Hi.
Here is my Version of KiCAD:
Application: KiCad
Version: (5.1.4)-1, release build
Libraries:
wxWidgets 3.0.4
libcurl/7.61.1 OpenSSL/1.1.1 (WinSSL) zlib/1.2.11 brotli/1.0.6 libidn2/2.0.5 libpsl/0.20.2 (+libidn2/2.0.5) nghttp2/1.34.0
Platform: Windows 8 (build 9200), 64-bit edition, 64 bit, Little endian, wxMSW
Build Info:
wxWidgets: 3.0.4 (wchar_t,wx containers,compatible with 2.8)
Boost: 1.68.0
OpenCASCADE Community Edition: 6.9.1
Curl: 7.61.1
Compiler: GCC 8.2.0 with C++ ABI 1013
At least the big coil footprint has bezier curves instead of straight lines. KiCad can read and even edit them, but apparently can’t plot them ATM. Bezier support is work in progress in the development version.
(EDIT: this would have been impossible to tell without the attached project files.)
Not really - if I understood correctly the support was missing altogether. Now KiCad supports them, but can’t plot them to gerber (the gerber format doesn’t have curves, they must be converted).
As a temporary workaround, until KiCAD would patch this behavior, you should export your DXF files after having exploded the curves to poly-lines (or just export your DXF in R12 format).
This would convert your DXF Bsplines to Poly-lines… then your footprint will be plotted correctly.
@wopo - if you want to use nightly builds for plotting, you should install the stable and unstable versions side by side, see Running several KiCad versions on the same Windows machine. It’s clumsy but works well after doing once. Installing a virtual machine/OS is another option. Rember to handle only a copy of the original project. Nightly builds may modify the project so that it’s not compatible with the stable version anymore.
I played arround with LibreCad to draw a footprint dxf-file. It worked well, because is has the option to store the file with the R12 modus. The Coreldraw IX version has other options except the R12. I will also try the nithly build version. Nevertheless thank you to all of you.
wopo.
I consider the 5.1.5rc1 builds to be almost release stable and usable for production. You could keep your Coreldraw symbols, just be careful sharing your PCB files until the official 5.1.5 release (this year I hope)
As davidsrsb said, they are stable (about as much as 5.1.x releases) and because the fix was added there, you have no reason to use unstable 5.99 nightly builds. Just update to the latest 5.1 testing build. The final 5.1.5 will be released within some weeks, you can then update to that soon. And remember that there’s still a chance to see some new bugs when plotting because the code is new.
I was surprised to see the fix in 5.1 at all, even more so before 5.1.5 release. But a development mailing list shows Wayne (the project leader) wasn’t completely happy about such changes creeping in between rc and final. Wopo, you were lucky to get this fixed so soon for the stable branch.
Something had to be done, a warning at least, as plotting Gerbers that don’t accurately match Pcbnew rendering is a very serious bug.
The whole purpose of KiCad is to generate these Gerber files.
Also note who did the patch, J.P. Charras himself.
