If you want to etch a PCB with a layout in Eagle then you will need to create an image like this one to transfer your design. This brief tutorial explains how to set things up so that you can use the Eagle export command.

Let’s say you are starting with this layout. This is Joe Davisson’s Antiquity Fuzz from his Analog Alchemy site.

First, change the background to white by entering the command “set palette white;” and then the command “window;” (or press function key F2 to refresh to the screen and see the change. I get this:

Next, display only the traces and pads by entering the command “display none bottom pad via;” to get something like this:

If you have any ground pour, remember to run the “ratsnest;” command. For this layout, I ran the GND polygon all the way around the board so that I get

Finally, enter “export image pcb.png monochrome 600″ and you will create a .png format graphics file at 600DPI that looks like this

The file will have the name pcb.png and it will appear in the same subdirectory as your board file. You can print this file with MS Paint or insert it into MS Word and it will print to scale. This is true no matter what resolution you choose for your file. For example, 300DPI works well for PnP Blue transfers to copper clad boards.

This is a multi-page tutorial about creating ground pour on an Eagle layout. The picture above shows an example. Note that the ground copper fills in space underneath resistors R1, R2, R4, and R6. It also runs up under the stack of components on the right and in between the +9V trace and C1.

First, I have a short editorial. Many people make a distinction between ground pour and a ground plane. What you see above is ground pour. In PCB fabrication, a ground plane is a layer of copper that is distinct from the layers for signal and power traces. Quoting the wikipedia article Ground plane,

A ground plane in PCB assembly is a layer of copper that appears to most signals as an infinite ground potential. This helps reduce noise and helps ensure that all integrated circuits within a system compare different signals’ voltages to the same potential.

It also serves to make the circuit design easier, allowing the designer to ground anything without having to run multiple tracks; the component needing grounding is routed directly to the ground plane on another layer.

Ground planes can also be placed on adjacent layers to power planes creating a large parallel plate capacitor that helps filter the power supply.

One more thing before we start. You need to have my Eagle environment for this tutorial. If you are following along with your version of Eagle, type in each of the following six commands:

grid mil 50 2
ch lay bot
ch wid 40
ch pour solid
ch the off
ch orph off
ch iso 40
set polygon_rat on

These set the units of measurement, make sure we are working on the right layer (bottom), set the trace width to 40mils, and some other stuff related to the Eagle POLYGON command that makes the ground pour.

In the picture below, we have selected the “Restring” tab in the Design Rule Check dialog window. The “Max” entry for vias on the “outer” layers of the board is highlighted.

To specify the pad size, set the “Min” and “Max” values. You can ingnore the “%” column. In the pictur, I have chosen 25mil for “Bottom” layer pads and “Outer” layer vias.  Typically, these are the only visible pads in one of my PCB layouts.

You can click on the “Apply” button and see the effect on your layout without closing this window. When you are done, just close the DRC window.

If the pad size set by the library is greater than what you specify in this dialog, then your entries will have no effect.

Here is some of what the Eagle help file says about Restring:

The Restring tab defines the width of the copper ring that has to remain after the pad or via has been drilled. Values are defined in percent of the drill diameter and there can be an absolute minimum and maximum limit. Restrings for pads can be different for the top, bottom and inner layers, while for vias they can be different for the outer and inner layers.

If the actual diameter of a pad (as defined in the library) or a via would result in a larger restring, that value will be used in the outer layers.

Starting in the Eagle Control Panel window, open a library to change.

This will start a window for Eagle’s Library Editor. This is the where all of the libraries available on this site were assembled.

Click on the “ULP” button below the “Options” menu and you will open a Run window like the one below.

ULP is short for User Language Program. Select the program called “change-pad-in-lbr” and click on the “Open” button.

Now you should see a dialog opened by the ULP that looks like the one shown here. Select “Change pad drill” and click on the “Change” button.

Alright, another window. This has three entries that determine which drill sizes in the library will be changed and what the new value will be. The new value is the “Drill diameter” entry where you see 0.6 entered.

