I have a 304 ss job. Its just about 7.1" long. The first 2.6" of OD is .472 +.0000 -.0004. Then it tappers down 1 degree for the remaining 4.1" with a full radius at the end of the taper. Also finish needs to be .032 or better. Any suggestions on turning this and keeping in the roundness, finish, and OD tolerance? Im using normal horizontal cnc lathe. Thanks in advance!!!
Do the 2.6" chucked up next to the spindle, then advance the material out all the way... Use the tailstock if possible... leaving some extra length to accommodate the center, which you'll face off when you're all done if the part can't have a center in the end.Originally Posted by Chais82
This part shouldn't be a problem at all.
You'll never, ever get a .032 finish. A 32, much more likely.
Thats a tricky one cause its balled on one end.
if your allowed to have a center in the ball end you have no problems, if your not your pretty much f'd
buts heres the way I would do it if you could have a center on the .472 end.
cut and finish everything with a tail stock. leave extra stock on ball end, (cut off side)
flip part around cut jaws to locate on BALL OD and have taper cut a close as possible.
then finish ball.
the Jaws cut like a ball will hold the ball so you can cut and finish the end of it.Obviously your going to have to cut your jaws to capture boh sides of the ball. cutting the jaws to the taper you have will help support the shaft from bouncing.
if you cant have centers make false centers and send out to o.d. grind then when it comes back cut off false centers. the ball side you will have to make special jaws.
Hope that made sence.
Delw
I was thinking it would have to be sent out to be ground too. Just was seeing if I could avoid that. I got .032 for finish because I converted ,8 finish to standard. I do realize it's a 32 finish. Thank you guys for taking the time to respond.
---
I am here: http://maps.google.com/maps?ll=42.001550,-71.540552
Please post your part print so I can review and offer suggestions.
http://www.kirkcon.com/
Here it is in two pics.
---
I am here: http://maps.google.com/maps?ll=42.001441,-71.540447
My recommendation (and how I would attempt to machine this part) would be to turn the 0.4720" diameter first with only 2.776" material sticking out. I would machine the 0.4720" diameter to a Z of 2.676". Then, in a 2nd operation set up, holding on 0.4720" diameter only 2.476" deep (this would leave 4.611" sticking out), I would turn the 0.1575" radius on the end at final part length and finish it. Then I would turn the 1 degree taper.
If for any reason I had difficulties with chatter or tool push off, I would regroup at this stage and build a 0.1575" radius concave nose piece to fit in my tail stock and use it to support the part for the roughing and finishing of the 1 degree taper.
http://www.kirkcon.com/
Looks like a prime part for a sliding headstock machine.
Otherwise, along the lines of txcncman's suggestion, turn the radius right at the spindle, advance the stock out for full-length machining, and support the radius'd end with a special cup on live tailstock, and the taper is easy. (your turning tool will need to be a 35deg profiler to clear the tailstock cup.... hint, hint)
Be careful and don't make the part out to be harder than it is.
(btw..... if you have the stock centerless ground, you won't have to worry about either the finish or the tolerance....just keeping the stock from getting beat up in the bar feeder or spindle.)
Last edited by fizzissist; 01-30-2012 at 01:45 AM.
To do it right with the least amount of run out and finish it needs to be ground, I'm pretty sure you can have a tiny center in both end, if not, make it longer and cut back.
You can cut the ball at last, making a tapered split sleeve and chuck close to jaws.
Use a sharp tool & cut cool !
Posting Permissions
LinkBack URL
About LinkBacks
