As unhappy I am to learn that something may be wrong with the software I develop and love, negative feedback is essential in learning whether i am doing everything right.

So a couple of days ago I received an email from a somewhat disappointed user. 

He (lets call him Peter) was complaining that HSMAdvisor calculator gave him "excessively high" speeds and feeds for his 3/4" 4 flute 3.0 LOC  end mill in aluminum.

With the data Peter entered he was getting around 10000 RPM(SFPM 2117) and the feed of 270 inches per minute while usual practice in the shop was side-milling aluminum at that (2.8" axial) depth at only 325 SFM

After double-checking the numbers I replied that in fact his numbers seemed very slow and if for some reason he HAD to run that slow (heck, i machine most steels faster than 325 SFM) due to some conditions, perhaps, he was ought to change the conditions themselves.

This is what I am getting for Peter's end mill setup:

We all have heard hundreds of times that when chatter is happening during machining, we should reduce our feed rate. The same advice we also hear for compensating for extra-long tools and unstable setups.

Let me explain why I think this is mostly incorrect.

Let’s list  the effects of reducing the feed rate:

1. Reduces tool life.
2. Reduces productivity.
3. Increases deflection.
4. Causes chatter.

Let me explain from my own experience and research I have made each of these points and a simple way to avoid chatter's adverse effects.

Lately there have been a lot of really interesting HSM topics on PracticalMachinist forums.

In one of them a guy who owns his own resharpening business posted a video of his endmill milling a block of D2 hardened to over 60 RC.
The forum topic is located here First try on D2 62Rc(video)

Here is his post so you know what we are talking about:

In the ensuing discussion i posted my own take on how and why HSM works

HSM works in many ways.

1) Reduced cutting time per edge per revolution allows it to cool down more.
2) Chip thinning allows to increase chipload (advancement per tooth per revolution)
3) Increased depth of cut combined with shallow radial positively affects deflection. Tool bends less as it is more rigid towards the tool holder.
4) Higher cutting speed actually reduces cutting forces as heat generated in the cutting zone makes it easier to shear off a layer of metal. Yet because the time of contact is so small, most of the heat is carried away with the chip.
5) Higher RPM also allows to get rid of hot chips faster thus further reducing heat transferred to the tool.
6) Higher feedrate actually reduces relative cutting speed.
7) At high axial engagements more than one flute is in contact with the workpiece at different points along the axis of the tool. This too helps combat vibrations and chatter.
8) You are using more of the tool than just its tip, so technically you can do more work with one tool before it gets dull.
9) lastly it looks cool as hell and is very impressive. Whenever we know visitors or bosses are coming we try to make sure some HSM is going on even if application does not merit that
I am not sure if the air that is moved by the endmill is doing much, but i suspect he didn't mean exactly that.

If you are working in mold-making, prototyping or even in a job shop you have had to use unusual form tooling before in your life.

Form tooling is often used to machine undercuts and other features on regular 3 axis machines that would otherwise require a multi axis machining centre or are not machinable o at all.

The classical example of a form tool is a tear-drop ball mil, also known as a "lollipop". It has a tip with a certain diameter and a much smaller shank that produces enough clearance to machine undercuts on straight walls. It can also be used to regular surface finishing and 2d milling.

Another example is a T-slot cutter that is used to produce key-ways and t- slots

The main thing to consider when machining with reduced shank end mils is deflection and torque.

While deflection is especially dangerous for long tools, torque becomes much more important for tools with severely reduced shank.

Torque required to break a tool is directly proportional to the diameter of its shank.

And when shank diameter is much smaller than the tip diameter it does not matter how short that weak portion is: unless you compensate for it you will snap the tool.

The first thing that crosses the mind in many such cases is "I gotta run this tool very slow". It may take forever, but in many cases job gets somewhat done.

Contrary to that many experienced machinists have been proponents of different approach. Instead of reducing feed rate to the point of rubbing and below, it is much more productive to reduce cutter engagement if possible and leave feed rate settings largely unchanged.

Trying to keep proper chip load is even more important when machining work-hardenable materials like stainless steel and titanium. In those cases rubbing is not just unproductive, it leads to a very premature, in many cases instantaneous tool failure.

Just how much of a cut is possible to take in each particular case is the black magic that separates beginners from seasoned pros.

Not to worry though

Here is an example

Shrink fit holders and extensions often come with a big through hole.

Its primary use is to allow the shank be knoked out from he back should the tool ever snap off. It is also used to supply coolant for CTS machines.

