Re: gEDA-user: How to change the length of multiple nets at once?
On 8/14/06, Ales Hvezda [EMAIL PROTECTED] wrote: [snip] Is there some way to adjust the length (i.e. end points) of multiple nets at once? No builtin mechanism exists at this point. This has been requested a few times in the past, so it's somewhere on the todo list, however, filing a feature request never hurts. This might be a good task for somebody wanting to get involved in development. I'm keeping a list of wishes based on first impressions. When I finish my design I'll review them and see how many are still applicable once I have more experience with the tool. The ones that still make sense will wend their way into feature requests, or, possible, patches to the code. The answer I came up with as I wrote this was to attach off-page connectors to each of the nets, then I should be able to grab multiples of those and move them left or right as I desire. It could be argued that having off-page connectors is a good idea in the first place. But I am still curious to learn if there is some other mechanism to do this. Clever workaround. -Ales The key to making that work would be another feature I miss... It would be nice if Redo redid the last paste, down (up, left, right) some increment. Then I would attach the first off page connector, copy it, paste it on the next net down, and then just hit R over and over again until all of the nets had off page connectors attached to them. This has an obvious application to attaching a bunch o' nets to a bus. It probably has other applications as well. It's enough to make me want to dive into the code... I just need to finish this design first... then I need to fab it... then I need to assemble it... then I need to debug it... then I need to write the code for it... then I need to breathe :-) Of course, if I don't get some funding for the design soon, then the fab, assemble, ... cycle will stall and I can distract myself with other ideas (such as tinkering with gschem). --wpd ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
gEDA-user: Renumber in PCB/Was/Is List
Does PCB have a renumbering command? This would be a command that would renumber the components on the circuit board say starting with the smallest value in the upper left and then proceeding to the lower right corner of the board. And this would also generate a was/is list, showing the old component refdes and the new one(ideally you would have an app that could take the was/is and update the sch file). ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Renumber in PCB/Was/Is List
Mike Hansen wrote: Does PCB have a renumbering command? This would be a command that would renumber the components on the circuit board say starting with the smallest value in the upper left and then proceeding to the lower right corner of the board. And this would also generate a was/is list, showing the old component refdes and the new one(ideally you would have an app that could take the was/is and update the sch file). Not currently. Sounds like a good idea though. I'd recommend that we try to make the was/is file be flexible enough to handle slot/pin swapping and maybe some other back annotation sorts of data. I'd also make it an easy to parse format that isn't tied to gschem. If you feel like putting together a patch, I'd be interested. It is probably not all that hard. If you're interested I can point you in the right direction. -Dan ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Renumber in PCB/Was/Is List
Is there documentation anywhere on how to get started in developing for PCB/gschem? No formal documentation, but it's not hard. Look at src/puller.c for an example of tying a custom function in (the action API is in hid.h). You can also look at src/hid/bom/bom.c for code that looks up the X,Y location of all elements. The only remaining part is to look in undo.h and change.h for the relevent functions to actually rename the elements. To add a file to the build, look for puller in src/Makefile.am and add yours in the same way, then run autogen.sh. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Renumber in PCB/Was/Is List
You probably need to update the loaded netlist too. I think the function that changes the element name should be responsible for that change also. No point making everyone's life difficult. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Renumber in PCB/Was/Is List
I think the function that changes the element name should be responsible for that change also. No point making everyone's life difficult. At least, with a flag that says to do it. I wonder if we'd screw the user by not letting them rename an element out of the net. OTOH they can always reload the netlist, if they can. No easy answer here, I suppose. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Renumber in PCB/Was/Is List
