View Full Version : how are speeds & speeds derived?

dan s
12-27-2008, 01:39 AM
While I was doing research to make my speeds & feeds charts, all the data I found was supposedly found by trial and error testing.

Has no one developed a theoretical method?

12-27-2008, 01:48 AM
Its based on a formula. Both are dependent on material the cutter is made from and the material being cut. Then there is the geometry of the cutter itself which plays a hugh role in the parameters of the cutter. For the non standard cutters like indexable carbide and variable flute or variable helix end mills you really have to start with manufacturers rated feeds and speeds and go from there.

Also your machine will have a lot to do with it as well. Rigidity and max HP will determine if your machine can push a cutter to anywhere near its theoretical maximums.

Feeds and speeds are just a recommended starting point. You have to use your own judgment to see how a cutter is cutting on your machine to know how to proceed from there. Sound, vibration, and the chips themselves will help you find a feed and speed that your machine will be happy with.

Your Old Dog
12-27-2008, 08:13 AM
I do it the way Macona suggest in his last paragraph. I have refined the method abit. I place a beer bottle on top the mill when I'm cutting. If the bottle starts to rattle I know I"m working the machine too hard. If the bottle falls off the mill I know I'm climb milling by mistake :D

I do listen to my equipment for signs of strain, slowing down of the motor and vibration. If I'm cutting aluminum I just go balls to the wall with the mill until I get alot of smoke, stop and clean off the welded on aluminum to the cutter, and then go a little slower. It works for me.

dan s
12-27-2008, 11:01 AM

I know the speeds and feeds are just a starting point; I'm just shocked at how rough the starting points are.

The equations that I have seen referenced a lot is the one Taylor came up with back in 1907. From what I have read, all Taylor's equation lets you do is take a known tool material, work material, and tool life, and extrapolate to find a different tool life.

I have seen other models that take a few more parameters , but basically work the same way. That is to say you use known values and extrapolate.

I just find it odd that the modern professional machinist is still playing a trial and error guessing game (educated guesses, but still guesses).

12-27-2008, 12:16 PM
I just find it odd that the modern professional machinist is still playing a trial and error guessing game (educated guesses, but still guesses).

I don't find it odd at all, its one of those deals where there are just too many variables. Its not just cutter material A and workpiece B and a tool life time.

You have cutter geometries, which can get insanely complex.

You have heat distribution, into the cutter, the part and the material, which can be effected by the geometry, cutter material, workpiece material and thickness of the part being cut. Add coolant into the mix and you are at the mercy of pressure to remove steam pockets and the ability of the coolant nozzles to get the coolant where it is needed, don't forget the high pressure additives(concentration), and don't forget the heat distribution properties of the coolant, which can be completely screwed up by improper mixing or tramp oils, (which can screw up your cutter to workpiece interface, which can throw everything out of whack).

Now add in the machine rigidity and natural and or induced frequencies(NOT a small part of the equation).

Also the many different depths of cut and chip loads and I think the best you can hope for is a ballpark. Nevermind coatings or variations from manufacturer to manufacturer on the base material of the cutters.

Even if you could create a reliable model, a lot of the data going into it is going to be trial and error, which is then going to be superceded next week by the new latest and greatest.

Liger Zero
12-27-2008, 12:44 PM
So in other words, crank it until it blows up then back off a quarter turn and run it at that setting?


12-27-2008, 02:14 PM
dan, machining is not an exact science. As stated, there are to many varaibles to have an exact perfect formula to do things with. If you are going to be a machinist you have to get rid of the engineer/scientist attitude and start machining stuff. You have to learn to machine by the seat of your pants and common sense. All the books you can find to read about machine work is just a start point to really learn how to do it.

You can read and formulate for 50 years but untill you actually put your hands on a machine and start working you really know nothing about machine work.

My suggestion is put your books and formulas away and start doing some work. In short time you will know very close what you can run cutters at and even then it will vary for every job.

Your a perfectionist aren't you? Perhaps an engineer or a doctor or professor?

Speeds and feeds are derived by doing.

EDIT: Ok, found your web site, so your a perfectionist techy.

12-27-2008, 05:09 PM
Your a perfectionist aren't you? Perhaps an engineer or a doctor or professor?

It's not like we can help it Carl -- we're born that way :p

Speeds and feeds are derived by doing.

