Finish cuts: how lite?

Awl--
Admittedly a pretty general Q, but here's the rationale/context:
I have observed that it is possible to take too lite of a finish cut, in
both side milling and face milling, and in turning.
I've forgotten the exact scenario, but something like .002-005 was too lite,
and .015-.020 seemed to have been much better.
Whatever the exact differences in the numbers were, the appearance was
strikingly different, in manual lathe work as well.
Are there any guidelines/rules of thumb for finish cuts?
For example, in milling, on alum or unhardened 4140, using insert face mills
or 4 flute em sidemilling. Also in turning.
Reply to
Proctologically Violated©®
Loading thread data ...
"Proctologically Violated©®" wrote in message news:F%Eui.16$ snipped-for-privacy@newsfe12.lga...
That really depends upon the metal, your tool geometry, and the tool's degree of polish.
I usually DO take less than half-a-thou on the last cut; normally, just for cosmetics, but also for close fit-ups.
Really light passes, just pulling black swarf, require that everything be very, very rigid. Take up all the lost motion everywhere, make sure your spindle bearings are at the right preload, and snug up every gib. (and don't forget all your feed screws' loading nuts, if you don't intend to lock a particular axis.)
LLoyd
Reply to
Lloyd E. Sponenburgh
To summarize what Lloyd sez:
Be sure the width of "finish" chips is less than the depth of chatter.
Bob Swinney
"Proctologically Violated©®" wrote in message news:F%Eui.16$ snipped-for-privacy@newsfe12.lga...
That really depends upon the metal, your tool geometry, and the tool's degree of polish.
I usually DO take less than half-a-thou on the last cut; normally, just for cosmetics, but also for close fit-ups.
Really light passes, just pulling black swarf, require that everything be very, very rigid. Take up all the lost motion everywhere, make sure your spindle bearings are at the right preload, and snug up every gib. (and don't forget all your feed screws' loading nuts, if you don't intend to lock a particular axis.)
LLoyd
Reply to
Robert Swinney
"Proctologically Violated©®" wrote in message news:F%Eui.16$ snipped-for-privacy@newsfe12.lga...
A lot of this depends on the rigidity of the machine and the tool geometry. The looser the machine the more careful you have to be as there is less pressure taking up the flex with a lighter cut.
Most of the machines I have worked on have been clunkers, so before I get to size I will play a bit to get the balance right. In school they had a nice Hardinge, and that machine was a dream to run.
I have noticed that a better finish is obtained when the bit is ground with a bit of a radius and there is a little rub on the face of the bit. The down side to this geometry is that you can't hog away as much. I suspect this is because the tool bit is retaining more heat that would be ordinarily carried away in the chips.
The bugger is when relying on the tool geometry to spring the cutter back a bit to take up the slack and the spring, is what happens when you are ending the cut. It can be a bit tricky to stop the feed and back off the pressure before the cutter reduces the size of the work at the end of cut. This is when it would be really nice to have three or four hands.
Reply to
Roger Shoaf
At a few tenths of cutting depth, even a "sharp cornered" tool can be given enough radius with a couple of quick licks with an Arkansas hard-stone.
Don't forget that your workpiece finish cannot be any finer than the finish on the tool. A burred-up tool face with visible grinding marks gives a burred-up finish. Attack a job with a rasp, and it'll LOOK like it was attacked with a rasp .
The less tool surface contacting the work, the narrower the chip; and thus, the less pressure and horsepower to cut. Less pressure means less spring in the works. Less spring means better finish with a less rigid machine.
Unless the material really needs a lot of rake to cut cleanly, I get my nicest burnishing cuts with approximately zero back and side rake, a very broad radius on the tool (I know; contrary to what I wrote above), a mirror polish on its edge, and the finest feed I can set -- or endure.
'Course, the width of the chip has to be greater than the feed, or you'll have to make numerous passes, polishing off the "highs" with successive cuts. (and not changing anything about the setup) Basically, repeating the process until it no longer moves any metal.
LLoyd
Reply to
Lloyd E. Sponenburgh
"Proctologically Violated©®" wrote in message news:F%Eui.16$ snipped-for-privacy@newsfe12.lga...
Suggest quit with crossposting this kinda shit--( already more than enough fruit loops in the bowl as it is )
Reply to
PrecisioNmachinisT
"You can't get a better finish on your part than what's ground into your end mill."
Reference: Bud Darling, San Fernando Valley Circa 1974. He had worked in 52 shops in 25 years. What an exposure he had. My Hero. Only met him once in ''74. I learned more that evening than any time afterwards in a the few hours we had.
He also said climb accross, conventional back. One: this gives you an automatic finish pass. Two: You can cut with more surface speed while climb cutting because the heat is being forced back into the body of the part. In conventional cutting as the cutter exits the edge of the part the heat concentrates in the thin edge and turns it dark. This is hard on cutter life.
Regards,
Stan-
Reply to
Metalcutter
"Proctologically Violated©®" wrote in news:F%Eui.16$ snipped-for-privacy@newsfe12.lga:
In turning 60% of the inserts nose radius is bare minimum as a "rule of thumb".
