Question 6 inch diameter and five feet long. Lathe turnin=g Job. End to end close tolerance (.001) How do you align this thing correctly so it ends up being a even diameter down its entire length>>??
Aligning LONG SHAFT IN LATHE
Collapse
X
-
You probably can't set-up a shaft like that on a lathe and reasonably expect it to cut a cylinder (as is geometric solid) within 0.001" tolerance without a lot of fuss and bother. You can get both ends to cut the same diameter by offsetting the tailstock but the part in between is another matter. For one thing a 6" dia shaft 5 ft long is skinny, it will deflect significantly under tool cutting force. For another, there 's over three miles of tool rub at 0.008" feed and that means significant tool wear. For yet another, the material will distort to a certain degree from the unequal relief of internal stress, thermal expansion from tool friction and unequal coolant application, tool wear, tool breakdown, and about a dozen other subtle factors.
0.001" over 5 feet is a tight tolerance on a lathe. That implies diameter, rainbow, cylindricity, and other errors form a budget the sum of which lies within a geometric cylinder whose tolerance band is 0.001" from perfection. I suggest starting with stress relieved stock, take a rough cut on it leaving about 1/8" stock, stress relieve it again, and after turning it to leave 0.025" grind stock, you cylindrical grind the shaft on a real cylindrical grinder to size (NOT a tool post grinder) between centers.
That said, you can cautiously work the diameter down on the lathe leaving a small amount of polishing stock and selectively finish it to diameter tolerance working a stretch at a time. This does not mean that you will get a round straight shaft within your 0.001" tolerance band, only that the measured diameter is within tol.
If I had the job and there were a number of pieces to amortize the extra effort, I'd make a follow bushing and take finish cuts with an upside down broad nose tool running the machine in reverse. With the right material, coolant, and tool grind, a 1/4" feed per rev peeled finish can be almost as smooth and accurate as a cylindrically ground finish.
This is a good place for a follow rest but it must be remembered that any roundness errors the follow rest encounters will be influence the work geometry for a distance until some other influence gradually intervenes.
If you don't use a follow rest you will need a steady rest to control harmonic chatter. Do not locate the steady close to the exact center of the work because it may promote second harmonic chatter. 60/40 seems to work well. Again, a steady rest can solve one problem but cause another.
Making long atraight stuff on an engine lathe aint a walk in the park. I used to make long skinny feed pump shafts out of 400 series stainless each with a dozen diameters and a half dozen lock nut threads. It was hard enough to make them run within 0.005" of straight then they went over to the mills for a half dozen keyseats and lock nut tab slots. It took a good deal of fancy presswork and scienfific peening to make them run within 0.001" on all fitted diameters referencing from their babbit bearing diameters.
I suggest starting from a cut piece of 6" dia T&P stock and, using the factory diameter for a reference, cut all subsequent features from it. The large cost of this material may well offset the cost of all that careful lathe work.
Another alternative is to concern yourself with the accuracy only of those parts of the diameter that have to be accurate and relieve slightly the parts that don't. That presumes you have a choice.Last edited by Forrest Addy; 03-02-2007, 09:39 AM.
-
-
Madman: Carefully!!
Set it up the same way you would a 1" diameter 10" long. You just need a bigger lathe and a crane to load it.
First question is this nice clean ground shaft material or somthing with mill scale and rust?
Drill centers on center use a large enough center drill to support the piece.
The most likely cause of taper here is a center on the part off center or the tail stock off center. If the part is smooth set up the shaft in the lathe. Put a test indicator in the tool post. run down the side of the shaft. this will tell you if it is set up paralel to the lathe center axis. then run it along the top. Also check both ends for runout.
If the piece has mill scale set it uf the beast you can take light cleanup cuts and then measure with mics to check for taper.
Let me rephrase that: What he said:Seriously though Forest has the greater experience here. If I had seen this before I posted I probly whould not have responded.
TinLast edited by Tin Falcon; 03-02-2007, 11:04 AM.Ad maiorem dei gloriam - Ad vitam paramus
Comment
-
-
At Northrup-Grumman, in the division that I worked in, we routinely had to do shaft work/ long parts without tailstocks. Lots of secondary operations, gear shaft blanks, replacement parts, roughed-out parts returned by heat treatment dept., etc.
We miked a suitable surface to ride in the steady. If the surface selected wasn't accurate enough, we ran that end in a four-jaw chuck and supported the free end as best suited for that part, and proceeded to cut a surface for the steady. We turned the part around, and then put the appropriate surface on the steady. We then indicated the chuck end.
We ran "upside-down," backward, etc. so cutting forces would pull the part down on the bottom rollers/pads of the steady.
We put a mag base and indicator on the part at the chuck-end. The mag base was on the part while the indicator plunger was against/ on the face of the chuck. We ran the indicator at the chuck end continuously. The indicator at the chuck end was dialed in by working the two bottom steady pads until we got 3 o' clock/ 9 o' clock, and 12 o' clock/ 6 o' clock readings of .001 or less. This was SOP in the lathe areas throughout the division.
Comment
-
-
Forrest and Mccin... have good advise.
When checking your spot for the steady, a micrometer may not pick up an out of round condition.
Tri-lobing caused by use of a three jaw chuck is a common cause of this.
Tri-lobing can occur in thin wall as well, as solid stock. Four jaw is best here.
An out of round center hole, drilled from a rough diameter will also produce this result.
When you machine your center hole, you have to run the steady on a ROUND dia, or the result is an out of round center hole.
This will transfer to the shaft od.
You need to machine your steady spot at the headstock, and reset the shaft.
This may meed to be repeated a couple of times to eliminate errors.
The center hole needs to be bored with a weany boring bar from the compound set on 30 degrees from the lathe axis.
A center drill will not produce a round hole by it's self.
You take shortcuts here, and will not likely succeed.
You are between a rock and a hard place.
Large tool radius will chatter, small radius will break down.
Setting steady mid cut will result in a miss match,
and may push the shaft off center causing taper on the end of the job.
Using a steady is a skill learned with experience.
We used to set a steady with the bottom rollers.
Set the front roller and push the shaft back say .002". Then, push it back to center with the rear roller. Just touch with the top roller.
Make a cardboard shield to keep chips out of the steady rest. A chip will make a real mess of your job FAST.
Take a couple of trial cuts with uniform tool conditions. Use flood coolant
and change insert, or uniformly regrind tool, between cuts.
Good luck,
Kap
Comment
-
-
Thank you, gentlemen, for your very helpful replies. Although I'm not the one who posted the question, I have a similar hobby machining job coming up, but it is much shorter.
One of the things I've been thinking of trying is an external lap. I can see why it wouldn't work to eliminate rainbow, but in my case that isn't so important. Would anyone care to comment on using an external lap to true up a 2" X 8" cylinder?
TIA
OrrinSo many projects. So little time.
Comment
-
Comment