What's new
What's new

HSS / TiCN endmill vs aluminum (Speed check)

cwtoyota

Cast Iron
Joined
Feb 11, 2010
Location
Washington State
I'm running a 1.25" three flute end mill (HSS / TiCN) in plain-old 6061-T6 Aluminum.

Is 590 SFM too much for HSS?

I ran a couple tests (slotting with 0.75" depth) in some scrap and came up with 590 (1800 rpm) 20 IPM (.0037 IPT).
The chips look great and clear the slot nicely. The finish is acceptable and the machine is happy.

I planned to slot at .0037 IPT, rough at .005 IPT, and finish at .002 IPT.

Will good HSS with TiCN hold an edge at 590 under these conditions?
 
I would expect so. Aluminum is almost a material you can run any speed in even with HSS. So long as you don't get HSS to a temperature where the edge starts to weaken, which would be hard with flood coolant in aluminum, I say crank it up.

We used to run a job where we took a 1" 3 flute HSS end mill with no coating (but a good manufacturer, Niagara) and shoved it through 1/2" or 3/4" thick material, full slot at some points. I believe it was 5000 RPM and 50 or 100 IPM. That's over 1000 SFM, in fact. Poor old Haas maxed out on those cuts.

Just make sure you keep coolant on it, else you will easily get a gumming problem and pop! ...wait, no, it's an 1-1/4" cutter. That'd be more like BANG!! Ha.
 
For kicks I punched it into HSMAdvisor. I'm assuming 6061 T6, and a 1" LOC on the tool. For full slotting it recommends 1746 RPM (571 SFM) at 16.14 IPM. Non slotting it recommends 1.1135" stepover, same RPM, 18.44 IPM. Since your test produced good results with slightly higher numbers I'd go with your numbers.
 
I'm running a 1.25" three flute end mill (HSS / TiCN) in plain-old 6061-T6 Aluminum.

Is 590 SFM too much for HSS?

I ran a couple tests (slotting with 0.75" depth) in some scrap and came up with 590 (1800 rpm) 20 IPM (.0037 IPT).
The chips look great and clear the slot nicely. The finish is acceptable and the machine is happy.

I planned to slot at .0037 IPT, rough at .005 IPT, and finish at .002 IPT.

Will good HSS with TiCN hold an edge at 590 under these conditions?
.
.
i would use a roughing corn cob end mill with flood coolant washing away chips. often limit is
1) holding part from moving
2) hp of machine and what cutter and tool holder can take and part vibration limits
3) getting chips out of the way and avoiding overheating where chips stick to flutes
..... roughing end mill usually far better at removing most of material and a separate finish cutter is better for a better finish
 
For kicks I punched it into HSMAdvisor. I'm assuming 6061 T6, and a 1" LOC on the tool. For full slotting it recommends 1746 RPM (571 SFM) at 16.14 IPM. Non slotting it recommends 1.1135" stepover, same RPM, 18.44 IPM. Since your test produced good results with slightly higher numbers I'd go with your numbers.

Depends on the length and how much deflection you can allow.

I am getting this for a stubby 3 flute regular cutter:
Material: 6061-T6 Series Aluminum 95 HB
Tool: 1.250in 3FL HSS TiCN Solid End Mill
Speed: 525.6 SFM/ 1606.9RPM
Feed: 0.0047 in/tooth 0.0141 in/rev 22.66 in/min
Chip Thickness: 0.0047 in
Reference Chip load: 0.0047 in
Engagement: DOC=0.66 in WOC=1.25 in
Capturegkjodooofe.jpg

Which is pretty close what he got anyway. At 0.75" deep i am getting 0.004" ipt feedrate
 
Depends on the length and how much deflection you can allow.

I am getting this for a stubby 3 flute regular cutter:

View attachment 209956

Which is pretty close what he got anyway. At 0.75" deep i am getting 0.004" ipt feedrate

aluminum can be easily pushed fairly high ipt often .010" or more ipt is common (done that for many decades) but if chips cant get out of the way fast enough i have had to use a hammer and screw driver to get stuck on aluminum out of the flutes
.
i have also had parts move in the vise before cause of the high cutting forces and vibration
 
Thanks for all the input guys.

Nice to see that where I ended up was in the ballpark of sanity.

This isn't a super long end mill, but not a stub. stick-out from the holder is a little over 3". The material is 2.5", so I needed some length. I tried a depth of 0.75" with the .0076" chip load and I had some flex.

I had some photos: (I forget things, so I keep a file on this kind of stuff to reference later).
The file names of each chip photo have the info for the cutting parameters.

IMG_1478.jpg
CUT-1_Chips (1.25 3Fl HSS TiCN @ 900RPM, 20.5IPM, 0.0076IPT, Z0.250, Slotting).jpg
CUT-2_Chips (1.25 3Fl HSS TiCN @ 900RPM, 20.5IPM, 0.0076IPT, Z0.500, Slotting).jpg
CUT-3_Chips (1.25 3Fl HSS TiCN @ 1800RPM, 20.5IPM, 0.0037IPT, Z0.500, Slotting).jpg


I will run the job next week and try to update this thread with my results.
 
I'm slightly confused. I'm not an aluminum-master, but my thought was that with aluminum, you simply run max-RPM, bury the tool, and increase the feed until you're at 100% spindle load... :confused: I seem to recall the Brother guys running wide-open with HSS endmills, all the time.

HSS still maintains it's hardness to nearly 1000*F - meaning well past the typical "blue" color that steel becomes at high temperature. I say that because, you almost can't run HSS too fast in that kind of aluminum - You won't overheat the tool with any amount of coolant. The biggest risk is simply clogging the tool and breaking it.

Your chips look good - just speed it up. :)
 
Have not had much luck running regular HSS faster than 600 SFM slotting even with coolant.
A magic "minicut" endmill did fine up to 1000 SFM. Those SOBs were as expensive as carbide ones.

I guess HSS cutter needs thicker core which leads to more heat and more clogging. Especially when the edge becomes dull.

For short bursts- yeah you can run it like carbide but then tool life will be an unexpected factor.
 
I said I'd update when I run the parts....

Lots of chips, a good first part and no problems.
Hit the bearing and seal bore fits right in the sweet spot on the first run.
The whole job stayed between 1600 and 1800 RPM roughing at feeds of 14.0, 18.2 and 20.5 with that HSS 3Fl cutter at mostly .500" axial depth.
I took some fairly heavy cuts that had my spindle load between 50% and 90% on the old Kuraki.

I have a few more of these gearboxes to make during the week now that the program/setup is proven.
The part is about 14" x 12" x 2" with 100mm bearing bores. It came from a 14 x 12 x 2.5 billet.

Gearbox (20171022).jpg
 








 
Back
Top