Home » Mold Tooling » Speeds & Feeds

Technical Information - Speeds & Feeds

CALCULATION OF SPINDLE SPEED FOR BALL NOSE TOOLS

  1. Choose the cutter diameter and depth of cut (DOC) you want to run.
  2. From the chart above find the “effective cutter diameter’,(De). If your workpiece is relatively flat, use the diameter directly from the chart.
  3. If your workpiece has steep walls, the effective cutter diameter must be further calculated. This “compromise diameter” can be found by averaging the “chart”
    Example: 0.500” insert; 0.020” DOC; workpiece with steep walls De from chart = 0.196“ compromise dia. = (0.196 + 0.500) / 2 = 0.348”
  4. Pick a cutting speed (SFM) from the "Speed Chart" based upon your workpiece material type and hardness. Note: pick a speed slightly above the middle of the corresponding range.
    Example: Alloy Steels and Tool & Die Steels: 350HBN 300-750 SFM ... Pick: 550 SFM
  5. Calculate RPM. RPM = (SFM x 3.82) / Effective Cutter Dia.
    Example: RPM = (550 x 3.82)/ 0.348 = 6037 ... To achieve an average of 550 SFM while milling at a depth of 0.020" with a 1/2" diameter tool cutting a steep walled work piece of P20 at 35 HRc (350 HBN).

FEED RATE CALCULATION

Once you have calculated your spindle RPM, you can now calculate the appropriate feed rate.

  1. Select an appropriate chip thickness for the material type and hardness you are cutting. Note that one should start at the smaller end of the scale for safety reasons. Cutters smaller than 1/2” (12mm) should decrease the chart numbers by as much as 50%.
    Example: Using the same criteria as the spindle speed calculation, RPM = 6037; from the chart, chip thickness is 0.005", and all of our ball nose finishers have 2 flutes. i.e.- 6037 x 0.005 x 2 = 60.37 IPM
  2. Your FEEDRATE (inches per minute) can be calculated by the formula: RPM x chip thickness x # of flutes.

Calculate De = Effective Cutting Diameter

Calculate DE = Effective Cutting DiameterDE
Insert Diameter
DOC 0.250 0.312 0.375 0.500 0.625 0.750 1.00 1.250
0.005 0.070 0.078 0.086 0.099 0.111 0.122 0.141 0.158
0.010 0.098 0.110 0.121 0.140 0.157 0.172 0.199 0.223
0.020 0.136 0.153 0.169 0.196 0.220 0.242 0.280 0.314
0.050 0.200 0.229 0.255 0.300 0.339 0.374 0.436 0.490
0.075 0.229 0.267 0.300 0.357 0.406 0.450 0.527 0.594
0.100 0.245 0.291 0.332 0.400 0.458 0.510 0.600 0.678
0.125 0.250 0.306 0.354 0.433 0.500 0.559 0.661 0.750
0.156 0.312 0.370 0.463 0.541 0.609 0.726 0.826
0.188 0.375 0.484 0.573 0.650 0.781 0.894
0.250 0.500 0.612 0.707 0.866 1.00
0.312 0.625 0.739 0.927 1.082
0.375 0.750 0.968 1.146
0.500 1.000 1.225
0.625 1.250

Steep & Flat Workpieces

Steep and Flat Workpieces

Speed Chart (SFM)

Material Hardness (HBN) Cutting Speed (SFM) Chip Thickness Ranges*
Uncoated Coated
Plain Carbon Steels 50-180 70-700 400-950 (0.004-0.012)
180-330 200-500 350-800 (0.004-0.012)
Alloy Steels and Tool 130-330 200-450 350-800 (0.003-0.011)
& Die Steels 330-450 300-700 (0.003-0.011)
Stainless Steels
200 & 300 Series 130-330 200-400 250-600 (0.004-0.012)
400 & 500 Series 130-330 200-450 250-575 (0.003-0.011)
330-420 150-300 200-450 (0.003-0.011)
PH Series 140-380 180-250 250-550 (0.003-0.010)
Grey Cast Irons 110-320 300-500 350-650 (0.003-0.014)
Ductile & Maliable Cast Iron 120-330 250-450 300-620 (0.003-0.011)
Nickel Base Alloys 140-380 50-250 (0.002-0.009)
Titanium Alloys 110-300 100-240 135-380 (0.003-0.010)
300-400 80-200 100-280 (0.003-0.010)
Aluminum-Low Silicone 750-1800 800-3500 (0.003-0.018)
Aluminum-High Silicone 250-800 300-1000 (0.003-0.018)
Graphite 450-1000 800-1500 (0.003-0.016)

*Chip Thickness Chart

DOC is less than 50% of insert diameter.

Chip Thinning Multiplier

Compensate the feed rate for the chip thinning that occurs. This is a function of the ratio between the insert diameter and the depth of cut. DO NOT USE the feed rate compensation or the effective cutting diameter chart when side wall milling. Your feed rate compensation can be calculated by: (D(insert ) / De(from chart)) x IPM from above calculation. 0.005", which helps promote tool life.