The physics of metalworking is an exact science, which is why books like Cincinnati's "A Treatise on Milling and Milling Machines", Moltrecht's Machine Shop Practice, Brown and Sharpe's, ... have several chapters on "the calculus of speeds and feeds" (including Taylor's equation), the physics and metallurgy of chip formation, chip thickness, up- and down-milling, resulting surface finish,...

That said, a pro machinist who has spent his whole life in the shop can dial-in a machine by sound/feel, but 9 times out of 10 he ends up with the speeds and feeds that are damn close to the tables in the various machinery texts (which you've probably noticed all agree with each other).

So when an amateur or part-time machinist, who hasn't had a lifetime of experience to learn the correct speeds and feeds, steps up to the machine, he can either d!ck around with it and hope to stumble into the correct speeds and feeds, or he can look up the "optimal" speeds and feeds from Machinery's Handbook, or here (http://www.hougen.com/tech_tips/speeds/speed.html), and at least have a reasonable starting point.

If you look at the speeds/feeds tables you'll notice that it has recommendations for HSS, plain carbide, and coated carbide, with the coated carbide speeds and feeds close to 100% higher than HSS. I've found that the HSS speeds and feeds recommendations work extremely well with the power/rigidity of metalworking machines found in the typical home shop.

12-27-2008, 05:53 PM
I started out as a semi perfectionist but when I had to make a living with what I had learned I found that I didn't have time for perfection and the employers or customers didn't want to pay for it. They wanted it RIGHT and as fast as posible without mistakes.

My perfectionist attitude fell in the dirt and never got up. I had to make a living and please the boss and customers.

Machining is NOT a exact science no matter what many may think. It is exact in what you have to remove to make the part but removing the waste is not an exact science. Perhaps the designing of what you will build is and exact science, but making it is not.

To take a perfect design and make it into a working product requires a lot of give and take and the final design is seldom like the original drawings. I and others have seen engineers draw a series of parts that would fit together with such close tolerances that the various parts can't be assembled. The parts had to be remachined with WORKING tolerances. Perfection was a mistake.

The last shop I worked at did some prototype work for UofL Speed engineering school. Talk about designs that won't work, we got them.

Speed and feed charts are just as many have stated, a guide to start with. Yes, I used them too and many times I just asked my favorite mentor where to start. I really don't mind a person being a perfectionist and they can if they are working in their shop on their stuff. I just hate to see someone reinventing the wheel and that is what dan is doing.

12-27-2008, 06:01 PM
Machining is NOT a exact science no matter what many may think. It is exact in what you have to remove to make the part but removing the waste is not an exact science.

Agree completely. But Dan is asking about how to generate a speeds and feeds table, which is exact part. Making your part after you get the speeds and feeds right (or at least, reasonable or close) is the art.

Speed and feed charts are just as many have stated, a guide to start with.

Speeds and feeds calculators/tables are optimized to remove the maximum amount of material in the minimum amount of time. In the case of Taylor's equations, it's how many cubic inches of material you can remove in unit time (20 minutes is typical).

Taylor's basic equations don't account for power or rigidity, but modern speeds/feeds calculators, like the one I posted, do: K is the equivalent horsepower of the machine (horsepower to the spindle after pulley losses), and there's a parameter for rigidity as well.

I just hate to see someone reinventing the wheel and that is what dan is doing.

He's trying to make a chart like this, which I have done with Excel, and I find is immensely useful:


J Tiers
12-27-2008, 06:15 PM
The main problem with speeds and feeds isn't finding the optimum, it is understanding why that does not apply to you.

usually it is quoted for optimum tool life, maximum production of parts, and hitting consistent dimensional performance, so SPC will work decently, etc. All very nice things, but way far removed from the HSM. Not to mention that they tend to interact, and optimum for one characteristic may be bad for another.

So, for the HSM, it is often best to take the quoted numbers, and as a standard practice, take 80% or 90% of the number given. Burns up fewer tools, and still gets the job done just fine.

Remember, industry regards cutters as disposable, they just have to cut much more than their cost to be a good life. You may not have extra loaded holders to slap in, etc, and prefer to get better tool life instead of absolute maximum production per dollar.

dan s
12-27-2008, 06:32 PM
Your a perfectionist aren't you? Perhaps an engineer or a doctor or professor?
B.S. in physics, Software developer by trade.

I know that their are two many variables to get you to home plate, but it's 2008 (soon 2009) and it would be nice to get to the infield, instead of just in the ballpark.

The HSS doc/feed correction factors from the machinist handbook are presented poorly, but are actually a nice mathematical curve. I plotted the discrete points listed in the machinest handbook, and then curve fitted them.

