Layers

Intended to be used within symbols to draw schematic sheet frames (graphics and texts). Usually not used directly within schematics, but mainly in symbols. No special treatment by LibrePCB.

General purpose layer for graphics and texts, e.g. to add some additional information to a schematic (like a formula, or a dawing of an external device). Not recommended (but possible) to be used within symbols. No special treatment by LibrePCB.

General purpose layer intended for comment annotations within schematics. Not recommended (but possible) to be used within symbols. No special treatment (yet) by LibrePCB.

General purpose layer for graphics and texts, e.g. to draw boxes around parts of a schematic and give them a title. Not recommended (but possible) to be used within symbols. No special treatment by LibrePCB.

Intended to draw outlines/content of symbols (e.g. a rectangle for an IC, or a thick line for a GND symbol). No special treatment by LibrePCB.

Used to define custom grab areas of symbols by drawing closed polygons or circles. These areas are not visible in the schematic editor, but the editor allows to grab symbols within these areas. Only available in the symbol editor, not in the schematic editor.

Intended for the {{NAME}} text of symbols. Not used directly within schematics, only in symbols. No special treatment by LibrePCB.

Intended for the {{VALUE}} text of symbols. Not used directly within schematics, only in symbols. No special treatment by LibrePCB.

Intended to be used within footprints to draw board sheet frames (graphics and texts). Usually not used directly within boards, but mainly in footprints. Ignored by the Gerber export, but usually contained when printing.

Mandatory layer where a single, closed board outline polygon (or circle) must be drawn. The line represents the board edge after manufacturing. It’s highly recommended to set its width to zero since it has no meaning. This layer will be exported to Gerber files and is usually contained when printing the board.

Any non-plated board cut-outs (millings) more complex than slotted holes must be drawn on this layer as polygons or circles. The line represents the board edge after manufacturing. It’s highly recommended to set its width to zero since it has no meaning. This layer will be exported to Gerber files (into the same file as the Board Outlines layer) and is usually contained when printing the board.

General purpose layer for graphics and texts, e.g. to add manual measurements (e.g. the PCB size) to the board. Not recommended (but possible) to be used within footprints. Ignored by the Gerber export, but might be contained when printing.

Intended to add alignment helper drawings to footprints, mainly just straight lines with zero width. For example in an edge-mounted device, the exact location of the board edge could be drawn on this layer as a help/reference for the board designer to correctly place the device in relation to the board edge. Ignored by the Gerber export, and usually not contained when printing.

General purpose layer for graphics and texts, e.g. to add some additional information or drawings to a board. Not recommended (but possible) to be used within footprints. Ignored by the Gerber export, but might be contained when printing.

General purpose layer intended for comment annotations within boards. Not recommended (but possible) to be used within footprints. Ignored by the Gerber export, but might be contained when printing.

General purpose layer for graphics and texts, e.g. to draw boxes around parts of a board and give them a title. Not recommended (but possible) to be used within footprints. Ignored by the Gerber export, but might be contained when printing.

Intended for the {{NAME}} text of footprints. Not used directly within boards, only in footprints. Usually printed on silkscreen (by the Gerber export), depending on the board setup configuration.

Intended for the {{VALUE}} text of footprints. Not used directly within boards, only in footprints. Might be printed on silkscreen (by the Gerber export), depending on the board setup configuration.

Intended for any drawings to appear on silkscreen, e.g. device placement/orientation lines, pin-1 dots and custom text. To be used within footprints or directly within boards. Typical line width is 0.2 mm, recommended minimum is 0.1 mm. Usually printed on silkscreen (by the Gerber export), depending on the board setup configuration.

Intended for drawings to represent devices in a nice way, including body outlines, leads and polarity/pin-1 markings. Basically as a 2D projection of the 3D model to somehow see the packages in 2D views, for example to export a nice looking assembly plan. Ignored by the Gerber export, but usually contained when printing.

Intended for footprints to draw the exact mechanical outlines of the device to be assembled. To be drawn with a zero-width polygon or circle. Used by the DRC to detect and warn about overlapping devices, or devices placed within the courtyard of another device. This DRC check doesn’t work if no package outline is drawn.

Intended for footprints to draw the courtyard (clearance) of the device to be assembled, typically just the package outlines with a small offset (e.g. 0.2 mm). To be drawn with a zero-width polygon or circle. Used by the DRC to detect and warn about devices placed within the courtyard of another device. This DRC check doesn’t work if no courtyard is drawn.

Used to define custom grab areas of footprints by drawing closed polygons or circles. These areas are not visible in the board editor, but the editor allows to grab devices within these areas. Only available in the footprint editor, not in the board editor.

Used to add solder resist openings, i.e. areas on the PCB where no solder resist shall be applied. So in contrast to most other layers, this layer has inverted polarity. Note that LibrePCB adds content on this layer automatically where necessary (pads, holes etc.), so manual usage of this layer is generally not needed. But it still allows to add custom solder resist openings. Any content on this layer is exported to the corresponding Gerber files.

Used to add stencil openings, i.e. areas on the PCB where solder paste is applied for reflow soldering of THT devices. Note that LibrePCB adds content on this layer automatically for SMT pads, so manual usage of this layer is generally not needed. But it still allows to add custom solder paste areas. Any content on this layer is exported to the corresponding Gerber files.

Should be pretty clear 🙂 Inner layers are numbered from top to bottom, i.e. Inner Copper 1 is just below Top Copper and on a 6-layer PCB Inner Copper 4 is just above Bottom Copper.