Looks like I am late to the party. Here are my recommendations and feedback.
First off you need two separate schematic diagrams. One for your printed board ASSY (PBA) and one for your Front Panel ASSY. Then you need to put them together in a system or interconnect schematic diagram like that of ANSI/ASME Y14.44 Figure 3.
Considering the Front Panel ASSY to be the final or top ASSY, the reference designators used would be basic designators. The PBA would be on the parts list (PL) of this Final ASSY with a ref des of A1 (A is the class letter for a separable ASSY–see IEEE 315 clause 22.4). For assignment of ref des prefixes see ANSI/ASME Y14.44 Figure 7 “Typical System Subdivision”.
Your J13 would be on the Front Panel ASSY schematic diagram, along with the crimp terminals and wire. Wire is a component just like a resistor, a capacitor, or any other part and uses the class designation letter of “W”. The schematic symbol of J13 should not show the outline of a D-sub connector, That is the job of the ASSY DWG. The J13 symbol should be that of 15 female terminals connected together with a dashed line indicating mechanical linkage. See IEEE 315A clause 5.3.4.1, which is from IEC 60617 and where you need to go these days for the proper schematic symbols. The PL for your Front Panel (Final ASSY) would be:
…
H1, QTY, PN, Screw (Class letter H is for hardware or use an item or find number)
H2, QTY, PN, Flat washer
H3, QTY, PN, Lockwasher
H4, QTY, PN, Machine nut
J13, 1, PN, D-sub connector body
J13-1, 1, PN, Crimp terminal
J13-3, 1, PN, Crimp terminal
J13-5, 1, PN, Crimp terminal
J13-6, 1, PN, Crimp terminal
J13-7, 1, PN, Crimp terminal
J13-8, 1, PN, Crimp terminal
J13-9, 1, PN, Crimp terminal
J13-10, 1, PN, Crimp terminal
J13-11, 1, PN, Crimp terminal
J13-12, 1, PN, Crimp terminal
J13-13, 1, PN, Crimp terminal
J13-14, 1, PN, Crimp terminal
J13-15, 1, PN, Crimp terminal
If you are going to stuff J13-2, and J13-4 you would list those also.
MP1, Total length used, PN, Heat shrink tubing (MP is the class letter(s) for a mechanical part or use an item or find number)
W1, Length, PN, Wire–size, color, etc
W2, Length, PN, Wire–size, color, etc
W3, Length, PN, Wire–size, color, etc
W4, Length, PN, Wire–size, color, etc
W5, Length, PN, Wire–size, color, etc
W6, Length, PN, Wire–size, color, etc
W7, Length, PN, Wire–size, color, etc
W8, Length, PN, Wire–size, color, etc
W9, Length, PN, Wire–size, color, etc
W10, Length, PN, Wire–size, color, etc
W11, Length, PN, Wire–size, color, etc
W12, Length, PN, Wire–size, color, etc
W13, Length, PN, Wire–size, color, etc
…
Do not use class letter “P” as connection points. The class designation letter P is for a connector that is the most movable of a connecting pair, with class letter J for the most fixed of a connecting pair (see ANSI/ASME Y14.44 and IEEE 315 clause 22.4). Your J16 should probably use the class letter P. For the connection points on the PCB schematic for the wires, I would use the terminal symbol whether the connection point is a plated through hole or a surface mount pad (see IEEE 315 clause A4.7 and clause 5.1.1–this is an IEC 60617 symbol. The symbol is “o”). The class letter(s) I would use is WP, which stands for wiring tiepoint and would not appear in a parts list because it is part of the PCB and not a part mounted to the board (see IEEE 315 clause 22.4). Your interconnect schematic diagram would show which wire number goes to which wiring tiepoint.
The reference designator prefix of A1 would apply to all parts on the PCB ASSY, including the PCB itself, which I use a reference designator of U0 (see IEEE 315 clause 22.2.5). For a complete parts list of the project/product you would have basic reference designators listed for the final assembly and then parts with the reference designator prefix of A1 for the PCB ASSY. Thus you would have J13, A1C12, and A1U0.
The ground or common return symbol that you should use on the PCB ASSY schematic diagram should be that of what I call the pitch fork (see IEEE 315 clause 3.9.2, which is an IEC 60617 symbol).
The schematic diagrams that you see are for a complete assembly. If there is a PCB then the schematic diagram for the PCB is a cutset of the ASSY schematic diagram. Here are a couple of cases in point. Let’s say you have ferrite beads on the leads of a transistor or ferrite beads on the leads of a connector or you use a pair of fuse clips for mounting a fuse. In each of these cases there are parts that would appear on the schematic diagram for the ASSY but there would not be an associated land pattern. For the case of the ferrite beads you would use the symbol of IEEE 315A clause 6.2.11, an IEC 60617 symbol, and the ref des to use would be E (see IEEE 315 clause 22.4). There would be no land pattern or footprint for the ferrite beads. The fuse would be reference designated F# and the fuse clips would be reference designated XF#A and XF#B. However, KiCad does not understand the use of suffix letters with individual parts so use XF#E1 and XF#E2 for the fuse clips. The fuse, of course, will not have a land pattern (footprint) as it is placed in the fuse clips. The fuse clips will have an associated land pattern (footprint) and may or may not have a schematic symbol–your choice.
) you should create a separate project and put those cable assemblies in there to not have them interfere with the pcb BOM/etc.
