[cncadmin]

When do I use a 2 flute end mill verses using a 3 flute end mill. I'm milling steel and alum.

[HuFlungDung]

Whenever you want!

Typically a 2 flute is ground with end clearance and a center cutting gash is made so it will drill a hole if required. Drill, then mill.

Some 3 and 4 flute cutters are also ground as "center cutting" but if not, then you cannot drill into the work with them.

Any cutter that is not ground for "center cutting", you can ramp into the cut at a shallow rate of Z descent, but that may require simultaneous 3d interpolation that your mill might not have available. But, you can start milling from an existing opening with these.

So it boils down to the surface finish that you want. The more flutes you have, the finer the effective feed per tooth. The 2 flute cutter has typically about the same feed rate capacity as a three or 4 flute, but has larger flutes, and can handle a larger chip, perhaps with less tendency to plug up in soft materials.

[E-Stop]

Using an odd number of flutes (3 flute, 5 flute, ect) also helps break up harmonics. You'll get less chatter than with a 2 or 4 flute mill. There are some exceptions, like SGS Z-Carb mills. These are 4 flute mills that have the flutes spaced unevenly so that you get varying chip load.

[cncadmin]

Thanks for the info.What about carbide or high speed steel, what is their application ?

[HuFlungDung]

High speed steel tools have a pretty good tool life in aluminum, but of course carbide is better. Carbide will hold accurate size for a longer period.

There is a special high helix flute design for milling aluminum, and this works much better than a standard helix. It is easier to find this high helix flute in HSS, than carbide.

In steel, you pretty well need flood coolant to use HSS cutters, whereas carbide often doesn't stand up well to the rapid heating and cooling cycles, should coolant flow be impeded temporarily for any reason. Carbide is often used dry, with an air blast (or lubricated air blast). It is important to not recut the chips, and flood coolant will often not move the chips out of the cut zone as good as an air blast will. By air blast, I don't mean a wide open 1/4 inch air hose, a small nozzle will do if properly directed.

It is pretty important to have the proper feed rate available for carbide, too. Beginners tend to overspeed and underfeed their cutters. Better to take cuts that are not all that deep, but at a high feed rate with carbide, depending on what your machine can handle.

That's my 2 cents

[cncadmin]

Great info, it's my first vertical mill, I know more about wood cutting. Now I'm trying my hand at metal work. Can't wait to get the mill converted to CNC.

[Paul_S]

Ether a 2 or 3 flute end mill can be used in aluminum. Steel it would be better to use the 3 flute.

It is important to know what surface speed you are going to use with the cutter. This is dependant on the material being cut and the material of the cutter.

Aluminm using a High Speed Steel (HSS) end mill will use typically a surface feet per minute (SFPM) from about 400 to 800. This is used to calculate your spindle revolutions per minute (RPM.)

Carbide cutters in aluminum would use 800 and up SFPM.

Steel will depend on a number of factors. Type of steel, and hardness. For an example: 303 CRES (corrosion resistant steel) using a HSS end mill, typically 70-110 SFPM. Carbide end mill would be 110-225 SFPM.

Surface feet per minute affects tool life the most. So use the lower end for rough cuts and the higher end for finishing.

Your feed rate is dependant on inches per flute of your end mill. And chip size if it is ether too small or too large will also reduce your tool life, second to spindle speed.

There are tables for material and end mill type of inches per flute and chip size or chip load.

And easy way to estimate chip load is to use an index value. For example: .010 per flute for a 1 inch dia two flue end mill in aluminum. .003-.004 per flute for a 1 inch dia 3 flute end mill in a steel.

So if we use a 1/2 cutter in steel. .003 x .5 = .0015. And using 70 surface feet per minute. The RPM = 12 x SFPM / (PI x dia) so given 70 SFPM the RPM calculates to about 535 RPM. The feed wil be in IPM = RPM x number of flutes x IPT, so given 535 RPM and 3 flutes at .0015 per flute the IPM calculates to 2.4 inches per minute.

For cuts less than the full width of the cuter increase the roughing feed IPM x square root (tool dia / width of cut)

It is generally recommended, not to exceed 60% or 75% the width of the cutter. So say, 60% width to cutter dia, the 2.4 IPM calculation is corrected to 3.1 IPM (3.09 = 2.4 * sqrt( .5 / .3) )

The faster you can remove the materal the better. But not too fast. Calculate your cubic inches per minute. CIPM = width x depth x IPM.

1. typically in steel, your width of cut and depth of cut should not be more than dia of the cutter squared (dia x dia.)

2. Know the horse power (hp) limits of your spindle of your machine tool. The material will have a CIPM/hp rating. Or sometimes given as unit hp/CIPM.

Aluminum is typical from 2.5 - 6 CIPM/hp or .4 to .17 unit hp.

303 is .7 for CIPM/hp or 1.4 unit hp.

You need to check your calculated CIPM divided by CIPM/ph (or times the material unit hp) to find the hp requirment. It should be less than what is available at the spindle at a given RPM.
This so not to overload your spindle and cause tool breakage and worse yet, machine damage.

Finishing feed rates would be done faster. And depending on whether the finish cut is an end cut or a peripheral side cut. And a finish feed rate is what will give you the required finish.

