Required Layers

Top / Bottom

These layers indicate where copper will appear on your board.

Using the Polygons tool on the copper layers will generate a “copper pour”, which can dramatically simplify connecting your board. For more details on ground planes in Eagle, see our Using copper pours page.

Pads

This layer indicates the copper ring around a through-hole pad. Unlike the Top or Bottom layers, Pads will generate a copper on both sides of your PCB.

It’s generated automatically when using a footprint that has a through-hole component. It’s very rare that you’ll need to manually add an object to this layer manually.

Vias

Similar to Pads, this layer indicates the copper ring around a drill hit. It’s generated automatically when using the Via tool.

The difference between the Vias and Pads layers is largely irrelevant, but can be helpful on occasions when you need to visualize to see only one type of drill hit.

Dimension

This layer has several special purposes in Eagle, as well as for our service.

Primarily, this layer serves to indicate the edge of your board.

The Dimension layer also serves an important role for Eagle’s DRC checking of copper pours. Eagle will automatically enforce the Edge Keep Out DRC rule, and push copper pours away from any line on the Dimension layer.

Since Eagle expects the board edge on this layer, our service uses the Dimension layer to generate a board outline gerber. Our fab will then use that layer to cut your board out from the fabrication panel.

tStop / bStop

These layers indicate spots where the fab should avoid putting the purple solder resist. This is generally used to let you access the copper for soldering.

In most cases, this layer is generated automatically by the Pad and Via tools, as well as for any component footprints that use them. However, you can also draw on these layers to create pads, heat sinks, or other structures.

It’s also common to create gold artwork on PCBs by using the Stop layers to expose the copper. Just make sure to add the copper too, otherwise you’ll simply expose the board substrate.

Silkscreen Layers

These layers are technically optional, but play very important roles in documenting your board for easy assembly. Eagle breaks the Silkscreen into several layers by default, to make it easy to differentiate what information you need on the board.

tPlace / bPlace

These layers are used for general purpose silkscreen. This is typically printed on the PCB.

Most component footprints will generate objects on the Place layers to indicate the rough position of a component. In many cases, this is a simple square or circle just outside where the component will sit.

It’s also a great place to draw neat PCB art or add text, logos, or other information you always want printed on your board.

tNames / bNames

These layers are used for component Names. These are also typically printed on the PCB.

The Names layer is full of automatically generated names for each component that match your schematic layout. Examples of this are R1,R2,C1,and U1. It’s usually worth your time to arrange them in such a way that you can easily read them when he board is printed. This makes it much easier to reference the names to your BOM or component list.

tValues / bValues

These layers are used for component Values, such as the precise resistance or capacitance. These are sometimes printed on the PCB, but many designers prefer to simply include the Name and referencing the BOM for the value.

The Values layer is also full of automatically generated names for each component that match your schematic layout. Since it’s not often printed, rearranging and organizing this layer may not be needed. An exception to this is kits and user-assembled boards. Having the values listed alongside the part can greatly simplify the assembly process. It’s also helpful for making large printouts of a PCB as a visual reference.

_tsilk / _bsilk

These layers have been depreciated in favor of tPlace and bPlace, but frequently seen on older footprints shipped with Eagle. These generally are not shown in Eagle’s layer list unless a footprint uses them.

Other commonly used layers

While not essential for every design, these layers often have special purpose within Eagle, and are common with standard footprints

tDocu / bDocu

These layers are “documentation” layers, and are not intended to be sent to a fabricator. However, it’s incredibly useful for designers.

May standard libraries draw the physical component size on this layer, to help provide a sense of scale when using their footprint.

It’s also common to see small diagrams or notes regarding enclosures or housings for the PCB. It’s often difficult to see non-pcb related designs otherwise, despite directly affecting the layout process.

2 , 3 , 4, … , 15

These are the internal copper layers, which require a paid Eagle license to use. You will also need to adjust the drc to add these layers to the stackup before they appear in the layer list.

These layers are ordered with the assumption that 1 represents the Top layer, and 16 represents the Bottom layer. As such, most 4 layer CAM jobs assume you’ll use 1 (Top), 2, 15 and 16 (Bottom).

bCream / tCream

These are the solder paste layers, which are used for making solder stencils. This layer is automatically generated over any SMD pads you place. While it initially looks similar to the Stop layers, the Cream layers don’t generate openings for vias or through-hole pads.

tRestrict / bRestrict / vRestrict

tRestrict and bRestrict layers are used to indicate areas where you want to limit the copper. This is mostly used for removing copper from copper Polygons. When Eagle fills in copper Polygons, any region that overlaps a Restrict layer will be removed.

When used with an auto-router, the router will avoid drawing traces that overlap the tRestrict or bRestrict layers. The vRestrict layer will prevent the auto-router from placing vias in the indicated regions.

Milling

Similar to the Dimension layer, the Milling layer also is useful for defining edges and slots on the board. However, the Milling layer does not interact with the DRC checker. This helps when defining slots near copper, since copper pours are not pushed away.

Generally, you’ll only see this in PCB footprints using plated slots, or on very small boards that need ground planes to extend to the very edge of the pcb.

Special layers that can be useful

tOrigins / bOrigins

These layers show the + on component footprints. If you want to totally lock down your component placements, you can turn these layers off, and avoid accidentally moving a component and attached traces.

Most of the time though, you’ll only need to explicitly pay attention to this layer if you turn off all layers, and then try to turn a few on selectively.

Drills and Holes

These layers provide additional details relating to drill hits on the board. Typically not very useful, but can be handy when placing mounting holes.

Instead of these layers, you can also use the Pads and Vias layers to help locate plated holes, or the Dimension layer for locating non-plated holes.

Typically ignored layers

Most other layers can be ignored, and have weird obscure names that make it obvious you don’t need them. These layers, however, look helpful, but tend not to be.

tFinish / bFinish

These layers are used to indicate a special finish, such as the “hard gold” plating on PCB card connectors. However, these special finishes tend to be expensive, and generally only used for commercial products.

200 (and higher numbers)

These layers are often used as custom user layers, often for imported bitmaps or other eagle scripts.

While you can simply modify the CAM file to include these layers on your output files, it’s generally better to move data from this layer to a more standard layer that does what you want. This prevents issues between revisions where the custom layers are forgotten, and the boards wind up missing the layer entirely.