PDA

View Full Version : working with stainlees steel



luis hernandez
10-04-2001, 09:24 PM
I will buy a Sherline mill and I will be using a 1/64 carbide end mill. I want to make a slot on stainless 316L bar .018" width X .030" deep x 1"long so my question is:

Can this machine handle this metal?

has someone tried a Sherline on this metal?

has someone tried a 1/64 end mill?

what should the RPM and feed rate?.

Would it be better to cut this metal with an Slotting Saw?

Thrud
10-05-2001, 03:56 PM
Make sure your workpiece is clamped so it cannot move. Because you are using such a small endmill crank it all the way up in rpm's and take he cut very slowly. Providing you do not break the endmill by force feeding it more than it can chew you will not have any problems.

It will machine nicely dry, but you could use some cutting fluid applied (easy does it) with a insulin needle if you wish.

Have fun.

Dave

SGW
10-05-2001, 08:48 PM
316 isn't the greatest thing in the world to machine, but given the size you're talking about I don't see why the Sherline couldn't handle it as well as anything else.

Personally, I've usually found slitting saws to be more efficient at making grooves than end mills; the question is, does the geometry of the cut let you use one.

If you use a saw, you'll want to keep the rpm down pretty low because of the saw's relatively large diamter. The important number is surface feet per minute (SFPM). For a 1/64" end mill, you can whizz it at a great rate and the SFPM of the cut will still be relatively low. With a 3" diamter slitting saw, though, even a hundred rpm will give you a pretty respectable SFPM.

luis hernandez
10-05-2001, 11:08 PM
How long would it take a 1 1/2" dia X 1/64" thick slotting saw to make a .030" deep X 1" long cut on stainless 316L? you do not have to be precise just give an estimate...

also give a estimate using an 1/64" end mill cutting the same size slot..



[This message has been edited by luis hernandez (edited 10-11-2001).]

SGW
10-06-2001, 07:55 AM
Time estimates?!? This is a hobby! Hobbies doen't take time. ;-)

But for a wild guess, never having done the exact thing you're asking about....

I'd guess the slitting saw might take 5 minutes, the end mill 15 minutes. And I'd worry a whole lot about breaking an end mill that small Maybe some of the more professionally-oriented members here are better at estimating time than I am.....

C. Tate
10-06-2001, 09:36 AM
Luis,

50 sfm divided by 1.5(dia of saw) multiplied by 3.82(constant) equals RPM. 50 surface feet per minute is a good place to start on any high speed tool in stainless steels like 316. The feed rate in inches per minute is determined by multiplying the rpm by the chip load per tooth and multiply that number by the number of teeth on your saw. I would say for a saw this size and on your machine .001 chip load per tooth would work fine. I get 127 rpm and about 1.27 inches per minute on a saw with ten teeth.

Remember that 300 series stainless steels are nickel based alloys. The stainless is soft in comparison to many types of carbon steel but it has a tendancy to build up on the cutting edge when run to fast. Use oil or water soluable cutting fluid to prevent build up. General rule of thumb is low rpm and increased chip load when compaired to carbon steel. Allways use very sharp tools on stainless and for the home shop I would save the money and use high speed instead of carbide. A .015 carbide endmill will not take hand feeding on your machine, the run out from the spindle will cause breakage almost immeadiately when you contact the material IMO.

Good Luck

BrianH
10-06-2001, 11:27 PM
Luis;
I would say if your job can be done with a saw, I would go that way. As mentioned before, run it slow; I prefer a slightly thicker sauce on stainless, not water-based, Tap Magic works great on all kinds of stainless.
HSS 1/64" em won't make it 2 passes in 316.
If your going to use an endmill, buy more than one, because a cutter that small will snap if you look at them wrong; plus stainless needs a sharp tool.
Carbide, at about 3 grand, plenty of sauce, one or two thou deep per pass, feed at an inch to an inch and a half a minute.
(You'll probably lose your cutter plunging your next pass, so if you can't start off the edge of the part, consider drilling a pilot hole to start your cut in....)

Dave the Nave
10-09-2001, 11:09 PM
So luis,how many of these do you have to make? Is it long run production?A few years back I had 150 pieces to make out of 304 S.S. with very similar dimensions that you described.Only in my case the slot was .025dp.x.031wide x .5 long.I did'nt use an end mill,a slitting saw,or even an E.D.M. for that matter.I used a Kurt Anglock vise.I just made a form punch out of O-1(oil hard)to the dimensions above,and used the Kurt vise to compress the form punch into the parts,(average time;5 seconds each) I used a 1in.travel indicator on the movable vise jaw repetative accuracy.Just my 2 cents.

luis hernandez
10-10-2001, 12:31 AM
If I can make that cut that fast I'll be really happy (1.27" per minute) wow.

also you said that if I used hss rather than carbide will be chipper So don't you think carbide will last more?. According what you said the end mill that size will break So basically there is not way to use End mill 1/64 on stainles steel?.

thanks you have answered almost all my question about this.. thanks..




