TL2 large hole question

I have a customer that would like me to quote 2" holes +-1/32 in 3.25" thick AISI 4620 CRS. The apparent HP requirement for insert cutters is about 30HP and 250 lbs torque which is way beyond the lathe. But when I look at how fast they are cutting this I am thinking not trying to cut 5" per minute should drop the HP requirement down a lot. Who has practical experience here with something like this that can suggest best practices?

My other alternative is to use something like a Hi Pos cutter from Ingersoll and do this on the mill which is a VF4 30HP direct drive.

Any thoughts? 410 of these bigol things

Use an annular cutter. Go in from both sides if necessary. Finish with a boring bar. I have a TL-2. For my small situation I like it a lot..

Andy

We have a TL-1, usually drill to 1-1/4 with Allied Machine TA Drill, .001 Feed max then bore the rest of the way.

Basic rule of thumb;
A U-drill take 10Hp per inch of diameter.

But you can play with the numbers quite a lot depending on the geometry;
You can use sharper inserts (LM geometry from Sandvik) and ease up on the feed;
A 2" 880 drill @ 375SFM gives about 720 RPM
Feed for the LM, you can go down to 0.004 / rev or so; I like to use 4044 grade on the periphery insert.

Comes to about 2.81 IPM; so drilling out a hole should be done in about 1 min 15 seconds.

Calculations make this 9.2 HP needed with about 800lb of Z axis force

You TL-2 should have 12HP and a max Z thrust of 1940 lbs

Fine on both parameters.
You'll need about 10 GPM through the drill.

My only concern is on shank size interface with how your are set-up on your turret.
Thant can always be addressed...
Cheers!
Fred

Thanks Fred, this is the info I may have needed. I talked to the local Sandvik rep and he was pretty clueless. My thought was that reducing the feed would reduce the HP requirements but the Sandvik guy was not much help with minimal requirements to make this work. I have the Dorian tool post to work with and it is pinned to the cross slide so I think it is pretty rigid if I can find a holder that would fit the drill. I doubt highly I could get 10 GPM as I have the lower output coolant pump and I would imagine it comes no where near that.

Tiny Troll said:

Use an annular cutter. Go in from both sides if necessary. Finish with a boring bar. I have a TL-2. For my small situation I like it a lot..

Andy

Click to expand...

I just don't get. Whenever there is a thread about making some big holes someone brings up annular cutters or tree panning cutters. WTH? What an expensive and slow way to make holes. Very unproductive.

Get a good insert drill. Just adjust feeds and speeds to the machine. It will work just fine. I'd make a nice tool block to accept the drill shank and bolt it directly to the cross slide. Forget the toolpost. We want rigidity.

david n said:

I just don't get. Whenever there is a thread about making some big holes someone brings up annular cutters or tree panning cutters. WTH? What an expensive and slow way to make holes. Very unproductive.

Get a good insert drill. Just adjust feeds and speeds to the machine. It will work just fine. I'd make a nice tool block to accept the drill shank and bolt it directly to the cross slide. Forget the toolpost. We want rigidity.

Click to expand...

How true. Yes it is a way it can be done but when you have 410 pcs and 3.25" in z to cut it has to be the best way not just a way.

With about 1.6 XD on the drill, the coolant GPM requirements can also bu fudged IMO.
I would recommend getting a 2" 880 drill with LM geometry, and just make it work...
You got the cycle time with those parameters, just add in the tooling cost, get the order, and get some chips going
Fred

Off topic... This is my TL-1 live tool set-up I made with a Sherline milling head. With the M19 option, bolt circles, are done on the lathe