The correlation coefficent is .998 (1 is perfect)
http://img135.imageshack.us/img135/3350/89619157jq5.jpg (http://imageshack.us)

The carbide correction factors... FUBAR


Have you seen any good models for milling tools, or for any type of carbide tools for that matter.?

dan s
12-27-2008, 06:37 PM
Any chance I can get my hand on that notebook? :D

He's trying to make a chart like this, which I have done with Excel, and I find is immensely useful:


12-27-2008, 08:14 PM
I was just reading a book on dynamic behavior of materials(Same place I came up with the comment about explosive hardening of Manganese steel).

It talks about machining processes inducing failure of the material (that is cutting it with a cutter and making chips) by a process called adiabatic shear banding. It said that bringing the material to the conditions where adiabatic shear banding occurred tended to correlate with what we would see as a nice machined finish.

ASB is a process where material impinged by a shock wave is compressed so quickly that it locally heats to a large fraction of its melting point (on a time scale that thermal conductivity cannot equalize the temperatures). This heating and pressure reduces the shear strength of the material locally allowing the material to be cut by a much lower force than would otherwise be required .

The hard core nerds who make things like armor have done a lot of computer modeling on adiabatic shear banding. This leads me to believe that with enough really painful theory, one could actually simulate the cutting process with Computational Fluid Dynamics and determine optimal values from first principles and materials properties.

I suspect that some of the makers of cutting tools do this kind of simulation already but some of it's pretty fierce math and out of my inclination and current capability. It may be possible that we could come up with some kind of simple equation for the situation that would cause adiabatic shear banding in the material and try to match speeds and feeds to it.

That being said, I'd bet the topic would make a great PhD thesis for a CFD guy.

12-27-2008, 08:36 PM
I understand what you and dan s are saying lazlo but I see no reason to make a new version of the old charts that work just fine as a starting point. It's not likely you will ever generate a chart with which you can set an exact rpm and feed rate and get a near perfect result when you cut metal. Perhaps with a CNC but only perhaps because of all the other variables that still exist.

I agree with J Tiers, in that the user of the cutter for his/her purposes and expectations of said cutter will be relevant to the speed/feed that should be used. With that said, there is no way a new chart could be any better than a chart from perhaps the 1950's. A chart of 100 years ago may not be relevant to modern tool steels and carbide etc.

That is why I still believe that anyone who creats a NEW chart is just reinventing the wheel and the new chart is still relevent to the old wheel and no better.

12-27-2008, 09:01 PM
I have a feeling a lot of feeds and speeds have been determined empirically. Vary both, graph tool life. Throw out any results with unacceptable finish.

Nose radius will throw out some feeds based on finish so you don't even need to go there in testing.


john hobdeclipe
12-27-2008, 09:14 PM
Umm, I use a Ouija board.

12-27-2008, 09:38 PM
I think the Ouija board and the CFD solution probably give similar results.

12-27-2008, 10:29 PM
A lot of this is "flying by the seat of your pants" stuff. It is more an art than a science. You just have to change parameters and settings until you hit the "sweet spot".

Welding and forging/Blacksmithing are good examples of a pure manual art. They get stuff "set" as near as experience or books or settings allow and then they get going making changes as necessary instantaneously and instinctively, quite often without conscious awareness of it - but it turns out right.

It is quite possible that of six different machinists on substantially the same machine and job each will set it up and run it differently to get substantially the same result in the same time.

A lot of formulae are in fact mathematical expressions "made to fit" plotted or recorded data. It is an empirical process. Perhaps it is best illustrated with the very well proved "Least Squares" theorem and "curve-fitting" and their application/s:


Having a good "Engineering" or "Science" and "wanting to know if/so/why/not" attitude and being able to look "through" rather than "at" a situation or a set of plots or tables can be very informative and rewarding in the shop.

Many but not all "Engineers" and "Scientists" "have it" - but a formal education while of great benefit is not always necessary as many have an "instinct" for this sort of thing. Machinists are just the same - some "have it" instinctively, some have to "work at it" to "get it" to varying degrees and some seem to never or rarely "get it".

Your machine and set up will soon "let you know" - just be aware and take notice and act accordingly.

I used to keep notes (still do - though as much) of my "stick", MIG, plasma and oxy-acet settings etc, but rarely have to now as I just "know" the settings or ranges etc. that I can work with or at least get started in.

Its a bit like driving a vehicle in many ways.

