The Place artwork on checkboxes choose output targets. The Preview layer menu chooses which selected target you are viewing. These have different jobs: inspecting Back silk does not by itself mean Back silk will be generated.
Stable 1.4.1 supports multiple target layers in one artwork item. For a first label, keep only Front silk selected. Enable additional targets only when you intend to produce the corresponding geometry.
Layer meanings
- Front silk — KiCad layer:
F.SilkS; Practical implication: Printed front markings; may be clipped near mask openings - Back silk — KiCad layer:
B.SilkS; Practical implication: Printed bottom markings; verify reading direction from below - Front copper — KiCad layer:
F.Cu; Practical implication: Conductive front material; check nets, spacing, pads and zones - Back copper — KiCad layer:
B.Cu; Practical implication: Conductive bottom material; check electrical clearances and orientation - Front mask — KiCad layer:
F.Mask; Practical implication: Mask-opening geometry; understand how it exposes material underneath - Back mask — KiCad layer:
B.Mask; Practical implication: Bottom-side mask openings; inspect the complete stack-up
Mask artwork is not a coloured ink layer. Copper artwork is not merely decorative: it affects the conductive pattern. The same visual design can have very different electrical and manufacturing consequences on these layers.
Front, bottom and mirroring
Kobee's bottom-layer preview uses a front-view mirror. In KiCad's board view, you are often looking through the board at bottom geometry. In the 3D Viewer, flip the board and inspect the bottom from its real viewing side.
Do not manually mirror the content just because its front-view appearance looks reversed. First compare the preview, PCB Editor, 3D Viewer and exported bottom Gerber from the correct side. A second manual mirror can create the wrong manufactured result.
Minimum feature size
Check both positive material and negative gaps. A font's thin stroke, the opening in a letter, a symbol's internal hole and a QR module all need to survive the chosen process.
Use your fabricator's current published limits for the exact layer, finish and process. Software defaults and guarded minimums help prevent obvious mistakes; they do not promise that every board supplier can make the result. Preview zoom does not change physical size.
For small markings, simplify the artwork before shrinking it further. Choose a heavier face, remove fine detail, increase the symbol height or shorten the label.
Silkscreen near pads
Kobee's geometric clearances and KiCad's Gerber clipping options are separate. An unbroken overlay in PCB Editor may be clipped where the exported silk intersects solder-mask openings.
For a connector test, export once with Subtract soldermask from silkscreen disabled and once enabled. Compare the actual result around the pins and plug opening. Then use the production export settings consistently. Do not assume a screen render proves the final silkscreen will be unchanged.
Copper and connector openings
The header tool forces an opening for copper output to help avoid joining connector pins. Inspect it anyway. Verify all pin clearances, nearby tracks, zones and unrelated copper. Run KiCad's checks with the finished artwork present and inspect any artwork-related findings.
When combining copper and mask graphics, inspect their relative size and registration. A mask opening does not create copper underneath it; it only changes the mask pattern. Check the intended visual effect in the actual board stack-up.
Verify before ordering
- Save a named board revision with the artwork applied.
- Inspect the artwork at real dimensions and near every component envelope.
- Open the 3D Viewer. Inspect both sides, reading direction, part obstruction and the intended copper/mask effect.
- Export the final fabrication Gerbers using the settings you will submit.
- Open them in GerbView or the viewer used for your manufacturing review. Check front and bottom silk, copper and mask separately.
- Compare clipping, tiny holes, borders, connector openings and code modules to the board view.
- Run the relevant KiCad board checks. Resolve electrical consequences of conductive artwork.
- For QR/barcode artwork, scan the final manufactured sample before treating it as a reliable production marking.
Keep the Gerbers and a few clear screenshots with your board release. Record KiCad version, OS, Kobee version and export options so a later change can be compared meaningfully.
Optional command-line export
If you use KiCad CLI, an explicit six-layer export can help compare revisions:
1kicad-cli pcb export gerbers \2 --layers F.SilkS,B.SilkS,F.Cu,B.Cu,F.Mask,B.Mask \3 --output gerbers acceptance.kicad_pcb
Use the CLI installed with your KiCad version, and review its export options rather than assuming defaults match your normal production setup. The command creates output; visual inspection is still required.