[This message has been edited by luis hernandez (edited 10-11-2001).]

luis hernandez
10-10-2001, 12:42 AM
Well it is long run production. I'm going to manufacture this small part and I do not see other way to do it. I took a look at MIM metal injection but that process is to expensive. you mentioned EMD, Are you talking about plasma? Do you think I can do this slot with a plasma?.




[This message has been edited by luis hernandez (edited 10-11-2001).]

Thrud
10-10-2001, 01:06 AM
Luis

He is talking about E)lectric D)ischarge M)achining. It uses high current to vaporize the metal.

I think Dave the Nave has the best idea. Make a steel punch the same size as the groove and press the groove into the metal as he suggests. (Those Dave guys are so smart...)

If the piece cannot have any distortion machining is the way to go.

The reason someone suggested HSS endmill is because the carbide shatters easily when it is that small from force feeding it into the cut - the HSS is more flexible but can still be damaged if you get carried away.

Dave

luis hernandez
10-10-2001, 01:02 PM
Well the piece should be with a smoth surface and the finishing of the part is very important. However; I can try that idea..




[This message has been edited by luis hernandez (edited 10-11-2001).]

C. Tate
10-10-2001, 10:43 PM
<font face="Verdana, Arial" size="2">Originally posted by luis hernandez:
If I can make that cut that fast I'll be really happy (1.27" per minute) wow.

also you said that if I used hss rather than carbide will be chipper So don't you think carbide will last more?. According what you said the end mill that size will break So basically there is not way to use End mill 1/64 on stainles steel?.

thanks you have answered almost all my question about this.. thanks..


</font>

Luis,

That was an estimate made on limited knowledge. It may take longer or it could be faster. I like the idea of forming the slot. If tool life is extremley critical you can buy carbide slitting saws they are fragile just like the emill but as long as you don't put too much side load on them or hang it in the part it will cut fine.

I am not saying that you cannot use an emill I just feel that it will be very difficult. Your machine will not even come close to generating the RPM necessary to run a .015 dia emill properly my calculations indicate you would need a little over 12,000 RPM to achieve 50 surface feet per minute.

Good Luck and keep us imformed of you progress.

[This message has been edited by C. Tate (edited 10-10-2001).]

luis hernandez
10-10-2001, 10:59 PM
Do you have any idea which stepper motor
I could use for this? 100 oz,150 oz or 200 oz?. Do you think a Sherline can hadle stainless?. some people do not like the idea to use a sherline with stainless but others claim that sherline will work just fine doing a cut like that. I would like to heard your opinion on this..



[This message has been edited by luis hernandez (edited 10-11-2001).]

Thrud
10-11-2001, 03:28 AM
Luis,

When you reply you should highlight and delete the quote to save space.

Haas has a CNC toolroom mill for $20,000. It could handle the carbide endmill without breaking it. And it looks damn nice in the shop, too.

Remember to use a screw slotting saw and not a slitting saw if you go the saw route.

I would still just mill it out with a Carbide 2 Flute or Single Flute Endmill - be gentle - it will work great. Crank the RPM's to max.

For all the yaking we have done on this topic it would have taken less time just to do it.

Dave

Come to think of it, a laminate trimmer could be set up to do this as well with a good jig, and the 20-30,000 RPM's would cut like crazy.

[This message has been edited by Thrud (edited 10-11-2001).]

luis hernandez
10-11-2001, 12:53 PM
what is the difference between a screw slotting saw and a slitting saw?

Thrud
10-12-2001, 01:38 AM
Luis,

A slitting saw has fewer teeth and is designed to part material not mill it. The teeth have a tendency to cut unevenly as if the saw is not running true. This is "normal" for slitting saws.

The screw slotting saw is actually a fine tooth milling cutter for making the slots in screws It will produce a flatter cut at the bottom of the kerf than a slitting saw can.

Dave

artificer in metal
10-14-2001, 12:14 PM
The shop I work in uses mainly HSS mills and these are even used in Monel!! By the way 304 SS is easier to work than 316. The formula says turn your 1/64" cutter at over 6000 rpm but 3000 with a very easy touch on the crank with some coolant will work. Carbide is great if you can easily control the feed but with hand cranking I would go HSS most always. (IMHO!!)

luis hernandez
10-14-2001, 01:16 PM
Many experts claims the 1/64 end mill will break as soon as it touch the metal but I will try it.

My other question is:
has someone works with 17-4 ss?. it is supposed to be a soft stainless steel.

any advise....

BrianH
10-14-2001, 07:31 PM
Nope. Not soft....but a little easier to work with; that's primarily because it has carbon in it. Also the preciptation-hardening process makes for a little more brittle chip, thus a little more freeier machining than, say, 304, with lots more nickel and chrome, and no carbon...that gives you a chip that won't move, won't sheer, and doesn't dissipate heat, so it just burns up your tool.

I spend probably most of my time working with various grades of stainless (engineers seem to love it), and it's all machinable, it's just some of that stuff that takes practice.