Well, that could involve a pretty length response but here's a shortened synopsis:
Loads models are generally pretty coarse (1-element deep floor beams and frames, etc). They exist only for pulling loads. Loads in FEMs exist in the form of gridpoint forces and element forces.
For plate elements the element forces will be a linear force (force/length). Generally loads models are set to only report the averaged load for each plate element (again think force/length).
For bar elements the element force is just a force (lbs).
Grid point forces are the forces acting on a give node by the elements attached to that node. Therefore when pulling grid point forces you have to select the attached elements you're interested in.
The way you pull loads depends on what you want to do. If you just want to find a load for a crippling calc in a chord (and if the loads model is a good representation of the real configuration) you could probably just pull the element force for the bar element.
Often you want the internal loads acting on a given section of a beam. In this case you would make a "cut" and pull the grid point forces for the elements on one side of the cut. This will give you the internal loads (axial, shear, moment) acting on a given portion of a beam for subsequent calcs (buckling due to combined shear and moment loads, etc).
Not sure how far this will get you. Like I mentioned, you could spend a great deal of time fully explaining this topic. If you're familiar with Nastran I'd suggest running some simple models, requesting grid point forces and element forces in the *.f06 output, and trying to freebody/trace why they loads are what they are. Just make sure you only request element force output at the center of the element or you'll get a bunch of element force outputs for each element.
