What's new
What's new

Lathe DOC, Feeds and Speeds, turning questions.

Higgins909

Aluminum
Joined
Nov 19, 2018
I'm trying to figure out depth of cut and feeds and speeds for lathes. We use Iscar tooling, VNMG 331-NF and CNMG 432-TF and maybe DCMT don't know the size. (DCMT might not be right but it's a 55 deg insert with 4 usable corners) They're all the IC907 grade if I remember right. In some machines we use VNMG and CNMG and one machine that I know of we use VNMG and DCMT. I'm looking at the cutting specs of these inserts and it makes we wonder if we're using them to the max.

Sometimes the first roughing pass just turns air and sometimes there are 2 finishing passes with the VNMG. The VNMG is usually used as a finishing insert. something I can remember is that we take 1" of bar stock and turn it down to .750" that's .250" of material. The CNMG has a max ap (DOC) of .157" and the VNMG is .098" Should I try to do 1 pass with each insert? This has me thinking that I could spread the wear over more area of the insert, then just the tip. As well as machine wear. Say .157 with the rougher and then .093" with the finishing insert? The VNMG usually only takes off something like .005" per pass. I assume the Vc would have the be lowered, but what about the Ft (IPR) Then about material deflection...

Can anyone give me some info on this without getting to technical as I'm learning. A lot of the internet stuff on CNC is mill stuff. (Titans, NY CNC, HAAS)

Thanks,
Higgins909
 
If this is a production shop I might worry less about using another .05 of insert DoC and remove those air cuts which are costing you a lot more than an extra few % on an insert.

Depending on your parts and machine I would be hesitant burying a tool almost .2” deep - especially on a 1” diameter bar. I think you will have difficulty breaking a chip at the feed rate you’ll end up at. Remember negative inserts already have a lot of tool pressure and that will only increase with DoC.

Two finishing passes may be perfectly reasonable once again depending on your part geometry and you haven’t given us much to go on.
 
First DOC is measured radially. It is what the insert sees. You only need .125" DOC to do it in one pass from 1.000 to .750.

What kind of machine do you have, what are you holding the bar with, and what is the material? What kind of tolerance are you trying to hold?

If you are taking .005" off of the diameter for a finish pass that is likely too little and causing chip problems. Try 2/3 of the insert radius as the minimum DOC (i.e. if you have a .015" radius insert take at least .020" off the diameter).
 
As I'm learning, my terminology might not be quite correct. This particular part is 1" bar stock 1018 steel (not sure on what steel it is, but it's gummy and hard to get a good finish) It gets turned down to .750" and a drill and tap and then part off. Then there is a whole 2nd operation. I just wonder on some parts if it's unnecessary to use a roughing tool and just use a finishing tool.

The machine is a Mitsubishi LT-350. 3 jaw, pedal clamp, 4k spindle. Something like a 8" chuck with a 2" bore. The material 20"~ just kinda floats in the spindle and we manually bar pull it. I really don't know too much about it. So, DOC... The lathe has NAVI which makes programming easier, otherwise it's more of a G-code machine or something like that. I think you can tell it a starting cut on the X axis and then where it stops on the X axis and there is a parameter for "Cut Amount" If I set that as .040" is that also radially? It would then take .080" off diameter, each pass until it hits the last pass and that pass might be less then the actual .040" "Cut Amount"
 
This particular part is 1" bar stock 1018 steel (not sure on what steel it is, but it's gummy and hard to get a good finish) It gets turned down to .750" and a drill and tap and then part off.
Without more info this is going out on a limb but ... if your lathe has any balls at all :

Traditionally, tool life was determined first by speed, second by feed and last by depth of cut. So for best tool life and fastest metal removal you went for the deepest cut the machine could manage, followed by the highest feed, and last the fastest speed.

In your case, I'd take one rough pass with the cnmg then one finish pass with your vnmg. I don't specially like vnmg's, they are kind of fragile but I guess you are using it to do reliefs or something ?

Also, I've never had good luck with such a light finish pass on gooey material. With 8620 I'd always go at least .020" on a side and kick the speed up enough to get shiny finish. That's not always the most accurate finish but shiny looks good for the customer, especially in any areas that don't count.

