Traditional machining is characterized by the production of chips. The chips are formed by a shearing process. This is contrary to the old misconception of viewing the tool moving through the material like an axe splitting wood. Instead, a better analogy is a deck of cards, sliding on top of one another. The tool causes the chip to slide along a shear plane. As the tool advances, so does the shear plane.
Note figures from Kalpakjian, Fig 8.4, p 478. He gives source as “After M. Shaw” As was mentioned before, machining involves chips. In traditional machining, these chips are removed from the material by a cutting tool. Even in abrasive processes, such as grinding, each tiny particle of abrasive can be viewed as a tool. Chips can be classified into 3 different basic types: 1 Continuous 2 Built Up Edge 3 Serrated and Discontinuous (Some consider the serrated and discontinuous chips to be separate types) Continuous chips generally result from high cutting speeds and/or high rake angle. They generally result in good surface finish. However, they are not always desirable as they have a tendency to tangle. For this reason a chip breaker is often used. A chip breaker can be an extra curve cut in the tool which will cause the chip to bend and ultimately break off into shapes like a number or figure nine. These figure 9 chips are indicative of a good cut. Built Up Edge (BUE) forms at the tool tip as layers of workpiece are deposited. Eventually it gets too large and breaks up, which will then mess up surface finish. BUE changes the cutting geometry and gives a poor surface finish. Generally quite undesirable, although very thin stable BUE is good as it preserves tool life. BUE is more likely with strain hardening materials, less likely with higher cutting speeds Serrated (segmented, inhomogeneous) chips have zones of high and low strain. Occurs in metals with low thermal conductivity and strength that decreases sharply with temperature. Discontinuous chips are segments which are loosely or firmly attached. They are seen in brittle workpieces, materials with impurities, at very low or very high cutting speeds and with non lubricated cutting. When machining, we want to plastically deform by shearing the workpiece. When the material can not handle the deformation, the chip fractures giving a discontinuous type chip.
The Relief angle is the angle between the trailing edge of tool and the workpiece. It is also called the clearance angle. Clearance is important because it drags the trailing edge of the tool along the workpiece, builds up heat, causes poor surface finish and reduces tool life. Shear angle is the angle along which the material shears. Notice that the actual chip thickness (given by t C ) is always greater than the nominal chip thickness (given by t O ). The shear angle is partially dependent on the material, but we can also affect it through the rake angle and lubrication. If we can decrease the coefficient of friction, the chip Free Body Diagram shows an increase in the shear angle results. This leads to a decrease in shear work in addition to the decrease in heat lost to friction. Lastly there is the rake angle, which is angle that the leading edge of the tool makes with the workpiece normal. On this diagram one sees basically three areas of interest when studying the chip formation process. The first “zone” is along the shear plane. In order to plastically deform the workpiece, we are concened with plastic flow and the characteristics (especially with regard to shear) of the metal being cut. The second “zone” is along the tool face chip interface. We are concerned with friction and wear characteristics. Finally, the third zone is the interface between the trailing edge of the tool and the already machined workpiece. Here, in addition to the wear, we are also aware of the surface roughness and residual stresses that are produced.
The rake angle is a very important factor in machining. Larger or positive rake angles result in smaller shear strains in the workpiece. Positive rake angles generally produce continuous chips and good surface finishes. However cutting tools with positive rakes are structurally weaker and more apt to have a cutting tooth break or chip. Smaller or negative rakes result in larger shear strains in the workpiece. Negative rakes are stronger, but are much more likely to produce BUE or discontinuous chips. The surface finish is usually poorer with negative rakes, although they can have good finish at higher speeds. (Carbide inserts usually have a negative rake to minimize breaking/chipping) Note that this picture is a 2-D cutter-- ie everything can be viewed as taking place in a plane. Most cutting is actually 3-D-- the cutter is oblique to the velocity. This basically results in 2 rake angles and 2 relief angles as well. Shaw describes how to combine the 2 angles, and determine an effective rake. As the cutter is increasingly inclined to the velocity, the effective rake angle increases. However, the net coefficient of friction drops as the angle of inclination increases. In purely orthogonal cuts, friction increases with rake. Examples of 3-d cutters are most lathe cutters, HELICAL milling cutters, etc.
