6" Deep boring w/ 8" 0.625 boring bar

[Donkey Hotey]

I have a bit of a problem and I could use a few opinions:

• Haas TL-1 Toolroom Lathe
• 0.625" diameter, carbide inserted boring bar, set up with flats. Clamped flat, the tip has a lot of negative rake.

The part is an aluminum intake nozzle for a Formula SAE car. It has to measure no more than 20mm at the tightest point. As a result, the students designed a converging/diverging cone nozzle. About 6" down inside, is the 20mm bore (0.787"). They actually gave me a bit of tolerance but, it's still tight.

The problem is that my boring bar is 8" long. I'm using 6" of it to get in to the orifice. I can't use a larger diameter bar because of the orifice size. It's so flexible that with all the negative rake, the aluminum is chattering like crazy. I'm not sure that positive rake would do much better (pulling into the part). The finish is terrible and I've already blown one part (orifice diameter). After buying another foot of 3" diameter stock, I'm going to give this another go on Friday.

I'm trying to get by without buying another boring tool. I'm making no money on this job (doing it as a favor to one of the teams). Does anybody have any tips? Neutral rake, positive rake, garden rake? I already hand dialed the spindle speed to keep it from getting out of hand but, that only kept the insert from hammering itself to death. I tried clamping a pair of Vise Grips to the bar during the feed to change the frequency. All that did was halve the frequency and double the amplitude (it wasn't pretty). I can't really sharpen the bit (insert).

My only remaining idea is to make a sleeve for the boring bar so I can rotate away from the flats and get more neutral rake out of it. Any other ideas?

[punchpressman]

Greg,
Small and long is never fun. Can you make a boring bar yourself and use HSS toolbit. Lite cuts with positive rake may stop the chatter. Is the stock length out side the chuck or split between the jaws. 3" sticking out of the chuck 3" in ? Try grinding an old insert if you have one.
Good Luck,
punchpressman

[Geof]

Wrap some soft solder, wire type like used for electronics, tightly around the boring bar and maybe overwrap with a layer of electrician's tape.

What you want to get is a situation where the extra mass you add onto the bar has a different resonant frequency so you get destructive interference between it and the bar.

Another possibility is try clamping your vise grips on but with a piece of hard rubber between the jaws and the bar; this makes a crude constrained layer damper. Clamping them on solid like you did simply increases the m ass of the vibrating system pushing frequency down and amplitude up as you discovered.

Also try a really sharp positive rake insert positioned slightly above center so that when the bar deflects the cut decreases in depth.


EDIT: Also turn on spindle speed variation; bet you didn't know your machine has that.

[Donkey Hotey]

Originally Posted by Geof Another possibility is try clamping your vise grips on but with a piece of hard rubber between the jaws and the bar; this makes a crude constrained layer damper.

Now that's a good idea. I hadn't considered making my own active damper. The only downside is that I was using all of the protruding bar. That meant I didn't have the luxury of setting up the rubber and vise grip and leaving it there.

Wrapping with solder wouldn't work either. The bar is going inside a 3/4" starter hole and it's burying itself within 0.25" of the holder. I even had to set my retract distance to zero to keep it from backing into the opposite wall on retract.

Last night I was digging through my drawer of holders to find out my boring sleeve diameter. I discovered that I have a 5C block for my toolpost that I completely forgot about.

So I could have rotated the boring bar to a neutral rake after all. I don't think a 5C collet is going to hold it as rigidly as screw clamping though.

I guess my only choice is to go with neutral rake, set it slightly above center line, leave myself enough material for a few 0.005" cleanup passes and hope for the best.

Originally Posted by Geof EDIT: Also turn on spindle speed variation; bet you didn't know your machine has that.

Actually, yes, I knew it had that and that's kind of what I was trying to do with the speed handle. I was too lazy to stop and go back to look for the setting and rerun it.

[sambo67]

the rubber dampener is the best idea.i'm sure you have slowed your rpm's to compensate for the extra long boring bar.you may be able to use a hose clamp to hold your rubber onyour boring bar

[metlcutr55]

i have had some luck at times using sharp tooling, and knocking speeds way way down, ie 100 rpm, multiple small depth cuts and a spring pass or 2, that being said it will take a long time.

[kwhizz]

The softer the material.....the higher the positive rake angle required....why would you use a negative tool for a material that requires high positive rake angle....you are just compounding your problems...........

Ken

[packrat]

I would go with a HSS bit in the bar,sharp point with just a hint of a radius stoned on it, and a chip breaker ground in its top surface. Breaking the chip help in keeping the load off of the bar.

Once the chattered finish is on the part you have to take real light cuts to get rid of it. Using soluble oil/water mix from a squirt bottle, not flood, is also a help. Or Tap Magic Aluminum, both evaporate with the heat from cutting and actually cool better than flood coolant.

On an expensive part and long/flimsy set up like this I like to set up the boring bar to do the part, but use a short scrap piece of the stock to see what it's going to cut like, before doing the actual part.

[DareBee]

I made a holder 14"L X 2.5sq CRS. Put in a hole for the stock boring bar (off center to the front). Turn the first bit of it round for some clearance (or mill the corners off). You will need to do a bit of machining to get it to fit in the toolholder.
If you need to get really fussy, make the holder out of H13, harden it and Jig grind or hone the Bar hole.
Designing and simulating the bar cutting the bore in CAD really gets it good without any need for tweaking with the hand grinder in the middle of a cycle.
This is for my aerospace "cones" (sounds similar type bore job).
Contrary to popular opinion, i get a better finish in these bores with negative rake. My machine is on the light side and has a turret TP instead of rotary. I believe the negative rake helps "push" any play off to the side instead the positive rake trying to suck it in and then it vibrate back and forth. A very rigid machine may not experience this. .0001" play in the system when it is 16" form the tip of the boring bar turns into a lot of potential movement as well as a massive amount of torque transferred back.

[Captdave]

Most OD tool holder use set screws to hold the tool in place, get rid of them. Use SHCS for better tightening and add a few more if space allows.

[PixMan]

Which sty;e of insert does the bar take? If I could know the insert nomenclature I could suggest the best insert for the application.

A 5/8" diameter boring bar will likely take a screw-down or top-clamp TPG type of insert. SO which style does your boring bar take?

[Donkey Hotey]

The part is long since done and delivered. As stated in the first post, this was a job to help out a university senior project. I made zero dollars on it, invested over 30 hours in the part and had no intention of buying anymore tooling to complete it.

Thanks to everybody for the input. As I had already decided, the bar was rotated to a neutral attack angle and fed 0.015" deep per side at 0.002" feed. It was far from perfect but, it did the job.