Ball Nose Milling Strategy Guide
Ball Nose Milling Without a Tilt Angle
Ball nose end mills are ideal for machining 3-dimensional contour shapes typically found in the mold and die industry, the manufacturing of turbine blades, and fulfilling general part radius requirements. To properly employ a ball nose end mill (with no tilt angle) and gain the optimal tool life and part finish, follow the 2-step process below (see Figure 1).
Shop Harvey Tool’s Vast Selection of Ball Profile End Mills – Click Here to Get Started
Step One: Calculate Your Effective Cutting Diameter
A ball nose end mill’s Effective Cutting Diameter (Deff) differs from its actual cutting diameter when utilizing an Axial Depth of Cut (ADOC) that is less than the full radius of the ball. Calculating the effective cutting diameter can be done using the chart below that represents some common tool diameters and ADOC combinations or by using the traditional calculation (see Figure 2).
Step Two: Calculate Your Compensated Speed
Given the new effective cutting diameter a “Compensated Speed” will need to be calculated. If you are using less than the cutter diameter, then its likely your RPM’s will need to be adjusted upward (see Figure 3).
KEY
ADOC = Axial Depth of Cut
D = Cutting Diameter
Deff = Effective Cutting Diameter
R = Tool Radius (Dia./2)
RDOC = Radial Depth of Cut
SFM = Surface Feet per Minute
Sc = Compensated Speed
Ball Nose Milling With a Tilt Angle
If possible, it is highly recommended to use ball nose end mills on an incline (ß) to avoid a “0” SFM condition at the center of the tool, thus increasing tool life and part finish (Figure 4). For ball nose optimization (and in addition to tilting the tool), it is highly recommended to feed the tool in the direction of the incline and utilize a climb milling technique.
To properly employ a ball nose end mill with a tool angle and gain the most optimal tool life and part finish, follow the 2-step process below.
Step One: Calculate Your Effective Cutting Diameter
The chart below that represents some common effective cutting diameters and ADOCs at a 15º tilt angle. Otherwise, the traditional calculation below may be used (see Figure 5).
Step Two: Calculate Your Compensated Speed
Given the new effective cutting diameter a compensated speed will need to be calculated. If you are using less than the cutter diameter, then its likely your RPM’s will need to be adjusted upward (see Figure 6).
KEY
Deff = Effective Cutting Diameter
SFM = Mfg Recommended Surface Feet per Minute
Sc = Compensated Speed
Thank you for this milling strategy guide. I especially appreciate your insight on milling with a tilt angle. I was unaware that this could extend the life of the bit. I will keep this in mind while milling in the future.
Thank you for sharing this method which I haven’t learned before. It’s helpful for me to learn a lot.
Faced with the choice of climb milling or moving in the direction of the incline, which is preferable for surface finish?
Great question Jordan! When your main concern is surface finish we recommend using the climb milling strategy
Could you perhaps assist with this in metric?
If anyone is looking to add this to excel…
=B44*SIN(RADIANS(B45+DEGREES(ACOS(1-((2*B46)/B44)))))
Where:
B44 is the Diameter of Cutter
B45 is Angle in Degrees
B46 is Depth of Cut
They don’t talk of feed. is there feed/tooth adjustment?
Hi Marc,
The adjustment is calculated with the “SC – Compensated Speed” part of the article. This post covers finding your Effective Cutter Diameter which you can linearly interpolate against the speeds and feeds chart to get your RPM. Speeds and Feeds are thus calculated after the fact. Please refer to the Speeds and Feeds 101 article here.