Hello,
I’m working with an LM117 voltage regulator in my schematic, and I could use a second set of eyes to help verify the connections. KiCad is flagging two error messages:
Pin of type ‘output’ connected to pin of type ‘output’
Pin of type ‘output’ connected to pin of type ‘power output’
I’ve reviewed the circuit multiple times but can’t identify the issue. I’m still fairly new to KiCad, so I’d really appreciate any guidance to help resolve these warnings.
Thank you!
Remove the PWR_FLAG on 3V3. It is already a power output (by the LM1117)
as far as i know there is no way to ‘resolve’ this, the ERC is a very simple tool, and cannot understand that this is not a real problem, this is up to you; simply ignore this kind of ERC.
Done, but I’m still getting the same error message. However, the arrow is no longer pointing at VOUT2, it’s now pointing at VOUT4 and the 3.3V power net.
Okay… Are you sure this won’t cause errors later on?
Then ignore it. This is a common “false flag”. Just consider it as an heads up.
Alright… Thanks for your input
just disable this two warnings (‘exclude this violation’ option and NOT ‘ignore all … violations’),
other parts of the circuit will be checked for multiple outputs connected together.
This kind of errors happens a lot with linear and switching regulators that have multiple pins for increased current capability, and i have not found yet a way to avoid it.
Thank you very much for your input… Much Appreciated
You’ve apparently created your own symbol and it’s highly problematic or more precisely: wrong.
The LM1117 does not have two outputs, ii only has one. That it’s connected to two pins (2 and heatsink) does not change that.
Why don’t you use the LM1117MP-3.3 already available in the library?
I downloaded the component from SnapEDA, and I noticed that the symbol includes two VOUT pins. However, according to the datasheet, there’s only one VOUT pin. I also tried other versions of the component, and it’s the same thing; only one VOUT is shown in the datasheet, but the symbol has two. That’s why I decided to post this issue here, to see if anyone else has experienced the same thing.
Ah yes. The other one is the feedback / adj. Try to fix that with your symbol. If the error persists, ignore it.
I personally don’t disable those power errors, I consider them as a warning asking for a second look. I got used to them.
No. It’s just that the output is connected to two pins in the device: pin 2 and pin 4 (heatsink). Electrically they are identical. ADJ has nothing to do with it.
But this is irrelevant to the symbol itself.
You are right!
padding chars
Reference Example
(LM117-317 Voltage Regulator Power Supply Project)
Variable DC Voltage Supply 1 Project
https://www.inventfx.com/_ifxkicad/VARDCPWR1.xip
Inventor eFX KiCad Website:
https://www.inventfx.com/_ifxkicad/_ifxkicad.htm
Thanks! I tried the regulator you suggested, and it works perfectly now.
It’s a bit confusing that the title mentions a LM117, while the screenshot is from a LM1117 (with three ones). Both IC’s exist (in multiple versions from different manufacturers).
I compared the LM117 and LM1117 and the latter is available in both fixed and variable voltage output.
Since the actual screenshot is the LM1117 (SOT-223) 3.3V Fixed Output Version I designed
the following:
LM1117.zip (278.4 KB)
GOTO:
IFX Kicad Works
TO DOWNLOAD SYMBOLS, FOOTPRINTS AND 3D MODELS
Based on the image above I feel obligated to point out that with the (negligible) heat sinking you’ve provided for the LM317 then with around 12V across it you wont get much current out of your board without the LM317 overheating. 20 or 30mA maybe.
Just sayin.
David
As the LM1117 3.3V is an SOT package I changed the Copper Pour for both top and bottom
layers to the VOUT Net. The IC will now dissipate the heat through the entire surface of the PCB.
