



Most hobbyists and many professionals use Eagle CAD as a daily tool in designing schematics and laying out PCB. I’m going to share with you the most important tips and tricks for using Eagle CAD, which make my work much easier and faster.

Tip #1: Keep One Hand on the Keyboard, One on the Mouse

I see a lot of friends and colleagues use the mouse as their main tool for routing and selecting tools in the sidebar, but it’s much easier and faster to use the command line whenever you can.

By using your keyboard, you will omit the time you spend searching for the desired icon and moving mouse pointer back and forth.

My advice is to keep one hand on the mouse to do wiring, etc. inside the editor workspace and use the other hand on the keyboard to write commands and select tools. My advice of using the keyboard is not only for selecting tools. You will see the other benefits of using the keyboard in Eagle CAD in the rest of this series.

It can be difficult to remember the spelling and the name of every tool. The good news that the command line only needs the smallest accepted spelling to select the tool for you, so you don’t have to write down the complete word.









The table below shows the most-used tools and their corresponding shortest commands. To avoid duplication, the common tools between the schematic and board will not be listed twice:





Schematic Editor Tool Name Command (All accepted for command editor) Add element to schematic a,ad,add Net ne,Net Move Mov,move Copy Cop,copy Name n,na,nam,name Value v,va,value Label l,la,lab,labe,label Text T,tex,text





Board Editor Tool Name Command (All accepted for command editor) Route rou,rout,route Ripup ri,rip,ripu,ripup Via Vi,via Ratsnest r,ra,rat,rasts,ratsn,ratsne,ratsnest





Other useful and exclusive uses of the keyboard can be mapped as below (just two examples for now):





1- Text Tool:

When you select the text tool, you write your sentence in the pop-up window and then drop it wherever you want. But what if you want to add more?

In this case, just write down your sentence and hit enter without needing to select the text tool icon again.









2- Show Tool:

This tool is used exclusively with the keyboard. You need to enter the element name using the command line to highlight it. For example:

>Show R1

Or

>Show R1* (to show all elements start with R1)

This applies also for signal names.













3- Others:

To keep you excited (and to make things more organized), I will delay talking about other tools that are exclusively used with the command line to their respective tip/trick.





Tip #2: Use Your Mouse Effectively

There are many practical uses of the mouse in Eagle CAD, more than just using it as a pointer:





1- Changing Layer Using the Scroll Button:

Let's say you are routing your PCB. A lot of people used to change the layer of an object using the layers drop-down menu.

However, by using the mouse, you can change the layer by pressing the scroll button.









2- Change Wire Bend Styles:

Changing wire bend styles is one of the most common processes while routing.

The hard way is to change styles by selecting the wire bend style from upper toolbar every time. The easy way is by pressing the right mouse button.

You can see the practice of the past two mouse usages in the gif below:









Tip #3: Hit RATSNEST to Know How Many Signals Are Still Unrouted

By pressing RATSNEST, the number of unrouted wires (airwires) is shown in the bottom-left corner of the editor.

This feature is very useful for double-checking that you didn't miss any airwires, especially since sometimes you may not notice them when searching visually.









Tip #4: Make the Help Manual Your Friend

Whenever you want to learn more about the tool you're using, press F1 and read about it!

You will find really handy hidden usages of each tool in the manual.





And now for the "tricks"!





Trick #1: Change Wire Width without Moving Your Mouse

You can change the wire width without going to the width menu! Just write the width number and hit enter while you're holding the wire.









Trick #2: Hide Any Unrouted Wires You Want

The most annoying signal that contributes to a feeling of incompleteness and complexity is the GND signal.

You could hide it, or any other signal, by using the RATSNEST command in this form:

>ratsnest !

For example:

>ratsnest ! GND

To make it visible again just omit ‘!’:

>ratsnest GND









Trick #3: Turn Polygons Off

Let's say you've drawn a power polygon, like VCC or GND, and now you need to change some routes. Polygons become very annoying in this case because whenever you hit RATSNEST, a polygon will fill the PCB again.

You can keep working without polygons until you want to enable them again. Without deleting them, you can just turn them on or off as you like.

To turn polygons off, select ripup tool, ripup polygon, then write this command:

>set poly off

To turn them on, type this command:

>set poly on









Tool Name Command (All accepted for command editor) Add element to schematic a,ad,add Net ne,Net Move Mov,move Copy Cop,copy Name n,na,nam,name Value v,va,value Label l,la,lab,labe,label ext T,tex,text

Tool Name Command (All accepted for command editor) Route rou,rout,route Ripup ri,rip,ripu,ripup Via Vi,via Ratsnest r,ra,rat,rasts,ratsn,ratsne,ratsnest





Tip #5: Best Practices to Find the Parts You Need

Before searching on the internet for new libraries to add to Eagle, first make sure that your device does not already exist in your local libraries. To check, use a search pattern that includes ‘*’.

