I designed a board for a client with V6.0.5; he built it and it worked on the first try. It was done as he requested - all through hole and a particular form factor he wanted. But I have done similar boards, and with some free time, I decided to re-do this one in a different form with all SMT.
One way would be to run the Footprint Assignment Tool; perhaps that’s what I should have done. But I used SaveAs to copy the existing board, and used Edit>Change footprints in the new project in Pcbnew. I deleted all the existing tracks and started replacing the footprints. It was mostly passives and a bunch of relays with the same pinouts as the TH parts. So far, so good. All the links between the sch and pcb remained. But there was a diode matrix consisting of 40 diodes; I wanted to use a diode array package.
I created a new symbol and footprint, and added it to the sch. I then invoked the Footprint Assignment Tool to link the two, and got the message that I need to fully annotate the schematic. It is fully annotated. I ran it anyway to see what would happen. It had a large number of errors and didn’t add my new part. I assumed it was because the footprints on the board were different than what they were originally supposed to be, but it wouldn’t let me open the tool to update it after the annotation message. I tried a couple of times without saving, but each time it asked me if I wanted to save it, so at one point I did - probably my fatal mistake.
So I deleted my new diode array symbols, and all the original links (ratsnests) returned. But now I have, in addition to the Root, I have 2 more pages to the schematic - labeled 2 and 3, plus 2 identical pages called Page #. If I go to the original board, everything works but I still have those 2 extra schematic pages. If I go to the new project, the root schematic appears, but if I try to open either page, they disappear. There are now no links back to the schematic from the new version of the board, but the original ratsnests remain.
One cryptic error message I received:
A duplicate library name that references a different library exists in the current library table. This conflict cannot be resolved and may result in broken symbol library references.
Do you wish to continue?
No idea what that means. I’ve tried to explain it correctly but I probably left something out. Now what? I still need to add the diode array component along with a similar transistor array package.
Did you try to update the schematic from the PCB after changing footprints?
Maybe if autosave was enabled you will save some of your time recovering (a situation like this shows one of the great great benefits of version control software).
Edit: Depending on the components, not all THT packages share the same symbol with their SMD equivalents, a better way dealing with this IMO would be to update the schematic and edit symbols’ footprints there, then update the PCB from schematic as usual.
Edit2: I can’t think of something regarding the added sheets and the error message ATM but this might be a bug.
Looking at this issue again. My original schematics are fine. The original pcb is fine. The links all work. But that project is done.
But somehow, with all the different things I’ve tried, the Navigator shows:
Root (page 1)
RF_Section.sch (page 2)
Selection_Matrix.sch (page 3)
RF_Section.sch (page #)
RF_Section.sch (page #)
RF_Section.sch (page #)
Selection_Matrix.sch (page #)
Selection_Matrix.sch (page #)
Selection_Matrix.sch (page #)
And there seems to be no way to delete those extra files.
Unfortunately, I did not document my experiments from then on. My bad. My 76 year old neurons tend to lose a few bits occasionally. I saved the original board using Save Copy As, which automatically creates a new project. But eeschema does not give me the same option to Save Copy As. I just tried this again and I now have a copy of my existing board saved under a new name, which also created a new project.
I made several tries to copy the schematic to the new project. I was successful but have been completely unable to reestablish the links.
I have wasted far too much time on this, and it was just an experiment; not a real project. At this point I may finish it without a schematic by manually placing the footprints for the new parts. But there must be a way to do this properly; I just haven’t found it.
Hi Paulvdh
I just tried that route. Saved the entire project to a new directory. All seems to be functioning properly. Next, I tried to open the Footprint Assignment Tool. It opens with the header that “Assigning footprints requires a fully annotated schematic”. Of course, it is fully annotated. So I tried to run it anyway, and immediately discovered what the problem is - but I have no idea how to get rid of it. Turns out the schematic Navigator still contains all the extra copies labeled (page #) discussed in my previous email. The annotater sees duplicates of all the components, which then appear as errors - in my case, 668 errors. I cannot see any way to delete these extra copies, and until I find a way, I cannot go any further. Any ideas?
I just did a Save As from KiCad’s project manager on a simple hierarchical schematic and it just worked as expected. No annotation problems and Schematic Editor / Tools / Assign Footprints also only sees the two connectors in the project. Therefore I guess that the “Save As” did not save your ass, but copied the error from the old to the new project.
Can you zip the project (or a section of it) and upload it? Then I can have a look at it and attempt a repair.
You have two instances of the Selection Matrix sheet drawn exactly on top of each other, and in one of them all the diodes are not annotated.
Apart from that your routing on the PCB looks quite bad. It looks like some HF channel switching thing (at what frequency?) but it does not look like any attempt is made at a proper GND plane or controllling impedances. No output buffer capacitor on the MC7805 (I think it needs one but have not checked) and neither a decoupling capacitor for the 74HC137. Also Metal can transistors? But it’s your project.
(Edit: Note I did not fully read your attached Read_Me.txt which mentioned the 8 part diode array).
For the SMT conversion, have a look at the BAT54. It’s a very common and cheap dual diode in SOT-23, and there are multiple versions of it. common anode, common cathode and series. Instead of the metal can transistors, you can use some P-channel MOSfets which do not need a series resistor at all, or you can use PNP transistors with built in resistors. These are also quite common in SOT-23 but I don’t know type numbers out of my hat.
I prefer to work with SMT parts a lot above those old fashioned wired things.
No need to turn the PCB for soldering.
No disorientation and re-orienting because of that turning (all those mirror images were driving me mad)
No need to cut leads to size.
Easier to replace parts if rework or repair is needed (especially with 2 soldering irons).
