Speeds and feeds for dynamic milling D2

[Smit]

I'm going to give it a try on some round D2 tool steel parts we've run forever.

Any recommendations on feed, speed, and radial depth of cut?

I'm going to be using a 1/2" variable pitch carbide end mill. It's on a Fadal, which of course is less than ideal, but it's not a precision operation. I just need to remove a bunch of material fast.

TIA!

[Guest]

SFM 300

RPM 2292

IPM 46.39

2X's dia DOC x 5% Step over

[crazy^millman]

With a 5 Flute endmill I got 940 SFM 7186 RPMS 215 IPM with 200% DOC and 5% Step over, but I am crazy.

[jeff]

Assuming it's 200-250 Brinell Hardness D2

I would go 600 sfpm, .05 stepover, .0069 ipt and 1" d.o.c.

 

 

You chickens and your 5% stepover  pffft  

[Guest]

It's a Fadal.....he'll be lucky if it doesn't shake itself to scrap metal  

[shazam/TPP]

+1000 to JP, you can always increase the RPM and Feed, don't want to blow up that end mill.  Jeff's would be the max!!

Quote

It's a Fadal...

[Smit]

Thanks for the replies gents.

I'm going to start with the more conservative speeds and feeds, see how it sounds, then ramp up from there. I am looking forward to finding a good application on one of our more rigid machines and trying out some of the more higher end feeds and speeds.

[#Rekd™]

16 hours ago, JParis said:

It's a Fadal.....he'll be lucky if it doesn't shake itself to scrap metal  

Too late...Fadal=Scrap metal...

[Guest]

Back in the day, I used to run Vipers 100% step over x 100% DOC at 12k at 250 IPM on Mori's

Tried the same exact program on one of out Fadals, nearly shook itself apart.....best we ever did was about 45% of those numbers

 

[jeff]

4 hours ago, Smit said:

Thanks for the replies gents.

I'm going to start with the more conservative speeds and feeds, see how it sounds, then ramp up from there. I am looking forward to finding a good application on one of our more rigid machines and trying out some of the more higher end feeds and speeds.

I highly recommend using the HSM Advisor if you haven't looked at it already.

[Smit]

4 minutes ago, jeff said:

I highly recommend using the HSM Advisor if you haven't looked at it already.

I just googled it and found out about it. It looks really interesting, I'll check it out. Thanks for the heads up!

[crazy^millman]

2 hours ago, jeff said:

I highly recommend using the HSM Advisor if you haven't looked at it already.

That was where I pulled the speeds and feeds from.

[Codeworx]

8 hours ago, Smit said:

I just googled it and found out about it. It looks really interesting, I'll check it out. Thanks for the heads up!

excellent product, i cant tell you howmuch time it saves me on a daily basis.

[Matthew Hajicek - Singularity]

Me to.  I use HSMAdvisor and the Helical Milling Advisor, which is free but for their specific tools.  Helical lets you choose the hardness of the material, and has a "Workholding Security" slider that you can adjust from loose to rigid.  For looser setups (or sloppier machines or more flexible holders) it will increase RPM and decrease feed.  To get numbers for another brand's tools you can just look up Helical's closest equivalent and plug in that part number.

Helical Milling Advisor is where I got the numbers for successfully peeling a slot in HRC 57 S7 on the Haas.  Worked the first time.

[Dan_AKA_ROY]

Downloaded HSM Advisor (did hear about it before). I think it integrates with Mastercam?

I have to cut some blades with D-2 tool steel (1 1/2" by 4" by 1" blocks).

Should I use air blast or coolant? I've read air blast is recommended to prevent hardening. (better heat transfer to chips)

Any input would be appreciated. I'll start the machining tomorrow..

[crazy^millman]

Air would be the better choice, but it needs to be a good volume of air to push the chips away.

[Dan_AKA_ROY]

Thanks Ron! Never cut D2 before but that was my guess. Confirmed.. (thanks again)

[nickbe10]

I use 250 sfm, 2x doc, 0.04 step over,.003 chipload and run it through RCTF in MC. Usually comes out in the 50 - 60 ipm range. Not broken anything yet in a beat up old Haas.....our swaging die mill....!

