What's new
What's new

Why are interrupted cuts in turning bad and ok in milling?

First of all, that is a relative question but in general milling is like sawing, but with a wider blade. The "teeth" are designed to enter the work in sequence. Also, because the feed is controlled encountering a gap is not that much of an issue.

In turning, the tools tend to be less rigid and interrupted cuts cause unwanted flexing. Because the work is spinning at a fixed RPM the shock of crossing the gap is more severe. Also, carbide inserts, being more brittle don't do well with interrupted cuts. A properly sized and ground HSS bit actually tolerates interrupted cuts quite well if feed rates are kept reasonable.
 
Pretty sure it is mostly to do with the fact that most endmills have a helix angle, so the cut is less of a CHOP and more like a shear action.

Secondary to that, and what would explain 90* facemills, is you -generally- have more than one cutting edge in the cut, kinda adding stability to it.

There's also probably a lot to do with grades of carbide, turning tools being designed for constant smooth cutting, but there are also grades that can take more shock.

This was a seat of the pants answer, hopefully my points are not wrong and I'm sure there's a bunch of other reasons. There's probably some peer reviewed studies and crap out there too.
 
Did you ever wonder why milling inserts are always more expensive (gram for gram) than turning inserts?

It's because they always get an interrupted cut, which means a tougher grade with more binder, etc., etc.

There are turning inserts designed for interrupted cut, but that comes with a trade off in wear resistance.

There are also insert grades that can take 1800 SFM in 1018, but the slightest interruption will blow them into oblivion.


Like Tom Lipton said, "The only good thing about an interrupted cut is that the chips break no matter what."



Uh oh, now I'm sticking my neck out before CarbideBob gets here.....:leaving:
 
My guess would be the direction of the tool pressure and the fact lathe tools are stationary and not spinning, so the chip load is varying in an interrupted cut.
 
inserts

general question , or are you considering to turn interrupted cut.
as said above not preferred but doable with the right set up, sometimes
un avoidable.
 
It just occurred to me...


If the OP could figure out a way to do milling operations without an interrupted cut (besides the obvious choice of drilling or shaping) please let us know.


I'm envisioning a blank carbide dowel pin pushing metal around like play-doh.
 
It just occurred to me...


If the OP could figure out a way to do milling operations without an interrupted cut (besides the obvious choice of drilling or shaping) please let us know.


I'm envisioning a blank carbide dowel pin pushing metal around like play-doh.


That's what happens when you try to cut beyond your flute length. AKA Friction Stir Welding.
 
That's what happens when you try to cut beyond your flute length. AKA Friction Stir Welding.

Too bad I've never made a part that was SUPPOSED TO BE stir welded.


Does anyone do chemical machining anymore? I've never seen it done but I'm young and relatively sheltered (I guess?).

I just remember seeing it in old machining books and would think that'd be pretty awesome and dangerous. Mostly the former. Seems it is/was used a lot for big stuff? That would be an uninterrupted "cut" I guess.
 
Why are interrupted cuts in turning bad and ok in milling?

It's not that they're "bad".

It's that typical turning inserts aren't designed for significant interruptions. Going from a harder grade (more wear resistant) to a tougher grade (more impact resistant), the tradeoff is reduced tool life.

There are plenty of turning inserts designed for interrupted cuts, but even then there's a wide selection because only the user knows the rate of interruptions. Unlike a milling cutter, where you know that the length of cut is unlikely to be more than 1/2 the cutter circumference before an insert exits the workpiece, on a lathe, the insert might be buried in the workpiece for a long time before hitting interruptions. Or the interruptions could be nonstop.
 
I forget what they call it, but there are mills and multi-tasking machines that can sling around a boring bar while interpolating in synch with the spindle rotation. In theory one could extrapolate that technology to do something like eccentric turning around the profile of a part of almost any shape, provided the transitions are smooth enough. You'd need machine axes that can move faster than your desired cut SFM with really fast acceleration, and either the spindle would need to be a precision servo or you'd lock the spindle and use a rotary axis.
 
Too bad I've never made a part that was SUPPOSED TO BE stir welded.


Does anyone do chemical machining anymore? I've never seen it done but I'm young and relatively sheltered (I guess?).

I just remember seeing it in old machining books and would think that'd be pretty awesome and dangerous. Mostly the former. Seems it is/was used a lot for big stuff? That would be an uninterrupted "cut" I guess.
it's been years since I was involved with it but yes was done often for sheet & plate to reduce the thickness,
and was very accurate, aircraft application.eg chem. milling. mostly aircraft skins, complex contours, but this was before CNC, so it may not be used any more don't know.
 
