Speeds and Feeds Speeds and Feeds CIM Product Development See teacher notes for instructions on how to play videos referred to in this presentation. Project Lead The Way, Inc. Copyright 2008

In This Lesson Discuss different cutting tools Learn the definition of speeds and feeds Calculate cutting speeds and feed rates Practice

Basic Cutting Tools Non-Center Cutting End Mill Ball End Mill Indexable Shell Mill Many different cutters are used during the milling process. The same cutting speed formula is used for each tool. Formula is presented on a subsequent slide.

Basic Cutting Tools Combination Drill & Countersink Spotting Drill

Flutes 4 Flute End Mill 2 Flute End Mill More cutting edges, longer tool life Used for harder metals Clogs easily in deep cuts More room for chip evacuation Used for light metals Weak, short tool life

Center vs. Non-Center Cutting 4 Flute Non-Center Cutting 2 Flute Center Cutting 4 Flute Center Cutting

Milling Tools Tool Description Application ¼” 2 Flute HSS Single End Mills For Cutting Aluminum – 3/8 Shank x 1 ¼ cutting length Facing, profiling, Pocketing, Slotting, Roughing and Finishing ¼” 2 Flute Ball End Mill for Aluminum – 3/8 shank x 1 ¾ cutting length Surfacing, Slotting, profiling, Roughing and Finishing

Milling Tools Tool Description Application ¼” Countersink & De-burring Tool – 90 Degree Engraving, De-burring, countersink, Spot drilling #3 Combined drill & countersink 90 Degree Spot drilling, Engraving

Spot drilling, Engraving Milling Tools Tool Description Application ¼” spotting drill 90 deg Spot drilling, Engraving

Cutting Tool Material Video Speeds and Feeds CIM Product Development Cutting Tool Material Video Play video: Cutting Tool Material Project Lead The Way, Inc. Copyright 2008

Speeds and Feeds CIM Product Development Definitions Cutter Speed – The rate of a tool measured in surface feet per minute. Spindle Speed – The number of revolutions per minute (RPM) that is made by the cutting tool of a machine. Feed – The distance advanced by the cutting tool along the length of the work for every revolution of the spindle. Cutter speed must be converted to inches per minute so that it can be expressed as RPMs. This gives us the spindle speed. Feed (or chipload) must be converted to inches per minute to give us the feed rate. Project Lead The Way, Inc. Copyright 2008

Spindle Feeds Formula Defined in revolutions per minute (RPM) Speeds and Feeds CIM Product Development Spindle Feeds Formula Defined in revolutions per minute (RPM) Found by dividing the cutter speed by the circumference of the tool CS (ft/min) C (in.) N = circumference S, the cutting speed, is obtained from a machinery handbook. A revolution is one complete rotation. This distance is called the circumference. The circumference of a circle is found by the formula d, where  is the constant value of approximately 3.14 and d is the diameter of the circle. In our formula, the diameter used is that of the tool being implemented. Cutter speed is defined in feet per minute while circumference is defined in inches. To convert so that the units match, we multiply feet by 12 since there are 12 inches in a foot. Different materials use different spindle speed rates. If the rate is too fast, the machine will wear out quickly. This can be expensive. If the rate is too slow, time is wasted. With some materials, the tool can actually bond to the material at slow speeds. This can also be costly. CS  12 (in./min) d (in.) N = Project Lead The Way, Inc. Copyright 2008

Recommended Cutting Speeds Speeds and Feeds CIM Product Development Recommended Cutting Speeds Milling Speeds for High Speed Steel Tools Material Cutting Speed in surface ft/min Magnesium 300 Aluminum 250 Brass and Bronze 150 Copper 100 Cast Iron (Soft) 80 Cast Iron (Hard) 50 Mild Steel 90 Cast Steel Alloy Steel (Hard) 40 Tool Steel Stainless Steel 60 Titanium High Manganese Steel 30 Note: Double Speed for Carbide Cutting Tools Notice how the speeds are slower as you look down the chart. Why? The materials are harder as you move down the chart. Project Lead The Way, Inc. Copyright 2008