But that said, I do check speeds and feeds from tables etc. I use my "Machinery's Hand-book" a lot too as they are not just sets of tables and reference material but are just as much tools as anything else that is needed to get the job done.

If I do have to make a change I like to know both why it was necessary and why the "new" method/setting is better.

I have no problems with machine spindle speeds as they are set pretty well. I don't have a variable spindle speed device other than on my "Sieg" X3 mill - but even then I don't always go by "tables" but just look at the setting as I just go by "sight and sound" initially and vary it until it "sounds sweet/right". I do the same with the "X" power-feed on my HF-45 vertical square-column dove-tail mill.

I don't have a power feed on my lathe saddle or cross-slide feeds and I don't miss them. I decided on my lathes on a "features" basis with a "weighting" applied to each and I got pretty well what I wanted for the price at the time. I could do better now - but that's life and I am satisfied with my "lot".

It is most important that tables and books (new and old) be tools be used as a means to an end and not the/an end in themselves.

It is equally important that they be used sensibly as a support and not as a crutch.

loose nut
12-28-2008, 11:21 AM
A lot of this is "flying by the seat of your pants" stuff. It is more an art than a science. You just have to change parameters and settings until you hit the "sweet spot".

Tifie's got about 99% of it right there.

Every situation is diferent,
Know your lathe, mill etc.
Know your tooling
adjust to the material your cutting.

12-28-2008, 12:23 PM
Every situation is diferent,
Know your lathe, mill etc.
Know your tooling
adjust to the material your cutting.

That's great if you're a pro machinist, and can do that, but most people can't. Which is why you see videos of guys spinning a 3" facemill at 1500 RPM on their Bridgeports :rolleyes:

I thought it was fascinating when Cameron was having trouble drilling A2, that Lane (a professional tool and die maker) recommended the speeds and feeds within 10% of Machinery Handbook's table, and I know damn well Lane's never looked at a speed/feed table :)

This reminds me of the thread about welding cast iron, and a couple of guys were saying that welding classes were useless -- "it's an art, not science, you just have to get in there and do it." Then Torker, who's got more welding certs than I knew existed, pointed out that most of the welds in the HSM articles were bubblegum welds, and that those folks could really do to take a class.

I think speeds/feeds tables are like knurling -- you're either the type that just mashes the knurl until it starts tracking correctly, or you're the type that calculates the pitch diameter of the knurl wheel so it tracks the first time. So you can knurl by pure art, or pure science, but you still end up with a knurl :)

12-28-2008, 02:37 PM
Lazlo, it's interesting you equate HSM types to professional machinists in that sense. I also suspect that Lane has used speed/feed charts at some time in his career.

I have seen machinists do things that a HSM'er would never or could never do. Why, because they had to do something to get the job done. If you use the speed/feed chart to establish a start point you can increase that by a lot more if you use a mister on the tool/work. A flood coolant can't always sustain that speed/feed. However, that is not a law and is subject to circumstances.

As to a knurl, if you have to put a knurl on a diameter that don't accept the knurl well, then are you going to tell the boss it can't be done when Joe has been doing it for years. Guess what he will tell you, and the last part may be don't let the door hit you in the butt on the way out.

For the HSM'er, if he would just try the method suggested by the man that is doing it for a living he may find, well I'll be, it worked. Then he don't have to redesign what he is making for the knurled part not working.

If you constantly live in the world of theory and calculation you will be missing a lot of things that can be done if you really want to or have to. That's not to say it don't have a place in the machining process, but you can't base your machining operation on just charts or books, they are refferences and they don't always work.

I think you and dan s make programs you sell to HSM'ers and I can understand your reluctance to accept that machining is an on the job learning experience. If you control your fears and experiment when doing something you will learn more than from a book or program. The reason is, "nothing is written in stone in machining".

In fact an HSM'er has more time to experiment and learn than a person doing it for a living so why should they limit themselves to set procedures. When I was working for a living and got a job we hadn't done before I may ask someone knowlegable or just jump into it. In the end, it had to be done and it was given to me. Sometimes I sure would have liked to spend some time working out the "perfect way" but I didn't have time. Now at home in my shop if I get something complicated in a project I may spend hours working out a process and in the process end up with a "near" perfect job. That's something I could not afford when I was working for a living and it's more fun now.

So I say, read books, collect books, use the charts, BUT, get on the floor and MAKE the machine do what you want it to do. Where there is a will, there is a way but you have to WANT to do it real bad for it to work.

