Please say what version of ANSYS you are running because they make minor changes to terminology over time.

1) ANSYS Help has a Chapter in the Mechanical APDL, Contact Technology Guide, Chapter 3.9.4 that explains a lot about Contact Stiffness.

2) When two bodies make contact, the solver must create an equal and opposite force to prevent penetration, but what direction should that force be applied? Consider a 2D case of a flat face on one side of the contact pair and two facets on the other side of the contact pair. A single node on one element is touching the face of the element on the other side. If the blue body is defining the nodal normal, you will get the blue direction of force for both bodies, which is what you want. If the orange body is defining the nodal normal, you will get the center orange direction, which is the average of the two orange face normals. That is not what you want. You can flip between the tilted force direction and the vertical force direction for the normal component of the contact force (have not considered friction here) by flipping which body is the Target and which body is the Contact side of the pair, or by flipping the Nodal Normal selection.

Now if there was no vertex with a sharp angle, and instead a rounded body that made tangent contact, then the two arrows point in the same direction.  The lesson here is to use smooth surfaces to make contact. Your geometry seems to have a lot of facets. That is going to make the results change as you change contact definitions. I recommend you create smooth surfaces in the geometry editor.

3) Offset does a geometric offset of the surface.  Adjust to Touch translates the contact surface in X, Y and Z in a direction to close the gap. These are different. The best option is to have smooth surfaces in CAD that are initially tangent and don't use any Geometric modifications. However, after meshing, you will get facets again. The best practice is to use small elements in the contact area to minimize facet angles on what was a smooth surface.