Another Parting Off Question.

Grits · Jun 30, 2007

Hello Everyone

I am parting off .500" slices from a 3.500" piece off round 4140, solid steel bar. I am using a carbide insert that is 0.160" wide. The maximum recommended diameter of my tool is 4.000". The first cut I made was at 100 RPM taking .0025" per revolution using flood coolant. The cutting tool was set slightly above center. The tool holder was perpendicular to the work within 0.0005". The cut was taken two inches from a eight inch Buck four jaw chuck. My lathe is a Nardini 1440E.

I got a good cut but it sure make a nice howl. Nothing bad happened but I had an uneasy feeling. I am somewhat new using a carbide insert for parting off. Am I in the ballpark with my feed and speed? What are your recommendations?

I had a bad experience parting off something smaller using a HSS cutter with an Enco lathe. There was no permanent damage except to my nerves.

Thanks for all your help.

Grits

i_r_machinist · Jun 30, 2007

Grits,
I don't know whose tooling you are useing but a 1.6" wide insert is incredible! Look in the Iscar.com tooling catalog for a tool and speed for what you are doing. I work with alot of Iscar stuff and and am very happy with them. 100 rpm is slow for the Iscar stuff.
Have fun.
i_r_

HuFlungDung · Jun 30, 2007

That 'uneasy feeling' has to do with your manparts increasing in size

Yeah, the tools make a noise, but put on your hearing protection, and let it rip.

Be careful to keep the speed up as slow speeds can cause built up edge to form, and chip the insert, because the chip comes off rougher at low speed, and we want smooth chips when parting. 350SFM in 4140 prehard, and using CSS (constant surface speed) to keep the rpm ascending gives excellent results. Don't forget to put a 'clamp value' on your spindle speed so your chuck doesn't approach infinity for rpm.

.004" feed works for me quite consistently, with good tool life.

If you don't have CSS available, then, I would recommend that you part down to about 1.5" diameter, then shift up to get your SFM back in the right range. At about X.5" decrease the feed to about .002"/rev and this may help preserve the cutting edge for many cuts.

dkmc · Jul 1, 2007

hum........I'm gonna bet .25cents that he meant .160 wide? Either that or it 'sticks out' 1.6 inches...

:eek:

Grits · Jul 1, 2007

Guys, I got the decimal point in the wrong place. I edited the mistake. The insert is 0.160" wide. The tooling is Dorian.

See what I get when I am trying to be precise and provide all the right information. At least it was not on the part.

The tool holder sticks out about 1.900". I looks like a mile but it is just enough to provide clearance for the workpiece.

Another error in my original post. The stock has a 0.750" hole in the center.

The incident I mentioned with my old lathe has me abit gun shy when working with larger stock. I was parting off a two inch piece if HRS with a HSS parting tool. The tool grabbed and tried to go under the workpiece. It may have been an illusion, but I swear I saw the compound and carriage roll forward before the cutter snapped. It would not be appropriate to post exactly what I said when it happened but no one would be surprised with the language and volume, especially if something similar had happened to them. The difference between the Nardini and the Enco is night and day. I am still getting use to the fact I can make bigger cuts with faster feed rates etc.

Thanks

Grits

Jaycee · Jul 1, 2007

Grits: just wanted to address the position of the parting tool, "the cutting tool was set slightly above center". The parting tool should be set slightly below center, probably why you got the howling, Rubbing just below the cutting edge. How far below center, .005-.010 . Keep your tool as ridgid as possible. Good Luck J.C. p.s. I would part a little closer to the chuck.

Grits · Jul 1, 2007

Jaycee

Do to the diameter of the part, I cannot get any closer. The next cut will be 0.660" closer to the Chuck and the last cut will add another inch even. I do have a solid grit on the stock.

I have been under the impression a parting tool set below the center line can cause the tool bit to try to roll under the stock. Am I mistaken in that concept?

Thanks,

Grits

Chris999 · Jul 1, 2007

100 RPM is only 90 fpm at the largest dia. Way too slow. For carbide parting tools to work properly you need to be in the proper speed range, and use lots of feed. I've found increasing the feed frequently makes the chatter go away, even though it is against your instincts. Parting with carbide inserts is night and day compared with HSS. Look up your insert grade online for speed and feed recommendations.

Annealed 4140 is fairly soft, for a similar Iscar insert my book gives ~500fpm at 0.012 feed and ~250 at 0.016 ipr.

Crank up your rpm to at least 300 and increase the feed, a 4mm wide tool is plenty rigid just keep it flooded and like Hu Flung said you could increase the speed as you get smaller although that's not always practical. You might be able to shorten the overhang so the tool holder is almost touching when you break through.

In short: Crank up the speed, crank up the feed, tighten yer undies and let 'er fly.

Jaycee · Jul 1, 2007

Grits: I assuming since you are using carbide, that you have a quick change holder (ALORIS or PHASE 111) or the like, if that is the case, the tool will be on the same plane as the center line of the work piece, and .005-.010 below center, as long as the tool is held ridgid will not present a problem. Keep it closer to -.005 as you are using higher speeds, and use lot's of coolant. Good Luck J.C.

Grits · Jul 1, 2007

My tool post is and Aloris BXA.

I started at 250 RPM and got just a little nervous and dropped back to 100 RPM. I will crank it up to the recomended speed and feed and I WILL STAND BACK.

