On 07/07/2014 02:34 AM, jp charras wrote: > Le 07/07/2014 06:20, Dick Hollenbeck a écrit : >> I added back annotation to Eeschema directly from Cvpcb when they are both >> running under >> Kicad.exe. >> >> I could have done it row by row. Instead I did it as a group batch when you >> "save" under >> cvpcb, on the idea that if you were to abort cvpcb without saving, you would >> not want to >> affect your schematic. >> >> >> For the TODO list, I think we have a problem with the hierarchical format. >> Here is a >> takeout from a nested schematic, used six times in the hierarchy: >> >> $Comp >> L R R1 >> U 1 1 520135B0 >> P 5400 3350 >> AR Path="/5201406D/520135B0" Ref="R1" Part="1" >> AR Path="/52014588/520135B0" Ref="R2" Part="1" >> AR Path="/52014893/520135B0" Ref="R3" Part="1" >> AR Path="/520134DE/520135B0" Ref="R4" Part="1" >> AR Path="/52015233/520135B0" Ref="R5" Part="1" >> AR Path="/520155E6/520135B0" Ref="R6" Part="1" >> F 0 "R2" V 5500 3450 60 0000 L CNN >> F 1 "R" V 5300 3450 60 0000 L CNN >> F 2 "Discret:R6" H 5520 3450 60 0001 C CNN >> F 3 "" H 5400 3350 60 0001 C CNN >> 1 5400 3350 >> 0 -1 -1 0 >> $EndComp >> $Comp >> >> >> If CVPCB sets only R3, and not the others, then the back annotation does not >> stick. This >> is not new that I can tell, I believe it failed this way when doing back >> annotation with >> the *.cmp file also. The code between the two means is similar. >> >> I used an s-expression on the KIWAY express, and parsed it with the DOM >> s-expression >> parser in about 5 lines of code. >> >> See SCH_EDIT_FRAME::backAnnotateFootprints() >> >> Jean-Pierre, what do you think? >> >> >> Dick > > If fact, it is hard to fix this kind of issue, because this is not > really a bug, and it exists with .cmp files. > You are using a complex hierarchy, therefore the *same* schematic sheet > (and therefore the same data) is used 6 times. > > Cvpcb (and Pcbnew) are seeing a flattened schematic, because they are > using a netlist, which is always built from a flattened schematic > representation. > In this case, R1 to R6 are the same component in schematic (therefore > only one footprint field, one doc field ...) and 6 different reference > fields. > However there are 6 different components for Cvpcb, and you can set 6 > different footprints (and in Pcbnew, you also can have 6 different > footprints, for the same schematic component) > > In your example, R1 to R6 should have the same footprint, to be > compatible with a schematic backannotation. > > (If not, this is the last footprint name read in the back-annotate file > which is stored in schematic) > > This is not really a bug, but a limitation of complex hierarchies. > But is it really a limitation ? > When your are using complex hierarchies you are doing that because you > want your changes (schematic modification, change a component value, or > a footprint name ...) made only once but reproduced 6 times on your board. > > In other words: > * If you want to back-annotate a complex schematic: R1 to R6 should have > the same footprint. > * If you want to design a board: R1 to R6 can have different footprints. > > You can fix that "issue", only by creating constraints in CvPcb, for > instance do not accept different footprints for R1 to R6 (which have the > same time stamp), or displaying only one component ( for instance only > R1 ), but it is a unnecessary constraint for Pcbnew (although it is not > a really strong constraint). > > This is more a decision to take. >
Jean-Pierre, My poorly phrased, open ended question did not mean to put you on the defensive about Tim's hierarchical sheet design. (It has served adequately for a number of years. A modern approach will move the bindings into the site of instantiation and out of the thing being instantiated.) Since you did not comment on the patch, I will check it off my to do list for milestone B). When I wear my user's hat, it saves me a step, so obviously I like it. Dick _______________________________________________ Mailing list: https://launchpad.net/~kicad-developers Post to : kicad-developers@lists.launchpad.net Unsubscribe : https://launchpad.net/~kicad-developers More help : https://help.launchpad.net/ListHelp