You can easily break the chip on a cnmg rougher. I'd break a .375" deep chip easily. Just kick up your feed. With cnmg's you need at least .015 fpr or they won't break. But if you've got the power you can nail it much harder than that. When it sounds like a machine gun with the chips hitting the enclosure, the motor is crying and you're getting blue sixes and nines, then you're in the ballpark.

Modern machines have doors. You don't have to be scared of burning to death anymore. Gas it up :D

And yeah, air cuts. Jeeze. That's a total waste. Nobody pays you for cutting air !
 
cutting air on first roughing pass, also called "what if big pass"
.
been around long enough, you see catastrophic and expensive damage when there are not enough what if big passes. when machine is broken and got estimate of 3 months til repaired it makes "time wasted" taking what if big passes look like the greatest time savings ever.
.
obviously if raw part is big in spots often by accident or mistake, do you really want to seriously damage machine? sure some simple parts you can measure raw part but as part get more complex and as operator deals with more many parts it only takes one big part to slip through and BAM severe damage.
.
some operators will go into and out of dry run mode at 200 ipm to fast forward past what if big passes. if operator running 2 machines best to let program run as is. if anything program might have extra M1 optional stops to wait for operator to be safe on some ops where problems occasionally happen.
.
extra finish passes are common where tolerances are exceeded with only one finish pass. if takes hours to recut even 40% of parts, it often saves time to add extra finish pass and get 99.999% in tolerance. when you record total actual time to make part including any problems with problem causes recorded you often see at end of year that adding 5 minutes of extra cuts thats say 50 hours per year added extra cuts, saves over 100 hours per year of recuts or rework. often going "slower" is actually faster
 
DMF, I've seen what if big passes be a thing on forgings and saw cut blanks but it sure sounds like a complete waste of time on hand pulled bar stock. If the part is tight tolerance I could see 2 finish passes so the part can be mic'd and offset before the final finish pass. That doesn't seem to be the case here.

1018 is soft and you seem to be holding it well. You can likely do the work in 2 passes no problem. One rough with the CNMG and one finish with the VNMG. If you wanted to do 2 roughing passes just to be "safe" it would still improve the cycle time greatly.

On the control everything in X is diameter or doubled while Z is not. If you want to leave a .010 DOC on the face and OD you need to leave .020 in X and .010 in Z.
 
FYI IC907 is a PVD grade and you would likely be better suited with a CVD grade like IC8150 at least for the roughing. CVD is a thicker coating. If the -TF is breaking chips you can keep that and change only the grade.
 
First DOC is measured radially. It is what the insert sees. You only need .125" DOC to do it in one pass from 1.000 to .750.

What kind of machine do you have, what are you holding the bar with, and what is the material? What kind of tolerance are you trying to hold?

If you are taking .005" off of the diameter for a finish pass that is likely too little and causing chip problems. Try 2/3 of the insert radius as the minimum DOC (i.e. if you have a .015" radius insert take at least .020" off the diameter).

Could you explain how .020" is 2/3 of .015"? Is there some math I don't know? Thanks.


On these I don't think it's a "what if big pass"

For finishing. Say a VNMG 432-TF IC907, would you do something like 2 passes of .005" or would one just be touching it at something like .0001". (Take a cut smaller then minimum insert Ap?) Depending on tolerance. We usually have a +- .005" tolerance but If the part calls for .750", I want it to be right there and very consistent. I asked my lathe guy, who is almost like a mentor. (I'd love to be a real apprentice, but shop doesn't run like that) How much material he leaves for the finishing pass and he says .005" for both X and Z if I remember right. I told him people are telling me .020" Ap for a finishing pass and asking why he takes smaller cuts in general and then he points over to the other guy and tells me look at his machines, they're all messed up. He has to zero the tools in a special way. I didn't really know where to go from there.

This machine has doors and some balls, just not sure how big. :D Even with coolant, should I see blue chips? How would that effect tool life?
 
Higgins, I think he means 2/3 of the corner diameter. Or 2/3 more than the radius. Doesn't matter really, just keep the radius buried. Unless you can't.

DOC is free
Feed is most operable
Speed kills
In that order.

R
 
This machine has doors and some balls, just not sure how big. :D Even with coolant, should I see blue chips? How would that effect tool life?
Yes, you can get blue chips even with coolant.

