I installed the last 7.0 version but I get many warnings under the schematic and pcb editors.
My projects were edited using 6.0.10 and loaded without those warnings.
I checked the path of my custom libraries folder (mod files). I only find that the main path used ‘\’. After reloading the folder, the path used ‘/’ although the three paths in the Path Substitutions still used ‘\’.
Under the schematic editor, I get too many warnings in the ERC window. For example, each instance of the most classic GND and VCC symbols generates a warning saying “has been modified in the library ‘power’”. Why can’t these be automatically updated using the new version ? Will large schematics require so many manual changes ?
Under PCBNew, I get a big number of warnings, most of which concern footprints which “do not match copy in library XXXX”. Can’t understand what this means, as this also concerns my imported footprints as well as those I edited (only saved locally for the project). I also get some other warnings like “text height out of range” although the text was perfectly printed on the pcbs manufactured (using 6.0.9 files).
So… Did I miss something ? Else, I’ll switch back to 6.0.10 until I can load my projects without trouble under the next 7.0 .
Did you save the project in version 7 after opening?
It’s the nature of development. If you don’t like new features you have to use the old version.
All these warnings (ERC + DRC) are newly added ERC / DRC checks. So it’s quite normal that v6.0.x didn’t show these errors - v6 simply did not have so many checks.
As always in life you have different choices:
- just ignore these errors/warnings. The ERC/DRC is only a help, you should understand what it tries to tell you. If the board was fine prior to update - it could be quite safe to ignore them
- disable all new ERC/DRC checks. The schematic setup / board setup allows to individually enable/disable checks, so you could mimic the old v6 behaviour.
- correct the warnings in schematic/board if you want clean ERC/DRC results
warning "text height out of range”
as said: new DRC-check. If you are fine with your text-size: adjust the corresponding value in Board setup–>Design Rules–>Constraint–>Silkscreen: minimum text height
“symbol has been modified in library”
“footprints do not match copy in library XXXX”
Can’t understand what this means…
You need a little imagination, what could this be? The symbol/footprint in the project doesn’t exactly represent the version in the library. There are two possible reasons:
- library-item has changed (error corrected in library, nicer drawn symbol, whatever)
- item in the project was modified (through dialog “edit symbol/footprint” - pad sizes/holes changed or such things)
At least there is difference - so you have to decide: is the difference on purpose or has the library developed? You can update your symbol/footprint in the board, but it’s up to you.
GND and VCC symbols generates a warning saying “has been modified in the library ‘power’”. Why can’t these be automatically updated using the new version ?
Automatic update? Please no.
Will large schematics require so many manual changes ?
If you want the updated symbols: run the “update symbols” command one time - not that much work.
Indeed. “updates” always have potential to break things and should never ever be done automatic. I still have a memory of a funeral of a sister in law, and halfway during a presentation with a beamer a message popped up that windoze had to reboot itself because it updated a printer driver. It’s one of the reasons I switched to Linux. It has many flaws but at least it does not annoy it’s users with stupid things.
And KiCad has quite capable tools for updating library symbols, or choose one of the other options mf_ibfeew mentioned.
Yet another option is to export the schematic symbols used in the project to a project specific library (Wit: Schematic Editor / File / Export / Symbols to New Library, and then point to that. This also makes the project fully independent of any external KiCad library.
I didn’t installed V7 yet. I don’t understand what that warning says. I use only my own libraries (power library also). 'Has been modified in the library ‘power’" I understand that KiCad finds that library was modified (by comparing with … what?.. previous version). But if it will have only my Power library and no standard libraries available will I get this warning also?
Kicad stores symbol+footprint inside schematic+board-files.
- during the schematic/board development Kicad allows the user to modify every single of these stored symbols/footprints independently from the library (through the Edit symbol/footprint command).
- Additionally the symbol+footprint in the library can be developed (corrected/modified/…) during time
All the mentioned ERC/DRC test does is to check: Are the current saved symbol/footprint in the project exactly == the current version in the library? If not equal → display warning
Kicad currently can’t check which of the two possibilities are the reason for the difference, all the report says: there is a difference, you may look at that.
It’s up to the user to decide: OK, update from library or not. If the symbol/footprint was deliberately modified in the project one should not update → as this process would overwrite the changes with the original version from the library. (main reason why I try to avoid the library-independent modifications).
If this check is tooo confusing: just disable it. Not every ERC/DRC check is for everyone (I also have some checks disabled).
Clear. I just didn’t imagined that someone have changed power symbols after adding them do schematic or that those basic symbols were changed in library. I don’t know at what moment (if V7 is that moment) when placing power symbol and changing its name will be enough to define the other power net (at that moment I expect - may be power symbols will be changed in library).
Whenever I modify anything in footprint library I do update for all footprints as I not modify them at pcb. But recently I modified at PCB 16 SO8 footprints (double Inteli-FET) to have solid connection to zone. Than because of some other modification (to allow solder mask between raster 0.5mm pads) I did update all and was surprised. I will probably have separate SO8 only from that reason.
Thanks for your explanations.
Updating the symbols all at once in the schematic editor was indeed trivial !
As for the footptints, I updated them. However I still got the “does not match copy in XXXX” warnings after customizing several pads, which required ignoring those warnings in the ERC. Why can’t we do so from the Pad Properties window for each pad customized ?
If I got into need of changing pads I define new footprint.
However I still got the “does not match copy in XXXX” warnings after customizing several pads
This is the goal of this check. If you regularly do footprint-modifications on board-level than this check might not be suitable for you - it will deliver too many “false positive” warnings for your workflow. Disable this check and you are fine.
After each symbol saved, a warning appears in the project library that the file directory was not found but the symbol is saved… How do I disable this warning?
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.