Machining a Slot in Stainless Steel

[ngr1]

Hello, I am trying to mill a slot in a stainless steel tube but I think I do not have the right end mill. I am struggling to cut through this material.

In the photos below I have created a fixture out of plastic which tightly holds the S/S tube while the slot is machined. The slot is started by drilling a hole through the tube first.

Is this the right approach for machining a 3/16” x 1” slot in a ½” OD (.035” wall) S/S tube?

I am using a bench top mill with a HSS end mill and my spindle is turning @ 8K. I flood the fixture and end mill with cutting fluid.

Which type of end mill is best suited for this task?

I was also thinking of machining both walls of the tube at the same time to keep both slots lined up.

Any help would be appreciated!

Thanks… Norman

[little bubba]

I'll take a stab, first, you don't say what size endmill your using, but I will assume a 3/16 and at 8000 rpms, your running close to 400 SFM, therefore, your endmill is fried. You didn't say what kind of stainless or condition, that shiny silver stuff comes in lots of different kinds. If its tubing assume it is 304.

Grab yourself a machinery handbook, Amazon is the cheapest at about $57.00, ebay has some older used ones, still just as good. In this book you will look up Surface footage, (Surface Feet per Minute). It will tell you that while milling, you are going way to fast. I would suggest with a HSS bit and 304, no more than about 50 SFM, this gives you (3.8/.1875) * 50 = about 1000rpms. I'm sure there is someone that can give you a better estimate, thats just a guess, but I think I'm pretty close. Now you have to think about your chipload. On a Cnc this is easy, on a maual machine its a bit more difficult, taking a full width cut is never a good thing, but on .035 thick wall, its not going to be too bad. Lets be conservative and say, .0005 per tooth on a 4 flute endmill, that gives .002 per rev. Multiply your 1000 RPM by .002" per rev and you get 2 inches per minute, now break that down into revoluttions of your handle and do the one mississsippi two mississippi thing to try and keep an even chip load. Now if your running in 304, keep that sucker cool, you say you flood the part with cutting fluid, now does that mean flood coolant, or you are just pouring a bunch of oily stuff on it before you start cutting, the bunch of oily stuff won't really keep the heat out, it will help, but you might be better just holding an air nozzel on it while cutting.

As far as the fixture, the functionality seems pretty good, the main thing is that it is made out of plastic. One thing that you will learn and may already have and don't know it, is that rigidity is key. Think about it, your using a benchtop mill, which is not the most rigid thing going, and then you have a plastic fixture, the endmill, HSS(not very rigid in itself) pushing off of one side of the slot and pulling itself into the other, now the spindle and machine flex, say .001" and then since cutting metal isn't the easiest thing to do, the fixture moves another .002". So all of a sudden, you've gone 2 revolutions without cutting anything, and then all of a sudden your cutter, with all the forces you've built up from the deflection, starts to cut and you have a .003 chip load on one tooth that you decided should only be taking .0005", this results in one roasted endmill and one unhappy machinist.

As far as endmills go, I like carbide, but on a smaller machine that bounces around a bit, its probably not the best idea. I would get a 1/4" cobalt rougher, and then finish with a 3/16 cobalt finisher.

[Mcgyver]

everything bubba said, and probably slower. theoretical speeds assume an optimal machine and set up and are rarely achieved by us home shop types - we either have light or old machines. and after safety glasses machinery's handbook should be the next accessory one buys on acquiring a machine tool .

stainless is difficult cut - the flood is good but the material tends to work harden in the area around the cut - sort of forming a leading edge around where the metal is being removed. So on one hand you need to take a light chip load on such a small cutter and fragile set up but on the other if you don't take enough off then you aren't getting under the area thats been work hardened.

Usually I'm anti-carbide in a home shop (believing hss to be much better value) but in this case the carbine might give you a better chance against the work hardening of the stainless.

you also don't say what kind of stainless. If you have the choice, and you may not, its better to use the free cutting stainless steels if you can - they a SOOO much nicer to machine.

[ngr1]

Gentlemen, sorry for not providing enough information.

Although the machine is CNC I was jogging the x-axis manually and moving 1/16" every 30 to 40 seconds. The walls of my fixture allow for the cutter and part to be submerged in flood coolant which I add manually.

