I am using KiCad 5.0.1 on Ubuntu 18.04.1 LTS OS. I have a design that uses all THT parts. I used PCBLibraries Library Expert Pro 2018.08 (right now a free download) to produce all my land patterns/footprints. I placed all my parts on a PCB outline and did a DRC that came back with “Footprint has incorrect courtyard” for all of the footprints.
A typical message for any part was “ErrType(46): Footprint has incorrect courtyard (not a closed shape)”.
“• @ (128.000 mm, 131.000 mm): footprint “PTH1” has malformed courtyard”.
Additionally “kicad information/log message” stated:
“PTH1: Unable to find the next graphic segment with an endpoint of (128.35 mm, 131 mm). Edit graphics, making them contiguous polygons each.”
Viewing any of the courtyard outlines does not show any gaps, they seem to be complete and enclosed.
If you check the coordinates of the courtyard lines, what do you find? Is the endpoint of one line exactly the start or endpoint of the next?
Is there possibly a line of zero length there?
Is the courtyard possibly self intersecting?
I checked the “endpoint” of a couple of footprints as reported being a problem from the DRC. For instance “PTH1: Unable to find the next graphic segment with an endpoint of (128.35 mm, 131 mm).” That point has nothing to do with the courtyard outline. There is a circle and a vertical and horizontal line, a cross, that mark the center of the footprint. The endpoint given is the right hand end of the horizontal line.
–Larry
The courtyard layer is not allowed to have any graphical element on it besides the outline it self. So move the your center mark stuff to a different layer.
If i understood you incorrectly and these things are on a different layer already then check in the file it self with a text editor if there really is nothing there.
I checked the footprints by turning off all layers except the front courtyard (F.CrtYd) layer. When I turned off the F.CrtYd layer not only did the courtyard outline go away so did the centroid marker, so I knew that was the problem. I got back with PCB Libraries and they said, yes they put the centroid marker on the same layer as the courtyard because other layout programs have a limit of 32 layers (silly them). What I have to do is in their preferences I have to turn off the centroid circle and cross hairs. PCB Libraries said in their next version of Library Expert (2019) they will look into changing this functionality (at least for KiCad).
I can’t believe I am the first/only one to use PCB Libraries Library Expert Pro version (a free download that you have to register for). Perhaps the KiCad footprint developers should use this program as it will cut down on development time, as you enter the physical dimensions of the package and it automatically calculates the land pattern/footprint and 3D STEP model.
–Larry
You aren’t, but I use an old version that doesn’t support exporting KiCad footprints so I would manually copy the dimensions from the generated footprint’s “datasheet”. I haven’t used it in quite a while, and I thought the newer versions required membership/subscription fees. Maybe I was mistaken about that.
Do you mind sharing the product link for the library expert so I don’t have to bother googling it? (Yes, I’m being lazy.)
The PCB Libraries “Library Expert Pro” version is free but is limited. Go to <www.pcblibraries.com>, register, and download the LE Pro version [2018.08 at this time and they are working on a 2019 version], it includes KiCad. The “Library Expert Enterprise” version is the full up offering. Here is what I got when communicating with PCB Libraries:
The Free Library Expert Pro is limited –
No Batch Build
No Global Preferences
Cannot save Calculator Package Dimensions or FP Designer custom parts to FPX library
Why don’t you manually delete the centroid crosshairs [and circle] in your KiCad library for now. [–Yes, that is what I have done and will do.]
We have a very affordable option coming up in a couple of weeks. The full featured Library Expert Enterprise will be Free [–not so!] with free access to 1 million parts on POD and free access to the BOM Builder service. All you pay is the yearly maintenance fee of 20% of the list price for a yearly Lease with a new Cloud Based License.
The list price for LE Enterprise is $624 [–times 20 % is $124.80, and the list price, no doubt, would increase over time.] and the yearly maintenance is $149 a year.[–Ouch! that is still quite pricey for a hobbyist.]
–Larry
P.S. I forgot to mention that the PCB Libraries “Library Expert Pro” or “Library Expert Enterprise” programs only run on Windows, so you will have to make accommodations if you run Linux. Personally I have two SSDs, one on which I have Ubuntu 18.04.1 LTS OS, on which I have KiCad 5.0.1, and the other I have Windows 10. I simply use a USB flash drive to go between them.
–Larry