There are many different types of tool wear. Two common types of wear are crater wear and flank wear. As seen in this figure, in crater wear, the tool wear is on the top or front surface of the tool. Flank wear wears the bottom of the tip surface.
In vertical milling, two key parameters for cutting are depth of cut and step over distance. For clarity, we distinguish between the step over distance and depth of cut. Depth of cut is measured normal to the workpiece. Step over distance is measured in the work surface (but perpendicular to the feed direction). When milling it is also called the radial depth of cut. Step over distance has a great effect on surface finish. In particular, when using a ball end mill to machine a flat surface, step over distance must be kept quite small to minimize the “scallops” formed between the centerlines of the cutter paths.
Feeds and speeds are often given in the form of look-up tables. Here, some base data are given for milling machines, and several other types of cutters. Values for the speeds found in these tables are those at which the material may be machined efficiently.
These table recommend the feed rates for milling machines with several types of cutters. Also, notice the table for the lathe. From the Machine and Machine tool presentation, the geometry of a cutter on a lathe is radically different from that of one on a milling machines. Feed rates are markedly different, and some differences exist in speeds as well. Recall that values for the speeds are those at which the material may be machined efficiently.
This information on this slide gives the recommended feed and speeds for drilling.
FW Taylor studied the effects of the feed, depth of cut, and cutting speed on the machining process and found: 1) Cutting Speed is the dominating factor in determining tool life, Feeds and Depths of Cut are the dominant forces in determining the force acting on the tool In the “typical operating range”, tool life (T) and cutting speed (V) are related according to Taylor’s Equation: Cutting speed times tool life raised to the nth power = C, where n and C are experimentally determined constants. Taylor recommended using the maximum allowable feed and depth of cut, then selecting the cutting speed, V, to balance tool wear with cycle time for the process.
Many machines have the cutter on a rotating shaft, or in a rotating spindle. You may be given cutter speed in SFM (surface feet per minute), but need to know how many RPM (revolutions per minute) this is, as you are able to directly control the RPM. Use the basic relationship velocity,v, equal angular velocity times r or = v/r in order to determine the speed in RPM. Note that you must use the largest effective cutting diameter. Thus if you have a stepped drill bit, use the larger OD. If you are using a ball end mill and making very shallow cuts so that the full diameter of the tool is well above the work surface, you should determine the effective diameter of the cutter at the top of the workpiece. Values you look up are those at which the material may be machined efficiently. The optimum cutting speed for any job should balance the metal removal rate and the cutting tool life. Of course there are many factors which influence the cutting speeds. They include: The type of work material The cutter material The diameter of the cutter The surface finish required The depth of cut being taken The rigidity of the machine & the workpiece set-up NOTE: book values are useful- but are ONLY a starting point.
How do you determine the diameter to use in the speed formula. It is 2 times the radial distance from the axis of revolution to the point where the tool and workpiece contact. ( Read slide to determine effective diameter)
Book values generally give the APT or advance per tooth for a full RADIAL depth of cut (at least 1/2 the tool diameter). To convert this into SFM (surface feet per minute), you need the number of teeth on the cutter and the cutter speed (rev/min). (Note, lathe cutters generally have just 1 tooth.) Actually what you really want to control is the so called chip load or nominal chip thickness (Notice NOMINAL NOT ACTUAL thickness). In end or face milling if the step over distance is at least 1/2 the tool diameter, then the chip load and APT are the same. However if the step over distance is much less than 1/2 the tool diameter, the chip load will be much less the the APT. Since you really want to control the chip load, you must increase the APT to keep the correct size chip load. Just as with cutting speeds, the optimum feed rate should balance the metal removal rate and the cutting tool life. Further, like cutting speeds many factors affect the feed rate, included among these are: The depth and width of cut The type of cutter The sharpness of the cutter The workpiece material, its strength and uniformity The type of finish & accuracy required The power & rigidity of the machine & the workpiece set-up NOTE book values are useful- but are ONLY a starting point.
