Toroid Cutting Tool Reference & Technical Info

Application Information

Technical Considerations

Recommendations

Feed Rate Compensation (Round Inserts)

After determining the desired chip thickness (FPT – 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)


Insert Diameter
Depth of Cut   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).

Compensation for 45-degree lead angle

Example:
For .007" chip thickness, feed @ .010" (.007 x 1.4 = .010)

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

Toroid Recommended Cutting Speeds

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

Troubleshooting
Concern Possible Cause Solutions
Insert wear appears high (flank wear)
  • Not enough chip load
  • Surface footage is high
  • Incorrect grade or coating
  • Verify correct speed and feed
  • Increase feed rate
  • Decrease RPM
  • Increase DOC
  • Use Harder Grade
Insert chipping
  • Surface footage is low
  • Incorrect grade or coating
  • Using dished insert incorrectly
  • Feed too high
  • Verify correct speed and feed
  • Increase spindle speed
  • Decrease feed rate
  • Decrease DOC
  • Use T-Land insert
  • Use tougher grade
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
  • Use coolant
Poor finish/chatter
  • Cutter hung out too far
  • Excessive runout
  • Inadequate tool holding
  • Reduce tool gage length
  • Check tool holder wear
  • Use high-rigidity tool holder
Tool shank breaks
  • Tool pressure too great
  • Fatigued cutter body
  • Decrease DOC
  • Reduce tool gage length
  • Decrease feed rate

A Proud USA Manufacturer