[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]

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.

[68rustang]

I have rigged up two more nozzles for a total of three.

I do not need to save this plug but there are other slots on the piece that I cannot make wider.

[justgary]

I've never cut stainless, but I have never had good luck with any full-width cut in any material.

I'm also wondering if turning your ramp into a shallower full helix (constant down Z) might help. If you haven't used it, Andy's Circle Routines would make a great addition to your wizard library. I found them in the Mach/Wizards forum, and they work great.

A corner radius endmill could also help keep side forces down, since the bottom cut actually pushes up against the corner radius. If you must have a flat bottom to your slot, you can always dress it up with a flat endmill after you cut the slot.

Please keep posting your progress. A lot of us would like to know how you eventually solve this!

Regards,

- Just Gary

[300sniper]

if there was that much full depth, full width slotting, i'd probably be talking to the local waterjet shop.

[justgary]

On thinking about it for a few more seconds, the helical ramp also changes your side cutting force to upward force since the end of the cutter is effectively plunging. It is very hard to break a mill with upward force, so that may be why your mill does not break during the ramp, but does as soon as you apply side force. Try the full helix.

Regards,

- Just Gary

[zephyr9900]

deleted (I was going to echo the mill kid's question whether the 4-flute bits are centercutting but realized that they are breaking after the ramp--I've never had good results even ramping non-centercutting bits, even in aluminum)

Randy

[68rustang]

I will keep posting but I don't know that I would consider it progress

Two additional nozzles didn't help. I really don't think it is a coolant/chip evacuation issue but I have been wrong before.

This last attempt it never actually cut anything. As soon as it came into contact with the discolored area it chipped the corners off the mill.

Andy's Circle Routines would make a great addition to your wizard library.

I will look at those, thanks.

A corner radius endmill could also help keep side forces down, since the bottom cut actually pushes up against the corner radius.

I thought the same thing and picked one up after lunch but I am hesitant to try it. It was double the cost of the coated HSS mills I keep breaking.

if there was that much full depth, full width slotting, i'd probably be talking to the local waterjet shop.

That was the original plan but with past quality issues we have had with them and the quote they gave me I have a bit of time to play with this before I would go into the red.

The cutters are center cutting.

[flick]

I will keep posting but I don't know that I would consider it progress

Two additional nozzles didn't help. I really don't think it is a coolant/chip evacuation issue but I have been wrong before.

This last attempt it never actually cut anything. As soon as it came into contact with the discolored area it chipped the corners off the mill.

It looks like it got hot where the ramp ends. Your cutter dulled and the piece is work hardened now. You need to get below/behind the work hardened skin somehow. Perhaps interpolate in the opposite direction.

Regarding your previous experience with waterjetting it... maybe you could get a better quote and end up with good quality if you specify a wide tolerance and undersize hole for the waterjetting, and then finish it on the mill. Two processes can be more efficient than one, in some circumstances.

[keen]

Hi - Quick post - I havnt read the others properly. - got a rush job on.

I do this type of work all the time on my tormach with tough steels. Your main problem lookes like the length of your cutter. In tough steel you want to avoid a cutter projection of more than 4 or 5 times the dia. Flex is expenential. But a large dia cutter in tough steel with the tormach brings other problems!

Also this type of channel through cutting is difficult to flush and the cutter will tend to eat some of its own swarf more and more after about 3 times cutter dia depth - unless you have advanced high pressure flushing.

This is more of a problem for wear - the early breakage is probably due to the first reason.