Figures from Kibbe, Fig O-47 and O-48, pg 777 If one were looking at an end milling cutter normal to the workpiece, we notice how a small step over distance cause a much smaller chip load. (They call chip thickness here, but it is not the actual chip thickness. It is really just the nominal chip thickness, or chip load.)
This slide depicts the sort of “double whammy” of using a shallow cut with a ball nosed end mill. In the first place, the effective cutting diameter will not be the full diameter of the tool, but will be something less. As a result, higher spindle RPMs are required for the desired surface cutting speed. Further, due to the so called radial chip thinning effect, the chip load will be less than the advance per tooth. As a consequence, you will have to increase the feed rate in order to maintain the correct chip load.
Figure O-51, Machine Tool Practices 5 th Ed, Kibbe, et al., p. 779. Here we see the Radial Chip Thinning Factor for a Ball Nosed End Mill with small depths of cut (this time, the depth of cut is in conventional usage). Note that with a ball nosed end mill, one must also account for the change in effective diameter with shallow cuts. This affects the cutting speed (as well as feed rates).
Figure O-49, Machine Tool Practices 5 th Ed, Kibbe, et al. p. 778 Here is a chart allowing you to obtain the radial chip thinning factor given the cutter diameter and the radial Depth of cut. (Note that depth of cut should be Radial Depth of Cut or Step Over Distance, it is NOT what we have previously referred to as the depth of cut.)
Tables for Radial Chip Thinning can be found in Kibbe, Fig O-49, p778 and Fig O-51, p779. Table and chart are attributed to Ingersoll Cutting Tool Company. One can use the chip thinning value with the chip load to get the actual APT, then plug this into the standard feed formula. Recall that the chip load is the APT at full (1/2 the tool diameter or more) step over distance. If you fail to use the R CTF when appropriate, the feed rate is likely to be too low. This often causes the cutting edge of the tooth to rub instead of cutting, which will reduce tool life (by increasing the tool wear). Low feed rates can also produce chatter. At the proper feed (obtained with the R CTF ), the tool really cuts. Sometimes books will list different feeds at different step over distances-- these have incorporated R CTF .
Feeds and speeds are often given in the form of look-up tables. Here, some base data is given for milling machines, and several other types of cutters. Values for the speeds you look up are those at which the material may be machined efficiently.
In these simple examples, one can more or less “plug and chug” into the basic formulas. The look up values are obtained from the following: Example 1, Cutting Speed from Table 61-1- Kenametals Feed Rate from Table 61-2- Kenametals Example 2, from Table I-5 Kibbe et al. All of these tables are on the two slides of feeds and speeds
In this second example, we need to estimate the depth of cut, the cutting speed, and feed rate required when rough turning a bronze shaft, from a diameter of 2.000” to 1.800.” Knowing the initial and ending diameter, we can determine the depth of cut. Then we can return to our tables to calculate for feeds and speeds.
From the feed&speeds table, the cutting speed for roughing bronze is 100 sfm and feed rate is 0.010 ipr
In these simple examples, one can more or less “plug and chug” into the basic formulas. The look up values are obtained from the following: Example 1, Cutting Speed from Table 61-1- Kenametals Feed Rate from Table 61-2- Kenametals Example 2, from Table I-5 Kibbe et al. All of these tables are on the two slides of feeds and speeds
Here you must be a little more detailed. First you must estimate the effective cutting diameter. Then, you must look up the Radial Chip Thinning Factor, and then, you can solve the problem. The R CTF is obtained from table O-51, p 779 Kibbe, et al. Notice how much smaller the effective diameter is, and the fairly small Radial Chip Thinning Factor. These are important here. Note that the values for the feeds and speeds are from the lecture slides cutting speed from Table 61-1 Kenametals feed rate from Table 61-2 Kenametals
Again, from the tables, the cutting speed for a high speed steel cutter used on a tool steel workpiece is 60 sfm. The feed per tooth on the end mill is recommended to be .005”.
