High Feed Milling starting numbers

[Rstewart]

Hey guy's, hope everyone is doing well

Anyways, I've somehow dodged the whole HFM craze, but I have a good application for a 4130 part. I ordered a 32mm ISCAR HELIDO UPFEED 4 flute inserted cutter along with the appropriate inserts for the material.
It's one of the M16 modular tools that screw into the holder (2.5" gage length Btw).

Material is Normalized 4130 bar

Machine is a New haas Vf-2 with 10K spindle. I need to hog off about 35Lb of material. Supposedly the inserts are good for a 1mm Depth of cut.  On the insert package, it recommends .025 to .034 Depth of Cut.

I can finish with regular endmills.  

I got tired of dicking with Iscar's site.


ANY Recommendations for SFPM and CLPT?

[gcode]

I can't make sense of their website either
For the high feeds I use, I'd run 400 to 500 sfm and .015 ipt
I've never run Iscar's high feed.
I use Ingersoll these days.

https://www.ingersoll-imc.com/product?ecatProductId=2253671#!ProductBulletins_LinkContent">https://www.ingersoll-imc.com/product?e ... inkContent">https://www.ingersoll-imc.com/product?ecatProductId=2253671#!ProductBulletins_LinkContent

Click on the Product Bulletin tab for programming info

[Rstewart]

I appreciate the info G.

At .015 clpt I'm not seeing the advantage of the high feed milling.  I'd assume .025 to 30 would be what you'd see in the videos. Maybe if the material was hardened or tougher but 4130 normalized is pretty basic.  
The inserts and tool I have is only rated for .032 depth of cut.

Maybe I bought the wrong tool for the job?  I just wanted to dip my toes in the territory.

[gcode]

The product bulletin says up to 800 sfm and up to .03 ipt for mellow steels
That would be 2400 rpm and 293 ipm for a 4 flute tool
I can`t do that
The big mills in my shop don`t even rapid that fast

[Rstewart]

Happy to report back that even a Haas can run this tool at it's intended speed LOL

.029 depth of cut .03 clpt and 530 sfpm.  Tool cut great and probably could have been pushed harder.

[rob@fain]

Did you order the FF EWX D32-4-M16-05?
Use the H600 WXCU 05T312T .035depth and.040ipt, program the radius .091
if the grade is IC830 do 425sfm, if it's the IC808 go about 500sfm.

Run this dry with air if possible.

let me know if you have questions.

[Rstewart]

Did you order the FF EWX D32-4-M16-05?
Use the H600 WXCU 05T312T .035depth and.040ipt, program the radius .091
if the grade is IC830 do 425sfm, if it's the IC808 go about 500sfm.

Run this dry with air if possible.

let me know if you have questions.

Yes, that's the exact same setup I have.  I was slightly easier on the feed, it did fantastic tho.  I was at almost 4" gage length, shorter and I would push a lil harder.  I'm very impressed with these tools

[neurosis]

We have a couple of old mitsubishi high feed mills that we use on a few 4340m jobs even after heat treat.  They do pretty amazing.  When the material is soft it cuts like butter.  

Did you make any videos?  

[gcode]

I use a lot of 4 5 and 6 in Ingersoll high feeds.
It's a real thrill watching a 100 hp mill pulling 60% spindle load with a 6" hi feed.
The chips will really hurt you if they hit you

https://www.ingersoll-imc.com/product-family/3344508">https://www.ingersoll-imc.com/product-family/3344508

these work really well in Inconel and stainless steels

https://www.ingersoll-imc.com/product-family/3725134">https://www.ingersoll-imc.com/product-family/3725134

[CADCAM396]

Happy to report back that even a Haas can run this tool at it's intended speed LOL

.029 depth of cut .03 clpt and 530 sfpm.  Tool cut great and probably could have been pushed harder.

maybe the question will be for how long.
worked for a company that had quite a few Haas. they went through at least 3 spindles a year. down time sucked.
i surmised they were hogging old school. 1 inch end mills 2-3 inches deep 1/2 radial. and sounded like chit.
I always programmed high speed and or dynamic with a bit smaller diameter tools to keep spindle torques down. those machines
had no spindle problems.
just throwing it out their.. good luck

[Here's Johnny!]

Looking for some starting speeds and feeds for a 5/8" 2 flute high feed index cutter for a guy I am helping out. Doing a full width contour ramp in mild steel. Going right through a 3/4" CRS bar (roughing a 1.25" hole). The Machine is an abused Haas TM1 and crappy tooling.

I was thinking about 400 - 450 SFM and about 0.02" IPT and a ramp depth of 0.01"

Any other suggestions other than get a better machine???

[neurosis]

I was thinking about 400 - 450 SFM and about 0.02" IPT and a ramp depth of 0.01"

Well, did this work out for you?

I'm reluctant to give any input not knowing the machine or tool that you're using.  

I've also never used a high feed mill to mill through the bottom of a part before.

[gcode]

I've also never used a high feed mill to mill through the bottom of a part before.

 high feed mills do not like doing this
When the floor gets thin it starts bouncing and crushes the inserts

[Here's Johnny!]

I was thinking about 400 - 450 SFM and about 0.02" IPT and a ramp depth of 0.01"

Well, did this work out for you?

I'm reluctant to give any input not knowing the machine or tool that you're using.  

I've also never used a high feed mill to mill through the bottom of a part before.

It did work okay but....I would do it differently in my shop given we have a better options of tooling. It was only a couple of parts but I agree on going through with these types of cutters.

Yes it sounded like a Haas when machining!!!!