I’m asking a further question in relation to my other thread on Git-less Revision tracking …
Q; from the software’s point of view what difference does it make if I open the .pro file first and within that open up the schematic or layout editors versus opening them directly by double-clicking on them (stand-alone mode editing) ?
I guess what’s confusing me about Kicad is the following: it seems to me that a project folder is “by name” intended to be used for the entirety of the project (not how some of us use it, granted) which seems to imply that it could have all revisions of the pcb saved as re-named copies withing the project folder - same with schematics. My understanding is that stand-alone mode (ie., not going thru .pro file) was meant mainly for achieving such a directory structure. yes/no ?? if not, then what is the purpose of having multiple pcb/schem files in the project folder other than having archival material used for “viewing” only ??!
So, to be real clear:
(i) what is the intended purpose of stand-alone (editing) mode ?!
(ii) what does the program do otherwise when going through the .pro file ?!
When you open a PCB in standalone, there is an extra menu in file that allow you to append another pcb in the current file.
It’s useful for panelization, or to get some stuff from one PCB to another.
In the schema in V5 it was the only way to copy paste between 2 schematic file, but now in V6 the copy paste works between project, so that is less needed.
I don’t know, but according to what I suppose.
A conception of having all included in project was introduced. Opening PCB - means opening PCB of that project. So being in project there is no way of opening files from other ones.
But people need sometimes to copy something from another project. So opening in stand alone was something like way around.
I was using for many years a Protel 3 (program from 1997). There were no conception of project so may be at KiCad V1 there also were no project (I don’t know) and programs were working by definition in stand alone mode. Than later project was introduced and we are now at this stage. When being in project everything will be possible than may be stand alone will go away.
As far as I know, standalone mode and being able to have multiple projects in a directory are not connected. As explained standalone mode enables additional behaviour.
You can have multiple .pro files in a directory and if you open one it will go use the corresponding schematic and board files that are linked by the basename. That’s how those multiple versions in a directory schemes work.
I am still in V5.1.12. There are fp-info-cache file having name not derived from project name. Having many .pro files in one directory ends with having that file only for last opened project.
I think that problem is gone in V6.
I often delete the fp-info-cache file with no ill-effect as it’s always regenerated as needed. It could be that if you add some footprints to your library, then you open another project it might not find a needed in the cache depending on the freshness of the cache. But I only did a quick test, as this is not the way I version my projects anyway.
“Standalone mode” seems to me like a workaround for data integrity protection.
Workflow in “project” mode is designed to be integrity-safe by design. All “data integrity risky” operations are disallowed.
In “standalone mode” all the operations are enabled, but some of them might be risky for maintaining data integrity. So it’s kind of “i know what I’m doing” mode.
Probably these operation could be implemented for default workflow, but proper design of additional data integrity checking would require addditional work.
I delete them always, but I was told here several times that I shouldn’t do that. I just assume that for someone it could be a problem if his projects are fighting for the rights to this file and because of it he shouldn’t have many .pro files in one directory.
Part of very important data is saved in kicad_pro file, like text variables and many settings for pcb, like soldermask clearance, predefined track sizes, custom rules. You should not modify neither schematics, nor pcb file in standalone mode in case these files are derived from project. For example: open pcb file in standalone pcb, go to File → Board setup → see yellow warning on top, stating that “Project missing or readonly, some settings will not be editable”.
In case you will try to export gerbers from standalone pcb, expect to get faulty gerbers, without proper soldermask clearances…
This makes kicad project files not portable, and I don’t like this behavior. I would like yo have completely portable pcb file, where zone revuild works, and correct gerbers exported from standalone mode.
I use standalone programs for quick board/schematic view and for quick setup of new projects: launching pcbnew or eeschema, clicking save, which creates project file in destination directory is faster for me than running kicaad itself and going throu file new project blah blah. Just close eeschema and double click on project file just created
The current stance of the developers is that a pcb file should be viewable but not (necessarily) editable without a project. There are other concerns than just having only one file.
I think nobody mentioned non-kicad imports yet. For some file formats schematic import and/or pcb import has been implemented but not project import. In those cases the corresponding standalone program must be opened to activate the import option. This is logical but IMO should be solved in some other way.
I think the developers have been willing to get rid of the standalone mode.
My first thought was that settings should be saved as low in hierarchy as possible so PCB settings in PCB file. But I remember here people asking how at schematic set a PCB parameters so may be it is the reason to have these in project file.
Yes, one important example is net classes. In v6 they can be used from Schematic Setup or Board Setup. They don’t belong to only one of them and are stored in the .kicad_pro file. If you share a board file you don’t have access to net class data, so it’s impossible to edit the layout.
It is also possible to create a board with no matching schematic, although this workflow has some limitations and is not recommended for most users. To do this, you must start the PCB editor standalone (not from the KiCad project manager). Before beginning your design, it is a good idea to save the board file, which will also create a project file to store board settings. Use “Save As…” from the File menu to choose where to save your board file. A project file with the same name will be created in the same location you choose to save the board file in."
at the moment i’m flying through a design and really digging the experience
thank-you all
