HELP!! slotting in 17-4PH again. this is getting costly

viper · Jul 15, 2008

A couple months ago we were doing a slotting job in 17-4PH with an H900 HT and we are again making them and again pulling our hair out. These are pins that are .3125 diameter and require a clevis type slot in the end that is 1.25in long and all the way through through the part so .3125 deep. The slot is .125 wide.

Before we were using 4FL EMs by Imco. They were varimills and we ran them anywhere from 5900-7500rpm with feeds of .0004-.0008/tooth. DOC also varied from 6 passes to 9 passes. Nothing I did would keep the mills from breaking after about 12-17 parts. Sometimes 20 if I am lucky.

Today, we are revisiting this job and tried some 60 degree helix 3FL mills also from Imco with much sharper edge prep. They made ZERO noise during cutting the first two and then broke on the 4th part. The broke part of the mill showed that two of the the three leading edges of the flutes broke and there was a chip higher up on one of the flutes. I ran these at 7500rpm, 10ipm, and DOC of about .055.

All the varimills we ran showed very little wear or damage on the cutting edges and always broke at the top of the fluted parts which indicate excessive load I guess. All mills are being run with a TON of coolant from three angle and 1in from cutter. If I run dry, the cutter will last one part if that.

I am just doing a linear mill from the open end of the part and because I cannot find much for mills below .125D, I don't have too many options for milling paths. So any ideas here?????

Perry Harrington · Jul 15, 2008

I forget, but why aren't you using a carbide slitting saw to make these slots? You say it's like a clevis on the open end, sounds like a straighforward saw job.

viper · Jul 15, 2008

Well, honestly, the only reason is because all my ops were designed to run off the same tool and I will have to destroy hours of work to use a saw for this. I guess if I can find a saw with a full radius tooth, I might try to figure that out. The way it looks now, I am in for about 30 hours of milling and 3-400 bucks in mills if I keep doing what I am doing.

Dunno, maybe doing two parts at a time will be faster than 4 parts to slow way. I have never used a saw but I am pretty worried about chatter because I will not have much support on the material right at the cut if you can image pinching a round part and then slotting it. You do have me thinking though.

rklopp · Jul 15, 2008

I see Travers Tool has 0.120 dia x 0.360 long 2- & 4-flute solid carbide endmills on p. 190 & p. 192 of their online catalog. They list numerous 1/8" dia x 3/8" long ones on p. 225 & pp. 230-236, p.240, p.242. One of those 0.360-long ones would be about as short as you can get and still make the cut, and they are <1/8" diam so you could contour the cut and climb mill both walls for a good finish.

Is it possible you are pinching the slot onto the cutter when you get at or near full depth, and you end up with the cutter loaded over a full 5/16" of length? If so, you might consider a necked down mill like Travers has in the middle of p. 275, though the shortest of those is 17/32 overall with a 3/16" flute length. With the solid shank, that still might be overall stiffer than a shorter endmill with flute the full length. I've used the 1/16" ball nose version of those at 15/32" length, but only on 7075 aluminum. Another approach would be to make the slot progressively narrower as you go down, then take a final light finish contour pass over the full depth wall. Of course that won't work with a 1/8 endmill. Do you get chatter fro the harmonics of the "tuning fork" prongs you are making?

fpworks · Jul 15, 2008

Although my experience is with a different material, it is a challenge for the tool, so I'll share this much: I have a part that has a .125 wide slot, 0.320" deep in ALUMINUM. I rough it in one pass at 12k rpm and 42 ipm...BUT if I use any type of toolholder other than a heat shrink or hydraulic, it will only last about 4-5 inches in the cut before it snaps. 0.0003" runout from an ER16 toolholder was too much. With a hydraulic or heatshrink holder, the endmill easily lasts the 2800 linear inches of the batch. (after which I kiss the endmill and toss it in the garbage.)

Clearly, these smaller tools are sensitive to runout...I would imagine this is even more important in your application.

viper · Jul 15, 2008

Yeah, before I was on a mission for zero runout to see if that was all the problem but never got there. I think about .0005 at the tip of the tool is as good as I can get right now. You comment is VERY interesting and that a DRASTIC difference in performance. I might try tomorrow to see how I can get like NO runout and see what happens. Wish I had one of those slick holders to try...

To answer the question above, the tool will break at random and many times near the top of the part so I do not think pinching is causing tool failure here. I would tend to look direct at that if I was near the bottom every time though.

I meant to send some scrap to Imco to see if they would do some testing with it but that did not happen. Just wish I knew what was causing the failure so I could fix it.

rklopp · Jul 15, 2008

With that much runout and your stated chip loads, it looks like one cutter flute is doing all the work, and then some.

PBMW · Jul 15, 2008

Saw cut it. I don't care HOW much time you have into it now., it ain't working . First thing to do when you realize youre just digging a deeper hole is to stop digging....

apestate · Jul 15, 2008

How exactly are you holding the part? Collet?

Is this what you are doing?

if it's like this, try slowing it way down so it doesn't chatter and bust the end mill, like 1800 rpm, 3 ipm, .08 depth x 4 passes or something.

GarlicDude · Jul 15, 2008

Can you drill a series of holes, say 7/64 that almost intersect for the length of the slot?
The time spent drilling the holes might be made up with fewer passes at a higher feed rate.

viper · Jul 15, 2008

Two questions, Is there any way to "tune" a holder for better runout? We test a BUNCH of new holders in several machines including G2.5 rated holders in new Haas spindles and it would seem that bigger mills have NO runout but small mills have runout. No ideas there...