A lot of this depends on the material and your part and what the shop philosophy is regarding tool life. I did "run it like you stole it" for a while, then tried the Jap "careful ! that tool costs money !" method. Did big cuts and little ones ... in the end I think it's all kind of the same. What you gain in speed by running hard you lose in insert changes. If you run conservatively then you don't get as many parts out. If the area on the part is a finished journal, then slow the feed and increase the speed a little to get a smoother finish. In an area that's cosmetic I'll hit it pretty hard to get shiny shiny, shiny boots of leather, whiplash girlchild, in the dark ... Anyway. Adjust your method to fit the circumstances and the material.

But I never had any luck in soft material doing what you are doing. On 9310 I would take it down to .002 away from finish then a .001 on a side finish pass with a hook to grab that razor-sharp long stringy chip coming off, or you couldn't get a finish. But on 8620 it was about .015 on a side and push it pretty hard on feed. 4140, 4340 are somewhere in between.

.005 isn't even a tolerance, you can do that in your sleep ! On 80's lathes with hard ways, dc drives, resolver feedback and a thirty second refresh rate, you could hold .0003 with a little effort. .0001 or .0002 you were just chasing your tail but at three, you could start to do something. A half was a picnic.

I always left more on x than z. And programmed a short dwell in the corners so that you got a real square corner all the way around the part. And a face that was flat all the way to the x dimension.

I find diameter programming goofy but to each his own.

On tool life, pushing it hard I'd get about fifteen minutes per corner on a coated insert at 400 fpm in softish stuff, longer for finish at a higher speed. Running Jap-style, maybe a half hour per corner. Inserts should be better now but probably cost more so there ya are, back where ya started.

The yuckiest thing about your parts is the small diameters. Down around one inch things get a little weird, the speeds are high and the geometry isn't so great. You'll have to experiment a bit. Probly somewhat less depth of cut than I am used to - but still a lot more than you are using now ! Just for a start, I'd go to two roughing passes and one bigger finish pass. That'd give you a feel for heavier cuts. Then try a single rougher. I can't imagine needing an air pass, cold finished bar stock repeats pretty good :D

Don't know why your guy thinks it hurts the machine ... they are meant to cut metal. I love the needle in the red. The motor can cool off on the retracts :) Just keep it oiled and clean and there ya go.

Made more than a few thousand round parts over the years and when the factory tech guys would drop by they always got a smile on their face from watching the machine work. But that was US-built lathes in a time long gone.

Anyway, doesn't hurt to try, yes ? Altho sounds like your mentor is going to frown when he hears them chips hit the enclosure like a little gatling gun :D
 
Could you explain how .020" is 2/3 of .015"? Is there some math I don't know? Thanks.
DOC is in radius. If you do 2/3 of a R.015 you get .010. That is in radius. Now make it diameter (.010 per side = .020 diameter). There isn't a per side in Z so you would just leave .010 to get the same DOC.
 
Could you explain how .020" is 2/3 of .015"? Is there some math I don't know? Thanks.


On these I don't think it's a "what if big pass"

For finishing. Say a VNMG 432-TF IC907, would you do something like 2 passes of .005" or would one just be touching it at something like .0001". (Take a cut smaller then minimum insert Ap?) Depending on tolerance. We usually have a +- .005" tolerance but If the part calls for .750", I want it to be right there and very consistent. I asked my lathe guy, who is almost like a mentor. (I'd love to be a real apprentice, but shop doesn't run like that) How much material he leaves for the finishing pass and he says .005" for both X and Z if I remember right. I told him people are telling me .020" Ap for a finishing pass and asking why he takes smaller cuts in general and then he points over to the other guy and tells me look at his machines, they're all messed up. He has to zero the tools in a special waw where ts machine has doors and some balls, just not sure how big. :D Even with coolant, should I see blue chips? How would that effect tool life?

Id find out how much experience your "mentor" has, especially with running other machines. Maybe he's only ever run the ones he's running now and he just hasn't ever considered doing anything different than the way he was taught. If thats the case you might need to ask a lot of questions here.
Best advice i can give u is this: If you have load-meters on your machine use them. And dont be afraid to try something different, maybe just ask for input from your "mentor" first, that way you guys can feel like you're learning together, rather than just you experimenting and learning on your own and ultimately progressing more quickly than he did when he was in your position.
 








 
Back
Top