[Dan_AKA_ROY]

Trouble trying to plunge outside the part. Guess will use helix entry into material. Getting 0.0008" depths per helix rotation. Should be fine. Never used dynamic milling for (really) hard steels before. Boss seemed nervous about it. (nothing ventured, nothing gained)

Using a 4 flute 1/2" diameter helical carbide endmill and coated (I think TiAIN coating, it is not specified. Says "A coated endmill" on the sleeve". The finishing ball endmill is a 3 flute 1/2" diameter carbide non coated. I do have a 4 flute coated carbide helical ball EM that our router uses (long story, I could switch out if the need arises).

Glad I downloaded the HSM Advisor. Embedded in Mastercam 2018..

[Rstewart]

2 hours ago, Dan_AKA_ROY said:

Trouble trying to plunge outside the part. Guess will use helix entry into material. Getting 0.0008" depths per helix rotation. Should be fine. Never used dynamic milling for (really) hard steels before. Boss seemed nervous about it. (nothing ventured, nothing gained)

Using a 4 flute 1/2" diameter helical carbide endmill and coated (I think TiAIN coating, it is not specified. Says "A coated endmill" on the sleeve". The finishing ball endmill is a 3 flute 1/2" diameter carbide non coated. I do have a 4 flute coated carbide helical ball EM that our router uses (long story, I could switch out if the need arises).

Glad I downloaded the HSM Advisor. Embedded in Mastercam 2018..

Dan, don't expect great results helixing into harder steels.  It'll cut a few but it really hurts the bottom of the tool.  If there's a way to plunge outside, or drill a start hole Do It.

If I ever have trouble trying to chain a start point for entry I find another route.  Just do  your op with a helical entry, next do a drill op and put it before your milling op where it helicals in.

[crazy^millman]

11 hours ago, Rstewart said:

Dan, don't expect great results helixing into harder steels.  It'll cut a few but it really hurts the bottom of the tool.  If there's a way to plunge outside, or drill a start hole Do It.

If I ever have trouble trying to chain a start point for entry I find another route.  Just do  your op with a helical entry, next do a drill op and put it before your milling op where it helicals in.

Good catch I didn't read the helix into the material.

I have been doing this is TI and other hard metals for a few years now and night and day difference. Make sure to use your stock models to control entry. Don't trust HST to helix the drill points out either. I will do a small helix path on the floors then run the HST toolpath. Again I make my stock models reflect all of this and the tool will plunge in that holes and take off from there. Yes I can have 20 operations and 20 stock models for some roughing, but that is what you have to do to keep the process live and control things.

[Dan_AKA_ROY]

Boss was too nervous about dynamic milling the part, so...old school machining it. Two pockets with a 1/2" 4 fl. flat helical style EM and then for the blade (0.07" of material left - what they wanted) I'm using flowline rough and finish toolpaths using a 3 fl. uncoated carbide ball EM (I have two of them so I'll give it a whirl) Hopefully 3 flute EM hold up, not much material to cut. (part geo favorable for a flowline cut). The top of blade will be .02" (they will sharpen it down from there).

Got ipm at 4.81, .04 depth cuts. Probably way too conservative. It's cutting well right now...Air blasting it. Plunging off the part.

[JoshC]

The tool vendor you got your tool from would probably know best in my opinion but if you dont get what you need from them i think i would start somewhere around Here:

 

[crazy^millman]

32 minutes ago, JoshC said:

The tool vendor you got your tool from would probably know best in my opinion but if you dont get what you need from them i think i would start somewhere around Here:

 

Aggressive for them is still conservative for my way of thinking, but I am the crazy^millman.

[Goldorak]

On 15/06/2017 at 3:01 PM, C^Millman said:

With a 5 Flute endmill I got 940 SFM 7186 RPMS 215 IPM with 200% DOC and 5% Step over, but I am crazy.

i can go up to 12.5%, i am crazyer lol