Example What spindle speed should be used to mill aluminum with a ½ inch end mill? CS  12 (in./min) d (in.) N = Cutting Speed for Aluminum is 250 surface ft/min

Speeds and Feeds CIM Product Development Example What spindle speed should be used to mill aluminum with a ½ inch end mill? CS  12 (in./min) d (in.) N = Cutting speed for aluminum is 250 surface ft/min Start with the formula and substitute the known values. 250 ft/min  12   0.5 in. N = = 1910 RPM Project Lead The Way, Inc. Copyright 2008

Your Turn What spindle speed should be used to mill soft cast iron with a ¼ inch end mill? CS  12 (in./min) d (in.) N = Cutting speed for soft cast iron is 80 surface ft/min 80  12 N = = 1222 RPM  0.250

Calculating Feed Rates Fm = ft x nt x N Fm = Feed rate in inches/min ft = Feed in inches/tooth nt = Number of teeth on the tool CS  12 (in./min) d (in.) N = Spindle speed =

Recommended Tool Feed Speeds and Feeds CIM Product Development Tool Feed (in./tooth) Material Face Mill Side Mill End Mill Magnesium .005-.020 .004-.010 .005-.010 Aluminum Brass and Bronze .004-.020 Copper .004-.007 .004-.008 Cast Iron (Soft) .004-.016 .004-.009 Cast Iron (Hard) .002-.006 Mild Steel .002-.007 .002-.010 Alloy Steel (Hard) Tool Steel Stainless Steel Titanium High Manganese Steel Note: Double Speed for Carbide Cutting Tools Notice that there are three feeds for each material, depending on whether it is a face mill, a side mill, or an end mill. Also, each material has a range of values attached to it. Typically, you will use the smallest value to be on the safe side. Project Lead The Way, Inc. Copyright 2008

Example Feed Rate Fm = ft  nt  N Speeds and Feeds CIM Product Development Example Feed Rate Calculate the feed rate for end milling aluminum with a 2 flute, ½ inch HSS end mill. Fm = ft  nt  N Tool Feed (in./tooth) HSS stands for high speed steel. What is the tool feed for aluminum? ft=.005 in./tooth Project Lead The Way, Inc. Copyright 2008

Example Feed Rate Fm = ft  nt  N Fm = 0.005  2  1910 Calculate the feed rate for end milling aluminum with a 2 flute, ½ inch HSS end mill. Fm = ft  nt  N Ft = 0.005 in./tooth CS  12 (in./min) d (in.) 250  12 N = = = 1910 RPM   0.5 nt= 2 teeth Fm = 0.005  2  1910 Fm = 19 in./min

Your Turn Fm = ft  nt  N Fm = 0.005  4  1273 Fm = 25.46 in./min Speeds and Feeds CIM Product Development Your Turn Calculate the feed rate for face milling aluminum with a 4 flute, ¾ inch HSS end mill. Fm = ft  nt  N Ft = 0.005 in./tooth nt= 4 teeth CS  12 (in./min) d (in.) 250  12   0.75 = N = = 1273 RPM 1273 has been rounded. It is actually customary to wait until the last step to round. Fm = 0.005  4  1273 Fm = 25.46 in./min Project Lead The Way, Inc. Copyright 2008

Factors That Affect Feed Rates Speeds and Feeds CIM Product Development Factors That Affect Feed Rates Power of spindle motor Condition of cutting tool Depth of cut Quality of surface finish required Roughing vs. finish cuts Condition of the machine Strength of fixture We can mathematically calculate the feed rates, but other factors affect the speed rate as well. If your tool is dull, for example, it will cut slower. Project Lead The Way, Inc. Copyright 2008