Using the data from the previous slide, the speed may be calculated to be 690 rpm.
Figure O-51, Machine Tool Practices 5 th Ed, Kibbe, et al., p. 779. Here we see the Radial Chip Thinning Factor for a Ball Nosed End Mill with small depths of cut (this time depth of cut is in conventional usage). From this table, the Rctf for the 0.5” nominal tool diameter with an effective diameter of 0.33” is 0.7 in.
Now the feed rate can be calculated as 9.9 inches per minute
(Data from Kalpakjian, p. 516) When talking about materials, people often discuss its machinability. In general machinability involves 3 factors-- Surface Finish (and integrity) after machining, life of the machining tool, and the force and power requirements while machining. Additionally the type of chip produced is sometimes included in the machinability. Machinability ratings are based on tool life. The standard currently used is “free cutting” steel- AISI 1112. When machining at 100 SFM (cutting speed), the machining tool life is 60 min. (Faster speeds would decrease tool life, slower speeds would increase the tool life). It is assigned a machinability ranking of 100 (100 SFM). Other materials are ranking based on the cutting rate which will give a tool life of 60 min under similar circumstances. Higher machinability rankings mean the material is more machinable.
Frequently, estimates of cutting forces or powers are needed One can get accurate values for a given process using a dynamometer but it is not practical (or possible) to test each case. The “specific energy of machining” (energy to remove a unit volume of material), u, is constant Similar concept is discussed powers are from Table 8.4 in Kalpakjian, p 496. NOTE that these calculations give the values needed at the workpiece-tool interface. Most machines are rated in terms of the power at the motor. Losses are always present. Losses are briefly discussed in Kibbe, p611-612 Kibbe estimates typical losses in a machine tool at 20-50% from the motor to the spindle.
This data is from M.C. Shaw (Metal Cutting Principles, Oxford: Clarendon Press, 1984. p 43.) Shaw says that the total energy per unit volume (or specific energy as Kalpakjian calls it) is dependent on 3 basic parameters. 1) Nominal (or undeformed) chip thickness 2) Rake angle (recall that increasing the rake angle decreases the cutting forces and powers) 3) Chemistry and hardness of the material Nominal, or undeformed, chip thickness-- the specific energy is roughly inversely proportional to the tenth root of the square of the thickness Specific energies of machining vary roughly proportionally with workpiece hardness, the table given (from table 3.3 in Shaw’s work) give the correct values for materials of “average” hardness within each class. (Thus the equation given makes no mention of hardness.) Power requirements can also be experimentally determined. Recall that power is another part of the machinability of a material. Thus, in general, materials with higher machinability ratings should have lower power requirements.
Here you simply need to find the total energy. Thus a volumetric rate is NOT needed. Instead, you must find the total volume of the material removed. Then the total energy is simply specific energy times volume.
In this presentation, we have learned much about traditional machining parameters. For chip removal, the tool orientation greatly affects the material surface, the tool life and the failure. Key factors for tool orientation are: rake angles, clearance angles, and shear angles. For milling and turning, the key parameters are the effective diameter, depth of cut, radial depth of cut (if applicable), speeds (tip and spindle), feed rate, material, tool material and energy. All these are important factors to determine the appropriate tools and parameters to machine efficiently and effectively.
Transcript
1. Traditional Machining
2. Chip Formation (Traditional Machining) In any traditional machining process, chips are formed by a shearing process Ref: Manufacturing Processes for Engineering Materials by S. Kalpakjian, Addison Wesley, 2nd Ed., 1991 Shear Plane Shear Plane Shear Plane
3. Chip Types Continuous Built Up Edge (BUE) Discontinuous Segmented BUE Ref: Manufacturing Processes for Engineering Materials Fig 8.4, p 478.
