HELP: Machining non-hardened D2 tool steel.

Tryhard · May 2, 2021

Anyone out there machine non-hardened D2 regularly and can give a few pointers?
All of my internet search results seem to contradict one another.

Right now, I don't even know what tools to buy. Much less speeds, feeds and depth of cut.

Machine: Haas VF-0E (20hp)
Material: off the shelf, bandsawed D2 tool steel.
Mat'l Size: 1.75" x 1.75" x 6.00" (roughly)

The part requires quite a bit of material removal. More or less making it a 3/8" thick by 6" angle with some c'bored holes and some dowel pin holes.

Any help would be greatly appreciated!

TH

eKretz · May 2, 2021

I always started at 250 SFM with unhardened D-2 using indexable tooling for turning. I found I could get away with a little more SFM when milling but not much. Flood coolant. That machine a 40 taper I take it? I'd run whatever square shoulder facemill you've got and run the feed and DOC about the same as what you would for something like 4140 Q&T. It generally cuts about the same.

WizardOfBoz · May 2, 2021

Tryhard said:
The part requires quite a bit of material removal. More or less making it a 3/8" thick by 6" angle with some c'bored holes and some dowel pin holes.

6" x 6" x length, with each flange of the angle 3/8" thick? Certainly cut out the 5.5" x 5.5" x length using a vertical band saw.

Tryhard · May 3, 2021

bosleyjr said:
6" x 6" x length, with each flange of the angle 3/8" thick? Certainly cut out the 5.5" x 5.5" x length using a vertical band saw.

I wish that were the case, but the shape is a lil more complicated than just an angle, only used that to help visualize the amount of roughing.
The material arrived and is actually 2.16 x 2.04 x 5.00"

TH

Tryhard · May 3, 2021

eKretz said:
...and run the feed and DOC about the same as what you would for something like 4140 Q&T. It generally cuts about the same.

Never have I run 4140 Q&T. So what would your suggestion be for feed and DOC?

Thank you eKretz!

TH

eKretz · May 3, 2021

What are you going to be using for a cutter? And you didn't answer...is the machine 40 taper at least?

RC Mech · May 3, 2021

eKretz speeds are bang on. I’m currently making some stamping dies and ran 298 SFM last week with a 1/2” solid carbide 4 flute. 40 taper machine.

spinninquin · May 3, 2021

I almost exclusively cut D2 and 4140PH on a 40 taper VF2, and run the same parameters for both. Using a .500" YG 5-flute endmill, dynamic strategy at 5% radial, I run about 450 SFM and 32 IPM. This is almost directly from our YG rep and I've had incredible luck with it. I know I could increase the radial percentage and probably chip per flute, but I don't run production and don't worry too much about cycle time. I'll bury this tool 1.2" and haven't had any issues.

Tryhard · May 3, 2021

Yes, 40 taper Haas VF-0E. All of my current tools are 2 and 3 flute carbide for Aluminum.
I don't have tools for this job yet. Guessing 5/8" or 3/4" 4flt endmills for roughing and another for finishing?
Do have a 3" 90deg x 7 insert face mill, but it currently has inserts for aluminum.

TH

Tryhard · May 3, 2021

spinninquin said:
I almost exclusively cut D2 and 4140PH on a 40 taper VF2, and run the same parameters for both. Using a .500" YG 5-flute endmill, dynamic strategy at 5% radial, I run about 450 SFM and 32 IPM. This is almost directly from our YG rep and I've had incredible luck with it. I know I could increase the radial percentage and probably chip per flute, but I don't run production and don't worry too much about cycle time. I'll bury this tool 1.2" and haven't had any issues.

Hey spinninquin, Would you happen to have a part number of your YG cutters you could share? Love YG endmills.
Also will be drilling what appears to be (2) standard depth 3/8 counterbores and drill/ream (2) .3745 holes.
Any pointers on drilling?
Coolant yes or no?

Thank you for your input!

TH

spinninquin · May 3, 2021

Tryhard said:
Hey spinninquin, Would you happen to have a part number of your YG cutters you could share? Love YG endmills.
Also will be drilling what appears to be (2) standard depth 3/8 counterbores and drill/ream (2) .3745 holes.
Any pointers on drilling?
Coolant yes or no?

Thank you for your input!

