Re: gEDA-user: Renumber in PCB/Was/Is List
>you have to be a bit careful here. >you have R1, R2, R3 on your board which will get renumberd as >R2 -> R1 >R1 -> R3 >R3 -> R2 > So it seems like maybe what needs to happen is generate an internal > was/is list and then for each pin on a net apply the was/is change. Protel generates a unique hash, which is a long random string, that is used as an anchor point, while things are being renumbered. The first placed part will be assigned a hash, the seconds place part the next hash. Then no mater how things are renumbered you always know the first place part, tho I've never find a reason to care about that. This method keeps things from getting scrambled during the renumbering. ___ 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
Dan McMahill wrote:
Mike Hansen wrote:
Is there documentation anywhere on how to get started in developing
for PCB/gschem? I am well versed in Windows C++ development but would
need quite a bit of time to get up to speed on performing code work in
PCB.
as DJ mentioned, no real docs other than the pcb web site says how to
get sources from CVS and the file README.cvs talks about what you need
to build from CVS sources.
Here is a patch which gets most of the way there. Basic functionality
is there and works, the big comment at the top of the ActionRenumber()
function lists whats left to do.
I got a bit overly motivated last night and at lunch today. I have the
renumbering pretty much all working.
What I did is add an action, Renumber(), which if called with no
arguments it will prompt for a file name. If given a file name as an
argument it will use that file. The renumbering runs top to bottom,
left to right. In other words you'll get
R1 R2 R3
R4 R5 R6
R7 R8 R9
The output file has all the changes.
The loaded netlist is modified
Parts that have no name keep no name.
Elements which are locked or elements with locked names do not get
renumbered.
Renumbering starts with the first character which is one of [0-9] or ?.
What is not working is when you renumber and then try to undo, the
netlist modification is not undone. This will require modification of
the undo infrastructure to deal with netlist changes.
At this point I'd appreciate some feedback. Apply the attached patch to
current CVS sources and then from within PCB, press ":" (without the
quotes) to get the action entry and then "Renumber()" (again with no
quotes).
I'm sure there is room for some more efficient algorithms as there are a
couple of pretty brute force searches and list insertions. Also, the
screen redraws after each element is renumbered. Doh!
-Dan
Index: src/action.c
===
RCS file: /cvsroot/pcb/pcb/src/action.c,v
retrieving revision 1.89
diff -u -2 -r1.89 action.c
--- src/action.c15 Aug 2006 02:50:42 - 1.89
+++ src/action.c16 Aug 2006 22:07:49 -
@@ -3115,4 +3115,317 @@
/* ---
*/
+static const char renumber_syntax[] =
+"Renumber()\n"
+"Renumber(filename)";
+
+static const char renumber_help[] =
+"Renumber all elements.";
+
+/* %start-doc actions Renumber
+
+%end-doc */
+
+/* FIXME
+ - add option for renumbering direction (top to bottom, left to right
+ is what I coded up). Numbering happens on a "row by row" basis.
+
+ - What to do about elements with no name? Right now they are
+ignored. Maybe they should get names like I1, I2 (for Instance)
+
+ - need to be able to undo the mods to the netlist. This will take
+adding infrastructure to the undo system
+
+
+*/
+static int
+ActionRenumber (int argc, char **argv, int x, int y)
+{
+ Boolean changed = False;
+ ElementTypePtr *element_list;
+ ElementTypePtr *locked_element_list;
+ unsigned int i, j, k, cnt, lock_cnt;
+ unsigned int tmpi;
+ size_t sz;
+ char *tmps;
+ char *name;
+ FILE *out;
+ size_t cnt_list_sz = 100;
+ struct _cnt_list {char *name; unsigned int cnt;} *cnt_list;
+ char **was, **is, *pin;
+ unsigned int c_cnt = 0;
+ int unique, ok;
+
+ if (argc < 1)
+name = gui->prompt_for ("Renumber annotation file:", 0);
+ else
+name = argv[0];
+
+ if ((out = fopen (name, "r")))
+{
+ fclose (out);
+ if (! gui->
+ confirm_dialog (_("File exists! Ok to overwrite?"), 0))
+ return 0;
+}
+ if ((out = fopen (name, "w")) == NULL)
+{
+ Message ("Could not open %s\n", name);
+ return 1;
+}
+
+ fprintf (out, "*COMMENT* PCB Annotation File\n");
+ fprintf (out, "*VERSION* 20060814\n");
+
+ /*
+ * Make a first pass through all of the elements and sort them out
+ * by location on the board. While here we also collect a list of
+ * locked elements.
