Ball Nose Reference & Technical Information

Application Information

Always use anti-seize compound on threads and screw body.
Thoroughly clean pocket and screw at each insert change.
Change insert screw every 10 inserts.
Use high-quality tool holders: power chucks and ER collets are recommended; end mill holders are not recommended.
Cutter bodies will wear and fatigue over time; inspect tool before each use.

Maximum Depth of Cut (DOC) for finishing should be less than or equal to 10% of ball diameter.
Stepover should be greater than or equal to DOC.
For roughing operations, maximum recommended Width of Cut (WOC) and DOC are 30% of ball diameter.
Starting Feed per Revolution (FPR) should be 1% of ball diameter. Example: .750" diameter x .01 = .0075" FPR
Climb milling is preferred.
When plunging with Ball Nose, use pecking cycle with a maximum of .05mm FPR; maximum recommended depth is 30% of ball diameter.
Back Draft and Flat Bottom Inserts are not designed for plunging; ramp in at a maximum angle of 2°.
Compensate for Effective Cutting Diameter (see Table/Figure below).
Compensate for chip thinning with Feed Rate Adjustment (see Table below).
Surface finish (RMS) is a function of stepover and feed per tooth.
Try to work within recommended speeds and feeds (see chart below).
Decrease feed rate coming into corners to reduce chatter.
For long-reach applications, utilize the Carbide Shank/Carbide Core cutting tools for increased rigidity and reduced chatter.

Select diameter of tool to be used.
Determine Depth of Cut (DOC) to be used.
Refer to Figure 1 and Table 1 to find the Effective Cutting Diameter (ECD).
Refer to Feed and Speed chart on back cover to select the surface footage to be used (SFM).
Calculate RPM using the ECD and Vc. (Vc x 318.5 / ECD = RPM)
Refer to Table 2 to determine Feed Rate Adjustment (FRA).
Refer to chart below to select Feed per Revolution (FPR). Calculate mm per Minute (IPM). (RPM x FPR x FRA = mmpm)
Calculate feedrate in mm per Minute (mmpm). (RPM x FPR x FRA = mmpm)

Use multiple above to calculate adjusted feed rate.

Troubleshooting
Concern	Possible Cause	Solutions
Insert wear at tip	Not enough chip load	Verify correct speed and feed Increase feed rate Decrease RPM Increase DOC
Insert wear appears high (flank wear)	Not enough chip load Surface footage is high Incorrect grade or coating/li>	Verify correct speed and feed Increase feed rate Decrease RPM Consider different insert
Insert Chipping	Surface footage is low Incorrect grade or coating Using CB style insert incorrectly Feed too high	Verify correct speed and feed Increase spindle speed Decrease feed rate Change insert selection Decrease DOC Use N style insert
Built-up edge on insert	Low surface footage Light chip load (feed per tooth) Incorrect coating	Verify correct speed and feed Increase cutting speed Increase feed rate Select different coating
Poor finish/chatter	Cutter hung out too far Excessive runout	Reduce tool gage length Check tool holder wear
Tool shank breaks	Tool pressure too great Fatigued cutter body	Decrease DOC Reduce tool gage length Decrease feed rate

Dapra Ball Nose products are made in the USA.

DAPRA Corporation: 1-800-243-3344; Phone: 860-242-8539; Fax: 860-242-3017; info@dapra.com