TH

Luckily MasterCAM is down so I have a bit of time right now haha. YG part number: UGMG34920. As for drilling. I mostly use modular drills, carbide tips, with TSC. With these I run between 180-200 SFM and 0.0025/rev. If I'm using a solid carbide drill I'm more in the 150 SFM with 0.0018/rev region. Reaming I use carbide-tipped reamers. Many years ago for reaming I was taught 2/3 the speed, twice the feed, and it works well for what I do.

I used to run Kennametal's Harvi endmills in the .625" to .750" sizes cause they used them on our production floor. When production dropped them, we lost our bulk-size pricing and we were draining cash. .500" seems to be the sweet spot for the VF2 I run and the cost is pennies compared to what Kennametal had.

Hope this helps you out!

implmex · May 3, 2021

Hi Tryhard:
Don't get too freaked out by the unknowns...it's truly not that difficult to find the sweet spot for your machine, your cutters and your setup.
Start with a relatively conservative surface speed...you can easily look up what a carbide cutter will tolerate with any number of down loadable cutter speed and feed calculators.
HSM Advisor is a fairly commonly used one.

Try it out...start with a small radial cut and an axial DOC as deep as the cutter diameter if you're using a solid carbide endmill.
If you're using an indexable start with a DOC of 1/10th of the insert height and the feed per tooth your downloaded utility recommends.
Take a cut...listen to it, watch the machine.
Decide if it sounds like too much or not enough and adjust accordingly.

None of this is rocket science, and gazillions of pounds of D2 are cut daily in die shops, and they all had to figure it out from first principles too.
So don't let the "tool steel" designation give you too many worries...it's a pretty simple material to cut when it's soft.
You'll very quickly learn what you can and cannot get away with on your machine.

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining

AARONT · May 3, 2021

Run dry for milling. Maybe an air blast to clear chips. 250-300 SFM with .0025ipt. Go TiAlN or AlTiN coated.

For drilling 135° split point cobalt stub drills work well. About 40 SFM and .003"/rev peck about 65% diameter and you'll be fine.

Tryhard · May 3, 2021

spinninquin said:
...As for drilling. I mostly use modular drills, carbide tips, with TSC.

I am without TSC and only have a decent index of cobalt drills and HSS reamers. Am I absolutely needing the carbide stuff or could I get by for 4 parts with about 8 holes total for reaming and 8 total for counterboring???

You are helping a great deal, thank you.

TH

spinninquin · May 3, 2021

Tryhard said:
I am without TSC and only have a decent index of cobalt drills and HSS reamers. Am I absolutely needing the carbide stuff or could I get by for 4 parts with about 8 holes total for reaming and 8 total for counterboring???

You are helping a great deal, thank you.

TH

You're good with cobalt and HSS. I just have access to the carbide from what our production people use.

eKretz · May 3, 2021

I'm generally used to big solid machines where we'd use as large a cutter as possible, so I probably won't be much help on suggested feed and DOC for your Haas. I'd just try what you try when cutting any old steel. Soft D-2 is pretty manageable as long as you keep the speed in the right range so you don't get too much tool wear.

HSS is pretty much what I always used for drilling and other holemaking ops. Stick to 45-50 SFM for fairly shallow holes and you should be fine. Slow down a bit if you have to go much over 2×D. Same speed relationship with reaming:drilling as is generally used, for me that would be about 1:3 for speed, 2:1 for feed.

Tryhard · May 3, 2021

Thanks ekretz & spinnin quin, you guys are awesome!

TH

Mtndew · May 4, 2021

Yeah soft D2 is fine, it's the hardened D2 that will make you pull your hair out.

Tryhard · May 7, 2021

Mtndew said:
Yeah soft D2 is fine, it's the hardened D2 that will make you pull your hair out.

Yep, just wanna cut it soft and not work-harden it in the process.

~TH

eKretz · May 8, 2021

It's fairly tough stuff even in the unhardened state, but nothing to be afraid of. You'll know you're not cutting 1018, but keep your speed down and everything will be fine.

HELP: Machining non-hardened D2 tool steel.

Aluminum

Diamond; Mod Squad

Diamond

Aluminum

Aluminum

Diamond; Mod Squad

Stainless

Aluminum

Aluminum

Aluminum

Aluminum

Diamond

Stainless

Aluminum

Aluminum

Diamond; Mod Squad

Aluminum

Diamond

Aluminum

Diamond; Mod Squad

Similar threads