Re: gEDA-user: default pcb stackup change?
Hello, I just realized, that the 'view'-label in the status bar is still displaying the 'old' boardsize-names. The appended patch replaces them with 'top' and 'bottom'. Should I do a separate bug-report for this? Kind regards, Felix Am 11.04.2011 01:42, schrieb DJ Delorie: I'm pondering a minor change in pcb's defaults to give us a more useful default stackup. How's this? LAYERNAME (1, top), LAYERNAME (2, ground), LAYERNAME (3, signal2), LAYERNAME (4, signal3), LAYERNAME (5, power), LAYERNAME (6, bottom), LAYERNAME (7, outline), LAYERNAME (8, spare), This encompasses a few changes: 1. Default to six-layer stackup. You can ignore the signalN or power/ground layers for smaller boards. This covers nearly all PCB users (2/4/6 layers), and the rest can edit the stackup as usual. 2. Always include an outline layer. Handling an empty outline layer will need to be tweaked. 3. Rename outer layers to top/bottom, which seems to be what other packages (specifically, eagle and kicad) use. Component/solder isn't as obvious with SMT. We've used front/back elsewhere before, too, but that seems to be even less common. 4. Make the default layers in the right order to reflect a physical stackup. Note that this would be an interim change until we get around to either a new-board-wizard or new-means-load-template. So, geda/pcb users - would such a layout be a better default for you? Or worse? Or would something else make more sense? ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user From dfee0f07d5ad0c7da01b10dd948e98fb8ded5b35 Mon Sep 17 00:00:00 2001 From: Felix Ruoff fe...@posaunenmission.de Date: Tue, 19 Apr 2011 16:04:40 +0200 Subject: [PATCH] Change 'view' lable in status bar to top/bottom Since 11 April 2011 the default layer names are called 'top' and 'bottom' instead of 'component' and 'solder'. --- src/hid/gtk/gui-misc.c |4 ++-- 1 files changed, 2 insertions(+), 2 deletions(-) diff --git a/src/hid/gtk/gui-misc.c b/src/hid/gtk/gui-misc.c index 8bda96d..d4aa4e4 100644 --- a/src/hid/gtk/gui-misc.c +++ b/src/hid/gtk/gui-misc.c @@ -508,7 +508,7 @@ ghid_set_status_line_label (void) bclearance/b=%.1f btext/b=%i%% bbuffer/b=#%i), - Settings.ShowSolderSide ? _(solder) : _(component), + Settings.ShowSolderSide ? _(bottom) : _(top), PCB-Grid / 100.0, (int) Settings.GridFactor, TEST_FLAG (ALLDIRECTIONFLAG, PCB) ? all : @@ -531,7 +531,7 @@ ghid_set_status_line_label (void) bclearance/b=%5.3f btext/b=%i%% bbuffer/b=#%i), - Settings.ShowSolderSide ? _(solder) : _(component), + Settings.ShowSolderSide ? _(bottom) : _(top), PCB-Grid * COOR_TO_MM, (int) Settings.GridFactor, TEST_FLAG (ALLDIRECTIONFLAG, PCB) ? all : (PCB-Clipping == 0 ? 45 : -- 1.7.1 ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: default pcb stackup change?
On Mon, Apr 11, 2011 at 10:58:51AM +0530, Abhijit Kshirsagar wrote: 1. Agree! I'd find this much more intuitive and easy to work with. The layers option will be a big help... +1 I also like the ieda of dropping component/solder side, replacing it with whatever else that suggests one side and the other side. 2. What would go to the outline layer? The gerber files have outlines for each layer right? If your board is not rectangular, the outline layer would tell the fab house what shape to mill. It's sort of a hack as you draw something that looks copper but PCB supposed to handle it differently because the _name_ of the layer is outline. Regards, Tibor ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: default pcb stackup change?
Peter Clifton pc...@cam.ac.uk writes: On Sun, 2011-04-10 at 19:42 -0400, DJ Delorie wrote: I'm pondering a minor change in pcb's defaults to give us a more useful default stackup. How's this? LAYERNAME (1, top), LAYERNAME (2, ground), LAYERNAME (3, signal2), LAYERNAME (4, signal3), LAYERNAME (5, power), LAYERNAME (6, bottom), LAYERNAME (7, outline), LAYERNAME (8, spare), I'm very keen to see this change. The PCB+GL renderer (for example), needs layers (actually layer group numbers) in the correct physical order to be able to figure out how to render 3D views. Our current default stack is totally useless for that. I'd very much like to not have any exporters/renderers requiring the layers to be in physical order, since I tend to move the final order around a lot. My layer order is defined in the README that goes to the board house, and little text numbers in the layers. A layer attribute that tells Ben-mode and PCB+GL how to render the stack may be the way to go. Is it really the layer order, or the group order that PCB+GL or Ben-mode uses? -- Stephan ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: default pcb stackup change?
Is it really the layer order, or the group order that PCB+GL or Ben-mode uses? PCB draws in group order, not layer order. So you can order the drawing layers as you wish, as long as the group order is set to your stacking order. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: default pcb stackup change?