The top two entries are the “minus percent” and “plus percent” amounts that fix the range of drill sizes that will change. In this example both are 40 and this means that any existing drill size that is within 40% of 0.6 mm will be changed.

If you click on the “OK” button, then you are told how many drills will change in the library. If you accept this, then the program runs and changes the drill sizes. Now save the library. To change the drill sizes in an actual board layout that uses this library, use the Library>Update all menu selections in the Board Layout Editor.

The Eagle “Add” command opens a window like the one below. The libraries that are in use are listed by name alphabetically. The “Description” column to the right shows the title of each library’s description.

There are also three window panes on the far right. The bottom pane shows the full description available for the selected library: the description title and any additional text.

These gm libraries give summary information about the values of the components in each library. For example, the ceramic capacitor library description shown here contains capacitors in the 1 – 1000pF range.

Expanding a library entry one level gives a window like this one. The entries are names for component packages, the size and shape of a component. Because schematics rarely refer to the packages of a component, this can be confusing for beginners looking for a component value like 47pF for a capacitor or 100K for a resistor.

In the example above, the package is called “050X030_025″ because the package is 5mm by 3mm with 2.5mm lead spacing. The description explains that the capacitors in this package come in values from 47pF to 120pF. So given that you are looking for a ceramic capacitor in the 1pF to 1000pF range, you can find the appropriate package quickly.

In the Eagle schematic layout editor (as in many other layout editors), you place a component package and then assign a value. This makes sense because a component usually comes in fewer packages than in various values. Also, because components vary along such other dimensions as voltage rating and manufacturer, a specific capacitance (like 47pF) or resistance (like 100K) comes in many different packages.

Expanding a library entry an additional level gives a window like this one. You can see both the schematic image and the circuit board image in the top right-hand panes.

In this example, the 5mm by 3mm package has a 0.1″ lead spacing for the circuit board image. If we just put the leads through the holes of a perfboard then we will have 0.1″ pad spacing on the solder side of the board. The other entries for this package give 0.2″, 0.3″, and 0.4″ pad spacing. These different versions matter only for circuit board layout. For schematic layout, which often precedes circuit board layout, any pad spacing will do.

I usually pick the smallest lead spacing, when I am paying attention.

This image shows what a package with 0.4″ pad spacing looks like. In the circuit board image on the far right, the leads of the capacitor are bent out from underneath the capacitor to reach holes 0.4″ apart.

If you lay out your schematic first, then you can also use Eagle to layout your circuit board using the information in the schematic. You can choose different pad spacing for a component during the board layout design.

Laying out your circuit board based upon the schematic you create in Eagle can be helpful. Many people enter a circuit more accurately as a schematic than as a draft circuit board design. Eagle’s circuit layout editor displays the correct connections among components as described by the schematic layout. It also flags components that are incorrectly connected.

First, we are going to create a new project that will contain our new schematic. Right-click on the project folder where the new project will go and select the “New Project” menu option, as shown below.

The projects folder will open and you are given the opportunity to name the new project folder. We will use “Basic Fuzz Face” as our new project name. You can always rename a project by right-clicking on the project folder.

Similarly, we create a new schematic for a project by right-clicking on the project folder and choosing the menu option “New > Schematic.”

Above, we are doing this for our new project folder “Basic Fuzz Face.” This will automatically open a new window for our new schematic. You assign a name to the new schematic when you save it in the Eagle schematic layout editor.

After choosing “New > Schematic”, a schematic layout editor window opens as shown here. The window’s title bar shows that the schematic has the initial name “untitled.” When you choose “File > Save as” you can assign another name, just as in many other Windows editors.

Although you cannot see it, my cursor was hovering over the “Add” button on the left tool bar of the window when I did the window capture. The button is highlighted and a little light yellow “Add” flag has opened beneath the button. Also, the comment “Add a part” appears near the lower left corner of the window.

Clicking on the “Add” button opens a new window described on the page eagle: components.

