When creating features, they are almost always based on planar sketches, so you need a face or plane to create the sketch on. I am not sure where you would expect to create a sketch on that cylindrical face, what shape the sketch would be, and what feature you planned to use to create the slot.
There are a number of ways to create this feature. Here are just a couple of the most straightforward examples:
Cut Extrusion with From Offset
Sketch a circle on the end face, then make a cut extrusion with the "From" set to an offset distance and then define the thickness of the slot you want to create using Direction 1. In the image below, only the yellow portion will be cut away:
Sketch a cross-section with a centerline on a plane that goes down the middle of the large circular hole and then do a revolve cut. Notice I haven't made the sketch profile exactly coincident with the inside face of the large circular hole; it is always good practice to avoid coincident faces like that and there is no harm in making the "cutting tool" larger than the geometry that will actually be removed. In fact, I could have just had that rectangle meet the centerline and it would produce a full thin disk, just like the geometry the extrude above creates to cut with.
Extrude Cut on Offset Plane
Create an plane offset from the end face to be in the middle of the part where you want the cut. Then create a circle and do a cut extrude with it. This is the same approach as the first example, but using a pre-constructed plane instead of using the From, Offset option in the extrude. Users often forget there is that Offset option in the extrude so would instead use this type of method.
I hope it helps,
Thanks Jim! This is an exercise in prepping for the CSWA exam that I was having trouble with. No actual use for the object.
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