For example, if you want to add a 7805 5v regulator, you must search for *7805* instead of 7805. This will search for any part with 7805 in the middle of the name, without regard for the beginning or end of the part name.

Certain manufacturers may have their own extensions, and Eagle search is not smart enough to know these extensions for you. This explains why sometimes search can't pull up a part that you know is present, even when you search in an explicit way. You can see from the below GIF how search results will change using this tip:









If you didn't find your part, or at least a reasonable alternative (for example, an atmega8 device instead of atmega328 device), then try to add public libraries from other popular producers and designers like:

If the parts you want to use were used in previous open source board, you can export these parts from (File>Export) and reuse them again in your design.





Tip #6: Don’t Always Trust Third-Party Libraries

Keep in mind that unverified parts are always there in the cloud. Especially when you use a library from an untrusted party, you need to make sure that you double-check the footprint and device connection with package pads to avoid errors in your PCB connections.





Tip #7: Use the Eagle Reference Library

When you build your own library, keep in mind that there is a reference library in Eagle called "Ref-packages.lib". This library has most packages' footprints, which make the creation of new libraries much easier.

Just copy the package to your library, then reuse it again to create a new device. This will save a lot of time and errors.









And now for the "tricks" section.





Trick #4: Ripup All Polygons with One Command

When you work on circuits with applications like high-power signals and you use more than just GND and VCC polygon planes, you can ripup all polygons using one command:

>ripup @ ;









This is much better than ripping up every polygon manually.





Trick #5: Route Your Trace from Any Point You Want

When you route a trace in PCB, you must have an airwire first. Eagle calculates the shortest path for the airwire and then draws it, but in some cases you need to use a different path than the default one.

You can draw a trace from any point by selecting the route tool and pressing ctrl with left click on the desired point.









Trick #6: Adding a Bar to a Signal Name

You can add a bar to a signal name,active low signal, using this formula:

>name !RES

If you need to add a bar just to a section, then use this formula:

>name !RES!_MCU





Trick #7: Enable/Disable Layers View

When you have your final design of PCB and you need to review it before sending the Gerber files to a manufacturer, a good practice is to review each group of layers individually.

For example, you can review the Top, tPlace, tOrigins, tNames, and tDocu layers, THEN the Bottom, bPlace, bOrigins, bNames and bDocu layers. Instead of choosing every single layer you want, you could disable/enable them using one command: DISPLAY.

The DISPLAY command is used to disable/enable view of the layers. Parameters of this command could be ALL to make all layers visible, or NONE to turn all layers off. You must put the layer name or the layer number as a parameter— when you use a negative sign before your layer name, the corresponding layer will be filtered out.

The following command will make just the Bottom layer visible:

DISPLAY NONE BOTTOM;

The following command will make TOP layer visible and hide BOTTOM layer:

DISPLAY TOP -BOTTOM ;

Here are some commands I formed that I'd like to share with you. I use these each time I review a design:

Top Layers:

DISPLAY Top tPlace tOrigins tNames tDocu Dimension -Bottom -bPlace -bOrigins -bNames -bDocu;

Bottom Layers:

DISPLAY Bottom bPlace bOrigins bNames bDocu Dimension -Top -tPlace -tOrigins -tNames -tDocu;

Complete:

DISPLAY Bottom bPlace bOrigins bNames bDocu Dimension Top tPlace tOrigins tNames tDocu;

Complete without naming:

DISPLAY -tNames -bNames Bottom bPlace bOrigins bDocu Dimension Top tPlace tOrigins tDocu;





Trick #8: Show the History of Some Icons

There is a useful hidden feature in EAGLE GUI which is shows the history of some icons, like ULP and Open.

So if there is a ULP and you use it in a regular base, you can just right-click on the ULP icon and a menu of the history of recently used ULPs will pop up.









Trick #9: The Renumbers Parts Tool

When you work on big projects and you have a really big schematic, you will need to do a lot of changes by adding and deleting components during verifying phase. This will make some mess in your number of parts.

For example, when you have resistors with numbers from R1 to R50, and you need to delete resistors from R10 to R12 and R25 to R30, R51 will be the number which Eagle will use when you add the next resistor.

For this reason, Eagle has a tool, ULP. In fact, ULP can do a renumbering for you instead of doing it manually, which is very hard in big schematics.

You can choose this tool via tools>Renumber parts— or via the ULP icon and selecting "renumber-sheet.ulp".











