Metric Ball Nose Reference & Technical Information
Application Information
Technical Considerations
- 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.
Recommendations
- 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: 20mm diameter x .01 = .20mm 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.
- 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.
Ball Nose Feed, Speed and Diameter Compensation
Table 1: Effective Cutting Diameter (ECD)
 |
||||||||||||
 |
.10 | .25 | .40 | .50 | .75 | 1.00 | 1.25 | 1.50 | 2.00 | 3.00 | 4.00 | |
|---|---|---|---|---|---|---|---|---|---|---|---|---|
| 10mm | 1.99 | 3.12 | 3.92 | 4.36 | 5.27 | 6.00 | 6.60 | 7.14 | 8.00 | 9.17 | 9.80 | |
| 12mm | 2.18 | 3.43 | 4.31 | 4.80 | 5.81 | 6.63 | 7.33 | 7.94 | 8.94 | 10.39 | 11.31 | |
| 16mm | 2.52 | 3.97 | 5.00 | 5.57 | 6.75 | 7.75 | 8.59 | 9.33 | 10.58 | 12.49 | 13.87 | |
| 20mm | 2.82 | 4.44 | 5.60 | 6.25 | 7.60 | 8.72 | 9.68 | 10.54 | 12.00 | 14.28 | 16.00 | |
| 25mm | 3.16 | 4.98 | 6.27 | 7.00 | 8.53 | 9.80 | 10.90 | 11.87 | 13.57 | 16.25 | 18.33 | |
| 32mm | 3.57 | 5.64 | 7.11 | 7.94 | 9.68 | 11.14 | 12.40 | 13.53 | 15.49 | 18.66 | 21.17 | |
- 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)
Table 2: Feed Rate Adjustment (FRA)
 |
|||||||||
 |
6mm | 8mm | 10mm | 12mm | 16mm | 20mm | 25mm | 32mm | |
|---|---|---|---|---|---|---|---|---|---|
| .10 | 3.6 | 4.0 | 4.4 | 5.0 | 5.6 | 6.1 | 7.1 | 7.9 | |
| .25 | 2.6 | 2.8 | 3.1 | 3.6 | 4.0 | 4.4 | 5.0 | 5.6 | |
| .40 | 2.1 | 2.3 | 2.6 | 2.9 | 3.3 | 3.6 | 4.1 | 4.6 | |
| .50 | 1.8 | 2.0 | 2.2 | 2.6 | 2.8 | 3.1 | 3.6 | 4.0 | |
| .65 | 1.7 | 1.8 | 2.0 | 2.3 | 2.6 | 2.8 | 3.2 | 3.6 | |
| 1.30 | 1.2 | 1.4 | 1.5 | 1.7 | 1.8 | 2.0 | 2.3 | 2.6 | |
| 2.00 | 1.1 | 1.2 | 1.2 | 1.4 | 1.5 | 1.7 | 1.9 | 2.1 | |
| 2.50 | 1.1 | 1.1 | 1.2 | 1.4 | 1.5 | 1.7 | 1.8 | ||
| 3.00 | 1.1 | 1.2 | 1.3 | 1.3 | 1.5 | 1.7 | |||
| 4.00 | 1.1 | 1.2 | 1.3 | 1.4 | 1.5 | ||||
| 4.50 | 1.1 | 1.2 | 1.3 | 1.4 | |||||
| 5.00 | 1.1 | 1.3 | 1.4 | ||||||
| 6.35 | 1.2 | 1.2 | |||||||
| 7.50 | 1.1 | 1.2 | |||||||
| 10.00 | 1.1 | ||||||||
Use multiple above to calculate adjusted feed rate.
Recommended Cutting Speeds & Feeds for Metric Ball Nose Finishing Mills
| ISO | Material Group | Vc in mpm (Uncoated) F1 |
Vc in mpm (Coated) | Chipbreaker | FPR* (mm) | |||
|---|---|---|---|---|---|---|---|---|
| FPX | FPO | FPA & FP-GLH | ||||||
| P | Plain Steels | < 3%C | 90-180 | 120-300 | 180-390 | 240-490 | N, CB | .08-.25 |
| 3%-6%C | ||||||||
| 5%-1.5%C | ||||||||
| Alloy Steels | Mo | 90-275 | 135-395 | 210-420 | ||||
| Cr | ||||||||
| NiCrMo | ||||||||
| Tool & Die Steels | ||||||||
| M | Stainless Steels | Ferritic/Martensitic | 45-90 | 75-240 | 110-300 | 100-360 | N, CB | .08-.25 |
| Austenitic | 45-200 | 65-265 | 90-330 | CB | ||||
| Precipitation Hardening (PH) | 45-150 | 65-210 | 90-270 | |||||
| K | Cast Iron | Gray | 100-180 | 90-275 | 135-320 | 150-360 | N | .08-.38 |
| Malleable | 135-300 | 120-330 | ||||||
| Ductile | ||||||||
| N | Aluminum Alloys | 300+ | 300+ | 300+ | 300+ | CB | .13-.64 | |
| Copper Alloys | CuNi: Refer to High-Temp. Alloys below | 120-180 | 120-240 | 150-270 | 150-300 | |||
| S | High-Temp. Alloys | 15-40 | 15-60 | 15-100 | 30-140 | CB | .05-.20 | |
| Titanium Alloys | 15-40 | 15-60 | 15-120 | 45-200 | ||||
* For tools below 20mm dia., use the lower half of the range. For tools above 20mm dia., use the higher end of the range.
FPX and FPO coatings are best suited for low to medium operating speeds (temperatures) and softer materials.
FPA and FP-GLH coatings are best suited for higher operating speeds (temperatures) and harder materials.
The parameters provided are suggested operating parameters. Actual speeds and feeds will depend on many variables, such as rigidity, workpiece hardness, tool extension, machine accuracy, Depth of Cut, etc. Start at the middle of the Vc range and the low end of the FPR range. Next, increase FPR to optimize productivity and tool life. Higher Vc will provide higher output but will reduce tool life. Try different combinations to find the parameters that best suit your needs.
Ball Nose Troubleshooting
| Concern | Possible Cause | Solutions |
|---|---|---|
| Insert wear at tip |
|
|
| Insert wear appears high (flank wear) |
|
|
| Insert Chipping |
|
|
| Built-up edge on insert |
|
|
| Poor finish/chatter |
|
|
| Tool shank breaks |
|
|
Dapra Ball Nose products are made in the USA.