The next steps are:
1 - create a D-Sub 62 footprint
2 - Assign footprints to symbols
3 - Generate a netlist
4 - Start the layout program and load the netlist

 

Thank you @hrs. Will get busy and see where it lands me. More questions to come, I am sure.

 

@hrs, I have found a footprint in the library that I think might match or could be very close. Can these be modified to amke it your own or do you have to start from scratch? The Digikey part # is A-HDS 62 A-KG/T if you want to look at the datasheet.
in the library, it is the first 62 pin male connector in the list
www.digikey.com/product-detail/en/assmann-wsw-components/A-HDS-62-A-KG-T/A-HDS62A-KG-T-ND/1241904

 

First note that post #21 is incorrent for step 1. The footprint editor is 2 icons to the right, but you may already have noticed that.

Yes, you can modify existing footprints. First you need to create a new foot print library in the footprint editor. File -> New library ... Then, still in the FP editor, load the FP that you want to modify and save it to your FP library, File -> Save as ... Browse to your library that should be in the list and double click it or select and press save. The FP is now in your library and ready to be edited.

 

I did catch the incorrect symbology but thank you for that.
So I opened the FP editor and found the closest replica of what i want which is the one in the post above. I went to Save As and I get an error referring to the fact that it is a Read Only file. Not sure what I should do with that.
1) Opened footprint editor
2) Located D-Sub 62 Pin Male connector that I wanted to use as starting point
3) Attempt to Save As
4) Error

 

1.b) Create a new FP library
3) Save the D-Sub connector in this new library. Note that you can change the name of the FP in this step
4) ...
5) Profit!

 

Okay so I am working on the footprint for this and took one from another library and adapting it to this unit. A little confusion has set in and I want to make sure I am correct in what I am doing. I would assume that all 62 pin connectors would have the same pin placements but it would seem that the one in the library has different coordinates than mine. I spaced mine out according to the second diagram at 2.41 mm between pins which was correct and 2.54 between rows but when I look at the one in the library, they are spaced at 1.98
If I am correct, 2.41 should be the spacing on the connection pins and 2.54 should be between rows. When I measure it on the board with a micrometer, this holds true. Am I missing something or doing something wrong?
Second question. There are two ref** points still in this diagram and they both point to Pin 1 when highlighted. One is for the reference to the schematic symbol, I get that, what is the other one for.

 

Maybe the KiCAD FP you're modifying isn't true to the D-Sub standard or maybe the A-HDS 62 A-KG/T isn't. Either way, go with what your datasheet says. As I see it that's 2.41 horizontal and 2.54 vertical spacing.

One of the two refs ends up on the silk screen the other field by default mirrors the reference value via the %R switch but it can be modified. It ends up on the F.Fab layer. I never use it. The documentation has this to say about that:

Fabrication (F.Fab and B.Fab)
The fabrication layers are primarily used for documentation purposes to convey information to, for example, the PCB maker or the assembly house.

 

Okay I think I have the proper coordinates for everything on my footprint. Could someone have a look at this and see if I am missing anything? One thing I took out of the exiting footprint was an arc that joined the two lines going from the PCB edge to each side of the mounting holes. Does that matter? Other than that, I think I am done. Once I am done do I assign the footprint to the symbol? Do I put all the footprints on the same page or how does that work?

 

Looks good to me. One more thing, you can set the two mechanical holes to "NPTH, mechanical" in the pad properties dialog.

 

Just to clarify. When you say mechanical holes, does that mean without copper pads? The two mounting holes are solder pads in this case. I am not sure what the white oval or the dot means. They were part of the symbol I borrowed from the library.
what does NPTH mechanical mean?

 

The datasheet wants 3.4(+.05/+.0) mm mounting holes I think. The hoIes in the KiCAD D-Sub are 3.2 mm. I don't know this connection type so I don't know how it's supposed to work:


NPTH means non-plated through hole. If you need to solder them then I guess you don't want NPTH, but it looks like spring loaded grabbers.

The white oval and the dot are zero, the pad number. Apparently the program doesn't care if you have two pads called 0.

 

All good information. Nice picture and exactly what I am using. Where did you get it from? Any ideas on the J1-J62 connections? I am trying to set up my banana_jack_01 in my footprints. The actual receptacle is 0.078" in diameter going into the PCB hole and the tube is 0.200 in OD. I think the annular ring can be the same size. Do I have to do the same thing 62 times or can I copy this forward somehow in my footprint to symbol list?

 

Nice picture and exactly what I am using. Where did you get it from?

It's from the link in post #23

Any ideas on the J1-J62 connections? I am trying to set up my banana_jack_01 in my footprints. The actual receptacle is 0.078" in diameter going into the PCB hole and the tube is 0.200 in OD. I think the annular ring can be the same size. Do I have to do the same thing 62 times or can I copy this forward somehow in my footprint to symbol list?

You do one of two things. You can either create a new footprint that macthes your receptacle. This would be simply a pad with an outline. This is the cleanest. Or you could banana_jack or whatever 1 pad footprint and do with it what I said in post #7.

 

Okay how does this look? I am in the Footprint Editor-Read only.
Do I need to change REF** or Banana_Jack to anything else? Is this symbol ready to go?
Do I save this as a new library now?

 

Yes, change banana_jack to whatever you like and save it in your footprint library, the same one that you put your modified D-Sub in. Of course you can organize your libraries however you want, i.e. you could make a new library for this footprint, but you can also put it in the one with the D-Sub.

 

Is the J1 in the right place or should that be in place of REF**?'
I have assigned footprints to J1-J62 but they all say J1 on them. How do i change them to J2-J3-J4....

 

That "J1" is the pad number. I would change it to "1". Since this footprint only has one pad, all 62 instances will show "1" for that pad. "REF**" will correspond to the pin references in the schematic and once you start working on the board layout those REF**s will be J1-J2-J3 or whatever you called them on the schematic.

 

Okay so I am on the PCB New part laying out my PCB. I have printed it out and hole alignment is dead on so I don't want to change anything but I have a couple problems.
1) I noticed that when I did the 62 pin footprint, I didn't change the mounting holes to pads and they should be pads because those tangs solder to it when it is mounted on the board. How can I add these in without damaging my layout now?
2) I have 6 mechanical mounting holes to add and I think I have this figured out but do I go into my schematic and add pad holes and make them NPTH mechanical holes? Do I then have to go through annotation, assignment and netlist again or how does that work?

 

1) I noticed that when I did the 62 pin footprint, I didn't change the mounting holes to pads and they should be pads because those tangs solder to it when it is mounted on the board. How can I add these in without damaging my layout now?

I've never tried that before but I think you could just modify the footprint. Maybe you need to generate a new netlist in the schematic editor and load it in PCB New, I don't know. Are you sure it doesn't have pads? If you worked from the existing D-Sub footprint that comes with KiCAD it should have pads.

2) I have 6 mechanical mounting holes to add and I think I have this figured out but do I go into my schematic and add pad holes and make them NPTH mechanical holes? Do I then have to go through annotation, assignment and netlist again or how does that work?

In PCB New, select the layer called Edge.Cuts. You can draw circles on that layer that will be mechanical holes. After this it may or may not be required to run the design rules check. That's the icon with the ladybug on it. I always do run it because that also recalculates the copper fill area that I invariably have. It doesn't hurt if you do.

Edit: I didn't know this but you can indeed add "MountingHole"s to the schematic and assign a hole footprint to it. This is probably the correct way to do it.