What are good cutting conditions for rough turning titanium? Depth of cut, cutting speed, feed rate. I've tried playing around a bit, but it seems very difficult to break the chips and inserts don't last too long. I was just wondering if anybody has any good combos that get the job done. (Currently using CNMG IC 20 and CNMG H13A inserts, if there are others that work better let me know also)
Follow along with the video below to see how to install our site as a web app on your home screen.
Note: This feature may not be available in some browsers.
Largest Manufacturing Technology Community on the Web
Stay Connected:
Turning Titanium
- Thread starter SLW
- Start date
- Replies 29
- Views 39,252
I don't know if you've seen this thread? If ya haven't ya might find it a good read.
Brent
http://www.practicalmachinist.com/vb/cnc-machining/issues-turning-titanium-284776/
Brent
http://www.practicalmachinist.com/vb/cnc-machining/issues-turning-titanium-284776/
65 to 70 meters a minute surface speed, lighter cuts ( 60-70% of what you would normally do in steel) and normal feed. Slower speed and lighter cuts is the key. Using normal grade steel inserts will work for a short run if that's all you have.
Rpm = (surface speed x 318) ÷ diameter for you imperial folks
Rpm = (surface speed x 318) ÷ diameter for you imperial folks
SeymourDumore
Diamond
- Joined
- Aug 2, 2005
- Location
- CT
Well, thank you for that last bit of information ( for those Imperial folks of us ....)
For what it's worth, a good starting point would be 80 SFM ( in imperial rather than M/min thank you very much ), let the machine figure out the RPM
Feed can be relatively high, easily as much as steel even if you have the torque, but use a good positive insert with a sharp edge and a decent chipbreaker.
You don't want too much of a honed edge.
Make sure you flood the cutter and don't let it dwell for long. Ever.
With TI, speed is the killer. a 10% increase in SFM above what it wants results in 100% increase in generated temperature.
When turning, you can almost feed as much as AL with the right grade/geometry insert, but there is hell to pay for SFM.
jkruger
Stainless
- Joined
- Feb 21, 2012
6AL-4V? Stick it in deep and go real slow.
I used CGGT ic20 from iscar and korloy with really good success. Basically did the same thing I do in aluminum but turned my SFM way down. Ti 6Al-4V cuts nicely with sharp positive inserts and low SFM. I was also able to take a really fine finish cut, although I'm learning that on rigid lathe parts a light finish pass isn't always necessary to get good dimensional results.
I've tried a few of your guys suggestions. It does seem to break chips better with a lighter depth of cut. .085 was the deepest I went, seems to work pretty good at .075. However, we've tried different speeds, and we have it running at 150-170 SFM with a .0125 feed... I know it's fast and different compared to your recommendations, but it does seem to work well. Thanks for all yalls input!
Well, thank you for that last bit of information ( for those Imperial folks of us ....)
For what it's worth, a good starting point would be 80 SFM ( in imperial rather than M/min thank you very much ), let the machine figure out the RPM
Feed can be relatively high, easily as much as steel even if you have the torque, but use a good positive insert with a sharp edge and a decent chipbreaker.
You don't want too much of a honed edge.
Make sure you flood the cutter and don't let it dwell for long. Ever.
With TI, speed is the killer. a 10% increase in SFM above what it wants results in 100% increase in generated temperature.
When turning, you can almost feed as much as AL with the right grade/geometry insert, but there is hell to pay for SFM.
Now when you say sharp insert, I assume you mean a sharper radius? I may sound dumb but I am asking to find out. We've been using inserts with a .0312 radius, so are you saying to try a smaller radius? Just wondering.
Terrible Juan
Cast Iron
- Joined
- Dec 22, 2009
- Location
- South Central Mountain USA
The IC20 is uncoated, it won't be able to handle that high of an SFM.
Get yourself some CNMG 432-TF IC907 or IC807 and you'll be good. Run it at 150 SFM.
PBMW
Titanium
- Joined
- Aug 13, 2005
- Location
- Bremerton, Wa
I turn and mill Ti almost exclusively now.
140ish sfm. WNMG inserts. .032 rad. Feed it pretty hard
DOC and feed will depend on your machine.
WNMG inserts offer far more support for the insert than anything else.
Lighter DOC's and you can turn it up.
140ish sfm. WNMG inserts. .032 rad. Feed it pretty hard
DOC and feed will depend on your machine.
WNMG inserts offer far more support for the insert than anything else.
Lighter DOC's and you can turn it up.
PMT
Cast Iron
- Joined
- Feb 5, 2004
- Location
- Franklin WI
Well if you Americans just change to bloody metric already everything would be fine.
When I was in school in the late 70's early 80's they talked about that and every one hated the idea, including me as I just got used to the fractions etc.
Now that I have been working on machines for the last 25 years and the 25.4 multiplier is etched in my brain it would have been a great idea to make the switch.
Hertz
Stainless
- Joined
- Apr 27, 2009
- Location
- Sudbury, Ontario, Canada
TeachMePlease
Diamond
- Joined
- Feb 11, 2014
- Location
- FL
Hertz
Stainless
- Joined
- Apr 27, 2009
- Location
- Sudbury, Ontario, Canada
BECAUSE 'MURRICA!
Hehe, actually had a good chuckle there. Thanks for that.
Kiwi 'smith Dean
Cast Iron
- Joined
- Jan 13, 2011
- Location
- Tauranga, New Zealand.
What is turning and threading 3Al-2.5V tubing like, in a cold-worked-stress-relieved condition? Any recommendations or other materials comparible with this?
Does anyone have a recommended Ti supplier for tubing?
Thanks, Dean.
