exxos's Atari, Amiga & retro forum

I know people are struggling with getting started with Eagle. I don't think later versions really help with the confusion. So here is version 5.6 to get people started. It shouldn't be too hard to get to grips with.


Once installed, choose "freeware" licence. Then go hunting where you installed it, bin folder, eagle.exe (assuming it didn't create a useful shortcut to the main program like it did for me!)

I'm going to show step by step a simple schematic using a basic 74LS04 inverter to drive a simple LED.

Once you have loaded eagle you get the main screen...


We then what to create a new schematic..


..and get the main editor window up..


While you may not need to change the grid size, I changed it here to 1.27mm. Notice I selected mm ( I hate inches, you you can set it to whatever you like of course) and turn the grid on..


If your confused , just copy the settings below..


The grid can be turned on or off, or use dots or lines. This can be changed at any time later if you so desire.


Next we need to use the "add tool" as shown below. It brings up Eagle's part lists where you can search for various parts.


At the bottom type in 7404*


Do not be tempted to put in things like 74LS04 as there are a million variations of the 7404 and Eagle doesn't care about it. All we need is the basic logic series number which is "7404". Notice the '*' (asterisk) on the end. This tells eagle to "search all" starting with 7404 and match anything which comes after it. I do this to show the 3 typical variations of the package, which is SMD, DIP, PLCC.


The first match which comes up kinda sucks...


It doesn't show the normal inverter symbol, so we select the next one down in the list and click the arrow to expand the variations...

Below I am just showing the 3 package types in the list...


So we can go with the 7404N, which is the normal DIP package.

Once selected, click on OK, and the mouse will move the inverter block around. So place it down somewhere by clicking the left mouse button.


You can simply move and keep clicking as many times as you want.. BUT...


Notice the 2 inverters on the right are called "IC2". This means you used up all the inverters in the first IC, and Eagle automatically created a second IC. As we only want to use 1 IC in our demo, we can use the delete tool and just click on the inverters we want to delete...


It can be worth checking the data sheets of such gates to easily see how many gates are in the IC..


So we have 6 inverters in the IC and 6 in the Eagle editor, Awesome!

Now we need to create some "wires" to wire up the inverters.

We use the "wire tool"...


Now we left click on the end of the inverter wire, and our wire now follows the mouse. Left click again to draw the "end" of the line.

Once done, press ESC to cancel the tool.

NOTE: The NETS layer should be selected in the menu near the top left by default. If it is not (or you change it by mistake) just click the box and select the nets layer.

TIP: Do not overlap the wires on the red wire of the inverter as it probably won't collect! If there is a gap between the 2 wires, it won't be connected either! So don't screw this step up! 8-)



Now draw wires as shown below. The bottom wire is intentionally left shorter for later...


Next we want to connected all the unused inverter inputs together, and later connected them to GND..

So we draw a new wire as shown below. Incidentally, once you start drawing the wire (left click where you want to start the line from) you can right click to loop through various "draw angles".

TIP: You can use the scroll wheel on your mouse to zoom in and out.


Draw the line between the first 2 inverter inputs to connect them togther.

Then Eagle will start asking you questions! (oh no!)


Basically when you create a wire, its given a "name". By default the first wire will be called "N$1", second wire "N$2"... etc... So Eagle will ask what you want to do.. In this case, we don't really care, so N$1 it is!

Click N$1 and click OK.

Keep drawing wires one at a time between all the inverter input wires (not the last one!) , and you should get something like below...

(The last one isn't connected for a reason) All will become clear later my friend ;)


Now if you raced ahead and drew a line from the first wire right down to the bottom to make life quicker/easier, then you likely just screwed up :) You should hold your head in shame and send exxos a million dollars!

If you drew each line one at a time between inverters, then give yourself a pat on the back for not trying to "beat the system". Eagle doesn't connect wires which "pass over" each other. Its a feature ;) (honestly it is!)

Either way, you should now select the junction tool. This not only visually tells you what wires are supposed to be connected, but also tells eagle they should be electrically connected.


Click on all the wire crossing points as shown below.

Next we need the ADD tool again and put GND in the search box then press enter. We then get a list of GND symbols we can use.

The one I like to use (mostly) is the one selected in the "supply1" library.


Click OK and the mouse now move the GND symbol about.

TIP: use the scrollbars in Eagle to move the schematic about where you need it. Use the scroll wheel on the mouse to zoom in and out. If you get "stuck" not being able to center the image or move it about enough, press F5 and it gives you more movement than the scroll bars (move the mouse about and press F5 and see what happens)


Now use the wire tool and draw a line from the bottom inverter input wire to the top of the GND symbol.

Eagle will then ask you a question again (uh-oh!)

It wants to know if you want to connect the signals "N$1" to "GND", as we want to connect the un-used inverter inputs to GND, we click YES!

