Front Panel as PCB

The Europi Front Panel is fabricated as a PCB with the following criteria:

• It is 1.6mm thick Aluminium substrate (this is actually cheaper than 2mm FR4)
• The text legend is ENIG plated Copper
• Solder Mask is Black

This gives quite a nice Gold lettering on Black Background appearance, though creating it is slightly awkward.

• The front panel is laid out in the normal way, with drill holes, legends etc. I used anchors on both the Front panel and the PCB so that I could then use relative co-ordinates to align the Holes with the underlying components.

Once I was happy with the appearance of the front panel, I did the following:

• plotted JUST the F.SilkS layer as an SVG file.
• imported this into GIMP using a very high resolution of 50px / mm. I then added a white background and cropped it to exactly the size of the front panel.
• Deleted everything apart from the text/graphics
• exported this Black-on-White image as a file called frontpanel_legend_F.Cu.bmp
• using KiCad's Image Converter, convert these into .kicad_mod files twice, to create frontpanel_legend_F.Cu.kicad_mod and frontpanel_legend_F.Mask.kicad_mod
• open the frontpanel_legend_F.Cu.kicad_mod using Notepad++ and search and replace every occurrence of F.SilkS to F.Cu
• open the frontpanel_legend_F.Mask.kicad_mod using Notepad++ and search and replace every occurrence of F.SilkS to F.Mask
• import these two .kicad_mod files as new footprints
• Add the footprints to the PCB taking care to align them with the original SilkScreen legend

I could then JUST create the following Fabrication Files:

• europi_main_frontpanel-NPTH.drl
• europi_main_frontpanel-Edge_Cuts.gbr
• europi_main_frontpanel-F.Cu.gbr
• europi_main_frontpanel-F.Mask.gbr

These can then be zipped into a single file to be sent to the fabrication house.

The settings at the fabrication house were

• 1 Layer
• Copper and Soldermask on top layer
• No Silkscreen
• 1.6mm Aluminium
• Black Soldermask
• No Silkscreen
• Immersion Gold (ENIG) 1u thick