Toroid Cutting Tool Reference & Technical Info
Application Information
Technical Considerations
- Always use anti-seize compound on screws.
- Thoroughly clean pocket and screw at each insert change.
- Change insert screw every 10 inserts.
- Use the shortest-length tool holder (end mill holder) for maximum rigidity; the shank of the cutting tool 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
- Tool is most appropriate for "Z-level" roughing; plunge to Depth of Cut (DOC) and clear entire level.
- End Mills – plunge rate should not exceed .010" per revolution (.005" per tooth).
Shell Mills – ramping is recommended (less than 5°). - Minimum diametric plunging engagement is 75% of cutter diameter.
- Width of Cut (WOC) should be 60-75% of cutter diameter whenever possible, creating a "scalloping" effect (end mills only) between passes, especially with longer length tools.
- Plunging creates a long, continuous chip; use a peck cycle with full withdrawal to break and evacuate this chip when plunging to depths greater than .150".
- The 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 DOC to take advantage of these benefits. High metal removal rates will be achieved without high horsepower consumption.
- Use the Feed Rate Compensation 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.
- Precision-ground inserts are accurate to within .0005", making this cutter excellent for semifinishing using profiling or raster-type cutter paths.
- When using high-feed inserts (HFDCH) ramp at 30-50% of the X-Y feed and maintain no more than a 2° ramp angle.
Feed Rate Compensation for Button Cutters (Round Inserts)
After determining the desired chip thickness (MMPT – see chart below), find the insert diameter and Depth of Cut 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 1" Toroid end mill with the 1/2" inserts @ .03" Depth of Cut (DOC), the factor for the chip thickness = 2.1.
So, if a chip thickness of .005" is desired, a feed rate of .0105" (.005 x 2.1) needs to be programmed into the machine tool.
or
Adjusted Feed per Tooth (AFPT) = chip thickness x chip thinning factor (from chart)
 |
|||||
 |
3/8" | 1/2" | 5/8" | 3/4" | |
|---|---|---|---|---|---|
| 0.005 | 4.4 | 5.0 | 5.6 | 6.1 | |
| 0.010 | 3.1 | 3.6 | 4.0 | 4.4 | |
| 0.015 | 2.6 | 2.9 | 3.3 | 3.6 | |
| 0.020 | 2.2 | 2.6 | 2.8 | 3.1 | |
| 0.025 | 2.0 | 2.3 | 2.6 | 2.8 | |
| 0.030 | 1.8 | 2.1 | 2.3 | 2.6 | |
| 0.035 | 1.7 | 2.0 | 2.2 | 2.4 | |
| 0.040 | 1.6 | 1.8 | 2.0 | 2.2 | |
| 0.050 | 1.5 | 1.7 | 1.8 | 2.0 | |
| 0.060 | 1.4 | 1.5 | 1.7 | 1.8 | |
| 0.075 | 1.3 | 1.4 | 1.5 | 1.7 | |
| 0.085 | 1.2 | 1.3 | 1.5 | 1.6 | |
| 0.100 | 1.1 | 1.3 | 1.4 | 1.5 | |
| 0.125 | 1.1 | 1.2 | 1.3 | 1.3 | |
| 0.150 | NR | 1.1 | 1.2 | 1.3 | |
| 0.180 | NR | NR | 1.1 | 1.2 | |
| 0.200 | NR | NR | NR | 1.1 | |
| >0.200 | NR | NR | NR | NR | |
Feed Rate 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)
Operating Instructions for High-Feed Inserts
High-feed milling creates significant chip thinning due to an extreme lead angle. Feed rates must compensate for this to maximize productivity. The figure at left shows an example of this condition. Use the chart below to determine the compensation factor by which to multiply the desired chip thickness to arrive at your actual feed per tooth (FPT).
| Depth of Cut | Compensation |
|---|---|
| Up to .030" | 5x |
| .030" - .040" | 4x |
| .040" - .050" | 3.5x |
Example: If cutting at .030" DOC and trying for a .010" chip thickness, multiply .010" x 5 = .050" FPT.
A – .050" DOC, Chip Thickness = .021"
B – .040" DOC, Chip Thickness = .018"
C – .030" DOC, Chip Thickness = .015"
D – at .060" FPT & DOC shown above
Hole Diameter Calculation
| Toroid Shell Mill Part Number |
Min. Hole Dia. | Max. Hole Dia.* |
|---|---|---|
| TRSM200-075-R4-4 | 3.25" | 4.00" |
| TRSM200-075-R5-3 | 3.06" | 4.00" |
| TRSM250-100-R5-4 | 4.06" | 5.00" |
| TRSM300-100-R4-6 | 5.25" | 6.00" |
| TRSM300-100-R5-5 | 5.06" | 6.00" |
| TRSM400-150-R4-7 | 7.25" | 8.00" |
| TRSM400-150-R5-6 | 7.06" | 8.00" |
Formulas:
Minimum Hole Dia.:
(Tool Dia. x 2) - (1.5 x Insert Dia.)
Maximum Hole Dia.:*
Tool Dia. x 2
* Not recommended. At this diameter, the center tip is at its maximum. It is suggested that you stay slightly under this number.
Helical Interpolation for Larger Diameter Hole Making
Larger diameter hole making can be quick and easy when a Toroid Cutter is used in combination with helical interpolation. This technique resembles thread milling in that all three axes (X, Y and Z) are in motion simultaneously. It differs from thread milling in that the tool is introduced into the material without a start hole of any kind. The tool simply is positioned at the inside diameter of the hole to begin its helix from there, achieving complete material removal from the hole by ramping down to the final depth. This smooth operation tends to avoid the high horsepower consumption characteristic of large diameter hole making. And with the high clearance angles of Toroid cutting tools, ramp angles during helical interpolation can be aggressive, without concern for rubbing the bottom of the cutting edge. This quick and easy process offers the added advantage of allowing many different hole sizes to be generated with the same diameter tool. Hole size variation is all in the programming.
Click here for more information on how Helical Interpolation can improve your manufacturing efficiency, or contact your Dapra Applications Specialist.
Recommended Cutting Speeds & Feeds for Toroid Cutting Tools
Click here or on the chart above for a larger version (opens in a new window).
This chart is also part of our Toroid catalog PDF.
Toroid Cutter 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 Toroid products are made in the USA.