I have an LM1117 regulator and I have this problem:

When I "Perform electrical rules check" I have this error:

ErrType(5): Conflict problem between pins. Severity error.
- @ (224,79 mm,92.71 mm): Pin 4 (Power output) of component U1 is connected to
- @ (224,79 mm,92.71 mm): Pin 4 (Power output) of component U1 (net 1)

Well I can see an 2 and 4 numbers in the VO, I click here and I have a list to choose values:

- Clarify selection
- Component LM1117-3.3, U1
- Pin 2, Power output, Line
- Pin 4, Power output, Line

Whatever I choose it doesn't work.

enter image description here

enter image description here

  • \$\begingroup\$ isd that a custom symbol? because you shouldn't have two pins over the top of each otehr.... \$\endgroup\$ – JonRB Nov 14 '18 at 20:43
  • \$\begingroup\$ I don't use any custom symbol, the kicad version is: version 4.0.5+dfsg1-4 \$\endgroup\$ – ZiTAL Nov 14 '18 at 20:46
  • \$\begingroup\$ If I choose another regulator works fine but the all type LM1117 regulators have a this kind output, 2 and 4 (invisible type) \$\endgroup\$ – ZiTAL Nov 14 '18 at 20:48
  • 1
    \$\begingroup\$ You have two pins on U1 defined as power outputs, and you have connected them together. That's pins 2 and 4, which are stacked on top of each other. \$\endgroup\$ – JRE Nov 14 '18 at 20:48

Please update your component library

enter image description here

This was taken by kicad-5

[ebuild R ] sci-electronics/kicad-5.0.0-r1::gentoo

What you have is an illegal part. It has two pins on top of each other and when you try to connect it is unable to resolve which one. The LM1117-3v3 is a 3pin part and it is therefore questionable what the 4th is. If it is a part that has a 4th pin associated with the exposed substrate for improved cooling then the symbol would clearly show the pin.

  • \$\begingroup\$ I'm going to install it from debian backports, thank you \$\endgroup\$ – ZiTAL Nov 14 '18 at 21:12
  • \$\begingroup\$ Works perfect with kicad 5 \$\endgroup\$ – ZiTAL Nov 14 '18 at 21:29
  • \$\begingroup\$ Placing pins on top of each other (stacking) is supported by kicad. (Stacked pins are always connected to each other.) --- Currently this is the only way to create a "one pin for many pads" connection. (Not everyone likes it that way. I like it as it moves responsibility to the symbol creator.) --- Typically only one pin in a stack is visible. For output pins (and power out) set the invisible ones as passive. (Avoids false positives for ERC.) --- Similarly for power input pins. (invisible power input pins are global labels.) --- For all other types all pins can have the same type. \$\endgroup\$ – Rene Pöschl Nov 15 '18 at 0:18
  • \$\begingroup\$ @ZiTAL you might want to read this as you updated from version 4 to version 5: forum.kicad.info/t/… \$\endgroup\$ – Rene Pöschl Nov 15 '18 at 0:22

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.