Not having any luck with 304 milling

[zaebis]

Cut my teeth with aliminum, time to move on to steels.

So put my 304 plate on a table, 3/16 4 flutes var helix coated carbo in a collet and opened a few round pockets (0.7" diameter) in a slab of 304 stainless. I assumed 30 as surface speed. This is a small CNC so I used 15% stepovers, 0.05" DOC and @4.5IPM. Spindle was 1000 RPM. Plunging was done at a mere 1 IPM. Level to level plunging was done straight down, no helix down.

Anyway got the job done but then looked at the endmill. All flute tips at the bottom were f***ed. The same thing happened to me on a number of other steels I tried to mill (from 1018 to cast iron). All my experiences ended with flute tips chipped on the tip on the endmill (all coated carbide US made).

1/
What am I doing wrong?

2/
Are those endmills still useable? Chips are very small but visible with naked eye.

[dertsap]

1/
your probably damaging the tools while plunging , ramp or helix into the cut , 30 sfm is extremely slow for any decent variable flute , you should be running around 300-350sfm if the tool is of quality

2/
as long as your getting the finish and sizes you need then use em till theres nothing left, after that use them as roughers till they're toasted , may as well get your moneys worth

[HuFlungDung]

I save endmills smaller than 1/4" for milling features that are small enough to require their use.

You need to feed aggressively in 304SS and the smaller diameter tools are not stiff enough to hack it, unless you use a shallow depth of cut, in which case you toast the tips because that is all that you are using.

Rough with at least a 3/8" or larger diameter, if possible.

[DMF_TomB]

3/16 4 flutes var helix coated carbo. (Do you mean carbide?) (sometimes 2 flute end mills work better)

30 as surface speed. (30sfpm for HSS for Carbide could go faster)
(30 x 4 =120rpm for 1" cutter or about 600 rpm for 3/16" end mill)

This is a small CNC so I used 15% stepovers (vibration from small machine easily chip small end mills)

0.05" DOC (Recommend 5-20% so 10% of 0.190 is 0.019" DOC or smaller, try 0.010" DOC)

4.5IPM. Spindle was 1000 RPM. Plunging was done at a mere 1 IPM. Level to level plunging was done straight down, no helix down. (Small dia end mills can get chips plugging flutes, you might need to Peg drill to let chips out)

(Any oil or coolant used?)

[PixMan]

Originally Posted by dertsap 1/ your probably damaging the tools while plunging , ramp or helix into the cut , 30 sfm is extremely slow for any decent variable flute , you should be running around 300-350sfm if the tool is of quality 2/ as long as your getting the finish and sizes you need then use em till theres nothing left, after that use them as roughers till they're toasted , may as well get your moneys worth

+1

Absolutely ramp or helix your way in, and if those are carbide endmills RUN 'EM! Way too slow on speed, and you need to load the flutes with a pre-determined chipload-per-tooth. Depending upon the quality of the substrate carbide, its coating and grind, you should be anywhere from .0003" to .0007" per tooth.