[Excelmachine]

I have a Haas SL10 that I need help with for programming a shape I have never done before. What kind of tool do I need to use to prevent it from dragging on the back side. I was planning on drilling most of it out and then use some sort of boring bar. Can anyone point me in the right direction? The shape I am concerned about is the blue line. Thanks.

[Geof]

I have used corner radius endmills as a mini-boring bar to do similar internal hemispheres. You know the corner radius accurately so you can program using tool compensation to get an accurate hemisphere.

The only slightly tricky part is getting the corner of the milling cutter aligned on center.

EDIT
Forgot to mention you might have to grind the opposite cutting edge of the mill back to get clearance but this is quite simple.

[ken70ss396@yaho]

I machine this type of shape almost everyday. Rough it out with a drill as you planned.You can also remove most of the drill point shape with a ball endmill. Then use a smaller 2 flute ball endmill lined up on center to rough and finish the profile.Program the endmill as if it were a boring bar (put the full radius in the offset page radius as if it were an insert corner radius). When you program the profile make sure you put in the existing hole size. Also step thru the program away(Z+) from the Chuck and watch when the G40 turns off the cutter comp and retracts from the part.This will help you edit the program so the tool won't hit the back side.
I also bought and modified an O.D. grooving tool with the smallest Round insert I could find.It has a 1 inch reach and I removed much of the support blade so it clears the shape and on retract. It has a 1" shank and I have it set as a face groove tool in the turret. Works great for finish passes.Most of the hemispheres I machine do not have any straight bore to accurately measure the diameter, so I leave stock on the Z face and program a straight bore section that gets faced off later.Using tool wear I leave stock on the ID ,and with the straight section I can measure the ID and adjust the tool wear to get the correct ID size.
Hope this helps.

[Excelmachine]

Thanks guys for the replies. I was out sick so I didn't respond earlier. I chickened out and ended up making them real quick by doing them on the mill and 3d surfacing with an 1/8 endmill. But, with your 2 ideas, I feel more confident if we need more using your methods. Thanks again.

[Ydna]

a straight-flute ball endmill would be nice to have in this situation...hah