Problem with the footprint or Symbol of the relay

Hello to all:

I’m doing this circuit with a relay:

I finished the skematic and checked electrical rules and i don’t get any errors.

After i performed the footprint assignement and for the relay i used the part “RelayTHT: Relay_SPDT_SANYOU_SRDSeries_Form_C” from the library (i supposse to i am using the default ones

After i performed the generation of NetList without any problem

After in Pcbnew i perform the import of the NetList

But i get these errors:

Error: Symbol K1 pad A2 not found in footprint Relay_THT:Relay_SPDT_SANYOU_SRD_Series_Form_C.
Error: Symbol K1 pad 14 not found in footprint Relay_THT:Relay_SPDT_SANYOU_SRD_Series_Form_C.
Error: Symbol K1 pad 11 not found in footprint Relay_THT:Relay_SPDT_SANYOU_SRD_Series_Form_C.
Error: Symbol K1 pad 12 not found in footprint Relay_THT:Relay_SPDT_SANYOU_SRD_Series_Form_C.
Error: Symbol K1 pad A1 not found in footprint Relay_THT:Relay_SPDT_SANYOU_SRD_Series_Form

Here is the image

And i can’t perform the routing in the PCB

Thank you and sorry for the english

I am thinking that to get a good answer from someone on this forum, it might be best if you zipped and posted your project FOLDER including sch and pcb files? It sounds like the pin numbers on your symbol may not correspond to pin numbers on the footprint.

Sorry I can’t attach files because i am new user

Edit the pads in the relay footprint to match the schematic. A1, A2, etc are standard identifiers on industrial relays. The schematic symbol probably has 1,2,3, etc.

Hello and thank you for the answer:

But this is the symbol that i’m using i couldn’t change the identifiers in the symbol neither in the footprint

In PCBnew click on the pad to select it.
Press E to edit the pad.

The other thing…maybe you are trying to edit the KiCad standard library. I think that such action is normally blocked. It is also a bad idea because a software update is likely to overwrite it. If you are going to continue with KiCad you ought to have your own libraries for all of those non-standard parts. Put the folder in a location which is convenient for your use and backup. FYI I sometimes start with parts from the standard libraries but I always customize and save them in my own libraries.

See Creating a new symbol library and a new symbol in KiCad 5

The file is read only i can’t edit it

Can i copy a the existing one and edit it?

Your LED D2 is the wrong way around and will never light up. Also when you’ve fixed that 220 ohms will allow about 40+ mA through the LED which is far too much.

1 Like

I am using a 5.99 version which is somewhat different. But I think you can open a symbol and save your own version into your own folder for custom symbols. You could also do a copy of the whole folder if you want to do so.

It is too much for many indicator LEDs but if you want to dimly light the room when the relay is energized it might work with the right LED.

Very true. That reverse connection of the LED might destroy the LED. FYI: D1 is there to clamp inductive spikes generated by the relay coil when Q1 turns off. The purpose of D1 is to protect Q1 from these spikes. Without D1, the turnoff spike could subject Q1 to overvoltage stress.


Generating a separate netlist, and then importing it in Pcbnew is deprecated (But is still taught in old tutorials). Since KiCad V5 (2018 or so) the recommended method is: Eeschema / Tools / Update PCB from Schematic.


These error messages literally mean what is written.
You have a schematic symbol with RefDes “K1” (Your Relay) and it has a pad with the name “A2”.

You have matched that schematic symbol with the footprint: Relay_THT:Relay_SPDT_SANYOU_SRD_Series_Form_C.

And that footprint does not have a pin with the name “A2”. As you can see from the footprint, the relay coil is connected to pins 2 and 5.

This means you either have to change the schematic symbol, or the relay Footprint.

In KiCad all default libraries are read-only (for good reasons), and normally you first make a copy of either the schematic symbol or the footprint into a custom (Project specific) library and then edit it.
However, KiCad makes copies of the library symbols and embeds then into the PCB file. As a result you can first draw the schematic, load the Footprints and Netlist into PCB, and then hover over a footprint of your Relay in Pcbnew and press [Ctrl + e] to edit it in the footprint editor. Then rename pads 2 and 5 to A1 and A2, and then save the changes directly back into Pcbnew (Just close the Footprint Editor, and it asks you if you want to save it).

Also, make sure that this footprint matches the relay you are actually going to use. Hopefully you did and you can ignore me, but relays have no standardized footprint.

Indeed, check it all.
The pin numbers for the switch for example also do not match.
There are probably 1000’s of different relays, maybe simeday the’ll all be in KiCad’s libraries…

Two 1/2 years ago I made a mini tutorial for a simple method for test fitting footprints in KiCad:

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