Slotting stainless steel shafts.

[TOTALLYRC]

I am cutting 1/4" keyways in 303 ss shafts that are 1" in diameter.
I hve been doing these on my little Atlas horizontal mill with a 1/4" wide 4"diameter? cutter and it is OK. The cutter is high speed steel as far as I can tell, but I am running the machine at its slowest speed and feed. I am using oil as opposed to a water based coolant. It is right at the upper limits of the little machine, and I would hate to break it doing this job.

I would like to move this over to my cnc bridgeport as on the Atlas it is done in 2 passes per slot and 2 slots per shaft.

I have tried a 1/4 endmill TiAlN coated but the results are less than perfect.
If I cut it in one pass the cutter seems to flex and the cuts are not very straight or I dull the cutter in three or 4 cuts.

If I do it in 4 steps, the sides of the slot slope towards the center and if I cut it so the key will reach the bottom, it will rock side to side do to the walls being slope outward. I have also noted that as soon as the cutter dulls a little bit, there is a raduis at the bottom of the slot that prevents the cutter from sitting properly, even it the rest of the cut is OK.

I am sure it is a speed and feed issue, or possibly coolant related, but I have already killed $100 in cutters. I am assuming I should be able to cut 100" of slot, which would be 10 shafts before I replace the cutter.

I tried 1000rpm and 14ipm and it snapped the cutter in seconds. I went to 1200rpm and 9 ipm and it was much better but it snapped the ends of the flutes off in the middle of the first pass.

Tried a smaller cutter, figuring I could pocket it and get a controlled width, but I jogged and snapped it off, too much coffee I guess. Before I go and buy more cutters, I would like some suggestions from the guys with lots more experience than me. Aluminum is much more forgiving if you make a feed mistake, you can hear that it is not right, but on the 304ss, I can dull a cutter and not hear any problem. The cut even looks good right until the cutter dulls.

Mike

[HuFlungDung]

303 stainless should machine quite readily, 304 perhaps not so easily. It is not clear from your post which grade you are machining.

You must avoid recutting chips, as this will easily damage an endmill. Now it is a small endmill and makes small chips, so you should be able to rig an air jet to move the chips out of the way. This doesn't require 90 psi to broadcast chips all over the shop either Get yourself some Loc Line, with a tiny nozzle (about 1/32" hole) and a Loc Line shutoff valve and a ball valve. Hook this all together, up to your airline. Using the Loc Line valve, feather the airflow until it is just a gentle airstream. Leave it at that position. Use the ball valve for your main on/off valve. Protect your eyes and bystanders from the chips.

I would probably mill that with a 3/16 or a 6mm endmill. You want a short stubby endmill that is very stiff.....perhaps only 1/2" of flute length or less, not the 7/8" long flutes of a finishing endmill. Check online at Maritool for some good double end endmills of this sort.

With the air on, make one or two roughing passes down the center of the keyway at 3000 rpm or so, 8 to 10 ipm. Use power feed if available to ensure consistent feed per tooth of the tool. Now if you have a lot of these to do, consider switching toolholders to a finish endmill, and take a finish cut on either side of center. You should be able to design a repeatable procedure for this.

Flood coolant is probably going to cause too much shock when roughing with carbide, but flood must always be used when cutting stainless with HSS. You could use flood coolant or cutting fluid to finish with carbides, because the heat generated is much less. But the air works pretty near as good, and is less mess.

Check the tool coating that you are using. Some coatings have less affinity for chip welding to the tool, which is a real problem when machining stainless and results in short tool life.

[TOTALLYRC]

In the first line it says 303ss, but I double checked and it is actually 304.
The tools that I have been using are tialn which is supposed to work well with stainless, but who knows.
I will look for a 3/16" ruffer and the do a finish pass with a finish mill.

I guess I could just call one of the big suppliers and get some advice on exactly what to use, but I thought I would ask here first.

Mike

[HuFlungDung]

Yes, TiALN is supposed to be good...I wasn't sure if it was still the best or not....seems to me there were some coatings I tried in the past that looked gold colored, but one worked a heck of a lot better than the other one.

Anyways, if you get a stub length endmill, you can feed it a lot harder without undue deflection. It is important to rough 304 quite aggressively and avoid recutting. Regular finishers just impede what you need to do because they'll snap off just when you feed them like they need to be

[One of Many]

I'd look into keyseat cutters. Typically much more stout capable of heavier chip load and accurate slot width than them wimpy endmills. Even setting up the BP with the Horizontal attachment should be more efficient.

DC

[Konrad]

HSS Keyseat cutters work best ....if you can allow a radius a the end, get it done much faster too, you always go full depth one cut, the same with endmill, get a 3/8 shank instead of 1/4, allot stiffer this way. I never like carbide this small, can cut more keyway with a good HSS endmill.

Konrad

[TOTALLYRC]

If I go the key cutter route, I can just hold the shaft between the 2 vises and come in from the side. This should allow gravity to help clear the chips.
I would like to use an endmill, but if it is going to be trouble, I will go with the keycutter.

