[Santiago99a]

I need help here. It is my first time to machine on S.S material and I have tough time machined on 304 stainless sheet thick (.032), I used diameter .125 flat endmill HHS and ticn, 1100RPM and pass cut per deep .010, use coolant, slower on feed rate .5. I run on ss sheet for profile program and pocket program but the flat endmill broken 3 times again after done 1 part, machined rec shaped about .75 x 1.20 i need to machined and make 9 parts. The flat endmill got chipping on corner edge and uneven. Any suggestion? Did i do something wrong? please let me know. Thanks.


Santi

[neilw20]

HSS is hopeless for stainless steel, and so is ticn (IMHO). Use solid carbide.
I have been using 0.125 flat endmill at 0.015 DOC, 0.5 IPM (max) 3600 rpm.
If you can't run that fast use 0.15 IPM at 1100 rpm.

You must go really slow, because the side load bends the cutter. I have been going to 6mm deep with that setup. Nothing broke in 10 hours.

For thin things I would just get a dead 1/8" broken very short carbide drill and grind it dead flat on the end.

The dead flat grind is for using the drill for a mill in THIN SHEET.

With the thin sheet I assume you are cutting slots. Easiest to pre-drill a starting hole. At edge of sheet advance at 10% of your normal feed rate until fully engaged both sides. The job supports the side loads.

For thin sheet I just drill through, and then use the drill drill as a milling cutter up near the end of the flutes.
Lots of flood coolant with soluble oil to clear the chips. The chips will break cutters.

When plunge milling, if you must, you must not ramp down in Z more than about 0.01" per inch. Any more will bust the cutter.
You need a slot mill grind to achieve this. I just sharpen broken drills for this.
You need a CBN or green grit wheel. Look at a slot mill and copy the grind shape used.

A good source of broken/blunt drill bits, this size is your local PCB manufacturer. Ask them to throw all the old bits in a box for you.

[HuFlungDung]

I'm not in agreement with Neil about using drills for endmills: drills do not have a relieved land, and make poor tools for side milling, especially in stainless. I also don't agree with the dead flat end grind, although I would grudingly admit that it might help hold the material down on the table. If it doesn't create a burn mark, then I suppose no harm done. I always give a regrind a bit of concave end relief to reduce friction.

Stainless requires sharp, rigid tooling. Standard length 1/8endmills are too long, you need stub length (or make your own by regrinding worn/broken endmills).

I would say that for HSS, your rpm is a bit slow, as is the feed. You should , at .010 depth of cut be able to cut 2500 rpm and 5 ipm. Running the feed too slow prevents the tool from getting under the chip, resulting in a whole lot more rubbing and heat buildup. Stainless is a poor conductor and heat rapidly builds up in the cut zone unless you can keep the feed up, quickly spoiling the sharp corners of any tool.

Keep the coolant on it. You might also perform a delicate chamfer of the flute tips, as these will endure much longer for roughing than razor tips.

[Santiago99a]

HSS is hopeless for stainless steel, and so is ticn (IMHO). Use solid carbide.
I have been using 0.125 flat endmill at 0.015 DOC, 0.5 IPM (max) 3600 rpm.
If you can't run that fast use 0.15 IPM at 1100 rpm.

You must go really slow, because the side load bends the cutter. I have been going to 6mm deep with that setup. Nothing broke in 10 hours.

For thin things I would just get a dead 1/8" broken very short carbide drill and grind it dead flat on the end.

The dead flat grind is for using the drill for a mill in THIN SHEET.

With the thin sheet I assume you are cutting slots. Easiest to pre-drill a starting hole. At edge of sheet advance at 10% of your normal feed rate until fully engaged both sides. The job supports the side loads.

For thin sheet I just drill through, and then use the drill drill as a milling cutter up near the end of the flutes.
Lots of flood coolant with soluble oil to clear the chips. The chips will break cutters.

When plunge milling, if you must, you must not ramp down in Z more than about 0.01" per inch. Any more will bust the cutter.
You need a slot mill grind to achieve this. I just sharpen broken drills for this.
You need a CBN or green grit wheel. Look at a slot mill and copy the grind shape used.

A good source of broken/blunt drill bits, this size is your local PCB manufacturer. Ask them to throw all the old bits in a box for you.

Hey NeilW20,

Thanks for recommand to use carbide flat endmill. I have been using .125 flat endmill (3 flutes) at .005 DOC, 6.0 IPM at 4200 RPM with lot of coolant. After done pocket program square about .25 x .25, I glad there is no break chipping on the cutter. It suppose running at 7.33 IPM 4900 RPM and .010 DOC but our CNC machine running limit up to 4200 RPM that is why I use 6.0 IPM and .005 DOC instead i dont feel conflient it may bend the cutter and break because it run too fast at 6.0 IPM with .010 deep.

I did run profile program with .25 flat endmill Carbide (3 flutes) at .010 DOC, 2400 RPM and 3.66IPM. It running fine and went smooth after 8 parts but there is chipping on the cutter (on 1 flute, another 2 flutes are fine) a bit after program 9th part. I need to machine one more part, i go ahead to use cutter with a bit chip on it, change a little slow on feed rate, it worked. Thanks for your help. I really appreciated it.

Santiago99a

[Santiago99a]

I'm not in agreement with Neil about using drills for endmills: drills do not have a relieved land, and make poor tools for side milling, especially in stainless. I also don't agree with the dead flat end grind, although I would grudingly admit that it might help hold the material down on the table. If it doesn't create a burn mark, then I suppose no harm done. I always give a regrind a bit of concave end relief to reduce friction.

Stainless requires sharp, rigid tooling. Standard length 1/8endmills are too long, you need stub length (or make your own by regrinding worn/broken endmills).

I would say that for HSS, your rpm is a bit slow, as is the feed. You should , at .010 depth of cut be able to cut 2500 rpm and 5 ipm. Running the feed too slow prevents the tool from getting under the chip, resulting in a whole lot more rubbing and heat buildup. Stainless is a poor conductor and heat rapidly builds up in the cut zone unless you can keep the feed up, quickly spoiling the sharp corners of any tool.

Keep the coolant on it. You might also perform a delicate chamfer of the flute tips, as these will endure much longer for roughing than razor tips.

Hey HuFlungDung,

You are right that my feed rate and rpm is a bit slow. I calculate what is best and right to use on feed rate and rpm. I did use diameter .125 flat endmill with 3 flutes at 4200 rpm, .005 DOC and 6.0 IPM.
Do u have any idease how many at RPM? i will use to run .25 flat endmill carbide (3 flutes). I not sure if i run too fast rpm at 2400 with .010 DOC at 3.66 IPM, plunge rate is .60. There is a bit chipping on the cutter after machine 8th part with profile program. Just curious what will be your RPM to running .25 flat endmill carbide. thanks for your help and I really do appreciated it.

Santiago99a