trouble with mill math...

[timcki]

I can see how to use all of the formulas...
but having trouble with chip load per tooth and applying the formulas

you need that (IPT)to figure IPM inches per minute but where do you get that info

seems like you need IPM to figure IPT and you need IPT to figure IPM
I'm confused

looking at charts I see a 4 flute end mill has about .001 to .002 chip load per tooth at the smaller end mills < 1/4. Charts to me are best case scenarios. How do you figure chip load manually or is that just a given?


this is where i get lost
example: Given..
6061 aluminum
1/4 end mill
* do I pick an RPM I like? = 600


this i where I get lost
********************************
S.F.M. = 0.262 x D x R.P.M.

first figure the rpm
R.P.M. = 3.82 x S.F.M./D

3.82x165/.25=RPM
*******************************
RPM x IPT x #FL = IPM
600 x .001 x 4 = 2.4

my table crank turns .100 per revolution
10 turns = 1 inch
so at 2.4 inches per minute I have to turn the table crank 24 time in 1 minute
to = 2.4 IPM?

somebody give me a pointer please

[DFMiller]

This is how I go about it.
But I am not a trained machinist.;-)
For small end mills in alum you normal cant get enough RPM to exceed SFM.
But check that first.
Then once that is decided then figure feed.
I alway check tables but I think you can easily do 600 SFM with HS in 6061.
So that's close to 10k.
So probably max on your machine is good.
Then calculate feed off of that.
6061 is gummy so use lube. Kerosene or WD40 is good
Does this help
Dave

[macona]

Don't bother trying to remember everything. There are online calculators like this:

http://www.daycounter.com/Calculators/GCode/Feed-Rate-Calculator.phtml

As for CPT, the only time you would use something as small as .001 is with a 1/8" or smaller end mill. I usually figure .003

[macona]

This is how I go about it.
But I am not a trained machinist.;-)
For small end mills in alum you normal cant get enough RPM to exceed SFM.
But check that first.
Then once that is decided then figure feed.
I alway check tables but I think you can easily do 600 SFM with HS in 6061.
So that's close to 10k.
So probably max on your machine is good.
Then calculate feed off of that.
6061 is gummy so use lube. Kerosene or WD40 is good
Does this help
Dave

600SFM is carbide territory. 250-300 for HSS.

[philbur]

Your starting point is always surface feet per minute (SFM). This is the speed at which the cutting edge of the cutter should travel at. You don't (can’t) calculate this, it is a fixed number depending on the cutter material and the part material. You can use generic numbers that are published all over the place (for example a high speed steel (HSS) cutter on a mild steel part is normally accepted as 100 SFM) or you can use numbers published by the cutter manufacturers specifically for the cutter and part material you intend to use.

Next you select which diameter cutter you intend to use.

Now you can figure the required revolutions per minute (RPM) of the spindle. If the cutter diameter is Dc in inches. Then:

RPM = (SFM x 3.8)/Dc

Chip load is used in a completely separate calculation for calculating feed rates, which is important if you are using CNC or power feed. However if you are hand feeding the cutter then it really doesn't matter.

Chip load per tooth (inches per tooth - IPT) is published by the cutter manufacturer, you can't calculate it. If the number of flutes on the cutter is Fn and feed rate per minute is FR then:

FR = IPT x Fn x RPM

Phil

[DFMiller]

Macona,
600 SFM is what the SME MillTurnCalc app on my IPad told me they claim 1200 for uncoated Carbide. I agree it seems fast. That was the only reference available sitting in bed with the lights out. ;-)

I stand by the comment that small milling cutters on most machines can be run max RPM.

Dave

[Horst]

I don't know where some of the others have gotten their numbers but here is my method.

The SFM (surface feet per minute) is the starting point and it is given (to you).

The SFM is the speed, in feet per minute, the circumference of the tool passes by a point. You look it up in tables. What you find in tables is theoretical and is based on research. There are variables. The condition of the cutter is one variable, the rigidity of the machine and the set-up is another. In a non-production situation I use them as maximums. The SFM's I use with a HSS tool are:

Mild steel - 100 sfm (70 sfm if my cutter is less than great)
most Al. - 200 sfm

The next step is to calculate your spindle speed (RPM). This is a function of the size of the cutter. Lets use your 1/4" endmill. You first need to know the C (circumference) and that is calculated using this formula:

C = pi x D (diameter). This is a formula you should keep in your head.
C = 3.14 x .25"
C = .785"

Since you want surface FEET per minute you must divide this product by 12.

C = 0.065'

RPM = 200 / 0.065 = 3,056.

I am going to stop here because I seldom calc. chip load. I have two more things to say.