+ *
+ * We'll actually renumber things in the 2nd pass.
+ */
+ element_list = calloc (PCB->Data->ElementN, sizeof (ElementTypePtr));
+ locked_element_list = calloc (PCB->Data->ElementN, sizeof (ElementTypePtr));
+ was = calloc (PCB->Data->ElementN, sizeof (char *));
+ is = calloc (PCB->Data->ElementN, sizeof (char *));
+ if (element_list == NULL || locked_element_list == NULL || was == NULL || is
== NULL)
+{
+ fprintf (stderr, "calloc() failed in %s\n", __FUNCTION__);
+ exit (1);
+}
+
+
+ cnt = 0;
+ lock_cnt = 0;
+ ELEMENT_LOOP (PCB->Data);
+ {
+if (TEST_FLAG (LOCKFLAG, element->Name) || TEST_FLAG (LOCKFLAG, element))
+ {
+ /*
+* add to the list of locked elements which we won't try to
+* renumber and whose reference designators are now reserved.
+*/
+ fprintf (out, "*WARN* Element \"%s\" at (%d,%d) is locked and will not
be renumbered.\n",
+UNKNOW
Re: gEDA-user: Renumber in PCB/Was/Is List
DJ Delorie wrote: 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. you have to be a bit careful here. you have R1, R2, R3 on your board which will get renumberd as R2 -> R1 R1 -> R3 R3 -> R2 if you work this out ahead of time, you can just iterate through the elements and change the names. But if the individual name changes update the netlist, you might go from an original netlist of net0 R1-1 net1 R1-2 R2-1 net2 R2-2 R3-1 net3 R3-2 and after the R2->R1 change: net0 R1-1 net1 R1-2 R1-1 net2 R1-2 R3-1 net3 R3-2 you see the problem already. R1-1 is now part of 2 nets. So it seems like maybe what needs to happen is generate an internal was/is list and then for each pin on a net apply the was/is change. I've done a sort of proof of concept patch for this but it is ugly and needs to be refactored a bit before it could be added. -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
Bob Paddock wrote: On Tuesday 15 August 2006 21:58, Dan McMahill wrote: 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. It is my preference that the designators do retain schematic page reference. I do projects with lots of parts, but only can print out Letter sized schematic pages. Makes the board a lot easier to stuff, and less clutter on the bench, if you only have to deal with one page at a time. That option should be configurable. 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 In my many years at a contract manufacture it has always been one of those two, I have never seen the others you listed, unless it was completely random; those sucked to work on. then perhaps in the KISS spirit (keep is simple, stupid) these should be the only 2 to support. Someone else suggested sorting by distance from the upper left corner but this seems like it could be a bit confusing in the end. -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
On Tuesday 15 August 2006 21:58, Dan McMahill wrote: > 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. It is my preference that the designators do retain schematic page reference. I do projects with lots of parts, but only can print out Letter sized schematic pages. Makes the board a lot easier to stuff, and less clutter on the bench, if you only have to deal with one page at a time. That option should be configurable. >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 In my many years at a contract manufacture it has always been one of those two, I have never seen the others you listed, unless it was completely random; those sucked to work on. -- http://www.softwaresafety.net/ http://www.designer-iii.com/ http://www.unusualresearch.com/ ___ 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
It should work like the renumber in gschem, the first digit is maintained as normally R is for resistor, C for capacitor, and so on. From: Dan McMahill <[EMAIL PROTECTED]> Reply-To: gEDA user mailing list To: gEDA user mailing list Subject: Re: gEDA-user: Renumber in PCB/Was/Is List Date: Tue, 15 Aug 2006 21:58:57 -0400 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 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 ___ 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 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
