Aluminum Cutters Discussion: Helix Angles
I thought it would be interesting if we could get some opinions on helix angles for cutting aluminum. Lately, all anyone sells is 45* helix and that is really all I have ever used. Recently I hired a 5 axis programmer to help get us up and running on a new project and all he talks about is using 35* helix cutting tools for aluminum (especially in long reach situations). Has anyone ever tested 35* helix vs 45* helix for roughing and finishing of aluminum? I'm not talking about 50hp cat 50 machines... I'd be using them on 30hp/20hp cat 40 and light brother bt30 machines. I was skeptical of him in the beginning but now I'm becoming a believer. You can tell the difference when switching from a 45* to a 35* helix with the way the machine handles the same cuts...
Higher Helix allows Smoother cutting action- chaterless.
Ligher side loads that reduce cutter deflection BUT higher helix end mills are LESS rigid than regular ones, so they bend more. and they also allow more bend before they break . Sounds crazy but i tested that.
For roughing its best to use high helix- they allow higher MRR up to 150% higher
For finishing where walls need to be straight use anything below 40Deg.
all above said is only IMHO.
MMR = (Maximum Material Removal?) How many flutes are we talking about, and what depth of cut relative to tool diameter are we talking about. I like three flute standard style end mills.
Please don't get me wrong.. this is a good topic of discussion. Two things I can reference are: Higher helix build higher lifting forces to pull parts from fixtures, and I also believe the added shearing action can wear the cutting edges faster. Shearing action is important to allow the cutting edge to "blend in" to the material without banging it's way in, hence the 30 degree angle. Many machine tool people have traveled this path before us, and seemed to have settle on this design. However, if there is new truth, I'd like to become aware of it. Really!
Another thought, think of a 1/2" headless bolt with one straight flute. Then imagine the thread was ground into a straight cutting edge, and you turned it on and begin to BANG your way though the part. Then since you didn't like the way it cut, you made another one with a 30 degree angle, and it cut better, so you tried again using a 45 degree helix. After that, you go off the deep end and make a 1/2"-13 threads per inch end mill with one cutting edge and try that one.
Some where there is an optimum design, with multiple lead threads (or flutes) and various helix angles.
We used to almost exclusively use 37° helix for aluminum until we had a job running on our mill-turn that required roughing and finishing. The 1/2" 37° 2 flute carbide endmill from OSG would chatter and scream to the point that the harmonics of it were damaging the 90° milling coupler unit. We had to repair/replace them every 6 months or so until we changed out to a 45° helix. Now, instead of screaming chatter, you hear a low pitch hum and we're getting about 4 years out of our milling couplers. That is my experience.
Last edited by Neslob660; 06-30-2012 at 03:05 PM.
Reason: I cnat tpye
I'm working on a part that has a pocket with .125 radius that is 2.250 deep in 6061 and I'm roughing it down in stages. 1/2 - 3.8 - 1/4 and there was a significant amount of decrease in chatter going from a 45* tool to a 35* helix. Both tools were stub loc, neck relieved, and had the same radii on the corners.
The only explanation i have is tool manufacturer somehow messed up the tool geometry.
Originally Posted by dstryr
Seriously i have a set of 7/32 Hi-Helix drills supplied by DORMER that would clog-up at only 2" depth and .25 pecking.
Inspection revealed that they actually had POSITIVE-NEGATIVE flute geometry and were pushing chips against the wall of the hole.
Anyway i believe 45 deg helix end mills chatter less than 35.
OH almost forgot: at some extra long lengths there may be no benefit to use hi helix when taking light cuts anyway!
Those endmills shine when doing slotting and roughing
The 45* cutter was from FORD and DESTINY Tool and the 35* was from Helical and Melen... This is using 3 different tools...it isn't because the "manufacturer" messed up...
Originally Posted by zero_divide
My experience has always been that higher helix angles allow higher feeds for the same finish, but that the tools are less rigid.
Qualitatively speaking I get the same finish at about 30% higher feeds out of a 45 coming from a 37. I don't know the difference if you were to actually measure the surface deviations. I've never run a milled part which had a measured surface finish requirement on the wall (only turned parts).
For general purpose I stick with 45* cutters - they're more versatile with regards to finish and chatter. I could see some instances where a lower angle could be better but I would probably only buy them for specific jobs.
That said, I've also found that chatter and finish have a lot more to do with the specific grind of the tool than they do the generic metrics like helix angle.
+1 i just love it when someone agrees with me
Originally Posted by sniper1rfa
I have 2 "identical" hi helix HP end mills from niagara cutter.
