A Bright Red, and Now Dead Endmill - Need Help!

[Minesgeek]

Hi,

I just finished getting my mill cnc capable, and thus far have tried doing some engravings ect... just to get things figured out. I'm attempting to make a key chain, and I have some aluminum stock shims that are 1"x4"x0.06" for the material. I'm attempting to radius the corners and simultaneously cut 0.5" off one end. This also included a hole for the key chain loop. Well, the bit turned bright red, I stopped it, reduced the cut depth, turned the bit around to use the other end, and now have one ruined 1/8" endmill. Here is the setup:

-HSS 1/8" 4 flute endmill
-Spindle speed 4200 (I calculated 3055, but the belt steps between 2600 and 4200)
-Feed Rate 3 IPM
-no coolant (do not yet have the capability)

I have attached the G code file as well, PLEASE TELL ME WHERE I WENT WRONG!

[riverrat]

well, first off, coolant or some lubricant is mandatory with aluminum.
if you have no coolant cappibility, try a light oil like wd-40.
second i would go with a two flute end mill and run it at about 5
ipm. (scratched my butt on that one) it should be a good starting point.
the chip load you are running on the 4 fluter is waaaay light less than
.0002 per tooth.
my .o2 cents

[InspirationTool]

What riverrat said.

You need to learn how to do the calculations to go from sfpm to rpm, from ipt to ipm. Once you know that you will have a good starting point

If you are confused, google around... this page looks like a good start:

http://www.stanford.edu/group/prl/do...pdf/mlspfd.pdf

I'd also add something for coolant/lube.

-Jeff

[wcopley]

2 flute endmill WD or kerosene feed is way to slow try 2o ipm you have to get the cips out of the way take it all in 1 cut
Bill

[Minesgeek]

Thanks for the suggestions,

I know my tooth load is low (figured I'd just get a really nice finish), but the calculations weren't the problem. I've concluded that the material I'm using is not aluminum. It is non-magnetic and slightly darker than most aluminums, and is also much harder (can scratch aluminum quite easily). It was sold to me as scrap aluminum, and I think it's heavier although I don't have a scale. In short I have no idea what material it is, so I don't think I'll ruin any more bits trying to machine it.

Thanks,

-Nick

[wcopley]

Oh Sh**t may be inconel or some other nickle based material slow down rpm and feed rpm is way to fast
Bill

[wcopley]

Im not sure if youre using carbide or not high speed use aprox 40sfm
carb 60 sfm aprox
Bill

[CarbideBob]

If you don't know what the material is start with a very low SFM ( around 30) and a chipload of 2-3 tenths per tooth. Too low of feedrates are very bad for endmills. You have to advance the cutter far enough to bite into the material to create a shear plane which pushes the heat into the chip and away from the cutting edge. Reducing DOC will not reduce the heat at the cutting edge (it simply use more edge length). I see more endmills ruined by lack of feedrate than any other problem. Start slow and work your way up.

[aggie_67]

Should be able to judge how hard it is (alum or inconel, etc) by a trial cut with a hacksaw!

[Minesgeek]

CarbideBob,

I've never heard that too low a feed rate is bad for endmills, what is the lowest chip load you suggest for HSS and aluminum? The material is harder than nickel, I was able to scratch an old nickel with a corner of the material.

Edit:

I tried cutting a scrap piece of aluminum with the original g code, worked just fine!

[CarbideBob]

You need enough feed to keep the tool biting into the material and not rubbing. At very light feeds the tooth rubs on the surface and the endmiill bends until enough force is finally applied then the next tooth can penetrate the surface. This generates lots of heat and workhardens the surface being cut. As strange as it may seem when applied properly the very edge of the cutting tool is not even in contact with the workpiece. What happens is the metal is being pulled apart ( from the chip flowing across the face ) creating a shear zone just in front of cutting edge. Anytime I see less than .0003 per tooth I get worried. Many factors influence the optimal chipload. Climb milling can user lower rates than conventional milling because the cutter enters the cut at it's thickest area. Basic rule 1 - thicker chips are better. Basic rule 2 - If the workpiece gets hot the tool is rubbing not cutting. Small endmills are problematic because they lack the strength to take high chiploads. I examine the chips produced and the surface that was cut under a 60X microscope to see it the tool is cutting cleanly but trying to describe what I'm looking for is very hard to do ( are the cuts evenly spaced, is the material rewelding to itself). This really is a trial and error process. With small endmills I start at 3 or 4 tenths per tooth but with a 2 inch cutter I start at .006 per tooth. Look at your used tools (after a few cuts but way before they die) with a microscope or magnifiying glass. Is the edge melting? Is the chip flowing smoothly across the front face? I hope this helps.

[dertsap]

Originally Posted by Minesgeek Thanks for the suggestions, I know my tooth load is low (figured I'd just get a really nice finish), but the calculations weren't the problem. I've concluded that the material I'm using is not aluminum. It is non-magnetic and slightly darker than most aluminums, and is also much harder (can scratch aluminum quite easily). It was sold to me as scrap aluminum, and I think it's heavier although I don't have a scale. In short I have no idea what material it is, so I don't think I'll ruin any more bits trying to machine it. Thanks, -Nick

is it possibly titanium ?