4. Tool Geometry The shape and orientation of the cutting tool greatly affects the chip formation mechanics
5. Rake Angle Of particular importance is the rake angle that the tool makes with the workpiece normal Positive Rake Neutral Rake Negative Rake Workpiece Normal + + Cutter Velocity Workpiece Normal 0 Cutter Velocity - Cutter Velocity Workpiece Normal
6. Tool Wear
7. Cutting Parameters (Vertical Milling) Depth of Cut - measured along workpiece normal Step over Distance - (also called radial depth of cut)- Measured in tangent plane of workpiece and perpendicular to cutter travel or workpiece feed s is step over distance d is depth of cut f is feed direction of workpiece s w f
8. Feeds/Speeds
9. Feeds & Speeds Ref: From Machinery’s Handbook 21st ed
10. Feeds & Speeds <ul><li>"For ordinary twist drills (HSS- high speed steel) the feed rate used is... </li></ul><ul><ul><ul><li>0.001-0.003 in/rev for drills smaller than 1/8 in. (dia.); </li></ul></ul></ul><ul><ul><ul><li>0.002-0.006 in/rev for 1/8 to 1/4 in. dia. drills; </li></ul></ul></ul><ul><ul><ul><li>0.004-0.010 in/rev for 1/4 to 1/2 in. dia. drills; </li></ul></ul></ul><ul><ul><ul><li>0.007-0.015 in/rev for 1/2 to 1 in. dia. drills; and, </li></ul></ul></ul><ul><ul><ul><li>0.010-0.025 in/rev for drills larger than 1 inch. (dia) </li></ul></ul></ul><ul><li>The lower values in the feed ranges should be used for hard materials such as tool steels, </li></ul><ul><li>superalloys, and work hardening stainless steels; the higher values in the feed ranges </li></ul><ul><li>should be used to drill soft materials such as aluminum and brass." </li></ul>Ref: From Machinery’s Handbook 21st ed Cutting Speeds for Drilling (fpm) Material Cutting speed (fpm) Wrought Aluminum Alloys (Cold Drawn) 300 Free Cutting Brass (Cold Drawn) 175 Wrought Magnesium Alloys (Cold Drawn) 350 Mold Steels- P20 & P21 60 1040 Plain Carbon Steel (CD ,Hardness 175-225HB) 75
11. “Optimal” Feeds & Speeds <ul><li>In the “typical operating range”, tool life (T) and cutting speed (V) are related according to Taylor’s Equation </li></ul>where n & C are experimentally determined constants <ul><li>FW Taylor studied the effects of the feed, depth of cut, and </li></ul><ul><li>cutting speed: </li></ul><ul><ul><li>1) Cutting Speed is the dominating factor in determining tool life </li></ul></ul><ul><ul><li>2) Feeds and Depths of Cut are the dominant forces in determining </li></ul></ul><ul><li>the force acting on the tool </li></ul><ul><li>Taylor recommended using the maximum allowable feed </li></ul><ul><li>and depth of cut, then selecting V to balance tool wear with </li></ul><ul><li>cycle time for the process </li></ul>
12. Cutting Speeds Cutting Rates- Often given speeds in SFM (surface feet/min), but control spindle rotation in RPM (rev/min). Note: Use the maximum effective cutting diameter of tool Formula for spindle RPM comes from basic kinematics v= x r
13. Cutting Diameter To select the correct radius (or diameter) to use in the formula-- Determine what the spindle is rotating Find the perpendicular distance from the axis of rotation to the furthest point where cutting occurs Double it to get the diameter Axis of Revolution Cutting Edge d Lathe- part turns(NOT tool) r is from center to tool if turning down - d is workpiece diameter Flat Nosed End Mill d=cutter diameter d Axis of Revolution Cutting Edge d Axis Ball Nosed End Mill if ball is not “buried” in workpiece, then d will be less than cutter diameter i.e. NO cutting occurs at full tool diameter
14. Feed Rates Feed Rates are commonly given as Advance Per Tooth (APT) To get the feed rate in surface inches per minute use: More properly one wishes to control the chip load or nominal chip thickness t l . If the cutter is NOT fully loaded, one must increase the feed (APT) to keep the same chip load (t l ). Most tabulated values of the APT assume a fully loaded cutter- they are really listings of the required chip load t l . Feeds on lathes and drills can be in ipr (inches per revolution): N is no longer required in formula:
15. Chip Load and Advance Per Tooth Step over distance (radial depth of cut) at least 1/2 tool diameter chip load (t )= APT Step over distance (radial depth of cut) less than 1/2 tool diameter chip load (t ) < APT APT APT l l t l t l
16. Shallow Cuts with Ball Nosed End Mill Decrease in Effective Cutting Diameter Decrease in Chip Load Notice how the chip load (t l ) is less than the APT for a shallow cut
17. R CTF - Ball Nose @ Small Depth of Cut Ref: Figure O-51, Kibbe, et al. Machine Tool Practices 5 th Ed, Prentice Hall,1995.
