Lathe roughing, how deep have you cut?
Got a big job coming up, lots of O.D. roughing on 15" 1045 hot rolled material, O.D gets turned down to 10" for a good distance, machine is a Daewoo 400 PUMA lathe with 21" 3 jaw chuck, gripping on 2" of material with soft jaws and with 6 to 12" hanging out of jaws, I plan on cutting a radius in the I.D. to run a bell center for the roughing operation, I have a WNMG 643 tool holder for the roughing, just wondering how deep a cut would be considered TOO deep? The deepest I have gone so far is about .265 per side @ .016 feed in 316 SS and the tool looks like it could go close to .5 deep. I just don't want to tear up something, suggestions?
What is the HP n your machine?
You gave the depth of cut and feedrate, but what SFM are you using?
Get the biggest 80 dgree insert, then about .3" depth at 400 SFM is a reasonble depth.
Good luck, just sneak up on deeper cuts carefully. Make the first 2 or 3 at lesser depth then slowly go deeper.
Be careful: Heinz. Fanuc CNC programming training. Learn CNC for Fanuc, Yasnac, Mitsubishi CNC controls, CNC Machining Videos and DVD's, CNC programming training, CNC education,and CNC consulting.
I have run 643's on a 12 inch chuck at .3 per side. 400 SFM with a feed of .02. This was on 4140 heat treated material, so I'm sure you would be safe at least duplicating that.
There is a calculation for max depth of cut on inserts. It has to do with the I.C. dimension of the insert, but I'm not sure what that calculation is. Someone might pipe up who knows it.
That sounds like a good cut. I think you could run 600 SFM in 1045.
Originally Posted by Dave K
I'll be interested to hear how deep you manage to cut.
On a reasonably heavy 28" manual lathe (12 speed and 25 hp to crank it), I've not had much luck going deeper than about .375" radial depth of cut in steel. There always seemed to be a low frequency rumble that would slowly grow in crescendo. But at 1/4" deep it was fine, and the feed could be boosted to .025"/rev. Use an insert with the proper land width for heavy feeds so as not to have a chip pile up and break the insert.
I have sucessfully cut .375 (radius) in 1045 with my 18x54 L&S (15hp), .250 is comfortable. If speed is a concern, a more agressive feed rate is preferable for good tool life.
we have manage to do alot of .375 DOC on ours manual lathe (30 hp) easyli. we were using a TNMG with a 1" holder. at 0.018 feed
Depends on a few factors obviously, main one how hard you can hold the piece, and how much power you can put to it before something breaks. Also check what the insert likes, sometimes you can go almost the full cutting edge but they don't all like too heavy a feed.
The info on the package will give a pretty good idea of the limits on either end.
Either way, no time saving if something breaks.
Hi there, have you consider the use of high feed inserts instead of a big DOC?
We have the exact same machine. Being you are out of the jaws more than I would feel comfortable with; I recommend you put the tailstock against it with a bull nose. This will assure you the part does not come out of the chuck. After you do this; put it in low gear and put the coals to it! Look at the max depth of cut on the insert, and back it off by 10%. Take a look at your HP usage (you have TONS of torque in low gear).
Good Luck and BE SAFE!
I used to run a Puma 800 and most of the time i took .400 per side with a .022 ipr at 350-450 sfm in 4140 and 4340 cutting api connections. most diameters were between 6"-10".
With todays inserts, I would agree with that.
Originally Posted by ewlsey
As I said above the parts WILL have a center in them, I'm using Iscar inserts and the max depth of cut isn't listed on the insert box and the website is impossible to find any useful information on.
Originally Posted by Polishpiper
400+sfm, wnmg 644-nr IC 9350, IC 8250 insert (Iscar nomenclature), .3-.4 doc, .025-.03 fpr. Like the grouchy old man in the first shop I worked at said: "There ain't no money in the rough."
A Canadian penny is about the same size as an American.
That was in 4145HT material
Originally Posted by alphonso
Kinda funny cause how fast you can rough all the material out of the way is often where most of the money and time saving is, but there's definitely no $ until its all done.
You sure he wasn't talking about golf?
Like the grouchy old man in the first shop I worked at said: "There ain't no money in the rough."
I'm glad you said you were using the tailstock, that ensures safety of you and the machine.
Most I ever took on my Okuma LB15 (8" chuck 15 hp two speed gear box) was .2" on the side, with hot rolled 4140 in hard jaws and a tailstock to support it.
On my Mori SL-3 it was a little more, about .3" on the side.
Most I saw ever was a giant Doosan lathe taking about .4" on the side. Wow!
I've cut carbon steel ( A236) that size at .300 doc @ 600 SFPM and .022 IPR using Walter/Valenite's new grade WSM10. I think you need to go with a 633 or 644 to use as large of a TNR as possible.
Originally Posted by Cuda
also, you might want to release the tailstock and reclamp your chuck to relieve the pressure build up.
Originally Posted by Cuda
feed 1.6 ipm (for 0.016" thick chip)
Depth of cut 0.250"
or 400sfpm *12 so 4800 Surface inch per minute so 4800*0.016*0.250= 19.2 ??
so 19.2 cubic inches per minute ???
material 1045 (0.6 cubic inches per min per hp)
32 hp required
2640 cutting force on the END of piece trying to push it out of chuck jaws
........ could be wrong but math I got says your DOC, chip thickness AND SFPM thus rpm are major factors basically at 100 sfpm it is ??
4.8 cubic inches per min
8 hp still at 2640 lbs of cutting force because rpm is 25.5 and now 1200 surface inch per minute (100SFPM) at 0.250 DOC at 0.016" thick chip
at 0.008" thick chip is 4hp and 1320 lbs of cutting force (2.4 cubic inches per min)
........ this is saying nothing about if chips are long and stringy and wrapping around part. Maybe more important to adjust chip thickness and depth of cut to get short chips breaking up nicely ??? 0.016" thick by 0.250" chips can be strong and hard to break.
my math could be wrong so check it yourself