High-Velocity Milling Reference & Technical Info
Application Information
Technical Considerations
- Always use anti-seize compound on screws.
- Thoroughly clean pocket and screwat each insert change.
- Change insert screw every 10 inserts.
- Use the shortest length tool holder possible for maximum rigidity; the shank of the cutting tool (end mill) should be up inside the machine spindle taper whenever possible.
- Use tool holders appropriate for roughing operations: end mill holders and power chucks are recommended; collets are not recommended.
Recommendations
- Climb mill whenever possible.
- Ramp entry should be used for solid pocketing, 1° to 2° recommended.
- Excellent for helical interpolation applications.
- Facing mills are measured by their Width of Cut (WOC) capability at the bottom of the cut.
- WOC should be 60-75% of cutter diameter when soft milling. Use 30% width of cut for hard milling.
- Round inserts provide a very strong cutting edge and the ability to machine much closer to finish size. Utilize high speeds and feeds with light Depth of Cut (DOC) to take advantage of these benefits. High metal removal rates will be achieved without high horsepower consumption.
- Use the Feed Rate Compensation chart below to compensate for chip thinning that occurs with round inserts; this will provide for optimum metal removal rates and tool life. The lighter the DOC, the more critical feed compensation becomes.
- Utilize flat-top (T-Land) style inserts for most steel and cast iron applications and sharper edge (Dished) inserts for nonferrous (including stainless steel) applications.
High-Velocity Cutting Edge Compensation
Dapra’s High-Velocity Mills, with a round or 45° cutting edge, are specifically designed to thin the chip formed during the cutting process, which allows for higher cutting feeds. The following charts provide valuable information regarding compensation for chip thinning.
Compensation for Round Cutting Edge (Round Inserts)
After determining the desired chip thickness, find the insert diameter and Depth of Cut (DOC) intersection in the chart at right. Multiply the desired chip thickness by the factor shown in the chart. This will be the Adjusted Feed per Tooth (AFPT), resulting in a true chip thickness of the desired amount.
Example: If using a 2" High-Velocity Shell Mill with the 5/8" I.C. inserts @ .03" DOC, the factor for chip thinning = 2.3. So, if a chip thickness of .005" is desired, a feed rate of .0115" (.005 x 2.3) needs to be programmed into the machine tool.
or
Adjusted Feed per Tooth (AFPT) = chip thickness x chip thinning factor (from chart)
 |
|||
 |
5/8" | 3/4" | |
|---|---|---|---|
| 0.005 | 5.6 | 6.1 | |
| 0.010 | 4.0 | 4.4 | |
| 0.015 | 3.3 | 3.6 | |
| 0.020 | 2.8 | 3.1 | |
| 0.025 | 2.6 | 2.8 | |
| 0.030 | 2.3 | 2.6 | |
| 0.035 | 2.2 | 2.4 | |
| 0.040 | 2.0 | 2.2 | |
| 0.050 | 1.8 | 2.0 | |
| 0.060 | 1.7 | 1.8 | |
| 0.075 | 1.5 | 1.7 | |
| 0.085 | 1.5 | 1.6 | |
| 0.100 | 1.4 | 1.5 | |
| 0.125 | 1.3 | 1.3 | |
| 0.150 | 1.2 | 1.3 | |
| 0.180 | 1.1 | 1.2 | |
| 0.200 | NR | 1.1 | |
| >0.200 | NR | NR | |
Compensation for 45° Lead Angle (Octagonal Inserts)
For all Depths of Cut:
Multiply desired chip thickness by 1.4 for Adjusted (programmed) Feed per Tooth (AFPT).
Example: For .007" chip thickness, feed @ .010" (.007 x 1.4 = .010)
Recommended Cutting Speeds & Feeds for High-Velocity Face Mills
Click here or on the chart above for a larger version (opens in a new window).
This chart is also part of our High-Velocity Face Milling catalog PDF.
High-Velocity Milling – Troubleshooting
| Concern | Possible Cause | Solutions |
|---|---|---|
| Insert wear appears high (flank wear) |
|
|
| Insert chipping |
|
|
| Built-up edge on insert |
|
|
| Poor finish/chatter |
|
|
| Tool shank breaks |
|
|
Dapra High-Velocity products are made in the USA.