Help milling broken tap

We have a 3/4" spiral flute tap broke off in a large, heavy, expensive part. Local EDM shop doesn't have height to reach, tapered shaft w/ball on the end and weight conspire against laying it down and doing it sideways. He suggested milling/drilling w/carbide. I have vertical room in VMC- - looking for recommendations on cutters, feeds and speeds. We'll need to start by milling, as end is rough enough that we'll never get a drill started.

TIA!

Ray

A ball carbide burr works pretty good to get started.

When it packs and starts smokeing and glowing red is when it really cuts good do it dry.

Sandvik makes "Hard Cut Drills" and they are designed for just this application....Drilling out broken taps.
Cutting area is square with a blunt pointed end, the shank is standard round so gripping in a collet is simple.
Run them at high speed (about 3000 rpm or so and feed constantly .
Have used these and they work pretty well.
Cheers Ross

i generally use carbide end mill, preferably a regrind. run high rpm's light feed about .5 ipm and a lot of pecks. although never broke on that big
good luck
dave

Crazy idea, but an edm shop might be able to jury rig up a system out side the edm. A tote on a cart, a wire to the part.
Milling might be easier and cheaper, just a thought...

Start with a carbide Ball end mill, then a Carbide spade drill just smaller than the minor D of the broken tap. You do not want to use too large a D bit, the broken teeth of the tap will jam, and guess the results. Keep pecking, and use a punch to break off the teeth as you go deeper, blow out often. Slow work gets the job done quick.

Centre cutting carbide end mill did the deed for me. Don't recall if it were 3 or 5 flute or the make except that it began with N. Shifted five 2.5 mm taps using a Bridgeport so running well under book speed. Light cuts, plenty of careful pecks and attention to swarf removal let the cutter survive intact until the last one was all but done. Lost the end of one flute but the remains were up to finishing the last half mill or so.

As its a reasonably large spiral flute tap you might do better milling out only the core and breaking out the spiral flute a bit at a time. Chopping into the flute proper by milling as close as you can top tapping size is likely to be hard on the sharp cutting edge but you also don't want a sizeable lump of flute breaking away to catch up in the cutter.

Clive

Helical bore using a 3/8 or 1/2 carbide EM, AlTiN coated, about 150 SFM, feed at 0.001" per tooth, spiral down 0.01" per rotation. Worst case you lose the endmill and start over.

Dremel tool with lots of smaller grinding stones. Takes a lot of time by hand, but almost no further danger to part if you're careful.

I've done this many times, though never with one quite so big. I think most folks thread mill 3/4" threads these days.

I've never had this not work. You clean it out with a carbide endmill fed down in a spiral tool path. Plunging isn't ideal, but a helical cut, with .005 per rev, is pretty fail safe. Replace the cutter if it starts sounding bad. I'd use a 1/2" endmill on a 3/4" tap. Try and stay inside the minor diameter...

rltco said:

We have a 3/4" spiral flute tap broke off in a large, heavy, expensive part. Local EDM shop doesn't have height to reach, tapered shaft w/ball on the end and weight conspire against laying it down and doing it sideways. He suggested milling/drilling w/carbide. I have vertical room in VMC- - looking for recommendations on cutters, feeds and speeds. We'll need to start by milling, as end is rough enough that we'll never get a drill started.
Ray

Click to expand...

This used to be my job at a shop where they figured out I had worked in a repair atmosphere for a while. You have a lot more wiggle room than I ever did, so here goes how I would approach it.
First, make sure you setup is dead set rigid. A little wiggle will snap the cutting tool like glass.
Start of with a carbide ball mill if you have one. If not, the a center cutting 4 flute will work to get a cut started. Use enough speed or you'll see a built up edge on your cutting tool break off and imbed carbide in your cut. Drill enough to see shavings(dust really) form. Come up, blow it out. Do it again. Those shavings have to be removed before they weld back to the parent metal, and the drill. So blow them out soon as you see them. Don't let them build up. Run it dry, most likely, as this will allow you to see how often to blow it out. You'll drill just a little, blow it out, and keep repeating. Till you get a good start.
Then, you start having options. I used to use a drill called a hi-roc drill. Carbide, no flutes. Ground sorta like a spade drill. LOAD IT IN A GOOD COLLET! NOT A DRILL CHUCK!!! Drill chuck can let that wiggle get you. Drill a bit, at that high speed, blow it out. Repeat. Use a moderate feed. I've done lots of them in a manual mill where I had some touch.
I like the idea of using a helical cut in this case. You have some room. Just stay near the minor diameter. Blow it out frequently, if not constantly. Helical cut would of course require a CNC.
Also, be careful when you get near the bottom, especially if it's broke off deep. If you get all the way through, the parts of the tap left in the hole will collapse on your tool. That sudden load will snap that carbide off in the part, leaving you worse off than you are now. Get almost to the bottom, use a punch to fracture whats left, and remove it with a magnet. Figure out why it broke, clean out the hole and threads with another tap(by hand) being careful of any tap fragments stuck in the threads. Bob's your uncle.
I've removed 1/2x13 spiral flute taps this way and had 3 perfect flutes in my hand with a good part on the bench. Main thing is be patient, don't let the chips build up, and use enough RPMs to prevent a built up edge on your cutting tool.

The thing to watch out for - when pieces of the tap come loose, especially at the end it will likely shatter your carbide endmill. Where I would start is about a 7/16 or 1/2 carbide center cut endmill. go in in the vmc in handwheel, cut a ways, back it up, blow it out. cut some more, see what you have. Don't get greedy don't feed it too fast. It sucks to have a carbide endmill stuck in the part along with the remains of the tap.

Radar987 said:

Helical bore using a 3/8 or 1/2 carbide EM, AlTiN coated, about 150 SFM, feed at 0.001" per tooth, spiral down 0.01" per rotation. Worst case you lose the endmill and start over.

Click to expand...

This has worked very well for me. Keep the dust blown out and cut it dry. 3/8" 4 flute end mill, bore to slightly under the minor diameter. The chunks that come out of the threads are the issue here, so keep it blown out with air.

I have a drawer I keep broken carbide end mills in just for task like this,I broke a 3/8-16 off in a finish part first thing Monday morning in the CNC lathe.
I reached into my drawer and got an old .250 carbide endmill that had snapped at the shank.Sharpened a chisel point on the end and stuck in a jacobs chuck in the machine and spun her up to about 1800 RPM,got about a half inch in and tap fragments shattered my carbide...no big deal,I have another,sharpened another and went the rest of the way...only took about 20 minutes or so..boss never knew a thing

a couple months ago i had a small AL. and stainless part that i broke a small 6/32 tap in and i tried the
McCormicks spice "Alum" method to disolve the tap.....it worked! Had a few micro specks,carbon?, form on the stainless and the AL. ,6061, discolored a bit but this trick is like majic.Alum. cost just a few dollars in the grocery store,i used one small ,2 oz?, jar to a small ceramic pan of water just big enough to submerge the part and brought it to a simmer.....6hrs later the tap was GONE.Dont use this on a ferrous part or use a ferrous pan,this stuff might make it disappear also.It will probably eat the points off the spiral flute pretty quick so you can just knock it out .You'll see pieces of the tap start to float around in the pan in no time........that'll be "1 millllion dollars" please. leave the pan to cool and the alum reverts back to crystals for reuse...Nice!

Another vote for helical bore with a carbide endmill at just under minor diameter.

I've also used straight flute Hi Roc carbide drills with varying success.