90° Square Shoulder Reference & Technical Information

Application Information

Technical Considerations

Recommendations

Optimizing Cutting Performance

Dapra's high-performance cutters work best when allowed to perform within their designed operating parameters. Adhering to the following steps will ensure that you are getting the most from your investment.

  1. Refer to the Feed and Speed Chart (see below) to find the recommended Surface Feet per Minute (SFM) and Feed per Tooth (FPT) at which to run your cutter, based on the material to be machined.
  2. Use the following formula to determine the Revolutions per Minute (RPM) for your cutting tool:
    (SFM x 3.82) / Tool Dia. = RPM
    Example: A 2" diameter tool operating at 900 SFM (900 x 3.82) / 2 = 1720 RPM
  3. Use the following formula to determine the feed in Inches per Minute (IPM) to be programmed into the machine tool: FPT x RPM x N (number of teeth in cutter) = Feed
    Example: A 5-flute cutter at .008" FPT (.008 x 1720) x 5 = 69 IPM
  4. If the Width of Cut (WOC) < 1/2 the cutter diameter, use the feed rate compensation chart (below) to compensate for chip thinning.
Width of Cut
Width of Cut (WOC)
(% of tool Ø)
50% or > 40% 30% 20% 10%
Feed Rate Multiplier 1 1.02 1.1 1.25 1.7

After determining the percentage of WOC for the tool diameter, multiply the desired feed rate by the corresponding 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" dia. end mill @ .100" WOC, the WOC = 10% of the cutter diameter.
Using the chart above, the factor for the chip thickness = 1.7.
If a chip thickness of .005" is desired, a feed rate of .0085" (.005 x 1.7) should be programmed into the machine tool.

or

Adjusted Feed per Tooth (AFPT) = desired chip thickness x chip thinning factor (from chart).

Hole Diameter Calculation

Hole Dia. Calculation
Part Number Min. Hole Dia. Max. Hole Dia.
SSEM0500-R35-1 0.63" 1.00"
SSEM0625-R35-2 0.78" 1.25"
SSEM0750-R35-2 1.03" 1.50"
SSEM0625-R45-1 0.75" 1.25"
SSEM0750-R45-2 0.88" 1.50"
SSEM1000-R45-3 1.38" 2.00"
SSEM1250-R45-4 1.88" 2.50"
SSEM1500-R45-5 2.38" 3.00"
SSEM1000-R55-2 1.28" 2.00"
SSEM1250-R55-3 1.78" 2.50"
SSEM1500-R55-3 2.28" 3.00"
SSSM2000-R55-5 3.28" 4.00"
SSSM2500-R55-5 4.28" 5.00"
SSSM3000-R55-6 5.28" 6.00"
SSSM4000-R55-8 7.28" 8.00"
SSSM5000-R55-8 9.28" 10.00"
SSSM6000-R55-7 11.28" 12.00"

Smaller holes may be interpolated by predrilling. Typical recommended ramp angle is 1° or less.

Helical Interpolation for Larger Diameter Hole Making

Larger diameter hole making can be quick and easy when a Square Shoulder 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. The 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 Square Shoulder Mills

Square Shoulder 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 Square Shoulder catalog PDF.

Square Shoulder 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
  • Consider different insert
Insert chipping
  • Surface footage is low
  • Incorrect grade or coating
  • Using sharp edge insert incorrectly
  • Feed too high
  • Verify correct speed and feed
  • Increase spindle speed
  • Decrease feed rate
  • Change insert selection
  • Decrease DOC
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
  • Inadequate tool holding
  • Use Carbide Core cutter body
  • 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