What's new
What's new

Runout (Roundness error) on a turned part

Jaanyaar

Plastic
Joined
Aug 19, 2016
Hi.
I'm a newbie at CNC lathe. This part is done on a 3 axis turning machine with live tool. Unfortunately it has 0.16 mm runout.
20240213_191735.jpg

OD = 134 mm
ID = 114
L = 21
Material = Steel 316

What is the correct process to achieve minimum error. (Runout = 0.02 mm). Appreciated for every little point for a novice like me.
 
Hi.
I'm a newbie at CNC lathe. This part is done on a 3 axis turning machine with live tool. Unfortunately it has 0.16 mm runout.
View attachment 428402

OD = 134 mm
ID = 114
L = 21
Material = Steel 316

What is the correct process to achieve minimum error. (Runout = 0.02 mm). Appreciated for every little point for a novice like me.
Sounds like a chuck pressure issue or part destressing. How much material are you removing and how much check pressure are you using?
 
Sounds like a chuck pressure issue or part destressing. How much material are you removing and how much check pressure are you using?
Around 100 psi.

Raw material is about =
OD = 143
ID = 102
L = 200 (several parts are achieved)

G71 is used for roughing with these parameters:
U = 2mm (depth of cut)

Is it necessary to have raw material balanced? Any side effect?
Is drilling/tapping any minus effect?
 
Sounds like you are parting it off. You can play around with the feed and DOC but I feel the results will be inconsistent as you move down the stock. You might try to rough it and partially part it off before finishing to let it relieve itself. How much to leave on part off will be trial and error as not to affect your finish pass as far as chatter goes. .02mm runout on that large of a diameter is pretty tight on a part off job in stainless.
 
Buy quality material that has lower stress in it to start with. I've had ok luck usually with USA/Italy material. I normally use solid bar and drill all the way through which releases some stress.
Rough, part most of the way through, mill/drill/tap, finish turn(or finish turn first if you get insert breakage issues from interrupted cut) then finish parting off, face/finish back side. Then see how far it went out of round, if not in spec find the high spot and press back into roundness.
 
It sounds like the parts "springing" from the stress relief of the material as its being machined and still attached to the parent bar it has structure behind it. The moment you part it off the part looses that structural backing and pop, out of round. Had this happen a few times. Always able to fix it.
 
For sure part most of the way through before finishing.

A good bit of out-of-round is likely telegraphing through from chuck crush. This crush can be measured with a bore gauge. Measure a spot free, then the same spot chucked. Try it in several positions.

You can reduce crush by using a three point adjustable spider. If you've got lots of these to make, build two spiders and install the second one while the first spider is in cycle. Rig an idicator to measure distortion when installing the spider and increasing this preload distortion until you achieve best roundness.

Alternately make a plug as thick as you are chucking. Relieve the od 3X so it only hits opposite the chuck jaws. Tap this into the id and chuck on it. If you don't relieve it you'll probably add distortion because the tube ID isn't round.
 
My preference would be to pull to achieve consistency. Move down in Z is never the best idea to hold tolerances.
 








 
Back
Top