Lathe, cut concave hemishphere in face.

[Andy]

So,

I need to cut a concave hemisphere in the face of a block of cast iron in the lathe.

Dia=3.000

Depth=1.5

The tool is the question.

Need a boring bar with an insert that does the whole job.

Turns out the only tool that seems to work would be a bar with a round insert located in the correct position at the end of the bar.

Most insert configurations dont seem to suit it well: like cpgm or tpg or vnmg. (clearance problems).

However I cannot find a bar with a round insert.

We will make one if necessary.

By the way, we used the facing outside in for the maching Op in MC. and it looks good. (using a round insert custom created bar)

 

Anyone know about the bar, or if the Op sounds ok?

Thanks

[McRae]

Sounds like you need a spherical boring tool, not just a boring bar. What I would use is a Millstar style indexable ball nose for this. Align the flat of the insert and set the job up.

 

Good luck on this, let us know how it went.

[Nominal]

I just did this last week. Although my part was smaller in dia, it was checked over a ball bearing which hit a target point +-.003. It was a conical surface in the face of the part with a spherical surface at the vertex of the cone. I used a full radius face groove. Just had to hand grind clearance on the insert.

[chris m]

Andy

 

Can I ask why one boring bar has to do the whole job? I would drill a 3/4" or 1" hole as far down as I could get away with with a UDrill or spade and bore all the stock out of the way first; then whittle away with a profiling bar or internal facegrooving tool of some kind to finish it off.

 

Give your Circle, Sandvik, or KM guys a call; I think they should have something (esp Circle 1-800-247-2533)

[Surface]

I'm not a lathe guy, but why couldn't you use a ball endmill, 2 flute. I realize the helix of the fultes will slightly change the radius when the tool is held in a stationary holder, but I can't believe it would be more than a couple thousanths.

[McRae]

quote:

---

but why couldn't you use a ball endmill, 2 flute

---

Is there an ECHO in here?? What are you man, a manager??

[Surface]

Andrew, I didn't mean to echo your suggestion, but to offer an alternative.

Quote "need to cut a" and "A" being the optimal word, means to cut one. The tool you suggest, may be a better tool for the job, but costs 4 times the price.

Perhaps Millstar is cheaper in Canada, if so I apologize.

[Andy]

We actually thought to use a ball end mill, but this is a one off, and the piece going in the chuck is already worth abou $900 and I would rather not experiment. The ball face groove tool sounds pretty good I will look into getting one.

The reason we want to use one tool is, set up is simpler, less ops, less chances for errors, and we dont care how long it takes to cut. In production we would definitely rough the stock out first.

[Mick]

I had to do something similar a while ago. As per a previous suggestion, I u-drilled, then whittled away with a profiling boring bar. I used a Sandvik SVQBR (VBMT insert on an angle).

Worked a treat.

[McRae]

quote:

---

Andrew, I didn't mean to echo your suggestion,

---

Surf,

 

I forgot no one can see me smile as I am typing - and by the way, that stuff is expensive where ever you buy it.

[Noel]

Couldn't you drill a hole say 1.5" dia as deep as you can.Then semi finish the front section.Then pick out the deepest part using a profiling boring bar with a 35 deg insert with 17.5 deg nose angle clearance. Then finish with the same bar.With a radius that big back clearace shouldn't be a problem,if it is we usualy clear the back of the bar a bit.

Noel

[chris m]

Speaking of echoes...

[Noel]

I guess I could have just put +1

 

 

Noel

[chris m]

quote:

---

the piece going in the chuck is already worth about $900 and I would rather not experiment

---

Let me then suggest putting a piece of stock worth $20 in the chuck first; at least you won't need to sweat boning your $$ piece first time out as this is definitely somewhat of an experimental process.

 

C

[Andy]

Good thinking Chris, We were going to do that as a matter of fact I just was dead brained when I answered. I guess what I have learned in this thread that the essental answer is to use a bore bar with a vnmg insert oriented the appropriate way and we will be able to take the finish pass in one continuous cut, which is really what I was asking. I actually found one in the MSC Catalogue, page 762 I think. Looks like it will be perfect. Ordered this morning.

Thanks all,

Andy

 

[ 05-07-2003, 08:14 PM: Message edited by: Andy ]

[McRae]

Remeber with a spherical cut, think in 3D and consider the clearance on the front of the tool as well. There may be enough clearance with a "V" and "B" at 11 degrees may be enough clearance. Draw it out just to make sure.

[Andy]

Thanks Andrew,

Yes, we did that, on a piece of paper, should be no problem.

Andy

[McRae]

quote:

---

Yes, we did that, on a piece of paper, should be no problem.

---

i had to smile when I read this. There was one time with the rotary axis toolpath that I thought I would be OK - On paper, only to see that I was wrong. The best part about it though, the tool will only rub once...

 

Is the bottom of the whole closed or is there a little thru hole?

[Noel]

Nothing wrong with bluing in the cutter is there?

 

 

Noel

[mmonica]

We just finished a job with a R2.0" +.002/-.001 sphere, we used a T-MAX drill to rough has much has possible. Finished with a Valenite BHP-EC-600 boring bar with a VNFM-332 insert, worked like a charm. Note: the customer allowed a small drill point at X0.

[Andy]

Andrew,

no, the bottom of the sphere has no hole.

However we can leave a little nipple and hand finsh later. I know not to go past x0.

 

Nmonica,

We just received the same bor bar from MSC. Great looking tool. I think it will be perfect.

 

Andy

 

[ 05-09-2003, 11:37 PM: Message edited by: Andy ]

[Andy]

Andrew,

Also, yes, I did cad the tool and contour side view to check the front clearance and had plenty of clearance.

[chris m]

Andy, you should be able to go to center and a little below on the last pass to clean that up; it'll just chip the insert.

 

Let us know how you make out

[monarch]

Andy, First make a boring bar from a nail, heat treat in a cyanide bath and spin the chuck by hand while holding nail-boring bar with large toe (as done in India). I have a part just like this on my bench right now ! Thanks great job ! Larry

[Andy]

Larry,

Actually, that is what I finally did. But I wore gloves. Are you wearing gloves??? Or is it too late?

Sympathetically,

Andy