Well at least with this proposed mod(the renumber) one would definitely want to update the netlist. The normal procedure would be to do the renumber, spit out the was/is list, using the was/is list update your schematic(of course it would be desirable to have a utility to update the schematic also with the was/is list). This is pretty standard functionality in commercial packages. The board stuffers like to have the components in a logical arrangement(R10 is near R9, etc.). From: DJ Delorie [EMAIL PROTECTED] Reply-To: gEDA user mailing list geda-user@moria.seul.org To: geda-user@moria.seul.org Subject: Re: gEDA-user: Renumber in PCB/Was/Is List Date: Tue, 15 Aug 2006 15:23:05 -0400 I think the function that changes the element name should be responsible for that change also. No point making everyone's life difficult. At least, with a flag that says to do it. I wonder if we'd screw the user by not letting them rename an element out of the net. OTOH they can always reload the netlist, if they can. No easy answer here, I suppose. ___ 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: Renumber in PCB/Was/Is List
This is pretty standard functionality in commercial packages. The board stuffers like to have the components in a logical arrangement(R10 is near R9, etc.). I always numbered mine by pages, like all R100-R199 were on schematic page 1, etc. They tended to get grouped together anyway that way. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Renumber in PCB/Was/Is List
The feature I'm most looking forward to coming out of this exercise is the ability to back annotate pin-swap information. Right now I'm just plugging my busses together between the processor and the memory (or interface connector, or whatever), anticipating that when I look at the rats nest I'll wish I swapped the order of a few things. If I can do that in PCB and then flow the information back to the schematic, that will be great. Otherwise, I'm anticipating a couple of iterations of the schematic until I see something I like. Perhaps those with more experience in this area in general, and with these tools in particular, would care to comment on a better approach. I've got thick skin -- be brutal :-) --wpd ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Renumber in PCB/Was/Is List
Perhaps those with more experience in this area in general, and with these tools in particular, would care to comment on a better approach. Having just went through this... I added more slots to the dual XOR I was working with; the extra slots had pins swapped. I kept gschem and pcb both open, plus an xterm. When I wanted to swap pins in pcb, I'd change the slot in gschem, save, Up-Return to rerun gsch2pcb, and File-Load Netlist in pcb. It goes quickly once you get used to it. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Renumber in PCB/Was/Is List
Patrick - On Tue, Aug 15, 2006 at 03:51:41PM -0400, Patrick Doyle wrote: The feature I'm most looking forward to coming out of this exercise is the ability to back annotate pin-swap information. Right now I'm just plugging my busses together between the processor and the memory (or interface connector, or whatever), anticipating that when I look at the rats nest I'll wish I swapped the order of a few things. If I can do that in PCB and then flow the information back to the schematic, that will be great. I've given up using schematics for this sort of thing. I just lay out the board, export the net list to a table (or spreadsheet, if you like), and then derive the mapping between FPGA signal names and pins from that list. The schematic is reserved for things other than connecting 100 dots on one chip to 100 dots on other chips. Example: http://recycle.lbl.gov/llrf4/ - Larry ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Renumber in PCB/Was/Is List
Well I am also very interested in pin swapping at the PCB level and then having the schematic corrected. Some of the devices use differential I/O it would be nice if these pin pairs were tied together. But on FPGA's the use of a pair of pins as differential or single ended is mostly up to the designer. I have been giving some thought (I need to be careful here because DJ might be listening and some of you might remember what DJ did with my meanderings about porn converted to PCB foot prints) to an expanded hierarchical netlist which would include information about which pins can be swapped and which of those pins can also be used as differential pairs. Retaining the order in which the pins are swapped is critical. Esentialy this is how I manualy do it today. 1) draw schematic 2) generate netlist 3) import netlist into PCB 4) figure out which pins to swap (write them down) 5) edit schematic and swap pins by hand 6) regenerate netlist 7) re-import netlist into pcb 8) repeat steps 4 through 7 until i am more crazzy then usual and the board is completed. 9) find and fix all the shorted pollygons ;) now i am much more crazzy then normal My general idea has been that for pin level swapping the symbol must be embedded in the schematic. A netlist which tells PCB which pins and slots are swapable. PCB would do its majic, correcting its version of the netlist and generating a list of swapped pins.. This list of swapped pins would then be output as a file and a new program would read in the file and swap the attribute information for the embedded symbols. This would mean that none of the nets would need to be moved. Also, I would suggest a move towards XML for these files (new netlist and swapped pins) Steve Meier On Tue, 2006-08-15 at 15:51 -0400, Patrick Doyle wrote: The feature I'm most looking forward to coming out of this exercise is the ability to back annotate pin-swap information. Right now I'm just plugging my busses together between the processor and the memory (or interface connector, or whatever), anticipating that when I look at the rats nest I'll wish I swapped the order of a few things. If I can do that in PCB and then flow the information back to the schematic, that will be great. Otherwise, I'm anticipating a couple of iterations of the schematic until I see something I like. Perhaps those with more experience in this area in general, and with these tools in particular, would care to comment on a better approach. I've got thick skin -- be brutal :-) --wpd ___ 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
