• Ron Davis

What’s all the fuss about High Feed and High Speed Milling? Part 2 of 2

It’s all about the "Chip!" Part 2

High Speed Milling

Let’s talk about making a lot of chips really, really, fast. The two primary methods utilized today to create a lot of chips are High Feed milling and High Speed milling. While they are very different in many respects they have some similarities. In this two-part blog series, I will attempt to explain both. As the title states; it’s all about chip.

As we discussed in last week’s blog High Feed milling is all about chip thinning. You must increase your feed rate to compensate for the chip thinning effect created by the large lead angle on the cutting tool which is typically 75° to 82.5°. In most cases your feed must be increased four to five times faster than standard feed rates utilizing square shoulder or 45° lead milling cutters. The large lead angle while somewhat limiting the axial DOC (depth of cut) pushes most of the cutting forces axially up into the spindle increasing radial stability. This allows for long reach capabilities with limited deflection. This too comes at a cost. Care must be taken when entering corners and changing cutter path directions. Slowing down in the corners can be important. Implementing smooth tool paths and transitions with arcs or radii larger than the radius of the tool prevent excessive cutter engagement and chatter. When applied correctly High Feed milling is an extremely productive metal removal process and can be a lifesaver in deep cavity and long reach applications. Now let’s take a look at High Speed Milling.

As the title states “it too is all about the chip”. In High Speed Milling your your feed rate must be increased to compensate for chip thinning just like in High Feed milling, but not because of the tools lead angle. Unlike High Feed Milling, the chip thinning effect in High Speed milling is created by limited radial engagement of the cutter diameter in the cut. Unlike a basic OD turning operation, a milling cutter cuts on an arc not a flat plane. In turning, your chip has a constant thickness. In milling, the chip thickness varies depending on where the cutting edge is in relation to the arc of the cut. When a milling cutter diameter is fully engaged in the cut; the chip thickness is zero on entry and exit and at it’s thickest in the middle of the arc of rotation. As with all metal cutting operations we must manage the chip thickness, but chip thickness is not always equal to your feed rate.

We first introduced the concept of chip thinning when we discussed lead angle. As your lead angle increases the chip thickness begins to thin. In a normal turning operation once the chip thinning factor for the lead angle is applied the chip thickness remains same. In milling we must factor in both the chip thinning factor for lead angle as well as the chip thinning factor for radial engagement. The result is called “average chip thickness” or hm. Now before any physics majors go off on me, hm is a physics term meaning the measure of the point in the middle of the group. Average is just that; the average of the entire group. I do not know why the metal cutting industry decided to conflate the two, but they did, so I will continue the charade.

Please see the attached illustration noting the chip thickness is zero at the beginning middle and end of the cutter rotation in the cut. The chip is the thickest on the centerline. The average hm is located between the centerline of the cut and the beginning and ending of the cut. So why do we care about the average chip thickness? Remember; what does it take to make a chip; heat and pressure. Where do you want the heat to go; into the chip. This is where average chip thickness hm comes into play. Your average chip thickness must be greater than your edge preparation, t-land or hone or you will turn your milling cutter into a piece of sandpaper. Sandpaper is abrasive machining not metal cutting. Carbide likes to cut, it does not like to rub. Rubbing creates uncontrollable friction and heat that is detrimental to the life of your tool life. This is where fz = hm x (SQRT(D1/ae)) x COS K comes in. This equation looks difficult but it’s not and it makes all the difference between success and failure.

The key to high feed milling is understanding the relationship between the radial engagement ae of the tool and the impact it has on the average chip thickness hm and your programmed feed rate per tooth or flute fz. As the radial engagement of the cutter diameter is reduced your programmed feed rate must be increased to compensate for the radial chip thinning that will occur. By using the formula, you may calculate the programmed feed rate fz required per flute or insert to achieve the desired average chip thickness hm. Most cutting tool manufacturers provide both the fz (feed per tooth) as well as the hm (average chip thickness) values based on the size and shape of the edge preparation for the given tool. Once you have calculated your required feed rate per flute or insert calculating your IPM (inches per minute) table travel is easy. In most cases, your IPM feed rate will be more than four or five times faster than standard feed rates.

