Pins of type power output and power output are connected usb

Hi everyone,

I’m getting the following error: pins of type power output and power output are connected.

I don’t know why it’s showing me this error if USB ground should be tied to GND.

Is there something I should change?

It’s complaining also about the + input pin of the ADC OPAMP, however I got the circuit from the ADS1251 datasheet for bipolar input.

Could I eliminate the need for a UART to USB converter by using USB C? Does anyone know how to hook up UART to USB C and output it to D+ and D-?

Is the MCP2200 compatible with Linux? I read on the datasheet it’s compatible with older Windows versions. Is there a newer alternative?

ECG_TL074_STM32.pdf (205.7 KB)

Also I had to connect a VUSB label to +3V3.

ERC is telling you that you may have connected two power sources (power output) together, you wouldn’t normally do that. You have either connected something wrong or you have an incorrectly labelled symbol pin.

Would it be because I didn’t use GNDD for the digital subsystem?
Should I separate analog ground and digital ground?

Whether to separate grounds is a complicated design question, but not one that KiCad ERC has an opinion on. In this case, all that it is telling you is that somewhere something is connected power output to power output, which normally shouldn’t be the case. Probably one of your IC symbols has a ground pin with type “Power Output” instead of the correct “Power Input”. To be clear, this probably isn’t an issue that will affect functionality, but good to be sure in case you’ve accidentally shorted something you don’t intend. In order to get more detailed help, you may want to upload the schematic itself.

Hi Scandey,

Thanks for the reply.

The schematic is attached above in the thread start.

Apologies, I should have said: schematic file. The PDF is a great start, but you can’t inspect pin types with a PDF.

Sorry Scandey, please find the schematic attached.
TL074_ECG_1010_V0.3.kicad_sch (188.4 KB)

I had a look at the schematic, but ERC did not reproduce this for me.
After a restart, it starts with:

That file is only one sheet, and hierarchical schematics do not work properly without the project file either. It’s easier to zip up the project (without redundant backup files) and post the zip file here, like you did the last time.

As an unrelated issue:

  1. Schematic Editor / View / Grid Properties and set it to 50 or 100mil.
  2. Select everything in the schematic, then right click and select Align Elements to Grid

That helps with making KiCad happy and everybody speaking the same language. KiCad is a bit picky about it’s grid settings in the Schematic Editor. (For the PCB it does not matter).

On another side note: R22 & R23 are wasting a continuous 9/(1k+1k) = 4.5mA which is a bit wasteful for a 9 volt battery. Consider using resistors in the mega ohm range and buffering the center with an opamp. (TL074 is also 40 years old, there are many more power efficient opamps now).

You still haven’t turned half the 1N4742 diodes around :slight_smile:

Apologies Paul, I’m sending the zip file here.

I’ll take into consideration what you said. I also searched about the transistors for openEEG. Would they connect RA and LA?

I sorted the diodes based on a ECG project schematic I found for the patient and ESD protection circuit.

The main reason for sticking to TL074 is cost. Right now, I’m trying to build a prototype that works, once it works I’m planning on moving to OPA333s and INA333s as they are better and more precise.

15-08-23 STM32 (391.7 KB)

I found the source of the ERC issue: you have two USB connectors both of which have GND pins set to type “Power Output”. One or both of them should probably have the GND pin be type “Passive” or “Power Input” to remove the ERC error (or the error can be ignored for this project).

I don’t know. I don’t now much more about that project beyond the simple fact it exists. I never looked at the schematic for more then 20s.
About the TL074… Prototypes, yay.

This seems serious: U11 is the AMS1117 and it’s unlikely it’s output should be connected to the GND of the USB connector.

This does not look right:

And shorting pins of USB connectors when they are defined as “Power Output” also does not work, as scandey found before me. It is part of why connector pins are usually defined as passive and power flags are used. Each net may have only one Power Output pin. See also: Schematics Editor / File / Schematic Setup / Electrical Rules / Pin Conflicts Map.

My experience with USB connectors, is that Kicad treats them as power sources. Which is logical. 2 USB connectors with coupled grounds could therefor toss ERC errors. So the tip provided by scandey should be the solution for you in this case.

I quickly examined the pdf. I think there might be an issue with the VCC line. I had some difficulties seeing in which thing needs which voltage. VCC is used for the mcp2200 and ads1251 but I couldn’t see where it comes from or what it should be.

Kind regards,



So Paul i’ll change R22 and R23 to 10M to decrease the current.

So bask, I’ll ignore the error for this project.

As for the voltage inputs, +5V is the input voltage from the USB from the PC. VUSB and +3V3 are the regulated voltages from the voltage regulators which power the MCP2200 and for the ADS1251 I decided to power it with +5V as the datasheet it’s ok to power it with 5V.

16-08-23 STM (390.7 KB)

You’re trying to be a bit too quick and/or distracted.
Now you have a shorted C23. That is not very useful, and your capacitor may feel discriminated for being shorted.

Also, when using 10M resistors to split your power supply, it needs extra decoupling and buffering, unless you can tolerate or compensate for drift of the “GND” reference in some other way.

This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.