Re: gEDA-user: "Source" file not found
Mike Bushroe writes: > John, > Thanks for the clarification. I checked and I have created a unique > 'name':'number' for each net attribute, and matched input to output names. > If a net is formed for each unique name:number, and all inputs and outputs > with that unique name are combined together, then that was exactly what I > was looking for. The number must be :1 in all cases, because it is pin 1 of the IO-symbol, that your net connects to. -- Stephan ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: "Source" file not found
On May 27, 2010, at 6:01 PM, John Griessen wrote: > I believe it's more a symbol pinnumber to pinlabel correspondence > that matches up symbol pin to subschematic refdes name same as pin label. > There's no number on a IO port symbol in a subschematic. You're thinking hierarchy, but Mike's not using hierarchy. He's trying to use symbols to connect pages at top level. Not the most natural thing to do in the gEDA paradigm, but gEDA is flexible... 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: "Source" file not found
Mike Bushroe wrote: If a net is formed for each unique name:number, and all inputs and outputs with that unique name are combined together, then I believe it's more a symbol pinnumber to pinlabel correspondence that matches up symbol pin to subschematic refdes name same as pin label. There's no number on a IO port symbol in a subschematic. John ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: "Source" file not found
John, Thanks for the clarification. I checked and I have created a unique 'name':'number' for each net attribute, and matched input to output names. If a net is formed for each unique name:number, and all inputs and outputs with that unique name are combined together, then that was exactly what I was looking for. I briefly tried the up/down hierarchy, but clearly did not understand what it was doing, so I went back to just using input and output symbols and giving each connection a unique name. Mike ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: "Source" file not found
On May 27, 2010, at 10:51 AM, Mike Bushroe wrote: > Then I did a text > search through each schematic file and found only one occurrence of > ROV_2010_ananlog.sch in any of the schematic files, and that was part > of an 'input' symbol and was listed as 'source'. That doesn't make any sense to the netlister. You use source= when you have made a symbol that represents an entire hierarcical subcircuit, with all its inputs and outputs. Then you associate source= attributes with the symbol so that the netlister can find the schematics associated with that subcircuit. You also have to tell the netlister where to find such schematics in gafrc. The whole input/output symbol thing can be very confusing until you understand how the netlister works. If you're not using hierarchy, I recommend avoiding those symbols and just attaching netname= attributes to nets. All nets with the same name will be connected together. I sometimes use busses to visually indicate global connectivity. If you want to use some sort of IO symbol to connect nets together on different sheets at the same level, use the net= attribute. Look at gnd-1.sym to see how that works. 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
gEDA-user: "Source" file not found
I am just transitioning from gschem to pcb for a robot controller board I am making. It spans several sheets, and has never successfully been exported by gsch2pcb. One of the error messages is "cannot find file "ROV_2010_analog.sch". This is one of the sheets in the overall motherboard, and is included in the project file. I even copied the file name and cut-n-pasted it into the project file to make sure that all the spelling and capitalization was correct. Then I did a text search through each schematic file and found only one occurrence of ROV_2010_ananlog.sch in any of the schematic files, and that was part of an 'input' symbol and was listed as 'source'. Do I need to have a source file name for every input and output symbol? Or is it not necessary if both schematics are read in at the same time as part of one project? If I have to add them to each input and output symbol, using gattrib won't help much because it does not create a column for data elements that are never called out in that schematic. Also, I clearly do not understand about the name:number convention on the net reference. Should I change the name for every type of signal, and only use numbers when I have a data bus or very similar signals? Or should I use one name for the entire sheet and number each output in sequence? If so, does the name have to be equal to the schematic's file name? I have not yet succeeded getting all the symbols translated to footprints, so I have not yet seen the results of the input/output pairs on the rats list to see if I got it to work or not. Any help getting that fixed BEFORE I start trying to move all the components and layout the traces would be greatly appreciated! Mike ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
