Every part that gets place on your schematic (and eventually your PCB) gets assigned a unique 'Name', which is used to distinguish parts during board assembly, or just to communicate basic information in an intelligent way.
Saying 'Change R23 on your board to a 10K resistor' is a whole lot less error prone than 'Change the third resistor down, just after the USB connector on the left hand-side your PCB to a 10K resistor'.
It's a good idea to have these names (R23, C14, U1), as well as the values (10K, 0.1µF, AT86RF212) visible on both our schematic and our PCBs. So how do we do that?
Eagle has two dedicated layers to handle exactly this kind of information on our PCBs:
- Layer 25 (tNames), which is used to store part names (R1, etc.) on the top layer of our PCBs
- Layer 27 (tValues), which is used to store part values (10K, etc.) on the top layer of our PCBs
The first thing you need to do with any new package, is add a piece of text with '>Name' somewhere appropriate in your package.
With the text still enabled (don't click anywhere yet and don't pressed escape!), you can either move your mouse up and adjust the current layer and text size in the 'Text' toolbar in the top of Eagle (highlighted below) ...
Pressing the escape key once will abort placing '>Name' and send you back to the text dialogue box, and pressing escape the second time will close the dialogue box and send us back to Eagle.
If you're not happy with the position of your text, just select the 'Move' tool and tweek the position a bit, but the position in the image above is generally good.
Remember Eagle BFF #2? You can also use that to adjust all of these properties. Simply place the '>Name' text in an appropriate position on your package, and after pressing escape twice to get out of the text tool, right-click on the label and select the 'Properties' menu item.
You can adjust the layer and size of your text in the Properties Window, shown highlighted below:
- Change the layer to 25 (tValues) and the Size to 1.016, then click the OK button, and the color should change to gray, which is the default for layer 25 (as seen in final image in option one above).
Similar to the >Name Placeholder, you want to place another text label with '>Value', which Eagle will automatically update to contain the parts value. Follow exactly the same process described above, with these two exceptions:
The >Value text should be place on Layer 27 (tValues)
- The size can be a bit smaller (perhaps 0.6096)
The exact size of your >NAME and >VALUE text is really a matter of personal taste, and with time you'll find your own way ... but you should at least be consistent about it.
Every part in my own library uses the following values (numbers shown on a mm grid!):
Name: Size = 0.8128, Ratio = 18%
Value: Size = 0.4064, Ratio = 10%
These are probably much smaller than many people may want -- the names aren't easily readable with a naked eye if you don't have good vision -- but I do a lot of boards with 0402 discretes, and tightly packed parts, so it's important to me to keep the labels small. During PCB layout I place the 'values' inside the parts so I know what values are related to what parts during assembly.
You can see this part with my own preferred label sizes below, but with enough patience you'll find your own style and figure out the values that work for you. For now, it's better to start bigger and simpler with the values use earlier in this tutorial:
It's important to make sure you have vector fonts enabled in Eagle.
By default, vector font aren't enabled, and not using them can make a mess of your Gerber files when it's time to go to production, so go to your 'Options > User Interface...' menu item, and enable the checkbox below if it isn't already. Your board manufacturer will thank you for it: