Hello!
I am running the erc check, and I get about 200 errors / warnings.
However, most of them should be ignored.
Reason to ignore them: I am using an FPGA board, and I don’t use
all the pins of all the connectors. So on the extension board I’m making, there are many errors and warnings.
It would be very handy to have a checkbox (for example) to disable any particular error and warning individually. Is this possible? Is there a setting for this feature?
What I do now is creating a report and process them 1 by 1. But it’s a lengthy process, and if I change
anything to the schematic, I have to redo it from scratch.
Any idea?
Thanks,
Pascal
I’ve seen this somewhere in the past but probably other software. There is a little ‘x’ in the right hand tool bar that is a no connect symbol. That should help some for now. It is probably a better method for unconnected pins than ignoring them in the list.
2 Likes
Hello!
Thanks for your reply. Yes, I’m aware of the cross for unused pins. I’m using it already.
But the problem is a little bit different.
In the following picture, connector K3 is the connector from a FPGA board. Anyway it’s a connector, and therefore cannot be defined for any possible application. All the pins are declared as input in the library. For instance, signals POTS_CLK is an output from the FPGA, and therefore it generates an error, that POTS_CLK has no driver. As I know it’s not an error, I would like to disable this particular error. The cross doesn’t solve it because in this case I couldn’t wire anything to it. I was thinking something like in Eagle, which allows to “acknowledge” an error, or something like that.
How can I solve this?
Thanks,
Pascal
as it is a connector, I would edit the symbol to have all the pins of the connector as “passive” Unless you want to manually specify what are outputs / inputs (helpful on larger projects where you can get things flipped)
1 Like
Hello!
Thanks for your reply.
It works! By the way, why passive and not unspecified?
Addendum: I have another problem with the errors.
On some power lines (or ground), I get an error, on some other no error. See pictures.
It says pin xxx of component ICxxx not driven.
Although there are no boxes at the end of the pin and wires, I tried to move it with G command, just in case it’s not connected. But it is actually connected.
Any hint?
Pascal
Try checking the pinconfiguration in the symbol librarie.
Maybe you have missconfigured the higlighted ones. Happens often enough to me…
the GND one is because you need to have a power flag for ground aswell, there is nothing special about ground in kicad, its treated just like any other circuit
The passive vs unspecified is more a personal preference on my part, a connector is a passive connection, so it falls under the most correct if you are not going to define it.
for the AVDD I assume it goes through an LC filter, so power flag needed after the inductor to tell kicad that it has power
Unspecified always throws an error and should only be used if you want generic symbol “templates” for configurable pins of a part where you want to force the user to derive a project specific symbol.
Check out the ERC matrix:
You can see an unspecified pin connected to any other type of pin will generate a warning. You can change this matrix by clicking on the boxes. Each click will cycle through “OK”, “Warning”, and “Error”. If you really mess up your matrix you can click the “Reset to Defaults” button and get back to how my screenshot is setup. (I’ve not personally played with this matrix so I don’t know how persistent changes are.)
2 Likes
Just because you can does not mean you should. And a few errors (like the pin not driven error) are not part of this matrix.
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.