Re: gEDA-user: PCB | how to update the pcb, if a change is made to the schematic?
On Fri, 13 Feb 2009 13:32:17 -0800, S. Aguinaga wrote: ** In the PCB, is there a command to move components to a specific x,y location? No. (This is one of my favorite feature requests) ** After starting on the PCB, I have to make a change to the schematics, is there a way to update the pcb file? Without affecting placement or All routing? Yes. 1) Save the current state of the layout in pcb. 2) call gsch2pcb with the changed schematic 3) If you changed connections, an updated netlist will be produced. If you changed the value of components, they will be updated in the pcb file. If you removed some components, they will be deleted in the pcb file. If you added some components, a file $NAME_new.pcb will be produced. This file contains all the footprints of the added components. 4) In pcb do a) File - Revert(if the changes affected the layout) b) File - Load_layout_data_to_paste_buffer (to put the new footprints somewhere on the layout with the buffer-tool) c) File - Load_netlist_file (if connections were changed) The tool xgsch2pcb reduces these steps to a single mouse click. ---(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 | how to update the pcb, if a change is made to the schematic?
On Fri, Feb 13, 2009 at 01:32:17PM -0800, S. Aguinaga wrote: ** In the PCB, is there a command to move components to a specific x,y location? Not really, although if you get my distribute/align plugin from gedasymbols you can bind a key to warp the selected elements to the cursor. So you can set the grid, move to a spot and hit a key to move the element. ** After starting on the PCB, I have to make a change to the schematics, is there a way to update the pcb file? Without affecting placement or All routing? You run gsch2pcb again. It produces a board.pcb.new which you load into your layout (File | Load layout data...) and a new netlist. Your board.pcb is unaffected except that deleted components are removed. I recommend you keep all of your working files under some kind of source control (RCS, CVS, SVN, etc) so you can save versions of your board before you do this. -- Ben Jackson AD7GD b...@ben.com http://www.ben.com/ ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: PCB | how to update the pcb, if a change is made to the schematic?
Ben Jackson wrote: On Fri, Feb 13, 2009 at 01:32:17PM -0800, S. Aguinaga wrote: ** In the PCB, is there a command to move components to a specific x,y location? Not really, although if you get my distribute/align plugin from gedasymbols you can bind a key to warp the selected elements to the cursor. So you can set the grid, move to a spot and hit a key to move the element. ** After starting on the PCB, I have to make a change to the schematics, is there a way to update the pcb file? Without affecting placement or All routing? You run gsch2pcb again. It produces a board.pcb.new which you load into your layout (File | Load layout data...) and a new netlist. Your board.pcb is unaffected except that deleted components are removed. I recommend you keep all of your working files under some kind of source control (RCS, CVS, SVN, etc) so you can save versions of your board before you do this. I completely agree with Ben's comment. I tend to check in things like schematics or layouts in progress quite regularly since it gives a good way to backtrack if you do something stupid like 'rm *'. Not that I've ever done that before It also helps if you manage to mess up something and just want to revert. -Dan ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
