Cannot connect power pins

I just started l;earning KiCad. I created a new project, and a new schematic. I placed one component (24AA02 from memory.lib). I then placed the GND and VCC power symbols, and connected them to the respective pins on the IC. I made all other pins no-connect. I am using only components that came with KiCad.

I then ran the Automatic Annotation. Now, when I run the Electrical Rules Checker, I get the following error:

ErrType(3): Pin conected to some others pins but no pin to drive it
@(5.600 in,3.850in): Pin 4 (power input) of component U101 is not driven (Net 5).

I followed all of the tutorials I could find, and read all of the docs I could download.

What am I doing wrong?

Thank you,

The reason for this erc error is that the power pins have the electrical type power input.
A power input pin needs to be connected to a power output pin. (In other words you need to have a supply for your pcb.)

Most pcbs are supplied with connectors. Connectors have the pin type passive because you do not know what the connector symbol will be used for. For this reason there is the so called power flag. This symbol is for telling erc where the power for your pcb comes from. (It has the electrical type power output.)

So if you supply your pcb with a connector, place a power flag once per potential. (One for the gnd, one for vcc, …) If you have a passive component in series to the connector (examples: fuse, filter elements, …) you need to place the power flag after this component.

If you have a dc/dc converter on your pcb than the symbol for this dc/dc converter should have the pin type power output. But again if you have some passive element in series you need the power flag after this element.

The power symbol is only a global label. All nets connected to the same power symbol are connected. But the power symbol is not a power source.

This turned into a big argument on IRC a month or so ago when someone really wanted it to be… :stuck_out_tongue:

They can not be both a label and a power source. One can not have more than one power source per net.

Well yeah, I get it :wink:

(okay we should probably stop derailing now. I won’t reply any more)

Thank you for your reply. I tried the Power Flag and this removed the errors. I understand the concept, but I don’t see the need for it. I have used many other electrical cad packages (lately Eagle) which do not care about power in or power out. That is a concept that is necessary for electrical simulation packages, rather than schematic capture. I have never before seen a schematic that includes these funny power flag symbols, and I have been reading and creating schematics since before it was done on computers.

Nevertheless, I will abide by the KiCad rules and hope that my clients don’t question these new symbols.

Thank you all,

ERC electrical design warnings don’t affect the PCB. What is important in ERC is avoiding accidental unconnected pins

I’ve read different reasons why the power flag symbols are needed. The following is my understanding.

They are needed for the ERC to work. The WHY of that is because when drawing a complex schematic, it is common to use the power symbols symilar to using GND symbols. If there is more then one power symbol placed, then the ERC has to allow for them all to be inputs; otherwise the ERC is finding there are at least two different outputs tied together.

So, if my understanding is correct, then it this is actually a GREAT feature that KiCad has to ensure the ERC can find the majority of problems.

Also, once the ERC runs on a schematic, the flag symbols can be deleted if the ERC will never be run again. They do NOT have to remain on a finished schematic.

Maybe the Power Flags should be visible only when viewing the schematic, but not when printing. Is there already such a feature in KiCad where you can create things that will not print? I know that there are invisible power pins.

On another subject, I read that there is a FreeRouter but it seems to have been discontinued. What is the status of auto routing for KiCad?

Thank you,

The power flag is not only for the drc check but also for the human viewer. It makes the intentions of the designer more clear. In other words it communicates with the reader of the schematic where the supply of this pcb comes from. For this reason i would want it to be printed. (but your preferences may differ.)

I do not know how do hide symbols when printing. You could just ignore the erc warning. (Again bad practice.)

If you need to start a sentence this way, it might be better to open a new topic. (Nearly all users only read the “headline” and decide based on that if they can/want to help the owner of the topic.)

Search the forum for freerouter or auto router. If you are not satisfied with the topics that come up this way ask a new question. (This way this topic stays clean and you have a higher chance of getting the attention of people who know this stuff.)