Start with a copy of LTspiceIV\lib\sym\Misc\DIP8.asy, which is the symbol for a generic 8 pin DIP laid out to match the physical pinout. Save it as MC33063.asy in your LTspice working directory.
Open the model .lib file and find where the pin order is described:
.SUBCKT MC33063 swc swe ct 90 2 vdd isns drc
* SW-col SW-em Ct gnd cinv vdd isns drive col
consult the datasheet for the pinout and match them to the pin order.
Yippee!!
they are already in the correct order for the symbol so you don't have to go through reordering them.
For each pin on the symbol, right click it and edit the name to add a brief abbreviation to the existing number with a space in between. Right click the <Value> below the symbol and change the text to
MC33063 (because there's only one model for both chips).
Next open the Symbol Attributes Editor dialog (menu: Edit: Attributes: Edit Attributes), DO NOT enter anything on the SpiceModel line, and enter the name (with extension, but without path) of the file containing the model on the ModelFile line. You should also put something meaningful on the Description line as this will be shown in the component browser.
Save it and you should have a usable symbol.
However that's all moot because the
OnSemi MC33063 subcircuit model uses the ? ternery operator which LTspice doesn't support, so if you dont want to have to wade through the model translating it line by line, you'd do better to find a model in native LTspice syntax. e.g.
https://www.eevblog.com/forum/beginners/simulate-mc34063-on-ltspice/