The red column in the table illustrates the resulting average chip thickness hm achieved when the radial engagement of the cutter is reduced and the feed per tooth fz is not increased. When using between 50% - 100% of the cutter diameter the standard feed rate of .006” fz will produce the .0042 hm required by the edge prep on this tool. As the “Percent of D1 Engagement” falls below 50%; however, the average chip thickness thins out to less than the thickness of paper very quickly. To achieve the .0042” average chip thickness required for this example the feed per tooth/flute must be increased from 50% to 200% as the “Percent of D1 Engagement” is reduced from 40% to 20%. So how does this all relate to High Speed milling?

In High feed milling the high feed rate is coupled with high axial depth of cut and specific cutter path strategies to achieve high metal removal rates. The higher axial depth of cut is possible do to the reduced radial forces created by the reduced radial engagement. Typically, axial depths are greater than two-times the diameter and up to six-times diameter can be achieved. The radial forces can be further reduced by using a higher helix angle which drives more of the cutting force into the spindle. Chip evacuation at the higher axial depth of cut is not an issue because the chips are not crowded into the flute as they would be with a higher radial engagement. The ease of chip evacuation also allows the use of tools with more flutes or inserts resulting in even higher feed rate capabilities. Tools with more flutes and inserts typically have a larger core diameters due to small chip gullets or flute spaces which further enhances stiffness, rigidity, and stability.

In addition, to the benefits listed above, High Speed milling also reduces the amount of heat transferred into the tool and the part thus enhancing tool life and reducing the possibility of work hardening the part. It is counter intuitive; when you hear high speed, you think high heat. Not true here. In a full slot application, the full diameter of the cutter is engaged in the workpiece or the cutter has a full 180° arc of engagement. This high arc of engagement means the

cutting edge is engaged in the cut a long time thus producing more heat. As the radial or arc of engagement decreases so does the amount of time each cutting edge is in contact with the workpiece, which produces less heat and provides the cutting edge more time to cool between cuts. This reduction in heat has a couple of benefits. It helps prevent work hardening in high carbon and stainless steels and reduces the amount of heat transfer back into the tool when machining refractory metals and superalloys. Bottom line it enhances tool life. With all these positive outcomes, what’s the catch?

There is no real catch; however, there are basic principles that need to be followed. Rigidity of the entire machining mechanism; the machine, spindle, holder, fixture, etc. is s always important. Keeping a constant load on the tool is important and it requires specific tool paths, no sudden, sharp changes in direction. Trochoidal Milling, Dynamic Milling, Volumetric Milling or Slicing are a few of the cutter path strategies supported by most modern CAD/CAM software that support High Speed and Feed machining. In many cases, it takes a combination of more than one strategy to complete the part. Every CAD/CAM supplier has a differing approach on achieving these goals so I have attached a couple of links below to get you started.

In summary, High Speed milling is all about radial chip thinning. You must increase your feed rate to compensate for the chip thinning effect created by the reduced radial engagement of the tool diameter in the workpiece. In most cases, your feed rates are more than four to five times faster than standard feed rates when utilizing more than 40% of the cutter diameter. The radial engagement is usually 20% or less of the cutter diameter. This reduces radial forces, allows for axial depths-of-cut of up to six times the cutter diameter, which produces high metal removal rates. The reduced radial engagement also provides the added benefit of reducing the amount of time the cutting edge is engaged in the material. This reduces heat buildup in tool and part which improves tool life and helps prevent work hardening.

High Speed and High Feed milling are all are great ways to increase your productivity by putting a lot of chip on the floor and parts out the door. It’s all about the chip!

#HighSppedMilling #Radialchipthinning #chipthinning


© 2016 All Rights Reserved | Davis Machining Technology, LLC |  1718 Sawmill Road |  Greensburg , PA 15601 |