Tool Feed Rate for Holes Speeds and Feeds CIM Product Development Tool Feed Rate for Holes Penetration rate in inches/revolution Tool Feed Rate (ipm) = ipr  RPM Feed in inches/minute The penetration rate is referred to as the drill feed. Spindle speed in revolutions/minute Project Lead The Way, Inc. Copyright 2008

Recommended Drilling Feeds Speeds and Feeds CIM Product Development Recommended Drilling Feeds Drilling Feeds Drill Diameter (in.) Drill Feed Rate (ipr) < ⅛ .001 – .002 ⅛ – ¼ .002 – .004 ¼ – ½ .004 – .007 ½ – 1 .007 – .015 > 1 .015 – .025 Again, we have a range of values for each diameter. Notice that the diameters are also in ranges of values. Project Lead The Way, Inc. Copyright 2008

Speeds and Feeds CIM Product Development Drill Feed Example What tool feed rate should be used for drilling a .375 inch hole in aluminum? Tool Feed Rate (ipm) = ipr  RPM CS  12 (in./min) d (in.) N = We will find RPM first since we have had prior experience with it. 250  12 =  0.375 = 2,546 RPM Project Lead The Way, Inc. Copyright 2008

Drill Feed The tool diameter is given in decimal form Drilling Feeds Speeds and Feeds CIM Product Development Drill Feed Drilling Feeds Drill Diameter (in.) Drill Feed Rate (ipr) < 0.125 .001 – .002 0.125. – 0.25 .002 – .004 0.25 – 0.5 .004 – .007 0.5 – 1 .007 – .015 > 1 .015 – .025 The tool diameter is given in decimal form The diameter is .375. To find the drill feed, we need to know where .375 inches falls on the chart. The easiest way to do this is to convert the chart to decimals, since these are common values. Since .375 is slightly larger than .25, we will choose a number higher than .004 We choose .005 (we could have chosen .004 to be on the safe side). Our drill feed would be 12.73 inches per minute. Tool Feed Rate (ipm) = ipr  RPM = 0.005  2546 = 12.73 ipm Project Lead The Way, Inc. Copyright 2008

Your Turn What tool feed rate should be used for drilling a .25 inch hole in copper? Tool Feed Rate (ipm) = ipr x rpm CS  12 (in./min) d (in.) N = 100  12 =  0.25 = 1,528 RPM

Drill Feed Our diameter is 0.25 Tool Feed Rate (ipm) = ipr  RPM Speeds and Feeds CIM Product Development Drill Feed Drilling Feeds Drill Diameter (in.) Drill Feed Rate (ipr) < 0.125 .001 – .002 0.125. – 0.25 .002 – .004 0.25 – 0.5 .004 – .007 0.5 – 1 .007 – .015 > 1 .015 – .025 Our diameter is 0.25 Since .25 is a limit, we choose the value assigned to it. In either case, that value is 0.25. Tool Feed Rate (ipm) = ipr  RPM = 0.004  1528 = 6.1 ipm Project Lead The Way, Inc. Copyright 2008

Special Operations CS  12 (in./min) N = d (in.) Speeds and Feeds CIM Product Development Special Operations CS  12 (in./min) d (in.) N = Other special operations require slower speeds: Reaming – ½ to ⅔ of that used for drilling the material Counterboring – ¼ of that used for drilling the material Countersinking – ¼ of that used for drilling the material Tapping (threading) – Determined by many factors (usually range from 50 to 300 RPM) There are some circumstances that require speeds slower than the one obtained from the formula. In tapping, there is no special formula. Project Lead The Way, Inc. Copyright 2008

References Kibbe, R.R., Neely, J.E., Meyer, R.O., & White, W.T. (2002). Machine tool practices. Upper Saddle River, NJ: Prentice Hall. Oberg, E., Jones F. D., Horton, H. L., & Ryffell, H. H. (2000). Machinery’s handbook (26th ed.). New York, NY: Industrial Press Inc.