1. the numbers others have proffered are probably products of combining steps in the formulas I have given. While that might save a few keystrokes on the calculator in my opinion it is an inferior method because it replaces logic with rote memory. I think applying simple logic will serve you better in the long run. Better to remember a formula.
To those who have different methods please don't take what I say personally. I have no criticism of your methods, I simply think the makes it harder to understand the math.

2. The final arbiter on these things is your ears and hands. Listen and feel your machine. It will tell you if it is unhappy.

[3jaw]

Your math is right, you just made a little mistake in your RPM calculation.

first figure the rpm
R.P.M. = 3.82 x S.F.M./D

3.82x165/.25=RPM
*******************************
RPM x IPT x #FL = IPM
600 x .001 x 4 = 2.4

That number should be 2521 and not 600 for a 1/4 HSS end mill in aluminum with a 165 sfm cutting speed. 200 sfm is more like it so the RPM would be even higher.
You should be getting around 10 IPM with the numbers you are using.

I'm a little concerned that you are using a 4 flute end mill in aluminum. If that is the only one you have then make double sure that you keep it lubed or it will clog up in no time. A 2 flute is better for soft materials like aluminum.

[Black_Moons]

Using 4 flute endmills in aluminum is not a big deal as long as your not making a slot, and/or trying to remove massive amounts of material.
Yes, a 2 flute endmill can remove more material when sloting then a 4 flute endmill in soft materials without clogging, No, you don't have to go quite that fast!

Also, More flutes are definately benifical when doing side milling where theres nowhere for the chips to clog up, Especialy when you want a better surface finish (Effectively, More flutes = More cutting edges = less load per tooth = smoother finish at same RPM/feed rate)

[Oldbrock]

down and dirty rpm equation is RPM = cutting speed x 4 divided by diameter in inches. HSS cutting speed for Al is about 200 feet per min.
so RPM = 200 x 4 / 1/4 = 200 x 4 x 4 = 3200 rpm
Two flute end mill at .001" per tooth works out to 6.4" per min. 12.8 for a four flute. Lots of flood coolant to get rid of the chips or they recycle in the slot wrecking the finish, size and could break the cutter. 600 rpm is about 5 times too slow. Peter

[hornluv]

The rule of thumb I use for chip load is a max of 1% of the cutter diameter., so a 1/2" cutter would be a max of .005". I use the max for roughing cuts and generally cut that in half for finishing cuts. Obviously, the bigger the cutter the larger that number is, so I tend not to scale that up too much.

[whitis]

I think you are probably expecting too much from a set of simple formulas. You can't just plug in a few numbers into a few simple formulas and arrive, cookbook style, at the optimum cutting parameters (or even viable parameters) for your job. The formula are very useful but they only provide some of the information you need.

People have been trying to figure out cutting parameters for centuries. Vast quantities of metal have been reduced to chips in lab tests. Huge dissertations and countless papers have been written on just small aspects of the problem. Books have been written on cutting theory. There are a range of possible values and you have to balance some constraints (sometimes conflicting). And dealing with missing data. It isn't just a matter of plugging some numbers into formula and coming up with the right cutting parameters. There is some art as well as science. The ratio of science to art has improved over the years. But you can still easily calculate the numbers to six decimal places only to get a result that is wrong by a factor of two for your job on your machine if the underlying assumptions don't match your situation.

IPT (or feed per tooth) and IPM are two sides of the same coin. They are proportional via the number of teeth on the cutter and rpm. One of those two values needs to be an input, possibly a tentative one. I.E. I want to achieve this feed per tooth, how fast do I feed? Or, I want to feed this fast, what feed per tooth does that give me? And the result may prove unacceptable and you have to change your input value or another parameter and try again.

You have a maximum IPM that your steppers or servos or hands can deliver. If you can't move fast enough to get a reasonable chip thickness, you may need to lower your RPM to less than the surface feet per minute calculation gives you (that is an upper bound). If you move too slow, it will take forever to do the job and you will be wearing out your cutters and heating the workplace. If you move to fast, you are going to clog (and maybe even break) the flutes of your cutter. Also the depth of cut, RPM, cutter diameter, and feed per tooth are going to affect the horsepower and torque required; on small machines you may overwhelm the motor. Also the higher the depth of cut and the feed per tooth, the more deflection you have of the cutter. If you are taking a finishing cut, you use a low feed rate but no so low you get chatter and the numbers are different than if you are roughing. A light cut on a rusty surface can destroy a cutter in a few seconds - you need to dig in. In some cases, the work is held less securely and you need a lighter cut. Lubrication also affect results. Some chip thicknesses make ornery chips. You are balancing speed of getting the job done with cutter life (and cost).