Grits

HelicalCut · Jul 1, 2007

.0025 feed, is that the feed you read off the dial? many machines halve the feed when cross feeding.

I use .007 ipr on the dial which is .0035ipr when cross feeding much less and it screams.

Grits · Jul 1, 2007

HelicalCut, 0.0025 rounded was the depth of cut. My dial also shows half and my cross feed is half the longitudinal feed.

Grits

Racer Al · Jul 1, 2007

Grits: I, too have experience with smaller, less-rigid machines, and exploding HSS parting bits.

Tighten up your gibs, and have at it. Have faith: things get a LOT better when you put enough **consistent** pressure on the tool to make a curl come off, not small chips. If you're on a manual machine, (sorry, not familiar with Nardinis) then you need to use a "hand-over-hand" method to provide an even feed rate. The sound changes as well, it makes an aggressive hissing noise. Too light feed invariably chatters and squeals.

Getting the parting tool exactly perpendicular to the ways is critical for parting thick pieces as the side of the tool will rub. If you keep cutting, it will deflect the tool sideways, which bends the cutter (very bad for HHS) and will make a dished cut.

Grits · Jul 1, 2007

Racer Al

My Nardini is a manual machine. It is 14x40 and weighs in at over 3K. That is over three times the beef of my Enco which was the same size. It seems to be a pretty rigid machine. Unlike the old Enco, the dials hit the numbers and it is as smooth as glass. I really like it.

Grits

adama · Jul 1, 2007

is that a square or angled insert? some times the angle crates a little natural deflection causing what u state as the problem. disadvantage of the square insert is the burr on the part but hell win some, lose sum.

i have just got myself a inset parting tool for my home lathe, its a 11" harrison and whilst its got a power cross feed, i cant go over 720 rpm at the moment, even then torque is limited so the surface speed might cause me major problems. hopefully soon the lathes vfd will be swapped to the surface grinder, a more manly one purchased along with a sensible sized motor like 3 real killowatts not 1kw

im then hopping for nearer the magical 1k rpm with some tourque too. the lathes solid as a rock way over enginered for a 11" lathe in my oppinion and has a L00 spidle so bags of rigidity there, just gota get the rpm to make use of it.

Grits · Jul 2, 2007

Well boys, I followed your advise and I have not had that much fun since I quit drinking. I guess I am easy to entertain. I ran the lathe at four hundred rpm with a feed rate of about .005" pr. Coolant and chips were going everywhere and I got a perfect cut. I have one "chip" that is six feet long and a perfect straw color with just a little bit of blue. It started making a little noise toward the end of the cut but thing were going so well I just left well enough alone.

Ya'll gave me a great advise and now I have a starting point for future work. I was way out of the ballpark. I am also learning what my machine is capable of.

Thanks again for all your help.

Grits

Grits · Jul 3, 2007

Hello Everyone!

Would someone critique my work? Below you will find images of one of the pieces I parted off and an image of the chips. Some of the marks on the work piece came from a file when I was deburring.

The work piece is flat within .001"

Thanks

Grits

Jaycee · Jul 4, 2007

Grits: Thats pretty much what you can expect, at 366 surface ft. per minute , .005 feed , 4140 alloy and carbide tooling. Those straw colored curls can be pretty nasty with a convential lathe, no problem with a cnc, lots of coolant, and the door shut. No doubt that's probably the fastest way to achieve what you are doing. Be careful sneaking up on the feed lever. You are drilling the bolt circle after parting aren't you? A interupted cut is hard on carbide. J.C.

Canyonman · Jul 4, 2007

Hi Grits,

This may not apply now that you have got your speed and feed but.......I hate when the parted piece "flys" when it separates.

I put a rod or even a piece of re-bar in the Jacobs Chuck in the tail-stock and run it up the center hole.

Then it is just like a "Ringer" in Horseshoes! Slide the parted one over towards the tail-stock, move up, and cut the next.

Maybe this sounds a bit stupid, but I've parted off items and impaled them into my sheetrock!

Ken

Grits · Jul 4, 2007

Jaycee

I had the shield closed over my chuck and still had coolant everywhere, especially all over me. It made the cuts pretty slick. I did not realize I was soaked until I was finished. I was fascinated with how well everything worked and how quickly the cuts were made. My previous experience was with a much lighter machine and HSS.

It is a whole new world working with a rigid machine that is accurate. I could forget about hitting the numbers, using the dials, with my Enco. The dials were almost useless. I rigged dial indicators on all axis including the compound. I have a Newall DRO I am going to install on my Nardini but I have not been in a big hurry to do so. Results have been accurate with it; however, I may tackle that this weekend.

With all said, learning on a machine that did not work right taught me a lot, especially dealing with flex. Machine error was so exaggerated with my Enco, I had to always pay attention and keep my thinking cap on. Not that I do not pay attention now because I do my best to stay focused; however, the results I achieve now are predictable. In the past they were not. To say the least, I am having a whole lot of fun.

Thank you all again for all your help.

Grits

Another Parting Off Question.

Stainless

Titanium

Diamond

Diamond

Stainless

Aluminum

Stainless

Hot Rolled

Aluminum

Stainless

Stainless

Stainless

Stainless

Stainless

Diamond

Stainless

Stainless

Aluminum

Hot Rolled

Stainless

Similar threads