How do you use a Brown & Sharpe box tool holder?

apestate · Dec 5, 2007

hi guys

I'm trying to find a way to finish a long part made out of titanium. It's .250 +0/-.005 for 9.81" and there is a .175 gun drill bore through most of the material.

I found a Brown & Sharpe roller support box tool holder and I'm going to set it up for some test cuts tomorrow morning. Is there anything special about setting up one of these tools?

For my first test cut, I placed a pin in the collet of the lathe and brought the tool over the pin, then I brought up the rollers until they spin. I'm going to set the box tool on the pin then give it a go on the part.

What depth of cut would you recommend for this tool?

dfw5914 · Dec 5, 2007

Probably ought to tell 'em what the initial stock diameter will be.

willbird · Dec 5, 2007

It has been 20 years since I used one...but the old fella that showed me told me to set it up without the rollers touching the part at all, and adjust the tool until the turned dia was .005" oversize, then adjust the roller 90 degrees from the tool to touch, then adjust the roller opposite the tool until the part dia was correct.

Procedures on a more modern machine may be different.

Bill

apestate · Dec 5, 2007

dfw, we're roughing the stock down so I can do basically whatever depth of cut I want.

Because of the way its getting roughed, there's going to be possibly up to .010" of runout. All I'm doing is inserting the tailstock, turning a little clean pass at the diameter I want, then I'm going to feed on the box tool with the box tool leading the rollers.

dfw5914 · Dec 5, 2007

I will now respectfully bow and back out of the room, apologizing for having posted in this thread at all...

jims · Dec 5, 2007

box tool

Like dfw said it would help to know dia stock you are turning .
If it is .5 to .75 dia then I would try to take in one pass with rollers ahead of cutter on od.
Box tools are good at taking heavy cuts but not at leaving good finishes. Also how the tool
is ground makes a big difference. And with rollers on od of stock cut should run true to od.
I would plan on leaving .01 to .015 stock for centerless grinding if finish is important. And you need flood coolent .
I am posting pic of production ss part done on a Logan. One pass then centerless ground
for size and finish.
Jim

ARFF79 · Dec 5, 2007

apestate:
You do not say what kind of machine that you are going to run this part on, or how many parts there are. That can make a slight diference. Since a box tool is designed for use in a turret lathe or a screw machine turret, tool travel must be considered. Based on your part description, you should be using an OO sized tool (5/8th" shank). All of my roller box tools have a through hole to allow the part to pass through if it is small enough in diameter. The problem in in the slide stroke, as most of the smaller sixed production lathes is only about 4-6 inches. This means that you would have to disengage the turret index mechanism,feed the part out to a stop, turn and retract the tool turret then feed the part out the rest of the way to enable you to turn the rest of the part. The tricky part is how to get the finished part out of the machine as it will now be in the tool body. Your better bet if you intend to use this tool would be to place it in a collet holder on a QC tool post on an engine lathe, center it up and after a trial cut, lock everything down. The only other way would be to use a roller equipt follow rest on your engine lathe. The plus with that would be tha ability to retract the tool bit from the work and avoid the scroll marks that occur with a box tool. hope this helps .

rockfish · Dec 5, 2007

Here's what I learned reading a Warner & Swasey publication:

1. Get the cutter on center.
2. Make sure you have a chamfer turned slightly below the desired diameter, because
barturners need to start on a chamfer.
3. Turn a test diameter approx. 3/4" long and .001 smaller than the desired size, as close
to the chuck or collet as possible.
4. Using a .0015 feeler gage, set the cutter that distance away from the diameter you've
turned.
5. Set the rollers slightly behind the cutter.
6. Set the rollers so that they touch the diameter you've turned, and so that the rollers
will slip under moderate thumb pressure.

Of course you need to be able to grind the cutter, which is too involved to learn here. I have a barturner cutter gage and I still find it extremely difficult to follow the geometry.

apestate · Dec 5, 2007

I have 4 box tool holders. Two triple aughts, and two big suckers with 1" shanks. One of the 1" shank tools has been completely disassembled, cleaned, and oiled. The 000 ones could be combined to make one good tool, as well.

Material OD is 1", and that's why I didn't mention it. I'm using a Romi/Bridgeport EZ Path lathe with QC tool post. My first plan is to rough down the material in sections until I get 9.81" at about .275, then run a finish pass with the box tool. Finish diameter is .250 +0/-.005 with 32 microfinish. I'm machining up to a shoulder that needs a .032 radius fillet.

This material is coming back from gun drill with a .175 bore throughout most of the length. Runout of the bores to the .250 OD is controlled by a block tolerance of .005 runout, that's what I'm most curious about...

Let's say I have the box tool holder all set up to turn at .250... Chuck part with roughed out diameter at .275.. insert tailstock and turn a clean diameter manually at .250 at the tailstock end... then run the box tool holder with the cutter leading the rollers, rollers on the finished diameter. Does anybody think the material will track well enough to maintain concentricity to the bore?

gbent · Dec 5, 2007

Runout to the gundrill hole will be a bear. You may have to set-up off the gundrill hole and center the far end to agree with the gundrill.