• Eagle’s Control Panel
• creating additional folders for libraries and projects
• editing folder descriptions
• telling Eagle to use new libraries

When it starts, Eagle opens a window called Control Panel. In the picture below, we have expanded the first folder labelled “lbr” under the first entry of the Control Panel called “Libraries.” The libraries available on this site are shown as they appear once they have been installed. Below, we show one way to install these new libraries in Eagle.

Step One

First, before doing anything in Eagle, copy the libraries from the zip file into a subdirectory on your hard disk. Our example uses the subdirectory C:\Documents and Settings\gaussmarkov\My Documents\Circuits\Eagle\lbr

Step Two

Second, tell Eagle about the new subdirectory for library files.

To specify an additional library directory, choose the “Directories…” entry in the “Options” menu of the Eagle Control Panel. A “Directories” dialog like the one pictured here will appear. In this example, C:\Documents and Settings\My Documents\Eagle\lbr has been added to the “Libraries” entry. The name of the subdirectory “lbr” appears as the name of the folder in Eagle.

Note that an additional directory is also specified for projects. As you can see in the picture below, adding the second projects directory shows up under the expanded “Projects” list.

Both subdirectories were given the name “projects” but the first one has the description “gaussmarkov projects” while the second one has the description “Project Folder” assigned by the software installation.

TIP: You can edit these descriptions by right-clicking on the folder names.

Step Three

Third, tell Eagle to “use” (or to activate) the new libraries.

In order to use the components in the libraries, you must tell Eagle to use them. After right-clicking on the “lbr” folder described as “gaussmarkov libraries,” choose “Use all.”

Note that we can also tell Eagle to “Use none.” This ability to deactivate libraries can simplify component selection when creating schematics.

TIP: Eagle is mouse-friendly. As you can see, right-clicking on objects brings up many of the features of this software. You can also right-click on a single library to use or not use that library.

The libraries that are in use have green markers beside them, as shown in the example below.

Now you can use the components in these libraries to create a schematic. That process is illustrated in eagle: schematics.

Installation of these libraries is described in the post Eagle 3: Setup.

Below is a descriptive list of the component libraries, showing their organization. Additional detail appears on the page eagle: components, which also explains how to add components to a schematic in Eagle’s schematic layout editor.

Below is a summary of how I designed a circuit layout with the Eagle Layout Editor. This is part of a series of posts about Eagle that introduce this software in step-by-step detail.

First, I made a schematic of the circuit using libraries containing symbols of the required components. The components snap to a grid that keeps the schematic neat. I drew in the connections and assigned values to the components with my mouse. This is usually the easiest way to record the relationships among the components correctly.

The circuit above is the “Basic Fuzz Face” found in R.G. Keen’s article The Technology of the Fuzz Face on GEOFEX.com, a classic diy pedal article. If you go to GEOFEX, you can find the entire “The Technology of …” series and much, much more.

Second, I prepared to layout a circuit board by arranging the physical shapes of the components on another grid. “Rubber bands” (the thin yellow lines) show the connections with nearby components so that you can experiment with where the connections will actually run.

The components and their connections come directly from the schematic, preventing omitted components and mistaken or missed connections. You can toggle between the two layouts, the schematic and the board, making changes in either and they remain consistent.

Third, I completed the layout of the board by routing the wires/traces. The software also has an autorouter that will complete the routing mechanically. Typically, placing the components and routing connections is a process with lots of experimentation.

Notice that two of the components, capacitors C1 and C2, have different lead spacing than before. I revised the placement and routing many times to get to this arrangement.

You can use this layout to make the circuit on perfboard or to create a template for etching a circuit board.

Images can be exported in standard graphical formats at a resolution that you choose. Here is an example of a template for etching a pcb produced from the layout above. All of the gm libraries use a drill size of 0.8 mm (approximately 0.03 inches). To make this image, all of the pad sizes were increased, the components were made invisible, and the image was made monochrome. I chose a 300dpi resolution.

Notes: See eagle: drill size for an explanation of how to change the drill sizes in an Eagle library and see eagle: pad size for an explanation of how to change the pad sizes.

For this perfboard layout image, various colors were changed.