Re: gEDA-user: Renumber in PCB/Was/Is List
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. 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. From: DJ Delorie <[EMAIL PROTECTED]> Reply-To: gEDA user mailing list 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
Re: gEDA-user: Renumber in PCB/Was/Is List
I was thinking something like this: -find the part that is closest to the upper left(use the hypoteneuse of the X,Y coordinates). This is our anchor part. Or we could allow users to specify which corner to start at. -iterate over the list of parts finding the next one closest via hypoteneuse from X,Y to X,Y. Basically the part renumbering would spread out from one corner having the lowest numbers to the opposite corner having the highest numbers. From: Dan McMahill <[EMAIL PROTECTED]> Reply-To: gEDA user mailing list To: gEDA user mailing list Subject: Re: gEDA-user: Renumber in PCB/Was/Is List Date: Tue, 15 Aug 2006 18:28:51 -0400 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 ___ 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
Sure there is... to make a maximum test of the shorted nets drc. On Tue, 2006-08-15 at 18:42 -0400, DJ Delorie wrote: > > 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
Re: gEDA-user: Renumber in PCB/Was/Is List
> 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
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: Renumber in PCB/Was/Is List
> 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? ___ 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: 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. While thats one valid method, please don't enforce it. I prefer to be able to find R101 near R102 on the board, and use text search in xpdf when I have to locate r101 on the schematic. john ___ 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:
Is there documentation anywhere on how to get started in developing for
PCB/gschem? I am well versed in Windows C++ development but would need
quite a bit of time to get up to speed on performing code work in PCB.
as DJ mentioned, no real docs other than the pcb web site says how to
get sources from CVS and the file README.cvs talks about what you need
to build from CVS sources.
Here is a patch which gets most of the way there. Basic functionality
is there and works, the big comment at the top of the ActionRenumber()
function lists whats left to do.
-Dan
Index: action.c
===
RCS file: /cvsroot/pcb/pcb/src/action.c,v
retrieving revision 1.89
diff -u -2 -r1.89 action.c
--- action.c15 Aug 2006 02:50:42 - 1.89
+++ action.c15 Aug 2006 19:19:58 -
@@ -3115,4 +3115,201 @@
/* ---
*/
+static const char renumber_syntax[] =
+"Renumber()";
+
+static const char renumber_help[] =
+"Renumber all elements.";
+
+/* %start-doc actions Renumber
+
+%end-doc */
+
+/* FIXME
+ - how to specify the file name? Probably have a option to get one
+ from calling the action directly like Renumber(logfile) and if not
+ specified have the gui prompt for a file name.
+
+ - add option for renumbering direction (top to bottom, left to right
+ is what I coded up). Numbering happens on a "row by row" basis.
+
+ - add an option to keep or override locked elements. I have mixed
+ feelings here. Do we really ever care about keeping the names on
+ some? But then again, locked is locked right?
+
+ - What to do about elements with no name? Right now they are
+ignored. Maybe they should get names like I1, I2 (for Instance)
+
+ - need to redo the loaded netlist so you can renumber and then hit
+'o' on a complete layout and have it still show correct connectivity.
+
+ - finalize the file format. I'd vote for something like
+
+command data
+
+where to start with you'd have something like command =
+{*COMMENT*, *RENAME*, *WARN*}
+
+and data is whatever the particular command needs. So for
+renames,
+
+*RENAME* "old" "new"
+
+Do we need any rules for quoting here? This file format is
+simple, similar to the PADS ECO file format, and extensible if we
+state early on that unrecognized commands should just be ignored
+(perhaps with a warning) by any tools which use this file.
