Once you have finished your schematic design, it’s easy to create your layout. Just click on the BOARD command in the Action toolbar of the schematic editor.


EAGLE opens the Layout Editor window and shows the components randomly arranged on the left of a sample board contour. The components are already connected with so-called “airwires”, the point to point connections that result from the nets you have drawn in the schematic.


Before you start to arrange the components and create the layout, here is some preliminary advice.


1. Back&Forward Annotation

From this stage onwards EAGLE performs Back&Forward Annotation. This function transfers each action executed in the Schematic Editor automatically into the Layout and vice versa: Let’s say you add a new component in the Schematic – it will automatically appear in the Layout Editor. Or connect two pins with a net – you will immediately see the corresponding airwire in the Layout. But please remember! For Back&Forward Annotation to work you must have Schematic and Layout both open together all the time. If you close one of the windows by mistake EAGLE will warn you with a clear message in the Editor window.


If any differences do occur between board and schematic, Back&Forward Annotation stops working. You must then compare board and schematic using the Electronic Rule Check (see Article 2: “Create a project and start drawing the schematic”) and correct the differences manually.


2. Design Rules

Before you start designing your layout, it’s important to set the Design Rules. Decide the number of layers your board will probably have and select minimum pad and track sizes, minimum clearance values, minimum drill diameters (for example for vias or micro-vias) and so on. If you are uncertain what values to use, contact our engineers at Eurocircuits either by email (euro@eurocircuits.com) or by online CHAT (click on green “Contact support” button).


They can give you advice on the optimum values for manufacturing all types of PCB.


You can also download the free EAGLE DRU design rule file: Eurocircuits-EAGLE_dru_18-09-17.zip. This includes the most cost-effective DRC values from our PCB services.


The Design Rules dialog is accessible through the Edit/Design Rules menu.


Okay, now we can start creating the layout. First set the board contour. Use the WIRE command and select Layer Dimension (20). Draw a closed contour to specify the size of the PCB. Now move the components into the board area.


Layout tips.

1. Start by arranging the components in the board. Use the LOCK command to fix components you don’t want moved (for example, connectors which need pre-defined locations).


2. Before you move the components, select the correct grid to avoid problems with design rules. Click on the GRID icon to select the grid that matches the components. Place components with a mm footprint on a metric grid and components with an inch footprint on an inch grid. Enter an Alt(ernative) grid value if you want to use two different grids. You can then switch quickly between them. You can use metric and imperial grids in the same layout if required by different components. Or set two grids in the same unit; for example, 0.2 mm to rout racks for fine components and 0.4 mm where there is more space available. As a general rule keep the grid as large as you can, allowing for the requirements of the finer components.


To place the component on the right grid, click into Layer settings and activate layers 23 and/or 24 to make the “t(op)origins” or “b(ottom)”origins visible. You can now see the cross that marks the origin of the component.


Activate the MOVE command – with <CTRL> + left mouse button you can snap the component on the correct grid.


3. To move a component to a defined position, use the command line. Type in, for example: MOVE IC1 (22 50) and hit the Enter key. This will move IC1 to the given location.

The properties dialog shows that IC1 was exactly placed with the coordinates given in the command line


4. To place components on the bottom side, use the MIRROR command. It will flip the component including silk screen and solder stop (solder-resist window), plus the cream frame (solder-paste opening) for surface mounted devices (SMDs).

5. While arranging the components, execute the RATSNEST command from time to time. This calculates the shortest airwires and makes the layout more visible. You can also hide signals if you want. For example, to hide GND type RATSNEST ! GND in the command line. See RATSNEST Help for more details.

6. Next step is to route the tracks using the ROUTE command. Click onto one of the airwires and start laying out the track. Set which layer to use in the parameters toolbar. To change the layer, press the middle mouse button or click into the Layer selection box and select the new layer. EAGLE automatically inserts a via as soon as you fix the next wire segment. The airwires are calculated dynamically and always point to the next object that belongs to the signal you are currently routing.

7. Use the DRC button to run a Design Rule Check (DRC) from time to time to make sure that all rules are met. If there are errors, EAGLE shows you where to look.

DRC shows where the problems are

8. When you think you have routed all signals, run the RATSNEST command again to make sure. If it tells you “Nothing to do”, the routing is complete.

9. To draw copper planes (sometimes called “copper fill” or “copper flood”) use the POLYGON command. First draw the contour of the copper area with POLYGON, then name it the same as the signal it should be connected to. Run RATSNEST. The polygon will be calculated and the copper area displayed. Objects that belong to the same signal will be connected through thermal pads, and unconnected signals will be isolated.

GND Pads are connected with thermal symbols to the copper area

Data output

You can upload the BRD file directly onto the Eurocircuits website to check your layout in PCB Visualizer, to calculate a price or to place an order. Alternatively you can extract Gerber and drill files using the CAM-Processor.

To do this, click on CAM-Processor icon in the Action toolbar.

In File – Open –Job you can select a predefined or matching Job-File. The Job-File contains all the steps needed for automatic generation of output data. All you need to do is to define which layers to use.

You will find predefined Job Files for extracting Gerber and drill files.

Always set Device to Gerber RS 274X 2.6 Inch to avoid rounding errors.

With Del or Add command you can add or delete Sections.

Save this job under a new name with File/Save job. That way the original job file remains unchanged.

Use Process Job to execute the job which has been loaded to extract Gerber files.

Click again on File – Open – Job and load the Excellon job to generate Drill Files.

Select the same Device setting, 2.6 Inch as for the Gerber files. This ensures that layout and drill data match exactly on the finished PCB. In the right menu you can see that Layers Drill and Holes are combined for drilling.

Click Process Job to execute the loaded job and extract the drill files.

TIP: You can save both Gerber output and Excellon ouput in one CAM-Processor job to generate Drill and Gerberfiles in one run.

To add a layer to the CAM-Processor job click Add, select the Layer you need, change the Section to the correct name, select the Device and the matching File extension then save it.

You can send us the BRD file or the Gerber and drill files. Once they are uploaded into our PCB Visualizer we will show you what the finished board will look like, as well as any DRC issues detected.