But one is a 2 flute and very stable and doesn't chatter at all.
The other one is 3 flute and tends to chatter when slotting ;/
Hard for me to wrap my head around since 3 flutes are usually more stable than 2
Note worthy they are .5 dia 2.5 flute Length and maybe 2.75 stickout.
I have found that the 37 degree 3 flute work better when doing deep pocketing but the 45 degree 3 flute work great on outer profiling (better finish). I tried some 45 degree 2 flute but they did not live long (no through spindle coolant) at the advertised feed rates.
I'll agree on the grind. It is not so much the actual grind, but the angles relative to the cut. You want positive rake tooling for aluminum......but there is a limit. If you get too much positive, the cutter will try to "dig in", much like you see when machining brass. This will create chatter. You can visually tell what is going on by looking at the chatter itself. If the chatter has smooth feature humps, the cutter is pushing away from the part..... i.e. not enough positive and it's rubbing. If the chatter is sharp edged, the cutter is pulling into the part and snapping back......... i.e. too much positive and it's hooking. Taking a close look at the actual chatter can go a long way to determining a fix.
Anyone pay attention to Climb or Conventional milling?
How about the dif alloys?... does that make any dif??
How about fixture design if your testing on a job rather than a test block held securely to the table??
What about the cutter makers claims?... are the instructions followed??
A lot of variables up there....
0 Degree helix will cause your cutting forces to act in radial and tangential directions only. It will also cause the cutting forces to pulse - as in an interrupted cut. This is because the flutes are suddenly entering and exiting the cut. As you increase the helix angle, you will be shifting part of the radial and tangential forces to the axial direction (along the tool axis). You will also be reducing the amplitude of the pulsation in cutting forces, but will have a increased mean cutting force as more of the flutes will be engaged in the cut.
Chatter is caused by by oscillations in chip thickness from the tool recutting a wavy surface. Depending on the shift between the waves of the previous surface and the vibration of the tool at the present surface, the chip load will grow or decay exponentially. If it grows exponentially, it is called chatter. If it decays exponentially, it is called a stable cut. To model it accurately involves delayed differential equations. Chatter basically indicates a source of flexibility in the machining process. Like electricity the machining process will chatter at it's weakest member and at a frequency very close to a natural frequency of the system. If you are using heavy roughing cuts, it will usually chatter at a mode of the spindle. If you are using a thin, flexible tool it will chatter at the tool. If you are machining thin-walled structures it will chatter at the part.
Practically, the main ways to eliminate chatter are:
1) Cut less material - reduce depth or width of cut.
2) Stiffen up the structure somehow - use larger tool shanks, stiffer spindles, for thin wall parts try and machine trouble spots in a thicker state if possible
3) Change RPM - chatter is mainly influenced by depth of cut, width of cut and RPM. Usually there are lobes of sweet spots and, actually increasing RPM will make the process more stable. There is software to calculate the lobes for simple 2D milling.
4) Reduce number of flutes - Stability generally (not always) goes down with increasing number of flutes.
You can also try designing variable-pitch or variable-helix tools to cancel out the chatter frequency. Or designing tools with low clearance to absorb the vibration. However, if surface quality is important, this may damage the microstructure and the tool will be banging on the part.
In my opinion, with a higher helix, you will be directing more of the cutting forces to the axial direction which is generally much stiffer than the bending direction. You may see a slight increase in stability, but the difference from 45 to 35 would probably not be that substantial.
Another way to kill chatter is to increase the damping of the system. Chatter is related to the lowest dynamic stiffness point of the system. Dynamic stiffness is composed of both stiffness and damping values. This explains why operators wrapping bike inner tubes around parts (yes I have seen this) and filling the cavities of integrally bladed rotors with foam will reduce the tendency of tools to chatter.
We use a lot of hydraulic holders (schunk). This is primarily for reduced run-out, but on one occasion we used them to reduce chatter as they damped (oil cavity)
Originally Posted by Red X
In order for the software to work some physical tests are required on the machine.
Originally Posted by barbter
Some of them test natural frequency of the tool in the spindle. and then plot prefect RPM vs Depth of cut graphs. Others test the frequency of the machine itself.
There is no accurate software-only model that i know of. (if anyone knows better- i am listening)
When i tried to build one the results were within 500 rpm of the sweet spot. Which is pretty damn too much and renders it useless.
Most of the time you only need to change rpm by a couple of percent to reduce or even eliminate chatter.
(in cases where this can be done. sometimes no matter what you do, the tool keeps chattering and you need to reduce the DOC or hone the cutting edge a bit)
We have them too. but apparently if reducing the vibration is the only goal, its better to put some thick grease into the holder behind the tool. works the magix!!!
