Good video, thank you for taking the time to record and upload it!
Couple notes though... in layout, you select the parts, the ^C to copy. You get a crosshair which is asking you for the "reference point" for the copy, and you can easily snap to the exact center of a pad or end of a line or, as you did, any arbitrary point. Then when you use ^V the paste center will be that point you selected when copying. This makes it VERY easy to offset pins or perform precise positioning relative to some point. You can also save a LOT of hassle by using the "paste array" when designing the footprints for ICs. The Wizard is the absolute fastest, but using the origin marker with copy/paste and using paste array go a long way in making footprint creation easier.
You may also want to make sure the silkscreen widths are compatible with your board house; I tend to make all my silkscreen line widths 4-5mil which works great with most PCB houses, including Hackvana, my favourite board house. I'm a little concerned about how you specify your soldermask expansion to zero; I tend to leave it at defaults which tend to give good results. I don't like soldermask defined pads, which is essentially what you've done by setting the expansion to zero. Some very fine pitch components want this (and others do not) but for the types of components in your video I don't see any clear advantage to this. Having the silkscreen butting right up to the bare copper can also cause problems with placement and reflow.
I also am not a fan of the schematic pin order being the package pin order. The schematic is the logical representation of the circuit; if it makes sense to have the logical and physical pins in the same location that's great, but I tend to organize my part's schematic object so that the pins yield to easy schematic "flow". i.e. my power and ground pins are grouped together and (when possible) offset by the amount of space that a capacitor symbol takes, that my enables or other inputs are on one side of the component and outputs on the other, etc.
You tend to also shift pads around manually; I like to double-click on the pin and explicitly set the x/y location based on the datasheet. This can get very frustrating, particularly if the datasheet mechanical dimensioning requires you to go through a lot of mathematical gymnastics to arrive at the correct dimension. It does pay off though by ensuring the footprint will match the part. This is helped a lot if the center of your footprint is at (0,0) too, because all the pin dimensions tend to be centered on the origin. You also seem to deviate from the recommended PCB footprint for unexplained reasons. My experience has shown that their recommended footprint often gives you the best mechanical connection and you should only deviate from it if there is a very good reason to do so. This is particularly important for fine-featured parts where they have specific soldermask or pad dimensions to ensure high reliability during assembly.
I've recently fallen in love with the 3D footprint feature. A LOT of vendors are providing IGES or STEP files of their components. This is particularly awesome when the datasheet has incomplete or missing footprint recommendations. You can use the 3D file to instantly tell if the part and footprint are compatible.
One final note/suggestion... if you move the footprints and schematic symbols so that the center is aligned with the center of the grid you will find that rotating and flipping the component works much better, in that it won't "jump" in annoying ways.
I'm looking forward to the layout tutorial. :-)