12-28-2008, 04:25 PM
In response to Carld, I'd say there are two kinds of "theory" involved with machining.

One is the accumulated practice which has been codified into tomes like Machinery's handbook over the last 200 years of work in machining. It's isn't theory at all really but it is accepted as such. It is data applicable to the exact situation in which the data was collected.

The other kind, real theory, comes first principles analysis which demonstrates some kind of physical law which is always adhered to. One example of this is Benjamin's Thompson's work in 1798 demonstrating that the amount of heat created boring cannon barrels could boil water. Later Sadi Carnot discovered that the amount of mechanical work done is less than the energy used to do it.

The problem is that "theories" of the first type are not generally applicable, only specifically applicable to the problem at hand, and that true theories of the second type are generally too complicated to deal with topics as complex as machining.

What we have when we machine is an attempt to reconcile the first type of "theory" with the second type of theory using knowledge of the problem at hand gained in situ: No theory of the first kind is likely applicable to whatever it is we're doing, and no theory of the second kind gives better than general guidelines of what might not work. We thus are left to our own devices to develop the art required to bridge the gap.

As computers and understanding improve, we might eventually be able to apply theories of the second type to the point of generating "theories" of the first type for all possible cases but until then, we are left with metal that needs to be cut and intuition.

loose nut
12-28-2008, 04:56 PM
That's great if you're a pro machinist, and can do that, but most people can't. Which is why you see videos of guys spinning a 3" facemill at 1500 RPM on their Bridgeports :rolleyes:

I'm only an amateur which is why I have adopted this way of doing machining.

I started out using the tables from Machinery handbook and still do but if I did everything that way, which was really set up for pro's working on heavy shop equipment I would probably destroy my lathe and mill in short order.

A lot of us HSM'er don't have the equipment to make proper use of the speeds and feeds so we adapt and thats the "art" of it. You need to know the capability of your equipment which you get with use, what tools IE: HSS ,carbide etc. works best with it and the material your turning (frequently it's unknoweum), so you do a little trial and error machining.

This may not cut it in the "pro" world because time is money, so you use the tables provided and have the equipment to meant for the job, well maybe.

The F and S tables are only a guideline not a law

oil mac
12-28-2008, 05:54 PM
The following was my experience, For home workshop practice, i found early on , by trial and error, that what seemed comfortable for the machine to handle, and my hard won tooling was not getting machined away by the workpiece, was for me correct practice and for home shop duties still holds true, If on the past occasions i have carried out some machine work as a paid task, it was different, Time was of the essence, as it is money gained or lost
For the proffessional jobbing shop, the guys are trying to beat the competition and we find exquisite tooling & more powerfull machines than the wee guy in his basement
More years ago than i care to remember, my first old belt driven lathe was dragged home, I hadnt a clue then as to feeds & speeds, One old foreman turner i knew, showed me how the speeds of my lathe headstock were exterpolated, using a calculation which gave a geometrical progression on speeds, from the lowest speed to the highest speed, both in open & in back gearing, Giving the correct speeds for the range of work, the machine will do.
This was the first ever scientific speed calculation system devised, This was at the turn of the century, and was the invention of Mr P.V.Vernon, the technical director of Alfred Herbert & co of Coventry England, and was first given to the West of Scotland Foremen Engineers
Society in Glasgow Scotland
However back to Dans problem, from my own perspective, if i dont have chatter to set my teeth on edge, the material is machining sweetly, the surface finish is good, & last but not least accuracy iis maintained and i am producing my workpiece in a reasonable time, i am pleased with my results
Its all down to experience hard won-- Good luck Dan.

12-28-2008, 06:29 PM
Sorry you all but I cant tell you any thing about feeds and speeds. I just do not know them.I could never figure out how to read the charts. If the machine had a RPM chart are gage that would help but most of them had no way of knowing what the inches per minute was on the feed. I learned to watch the vibrations in the machine watch the cutter and the color of the chips.And to listen to the machine.
Their should be no unusual noise when cutting.
You should not be getting blue chips.
You are not cutting wood are plastic slow it down.
Learn to feel the machine cut.
Small machines will let you know real fast if you are doing it wrong, Large heavy machines will not. I very seldom run a lathe faster than 900 RPM and a mill faster than 1500. Most of my milling is between 500 and 1000 RPM Max feed May be 2 on the Servo feed dial. 3/4 end mill between 375 and 425 RPM .1/8 end mill may be 1500RPM. Right wrong are other wise it works for me.
What I see most beginners are doing wrong is trying to run too fast .
and I have seen plenty. Most self taught run way to fast and wonder why their cutters want hold up.
What I tell people is start slow and speed up If you start fast you will more than likely burn cutter up before you can slow down.

