What's new
What's new

First time high feed milling

Rstewart

Stainless
Joined
Jun 14, 2006
Location
Huntsville Alabama
Hey guy's, hope everyone is doing well and making lotsa $$$

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, I can finish with regular endmills.

I got tired of dicking with Iscar's site.


ANY Recommendations for SFPM and CLPT?
 
Hey guy's, hope everyone is doing well and making lotsa $$$

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, I can finish with regular endmills.

I got tired of dicking with Iscar's site.


ANY Recommendations for SFPM and CLPT?

We run one of the similar tools from them in a 2" cutter. We run it between 576 SFM (1100RPM) and 675 SFM (1290 RPM) and a feed around .015 IPT. The lower SFM is for when we run it through bar with nasty scale. For clean bar we can run it at the higher speed.
 
We run one of the similar tools from them in a 2" cutter. We run it between 576 SFM (1100RPM) and 675 SFM (1290 RPM) and a feed around .015 IPT. The lower SFM is for when we run it through bar with nasty scale. For clean bar we can run it at the higher speed.

Ok, thanks for some info.

I planned on starting with 500sfm and .026 clpt with a .03 depth of cut. Those are low end of the scale as far as clpt (on the back of the insert pack)

Honestly, if I can't run at least a .026 or .03 clpt then this is a Time Waster....
 
I've found for higher tensile materials that they tend to like a lighter depth of cut .03 should be good but I'd bump that feed up to like 0.040 per tooth.
the higher feed will help remove heat in the chip and make the insert last longer, run dry with airblast, or through tool air if you have it.
 
I did a shit load of high feed milling in tool steels a few years ago, we ran 250m/min surface speed, 1mm depth of cut 1mm feed per tooth. our tool rep at the time gave us those numbers and they worked a treat. never tried any slower in steel, but was told that if you slow it down it will just kill the inserts.

make sure your taking as close to 100% WOC as you can at all times and dont put the tool into small corners. loads of air blast.
 
I ran the listed feeds & speeds supplied by Iscar. (the brand of FeedMills I have)
On my VF-4 or my VMX24, I can usually get away with about 55-60% of diameter WOC, on a Ø2" cutter Ø, 0.027-0.039 DOC, and 0.025-0.04 IPT.
We do this in welded A514, 4140HT, 4130 RC38-42 (different SFM) and occasionally 4340.
We run 3 sizes of feedmills: Ø1" 2fl, Ø2" 4fl, Ø2.5" 5fl.

We have cutters for both FF WOMW, and H600 WXCU.

They are great for high CFM material removal.

Doug
 
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.
 
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.

Good to hear..HFM is always fun to do. Back when I was running a lot of 4140 we would rough the 2" cutter 0.05-0.06" DOC at 600SFM and 0.04-0.06 FPT. Insert life was very solid unless there was catastrophic failure. Shit burns thru inserts but it is absolutely worth it for the cycle time.
 
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.

how do you know its actually running at its intended speed? we talking RPM or feed?
 
I think he was referring to the fact that Haas aren't know for their accel/decel, and that only the newest controllers show actual feed - the older ones all showed the commanded feed as actual even when it wasn't. It is not difficult to think you are running faster than you actually are.

When I cut 4140 and 4140PH with a high feed, I usually rely on chip color to tell me when I'm at the SFM limits. I crank up the SFM and linear feed rate until the chips look good and lock it in.
 
I think he was referring to the fact that Haas aren't know for their accel/decel, and that only the newest controllers show actual feed - the older ones all showed the commanded feed as actual even when it wasn't. It is not difficult to think you are running faster than you actually are.

When I cut 4140 and 4140PH with a high feed, I usually rely on chip color to tell me when I'm at the SFM limits. I crank up the SFM and linear feed rate until the chips look good and lock it in.

Yup, I remember running a pretty new Super 2, early 2000's model, where we were trying out high feed milling and we were seeing how far we could push it so we started at around 200IPM, then 300, then 500, but at 500 there was no difference at all in the cycle time from running at 300 even though it showed 500 the whole time.
 
By what is recommended from the manufacturer. I went right in the middle of the clpt and towards the upper end of the sfpm.


I removed about 30Lb of material and the inserts still look great!

thats not what i was asking. you said the haas can run the tool at its intended speed. how do you know that its actually running at the speed you programmed it at? i dont doubt the tool works great.
 
I think he was referring to the fact that Haas aren't know for their accel/decel, and that only the newest controllers show actual feed - the older ones all showed the commanded feed as actual even when it wasn't. It is not difficult to think you are running faster than you actually are.

When I cut 4140 and 4140PH with a high feed, I usually rely on chip color to tell me when I'm at the SFM limits. I crank up the SFM and linear feed rate until the chips look good and lock it in.

not even the new controls show actual speed, i'm sitting in front of a 2020 machine thats the same exact bullshit
 
One basic thing with high feed milling cutters.
Go fast or go home.
They do do like lower or anything like normal feedrates.
As shown above it is chip thinning to extremes.
Measuring your cut chip thickness can give you an idea of what is going on.
Bob
 
They work great in Ti these days. Different carbide, coatings, geometries?

We run these every day in Ti on our Yasda. 2.5" Ingersoll DiPos Feed, 8 tooth, with IN7035 grade inserts. I don't recall the S/F off the top of my head, but it's gettin' it. VERY impressive. Consistent tool life. Can't ask for any better. Tech comes a LONG way in 12 years.

**EDIT** - 170SFM, .025IPT, .025 DOC, 100%WOC. On a dovetail, in a 40 taper machine. It was able to be pushed harder, but this is where tool life was the best.
 
Last edited:








 
Back
Top