Need Help!- Slotting 316 stainless with my PCNC-1100

[68rustang]

I am asking this here instead of "general machining" because you guys are familiar with the machine.

I have had my mill for about two years now. I mostly use it for cutting polypropylene and brass. I have a need to cut some full width slots all the way through 1" thick 316 stainless steel and need some help with the calculations.

Material: 1" thick 316 SS
Cutter: Held in TTS set screw holder
Niagara Cutter four flute single end mill
5/16 DIA
TiN coated HSS
List SMC411T
EDP 41100

In looking around I am seeing feed and speed ranges all over the place. I am looking for some real world numbers or recommendations.

[the mill kid]

Hey There,
not sure about your machine but I have cut plenty of 316 on a verticall mill and maybe I can give you a good starting point. With a hss endmill I would start between 70 to 100 sfpm. so sfpm x 3.82 divided by dia. = rpm. I would run the feedrate about .0008 per tooth so about .003 feedrate. Normally when slotting your depth of cut should be half the dia. of the endmill. If you are plunging into the pc cut your feedrate in half on the z move and make sure your endmill is center cutting! If you decide to get yourself a carbide endmill you can run your sfpm starting at 200 and pick up you feed to about
.0015 per tooth. SGS makes a great carbide endmill called a z carb that runs at 300 sfpm! Depending on how many pcs you could seriously cut your production time. Good luck.

[68rustang]

I appreciate the input.

Half of what I read says light slow cuts, half says heavy fast cuts, and the other half says light fast cuts. Half + half + half = I'm confused

Reading about stainless I need to watch out for work hardening yes?

[BlueFin]

Originally Posted by 68rustang Reading about stainless I need to watch out for work hardening yes?

I have never cut stainless, but I have read something from Greg of Tormach where he explained that the first pass will go smooth if you make a light cut but then the second pass will be hard because the cutter teeth hitting the material is like little hammers. The cutting should be climb milling so the teeth engage at a 90 degree angle and plunge straight in, and the cut should be deep enough so when the cutter passes through the cutting arc to a perpendicular motion you are now below the hardened zone. I think I saw this in the owners manual.

[the mill kid]

I have never really had a problem with work hardening while milling, sometimes this can occur when drilling at to low a feedrate, but i'm sure if your running to high an rpm and a slow feedrate some workhardening will happen. Check out your endmills manufacturers web page they should have some good starting points for the material and endmill you are using, or try calling there tech support.

[68rustang]

Well this isn't going as smoothly as I hoped

My settings:
SFPM = 85
RPM = 1040 (actual 1074)
Feed = 3.5 IPM
Axial DOC = .0781
Ramping into the material @ 15*
Flood cooling

All is fine until it was about halfway through the material (.4686", 6th pass) it broke the cutter just after it finished ramping down. I replaced the tool, restarted and it finished that pass with no issue and then broke in the same place on the next pass (.5467", 7th pass.)

From what I can see looking at the resulting cut the issue starts during the ramp down and it can be heard in the machine.

Any ideas?

[Runner4404spd]

I'd be willing to be that you don't have flood coolant or are not evacuating the chips from the slot. if you recut stainless chips you will break your end mill.

[the mill kid]

is your feedrate cut in half on the ramping? also are you running a rough and finish endmill, if so you can use an endmill a little smaller than the width of your slot and do a helical move down to your depth on your roughing passes, this will work pretty well. If your still having trouble cut your depth of cut in half and plunge straight down with no ramp. runner4404spd is right too make sure the chips are evacuating get good coolant pressure right at the tip of the tool

[68rustang]

My feedrate is constant. The coolant is keeping the slot clear of all chips. I am going to try adding more coolant nozzles. It is a circular slot so getting the coolant on the tool at all points is difficult.

[the mill kid]

you could also try drilling a hole at the plunge point and start your endmill in that hole.

[68rustang]

Some pictures:

Circluar Groove

Circular Groove

Coolant Nozzle

Broken Mills

First broken mill on the left, second on right was stopped before it shattered.

[300sniper]

looking at your pictures, i had a hell of a time doing something very similar in a-36 steel. i was trying to use a 4 flute 1/2" carbide endmill full width with a finish depth of about an inch. i could not get the chips out of the way and i was killing my endmills. on my project, only the inside diameter was critical so i made the cut .75 wide instead. i'd make a full width pass around and then the next pass was only 1/2 the cutter diameter. i'd go down in z and do the same thing until i got to my final depth. this kept the slot wide enough compared to the depth that chip evacuation was much easier and recut became no existent.

i think 1" deep, 5/16" wide is going to be very tough to get the chips out of the way without some serious coolant pressure. i think chip evacuation is more of your problem than the material although i don't have much experience with stainless.

edit: if you don't need to save the plug that comes out of this, what about doing a circular pocket? this would allow plenty of room for coolant. sure it would take longer but it would probably be cheaper than replacing endmills.