Machine rigidity can be a factor; the tables you find in the books are probably based on tests done with fairly heavy duty equipment and lube flying and may not necessarily work well on a hobby machine. Collet gripping strength may be an issue. You may have to baby your machine a bit. But trying to baby too much can be bad, too; it can be especially hard on carbide cutters. How much tool or machine deflection can you tolerate before the loss of accuracy or chatter is unacceptable? 1HP of spindle power seems to translate into about 200lbs of tangential force. If you get 5mils of deflection on your roughing cut, then your 1mil finishing cut might really be 6 mils or you may have already cut away 4 mils too much material in places before the finishing pass starts depending on whether you are climb or conventional milling and your trajectory. You can measure how much deflection you get per pound of force.

The force required to actually cut the material is about the same if you are cutting a thin or thick chip but it takes more force to bend a thicker chip or a wider (depth of cut) chip or to bend it further.

Trajectory matters. If you are cutting a pocket, for example, the chip load can double when you hit the corners; a feed rate that works fine on the straight away can wreck the cutter in the corners. If you are using carbide, the geometry of the cut can make a big difference in cutter life. Is the center of the cutter inside the cut? If not, you are may be hitting the fragile edge of the cutter against the work on each revolution which will quickly destroy it; the impact on the carbide needs to be on the face of the cutting insert, not the edge. Increase the width of cut and decrease the depth to compensate if necessary. But this depends on the type of cut and whether you are climb or conventional milling.

What works on one 1/4" endmill might not on another; one might have been designed for rigidity (shallow flutes) and another for chip clearance. Besides the differences between carbide and high speed steel, flute angles, rake angles, flute width and depth, number of flutes, and surface coatings may be different.

Compare your proposed chip thickness with the depth of the flutes on your cutter. Will the chip actually fit in the flutes? Does it have room to curl up? Do you have enough horsepower to force it to do so? When it does curl up, will it travel up the flute fast enough (consider flute spiral angle) that it doesn't overlap with itself (depth of cut)? And if it is two thin, it may bunch up and clog instead of curling up the flute properly. And the situation is different depending on whether you are profiling, pocketing, or cutting a slot. And bear in mind that your chip thickness isn't actually the same as your feed per tooth; rake angle affects how much thicker your chip is. There is a formula here: http://www.fordtool.net/pdf/209.pdf
If you are doing it by hand, rather than CNC, you can adjust the feed by feel. Your eyes, ears, and hands can tell you a lot about what is going on.

Experience as well as data on the cutter and the material will give you an idea what ranges of feed per tooth, depth of cut, and chip cross sectional area are within reason. Over at cnccookbook.com, there is a program called g-wizard ($69/year on sale for $55) that has some of that info built in. Read the blog there and you will see some of the considerations that went into it. The author posts on this forum as bobwarfield.

Machinery's handbook has some tables of recommended feed per tooth. The values are probably wrong for your machine, but they are a starting point.

kennametal has some online calculators that are handy for playing with the numbers.

Keep a logbook of what cutting parameters you used for what kinds of cuts in what material with which cutter and what the results were. Use your formulas to calculate some of the derived values such as feed per tooth, chip cross sectional area, horsepower, etc. for future comparison. You won't see all the patterns if you don't log all the numbers.

[MaxxLagg]

People have given you all the info you need but I can't remember the last I actually took the time to calculate speeds and feeds. I realize that this is primarily a HSM forum and many are working with marginally sized machines and questionable quality cutters just due to costs involved. I work in a manufacturing environment and lot sizes are small or one-off and making money by cheating cycle time isn't something I have to worry about. IMO, the best calculator is experience and a practiced ear. Knowing the limits of your machines and knowing the machining characteristics of whatever material you're working with is more important than whatever numbers you spit out by calculation. The sound of the machine process, appearance of the stock/chips, and just the general feel of the machine as it machines is how I gauge speeds and feeds. All this comes from years of observation and experience.


Edit********* Yeah, what Whitis said, he beat me to it.

[timcki]

Whitis and everybody

Whitis,
Thank you for your insight... I was getting frustrated with not being able to make a "pretty" cut. I was looking for a magic number to plug into the machine
and have the part come out perfect, shiny deburred and maybe anodized too...
I forgot that trial and error and learning along the way is what learning is all about. Experience IS the best teacher. I knew that but was frustrated.
You have put it all back into perspective.
Learning the math will be a great starting point for me to try "Making chips" on the mill/drill.

Everybody else, thank you for your help... I now have a better understanding with the math.. I was using my ear to know when I did something wrong, now I will be using it to know when I do something right..

Tim