Also, where would I get a saw setup if I wanted to go that route? Do I need carbide teeth for this? Do you think 1-2 saws would do say 1000 slots?

Perry Harrington · Jul 15, 2008

The only way I see to end mill that [reliably] is to use an undersized endmill with the trochoidal pathing, but I think that was a suggestion you got last time too...

Perry Harrington · Jul 15, 2008

viper said:
Two questions, Is there any way to "tune" a holder for better runout? We test a BUNCH of new holders in several machines including G2.5 rated holders in new Haas spindles and it would seem that bigger mills have NO runout but small mills have runout. No ideas there...

Also, where would I get a saw setup if I wanted to go that route? Do I need carbide teeth for this? Do you think 1-2 saws would do say 1000 slots?

Robbjack makes good saws, call them up and ask them what to buy and how to run it. Off the top of my head, I'd run the saw at just barely the DOC needed to go all the way through, then once I got to the point where the slot ends, mill it straight across the face. If you want a radius, go back and plunge it with an endmill. Or do the radius first and stop your saw 1/2R away.

viper · Jul 15, 2008

6 flute, .125 EM for nasty hard stuff??????

I found some of these and was just wondering if this could work?? I know 6 flutes does not give much evacuation but maybe it can create a finer chip that will flush out better?

After talking with Curtis, I am going to try another of these tools and pull it BEFORE it snaps and see if I can determine what is failing on the cutter or find a wear pattern. Curtis agreed that this method "should" work though I am still shopping for saw components as a backup.

Mud · Jul 15, 2008

There are saws made that hold carbide grooving inserts for teeth, that would make mistakes less expensive than solid carbide saws or brazed carbide saws. They mount on regular 1" arbors.

apestate · Jul 15, 2008

viper

go up and look at post #9 -- I posted a picture but it wasn't there for about half the day today for some reason

I can't really visualize what you say you are doing. Are you holding the thing in a collet and sticking it out 1 1/2" or whatever then machining a pocket down the middle? I drew a picture of a 5C collet block with a part sticking out horizontally, unsupported for about 1 1/2". The 1/8" end mill comes in, feeding X-. Is that kind of what you're doing?

SLOW IT DOWN. Try 2000 RPM and 3 ipm feed with 3 or 4 passes, regardless of how you're holding it.

Stick a 4 flute high speed steel end mill in there at 2000 RPM and 3 ipm feed, if that don't work.

That'll take you all of 30 minutes before you abandon your setup. Please clarify how you're holding the bugger. :>

viper · Jul 15, 2008

Here is a pic of the part and the fixture. The jaws hold 4 part and the LH side, the part sticks out about .25, the RH side has 100% support. I have tried barely clamping and getting serious with the clamp, no change. On the right side, you can see my witness cuts in the tool from a .375 cutter. The .125 cutter does a full depth trim cut on the end of thepart to trim off a tit from the lathe as well as .010 of the end. NEVER broke one on that pass. It then goes over and starts the slot cutting entering from L or R. I am not plunging into the part. I enter L of the part and only cut radially.

I just cut two more with the 3FL cutter at 10.4ipm and 221 SF, right out of the book. There appears to be ZERO wear. I also have another 4FL varimill that has cut 3-5 parts and it shows zero wear too. I don;t get it.

I want to try these 6FL necked cutters because it will only have .25 of flutes so it should be rather ridged. I will try a few more cutters, then dump the idea and move to a saw. I really like the idea of inserts in a saw so I can swap teeth but I bet those part PRICEY! Guess I just want an answer at this point of why the cutter is breaking. I know some more experienced people are wanting to reach through my monitor and slap me for still trying, knowing a saw can do this.

huskermcdoogle · Jul 15, 2008

Did you try running without coolant? Running an air blow.

Husker

rklopp · Jul 15, 2008

apestate, Viper had a picture of his setup in his previous thread about this issue http://www.practicalmachinist.com/vb/showthread.php?t=158337. He is holding them laying down in soft jaws in a vise.

Oops on edit, viper beat me to it.

I have one of those insert-tooth saws. Its from Iscar and uses their parting inserts. Though there doesn't seem to be much holding the inserts, it works good on cast bronze and on wrought aluminum. I've never tried it on 17-4! I'd hate to wreck the cutter body finding out it won't work. You go first

!!

RKlopp

apestate · Jul 15, 2008

You realize an indexable saw cutter is gonna cost you like $400 plus two dozen inserts at least... plus a suitable arbor tool holder plus a totally new setup.

I mean, a HSS convex radius mill cutter would be the ideal way to do the job, yes. MSC has got them on page 488 of 2007/2008 catalog, but they're only 2-1/4" in diameter with a 1" arbor hole. Won't reach.

You really should try slowing it down. 6000 and 7000 rpm has a way of exaggerating little problems. I would try 2000 RPM and a 3 i.p.m. feed with your carbide end mill. If that sucks, I would try the same speed and feed with a high speed steel 4 flute.

Try tapping the ER collet true when you're tightening it up. I've done this with reamers that ran out .005 and got them under .0005". Of course, I had all that shank of HSS to bat on. You might stick a bar on the face of the collet and tap it up to try to get it to shift.

HELP!! slotting in 17-4PH again. this is getting costly

Titanium

Titanium

Titanium

Diamond

Stainless

Titanium

Diamond

Titanium

Stainless

Cast Iron

Titanium

Titanium

Titanium

Titanium

Diamond

Stainless

Titanium

Stainless

Diamond

Stainless

Similar threads