Missing lines in FSilk-Layer in Gerber-File

Hi.
When I create a gerber-File some of the FSilk-line disappear.
Please look at the file I uploaded.
Please help me.
Best regards, wopo

It’s pretty much impossible to say anything about the problem. We can only see that there is a problem. Those pictures aren’t enough.

  1. Give exact KiCad version information (always when asking a question) (Help->About->Copy version info).
  2. I can’t say how you generated the picture. I can’t even see if it’s really the silkscreen layer. Giving screenshots of running KiCad pcbnew and gerbview windows would be better.
  3. If there’s something wrong with the project or settings, the easiest way to find it could be to try the actual files. We could generated the gerbers ourselves from the beginning. Now we can send back and forth these messages with piecemeal information - or just download the project and find the reason of the problem. Sometimes screenshots are enough, sometimes the board file or the project in zip file is better.
1 Like

My guess: the detailed drawings are on some other layer than F.SilkS

Give that layer a very distinct unique colour in pcb_new. This should allow you to check if the drawings you miss are indeed on the F.SilkS layer. If yes then something strange is happening. if not then kicad behaves as expected and you will need to modify the footprints you use such that they appear on the silk layer

2 Likes

Some of the detail in the upper picture, eg the fuse holders and output transistors would not normally be drawn in a silk screen. Are you sure that you are not viewing a Fab layer?

2 Likes

What is also odd is that, assuming more then one layer, they are the exact same color.

Multiple layers can have the same colour assigned (both in kicad and also in most gerber viewers.)

1 Like

Is this a new user who believes that, in KiCAD, you assign features to a particular layer by changing their display color? That would be a reasonable assumption, but it is NOT the way KiCAD works.

@wopo, can you post again, and attach the footprint files for some of the components which do not show up in the silkscreen? The large power devices, the fuses, the heatsinks, and the wirewound inductor (or is that a helical antenna?) would be good choices. Because you are a new member on the Forum, it may be necessary to make several posts, with one file attached to each post. Like @davidsrsb suggested, there may be some confusion between the silkscreen layer and other layers. (The “fab”, “usr” and “eco” layers, for example, are mainly used to document the design for humans, not instruct a machine about how to fabricate the board.)

Dale

@dchisholm
Thanks for doing all that typing such that I did not have to. :wink:

@Rene_Poschl
I can only think of one reason, and it’s not a good one, for the average person to use the same color for more than one layer item.

1 Like

It looks like an audio power amplifier from several years ago, the coil is the output inductor and the power devices are the transistors with temperature compensation diodes in the same package.

If @wopo could post the footprint files for the transistor and coil, we should be able to figure out what is happening
I don’t think that these are not standard KiCad footprints

1 Like

Hi.
The Version of KiCAD is:
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

Build settings:
USE_WX_GRAPHICS_CONTEXT=OFF
USE_WX_OVERLAY=OFF
KICAD_SCRIPTING=ON
KICAD_SCRIPTING_MODULES=ON
KICAD_SCRIPTING_PYTHON3=OFF
KICAD_SCRIPTING_WXPYTHON=ON
KICAD_SCRIPTING_WXPYTHON_PHOENIX=OFF
KICAD_SCRIPTING_ACTION_MENU=ON
BUILD_GITHUB_PLUGIN=ON
KICAD_USE_OCE=ON
KICAD_USE_OCC=OFF
KICAD_SPICE=ON

Here are again the Screenshots:

Here is the zip-File of the Projekt:

Thank you.
Wolfgang

Can you just post a power transistor or the output inductor footprints here, I cannot access Dropbox

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

Build settings:
USE_WX_GRAPHICS_CONTEXT=OFF
USE_WX_OVERLAY=OFF
KICAD_SCRIPTING=ON
KICAD_SCRIPTING_MODULES=ON
KICAD_SCRIPTING_PYTHON3=OFF
KICAD_SCRIPTING_WXPYTHON=ON
KICAD_SCRIPTING_WXPYTHON_PHOENIX=OFF
KICAD_SCRIPTING_ACTION_MENU=ON
BUILD_GITHUB_PLUGIN=ON
KICAD_USE_OCE=ON
KICAD_USE_OCC=OFF
KICAD_SPICE=ON

Here the screenshots:


Here are the project-files and some used footprint-files:
https://www.dropbox.com/s/4sazi1l4va8gyj5/footprints.zip?dl=0
https://www.dropbox.com/s/bhqci2hr6wzuojc/Leach_3.zip?dl=0

Regards,
Wolfgang

1 Like

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.

image

(EDIT: this would have been impossible to tell without the attached project files.)

https://bugs.launchpad.net/kicad/+bug/1851360

Three years ago this was noticed.


The power transistor is also made up of fp_curve elements

A warning would be enough in the short term

@wopo where did these footprints come from?

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).

So when did Pcbnew start displaying the Bezier Curves?

I don’t know, but the screenshot above (editing a bezier curve) is taken with 5.1.5rc1. Previously I thought it was a pre-6.0 feature only.

@davudsrsb: I use Coreldraw IX to draw the footpints and export them as dxf-File.

1 Like

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.

2 Likes