Need Help!- Are these end mills made of carbide or glass???

[ryansuperbee]

Hey everybody. I am CNC milling 1/4 inch thick 304 stainless steel. I have brand new 3/16 diameter end mills that I am trying to use. I am only sinking them down 0.09300". At 2000 RPM and 4 inches per minuet. the bit sinks down into the material fine, but as soon as there is any X/Y travel, the bit instantly breaks! I went through two of them, and finally went with my HSS bit, which worked fine for a while. Are carbide bits this small not recommended for stainless work? Should I be using a 3/16 cobalt end mill instead? Please help!!!!

P.S. I have a large CNC mill, so clamping and horsepower are not the problem. And anything larger than 3/16" is not an option.

[sti2011]

Sounds like your RPM is way too low and, feed at that RPM too slow.
I would start at 300sfm and work up from there if possible. I would keep chipload on the low side as it sounds like you are "slotting"
6000rpm, 4 IPM for a 2 flute and maybe 5-6 IPM for a 4 flute. Keep the coolant right on the tool.

[Cruiser]

2000 rpm with that size of carbide is way too slow ! go for max rpm you have available and feed at .0005 chip load per flute. you did not say how many flutes you have, should be 4 or 5 flutes with stnls steel & modest feed, speed should be about 5300 rpm for that size or even a bit more. Also, there is a chance of building a bug on the end of the end mill plunging, so it is best to angle feed to depth or use a circular interpolation to depth and .09 may be too deep, try .03/.045 and work up from there. with stainless you don't want to push too hard and definitely don't want to rub at all or it will work harden at the tool.
Good Luck

[PixMan]

While I agree that 2000rpm is too slow for a 3/16" end mill, I would arbitrarily say "go for the max rpm you have available". How fast you go depends upon the carbide substrate, coating, chip load per tooth, chip evacuation, depth of cut, width of cut, etc.

2000 rpm is only 98 sfm. A cheap, uncoated C2 grade of carbide in 304 is something I might start at 250sfm, so about 4500 rpm. At a .093 depth of cut and if cutting full width (.1875"), I might start at .0003" chip load per tooth and flood coolant. Those are starting values. A high-quailty sub-micron grain carbide coated with AlTiN with 45º or 50º helix of at least 3 flutes, I might run at over 650 sfm, .0005" ipt and dry.

What end mill is being used, how much speed do you have available?

[universalfab]

If you can't go faster then 3,800RPM you should be using HSS.

[dertsap]

Originally Posted by ryansuperbee the bit sinks down into the material fine, but as soon as there is any X/Y travel, the bit instantly breaks! .

when you say the bit sinks down into the material , do you mean that you are straight plunging into the stainless ? are these center cutting tools ?

[bret4]

That is what I was thinking. Are they center cutting tools?

Also I think .093 is a bit deep of a cut. I'd back off to .015 to .025 deep.

Also rev up to rpm and if needed cut the feed to 2ipm.

Another thing is are you sure on the grade of the St St? I know the knot head that cuts our metal for our shop sometimes cuts the wrong grade and you know as soon as you go to machine it.

[BobWarfield]

Originally Posted by ryansuperbee Hey everybody. I am CNC milling 1/4 inch thick 304 stainless steel. I have brand new 3/16 diameter end mills that I am trying to use. I am only sinking them down 0.09300". At 2000 RPM and 4 inches per minuet. the bit sinks down into the material fine, but as soon as there is any X/Y travel, the bit instantly breaks! I went through two of them, and finally went with my HSS bit, which worked fine for a while. Are carbide bits this small not recommended for stainless work? Should I be using a 3/16 cobalt end mill instead? Please help!!!! P.S. I have a large CNC mill, so clamping and horsepower are not the problem. And anything larger than 3/16" is not an option.

If you're slotting with a 3/16" at 0.093 DOC, 2000 rpm, and 4 IPM feed, your predicted tool deflection is 0.002" with a 1" stickout (deflection calculated by G-Wizard). That's about twice what you should allow and will make your tool more prone to breaking from the flex.

That cut has a chipload of 0.0005, which is a little more than half what it should be. That can lead to work hardening in stainless.

If you're width of cut is significantly less than full slot, say it's 0.040" for example, radial chip thinning make make your chipload even less, which makes the cut even more prone to work hardening.

Best,

BW