In milling it doesn't matter provided you've got a good end mill and enough rpm and feedrate. But you'll need to trade in the Fadal and buy a CAM system.
Reply to
D Murphy
Why would one need a CAM system to control finish depth of cut? Couldn't tool comp be utilized?
Reply to
Bart
Invalid argument. A wheel has an essentially infinite number of cutting edges, all (eventually) playing at the same cutting depth. A tool bit has a single cutting edge, whose cutting-plane defects will telegraph to the work.
Sure, with an infinite number of cuts at an infinite number of starting positions, even a rough tool can give a smooth finish.
(chatter doesn't count in this discussion -- you're supposed to have eliminated all that before the tool finish becomes important)
LLoyd
Reply to
Lloyd E. Sponenburgh
"You can't get a better finish on your part than what's ground into your end mill."
.... heh! Where'd I hear something like THAT before ?
He also said climb accross, conventional back. One: this gives you an automatic finish pass.
.... yup... but there's a "yeahbut" in there. Yeah, but a lot of the cheap machines built of grey-colored jello (and old, worn machines) have so much flex and slop that conventional won't allow you to hold a dimension. So, many rec. machinists end up climbing on all cuts, lest they over cut or chatter the hell out of the surface.
Gotta have near-perfect rigidity to do it right.
LLoyd
Reply to
Lloyd E. Sponenburgh
I've always had good luck with it LLoyd.
But then my experience is fairly narrow and limited to Blue Hurcos and an Index mill. :-) I've never run BIG stuff.
The theory was: The climb cut would stress the tool and machine away from the part and then when coming back on the same setting the tool and machine would relax; and that small movement would allow for a finish cut. Hand mill stuff.
As for CNC-ing I usually just run the same path again after the roughing cut. That usually puts me within .001-.002 of where I want to be.
Regards,
Stan-
Reply to
Metalcutter
On a real machine 0.020 to 0.030 is a finishing cut. Many on r.c.m have light machines where that is roughing and due to the rigidity of the machine they tend to burnish the part to size.
Wes
Reply to
Wes
"Bart" wrote in news:1b23e$46bc4760$d8444218$20689 @FUSE.NET:
The link was to a high speed machining article. HSM is hard to pull off without the proper software.
Reply to
D Murphy
You sure of that sequence? I've found that the reverse is usually preferable.
You typically get better finishes from a light climb cut than from a light conventional cut. With a conventional cut, the chip goes from thin to thick, and the cutter may skid on the surface until there is enough pressure and depth to get it to start taking a chip. With a climb cut, the chip goes from thick to thin, and the cutter is cutting from the start.
The problem with climb cutting is that it requires more machine rigidity and less slop in the feed screws. And tight gibs. On my horizontal mill, I can take a heavy conventional cut, but anything more than a very light climb cut will try to pull the table along. Not good.
So, for me, it's a heavy conventional cut followed by a light climb cut.
Same thing with woodworking, but for somewhat different reasons. A conventional cut tends to pull fibers up out of the surface, a climb cut does not. But you don't want to try one with a router or shaper unless it is a very light cut, unless the work is controlled by a stock feeder.
Just my $.02 worth. Anyone else?
John Martin
Reply to
John Martin
It's worked for me John.
No my work if the table starts running ahead I just tighten the table brake to just eliminate it.
Most of my equipment isn't all that worn though.
Thanks for the reply,
Stan-
Reply to
Metalcutter
Im afraid there are no cut and dried answers to this one.
It largely depends on material, cutter type and material, rake, relief and so forth. As well as machine rigidity, vibration, rpm etc etc
HSS "properly ground" will allow you to more often make a .0005 cut..than will carbide in more materials than will carbide. YMMV
And it depends on what finish you want..a 16 or an 8
Based on my interaction in machine shops..one has to experiement a bit..or be a really experienced machinist who has used the particular machine and material combo before.
Shrug
Gunner, waiting for the flames
Reply to
Gunner Asch
I second that and extend: * coolant or cutting oil or dry cutting * lubrication of lathe's bed and feed spindle. * spindle temperature * slightly clamping the saddle or not
and and an. It is not just the tool!
Re material: I have some round (thanks good almost used up) that is nice to turn the first mm, then there comes a region of 1mm that is a pain and then it gets nice again.
Nick
Reply to
Nick Mueller
I generally use .010" as my default, and rarely have to change it. On rare occasions I have to go up, as the roughing pass in a slot wanders more than that due to tool deflection. Probably doing too deep a Z step on that one. This seems to work quite well for me. It might be machine dependent, as well as tool and workpiece material.
Jon
Reply to
Jon Elson
Yes, I agree completely. I do as much climb milling as possible, now that I have a pretty rigid CNC machine with ballscrews. I get better tool life and much smoother finish. I used to always finish with a climb cut on my manual machine as it gave a better finish, and a light climb cut would not cause the table to jump toward the work.
Jon
Reply to
Jon Elson

PolyTech Forum website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.