import PCB components into KiCAD which are sold in the electronics industry
The Kicad philosophy is: There are components and there are footprints, and you need to match the component with the footprint. Why? Because the same component might be available in different footprints. AFAIK, all common footprints are already present in Kicad. Only footprints I have had to make were of heatsinks and connectors.

After you draw the schematic (and have run annotate), you have to run CvPCB. This will pull up the browser where you can select your footprints. Only after all components have been assigned footprints, should you create the netlist. Then start the board editor and import netlist. If some components do not have footprints assigned yet, the board editor will issue warnings when you import the netlist there. Go to the schema editor, and run CvPCB to fix that.

The issue with components and footprints also extends to the schematic editor. There are devices and there are components and you need to match the device to the components. e.g. there are 3 leg transistors, 4 leg transistors etc... and you need to match your part with the correct schematic, and then again match the correct footprint with that schematic. Only constraint is the number of pins on the schematic and footprint must match, and they must be numbered the same. You need to check that the numbering is in correct order. e.g. there are transistors with BCE, CBE, ECB... and all of them have pins numbered 123. You will need to make sure 1,2 and 3 correspond to the correct transistor leg. There is a footprint viewer from CvPCB, which will show you which pad corresponds to which pin number. The schematic editor already shows the pin number.

All this is unlike eagle, where footprints are hardcoded with the component. In Kicad, it is perfectly possible to assign a capacitor footprint to a diode, intentionally, or by mistake. Very flexible.

PS: CVPCB may need internet to run. There is a way to force it to use the already installed libraries. Open the settings from CvPCB, and change the KGithub to KISYSMOD. Hope you're using the latest version of Kicad.