Can you hardturn?

If you can...please spill yer guts. I'm about to embark on a hardturning cruise, and I could use some pointers.
So far...I'm not using coolent1..but should I hook up an air blast?
Also, I can hardmill, so I understand the sparks need to look like I'm arc welding, so I can handle the feedrate.
What I don't yet understand is rpm, and how much to take per pass. The first parts I'm doing are about 1.5 inches diameter, length of cut is about 3 inches max. Tolerance needs to be grinding tolerance, surface finish needs to be at least close to grinding. .004-.005/ side stock max. Steel is S7 tool steel, maybe 52-54rc.
Mid grade lathe, good tooling.
Does it make a difference to feed towards or away from the spindle?
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
vinny wrote:

I've done a lot of it. What kind of inserts do you have?
CBN 432 size: 300-450 SFM .005 to .010 D.O.C. .002 to .006 IPR
CERAMIC .5 dia button: 350 to 500 SFM .005 to .020 D.O.C. .008 to .015 IPR
CERMET 432 size: 150 to 300 SFM .004 to .010 D.O.C. .002 to .004 IPR
the bigger the tool nose radius, the more side pressure developed. Watch for edge notching if you have to take a lot of passes, vary the D.O.C..
--
Steve Walker
snipped-for-privacy@verizonwallet.com (remove wallet to reply)
  Click to see the full signature.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

The first set of 40 blocks only had .005/side. H13. 52-54rc. Approx 2.4" dia. The inserts had a .031 radius. I used flood coolant. .005/rev feed. 400sfm. Used 2 identical tools. Had to rotate the first tool 3 times. I left .0005/side for the second tool. Interupted cut. In steel soft jaws. Results....+-.0002 on all diameters. Most +-.0001. Finish ok. Not as good as grinding, but ok. Went great. Took a day, not too bad considering we were training. (This was my training, not my setup.)
Next set of 20, .004/side. S7 stainless tool steel. 56rc. Steel soft jaws. 2 tools, .0005/side on second tool. .008 radius inserts. I USED AIR!!! (That pissed off my trainer for some reason, lol) Non interupted 3" long cut with shutoff angles and radius cuts. approx 1.4" dia. .0025/rev feed, and 500sfm. Results...went great, held +-.0001 on all parts except angles more than a few degrees. Seems this lathe doesnt repeat so well on dual axis cuts when hardcutting. Took me a few hours to setup and program(first job on my own), but after that....35 seconds a part. I did not change any inserts.
What Iv'e learned....................... 1.) Interupted cuts suck. 2.) Air rules over coolant, hands down. The chips come out as carbon powder. You can squeeze them to dust in your hand. There is no chip problem because they are charcoal chips. It's cleaner and quicker to change parts. Easier to get in the chuck closer because theres no coolent goo all over. 3.) If you have a cheap lathe, here's a trick I figured out on my first day using IPR. It's prolly common knowledge. Find out the max rpm you want to run your chuck. We have a 4000 grand lathe, but It shakes at 2000. So I set a max rpm to 1800. Now set your sfm higher until the spindle is limited. Thats the best your gonna get. If you have a badass lathe, why are you reading this dumb shit? 4.) That's all I got on my first day as a hard turner.
Somebody add something please?
I'll list my inserts tommorrow. They are generic for stainless soft machining. Iscar 8 sided.
I heard once coated inserts suck. The carbide under the coating is crap, so when the coating wears off the insert desolves. Anybody heard that before?
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

I read an article from Hardinge that liquid N2 is the best coolant for hard turning. Can't find the article now :(
Thank You, Randy
Remove 333 from email address to reply.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
Randy wrote:

Did you check MMS Online?
--
John R. Carroll



Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

Nope. You need to avoid thermo-cycling the insert.

RPM don't matter, surface feet per minute is the parameter you need to play with. Start at 300 SFM, and go up or down from there. Feed at 0.002 to 0.005" per rev.
You'll have to burn some inserts to find the right grade, speed, feed mix for your application. There's just too many variables to give you a hard fast answer. The biggest variable is your lathe. Different brands have different sweet spots.

Speaking of tooling, you're using a PCBN or a Ceramic insert, right?
As far as the lathe goes, it will either hard turn or it won't. If it won't you can screw with it forever and it's never going to work. You have to have a stiff spindle. If you don't, you'll have some sort of chatter, usually high frequency, and you'll bust insert after expensive insert. The cut should sound like a whisper. If it sounds like a whistle, find someone with a good lathe and farm it out to them.

Yup. Sometimes. Maybe. Depends.
--

Dan

Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

Polytechforum.com is a website by engineers for engineers. It is not affiliated with any of manufacturers or vendors discussed here. All logos and trade names are the property of their respective owners.