And end cut will typically be slower by 1/4 to 1/5 feed to a peripheral cut. A 32 roughness average finish will be 50% the feed of a 125 roughness averge finish for a peripheral cut or a end cut with a ground radii. Otherwise 32 roughness average will be 25% the 125 roughness averge (Ra.)

To calcalute a 125 Ra finish use an index of .0405 * square root of the dia. And the feed is NOT per flute but by inches per revolution for peripheral finish cuts. So at 535 RPM using a 1/2 dia cutter feed for a 125 Ra finish calculates to 5.3 IPM (inches per minute.)

For 125 Ra finish the index value of .0405 x sqr(tool dia) * RPM
For 63 Ra finish the index value of .0287 x sqr(tool dia) * RPM
For 32 Ra finish the index vaule of .0205 x sqr(tool dia) * RPM

To correct for a RMS (root mean square) finishes:

For 125 RMS finish the index value of .0382 x sqr(tool dia) * RPM
For 63 RMS finish the index value of .0271 x sqr(tool dia) * RPM
For 32 RMS finish the index vaule of .0193 x sqr(tool dia) * RPM

RPM = SFPM * 3.82 / tool dia inches
SFPM = RPM * tool dia / 3.82
IPM = IPT * number of flutes * RPM
IPT = index chip load * tool dia * sqr( tool dia / cut width)
cut width =< tool dia

[tauscnc]

wow, thanks guys for the info. A question I have asked many times to myself

tauseef
www.cuttingedgecnc.com

[Jaws]

http://www.cuttingedgecnc.com/

Dead link!

[tauscnc]

Hey Jaws,

Sorry about the link not working right now. IT'S NOT DEAD, I am just over my bandwidth and plan to change servers in the next month or so. I never thought I would of hit it but am more often now.

The site will be back up at the beginning of the next month so if you would like to check back then it should be working.

thanks
tauseef
www.cuttingedgecnc.com

[camminc]

Generally the number of flutes you use depends upon the chip that is produced by the material being cut, for chip clearance. More teeth the better as far as feedrate for a given RPM. This is the first line of defense in determination of how many flutes to use.

Secondly, it does not matter how many flutes you use to interrupt harmonics that cause chatter, it is the timing of the flutes which will determine it. Although, when you change the number of flutes, you also change the calculation of dynamics, which a formula is given below and this number of flutes could fit into the proper RPM’s of the operation for one to further maximize that operation. But is only by chance that it happens and it certainly does not maximize the operation.

When standard cutters are made they are indexed in a standard set non-variable, such as: A 2 flute cutter will be timed to have 180 degree per flute of index, a 4 flute will be every 90 degree, etc. The trick is to offset these flutes either plus or minus to break up the harmonic effects. One flute + 5 degree, one flute minus 5 degree, example. This will tend to breakup any harmonics of the operation, but it will only maximize the machining operation if it is in a proper RPM, of the natural frequency of the cutter assembly. It might help at your current RPM but will not reach full potential of that cutting operation unless you run the proper RPM which can be calculated by knowing the Natural Frequency of the cutter assembly. Formula: Natural Frequency * 60 / number of teeth.

Three flute cutters work nice because they still give you a deep gullet for chip clearance and are tough on the secondary side (Back side of the cutter) because they have a sufficient amount of material to be strong upon the flute, a 5 flute leaves you with less chip clearance and weakened flutes on the back side, causing breakage.

To learn more about this subject please see MoldMaking Technology Magazine in April – Chatter Myths. Although this article does not refer to number of teeth and timing of it, it will give you the basic outlook of chatter and what it is and how to eliminate it. I will add the Myth of 3 and 5 flute cutters break up harmonics in a later article, seems it is another Myth to be reckoned with.

[Stevie]

One other thing even good machinest will sometimes forget over the years; only cut Keyways with 2 flutes; this will maintain size better; 4 flutes tend to cut big

Another really good cutter to look into if you have big amounts to remove is a ripper rougher; these babies have the edges ground to a pattern to cut small semi circles one staggered after the other on all the flutes; it looks like a screwthread when spinning; there are several types; rough cut semi rough and finish rough; if finish is not an issue use the full rougher; this will cut 150% it's diameter easy; I've even gone more and had good luck; I regularly cut 516-70 plate with a 3/4" cutter and take 1 1/4" deep; I use 355rpm and a high feed rate (can't remember the feed i use; I just know what the dial is set to; numbers rubbed off years ago) if you start in a hole; make sure the first 1/2" you blow the chips out or the flutes will clog up and the cutter will explode; run plenty of coolant and just watch these things eat steel; I'm using a combo machine (fully manual; and the name has been gone for years too) vertical head on a slide with a side cut head in the back support (they are made in Poland; kind of a toolroom mill) the machine has about 0.05-0.08" backlash in the leadscrews and even with this drawback I still take the 150% every time; plus to top it off I "climb mill" once I've gone my distance across the job (leave 0.1" each end) I then take 1/2 the cutter each pass to the width -0.1" then take the last 0.1" to finish still climbing even into the corners (need to watch the DRO carefully) no one else in the shop can seem to do it; but I find it easier and way faster