View Full Version : what is the recomended way to put a slot in stainless angle

10-17-2011, 07:24 PM
I should probably know this but I've only done it on CNC which is alot easier. A friend of mine is trying to make some brackets out of some 2" x 2" x 1/4" 304 stainless steel angle. He has to put a slot about 1/2" wide in the center of the angle (not cutting the full length of the angle). When he plunged into the angle the end mills keep breaking. Dont know if the speed and feed was right but I'll make sure when I go over to his shop. The way I have done it is to plunge straight down through and move the mill to make the slot. Is there any other ways of doing this on a manual mill. He is using a 1/2" solid carbide center cutting end mill.

10-17-2011, 07:35 PM
obviously, this depends on the machine, the end mill, and the material, but, it has been my experience that you cannot make 1/4" DOC passes with a bridgeport sized mill in 304 stainless, especially 1/2" wide slots.

you are gonna have to do multiple passes, with the DOC dependent on your machine's rigidity and the end mill- me, I would probably just be taking off .020 or .025 per pass. Thats with my 3hp taiwan mill.
Yup, its slow.
But I have made my end mills last a long time this way, on 304.
I manually lube with a paint brush dipped in oil or cool tool or something like that, too, and if you are using carbide mills, you definitely want to do a fair amount of chip clearing- carbide does NOT like recutting chips, especially in 304.

10-17-2011, 08:53 PM
Also, an end mill is a lousy drill bit, especially in stainless. Better to use a drill bit to make a hole first. It can be a little undersize if desired, maybe 15/32 or so. The next best thing would be a 90 degree mill drill, better than a square end mill would be a ball end mill.
In this case, trying to drill with an end mill is a pretty sure way to chip or break it.

10-17-2011, 10:08 PM
I just cut 8 slots 5/16 wide and 2.625 long in 304 sch 40 pipe using quality carbide 1/4 inch 4 flute endmills.

A miserable experience:mad: I ran the speed and feed at the low end for carbide - busted 2 end mills in a few minutes. Everything worked fine for a few seconds, then a ball of red heat at the endmill and busted in a fraction of a second. I called a very experienced friend and stepped him though my setup. He he told me "you're doing nothing wrong, but unless you use flood coolant, you won't suceeed". He suggested slowing the speed/feed down to HSS rate, and misting. Flood coolant at home on my BP isn't an option...

With a squirt bottle of Koolmist to "flood", I ended up roughing in small nibbles (by manual hand control - maybe 20 thou bumps with slight backoff each time) for the 1/4 inch slot, then CNC control to cut to final dimensions. Still took out more 2 endmills..:mad: :mad:, but the end result looks perfect.

I plunge cut the inital hole at about 2in/minute feed, kept coolant flowing, and had little problem. Side milling the pipe was where I failed. What made it more frustrating was that I'd just cnc cut about 60 similar slots in mild steel angle with no coolant and no problems.

Next time - 303 or forget it...

10-17-2011, 10:41 PM
Unless your running flood coolant ditch the carbide.Use just a quality two-flute HSS endmill.
Drill a start hole at the end of the slot with a drill bit,7/16 is a good size for a 1/2" slot.Run the mill at 1/2 the speed you would for mild steel,about 250 rpm.
Plunge all the way trough and mill it in one pass running about .002" chipload per flute.Brush on thread cutting oil forget all the floozy perfume.

I regularly cut 13/16 wide x 3" long slots in 3/8 thick 304ss on a 2hp b-port clone single pass.It takes a lot more time than the same cut in MS,just be patient.

Dave P.
10-17-2011, 10:45 PM
I just had to do several slots .750 wide x 7.50 long in 1/4 wall 2in sq.
tubing 304 stainless. I used a new 9/16 stub HSS end mill, drilled a
9/16 hole about .050 shy of one end of the slot. Raised the table
to minimize quill extension and chucked the endmill as short as
possible. Mist coolant cranked way up, full depth and hand feed.
Plow down one pass climb back up and climb down the other side to
hit size. I think it works better and less heat than having the end
of the mill also in the material.
BTW Bridgeport vari-speed mill.
Dave P.

10-18-2011, 01:02 AM
The way I would do it is drill a starting hole slitly undersize Then plung the 1/2" mill through move over 1/8" plunge again. work your way down the lingth of slot , then clean up the sides . Goes much faster than it sounds. I did a 18" slot in undr 2 min. that was 1/2" A2

10-19-2011, 10:12 PM
Thanks to everyone for all the help. I will have to go over to his shop and help him out when I get some time. This is something he will be doing often, so it will just be a very slow process.

Grind Hard
10-19-2011, 10:51 PM
Can you put up a drawing? It is *possible* that someone might be able to laser it for you... maybe a G-work project after hours.

mike os
10-20-2011, 03:44 AM
sounds like it is a laser or water jet job, if it were a one off then OK, but why make a rod for your own back?

10-20-2011, 11:36 PM
Yes, the ideal way to cut them is with a waterjet/laser. The thing is all of the brackets are different. It is easier for him to make them in his shop due to the constant changing of dimensions.

10-21-2011, 12:50 PM
The best way to slot the material is with a punch, but that requires a machine and tooling.

10-21-2011, 02:11 PM
How accurate do the slots have to be. Can they be cut with a plasma cutter?

Grind Hard
10-21-2011, 03:56 PM
Well, I can load multiple programs into the machine and run them in sequence.

We laser-cut fixtured parts all the time in sets... one of these, one of those, two of this and one of that.

To us, this is a thing that is not a thing really.