like the title said i directly used footprint from the library in schematic I didn’t change any names I may have rearranged the pin position but that to in USB . i didn’t do any changes to this jst connector but why is this showing this error.
Please show the footprint assigned with J1. Looks like the pins are named differently for that footprint.
All your errors are of the same form, so let’s pick one:
Error: J1 pad S2 not found in Connector_USB:USB_C_Receptacle_HRO_TYPE-C-31-M-12
J1 is the USB connector on the schematic, and it has a pin with the pin number S2 which is one of the 4 shield pins. (Yes “pin numbers” can have letters too, but don’t confuse them with pin names). KiCad is telling you that it can not find this S2 pin in the footprint. If I open that footprint in the footprint editor I see:
It does have 4 shield pins, but they all have the pin numbers S1. And this is OK in KiCad. It just means that whatever is connected to the S1 pin in the schematic, gets connected to all those S1 pins on the footprint.
You also made another mistake here. According to the USB standard, the shield must always be connected to GND.
The other ERC violations are very similar. There is no pad i the footprint with the number “A1_B12” (Hmm, I thought there was a 4 character limit for pin numbers)
The schematic symbol you used is apparently not a standard symbol, or maybe it is from an old library. What KiCad version are you using? (and what library version?)
Looking in KiCad’s symbol library I see a USB_C_Receptacle_USB2.0_14P that has all the right pin numbers to fix this connector (receptacle)