gEDA-user: Python equivalent for $realtobits
Does anybody know how I could perform the equivalent of $realtobits in Python? Thanks, Matt ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Renumber in PCB/Was/Is List
Mike Hansen wrote: Does PCB have a renumbering command? This would be a command that would renumber the components on the circuit board say starting with the smallest value in the upper left and then proceeding to the lower right corner of the board. And this would also generate a was/is list, showing the old component refdes and the new one(ideally you would have an app that could take the was/is and update the sch file). Is there any value in having some controls to how the renumbering would work? In particular, you might want to number left to right, top to bottom like: R1 R2 R3 R4 R5 R6 R7 R8 R9 but maybe you want left to right then top to bottom like R1 R4 R7 R2 R5 R8 R3 R6 R9 I guess one could support tblr, tbrl, btlr, btrl, tblr, tbrl, btlr, btrl. Would this just create confusion? It could be that tblr is the default if not specified. Renumber() = uses tblr, prompts for filename Renumber(lrtb) = uses lrtb, prmopts for filename Renumber(tblr, filename) = uses tblr and specified file -Dan ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Renumber in PCB/Was/Is List
DJ Delorie wrote: While thats one valid method, please don't enforce it. Enforce, no, but I was hoping the final code could perhaps support it. Say, by only modifying the last N digits? In this case, is there really much value in renumbering at all from the layout end of the flow? -Dan ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Python equivalent for $realtobits
I'm not 100% sure what you want but you could try looking at the struct package in python. I have used that to pack and unpack bit streams into ints, chars, longs, etc... it probably supports floats as well. --wpd ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
gEDA-user: Re: Documentation in spanish
On Mon, 14 Aug 2006 22:30:17 -0500, Jorge Ernesto Guevara Cuenca wrote: and if is possible link in some place of the wiki the next documents: Just in case you haven't already: You may ask Ales for an account, so you can add the links to the spanish pages yourself. It is a Wiki! :-) (http://geda.seul.org/wiki/#about_the_wiki) ---(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: Re: Documentation in spanish
On 8/15/06, Kai-Martin Knaak [EMAIL PROTECTED] wrote: On Mon, 14 Aug 2006 22:30:17 -0500, Jorge Ernesto Guevara Cuenca wrote: and if is possible link in some place of the wiki the next documents: Just in case you haven't already: You may ask Ales for an account, so you can add the links to the spanish pages yourself. It is a Wiki! :-) (http://geda.seul.org/wiki/#about_the_wiki) Ouch!, it asks made. ---(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 -- Jorge Ernesto Guevara Cuenca http://www.el-directorio.org El sitio de Software Libre y Linux en Colombia ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Renumber in PCB/Was/Is List
Mike Hansen wrote: I do find this useful(of course it was me that started the thread). My schematic workflow may not be the best. I just plunk down refdes's that are unique and then when I get to the PCB I would like to simply renumber and then do a was/is on the schematic once I am done. Just to be clear, DJ was talking about the case where R1## are on page 1, R2## on page 2, etc and was suggesting that a board level renumbering wouldn't mess with the 1st digit. It is this particular case where you're trying to maintain some of the schematic numbering where I wondered if renumbering from the layout made sense. In the case were you're globally renumbering from layout I can certainly see that it would be a preference for some people. In this day of automation the part numbering on the PCB may not be as big a deal as it once was...back in the day the board stuffers had people sitting on row after row of benches stuffing parts into the PCB and sending them off to wave soldering. It was a good idea to keep part numbers in a logical order so that they weren't searching for the next part to stuff on the board. But even when I do protos I find myself lost on the board if there isn't a logical order. I will see if I can squeeze in some time to look at the example code to perform this task. ok. I actually made a little more progress, but there are some details left on what it should do to be worked out. From: DJ Delorie [EMAIL PROTECTED] Reply-To: gEDA user mailing list geda-user@moria.seul.org To: geda-user@moria.seul.org Subject: Re: gEDA-user: Renumber in PCB/Was/Is List Date: Tue, 15 Aug 2006 18:42:09 -0400 In this case, is there really much value in renumbering at all from the layout end of the flow? Good point ;-) ___ 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 ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
