You can edit the sketch and use the convert entities feature, but be careful you don't set up a circular relation..
You can copy/paste a 2D sketch from the assembly to the part. (I don't think you can copy/paste a 3D sketch)
Basically, just select the sketch in the tree, hit CTRL + C.
Then go to your part, select a plane/planar surface to place it on and hit CTRL + V.
The only thing is:
INTERNAL references are kept, while EXTERNAL references are lost.
What I mean is this:
If you have an arc and a line inside the sketch and they are set tangent to each other, then the tangency will remain through the copy/paste.
However, if you have a line that is coincident to an edge on a part (i.e., not INSIDE the sketch), then that reference will be lost.
You can't directly move a sketch from an Assembly to a Part. In the case you posted, your sketch point is coincident with the Assembly origin, so why do you need to move it? Why not just delete the sketch and start a new one in the Part, with the same relation (although I'm having problems imagining why you need it at all)?
Q:) Why the need to move it? A:) Some features, like extrude, want that sketch in the part that is being extruded.
Q:) Why not delete it? A:) There are some of us who made the grievous sin against nature that is to spend (2) hours making a complicated sketch only to find out we defined it on the face of a part in the 'Assembly' and SW refuses to extrude it or anything because it needs to be with regards to the 'Part'. The reason we aren't quick to delete our old sketch and make a new one is an attempt to maintain some of our sanity.
How to get SW to acknowledge the sketch can be applied to a part? I think Dan Pihlaja has the best solution; copy the Sketch from the assembly (Ctrl+C); edit/open the part in question, and paste (Ctrl+V). The sketch should appear at the bottom of your feature-tree. Only catch is; yes, the 'location' of that sketch depends on where you (Ctrl+V) that sketch. If you paste it as soon as you edit the part, it may appear on a completely different plane then intended. You can move/rotate the sketch it into compliance (even redefine the target plane)... OR, you can select the desired face (i.e. the face you made the sketch with in the first place) and paste; this will at least place the sketch in a reasonable location w/ regards to your desired result. Remember, select the face you want to past the sketch to, don't just paste the sketch randomly within the part model.
but why would you need to???
if you know the sketch belongs to a part.....
just draw it in the part file???
I have have to:
I will use the model to cut bits away form a part, I will propagate the feature to the part
then go to the part, break the link and add new relations in the part file it self, and remove the feature from the model used to create the feature.
Not to sure but I think if you drag the sketch into the part in the feature tree it might work. you would also need to make sure the sketch plane is a part of the part though.