Yes, if you mean the regenerate button, I regenerated it several times. I also tried a complete PC shutdown and reboot. None of that made a difference.
Note that Regenerate in assembly regenerates the Assembly only. This may seem obvious but it refreshes only assembly-specific things, like constraints, patterns, etc. It does not go into each part and regenerate individual components. However, since interdesign relations are part of assembly definitions, it will update those within parts as needed. Just something to keep in mind.
You are definitely dealing with an interdesign relationship here. This happens when you design a new part within the assembly and insodoing you reference an existing part in some way, typically by:
1) Projecting some edge of another part into a sketch of the new part and check on Maintain Association
2) Sketch directly on a flat face of another part
3) Create reference geometry in your new part using another part's geometry or reference geometry as an input. For example, as the center of a circular pattern you click a cylindrical face of another part.
Etc. The common theme here is that you're using a persistent reference of another part in your new part.
Generally speaking this behavior can be useful or maddening depending on your intent. The most unpredictable part (if you don't know what's happening) occurs when you move components in the assembly. If you sketch on a part's XY plane and extrude ToGeometry and you pick the face of another part in the assembly, it will work. And if you then move your new part away, it still going "ToGeometry" and will make the extrusion longer because it doesn't care how long it is, only that it goes all the way to the target.
The same is true when projecting edges / faces of Part A into the sketch of Part B and enabling Maintain Associativity. And many other examples.
When in doubt, and especially if you have decided "I never want to mess with these types of things", look at the Interdesign Relations node in the Assembly Explorer from time to time. If you do any of these actions listed above, a new subnode will appear. You can right-click them and delete them. Typically this will stop whatever behavior you are finding unpredictable.
To avoid getting into this scenario, if in fact you do intend not to, try:
1) Always sketching on the core planes, versus plopping your first sketch on the flat face of another part. You will then likely have to position it through 3D constraints, but will avoid interdesign relations.
2) If you project, disable maintain associativity. Instead, consider using Global Parameters. For example, if you have 20 plates that fit on top of eachother and they all have a 1" hole 2.5" apart, make a global parameter called "HoleDiameter" and "Hole Offset" and you can reference those in each sketch of each part.
3) Take care when defining inputs in general, for example the center of a circular pattern or the direction of a linear feature pattern. If those inputs to that kind of thing belong to other parts, an interdesign relation is made.