19. Feeds w/ Radial Chip Thinning Factor Proper feeds come from finding the required advance per tooth (APT) to get correct chip load (feed value commonly given in books) As we use it, the R CTF is a “first pass” improvement 1) R CTF s for FLAT end mill with small step over distance 2) R CTF s for BALL end mill with small depth of cut 3) Anything over tool radius is assumed to be fully loaded In some cases tables incorporate R CTF s and give true APT But usually what you look up in a table is really t l
20. Feeds/Speeds
21. Feeds & Speeds - Example 1 Estimate the cutting speed and feed rate required for a 3/4” diameter 2 flute HSS end mill in Cast Iron, with a depth of cut of 0.375” and a step over distance of 0.375.” The spindle rotational speed is given by: The machine feed rate is given by:
22. Feeds & Speeds - Example 2 Estimate the depth of cut, the cutting speed, and feed rate required when rough turning a bronze shaft, from a diameter of 2.000” to 1.800.” Refer to tables to get recommended speed and feed.
23. Feeds/Speeds for Example 2
24. Feeds & Speeds - Example 2 (Cont’d) Estimate the depth of cut, the cutting speed, and feed rate required when rough turning a bronze shaft, from a diameter of 2.000” to 1.800.” The recommended speed is The recommended feed is
25. Feeds & Speeds - Example 3 Estimate the cutting speed and feed rate required for a 1/2” diameter HSS 2 flute ball nose end mill in “medium” tool steel, with a depth of cut of 0.0625” and a step over distance of 0.250.” The ball end mill depth of cut is less than the radius. Therefore the effective diameter must be computed: Find speeds and feeds from table.
26. Feeds/Speeds for Example 3
27. Feeds & Speeds - Example 3 (Cont’d) Estimate the cutting speed and feed rate required for a 1/2” diameter HSS 2 flute ball nose end mill in “medium” tool steel, with a depth of cut of 0.0625” and a step over distance of 0.250.” The recommended speed is: Find the chip reduction factor from table.
28. R CTF - Ball Nose @ Small Depth of Cut for Ex 3 Ref: Figure O-51, Kibbe, et al. Machine Tool Practices 5 th Ed, Prentice Hall,1995.
29. Feeds & Speeds - Example 3 (Cont’d) Estimate the cutting speed and feed rate required for a 1/2” diameter HSS 2 flute ball nose end mill in “medium” tool steel, with a depth of cut of 0.0625” and a step over distance of 0.250.” The recommended feed rate is:
30. Machinability Machinability generally involves three factors 1) Surface Finish 2) Tool Life 3) Force and Power Requirements Machinability Ratings are the cutting speeds required to obtain a tool life of T=60 min-- (in general, for a given material, higher speeds decrease the tool life, & slower speeds increase it Standard is AISI 1112 steel- rating of 100 for a tool life of 60 min, use cutting speed of 100 SFM (AISI 1112) From example 8.5, Kalpakjian. Manufacturing Processes for Engineering Materials 2 nd Ed, Addison-Wesley 1991.
