Given the design intent is generally dependent on the engagement of a mating part if is is not tapped, industry practice dictates that the depth dimension provided is to the body diameter, never the point. There are rare exceptions to this, as in cases where the part may have a near intersecting hole where the drilled hole potentially could either penetrate the existing hole, or create a small "thin" spot that may not support the pressure of the system, if any. Downhole, the pressures can be several thousand PSI, so it can be important. VERY important.
Consider the difference between a 118° and a 135° drill point in terms of distance from the end of the drill (the point) and the body diameter. Naturally, the larger the drill, the more difference there is between the two. Throw in the fact that many of us hand sharpen drills and don't particularly care if it is exactly either, as long as it cuts on size. The draftsman cannot know what drill will be used, and shouldn't have to care. His interests are in mating part fits or threading depths. I have always been told that they do make an assumption that a 118° drill is used.
If things are extra tight on getting the required tapped depth, given the drilled depth, I have taken a flat bottomed drill and done away with any conical section, thus preserving any wall thickness designed, but gaining a little on available tapable hole depth. Some engineers understand and sympathize and have no problem with this practice, but typically young, green engineers are so smart they believe you can tap a hole 2 turns past the bottom of the hole without a problem and think you are pointing out a mistake they made and don't like it.
On older drawings, I have seen noted DP for "Drill Point" where the absolute maximum depth is critical, as mentioned above, as opposed to dp, which simply means "deep", which means depth at body diameter. These days, with GD&T, the symbols used take the guesswork out of it......you just have to look one up now and then if it's an odd or unusual one.
RJ brings up a good point. It's not unheard of to see only the thread depth specified, with the hole depth more or less left up to the operator. Of course, there are limits to this. I doubt many customers would accept a plate full of holes drilled thru when they only needed to be tapped 25% of thickness. I have never let an engineer off the hook on that. I make them give me some kind of number. It is standard to provide a max drill depth if nothing else, and the machinist should hope the engineer is generous enough not to make it unnecessarily difficult to tap to the required depth. My rule of thumb in design work, where there is room, is to spec the drill depth equal to the major diameter x 1.5 + the required thread depth. Rarely is there a need for a bottoming tap that way.