+
+*/
+static int
+ActionRenumber (int argc, char **argv, int x, int y)
+{
+ Boolean changed = False;
+ ElementTypePtr *element_list;
+ unsigned int i, j, cnt;
+ unsigned int tmpi;
+ size_t sz;
+ char *tmps;
+ struct _cnt_list {char *name; unsigned int cnt;} *cnt_list;
+
+ /*
+ * Make a first pass through all of the elements and sort them out
+ * by location on the board.
+ *
+ * We'll actually renumber things in the 2nd pass.
+ */
+
+ printf ("Allocate memory for %d elements\n", PCB->Data->ElementN);
+ element_list = calloc( PCB->Data->ElementN, sizeof (ElementTypePtr));
+ if ( element_list == NULL )
+{
+ fprintf (stderr, "calloc() failed in %s\n", __FUNCTION__);
+ exit (1);
+}
+
+
+ cnt = 0;
+ ELEMENT_LOOP (PCB->Data);
+ {
+cnt++;
+/*
+ printf("Pass#1: Element name \"%s\" is at %d, %d\n",
+ UNKNOWN (NAMEONPCB_NAME (element)),
+ element->MarkX, element->MarkY);
+*/
+/* search for correct position in the list */
+i = 0;
+while (element_list[i] && element->MarkY > element_list[i]->MarkY )
+ i++;
+
+/*
+ printf ("Index (from Y position is %d\n", i);
+*/
+
+/*
+ * We have found the position where we have the first element that
+ * has the same Y value or a lower Y value. Now move forward if
+ * needed through the X values
+ */
+while (element_list[i]
+ && element->MarkY == element_list[i]->MarkY
+ && element->MarkX > element_list[i]->MarkX)
+ i++;
+
+/*
+ printf ("Index (from X position is %d\n", i);
+*/
+for (j = cnt-1; j > i ; j--)
+ {
+ element_list[j] = element_list[j - 1];
+ }
+element_list[i] = element;
+ }
+ END_LOOP;
+
+ /*
+ * Now that the elements are sorted by board position, we go through
+ * and renumber them.
+ */
+ /* FIXME -- need to grow the list dynamically, this line is LAME */
+ cnt_list = calloc (100, sizeof (struct _cnt_list));
+ for (i = 0; i < cnt; i++)
+{
+ printf("Pass#2: Element name \"%s\" is at %d, %d\n",
+ UNKNOWN (NAMEONPCB_NAME (element_list[i])),
+ element_list[i]->MarkX, element_list[i]->MarkY);
+
+ /* If there is no refdes, maybe just spit out a warning */
+ if (NAMEONPCB_NAME (element_list[i]))
+ {
+ /* figure out the prefix */
+ tmps = strdup (NAMEONPCB_NAME (element_list[i]));
+ j = 0;
+ while (tmps[j] &&
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
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
> 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
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
> 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
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 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
> 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
> 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
DJ Delorie wrote: 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. You probably need to update the loaded netlist too. Also you may need to turn off the 'unique name' and (maybe) the 'locked element' checks. If you don't turn off the locked element checks you'll have to deal with that too. If I get overly motivated tonight I'll send at least a partial patch. -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
Is there documentation anywhere on how to get started in developing for PCB/gschem? I am well versed in Windows C++ development but would need quite a bit of time to get up to speed on performing code work in PCB. From: DJ Delorie <[EMAIL PROTECTED]> Reply-To: gEDA user mailing list To: geda-user@moria.seul.org Subject: Re: gEDA-user: Renumber in PCB/Was/Is List Date: Tue, 15 Aug 2006 11:33:12 -0400 It doesn't, but it's the kind of thing that's easily added, say, as a beginner's project (hint). ___ 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
It doesn't, but it's the kind of thing that's easily added, say, as a beginner's project (hint). ___ 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
