"Intersect" has the unfortunate dual use as a boolean function, as shown by Vance Wright above, but it is also the name of a SolidWorks feature. the Intersect feature is better when you have a lot of surface bodies and/or planes (with or without solids), and the Combine feature is better with a lot of solid bodies (without surfaces).
"Combine" is really a boolean function for add, subtract, intersect.
"Intersect" allows you to use planes, surface and solid bodies to divide solid bodies into regions, and you can select multiple regions. The result of both features is solid bodies. Intersect can do what Combine does, plus Cut With Surface and Surface Trim do.
In this Intersect feature below, a planar surface cuts one solid body intersects a second solid body. The output of this feature is two regions that become solid bodies.
In the below feature, 6 planar surfaces were used to create a single solid region, which is made into a solid body. The thing with Intersect is that it doesn't do anything you weren't able to do before, it just enables you to combine several features into one. This sometimes makes it complicated to visualize what's going on. You could do the same thing shown below with the Trim and Thicken commands, and a lot of face selecting.
One thing to consider is that Intersect would work even if solid bodies are not touching. So it will merge only what it can. Combine would fail if there is no surface contact between bodies.
None can address zero thickness situations for merging solid bodies.