Also, make sure the driller is turning the part and not the drill. The skill of the driller will be critical in making this part. There is more magic in gun drilling than almost any other machine shop task.

willbird · Dec 5, 2007

We never EVER ram the rollers on the bar, only on the finished part. In fact the old fella found one set up to run on the bar from a guy's setup that got fired and he ranted for DAYS about it :-).

When I worked in Toledo we had a couple swiss turns, making long skinny parts they had to turn an OD in one pass due to the fact that swiss turn holds the bar in a collet...the bar moves in and out in Z and most tools stand still, if you turn a long od you no longer have support of the stock in the collet.

For this reason and the fact that the parts were made of TI and some nasty stainless (medical implants) the guy that ran and programmed those machines would often try EVERY insert he could find in the size he used, maybe one typically NOT made for the material he was machining WOULD work out to finish a dia like that in ONE pass.

MY experience with long skinny parts is limited, but the experience I DO have leads me to think your best luck for concentricity will be with what you can machine in one pass while the part ahead of the tool is still rigid.

I have seen some very pretty finishes in 12L14 with a box tool, but that is one of the few materials I have used them on.......20 years ago :-).

Bill

beege · Dec 5, 2007

I have a part I make in 303 Stainless. About 4" long, from .312 stock diameter to .182 finished diameter, on a CHNC II+ Hardinge. Here's what I do:

Turn a portion of the diameter (.182) close to the chuck, .100 long.
Feed the stock out to full length
Box turn, with the rollers hitting the .182 diameter before the cutter engages
Feed in at .003 ipr, back of at 3X that, or .009 ipr

Finish is nice, can hold diameter ±.0002 all day long
Adjustment on the tool is 1:1, so if I adjust the diameter of the cutter, I put an indicator on the edge and tweak until perfect.

Setting up the rollers, I turn a piece of anything to finish size, and set the rollers to just touch the diameter and lock then down. Then move the cutter to touch the diameter, and back off a little for one more adjustment after the first cut.

apestate · Dec 5, 2007

Thank you all for your help, it's much appreciated.

I'm playing with the tool now, taking some test cuts. I set the cutter up on a .335 gage pin. Then I chucked a part with 9.81" roughed down to .350. I inserted the tailstock in the drilled hole and turned about .4" back to .335. Remove tailstock, insert part into box tool holder, and then fed .0005" at 250 rpm.

So far, it's actually functioning. Finish isn't awful but it looks kind of squirrely. The chip is evacuating nicely and not tracking over the rollers too bad.

I'm going to experiment with feeds and speeds and hopefully this noodle won't whip out of the holder or something :>

What would you guys try for speed feed and depth of cut for the finish pass?

I also noticed that the tool holder doesn't allow me to place the box tool on center. I even tried to fix the tool holder to get it down there but it's still about .02 below center. Is this part of the design?

jim rozen · Dec 5, 2007

There should be a rocker mechanism, with two setscrews to allow you do that.

Maybe a photo of your box tool?

I like the 'turn the part five over, set the top roller on the part, and adjust the
rear roller for size' approach.

Jim

apestate · Dec 5, 2007

So how do you keep the chips off the rollers?

I finally got the cutter on center and made a pass at .005 depth of cut and .0005 feed, which creates a chip in the titanium that can be blasted away with coolant. However, it's still gouging up the part like mad.

I'm happy, though. We had two guys setting up for the job and the other guy came through. I got the tool to work, kind of.

jims · Dec 5, 2007

box tool

Went to my turret lathe operators manual about bar turner cutters aka box tools.

One pic shows how tool can be below center for small dia parts. One pic shows
rollers ahead of cutter. I used to use box tools all the time and was the set up man
for years. I ground all the box tool cutters by hand . It is easy to grind the .032 radius
on the tool. Taking a small .oo5 cut will allow the chip to go where it wants and that is usually under the rollers where it will imprint on the turn. If you have a heavy machine and flood coolent I would try to take that cut in one pass still with the rollers on the od of stock
leaving grind stock as I don't think you will ever get a 32 finish with a box tool. If you look closely at pic of cutter it is below c/l of machine but still on c/l of part due to the way it is ground. Third pic shows rollers on od of mat and that leaves lots of room for chips to clear.
Jim

beege · Dec 5, 2007

APESTATE<

I suggest you call Hardinge (or even Boyar-Shulz) to get their recommended feedrates. I think .0005 IPR is way too light for your app. Chips will be microscopic, and get in the way more than larger ones. Those people are very willing to give you tips.

Search

Largest Manufacturing Technology Community on the Web

Search

How do you use a Brown & Sharpe box tool holder?

apestate

Stainless

dfw5914

Stainless

willbird

Banned

apestate

Stainless

dfw5914

Stainless

jims

Hot Rolled

ARFF79

Hot Rolled

rockfish

Titanium

apestate

Stainless

gbent

Diamond

willbird

Banned

beege

Stainless

apestate

Stainless

jim rozen

Diamond

apestate

Stainless

jims

Hot Rolled

beege

Stainless

Similar threads