/lookup?search=0x6C0B9F53 increasingly unhappy 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: gschem vs. PCB diode pin numbering
On 08/23/2011 08:47 PM, Matthew Lewis wrote: I was double checking a pcb layout today and I discovered a rather nasty gotcha. It seems that gschem and PCB don't agree on which end of a diode should be pin 1. Gschem views pin 1 as the anode and PCB considers pin 1 to be the cathode. It doesn't prevent you from laying out a board correctly, but it does cause the silkscreen polarity to be printed backwards (for the SOD devices at least). I've defined my own symbols and footprints to use 'A' and 'K' instead of 1 and 2. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: gschem vs. PCB diode pin numbering
On Aug 24, 2011, at 5:21 AM, Ethan Swint wrote: On 08/23/2011 08:47 PM, Matthew Lewis wrote: I was double checking a pcb layout today and I discovered a rather nasty gotcha. It seems that gschem and PCB don't agree on which end of a diode should be pin 1. Gschem views pin 1 as the anode and PCB considers pin 1 to be the cathode. It doesn't prevent you from laying out a board correctly, but it does cause the silkscreen polarity to be printed backwards (for the SOD devices at least). I've defined my own symbols and footprints to use 'A' and 'K' instead of 1 and 2. This is what we do at my work as well. Steve ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: gschem vs. PCB diode pin numbering - anode/cathode definition
On Wed, 24 Aug 2011 08:21:17 -0400 Ethan Swint eswint.r...@verizon.net wrote: On 08/23/2011 08:47 PM, Matthew Lewis wrote: I was double checking a pcb layout today and I discovered a rather nasty gotcha. It seems that gschem and PCB don't agree on which end of a diode should be pin 1. Gschem views pin 1 as the anode and PCB considers pin 1 to be the cathode. It doesn't prevent you from laying out a board correctly, but it does cause the silkscreen polarity to be printed backwards (for the SOD devices at least). I've defined my own symbols and footprints to use 'A' and 'K' instead of 1 and 2. That's a good idea. Anything you can do to error-proof yourself is a Good Thing. However, I refuse to use “anode” and “cathode” for diode symbols, since these terms refer to electron flow and are _incorrect_ when the diode is reverse-biased (most obvious for common Zener diode circuits). I understand that it is electrical convention to name diode terminal anode and cathode, but I reject it as a confusing and ambiguous naming convention. For my diode symbols and footprints, I choose to name the terminals “P” and “N“ (for the p-type doped side and the n-type doped side). This models the structure of the device in an unambiguous way. This works perfectly for all types of diode (including LEDs), no matter how the device is used in the circuit. John Denker describes the most obvious problem with anode/cathode for Zener diodes [1]: You should never apply the terms anode or cathode to a Zener diode, because the potential for confusion is too great. Instead you should refer to the P-doped side and the N-doped side, and you should insist that others do the same. Note that reversing the labeling convention for Zener diode arrays would not solve the problem in any fundamental sense, because there are perfectly reasonable circuits in which – part of the time – a Zener diode is forward biased, so that it conducts just like any other diode. This is the same situation we encounter in connection with rechargeable batteries: if you attach permanent anode/cathode labels to the structure, you will be wrong at least part of the time. The terms “anode” and “cathode” properly apply to function, not structure. Rechargeable batteries are another place where the terms anode and cathode can cause confusion due to the fact that current can flow either direction between the battery terminals [2]. User PaulW had an interesting insight in comment #8 regarding the fact that “anode” and “cathode” are important from a battery chemistry standpoint, but “positive” and “negative” terminals are more useful from an electric perspective. Regards, Colin REFERENCES [1] John Denker. “How to Define Anode and Cathode.” http://www.av8n.com/physics/anode-cathode.htm#i-zener. [2] candlepowerforums.com thread started by Clifton Arnold. “anode is it positive or negetive” (sic). http://www.candlepowerforums.com/vb/showthread.php?41548-anode-is-it-positive-or-negetivep=453381viewfull=1#post453381. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
gEDA-user: gschem vs. PCB diode pin numbering
I was double checking a pcb layout today and I discovered a rather nasty gotcha. It seems that gschem and PCB don't agree on which end of a diode should be pin 1. Gschem views pin 1 as the anode and PCB considers pin 1 to be the cathode. It doesn't prevent you from laying out a board correctly, but it does cause the silkscreen polarity to be printed backwards (for the SOD devices at least). I've also noticed that gschem searches the older m4 library first ahead of the new pcblib. Is there a way to get PCB to use the newlib first? The reason I ask is because I swapped the pins on the diodes to match gschem in the newlib, but the change had no effect since the older m4 lib is being used when you import a schematic. You have to go back and manually replace the footprints if you want newlib. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: gschem vs. PCB diode pin numbering
It seems that gschem and PCB don't agree on which end of a diode should be pin 1. Welcome back to the transistor problem :-P I've also noticed that gschem searches the older m4 library first ahead of the new pcblib. Is there a way to get PCB to use the newlib first? Probably. I've been thinking of doing that within pcb at least (won't help gsch2pcb) and trying to think of any gotchas. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
