Feeds and speeds 47/64 cobalt spade drill Ticn coated, in 7075 T6

P

partsproduction

Titanium

Joined

Aug 22, 2011

Location

Oregon coast

• May 13, 2020

• #1

Suddenly breaking drills. I was told 400 SFPM and .016" per rev but the guy didn't know the difference between 6061 and 7075, which makes me wonder.
Any advice Greatly appreciated,
parts

 

litlerob1

Diamond

Joined

Nov 4, 2013

Location

Utah, USA

• May 13, 2020

• #2

Diameter of the Drill/.0312/2=feedrate in chipload per flute.

SFM is up to you. 400 sounds okay, assuming you have decent coolant.

So I'm getting about .0115 feed per flute.

R

 

M

Milland

Diamond

Joined

Jul 6, 2006

Location

Hillsboro, New Hampshire

• May 13, 2020

• #3

Different batch of alloy (more gummy)? Coolant off spec? TSC (if using) filter plugged or other flow deficiency?

What sort of buildup, if any are you seeing on the inserts? Same grade as before?

 

D

Delw

Stainless

Joined

Jan 8, 2019

• May 13, 2020

• #4

partsproduction said:

Suddenly breaking drills. I was told 400 SFPM and .016" per rev but the guy didn't know the difference between 6061 and 7075, which makes me wonder.
Any advice Greatly appreciated,
parts

Click to expand...

you said suddenly breaking drills. were they running good before? what did you change?

I find both machine close to the same. I like 7075 better but thats me.

lathe or mill
you on center? how deep? any pecks?
Robs feed rate sounds better than what your doing.
personally I go slower on both smf and feed but thats me.

 

P

partsproduction

Titanium

Joined

Aug 22, 2011

Location

Oregon coast

• May 13, 2020

• #5

Actually the drills we were breaking were HSS silver and demming, they were chipping down .015" below the cutting edge. So I asked my programmer why he isn't using spade drills and he didn't think we had any, which turned out to not be true.
The flutes of the S&D were clogging with a 2 peck dive into a 2" deep hole, I also suggested three or four pecks for the spade drill because we don't have through the drill coolant on the mill.
Apparently 400 SFPM is working with .004"per rev (3 IPM) with the spade now. The reason I asked was because we just can't afford to blow through the inserts and/or spade holders anymore and the mill motor was erroring out with clogging.
Times are tough!
Thanks for the answers! I told him he can start raising F&S's as he goes through the crates of parts. BTW, that HSS S&D is 1/2" shorter now.

 

D

DanASM

Hot Rolled

Joined

Mar 11, 2019

• May 13, 2020

• #6

I punched it into my software and got approx 220-250 SFM with .0135-.0158 IPT (.027-.031 IPR)

Just what my numbers say. Not from experience, does not say to peck at 2.00" deep

Spade Drill

 

litlerob1

Diamond

Joined

Nov 4, 2013

Location

Utah, USA

• May 13, 2020

• #7

PP, in your original post you said you were "breaking drills". What does that mean exactly?

.004 per revolution is beyond painful. You are costing yourself more in time than the latest greatest wazzoo Drill on the market.

R

 

P

partsproduction

Titanium

Joined

Aug 22, 2011

Location

Oregon coast

• May 13, 2020

• #8

breaking drills

Click to expand...

Yeah it did look that way, I meant I was afraid we would be, because the S&D's were breaking at the cutting edge face. I assumed the spade drills would be soon and we can't afford to replace them due to excessive speeds & feeds. The drill is followed by a carbide BB so size isn't too important.

.004 per revolution is beyond painful.

Click to expand...

As I said, he can push it up from here, way too much time was wasted regrinding that S&D.

 

M

Milland

Diamond

Joined

Jul 6, 2006

Location

Hillsboro, New Hampshire

• May 13, 2020

• #9

partsproduction said:

As I said, he can push it up from here, way too much time was wasted regrinding that S&D.

Click to expand...

No offense to your operator, but it would be interesting to see the resulting repointing. If the grind is off, it could an explanation as to the poor performance.

 

TRussell

Aluminum

Joined

Mar 17, 2015

• May 14, 2020

• #10

You find that 7075T6 machines the same as 6061T6? Have you ever cut them dry? 6061 is way, way gummier. It's the only heat treated aluminum alloy that I've ever had problems with loading up the cutter. I don't know of a friendlier alloy than 7075T6, except possibly 7050T7.

 

A

AARONT

Stainless

Joined

Feb 19, 2013

Location

Madison, WI

• May 14, 2020

• #11

Are you running Allied inserts? It looks like those are the recommended numbers for that insert.(page 32)If the length of drill is more than 3xD you're going to have to slow it down on feed and speed. How's the runout of the drill?

I would start at 250 SFM and .012"/rev and walk up the feed and speed from there. Also pecking every 1xd. The factory recommended feeds and speeds are only going to be valid with through tool coolant.

 

Bobw

Diamond

Joined

Feb 8, 2005

Location

Hatch, NM Chile capital of the WORLD

• May 14, 2020

• #12

TRussell said:

You find that 7075T6 machines the same as 6061T6? Have you ever cut them dry? 6061 is way, way gummier. It's the only heat treated aluminum alloy that I've ever had problems with loading up the cutter. I don't know of a friendlier alloy than 7075T6, except possibly 7050T7.

Click to expand...

2024 is right up there, I think its a little friendlier than 7075, it doesn't seem
as abrasive. I've also never had a melt down in 7075. 2024 either.

6061 on the other hand.