Laslo right . If I can see what you are doing I can tell you what you doing wrong But I sure cant tell you what feed and speed to run are how to read the chart.

12-28-2008, 08:25 PM
my opnion is its all trail and error know one knows right off the top whats right or wronge. its what works or does not work for them so they give you this info based on there own experience and make a book give it a name and make millions.

there is no magic numbers of this is the exact speed or feed for this or that, but based on some one elses ideas and expereience is how we have an idea what we can and can not do what the fail to mention is the duty rate of the machine they did this on so tehy dont own every lathe andmill and drill out there so if oyu try there speeds and feeds on a lighter machine then you have to slow things down alot if you have a heavey duty machine, then you gota good chance so was theirs when they wrote their book ..

if your still woronge then slow it down more till you gota it right for the equipment and metal your munching into and so on ,,

12-28-2008, 08:38 PM
I figured out the ins and outs of feeds and speeds within the first few hours of using milling machines or lathes ..

There is a lot of feedback that comes back to the person using the milling machine or lathe

Sound of the cutting...sound of the motor ..vibration .......colour of chips.......heat.......finish left on the work.

if someone cant use their senses to detect the above after a few hours .....then they may as well not bother entering the hobby .

cnc machines are a different ball game.

all the best.markj

12-28-2008, 09:56 PM
In 1974 I bought my first machine . a ten inch Atlas lathe with every thing made for it . got it home set it up. Picked up some scrap material at work brought home and tried to machine on it. Was going to make a bolt for lack of any thing else. After a few tries I gave up . Thought I had bought a piece of junk. I had never seen a lathe that small and did not know machines were made that small. I had been working for about 7 years in the trade by then. I kept fooling with the lathe but no luck. Then one evening it hit me like a ton of bricks. I was used to running large industrial machines lots of iron. Just about any thing would work on them so big they could not do any thing but cut.
This lathe was little. So I dug out an old text book I had from trade school looked up how to grind a bit just right. Slowed down the lathe and started cutting worked good . Then since I was just making chips I started speeding up and down to see how things worked and played around with the feed leavers. Doing this I found out what the machine was capable of . I would berry the tool 1/4 to the side go to back gear and change feed rate and see what would happen . I found I could cut 1/4 to the side in CRS if I took it easy It might take 20 minutes to travel 2 inches but it cut and cut good finish.
The trick is to remember what works when and why. so next time you can do it.
When my buddy Monty are Bill watch me make something they just cant believe the machine will do that and we all have basically the same machines. The difference is they are self taught and have never seen it done.
I`m the same way with this computer about like a 7 year old. I can point the mouse and click ,but that is about it . Move a file are folder I have know idea. I try to teach them machining and they help me compute.
Like said earlier in this post you need to play with your machines and find out just what they will and will no do.

dan s
12-28-2008, 11:54 PM

The point of my original post, was to find out how (“in general”) the feed and speed charts are derived. As I stated earlier, the HSS turning speed & feed data from the machinery handbook is excellent. The feed & doc correction factors are so good that they can easily be curve fitted by a simple power curve. They are so good in fact, that I guarantee they were pulled from a power curve and then rounded to 2 decimal places.

I can easily take the HSS SFPM provided in the handbook and correct it, so that I can run my machine all out. Put another way, I don’t have to spend time playing with different sfpm/doc/feed combinations to find what works on my lathe. I can (within reason) just look them up, and get on with the project.

The carbide correction factors on the other hand are a complete waste of time. Does anyone know how they where derived?

12-29-2008, 08:58 AM
Take a look at Moltrecht's Machine Shop Practice. Good info there on cutting theory, and DOC/Feed/Speed/Tool life/Power/Rigidity relationships.

These charts were derived, or refined under controlled experimental conditions by smart guys working for big companies that wanted to optimize production costs. The work has been done, gozillions of dollars have been spent, just a matter of finding it and putting the results in a form you can utilize.

Carbide tends to show some non linear results due to issues of critical speed and built up edge. Carbide grade and insert geometry add to the confusion.

Some of these guys act like it's unmanly to use a chart. I contend that minute or so per job I spend looking at a chart or mentally running SFPM and tooth load is my most profitable time in the shop. I can do the math faster and cheaper than I can change a smoked insert or endmill.