Milling 4340 annealed

[dforsythe]

Im not familiar with this material.  It is customer supplied and everything I can find say it’s around Rockwell 40.  We are seeing poor tool life while dynamic milling.  The chips are coming of red hot and look burnt.  I tried dropping the SF and it’s the same.  Below are the parameters we started with.  Any suggestions would be great.  Also can’t seem to drill using cobalt will switching to carbide help?

 

40 taper

Milling chuck

.500 5fl coated endmill 1.250 loc

 

 SF = 1105

IPT = .0042

Rdoc .035

Adoc = 1.00

 

rpm = 8437

feed = 177

 

Entry = ramp @ 1 deg with 50% reduced feed and speed

 

Thanks, Damian

[Rstewart]

Your SFPM is Too high.  You'll be much more productive at around 6 or 700 sfpm

 

Cobalt drills can only run at about 55sfpm in hardened 4340

 

Have you checked the hardness?  Annealed is in the soft state BTW

[dforsythe]

thanks for the sugestion.  No i dont have a way to check the hardness.  i was using 60 sf for the drills.  i will drop that down also.  I just talked to the local tool rep and he mentioned running it wet.  any thoughts on that?

[djstedman]

As RStewart said.. that SFM is WAY to high..

 

I would run 590 SFM with Air Blast, dynamic milling use 10 to 15 % stepover with depth up to 2X Dia no problem.. with the tool listed above .. I would be going about 4507RPM 131IPM..  That's about .0035 IPT adjusted for Radial Chip Thinning at 10% stepover..

 

Chips should be coming off with air blast a nice amber color.. tool life should be great using tialn or altin or alcrona coatings ..

 

I cut this stuff all the time.. Hard or soft this stuff is great to cut..

 

Shouldn't need carbide to drill this stuff 55SFM on drills should work.. its kind of slow though so if you have a lot of holes carbide is going to be the way to go ..

[dforsythe]

Thanks guys.  I will give it a shot.

[Guyinthedesert]

What they said.  I just cut a ton of this, 1/2 5fl, .800 depth, 12% radial, 4800 rpm and 120 ipm.  I started drilling start holes at the entry points and my too life went way up. The helical entry seems to be a bit hard on the corners.

[dforsythe]

I tried the lower SF yesterday.  glowing ball of death was the result.  Im sending the material for for a hardness check.  somthing isnt right.  i tried using a file on it to a rough guess at harnedness, and the file will not  even leave a mark on it.

[Matthew Hajicek - Singularity]

I use HSMAdvisor for feeds and speeds.

[dforsythe]

hardness test is showing RC 48-49.  much higher than i expected with the annealed state.

[jeff]

hardness test is showing RC 48-49.  much higher than i expected with the annealed state.

Then it's not annealed. Can't be. 4340 Annealed is around 17Rc. Do you have material certs from your supplier?

 

http://asm.matweb.com/search/SpecificMaterial.asp?bassnum=M434AA

[dforsythe]

Jeff,

 

Im the sub on this one.  just asked for the certs........havent heard back......crickets.....

[dforsythe]

per the note on the print:  Material: 4340 per AMS 6414 annealed condition

[Rstewart]

per the note on the print:  Material: 4340 per AMS 6414 annealed condition

 

You got the shaft on that one

 

I'm machining some 4140 @ 45Rc currently with coated carbide and it cuts beautifully.  Not sure how much difference there is between 4140 & 4340 tho. Running 550 - 600 Sfpm

 

I rough with air blast and use coolant for light finishing, and Always use coolant for drilling. 

[jeff]

  Not sure how much difference there is between 4140 & 4340 tho. 

 

 

Not much. It's more or less based on Rockwell hardness.

Maybe 100-150 sfpm less than regular 4150pht at best.

[dforsythe]

so all the certs looked corect.  I took the material back to the customer and they check it also 47-48 RC.  the sent it back out to get annealed agian.  check it this morning...........still at 47-48 RC.  has anyone ever seen anything like this?  im questioning what type of material this actually is.  its been a rough week and it looks like only getting worse

[djstedman]

If its 47-48 RC then its not annealed state if you ask me.. shouldn't be nearly that hard.. you would have to wonder if it being that hard was acceptable for the finished part based on design intent..

 

Anyhow.. assuming it is ok for it to be that hard change strategies and use high feed mills to cut it.. depending what you have to do .. I remove a ton of stock from 4340 parts at 55HrC using Kennametal KMDA feedmills and they work great..

 

Hard Drilling.. still no problem.. just expensive tools.. Walter/Titex coolant through

 

You can still finish with regular carbide using air blast .. or coolant works too..

[jeff]

so all the certs looked corect.  I took the material back to the customer and they check it also 47-48 RC.  the sent it back out to get annealed agian.  check it this morning...........still at 47-48 RC.  has anyone ever seen anything like this?  im questioning what type of material this actually is.  its been a rough week and it looks like only getting worse

I'd be ordering a new piece of stock and charging the customer. If it's 47Rc, then it's already not to print and no good anyway, right?

Maybe consult with another heat treat source to see if it's your normal HT house making a mistake? 

[Bob W.]

47Rc is pretty hard and right on the cusp of needing specific tooling for it.  Is your customer trying to pull one over on you?  I machine parts for a customer of mine that has two versions.  One is Rc45 and the other is Rc54.  The parts at Rc54 are a completely different animal and a real pain to deal with.  Once you get up to 45+ a few points makes a big difference in speeds and feeds and tool life.  The annealed state should be WAAAY below Rc47 though...

[dforsythe]

Not sure who isnt being truthful here, But the customer has decided to cover the tooling and extra run time.  so i just spent a good chunck of change on a high feed mill, inserted thread mill, and thru tool carbide drills.  atleast i know what im up agianst now.  just have to execute.