Did you know that there are two major endmill designs available on the market today? The first is the “Conventional” design, which is most common. It features primary “relief” with a secondary clearance that is flat or concave. The clearance angle is measured over the high points at the angle transitions. It is easy to regrind and can be used for both axial and radial clearances.
The other design is “Eccentric.” Eccentric relief endmill design on the other hand, combines the primary and secondary relief into one constant drop. The continuous drop provides the strongest cutting edge. However, the eccentric grind is primarily used for radial clearance. So, on many endmills with the ER grind, you will still see the Primary/Secondary on the face.
Now that we understand the technical differences between the two styles of endmill designs, the next question is which design is likely to work well for your next application. The chart below shows when each type of design is likely to work best with your application:
The eccentric relief works very well in most materials, but there is still a valuable reason to use the primary/secondary grind. The primary/secondary grind is capable of machining softer materials, light depths of cut, thin walled parts, etc. For this reason, you’ll always see a combination of the two styles offered, to cover most situations.
Heat is the enemy of carbide.
Excessive temperature breaks down the Colbalt Binder, which holds the Tungsten
Carbide in place. WIDIA-Hanita has developed a coating that gets you more time
out of your tools.
WIDIA-Hanita Victory solid carbide end
mills use a combination of pre-coat process, coating, and post coat treatment.
The pre-coat process removes any grinding damage. You can’t see it with the
naked eye, but it’s there and can affect the cutting-edge integrity and chip
flow characteristics. This process smooths all surfaces in preparation for
coating. The Victory coating is an Advanced AlTiN treatment with aluminum
content which oxidizes with high temperatures and lends itself to high surface
speed capability and better tool life. After coating, the post-coat process
creates a smooth and hard surface. This also improves the compressive strength
of the coating, preventing it from flaking or wearing too soon. The cutting
edge is very consistent for strength and enhanced chip flow.
Innovative edge preparation provides consistent tool life by eliminating most microchipping caused by grinding. The post-coat finish reduces the chip build-up and improves chip flow. Combined, Victory grades increase tool life and provide higher MRR, shorter cycle times, and fewer tool changes.
competitive machined component market, companies seeking to get more out of
existing CNC Machines constantly look for ways to increase Metal Removal Rates
(MRR) i.e. removing more metal in less time. One of the best ways to increase
MRR is through more aggressive spindle speeds and feed rates. To accomplish
this, it takes more than simply turning up the parameters in the CNC program –
one must account for chip formation. Creating proper metal chips and getting
them out of the way of the cutting tool is critical to machining faster.
In this post, we examine the concept of chip thinning in
CNC Milling applications, and its impact on enabling higher feed rates in
This diagram below shows the impact of radial width of cut, and its effect on chip thickness. When the radial WOC is 40 percent or less, the average chip thickness reduces, and the feed rate must be increased to compensate.
In the upper left-hand corner, you can see a full width pass which is 100% engagement. As the cutter is rotating clockwise, the cutting edge enters the cut at .000 chip load. As it progresses through the rotation, the chip load increases to the programmed chip load (Fz) until it passes center. This portion of the full pass is known as conventional milling. As the chip is very light at the start, more heat is generated which can damage carbide. As the cutting edge moves past the centerline, the chip load decreases from the programmed Fz, progressively back to .000. This portion of the full pass is known as climb milling. In this motion, the chip starts at its maximum and decreases which generates less heat, better finishes, and higher tool life. Since climb milling is the preferred method in milling, a 2/3 relationship is recommended between the cutter diameter and the width of cut. This ensures a climb cut engagement. However, at times the width is less than the 2/3 recommendation. Generally, feed rate compensation is not required until you get to 40% and less. The average chip load, hm, is generally used when widths of cut vary, so the maximum is not exceeded. In the case above, notice the average chip thickness is .0042 and the programmed feed is .006.
In the lower
left-hand corner, at 50% engagement, the average chip thickness (hm) is still
at .0042 and the programmed feed is .006. No compensation is required, although
notice we are now in a climb cut motion. This is desirable for milling.
In the upper
right-hand corner, at 20% engagement, big changes start to happen to the
average chip thickness (hm). At a programmed chip load (Fz) of .006, the actual
chip load is .0026, which may be below the recommended range for the cutting
edge (profile, edge prep, etc.). To maintain the average chip load of .0042,
the programmed chip load (Fz) must be increased to .0093.
Last, in the
lower right-hand corner, the radial engagement is now 10%. The actual chip load
is .0018, which may be below the recommended range for the cutting edge. This
low chip load causes excessive heat generation and can cause the cutting edge
to fail prematurely. To maintain the average chip load (hm) of .0042, the
programmed feed per tooth must be increased to .0132.
changes, based on the radial width percentage can increase tool life and
production rates. To find the radial percentage of engagement, use ae/D1
Ex – .05/1.000 =
Ex – .50/2.000 = 25%
These examples all show how important chip thinning is, as
when done properly, it enables increased feed rates. If a chip load is too low,
the cutting edge can generate excessive heat which can damage the carbide and
reduce tool life. The excess heat can have other effects, such as work
hardening certain materials.
Did you find this post helpful? Tell us what else you might
like to learn more about?
Many metal cutting professionals may not realize that the way an indexable milling insert is manufactured has an impact on tool life and surface finish. Let’s start with the basics. There are two basic ways to ensure the size and edge prep of an indexable milling insert: A) either the insert is “pressed and sintered to size (PSTS),” meaning that the finish size and edge prep is engineered into the press molds and heating calculations, so that the insert meets the tolerance requirements, or B) the insert is “periphery ground to size (PG),” meaning a secondary grinding process is used to bring the insert to the final size. Regular industry standard is following the “M” tolerance for PSTS inserts which allows for greater tolerance variation on the diameter. WIDIA global standard is set up to a tighter tolerance “P” for high precision PSTS inserts to achieve a better axial runout and positive impact in better tool life and surface floor finish.
are the first choice for finishing, high precision applications like die and
mold. In addition, due to sharper edges, PG inserts are well-suited for
machining of non-ferrous materials, like aluminum and brass.
Whereas, PSTS inserts are the first choice for semi-roughing and roughing applications. Inserts with tolerance class G, K, C, H are PG. Those with tolerance class P are PSTS.
class tolerance is much more wide open when it comes to the IC and the “M”
dimension (distance from IC to the wiper flat). The P tolerance is a balanced,
+/- 0,038 (.0015), for more consistent size.
To get the best surface possible, be sure to align the
topography letters on the insert the same way each time. i.e. MM should start
in the same position in each pocket and roll inward with each index.