Re: gEDA-user: pcb bug: EPS output omits pads
pcb -x eps \ --element-color '#ff' \ --pin-color '#00' \ --layer-color-1 '#ff' \ --as-shown \ --layer-stack 0,elements,pins \ --eps-file testprint.eps \ powermeter.pcb Besides layer names, it accepts rats, invisible, pins, vias, and elements. This is a partial work-around for some cases, but I would agree with the original assertion that something is amiss with the eps export. For some documentation that I'm writing, I need a vector drawing of my circuit board *as it appears*, i.e., with silk, pins, and vias -- but not tracks-- visible. (Kinda like ben/photo mode, but in vector.) So far as I can tell, pcb is quite incapable of exporting an eps drawing like that, even though it's trivial to display just those parts by clicking which layers are visible. Since this is considerably different from what would be expected by a reasonable observer, I would indeed classify it as a bug-- either in the function executed or in the label, because it cannot generate an eps as shown. The method that you describe above-- exporting a file with some parts invisible-- can be used to make the tracks invisible as well. I can use that method to produce a fake version of what I need, with the tracks in white but the silk, pins, and vias visible, but those white tracks are *still there* and actually do get in the way of what I'm doing. I did find a genuine but invasive work-around that can generate the output that I wanted, which *may* also help with the pad-omission problem as well. Make a duplicate pcb file for documentation/output: circuit-doc.pcb Open the circuit-doc.pcb file in a text editor, delete the entire contents of all layers with tracks on them. Pins and pads should not be affected, since they are stored as parts of the element. Save and then open the modified file in pcb. Make all layers visible and export eps. This should everything but the tracks to the EPS file. - Windell Windell H. Oskay Evil Mad Scientist Laboratories http://www.evilmadscientist.com/ ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: pcb bug: EPS output omits pads
On Thu, 22 Jan 2009 14:51:43 -0500, Windell H. Oskay wrote: Since this is considerably different from what would be expected by a reasonable observer, I would indeed classify it as a bug-- either in the function executed or in the label, because it cannot generate an eps as shown. Ack. The as-shown not printing as shown option made me feel uneasy too. Anyway, I filed a feature request Better Control of Postscript Output http://sourceforge.net/tracker/index.php?func=detailaid=2528814group_id=73743atid=538814 I wish I could specify print properties according to layer _and_ object type. This is one the topics, pcb could adopt from protel95. ---(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
gEDA-user: pcb bug: EPS output omits pads
The eps output of pcb does not contain pads if the option --as-shown is active. Pins are drawn correctly. ---(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 GPG key:http://pgp.mit.edu:11371/pks/lookup?search=Knaak+kmkop=get ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: pcb bug: EPS output omits pads
On Wed, 21 Jan 2009 11:56:41 -0500, DJ Delorie wrote: The eps output of pcb does not contain pads if the option --as-shown is active. Pins are drawn correctly. Could you be more specific? Like, the entire command line? Option --as-shown is only meaningful, if some layers are switched off. However, I don't see a way to switch off layers with the command line. The option --action-string ToggleView(1) does not seem to have an effect on pcb. (Yet another bug?) To reproduce the eps output bug in GTK-GUI: 1) Load a layout with SMD pads 2) switch off visibility of the first copper layer ( :ToggleView(1) ) 3) Got to: file - export_layout - eps 4) check as-shown 5) click ok The produced eps file will contain the visible layers, and pins, but no SMD pads. ---(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 GPG key:http://pgp.mit.edu:11371/pks/lookup?search=Knaak+kmkop=get ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: pcb bug: EPS output omits pads
Option --as-shown is only meaningful, if some layers are switched off.However, I don't see a way to switch off layers with the command line. The option --action-string ToggleView(1) does not seem to have an effect on pcb. (Yet another bug?) That's what the --layer-stack option is for. To reproduce the eps output bug in GTK-GUI: 1) Load a layout with SMD pads 2) switch off visibility of the first copper layer ( :ToggleView(1) ) 3) Got to: file - export_layout - eps 4) check as-shown 5) click ok The produced eps file will contain the visible layers, and pins, but no SMD pads. Amusingly enough, that's kinda intentional. The exporters deal with copper layers, so turning off layer 1 turns off all the copper on layer 1. The pins you see drawn are actually from layer 2. The GUI hids are treated special in the draw routines, since the core knows that the GUI will be overlaying each layer (for example, it knows it doesn't need to draw the pins on every layer, just the last-drawn one). One thing you could try is setting the gui flag in the HID structure for EPS and see if it draws what you want. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: pcb bug: EPS output omits pads
On Wed, 21 Jan 2009 13:14:04 -0500, DJ Delorie wrote: line. The option --action-string ToggleView(1) does not seem to have an effect on pcb. (Yet another bug?) That's what the --layer-stack option is for. How would I use this option? What is the syntax of a layer stack? I can't find neither in the manual. ( http://pcb.sourceforge.net/pcb-20081128/pcb.html ) Seems like the description of options is completely out of date in the manual. By the way, where can I access your shiny new pcb HOWTO? Amusingly enough, that's kinda intentional. The exporters deal with copper layers, so turning off layer 1 turns off all the copper on layer 1. The pins you see drawn are actually from layer 2. I see. However, there are legitimate reasons to print only certain groups of objects. In my case, our assembler suggested to remove the tracks but keep pads and pins. In addition, they'd like to have the pads drawn in a different color than the pins. Since SMD components require Maybe, I can tweak the postscript output HID to my needs. I assume, the information which layers to print on what page is hard coded into source. Can you point me to where this information sits? One thing you could try is setting the gui flag in the HID structure for EPS and see if it draws what you want. -vv, please. I don't see a gui flag in pcb -h ---(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 GPG key:http://pgp.mit.edu:11371/pks/lookup?search=Knaak+kmkop=get ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: pcb bug: EPS output omits pads
How would I use this option? What is the syntax of a layer stack? I can't find neither in the manual. ( http://pcb.sourceforge.net/pcb-20081128/pcb.html ) Seems like the description of options is completely out of date in the manual. By the way, where can I access your shiny new pcb HOWTO? The manual is out of date in general. While we document actions automatically, we don't do that for command line options as well. Here's an example: testprint : pcb -x eps \ --element-color '#ff' \ --pin-color '#00' \ --layer-color-1 '#ff' \ --as-shown \ --layer-stack 0,elements,pins \ --eps-file testprint.eps \ powermeter.pcb Besides layer names, it accepts rats, invisible, pins, vias, and elements. I see. However, there are legitimate reasons to print only certain groups of objects. In my case, our assembler suggested to remove the tracks but keep pads and pins. See my snippet above, which does something similar. I don't know if you can do pins and pads separately, though. Maybe, I can tweak the postscript output HID to my needs. I assume, the information which layers to print on what page is hard coded into source. Can you point me to where this information sits? The eps hid is in src/hid/ps/eps.c -vv, please. I don't see a gui flag in pcb -h It's a compile-time flag that tells the core what type of HID each HID is. You won't find it in the help. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
