Issue with PWR_FLAG + power regulator

Hi, newbie question: I got a voltage regulator on a local schema, which gives me errors… tried to work it out with no luck. I suspect this has to do with the fact that the regulator has an output pin. This pin is connected to a schema output label (and connected in the main schema).

What am I doing wrong here ?


ErrType(5): Conflict problem between pins. Severity: error
** @ (21,59 mm,22,86 mm): Pin 1 (Power output) of component #FLG020 is connected to **
** @ (76,20 mm,26,67 mm): pin 3 (Power output) of component U11 (net 29).**

It appears from the message, that your schematic somewhere outside of the screen shot has a power flag attached to the +5V net. Deleting the extra power flag will fix this error.

The reason the extra power flag is not needed is because pin 3 of the 7805 is set as a power output.

These are the only power flags in all of the 3 schemas in the hiearchy, except for a battery socket… meaning, the +5V net does not have a power flag anywhere.

Let me add, that I changed the VO pin on the regulator to “passive”, which made the error go away. Not convinced this is the way to “fix” it though…

I think what you need to do is eliminate the power flag and use a label on the net. Or the “+5V power-flag symbol” Similar to Vcc but I don’t believe it is an actual PWR_FLAG in the same sense. If it complains, just go with a Label.

If i read the error message correctly then the output of U11 (5V) is directly connected to GND somewhere.

Sadly we can not help you without seeing the complete circuit. But i would advice you check every connection from any GND pin.


That’s what I was thinking too, but didn’t find anything. I’ll go over everything again.

I’m still learning the ‘nightlies’ but they have a ‘display net’ button which sure would come in handy here. Is it not in the stable version? How much we forget in a week. :wink:

1 Like

I don’t see that button… perhaps I should try nightly builds :slight_smile:

Have you started laying out the PCB yet? You get the same functionality there when routing.

I laid out some of it, but I haven’t set footprints on the particular module I am having issues with yet. I’ll try that tomorrow :slight_smile:

The image and text provided do not match my understanding of the ERC. As can be seen, I have created the same error, and the flag location is different from the original screen grab.

Folks… my bad. I went through everything again, and found that I had somehow connected the VCC on a shift register to GND. After fixing that, everything works like expected.

Difficult to find, but, no pain, no gain :smiley:

@Sprig: The difference might be due to the location of the PWR_FLAG in the schema ?

Well, as said earlier, you now have two power outputs connected together. I don’t think you need a power flag there. In the initial the power flag is connected ground and showing a conflict there. I’m guilty of glossing these things over but I’m not sure that one is needed for ground.

The reason a short is suspected is because the +5 shouldn’t be connected to the ground power flag. I’m working on very little sleep though so if I’m totally off base forgive me. I normally get to sleep at 4am. I have to get up in two days at 4am to catch a flight and I’m struggling to adjust my schedule. :wink:

EDIT. Heard the ding as I was typing. Should have checked. Rene got me on the right track in terms of thinking about the error. I’ll stick with my lack of sleep theory. :smiley: I’ll have to heart Rene’s post. V5 will make this easier when it comes out though.

I am somewhat sleep deprived too. That’s why I’m going to be right now :smiley:

Thanks for the input, helps the neurotransmitter device to focus.

1 Like

A little bit of tinkering with creating intentional errors goes a long way towards understanding errors not created on purpose.

Here is an example of a short from power to ground:

The text indicates that Pin 2 is connected to Pin 1 of BT1; this is clearly a short. The short is not at the battery, but was intentionally created at the left of the screen grab. The tricky part is that the arrow is not where the problem actually is on the schematic. The text is however, describing the issue perfectly.

Here is an example of two power outputs being tied together:

The text indicates there is a power flag attached to pin Pin1 of the battery; and there is.

Power flags are pins assigned as “Power output”. But any pin can be assigned as a “Power output” if it makes sense. A battery having it’s pins set as “Power output” is a good example; same for the output pin on a regulator.

The reason that pwr symbols are not set as “Power output” is so that they can be conveniently used to de-clutter the schematic:

As can be seen from above, the DRC will run just fine as long as there is one, and only one, “Power output” on a net.

I’m too far behind on the unintentional a the moment. :wink: