I’m trying to fix up an existing KiCad project as part of trying to learn KiCad (been meaning to for some time and this was as good a reason as any to dig in) and also trying to get a small batch of the hardware defined in the KiCad project made. So naturally I wanted to make sure there were no errors from missing symbols, changes in versions and so on… I write software for a living so I know how it goes, changes between versions and that sort of thing. But other than finishing going through the symbols and making sure I switch to the default library or add specific symbols from an EDA library source like SnapEDA (like the Ferrite Beads) … I’m still stuck with a few ERC errors I just don’t understand. I’ve been wading through the bug tracker and forums and after several frustrating and confusing hours I just want to ask what the established wisdom about fixing these is. I’ve learned a bunch and fixed 6 other ERC errors before I got stuck on these ones.
It would be super helpful anyone offering advice on how to fix these ERC errors can explain why the fix works… because I’m dealing with an existing design that I am reasonably sure was actually sent to production I don’t really understand how I have these errors other than…
A: They never bothered to run the ERC before paying for a prototype batch ( is this normal? ) or
I uploaded an archive of the project in the original post to let anyone open it in nightly and check, but for anyone not looking at nightly. Heres the schematic Schematic.pdf (220.5 KB) and the ERC errors are as follows.
Text Version:
Pins of type Power output and Power output are connected
Symbol U2 [SPX3819M5-L-3-3] Pin 5 [OUT, Power output, Line]
Symbol U3 [FT200XD] Pin 3 [3V3OUT, Power output, Line]
Input Power pin not driven by any Output Power pins
Symbol U2 [SPX3819M5-L-3-3] Pin 2 [GND, Power input, Line]
I just had a look at it, and I’m surprised by the amount of time you claim to have spent on this.
The first ERC error:
[pin_to_pin]: Pins of type Power output and Power output are connected
; Severity: error
@(128.27 mm, 31.75 mm): Symbol U2 [SPX3819M5-L-3-3] Pin 5 [OUT, Power output, Line]
@(233.68 mm, 201.93 mm): Symbol U3 [FT200XD] Pin 3 [3V3OUT, Power output, Line]
If you look at the datasheets of U2 ( A voltage regulator) and U3 (Some weird chip that also has a built-in voltage regulator) then it clearly shows that you connected the outputs of two different voltage regulators to each other. That’s not going to work properly. (I did not read the datasheet on how the voltage regulator in U3 is supposed to be used)
The second error:
[power_pin_not_driven]: Input Power pin not driven by any Output Power pins
This is the a common problem caused by a missing PWR_FLAG on the GND net.
You have used a PWR_FLAG on the input of U2. The GND net also needs a PWR Flag.
Something like this works:
Or make something similar that looks better
I have a habit on putting the PWR_FLAG symbols close to the connector that serves as the power input.
Another small (and mostly cosmetic) thing. You have a “stray wire” on the GND pin of U2.
I looked at FT200XD and in pin3 description: “When VCC is 3V3; pin 3 is an input pin and should be
connected to pin 4.” So connection of this pin to VCC = 3V3 is simply OK.
My way of dealing with ERC errors is to not run ERC ever
Which makes it more likely that either the person who made that schematic symbol used it in another configuration, or (like me) did not read the datasheet properly and assigned the wrong pin type.