Yes. Zero Divide is correct. To accurately predict chatter with the software, you will need to do physical tests. To do this, you will need an impact hammer with an integrated force sensor (Kistler, Dytran, PCB, etc), an accelerometer and an I/O box. If you want really accurate results at low frequencies you can use a laser displacement sensor instead of an accelerometer. I know Keyence is one company that manufactures these, though these sensors are significantly more money than accelerometers. You will also need an I/O box (National Instruments sells some) to capture the signals.
In a nutshell, you place the sensor on the tool directly opposite to the direction of impact and hammer the tool. The hammer will measure the applied force and the accelerometer will indirectly measure the displacement. By dividing displacement by force at each frequency you can get the stiffness/ of all the modes of the machine at the tool point you measured. The dynamics of the entire machine / tool / spindle assembly will be captured as reflected at the tool tip. Using this, your radial immersion (slot, half, quarter cutting), some fancy equations and a material model, the software can predict the saw-tooth shaped lobes where depth of cut and RPM are ideal.
The two main companies that I know if of that sell this software are:
MALINC - Cutpro
Machine Tool Testing Software and Machining Problem Diagnosis Software
Manufacturing Laboratories Inc - Harmonizer
Manufacturing Laboratories, Inc. (MLI)
You can also write your own code for 2D milling. It can be found in:
However, you will still need the hammer setup to find the machine dynamics. You will also need to find the cutting coefficients. You may be able to obtain estimates of these from sources like Sandvik (their catalogues). In my opinion for chatter prediction, the software is really only useful for 2D / 3D milling cases. It is not there yet for 5-axis sculptured surface machining or in very low RPM machining. However, in time these will be modeled more accurately.
To eliminate the impact testing with the hammer and simulate the dynamics of the machine requires finite element (FE) modeling. Although these can estimate the stiffness of structures, they cannot find the damping - this is impossible to predict as of today. Also, FE is notoriously unreliable if not checked and tuned with the real world system. The expression "Simulation is like masturbation. The more you do it, the more you think it's real", could not be more correct.
Barbter: Yes I love the corncob cutters for roughing too. They make the tool behave like one with the stability of a one-fluted cutter but remove material like a multi-fluted cutter. Combine with variable pitch and these things can devour nasty alloys at insane depths of cut with virtually no chatter.
HOLD THE BUS!!
Sorry almost missed it.
My spidey senses are tingling so i went and did little google search.
You said TWICE that less flutes means more rigidity and it did not really make sense to me.
Info from CWD.edu
And if you look everywhere the only guy who says otherwise (that less flutes means more rigidity) is Mr. Bob Warfield, creator of G-Wizard.
Four Flute End Mills.
Best for providing good finish when milling the edge of a work-piece.
1. Use for cutting harder materials where small chips and rigidity are necessary.
3. Use center-cutting types for plunge cutting.
There are some reasons why it may be preferable to use a four flute end mill even when cutting aluminum.
Two flute end mills are not as rigid as equivalent diameter four flute end mills because two large flutes provide a smaller cross sectional area to resist bending forces.
Given equivalent speeds and feeds, a two flute end mill will have twice the chip load as a four flute end mill. Because of increased chip load under similar cutting conditions, cutting pressures are greater. The only method to reduce chip load is to reduce feed rate or increase spindle RPM each of which may have negative consequences
I don't know where his info is coming from but can you state your source?
Other than that sounds like you are pretty knowledgeable guy. Thanks for the link to that amazon book, gotta take a peek at it when my overtime finally runs out.
edit: OMG that book is 125$ !!! its like i gotta work a 2 days to pay for it!!!!
At a recent MSC tooling seminar one of the mill manufactors, was telling us that most endmills as designed to cut at certain depths. His example was if you have a 1/2 endmill you should be cutting either .000-.400 depth or .550 and deeper. That with a half inch endmill you should never cut a .5 depth of cut.
One other thing I have used in machining alum is progressive helix angle end mills. We used the accupro 30deg - 40 deg end mill starts at 30deg and changes slowly to 40deg at the shank. 3 Flute Progressive Helix Single End Mills for Aluminum - Square End Mills | MSCDirect.com And then we finnished with a 6 flute carbide. The mill operator thought I was nuts when I took him the tooling. With that said they worked great, we had no chatter from the progressive helix mill, even at full depth of cut. and the 6 flute provided a supper finish, that we needed.
The parts were big round parts with thin walls, too thin for us to chuck in a lathe so we decided to mill them instead.