1) C1, C2, C5, C6, C11, C12, C13 should be 0.22uF. C14 could be 0.22uF as well to simply your Bill of Materials.
2) The ground side of C2 needs to be connected to the ground side of C3.
3) Your BDM circuit is very wrong as is your LOAD/CEL circuit that you have connected to the BDM circuit, see my schematics at
https://github.com/DeuceEFI/Jaguar/tree/dev to see what they should each look like.
4) You have PE1 (connector pin 15) connecting to both Port A5 and Port P0, you should only connect to one or the other.
5) R5 (1M ohm) is not needed with the XDP512 processor, you can safely delete this component from the schematic.
6) On the CAN transceiver circuit the R12 pull up resistor should be a 10k ohm resistor.
7) Many of your connection points at the processor and the other components are missing the green junction symbol, so they may not be electrically connected when you go to perform the electrical rules check or create the netlist. It is proper form to make sure that all the wire and component connection points have the green junction symbol if they should be connected.
8) Once you correct the above items, the next thing you need to address is the ground plane under the processor, it should look like the one in the MC9S12XDP512RMV2.pdf Figure C-2 on page 1295.
9) One thing you might want add is Port K4 as the firmware can use this as the radiator cooling fan relay output.
10) I do have concerns regarding your choice of connector, I'm not sure how many insertions/removals from the socket on the main PCB the pads/solder joints will take before the pad(s) lift off the PCB or the solder joint(s) fail.
11) One thing to keep in mind is the difference between the M$ BRV circuit and the FreeEMS BRV circuit, you will need to modify the M$ circuit with the proper resistor values or your readings will be incorrect. See the Jaguar schematics that I linked above for the proper values.
OK, that is all I see from a quick 20 minute review of the schematics.
What operating system are you using with KiCAD? If you are using Windows, you can use CutePDF Writer (free download) to create PDFs of your schematics. I use both Debian Wheezy and Windows 7 with KiCAD, but I haven't had much luck with creating PDFs in Linux, the fonts won't render correctly when the PDF is created. So I use my Windows machine with KiCAD and CutePDF to create the PDFs in my github repository.