Unfortunately said hole affects rigidity of the holder making it more likely to chatter leaving bad surface finish and badly affecting tool life.

There is however an old trick to prevent or minimize the chatter.

All you have to do is pack that hole with some thick grease.

Don't forget to cap off the oppening so that grease does not escape when the tool is spinning.

Here are several photos of surface finish before and after grease application. All cutting parameters were exactly the same in both cases.

before. deep chatter marks after. surface finish is ideal tool in extension holder showing capped hole

We all have manufacturer speed & feed charts and have used their recommendations.

But sometimes those charts just don't apply.

For example manufacturer charts assume you are using their endmills at a certain stickout length, flute length and at a certain depth of cut.

But in the real life you rarely match all these conditions.
Sometimes you need to use longer endmill. Sometimes your flute is longer than what manufacturer gave you speeds and feed for.

What i am trying to say is that whenever your real life conditions differ from "normal" you "need to adjust accordingly".
In fact this is what is printed below many charts.

Too bad not many sources tell you how and what to adjust.

While failure to adjust cutting parameters often leads to chatter, poor surface finish and even tool breakage, one of the biggest mistakes people do when machining is

Sometimes people ask me: "I tried your calculator, and i liked it, but it seems to me a little too aggressive...do you actually do any testing?"

Well, to those I say that not only i do testing, but i run production jobs 100% calculated with my own HSMAdvisor.

Many machinists say that nothing beats an experienced operator holding his hand on feed hold button and playing with speed and feed override trying to find the "sweet spot" where cutting speed and feed rate are maximized and chatter is eliminated or reduced.

And it is correct, but not any machinist is experienced or actually knows what he is doing.
Many machinists also finish their apprenticeship program and never learn a single thing about new tooling types and materials since. They bag years of experience, but their knowledge is stuck on a level it was when they first got their license.

Also not a single person can possibly know cutting conditions for hundreds of materials and remember all of the jobs he had ever ran.

This is where tool database comes in.

Not only can you save tools to cut down and in many cases eliminate entering parameters for every calculation.
But you can (and should) save cutting data for each particular case.

A single tool entry can contain an unlimited number of cuts attached to it, so machinist never has to remember everything.

Here is a i made video of slotting D2 with variable helix hi-performace endmill.

Material: D-2 Tool Steel 200-250 HB
Tool: 0.500in 4FL Carbide TiAlN coated Solid HP End Mill
Speed: 360.0 SFM/ 2751.6 RPM
Feed: 0.0023 ipt/ 0.0094 ipr/ 25.76 ipm

Engagement:  DOC=0.330 in   WOC=0.500 in

Hi-helix end mills have several advantages inherited with their design.

Simple math says that a an endmill with 45 degree helix angle directs 50% of the cutting force downward versus  25% for a 30 degree end mill.

Main advantages are:

• Higher rake angle directs more of a cutting force downward.
  This reduces side load on the cutter, that leads to less deflection and less tendency to chatter.
• At high axial engagement (deeper depths of cuts) more flutes remain in the contact with the work piece. This leads to much smoother cut, again reducing tendency of the cutter to chatter.
• High helix angle pulls chips upward and away from the cutting zone.
  This reduces chip re-cutting and helps prevent cutter from getting clogged up. This also allows to take deeper cuts and increases productivity.
• Because of higher helix more of flute length is being used in the cut. Better surface finish is achieved even when using the same chip load.
  Generally an end mill with 45 degree helix can be fed 30% faster than equivalent one with 30 degree helix and still achieve same surface finish.

High helix end mills also have disadvantages that a machinist has to take into consideration:

• With more of cutting force directed axially, the load on spindle bearings in downward direction is increased.
• Tendency for both the end mill and the work piece to pull out is increased. So a more rigid tool holding and work clamping should be considered.
• Higher helix end mills are also less stiff that regular helix end mills. This may cause more deflection and may become a problem when having to machine straight walls.
  This effect should be mostly diminished by lower side radial load, but it still needs to be considered in some cases.

If you are finishing a pocket with wall corners' radius close to the radius of a cutter. The tool tends to chatter, especially with longer tools and harder materials.

To avoid this you can do one of the following:

• When programming. After roughing the pocket and before finishing. Create a simple drill cycle with finishing tool to remove extra material from the corner. This way when finisher goes to the tight corner, the chatter will virtually disappear.
• Do the same with a drillbit. Before Roughing.