Milling 4340 40BHC

[John Spangler]

Hi

Need some recommendations for tooling on a new job. We have 28 pcs that we are machining out of 4340, that will be roughed out, then heat treated to 40 Bhc, then finished. The part is shaped like a "U" with 2 legs, kind of like an Omega symbol. The stock is 1.75 x 10" x 20" and the part has 1.25 walls, with the middle pocketed out. My main question is: what type of tooling do you recommend for all this material removal? for 28 parts, I'm leaning towards indexable tools. The boss wants it set up and running on 2 machines, so I have to double up on everything.

 

Also, these parts need to be roughed, heat treated, then finished.

Walls are .250 thick x 1.25 tall. I was planning on leaving .250 per side before heat treat, in case of warpage.

Any suggestions?

 

Thanks

John

JOHN.pdf

[jeff]

What is 40Bhc? Are you saying this is 4340PHT stock? 28-32 Rc? You say that it gets heat treated after roughing, so I would assume that it's not a PHT material.

I cut this stuff every day. A variable flute endmill like the Varimill or many other brand names will cut this stuff easily, and can go at least 400sfm (that's being conservative) depending on stepover.

If you've ever cut 4140PHT or 4150PHT it's pretty much the same,maybe a little bit tougher,but not enough to write home about.

 

What is the rockwell after heat treat? If it's not too hard, you can always machine after HT.

 

Edit:

No need to leave .250" per side.

If you're concerned, I would leave .050" max and send one to HT to see how it acts.

[mkd]

^^^ I Have nothing to add ^^^^

except personally leaning towards machining after heat treat....

[RaiderX]

YA Jeff nailed it.

material may be on the gummy side as received, might consider normalize prior to rough op to even grain structure of material.

may I add or re-iterate you will only need to leave .06-.125 stock for finish. I would lean toward .125 (this part may twist in heat treat).

do not leave any sharp internal corners in rough op . this stuff is prone to fracture cracks during heat treat.

 

I am guessing spec. requires min. cross section prior to heat treat or I would heat treat blocks then machine the part if only 40 rockwell

 

Doug

[John Spangler]

Thanks.

I thought .250 was a little overkill, but since I don't have experience with heat treating, or the materials that require it, I'm a bit lost.

Thanks

John

[workmantm]

I just ran some parts here and tried out the OSG Aero UVX line of cutters. Ran like a champ with high SFM and decent feed rate. I'd have to go dig up what it was at this point. Tool lasted thru the entire run, I expected the 1/8 cutter to die on me just because of the small diameter.

 

We HT to 160-180 KSI and machine it all from there. For all out hogging we run Iscar's FF geometry tools. Need a little modification on the body, but I run at 100+ IMP on a 3flt body. Inserts last a decent amount of time given how abrasive the material is. Might want to look into those. .060 DOC max. Otherwise use a dynamic toolpath and run the OSG like the book tells you to. One cutter might be enough to get you thru the entire 28 pc lot. I run them wet here on our Hass machines.

[Robert Ouellette]

I use the same OSG cutters here and I love them. I run them about 25% over what the book says and they last long time. try the 5 flute series and run it full flood coolant. leave 1/8". heat treat. and finish. I don't see any problems machining that part.

[workmantm]

I use the same OSG cutters here and I love them. I run them about 25% over what the book says and they last long time. try the 5 flute series and run it full flood coolant. leave 1/8". heat treat. and finish. I don't see any problems machining that part.

 

I'm afraid if I tried to push my old Haas mills to 25% over the book I'd choke them worse. Good to know that they can perform that well if the machine is up to the task.

[Robert Ouellette]

I know what you mean. I run them on a HAAS TM-2 that is 5 yrs old and on a 3 yr old VM-6. I wish I had a new MAKINO or MATSUURA to really push those cutters but I have to refrain myself and just be happy with what I have. maybe one of these days the boss will get the machine that is a good performer not the machine he thinks is a good price.

[scott10]

Have you tried hitachi high feed mill (radius mill) ? I run them on my haas VM-3 and VM-8

love them for hogging .04 deep 75% stepover 1650rpms 260ipm .Inserts last a long time.

Run with air no coolant.

[workmantm]

I've got a '96 VF1 and a '98 VF4. They only have so much to give... Talking the owner into looking at the PS95 and several other builders for the mills here. That will be our next new machine. Proving the ROI will be the biggest hurdle I face with that though.