Newbie : how to make a PCB with provision for different components?

Layout Footprints
1

Hello Guys,
I would like to draw a PCB for a stroboscope to adjust the speed of vinyl turntables.
As the design is not mine and was shared by a guy from South Africa, I intend to gave the Kicad work I do to the community which shared it with me. After all I only spend some time in front of the computer, and learned how to use Kicad in the process…
So I’ve a problem. I would like to make the PCB as universal as possible.
For example, the Xtal. There are 2 possible layouts for these. The standard 5 mm between pins and the smaller one you can find now. Or the 4060 IC which can be in a 16 pin DIL or SMD. Same with the capacitors…
How would you do to design a PCB with the two formats on the same PCB and choose the actual component when actually building the device ? This way I would only have to generate one set of Gerber files and let the guy wanting to assemble it to decide which component to get.
I could not find how to do this but it may be that I am also not good at searching :wink:
So I would love to hear from you and follow all the leads you can provide.
Many thanks in advance for your help.
Edit : My Linux box only has Kicad 7.0.11 availlable.

2

Flatpak is always available. What distro? In Debian there are “backports” and I’m sure other distros have similar methods for installing a later version using the package manager.

3

Sometimes footprints can be nested within each other depending on pin layouts and component size . . . sometimes they cannot, then it gets messy . . . in the cases where they can you add a symbol for each variant and select the footprint for each variant. You then position the footprints one within the other and do the track layout.

You can mark components Do not populate (fit) to show the different options. There is a KiVar plugin to do some of this for you but I don’t know if its compatible with V7.x.y

1 Like
4

Hi,
Yes, I know I can bypass the version delivered with my distro but I do prefer not to mess with that.
I had HUGE problems with Virtualbox trying to keep current version installed instead of the one I got with the distro.
But YMMV…

5

Ah ! Kivar is available in 7 but it is an earlier version. I’ll test it, thank you very much !
(but speed reading the documentation I do not understand how it work and how to make it work…)
Newbie, you said ?

6

One way to do this is to create “special” footprints, which have the pads for both IC’s.

The wokflow can be:

  1. Create a writable footprint library.
  2. Start the footprint editor, create an empty footprint in your new library.
  3. Switch to the PCB Editor and then add both footprints on the PCB.
  4. Copy one of the footprints in the PCB editor, and paste it in the footprint editor.
  5. Copy the other footprint from the PCB editor and also paste it in the footprint editor.
  6. Save the footprint in the footprint editor.
  7. (The extra footprints in the PCB editor are now also not needed anymore, and can be deleted too).
  8. In the Schematic Editor assign the new footprint you just created in the footprint editor to the schematic symbol.
  9. Update PCB from Schematic [F8] to put the new footprint on the PCB (and attached to the netlist).
    10 Route the tracks.

This works because KiCad assumes that when a footprint has multiple pads with the same pad number, they must all be connected. So all the double pads will become a part of the netlist. You also have to be aware that different sized IC’s do not always have the same pinout. If that is the case, then you have to fiddle with the pinout of one of the two combined footprints, and hussle up the pins so the pin functions match with the two IC’s.

Another way to do it is to use two symbols in the schematic for each IC, and then simply connect them in parallel. This works but it’s extremely ugly.

Yet another option is to design the PCB with THT parts, and then use adapter PCB’s if SMT parts have to be used.

But overall, I would not do this for the whole PCB. Maybe I would do it when a certain IC is known to be difficult to obtain, but not for the whole PCB. Instead, I would just ask the client to make a choice, and then make a PCB for that. If it has to be changed later, making a respin of the PCB is not so difficult either.

1 Like
7

Hello Paulvdh,
This is a good idea ! As I only have two IC’s (4060 and 4013) it won’t be too much trouble!
Another way I thought was to select DIL footprint in the schematics, design the PCB with this form factor, then generate the Gerber files and save them somewhere. Then select SMD foot print on the PCB and redraw the PCB and save this second set of Gerber files.
As this is a very small project and as I’m learning Kicad, I think I’ll try the 3 approaches and see where it goes…
Thanks a lot for your help, all of you !
Have a nice day !

8

Yes, that’s the normal workflow for a project. But do NOT do:

Instead, just use Project Manager / File / Save As … and then save it with a different name (“Project_SMT” or something) Then you simply have a complete project for each version. Gerber files can always be re-generated, but they are mostly useless if you want to make any modification later (even changing a connector). For that you need a correctly working KiCad project.

Also, for things like crystals, there are 100+ different footprints. How many of those do you want to fit?

9

I told you I was a newbie…
Regarding crystals, the seller I use most often has only two variants of the one I need…
I’ll do as you say
Thank you for your help !

10

Yup, it is a little “comprehensive” . . . I had the same issue, but look at the examples given and you can probably figure it out . . . I did :wink: