.035 Hex broach in Titanium on a Citizen C16

Hi ,I am trying to do a .035 hex broach in grade 4 Titanium. Im doing this in Citizen c 16 from the center tool post. Ive tried using a rotary holder wich didnt work at all as the broaches are so small that they just snap after a few pieces.Right now I am trying a peck broaching method but am only getting about 50 pieces before the broach bends instead of breaking. I only have to go .045 deep,Im drilling the hole to .037 dia by .075 deep with an undercut.Any suggestions on making the broach last longer? It is a full form broach made out of m42 cobalt held in a collet.

Is this a rotary broach? One that wobbles?

I tried the wobble broach method but it is to small to put enough pressure on it to spin the holder.

I did .050" in that material and I found that "Powdered metal" broaches lasted longest. I got them from Hassey Savage. What helped the most was having a hole through the center to let the air escape.

Pit,

Put your drill in the adjacent staion to the broach. Then drill the hole to depth, then broach around .003-.005" deep, re-drill so the body diameter of the drill goes .005" deeper than the broach, then broach again .003-.005" deep, then redrill, etc. Broach without coolant. As coolant doesn't compress very well, and it takes up room which would be otherwise occupied by the chip.

While this is a PITA, I've found it will give you much better broach life. The pressure really increases dramatically on the broach the deeper it has to go. By clearing the chip out with the drill every three to five thou, it takes the pressure off.

If you think about how the chip is formed, it comes into the center of the broach from all sides, so the chip mashes into itself, then gets forced down the hole ahead of the broach. So with such a small tool it doesn't take much to chip the cutting edge.

Also I've found that Blaser Vascomill cutting oil (vegetable based) helps out quite a bit with finish and tool life when machining small Ti parts.

If it's a full form broach, it needs to have a vent hole through it too. You can buy a broach like that from Rayco Tool in Warsaw, IN.

http://www.raycotools.com/

You also need to be lined up perfectly which will be difficult given that you can only adjust your location in "X" and there is no provision for adjusting "Y". But I wouldn't even bother getting started if the broach isn't within .0001" TIR to the main spindle.

Good luck.

Wow, thanks for the help guys!Swiss, Im already using the Vascomill and it is FANTASTIC. I will try your suggestions as soon as I get some more broaches in. I have the option of of broaching in a gdf holder on the gang .So then I can adjust in Y.I am having a couple made with two sides ground off to vent it nad then I will index 60deg and broach again. I will also try your method as well. Thanks again.

Pit,

If you've still got a dull one kicking around just grind the face flat to resharpen.

I ran some Maxilofacicial (sp?) screws a while back that had a full form square broach in it around the same size you are doing. I sharpened them on an Accufinish grinder, holding them in a collet chuck in a V-block. I also polished the face using the polishing wheel and diamond spray after grinding them sharp.

With these parts the pilot hole had to be smaller than the broach. No witness marks allowed at all. Without pecking back and forth between the broach and drill, you couldn't make ten good parts in a row.

Anyway, the broach lasted 7+ hours at around 80+ parts per hour. Not bad at all.

Polishing the face of the broach made some difference too. Probably an extra hour or two of production time.

Hi All:
I've had good success relieving the sides of the broach 0.0002" or so, to make it non-parallel along its length (skinnier at the shank end of course)
I've had best success with home made carbide broaches, and I've found that dressing them with diamond paste on a brass lap to eliminate the transverse grind marks improves their longevity considerably (eliminates the stress risers I suppose).
It's a lot of work prepping the broaches this way, but I get better life from them than I've gotten from commercial HSS broaches.
Smallest I've broached this way is 0.048", 0.060" deep.
I don't know if carbide would survive at 0.035" across the flats...I've never tried.
Cheers

Marcus

Another clever way to wobble broach a very small broach or to wobble broach a form oriented to milling elsewhere on the part is to use the polygon turning function or hobbing function. Which is usually an option.

You also need an adsustable angle face drill unit as well. What you do is mount the broach in the face drill. I mean the actual broach (cutting tool) and not a wobble broach holder.

Set the angle of the face drill unit at 1-1/2 degrees. Which is what a wobble broach holder does, it holds the broach at a 1-1/2 degree angle reletive to the work spindle.

In the program synchronize the rotation of the live face drill unit to that of the main spindle by programming a 1 to 1 ratio using either the polygon function or the hobbing function.

Since the broach is now driven there is no torsional load on the small tool.

The main problem is most shops don't have the attachment and control option required to pull this off. But if you need to do a lot of small diameter broaching or oriented broaching, this is probably worth the investment.

Other advantages are that there is no twist on deep holes. You can also broach part way, re-drill to clear chips then go right back into the hole with the broach. Since the broach is driven and oriented electronically there is no worry about misalignment.

On a Fanuc you can also program an angular relationship from the polygon spindle to the main spindle. If you have to say broach an internal square and put a cross hole through the flat, then you can use the angular call out to adjust the angle of the broach electronically.

WOW!! You guys are good!!!Swiis I take it that you have some experience with these things. I do have an adjustable face drilling holder and both polygon and hobbing function. I will try your method as soon as I get some new broaches in .That sounds like it should work Pissah as we say here in New England!Thanks for the help I will let you know how I make out!!!! Thanks again.

Pit,

It will work wicked pissah. I'm a refugee from N.E. myself, it's where all the good Swiss guys are from isn't it?

Anyway, don't tell any of the boneheaded apps guys from Brookdale or CMA or whatever how to do this, OK? I'm tired of teaching Citizen how to compete with us.

Anyway, sorry I didn't mention this method sooner, I just ASSumed you wouldn't have all of the goodies to make it work. My bad.

Don't forget to peck and re-drill though, it will make a huge difference in tool life.

I agree with swisspro, pecking method should not be forgotten with rotary broaching, it has helped many of our customers out of a jam. The next best thing is if you can open up your pre-drill, even a small amount can GREATLY reduce the pressure. www.rotarybroaching.com

Broaching Tougher Materials

We manufacture a broach that has the rake angle/dish only in the center of the rotary broach, not out to the edges, that way the cutting edge is more robust and rigid. We also recommend a small corner radius and slightly stoning the sides of the broach at a 45 degree angle. Our broaches also come with a pressure relief vent hole to relief pressure build up You can learn more here:www.polygonsolutions.com