This is how I would do it.
17:36 I start with creating a schematic. On it I put two connectors, each with 32 pins.
17:39 Mirroring one of the connectors, putting its pins on the other, and then pulling it apart, already draws most of the tracks:
17:41 Draw a single wire, hold down
[Ins] key to make some more copies (better to have too many, then too little:
17:43, Press
l (lower case
L) to place a label, I will call it
DIP25 for it’s pin number, and place it on the wire:
![image](//kicad-info.s3.dualstack.us-west-2.amazonaws.com/original/3X/4/8/4822e568f2e41a0dd01a2ca2c22da36cc16c7c2f.png)
17:45 Press the
[Ins] key for a while untill you have enough labels:
![image](//kicad-info.s3.dualstack.us-west-2.amazonaws.com/original/3X/8/1/817513efb614719a70b5a22de1fc7bcdaf91e1a1.png)
17:46 Delete all the excessive wires and labels, by drawing a box around it and pressing the
[Del] key.
17:47 Drag a box on the remaining 8 wires and labels (there is a difference in dragging the box from left to right, or from right to left) and then press
[Ctrl + D] to duplictate the block.
17:49, The block is now attached to your cursor, drag it to it’s end location and place it on the other connector.
![image](//kicad-info.s3.dualstack.us-west-2.amazonaws.com/original/3X/e/7/e7cbd27beca1e343dc3327c184b9f0d7de4a49d4.png)
17:50. That is the whole schematic. Without taking the screenshots and this typing, it would have taken me less then 5 minutes.
17:51 Footprint assignment. This I have to be a bit careful with, because you have modified footprints.
17:52 PCB Editor / File / Export / Footprints to new Library. Project specific library, and I just accept the default Library.pretty name. KiCad asks: Update footprints on board to refer to new library, answer this question with Yes.
17:55 Go back to the schematic, use one of the many available ways to assign footprints to schematic symbols, and then make sure you select the new footprints from the newly created library.
18:00 Both on the PCB and in the schematic, give U1 as reference for the DIP32, and change the reference for the 32TSSOP to U2.
18:01 Schematic Editor / Tools / Update PCB from Schematic [F8] and make sure the option: Re-link footprints to schematic symbols based on their reference designators is on.
18:04 On the PCB undo the grouping (I had no apetite for figuring out how your grouping works exactly.
18:06 Run DRC. I see three errors left. Two for the corners I already mentioned earlier, and one for overlapping courtyards, and that is intentional, (but KiCad does not know this).
18:07 Zip up and upload the project:
18:14 Fixed a mistake I made in the project.
tsop-dip32_adapter-2024-05-31_181300.zip (23.4 KB)
I have left the two clearance violations for you to solve yourself. You will notice a big differnce now, because KiCad will simply refuse to make faulty connections, and always keeps a minimum clearance distance between different nets. (This is configurable See “netclass” topic in the manual) You will also see that all nets now have net names. Some auto generated, and some with the labels given to it in the schematic.