Eagle’s popularity is partly due to the sheer number of parts and footprint libraries available for it. Sometimes you can’t find the part you need in an existing library though, and it’s time to make your own. Making a new part in Cadsoft Eagle can be intimidating for new users, but the guide below shows how we make our own Eagle parts step by step. Alternately you can check it out on the Wiki.
A part is composed of 3 sections:
Lets take the LM5022 as an example, a simple 10 pin chip. The datasheet shows the connection list we need to build the symbol.
The datasheet also has packaging dimensions we need to build the footprint.
It’s very important to have the landing pattern and not just the pin dimensions. Some datasheets will only give the pin size, the landing pattern is larger and optimized to help the chip solder easily.
Let’s start with the symbol. Symbols are what you connect to other parts in the schematic diagram. We’ll design this one as simple as a block with pins.
Create a new symbol by clicking the symbol icon in the library editor
Hint: If you haven’t created a library yet just go to Panel > File > New > Library in Eagle Control
A window will open and ask for a symbol name. Enter the chip name or part number and click OK, then click Yes when asked to create a new symbol.
In the chip’s datasheet find the pinout or connection diagram, this will be the basis for our symbol
Start making the symbol by using the ‘wire’ command in the 94Symbol layer as an outline, ICs are rectangular so we just make a simple box to represent the chip. Always put the symbol on its center (0 0) as this will be your anchor when moving in the schematic.
Place pins on the chip. Click the pin button, then click on the symbol to drop pins.
Hint: When placing the pins just leave the current settings for the grid (0.1inch), this makes the connection easier to snap when working with the device later.
Name each pin by using the ‘info’ command, and clicking on the pin. Name the pins according to the datasheet to make life easier later. You can tweak other pin attributes in the info window too.
Add a space for the part designation on the 95Names layer. This is where the part number such as IC1, C3, or R2 will appear on the schematic.
You can also place the ‘value’ label for the part on the 96Values layer. We don’t usually assign a value because we usually change it in the schematic design phase.
Hint: The prefix ‘>’ is not necessary for these texts. It’s just a style decision.
Footprints, sometimes called landing patterns, define where a chip attaches to a circuit board. The footprints will be the silver shiny pads that you’ll solder parts to later. Eagle calls this a package.
To access the package editor click the ‘package’ icon.
Name the package, this time by the package type which is MSOP-10 for this chip.
The datasheet gives the units in inch and mm. We’ll go for the metric unit, but you could also use inches.
Check the datasheet for the dimensions of the recommended pin pads. We’ll use this to make the optimal pad in our footprint.
Here, the manufacturer recommends 0.3 x 1.02. This area will be slightly larger than the pin itself, and is optimized for the package type.
Important: It’s very important to have the landing pattern and not just the pin dimensions. Some datasheets will only give the pin size, the landing pattern is larger and optimized to help the chip solder easily.
This is a surface mount part, so we click ‘SMD’ to get the right pad. For through-hole parts click the round green via next to the SMD button.
Set the dimension of the pad to the values we pulled from the datasheet.
There are many ways to place the pad in the correct position. You can place it manually if the grid you set (View > Grid) fits the pad pitch. Alternately you can calculate the correct pad coordinates, we’ll use this method.
What we’re going to do is calculate the location of the center of each pad using the values from the datasheet. This seems a little tedious, but we think it’s easier than messing with the grid values constantly.
The formula for the X axis is Px=(n-1)Dpx where:
For Pad 1 X (3rd pad from X center)
Pad1X=(3-1)0.5 will be 1. Since pad 1 is located on the 3rd quadrant its X value will be negative hence -1.
The formula for the Y axis is Py=Dpy/2 where:
For Pad 1 Y
Pad1Y=4.8/2 will be 2.4. The lower pads are below the X axis, and should be negative. The Y location of Pad1 is Pad1Y=-2.4. On this chip pins 1-5 will have negative Y axis value (-2.4), and pins 6-10 will have a positive Y axis value (2.4).
Now we have: Pad1 at (-1 -2.4), Pad2 at (-0.5 -2.4), Pad3 at(0 -2.4), and Pad4(0.5 -2.4). Repeat for each pad. Remember that the Y values only need to be calculated once.
(-1 -2.4)(-.5 -2.4)(0 -2.4)(.5 -2.4)(1 -2.4)(1 2.4)(.5 2.4)(0 2.4)(-.5 2.4)(-1 2.4);
With these coordinates we can place the pads easily.
The order of the coordinates in the command box assigns numbering to the pads. Its not necessary to do it like that. You can always use the ‘info’ command and edit the pad name or fix mistakes.
Now we’ll make the chip package and pin outline, again using the values from the datasheet. This is a 3×3 mm chip with 0.23x.95 sized pins.
Use the ‘wire’ command to draw the outline on the top silk 21tPlace layer.
We used the package dimensions in the datasheet to calculate the coordinates of the chip’s 4 edges.
It’s nice to see where the actual pins will be when you route the PCB. We’ll create a pin reference on the Document layer. We use the Document layer so the reference will not be included on the top silk or overlap the pin pads.
Use the ‘Copy’ command to copy the first pin. Place a copy on each pad with its base touching the chip outline.
When we’re building the board we need to know how to position parts. Mark pin 1 with a zero width ‘circle’ on the top silk 21 tPlace layer. The zero width circle will fill up.
Finally put a ‘name’ text near the chip, on the top silk name layer 25 tNames, and we’re done.
Device links the symbol and package and makes the whole part.
Create a new device by clicking the ‘Device’ symbol
Import the symbol by clicking the ‘Add’ icon.
A window will pop-up with a list of symbols in the library. Pick the symbol that we made before and click OK.
Now import the package by clicking the ‘New’ button.
Eagle highlights packages that will fit the symbol. Choose the package/footprint we created before.
In the variant name box enter the same name as the package. This can be used to make different sizes of the same device. Click OK.
The footprint appears on the package list with an ‘!’ icon showing that the symbol and the package are not linked or connected yet. Click the ‘connect’ button to link both.
After clicking the connect button, another window will appear showing unpaired pins.
Match each symbol pin with the corresponding pad and click connect. Each pin should only connect to one pad.
Finally, click the ‘Prefix’button and specify a prefix for this chip. Eagle will automatically increment this when you make your schematic, eg IC1, IC2, IC3. It will also identify this part in your bill of materials.
Save the library and you can try your newly created part.