any advice on machining these parts?

[cherokeechief79]

i have to machine some big turnbuckle eyehooks similar to these but not nearly as big.the blocks are 5 in tall by 8 in wide by about 14 in long heat treated 4140 or 4130.they are about 30 or so rockwell range.ive never done anything like this before on this large scale.i can do this anyway i want but there are only 4 of them(2left-2 rights).i have a haas tl3 (toolroom lathe)with a big 4 jaw chuck and a tailstock.i also have several haas and hurco cnc verticals to use.they have never done these type of parts here before and i was told the way to prolly do it is to chuck it up in the lathe and turn the 3.5 in 12 threaded end 1st.then hold it in a celf centering chuck on the thread (with an alum sleeve)to do all of the milling.

im thinking of maybe trying to get a solidmodel of it and surfacemachining one side then flipping it and surfacing the other side leaving .100 all over.then finish the milling end and lastly holding on the milled end in a 4 jaw and turning the threaded end.

does this sound logical?

any advice is greatly appreciated.

i have mc 9.1.

thanks

mark

 

 

[horsepowered]

I would do the whole part on a mill with the threaded end being the last operation. I would cut the threads with a thread mill.

[cherokeechief79]

there are some high finishes required on the thread and the undercut area after the treads.also they are "j" threads with a controlled radius at the thread root.i dont have confidence in myself holding the tolerances required here holding these upright in a haas mill(maybe its easily obtainable but ive never done it)

these parts are going to go through a very strict inspection.

[cherokeechief79]

ok so i googled "machining a large turbuckle"and came up with this.

why does these things only happen to me?

 

may not be work safe

 

web page

[TheePres]

Cherokee,

My 1st job was at place that made this type of part for the nuclear industry. With some quite a bit larger than picture shown.

The thread end was cut 1st on large behemoth lathes. Then we would screw the part unto base with matching threads (with monster size wrench) and face both sides and bore hole on horizontal mill. The direction of cuts was important so as to not un-screw part from base.

[cherokeechief79]

ok so these parts finally came back from heat treat again.i tried roughing them somewhat to shape(just square from a solid i made in mc)1st i tried a 4 flute insertmill.worked ok for a while but didnt like coming out or going back into the cut and it faile after a bit.then i tried a 1 in carbide rougher which worked but took forever and i used 3 of them for 1 part.if this were aluminum i would know exactly how to tackle this but being 35 rockwell in 4340 is leaving me stumped.we had a meeting about the job today(im the new guy here)and i was just going with the flow of how everyone else thought they would tackle it even though i thought that is was not the way to do it.i made a complete solid model of the part in mastercam and it looks great but i could not bring myself to say let me surface machine it from the solid because of how hard it was on the machine and tooling just roughing one pc.i am now roughing most of the material off on an old cincinati manual mill with a 6 inch facemill and leaving the threaded end square for now.

am i wrong for not speaking up?

im not familiar with machining hard steel like this.

in my heart im thinking just rough this with small cuts driving off of the solidmodel but all i can think about is tool failure and being the only one who wanted to do it this way.we have several 3/4 and 1/2 inch multi insert cutters but im not sure how they would do in this material.

any advice is greatly appreciated.

[greg@kohler]

Cherokee,

 

Have you looked for the recommeneded chip load and SFM for the grade of inserts you have. I have cut many hardened parts this way and have had great luck with it.

 

 

good luck

Greg

[Chris Rizzo]

first off in my experience for that material, it's all about working with the manufactures recommended feeds and speeds, d.o.c. and radial engagement.

 

IMHO, also sounds like the "biggest cutter / biggest hp" method might be stuck in peoples heads, and you've got some new thinking going on with the fast light cut trend in machining. I'd say do your research and go for it. Seems it can't get much worse anyway! First off however get with cutter rep on cutting conditions and strategies to give you the best chance at success.

m2c

 

oh, do a search on the forum for highfeed cutters. some great info there.

[88Matt]

I have to agree with TheePres & Chris,

 

Go with the manufacturers specs and run it. With the quantity you have don't spend much time on optimizing it. Turn the thread and mill the rest. I would make a lock nut for it though.

[LansB]

Yep...go with the recommended grades, feeds, and speeds. When in doubt, give your tool supplier a call and see if they can get a rep in to advise on tools/toolpaths. Our Sandvik guy is awesome at helping out with this type of stuff.

 

As far as machining process goes I agree with TheePres. I would run these parts out of round stock if at all possible (if not use a four-jaw chuck). I would turn the threads on a lathe first. Next, I would screw the part into a mandrel on a 4-axis VMC or an HMC and mill the flats/hole and outside contour.

 

Even without an HMC or 4-axis VMC I would probably run them the same but manually rotate the part 180 degs for the second flat side and just indicate it in if four parts is all you have to do.

 

Hope this helps.

[Kyle Waters]

I agree with Chris. If you can get your hands on a high feed cutter, at the correct parameters, it sounds like you could open alot of eyes over there. And since they have such a high positive rake, you can save a little on the horsepower required to get it done.

 

HRC30 isn't crazy for 4340, well within indexable range, but it is definitely in your best interest to call your rep, and as I hear it, they will be glad to hear potential work is looking for them!

 

HTH

[TheePres]

This Cutter will cut 4340 like butter: Iscar HeliDo Upfeed.

.06 depth of cut with .05/.06 chip load/per tooth on a 40 taper machine requires very little horsepower.

[MotorCityMinion]

That Iscar is similar to the Mits AJX cutters. We've been using them on a 40 taper, 15hp HAAS, and it's like running a different machine. Watching it run the first time, you can't help but be impressed. Excellent insert life as well.

[cherokeechief79]

thanks for all of the advice.im going to pick out a few cutters so we have them on hand but it will have to be on another upcoming job.

do you have any more info on this cutter?"Mits AJX cutters" is this mitsibishi?

im off of the milling end of this job for now and im setting up a 4jaw in the lathe for the threaded end.

[MotorCityMinion]

Yes indeed, it's Mitsubishi. The local rep practically twisted our arms to take advantage of a free trial, and 20 free inserts. We got a 1" tool, peeled back the shank a bit and have over 3.' of reach now. 2 inserts at 1400rpm and 90. ipm. Doc between .03 to .05. I've channeled with this tool for hours on end in P20 without indexing, sticking way out of the holder, on a 15hp Haas. It's probably not the fastest feedmill out there, but it's a very versatile tool. Worth every penny.