Thanks for the feedback, I will try the suggestions provided.

Norman

[ngr1]

Can someone please suggest which one of the S/S metals below would be easier to machine.

STAINLESS STEEL ROUND TUBING T-304

STAINLESS STEEL ROUND TUBING T-316

Thanks... Norman

[Geof]

Norman;

304 stainless steel is easier to machine than 316. But don't get mislead; 316 is a real b***h to machine unless you have a good rigid machine, preferably CNC, or power feed at least, so you can apply a consistent feed; 304 is only a b***h to machine. As the other people mentioned slow speed and steady feed to avoid work hardening. Hand feeding is very difficult because it is almost impossible to avoid slowing down and creating a work hardened surface. Snug your cutter as high in the collet as possible and try to work close to the top of the flutes to reduce the end load on your cutter.

[One of Many]

Originally Posted by ngr1 Can someone please suggest which one of the S/S metals below would be easier to machine. STAINLESS STEEL ROUND TUBING T-304 STAINLESS STEEL ROUND TUBING T-316 Thanks... Norman

The 304 is softer. 316 will get a premium price in comparison as I recall.

Use the shortest cutter you can find and avoid taking the full wall in one pass. Step down about .02 at a time, at least until you break through.

If you expect a 3/16" finish slot, start it with a 5/32" down the middle and finish with a 3/16" or program a path to cut to size with the 5/32".

Bubba has got to be good! I need to buy some of them cutters to start with a 1/4" rough cutter and finish off with 3/16" and still end up with a 3/16" slot........ The rest of his advice was great! There are some days when I can use a "Cut on" cutter. LOL!

The 1000rpm suggested should be fine as long as the cutter is sharp. DO NOT let the cutter dwell. If your chips are coming off blue then reduce the RPM and/or replace the cutter. Realistic feed rates will be around 1"/minute, but 2"/min could be a starting place if you can control the feedrate on the fly. If you have a feedrate over ride control, I would reduce it to 10%(.200/min) and raise it from there to match the chip load, material and cutting conditions. You can always grab a (cool) chip and measure it. .002-.003/tooth is going to be the upper limit for this small of cutter. You should not need flood coolant. A good sulfer based cutting oil would be plenty adequate brush applied.

If the tube needs the slot all the way through. You should consider a 5C collet block against a stop in the vise so it could be flipped over while gripped in the collet to cut the slot in the opposite side without losing the origin or index.

DC

[Joey]

greetings to all.
there`s some great advice given above,
if you have a Z axis handwheel you could also try slowly ramping the tool up and down in the Z axis while traversing the slot length.
This has the effect of presenting new cutting edges and preventing glazing and build-up on the tool.

[DareBee]

No need for more info, very well covered by all above

[ngr1]

Gentlemen, thanks for all of the feedback.

I was thinking about the rigidity (lack of) of my machine and whether or not the end mill option would yield the appropriate results.

After looking through the KBC catalogue I came across slitting/slotting saws with a thickness of 1/8”, which would be the ideal size for my slot. There are also cutt-off wheels with a 2” diameter that are designed to cut S/S.

Any comments regarding this option?

Norman

[Mcgyver]

imo , no. generally big cutters like a rigid set up – how slow will your mill go? Enough for a 2" cutter in stainless? also, with an end mill you can reduce depth of cut to reduce the cutting force, with a 1/8 slitting cutter you are taking the whole 1/8 at once – ie feed will control the thickness of chip but its still a 1/8 wide chip. the final thing, that pushes it over the top, is that its almost impossible to get a saw type cutter on an arbor cutting perfectly - they end up slightly eccentric and most of the of the cutting is done by a couple of teeth. This means your carefully planned chip load calc means nothing the cutter, when it connects, crushes the tube or rips it out of the fixture.

[little bubba]

Well, you have a CNC, you can get at least 8000 rpms, and obviously your slot tolerance is not critical. Get yourself some 1/8 carbide endmills and ramp ramp ramp ramp, maybe .01 per pass. Its an easy program to write. Light chip load, about .001 per rev with a 4fl. and about 130-150 sfm (being conservative). The endmills shouldn't be more than $10 bucks a piece, and should last a reasonable amount of time. Your plastic fixture would probably be fine with that too.