It’s the second time I wasted time and money due to a silly fact: I sent my Kicad pcb file to a board house and the resulting PCB had wrong filled areas.
(please note I’m aware for production it’s better to use Gerber files, but because often I need just a couple of prototypes I tried this way)
I discovered the board house does not update the filled areas so they kept the previous shape. Usually I set the visibility to outline only, in order to have a more clear view of the traces.
I understand I should remember to update the areas manually before send files to production, but I wonder two things:
why Kicad does not update the areas automatically at least when I save the file?
from your experience, it’s normal that the board houses do not do this when they open the file?
I mean, from my perspective an outdated filled area makes no sense at all. I understand when routing you may want to save some milliseconds to update the areas, but at least when you save the file what’s the point to leave a wrong area?
Thanks for your kindness. The question is why Kicad would save a wrong layout, given that it knows (better than me) that the areas are outdated - regardless the fact I sent the files to the board house.
regarding this, I would not want a board house to make any assumptions and changes to the files I send them, beyond those necessary for their CAM process.
I would use the “hole” left by a zone as a reference to draw the perfect® zone, it would be annoying if the program deleted my “reference” when I save the layout to prevent the loss of my work.
A zone refill is one of the most CPU intensive operations in KiCad. It does not matter much for small PCB’s, but on a complex PCB with many layers and zones this is very noticeable. I often save the PCB while working on it, for example before a big move operation that can possibly go wrong, so I can just exit KiCad and re-load the old PCB. Re-calculating those zones for nothing would be a waste of time for me.
Sending out your artwork for manufacturing is always a big step and has risks.
To minimize those risk, make a checklist, and follow that checklist before sending out your artwork.
I sent my Kicad pcb file to a board house and the resulting PCB had wrong filled areas.
Can this be interpreted as you sent the .kicad_pcb file directly to your board house? A few exist that take this file directly instead of the GERBER Files.
I mention this because there are a couple of UI which prompts the user to fill the zones
GERBER generation
DRC
While this is unfortunate, you really should not be packaging up anything without a final design check .
Saving KiCad files saves your progress. If you chose to unfill your zones, why should that choice not be saved? Unfilled zones is not a “wrong layout”, it’s a perfectly valid step along the way to a finished board. KiCad cannot know that you are about to send that board file off to a manufacturer.
I would not expect any manufacturer to make adjustments to a board file without confirming with me. However, I have worked with several board manufacturers that did flag strange things and ask if they were OK before proceeding to build the board. So, perhaps you could request that EuroCircuits flag boards they receive that have unfilled zones.
After all, in KiCad 5.99/6.0, just having the kicad_pcb file is not necessarily enough information to re-fill zones correctly: you could also need the project file (which contains the standard design rules) and custom design rules file, if they are used to control zone fill. So if you just send a kicad_pcb to the manufacturer, they can’t possibly refill zones and know they are doing so correctly – the only reasonable thing for them to do is to warn you that you have some unfilled zones, and ask if you want to proceed or to send a new file.
I don’t trust the CAD file exchange method as the detailed rendering does change between KiCad versions as bugs have been fixed, or even just down to changes in thermal relief spokes handling.
I don’t know if different OS might have subtle effects as well.
Once you have Gerber plots, many of the uncertainties are eliminated
There are various technical reasons for this, but basically our stance is that the board and schematic file formats should be viewable by themselves, but not necessarily editable with full functionality. Refilling zones is an editing operation. Putting the new design rules system outside the board file format allows for faster and easier development, which ultimately is an important thing to optimize for if we want to keep delivering the features people are asking for in KiCad.
We know this is not a perfect trade-off, but in my opinion it’s worth it.
Especially in the future when KiCad supports multiple boards per project and other things like that, I would encourage you to think about a KiCad project as a thing involving multiple files that work together. We already have some functionality to make that easier (the project archiver/backup feature) and in the future, certain features we plan to add will only add to the reason to consider a KiCad project as a sum of files (schematic sheets, board file, project file, etc).
In my case it would be not possible to do any design needing more than one day of work if KiCad would refuse to save wrong layout.
May be you have 24/7 working system so you can go from start to the end before saving your work.
to point 1: filling areas should be the very last step right before you triple-checked everything else and right before you produce the Gerbers. As mentioned, updating them automatically could have unwanted side-effects.
to point 2: yes, that’s normal. unless you got something obviously wrong, they’re not going to check some overlap of a zone with a via as they don’t know what your intentions are.
I’d consider that the board house not changing anything to be a good thing. I often tile small boards by copy/paste, once I made the mistake of updating the fill, the ground plane, and all the grounds became disconnected in the copies, resulting in three out of four boards have no ground connections. That time it was my fault, but if the board house had done the same, after me carefully not doing so, I would be very unhappy with the result. I always send gerbers though, after checking them.
Hi
I appreciate your frustration, although Kicad cannot be blamed for this as it is what you asked for, but if you can may I suggest you try and get the hang of exporting to gerbers, for several reasons.
1: Not all board houses accept board files.
2: Any program can introduce anomalies which will be masked
3: It is easier to spot any trace clearance errors (or cosmetic routing) that you may know about that you haven’t included in the constraints, as the layer colour is all one colour without highlights and any “anomolies” stand out very clearly.
Also while the Kicad gerber viewer is excellent, use a 3rd party viewer, eg Viewmate (which is free) as it will be a totally removed from any Kicad code - I do this with the very expensive PCB package I use as well, just for this reason.