31. Power & Force Estimation Power, P, requirements can then be determined as... where MRR is the Material Removal Rate Torque, , is found from where is the spindle speed F p, the force in the direction of the cutting velocity, V, is
32. Specific Energies of Machining Ref: Shaw. Metal Cutting Principles , Clarendon Press 1984, p. 43 Material Aluminum Alloys 100,000 Gray Cast Iron 150,000 Free Machining Brass 150,000 Free Machining Steel (AISI 1213) 250,000 “ Mild” Steel (AISI 1018) 300,000 Titanium Alloys 500,000 Stainless Steels 700,000 High Temp. Alloys 700,000 u can be determined from where is the effective rake angle (in degrees) & t l is the undeformed (nominal) chip thickness (in inches)
33. Cutting Power - Example 1 Find the power for an 8” HSS face mill (10 teeth, e =30 o ) to remove 0.1” from Cold Drawn, Wrought Aluminum, with a step over distance of 4.0” at a speed of 600 fpm and an APT 0.022.” Compute the speed and feed. The material removal rate is:
34. Cutting Power - Example 1(cont’d) Find the power for an 8” HSS face mill (10 teeth, e =30 o ) to remove 0.1” from Cold Drawn, Wrought Aluminum, with a step over distance of 4.0” at a speed of 600 fpm and an APT 0.022.”
35. Cutting Power - Example 2 Estimate the work required to turn down an annealed 304 stainless rod 6 in long from a diameter of 0.500” to a diameter of 0.480.” (Assume e =13 o , & ipr=0.003”)
36. Summary <ul><li>Factors for Chip production: </li></ul><ul><ul><li>rake angle </li></ul></ul><ul><ul><li>clearance angle </li></ul></ul><ul><ul><li>shear angle </li></ul></ul><ul><li>Factors that affect machining parameters: </li></ul><ul><ul><li>effective diameter </li></ul></ul><ul><ul><li>depth of cut </li></ul></ul><ul><ul><li>radial depth of cut (if applicable) </li></ul></ul><ul><ul><li>speeds (tip and spindle) </li></ul></ul><ul><ul><li>feed rate </li></ul></ul><ul><ul><li>material </li></ul></ul><ul><ul><li>tool material </li></ul></ul>
37. Credits <ul><li>This module is intended as a supplement to design classes in mechanical engineering. It was developed at The Ohio State University under the NSF sponsored Gateway Coalition (grant EEC-9109794). Contributing members include: </li></ul><ul><li>Gary Kinzel …………………………………….. Project supervisor </li></ul><ul><li>Chris Hubert and Alan Bonifas ..……………... Primary authors </li></ul><ul><li>Phuong Pham and Matt Detrick ……….…….. Module revisions </li></ul><ul><li>L. Pham …………………………………….….. Audio voice </li></ul><ul><li>References: </li></ul><ul><ul><ul><li>Machinery’s Handbook 21st ed </li></ul></ul></ul><ul><ul><ul><li>Kalpakjian, S. and Addison Wesley, Manufacturing Processes for Engineering Materials , 2nd Ed., 1991 </li></ul></ul></ul><ul><ul><ul><li>Kibbe, et al. Machine Tool Practices 5 th Ed, Prentice Hall,1995 </li></ul></ul></ul><ul><ul><ul><li>Shaw. Metal Cutting Principles , Clarendon Press </li></ul></ul></ul>
38. Disclaimer This information is provided “as is” for general educational purposes; it can change over time and should be interpreted with regards to this particular circumstance. While much effort is made to provide complete information, Ohio State University and Gateway do not guarantee the accuracy and reliability of any information contained or displayed in the presentation. We disclaim any warranty, expressed or implied, including the warranties of fitness for a particular purpose. We do not assume any legal liability or responsibility for the accuracy, completeness, reliability, timeliness or usefulness of any information, or processes disclosed. Nor will Ohio State University or Gateway be held liable for any improper or incorrect use of the information described and/or contain herein and assumes no responsibility for anyone’s use of the information. Reference to any specific commercial product, process, or service by trade name, trademark, manufacture, or otherwise does not necessarily constitute or imply its endorsement.