Huflungdu,
I did see on the speed/feed chart that I was looking at that it was important to feed fast enough as to not work harden the material. Since the machine has flood colant and some shrouding, coolant is not a problem.



Conrad
I have hss endmils in the "pile o stuff" and can try one today as it is Sunday.

One of many.
I don't have the horisontal attachment for it. Since I am currently doing this on the Atlas mfc horisontal mill, a key seat cutter would be OK.

It might be an option to cnc the atlas and do it in three or four passes, as long as I can start the process and walk away until it is done, but I really would like to do it on the bridgeport.

I will try several of the different options presented here and report back.

Thanks for all the help and if anyone else has a better option. please chime in.

Mike

[TOTALLYRC]

Well it is a week later and here is the update.

I took the cutter off of the atlas and made an arbour for the B-port mill.

I found a 1" endmill holder. I took a piece of the 1" stainless shaft that I had and put a flat spot on it where the setscrew would go. I pushed the shaft all the way in and set the screw as tight as it would go. I plan on never taking it apart.

I then set this contraption up in the lathe and shimmed the whole thing so it ran true. Turned the shaft down to .8755. It gives a nice tight fit to the cutter with out having to drive the cutter on.
Since I would like to be able to use different thicknesess of cutters, I made the cutter area .500 wide. Then I threaded the rest of the shaft 3/4-16 to match the Atlas nut. Found a suitable spacer in the pile-o-parts and put it all together. 2ipm at 1200 rpm works pretty well and is definitely faster than the Atlas was cutting at.
The slot is cut in three passes and it works real well. I have done three slots and I am very pleased with the final result. It remains to be seen how long the cutter will last.

Thanks for all of the help and idea's.

Mike

[Konrad]

Mike,
I see...you're going the key seat cutter route,...good!
Can you not do it in one pass??
Not sure what diam. your cutter is but 1200 RPM seems high,
just by the looks of it, 200 RPM is more like it?
Are you not throwing dark chips?..if you do, the cutter will not last.
Another thing I see, Your cutter could have been placed closer to
your spindle or adaptor.

Konrad

[TOTALLYRC]

Hi Konrad,
I forgot to mention that the setting is 1200rpm, but I had to shift the machine into low gear, so the actual rpm is about 260.
On the todo list is to automate the gear changes and the rpm readouts.

I am using the cutter from my atlas mill since it was doing a fine job. It is actually 3"+ in diameter. Total cost=0 since I had all the stuff lying around.

I could have put the cutter closer to the actual tool holder, but when I do stuff like that, I always have to move it away later.

I am taking .050 at a time, for a total of .150". I guess I could try to do it in one pass, but it is working well. I might shoot for just 2 passes, but if I have to slow way down to keep the cutter happy, I can't see any benifit.

I find when the cutter is moved in for the third pass, even at 1 ipm, the cutter makes a lot of noise and shudders, at least until it starts moving in the x axis and stops having so much of the cutter engaged.

When I do another batch of these, and have it set up to do both of the slots in one setup, I will experiment with a deeper cut.

The shaft that the cutter is on is 304ss. I am not sure if it is rigid enough to make the cut in one pass.
I used the 304ss since I had a scrap from this job on hand. If I make another one, what should I use for the shaft?

Mike

[Konrad]

OK Mike, this is starting to make sense.
I was going to mention on the arbor using 304 SS, I guess in a emergency situation you can get by but it's always nice to have the proper tool on hand down the road. For a staggered tooth milling cutter, preferably used against chattering and smother operation, or a straight tooth cutter you're using now, I would hold this cutter on a stubby one piece milling cutter arbor, which is close to your spindle.
Actually I prefer the smaller staggered Woodruff cutters,...if you can get away with??.. these need less horse power and make a better job, no chattering.
If you're making another shaft, a harder material is preferred, [SS is too soft and flexible] I would use 4140 H. if I'm in a bind, sometimes I build better one's with 8620, then carburize heat treat then finish grind,...since we're into grinding too, it's not a big deal for me but otherwise 4140 should do.
If you're taking multiple cuts, you have uneven wear on the tool, eventually more wear on the end of teeth and after a while your slots will have a taper thus seeing the 2 or 3 pass over lap on the side, taking one pass, you're avoiding these problems, go slower speed....not necessarily slower feed, slower speed will help the chatter, thus increasing the cutting life of your tool.
Remember...when you see dark chips on HSS tools, slow down on RPM.

Milling arbor
http://www.fisherlamco.com.au/products/milling_A-B.htm

Konrad

[TOTALLYRC]

Hi Konrad,
thanks for the link.

The problem with readymade toolholders is that my machine takes a modified nmt-35 taper with modifications to be held in the tool changer.
I will look and see if I can modify one of the other holders so it can take the cutter and be more ridgid. Like I said, this was made to get the job done. I will also look to see if I can find some 4140h and give it a try.

I plan on making a few speciality tool holder and could always make a side milling holder from scratch.

If a woodruff key cutter will do the lob, then that is always a possibility.

I must admit that making the tool holder was very satisfying. I was able to shim the lathe to within a thou or so and then made the threads and such. Lots of fun.