Now to verify all the signals are connected, click the "eye" as shown below. It is basically a "highlight signal" tool. Click on the green signal wire (anywhere will do) and the whole lot should now be highlighted in a lighter shade of green.

If a signal isn't highlighted (which looked connected) , then you mess up, in which case good luck ;)


NOTE: The last wire on the bottom inverter isn't yet connected, so of course it will remain "dark" as it isn't part of the GND signal.

Next up , lets add a pull up resistor onto the bottom inverter.

Using the ADD button again, we type in "resistor" and we get a huge list. There are many variations, so I just chose a typical one..


After clicking OK, the mouse moves the resistor. We want to connect it to the bottom inverters input as shown below. Do not overlap the resistor onto the green nets line, the resistor has to connect at the very end of the line.

TIP : Use the wheel mouse to zoom in and out if you need a closer view.


Now the resistor automatically gets named as R1 after placement.

It is very close to another signal wire, so we can use the MOVE tool, to move things about to give us a little bit more space to play with.


Now we can click R1 to select it and move it about..


.. In this case, I move it down and to the right (just as a example of the movement).


Next, using the line tool, draw a wire as illustrated starting from the free end of R1..



Using the ADD tool once again, we search for a VCC power symbol such as the one used below.


Place the VCC symbol onto the end of signal wire as shown below.


You will get asked another question...


The wire we are connecting to in this case is simply named "N$7", and Eagle is asking if we want to connect to VCC, which we want to do (and keep the VCC name) so we click YES.

Back to the ADD tool and we look for something we can use as a simple jumper switch. In this case lets just use a normal 2 pin jumper header..

Now place JP1 as shown place.

TIP: Left clicks place the parts (right click rotates the parts) , press ESC to exit the tools.


Next use the WIRE tool and draw a signal net as shown below connecting the jumper to the inverter input signal net.

Don't forget to use the junction tool to create the "dot" joining the signals together.


Next we need a GND connection. We can be lazy here (yay!) and use the COPY tool instead of looking for it in the ADD parts window like we have done before.

Simply select the COPY tool, click the GND symbol on the schematic, and Eagle will create a new GND connection which we can move with the mouse..


Connect GND as shown below.

Now lets ADD a LED.

I knew already there is a part called "LED5MM" So I typed that in to use.

TIP: If you put "LED*" instead, you would get a much larger list of LED packages to use.


We should have enough skills now to link the LED, ADD a resistor and GND symbols.

Now lets say we wan't to tidy it up a little bit.

We can use the GROUP tool to select a area.

The GROUP tool works just like the "rubber band" in GEM or Windows etc. So we will have successfully transferred our rubber banding skill over to Eagle (yay!) I guess randomly clicking stuff also counts as a transferable skill...

TIP: At some point using another transferable skill, save the file ;)


Draw the box around the group of parts you want to move, such as the LED section as shown below..


Now the section will be highlighted where you can now right click to move the group of items with the mouse. Left click to plonk it down again..


So we should have something like this...

Now we can give our a resistor a VALUE using the VALUE tool...


A typical LED current limit resistor is 470R, So let's go with that.

TIP: LED current is typically something like 5V - LED VDROP (lets just say 1V as we are lazy) and we want about 10mA.. So 5V - 1V is 4V.

So to be lazy with the calculation, we can just do 4V / 0.01A = 400 ohms. So 470R is close enough for a generic value.

Voltage drops across LED's can be found in the datasheets of what ever LED you are using. But also be aware the inverter (or any gate) may not output the full 5V on its output. It could well be 4.5V for example.

Also be aware the output current of the gates you are using. Check the datasheets of your part. Output current can vary between 5mA to 50mA for example. So don't be tempted to add 100R resistor in there, as you may burn out the inverters output.


Now the value is displayed on the schematic.


R1 should have a VALUE of 10K typically. But can be 1K - 100K as its only a pull up.


But wait... there is something missing still.... did anyone spot it yet ? nope ?

The IC hasn't yet got any power rails. So we need to add them by using the INVOKE tool

NOTE: Some parts may list power rails on the symbol itself, other parts have a seperate power pins, so need to to add those in.



Then click on the "+" on any of the gates and you get this little box pop up. There is only one selection we can make (or course the IC only has 1 group of power pins) So we select it and click OK...


Now we get this power symbol...


We can place it pretty much anywhere....

So your task now is to draw the wires and connect VCC and GND to it as shown below.

So we have now finished our first schematic!

What we have designed is a simple test circuit to turn a LED on and off via a inverter IC.

PART 2 will see the start of the PCB side of things...

To be continued in a new thread......

I found this site that has a lot of cad symbols for eagle and kicad.
[url]https://www.snapeda.com/home//url]

They offer a lib service as well. They made my max10 lib for me, cost me £50 tho :roll:

I will upload my lib folder soon. I downloaded all the libs I could find a few years ago.