I hereby certify that I am not simply asking someone else to design a footprint for me.
I have assigned the selected foot print in schematic that I have placed and pre-positioned on the PCB, but when I try to save it…
‘RJ45_OST_PJ012-8P8CX_Vertical’ is not a valid library identifier format.
it clears the field waiting for a correct entry, but I selected this one and placed on the PCB?
Any thoughts,
VinceDent56
1). In the PCB Editor, place a resistor (Example, you already have something else).
2). Edit your part, and change the reference. The reference should end in a number. Every Reference Designator must end in a number in KiCad. If it does not end in a number then, KiCad adds a number.
3). Place a resistor in the schematic, and give it the same Reference Designator:
4). Schematic Editor / Tools / Update PCB from Schematic [F8] Make sure to turn on the option: Re-link footprints to schematic symbols based on their reference designators
At this point you have created the a link (in the form of an UUID) between the schematic symbol and the Footprint on the PCB. The last step is:
5). PCB Editor / Tools / Update Schematic from PCB This puts the footprint library location into the schematic. If I now look at the schematic symbol properties, the footprint field is filled in:
Note: In the Update Schematic from PCB step, the 4k5 value of the resistor in the schematic got overwritten and I had to fix that afterward.
The most important step was 4). where the Ref Des. is used to link the UUID’s of the schematic symbol and PCB Footprint to each other. Once that has been done the everything after that follows the normal design workflow.
In addition:
In KiCad, Footprints always come from libraries, and the library should always be named in the format [Library name]:[Footprint Name] and your identifier is missing the library name and the colon.
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.