Stand alone Pin or Wildcard

[werner]

Question 1:
Among other things, I would like to solder a resistor onto a circuit board. However, I am not yet sure whether I will mount it upright or lying down (this will only become clear when I insert the board into the existing housing). Picture 1

This is R1, for which I have chosen the lying variant.
To be able to mount the resistor standing up, I need a single pin. Since I searched for a long time, but did not find something like this, I drew a soldering nail as a placeholder in the schematic. For this I added the designation R’ on the silkscreen by hand. Picture 1 and 2

Are there more elegant solutions for the application of single soldering pins

Question 2:
When checking the schematic, a lot of error messages are displayed. But these should not cause any problems in the implementation on the board - right? Picture 3

[retiredfeline]

Just make a special resistor footprint with 3 pads for the horizontal and vertical spacings and two of the pads have the same number so a track will have to join them.

[jmk]

On the left are your vertical and horizontal footprints.

In the middle , they are on top of each other. (This creates a bunch of DRC errors)

On the right, as @retiredfeline suggests, is a new style of resistor.(no DRC errors)

To make R3, copy the horizontal footprint from the Kicad library to a Personal library then duplicate pad 2, move the duplicate pad 2 to where you wish and save. All up job, maybe 10 seconds to make this new footprint, after you find the Kicad resistor you wish to modify.

[joojala]

Shouldn’t there be a builtin copper bridge between the pads 2 to avoid possible issues later? Or maybe the pin should be 3 and the schematic should tie them?

[jmk]

No.
If you look carefully, you will see a blue ratline connecting the two pin 2s. This means they can be joined with a normal track while the rest of the board is being laid out and DRC will warn if that track is forgotten.

[retiredfeline]

@joojala

Shouldn’t there be a builtin copper bridge between the pads 2 to avoid possible issues later?

What I wrote.

@retiredfeline

two of the pads have the same number so a track will have to join them.

And they can be joined by a track in any Cu layer. It’s a technique worth remembering.

Edit: Here’s another frankenfootprint that I made. It can accommodate either the square or rectangular active crystal oscillator in a can.

[jmk]

And if @retiredfeline places the crystal footprint on a PCB, there will be a ratline between the two pin 14s and another between the two pin 1s.

[werner]

Thanks for all who responded!
I have chosen the solution of @jmk.