It is true that the TO-252 footprint is in the wrong category: obviously it should be in the Surface Mount category. However, please bear in mind that different devices from different manufacturers may have a wide range of pin naming and/or numbering so there is no one set of pin naming or numbering that is "correct" for a given package or to match any given schematic symbol. In this case pin 2 is missed out simply because the TO-252 package is a direct descendent of the TO-251 which has three pins and a tab. The TO-252 package is a simply a TO-251 with the leads bent and the centre pin cropped to make it a three pin surface mount package but using what was pins 1 and 3 plus the tab of the to-251 package. The pin assignments can easily be changed by editing the schematic symbol pin assignments. Click on the symbol in the schematic to select it then type 'i' to open the **Modify symbol information** dialogue box. There you can change the symbol pin names and numbering to match that of the footprint. Alternatively, you can save your own edited copy of the TO-252 footprint with the pins named and/or numbered as you require. Another possibility is to use the 'Seeed-DPAK' from the SHIFT+F searchable library.

Hmmm, right, makes sense. Yet, I feel like it's a mistake too easily made. I wonder if, when changing a package, it might not be a good idea to prompt the user with the pin assignment menu...

`Yet, I feel like it's a mistake too easily made. ` True but no matter what pin numbering you have on the symbol or the footprint, it will be wrong for someone at some point. :) `I wonder if, when changing a package, it might not be a good idea to prompt the user with the pin assignment menu...` sounds like a good idea but it may be of limited use because the user needs check the pinout anyway whenever they put a symbol into the schematic, not just if they've updated an existing or created a new one. Pinout and name mismatch errors will get picked up by the Design Rule Check (DRC) that EasyEDA automatically runs whenever a schematic is passed into PCB. There's also a raft of checking that the user has to do before finally submitting a finished PCB for manufacture. One of the things I have done (although not consistently!) is make a dedicated symbol for a device and make a dedicated footprint with the same name (sometimes with a suffix for different package or pin variants). But that gets messy if you decide to change the package. If the schematic symbol is for a part in a dedicated package then you have to go back and change the schematic symbol and not just edit the pin information. It gets even worse if you have a simulation schematic (which you may well want to reuse as the core of the schematic that will eventually be passed into PCB) that uses spice symbols and where the spice model for all the op amps or transistors in a multi-part package is simply the spice model for a single device, used N times for however many instances of the op amp or transistor there are in the package.... :)

@andyfierman DRC won't pick up a lot of these errors, esp. when names are numbers, and it won't pick up unassigned pins. Just sayin'. Not a slam dunk fo sure.

The transfer from schematic to PCB will pick up any mismatch between the schematic symbol and the PCB footprint pin numbering. If they're different then there will be an error message. This applies even if names are used instead of numbers for the pin numbering. If the pin numbering is the same then the transfer into PCB will go through but obviously that doesn't protect against having got the assignment wrong in both. For example if I make a simple little circuit with the 2DC2412R npn bjt from the EasyEDA Libs and three resistors wired up and then assign the TO-252 package to the schematic symbol, ![enter image description here][1] then when I pass it into PCB I get: ![enter image description here][2] [1]: /editor/20160308/56de155a6627d.png [2]: /editor/20160308/56de15d59b8fd.png