I basically agree, but why stop here and not add a Z coordinate to each layer? You deleted the answer to that: Note that this would be an interim change until we get around to either a new-board-wizard or new-means-load-template. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: default pcb stackup change?
On Mon, Apr 11, 2011 at 03:20:11AM -0400, DJ Delorie wrote: I basically agree, but why stop here and not add a Z coordinate to each layer? You deleted the answer to that: Note that this would be an interim change until we get around to either a new-board-wizard or new-means-load-template. Well, I did not really understand that paragraph. Anyeay, fine with me, although I don't really see the interest of an interim step. Regards, Gabriel ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: default pcb stackup change?
Well, I did not really understand that paragraph. Anyeay, fine with me, although I don't really see the interest of an interim step. I.e none of us have time right now to completely rewrite how layers work This was a fairly quick change which should make the current PCB more obviously usable to new users by pre-exposing some of the newer features and setting things up to resemble reality closer. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: default pcb stackup change?
On 04/11/2011 02:11 AM, Gabriel Paubert wrote: consider layers with the same Z coordinate as a layer group OK, that could be used for stackup, and also farther along, Z is a general axis designator, so would become Z position in the stackup, so your group number attrib should be some other name than Z. Why not add it? Because DJ is doing a minor change and has no time budget for a sweeping overhaul. John ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: default pcb stackup change?
On Mon, 2011-04-11 at 08:18 +0200, Stephan Boettcher wrote: Peter Clifton pc...@cam.ac.uk writes: Is it really the layer order, or the group order that PCB+GL or Ben-mode uses? The group numbering - and I don't see any reason why we can't stipulate that is the rendering sequence. -- 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!) Tel: +44 (0)1223 748328 - (Shared lab phone, ask for me) signature.asc Description: This is a digitally signed message part ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: default pcb stackup change?
The group numbering - and I don't see any reason why we can't stipulate that is the rendering sequence. I think we decided that a while back. The group order *is* the stacking order. Now we just need to figure out how to enforce it :-) ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: default pcb stackup change?
On Mon, Apr 11, 2011 at 11:35 PM, DJ Delorie d...@delorie.com wrote: Now we just need to figure out how to enforce it :-) With a stick! ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: default pcb stackup change?
On Mon, 11 Apr 2011 02:45:18 +0200 Kai-Martin Knaak k...@lilalaser.de wrote: DJ Delorie wrote: I'm pondering a minor change in pcb's defaults to give us a more useful default stackup. How's this? LAYERNAME (1, top), LAYERNAME (2, ground), LAYERNAME (3, signal2), LAYERNAME (4, signal3), LAYERNAME (5, power), LAYERNAME (6, bottom), LAYERNAME (7, outline), LAYERNAME (8, spare), This encompasses a few changes: 1. Default to six-layer stackup. You can ignore the signalN or power/ground layers for smaller boards. This covers nearly all PCB users (2/4/6 layers), and the rest can edit the stackup as usual. I like KMK's idea; I'd suggest his proposed switches establish the following: I like to have a comment layer just below the outline layer. In this layer I put internal notes. [...] Make the default layer stack depend on options: --2layer 1, Top 2, Bottom 3, Outline 4, Notes --4layer 1, Top 2, Signal 2 3, Signal 3 4, Bottom 5, Outline 6, Notes (This is similar to the stackup I usually use, except with different names). --6layer As DJ suggested originally, with Notes on layer 8. -- There are some things in life worth obsessing over. Most things aren't, and when you learn that, life improves. http://starbase.globalpc.net/~ezekowitz 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: default pcb stackup change?
On Sun, Apr 10, 2011 at 6:42 PM, DJ Delorie d...@delorie.com wrote: I'm pondering a minor change in pcb's defaults to give us a more useful default stackup. How's this? My netlist enters pcb by way of gsch2pcb, which supplies its own default stackup. Can these be kept in sync somehow? Regards, Mark markrages@gmail -- Mark Rages, Engineer Midwest Telecine LLC markra...@midwesttelecine.com ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: default pcb stackup change?
Mark Rages wrote: My netlist enters pcb by way of gsch2pcb, which supplies its own default stackup. Can these be kept in sync somehow? My current work-around is to call pcb without a filename but with multiple command line options to set the layer stack. After a save with the desired name, gsch2pcb happily adopts this empty layout. The scripting feature of pcb can be used to do this without GUI interaction. Here is a snippet from my create-project-script: /- # Create an empty layout echo \ ChangeName(Layout) \ SaveTo(LayoutAs,$NAME.pcb) \ Quit() \ | pcb --listen \ --fab-author \$AUTHOR\ \ --groups 1,2,3,c:4,5,5,s:7:8 \ --layer-name-1 top \ --layer-name-2 top-polyg. \ --layer-name-3 top-GND \ --layer-name-4 bottom \ --layer-name-5 bott.-poly. \ --layer-name-6 bott.-GND \ --layer-name-7 comment \ --layer-name-8 outline \ --bloat 600 \ --shrink 1000 \ --min-width 600 \ --min-silk 600 \ --min-drill 1500 \ --min-ring 1000 \ --route-styles \ Signal,1000,3600,2000,1000\ :Power,2500,6000,3500,1000\ :Fat,4000,6000,3500,1000\ :Skinny,600,2402,1181,600 \ --default-PCB-width 60 \ --default-PCB-height 60 \ --grid-increment-mm 1.00 \ --grid-increment-mil 20.00 \ --size-increment-mm 0.20 \ --size-increment-mil 10.00 \ --line-increment-mm 0.10 \ --line-increment-mil 8.00 \ --clear-increment-mm 0.50 \ --clear-increment-mil 2.00 \-- ---)kaimartin(--- -- Kai-Martin Knaak Email: k...@familieknaak.de Öffentlicher PGP-Schlüssel: http://pool.sks-keyservers.net:11371/pks/lookup?search=0x6C0B9F53 ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: default pcb stackup change?
On Sun, 2011-04-10 at 19:42 -0400, DJ Delorie wrote: I'm pondering a minor change in pcb's defaults to give us a more useful default stackup. How's this? LAYERNAME (1, top), LAYERNAME (2, ground), LAYERNAME (3, signal2), LAYERNAME (4, signal3), LAYERNAME (5, power), LAYERNAME (6, bottom), LAYERNAME (7, outline), LAYERNAME (8, spare), I'm very keen to see this change. The PCB+GL renderer (for example), needs layers (actually layer group numbers) in the correct physical order to be able to figure out how to render 3D views. Our current default stack is totally useless for that. -- 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!) Tel: +44 (0)1223 748328 - (Shared lab phone, ask for me) signature.asc Description: This is a digitally signed message part ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: default pcb stackup change?
DJ Delorie wrote: I'm pondering a minor change in pcb's defaults to give us a more useful default stackup. How's this? LAYERNAME (1, top), LAYERNAME (2, ground), LAYERNAME (3, signal2), LAYERNAME (4, signal3), LAYERNAME (5, power), LAYERNAME (6, bottom), LAYERNAME (7, outline), LAYERNAME (8, spare), This encompasses a few changes: 1. Default to six-layer stackup. You can ignore the signalN or power/ground layers for smaller boards. This covers nearly all PCB users (2/4/6 layers), and the rest can edit the stackup as usual. Make the default layer stack depend on options: --2layer --4layer --6layer 2. Always include an outline layer. Handling an empty outline layer will need to be tweaked. Very good. 3. Rename outer layers to top/bottom, which seems to be what other packages (specifically, eagle and kicad) use. Component/solder isn't as obvious with SMT. We've used front/back elsewhere before, too, but that seems to be even less common. yes, please! Top/bottom is the preferred naming schema at my place and of my favorite fab. 4. Make the default layers in the right order to reflect a physical stackup. nice. Note that this would be an interim change until we get around to either a new-board-wizard or new-means-load-template. IMHO, pcb already sort of behaves like that -- If I start pcb from scratch, I get an empty layout with the stack like it is defined in .pcb/preferences So, geda/pcb users - would such a layout be a better default for you? Or worse? Or would something else make more sense? I like to have a comment layer just below the outline layer. In this layer I put internal notes. ---)kaimartin(--- -- Kai-Martin Knaak Email: k...@familieknaak.de Öffentlicher PGP-Schlüssel: http://pool.sks-keyservers.net:11371/pks/lookup?search=0x6C0B9F53 ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: default pcb stackup change?
3. Rename outer layers to top/bottom, which seems to be what other packages (specifically, eagle and kicad) use. Component/solder isn't as obvious with SMT. Sometimes the outer layers are called Primary and Secondary. Consider a board of memory chips. Some memories come in mirror image footprints. One side looks exactly like the other side when you populate both sides with such mirrored chips. Gets even more interesting when the 'Top Side' gets put in an enclosure upside down and production doesn't realize the connector can't be mirrored too. :-( I concede that Top/Bottom is more common, not necessarily accurate. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: default pcb stackup change?
I concede that Top/Bottom is more common, not necessarily accurate. We can't just call them this side and that side :-) ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: default pcb stackup change?
On 04/10/2011 06:42 PM, DJ Delorie wrote: would such a layout be a better default for you? Fine by me. JG -- Ecosensory Austin TX ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: default pcb stackup change?
On 04/10/2011 08:26 PM, Bob Paddock wrote: Sometimes the outer layers are called Primary and Secondary. Main and Second are shorter and might convey similar meaning and be more usable... JG ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: default pcb stackup change?
Pci cards call them A and B sides. But that too is odd. It seems that, like it or not, top and bottom are the industry standard. On Apr 11, 2011, at 11:24 AM, John Griessen j...@ecosensory.com wrote: On 04/10/2011 08:26 PM, Bob Paddock wrote: Sometimes the outer layers are called Primary and Secondary. Main and Second are shorter and might convey similar meaning and be more usable... JG ___ 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: default pcb stackup change?
1. Agree! I'd find this much more intuitive and easy to work with. The layers option will be a big help... 2. What would go to the outline layer? The gerber files have outlines for each layer right? ~Abhijit ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: default pcb stackup change?
2. What would go to the outline layer? The shape of your board, for example. The gerber files have outlines for each layer right? Not by default, no. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