Does anyone do chemical machining anymore? I've never seen it done but I'm young and relatively sheltered (I guess?).

I've seen it a few times (not in person, but on a print and the final product). Big piece of sheet metal. Formed and drilled/machined, and them chem milled in the non-important parts to make the metal thinner. I've seen it as optional on some electrical panels, say .100" thick material, bunch of switches and crap going through it, and then thinned out to .040 to .060 or so anywhere there wasn't something bolted to it. Hey.. That's a gram more of bombs or fuel you can carry.
 
Why are interrupted cuts in turning bad and ok in milling?

An interrupted cut is not necessarily bad, but it requires a different strategy to maintain acceptable tool life. Tool geometry and grade of carbide are the two key factors. Closely followed by Lead angle and edge prep. A flat top negative rake, reverse lead angle insert in a P40 grade with a hone will machine concrete effectively provided the set up is rigid and the machine has the balls.
And: HSS is not superior to carbide in TRS under adverse conditions. Go to a tube mill and watch a tube scarfing op. That’s true abuse.
 
I should have added: the only acceptable mode of failure is abrasive wear. The other modes are heat related (excessive sfm) and catastrophic mechanical failure.. breakage.

Interrupted cuts often cause breakage or chipping. Many times just going with a tougher grade will fix the issue. Next would be edge prep. I’m a big fan of medium temperature CVD coatings with a thick columnar structure. They offer a tremendous amount of compressive strength and bond well with the substrate. If you get bored sometime look up the history and technology behind the development of Kennametal’s KC850. It turned the entire industry on it’s head.
 
I should have added: the only acceptable mode of failure is abrasive wear. The other modes are heat related (excessive sfm) and catastrophic mechanical failure.. breakage.

Interrupted cuts often cause breakage or chipping.

Curtis, that is way out of my league. But one thing I personally do with interrupted cuts. Like on a mill when the speed gets up there. I turn off the coolant for the interrupted cuts. And then turn it on again when it gets into a constant cut. Low feed, high depth.
 
.... If you get bored sometime look up the history and technology behind the development of Kennametal’s KC850. It turned the entire industry on it’s head.

The coating or the cobalt enrichment made this work so well?
For those not in this world this is twice baked carbide which migrates a thin layer of higher than normal cobalt to the surface.
Ground tools have to be finished first and then go back into the oven. Then off to coat.
Makes for a very tough "skin" at an added making cost. Sort of a coat below the coat.
Under expired patent Kennametal was at one time the biggest innovator and truly the leader. Many "firsts". .... and then....

Interruption always bad, you live with it in milling.
Your milling tool will have say four or more tips. Four times the material removed vs one lathe tip before a change?
Most lathe tools do not like a keyway or such due to geometry and edge presentation as you are pounding on the tip at it's weakest point, milling is different and cutter designed so.
Tool life is not only metal removed , number of impacts count big even it the geometry spot on.

Take all this with a grain of salt and toss it over your shoulder or in the trashcan, it is all so hard for me to wrap my head around so I'm a poop amateur and so free to admit that.
Why is this tooling world so complicated? It seems so straight forward yet crazy land prevails.
One thou change in a hone, land or not, 2 degree change in a rake, 2% change in cobalt, mid, high or low temp coat, layers in that coat.........

A milling tool has time in air or coolant which a lathe tool does not. That presents a different heat load on the sliding chip face and tool heating. Then hits or impact on that face vs the higher running temp.
What works for you works, do not go down this rabbit hole, it has no end and you will become mad as a hatter like the member CarbideBob.
 
Plus an Endmill with a high enough helix is going to start cutting with one side while it's finishing on another. The interruption is smoothed out by the helix of the Endmill. If the Endmill had straight flutes it would be a noisy mess.

And there is size to consider. An average workpiece in a Chuck is bigger than an average Endmill, thus the Endmill is easier on the Machine itself. If you were turning a .5" square, it would not be considered "hard" on the Machine or the Tool. If you were using a 10" Shoulder Mill with One insert it would be similar to the interrupted cut we most think of on a Lathe.

R
 
It just occurred to me...


If the OP could figure out a way to do milling operations without an interrupted cut (besides the obvious choice of drilling or shaping) please let us know.


I'm envisioning a blank carbide dowel pin pushing metal around like play-doh.

Take a fly cutter, and circle the spindle around synchronized to the cutter. Done properly you will have a continuous spiral of cut.
 








 
Back
Top