LOOKING FOR A FORMULA??????

[rjoyner]

I looking for a formula for turnning to get a Depth of cut. I have everthing else I think:

 

Surface FT/Min = 1200

RPM = 9167

IPM = 64.17

IPR = .007

 

Work Piece is .500

 

WHAT IS THE FORMULA FOR THE DEPTH OF CUT???

Can it be done?

[Charles Davis]

[i believe you are looking for a horsepower equation that you can re-arrange to get depth of cut. You will also need the machineability (???) factor for the material.]

 

Oppsss.. just realized this is turning, not milling. Not sure if there is a formula for this. I usually consult the recommended parameters from the tool manufacturer.

[dan m]

9167 rpm's now thats spinning. what I was always told was you could cut up to 70 percent of the ic plane of the insert. hth

[crazy^millman]

Charles you can still use the horsepower for the depth of cut you need to go back to our math problem about 3 or 4 months ago I think the thread was called is this to hard: Is this too hard?

 

Look over the thread we covered alot of things about this very thing there.

[crazy^millman]

Ryjoner if you got the machine to push it sure can. But you have to take the holding force of the chuck and the amount in the chuck and do you have a tail stock which I sure hope not at that RPM. I would hate to be near the machien when you trwo those chips of at:

quote:

---

9167 rpm's now thats spinning.

---

and they think I am crazy. I hope you are cutting Carbon Steel or Plastic or Aluminum. Toolsteel, Stainless, or any Hardened Steel and I would say you have gone outside of a good SFM for the ability of the insert.

[Code_Breaker]

Here are some "quick" rules:

 

1) No tool can ever take more than 10% of its diameter--including the cusp height.

2) Plus stock (PS) is 6% if semi finish cutter (commonly referred to as the depth of cut or effective diameter)

3) Finish (F) stock between .250 and 1" leave .007

4) Semi Finsih = PS - F

5) Rd = (srt(H * 8 * R)) * cosA

[note: leave out cosA on flat surfaces)

Rd is radial step over

H is from calculation of #4 above

8 is constant

R is radius of tool

6) Finish Stock ie 64 rms (.000064) for H

 

for example:

Tool:

ruff is .500 dia

semi is .375 dia

finish is .250 dia.

1) ruff = 10% of .500 is .050

2) PS is 6% of .375 = .0225

3) finish is .0225 -.007 = .0155

 

steps

1) finish calcuation first:

==>flat area = srt (.000064 * 8 * .125) = .0077 step over

==> angular area srt(.000064 * 8 * .125 ) * (cos48) = .0051 step over

2) semi finish:

==> 10% of finish cutter = .025

==> H is .025 - .007 = .018

==> srt (.018 * 8 * .1875) * (cos48) = .1099 step over

3) ruff:

==> 10% of ruff cutter = .050

==> .050 - PS (.0155) = .0345

==> srt(.0345 * 8 *.25) * cos48 = .1403 step over.

 

The key question to ask yourself is "How much can the NEXT cutter handle."

 

For speed and feeds

 

1) Find effective diameter (ED) (6% of tool dia based on 10% depth of cut)

2) RPM = 3.82 * SFM/ED

3) IPM = RPM * # of flutes * chip load

 

 

HTHAW

Code_Breaker

[chris m]

If you've got a 10,000 RPM lathe, please post a pic; that's some machine! I don't really understand your question but if you are trying to back-figure max DOC from available horsepower there are typically formulas to be found in the back of your Sandvik or KM turning books. Sandvik's is too ungainly to post here, but it is in the book.

 

My Sandvik guy claims that in the right conditions the inserts will take at least 50% of the inscribed circle [.250 radial DOC with a CNMG 43X, for instance] but that is typically too much for setup rigidity. In my most rigid setups I'll rough steel with a .150 radial DOC with 1/2" IC but that's about it. If you're turing a 1/2" part, I wouldn't sweat the DOC too much...

 

As a side note, you'll often run out of axis thrust before spindle horsepower on newer machines.

 

C

[Guest CNC Apps Guy 1]

Horsepower at the cutter.

 

code:

---

      MMR

HPc= -----

K

---

MRR = Metal Removal Rate

K = Material (From Machinery's Handbook)

 

code:

---

MMR = 12 x DOC x IPR x SFM

---

HTH

[Tim Johnson]

If you don't have 9000 rpm, then you may want to drop the feed to .004/.005 with .060 doc. Once the spindle hits max rpm, then your insert is going to cut at a lower sfm which will start tearing it up.