If you are doing a Z level profile with a ball or bull nose tool it does not keep the radius of the tool in consideration.
For example if you 3d a .020 radius with a 1/4 bull nose with a .060 radius the Z level operation needs to go .080 deep in order to completely machine the feature. But if you just select the face and generate it only goes .020 deep...
Can you show a picture of the situation?
If it is the case below, the automatic cut levels will set the range bottom at the lowest point of the cut area. You should set "Cut Below Last Range" to the tool corner radius (.060).
Yes it is this case.
My programmer in training cut a couple parts where he did not offset for the radius.... my question is why doesn't NX automatically default the corner radius to "cut below last range".
The only time you wouldn't was if you were intentionally not trying to machine the part or if you were trying to avoid something....
The standard care should be to fully machine the whole part.
The reason I prefer it the way it is, is because when I pick a floor with an open side I wouldn't want the tool to roll over the edges to the top of the tool's corner radius without me specifically telling it to. I think Surface Area or Streamline drive methods in a Fixed Contour operation would be a better approach for what you are doing.
The planar and face based processors approach this situation differently.
The Z-level and Cavity Milling processors are based on making planar cuts at a range of cut levels. First the levels are defined, then at each level we create a cut region where the tool touches the part at that level. That's why in ZL and CM, you need to set the levels first - in this case extending below the cut area.
If you use a surface controuing method on the same cut area, we start with tool contact points all across the cut area, and from there we calculate a tool path. So if you used area milling or stramline, and selected the entire cut area, the tool would cut it completely.