What Does A CNC Machining Center Do?

Transcription

1 Lesson 2 What Does A CNC Machining Center Do? A CNC machining center is the most popular type of metal cutting CNC machine because it is designed to perform some of the most common types of machining operations. It is important to understand these machining operations in order to properly use a CNC machining center. In this lesson, we will describe the function of CNC machining centers. We will start by comparing CNC machining centers to other types of machines with which you may have some experience. We will then introduce the cutting conditions that are related to machining operations. Finally, we will describe in detail the two most basic kinds of machining operations that can be done on machining centers, including hole machining operations and milling operations. At the completion of this lesson, you will know what a CNC machining center is designed to do. Comparing a CNC machining center to other types of machines CNC machining centers replace certain conventional machine tools. While you may not have experience with CNC machining centers, it is likely that you have had experience with at least one of the conventional machines they replace: the drill press. At the very least, you probably know what a drill press is and/or have seen one in use. If so, you know that the primary function of a drill press is to drill holes. The next illustration shows a typical home-shop drill press. A drill press is used to machine holes. The operator manually loads the drill, starts the spindle, and turns a crank to drive the tool into the workpiece which in turn drills the hole. The tool is then retracted from the hole and the spindle is turned off. Cutting tool (drill) is placed in drill-chuck A typical drill press A drill-bit is but one of many cutting tools that can be used to machine holes. And while a drill press can be used to machine holes with other types of cutting tools, most people in a home-shop don t do much more than drilling operations. We ll discuss other types of hole-machining tools a little later. Copyright 2011, CNC Concepts, Inc. Machining Center Setup and Operation Page1

2 Understanding Machining Direction With a drill press, machining occurs as the crank is turned to drive the drill downward into the material. So when drilling, the machining direction is downward, along the length of the drill. It is important to understand that with any machining operation, there must be adequate support to keep the cutting tool and workpiece stable while machining. With a drill press, the machine s spindle and quill provide the support needed for the cutting tool. Support for the workpiece is provided by the operator, who is firmly holding the workpiece in place with one hand while turning the crank with the other. Compare this to using a hand-held electric drill. With a hand drill, your hands supply all of the support one hand for the drill s stability and the other for the workpiece being drilled. With a drill press, the machining direction is downward. Milling machines Downward (along the length of the drill) is the only feasible machining direction with a drill press, meaning a drill press is not designed to machine in any other direction. But there is a type of machine tool that can machine in other directions. It is called a milling machine. The milling machine is not nearly as well-known as the drill press. It is unlikely, unless you have previous shop experience, that you have even seen one let alone used one. From a machinist s standpoint, a milling machine is much more flexible than a drill press. That is it can still machine in a downward direction (along the length of the tool), but it also has the ability to machine in other directions. The next illustration shows a popular type of milling machine called a knee-mill. Moves quill/tool up/down Moves table fore/aft Moves table left/right Moves knee up/down Knee style milling machine Copyright 2011, CNC Concepts, Inc. Machining Center Setup and Operation Page2

3 Notice how much sturdier the knee mill appears as compared to a drill press. The workpiece will be clamped to the table in some fashion (not held by the operator). A knee mill provides much more support (than a drill press) for the cutting tool and workpiece. Notice also that the machine s table is moved left/right and fore/aft by handwheels. There are also handwheels to move the knee up/down and quill (cutting tool) up/down. These handwheels provide precise control of the movements they cause. A milling machine provides the stability to machine in at least three directions. First, like a drill press, it allows a cutting tool to be plunged (along the tool s length), as is necessary when drilling a hole. Second, it allows machining with table movement left/right. Third, it allows machining with table movement fore/aft. When machining is caused by table movements (left/right, fore/aft, or combining the two), it is called a milling operation. The next illustration shows a milling operation. Milling is done here to machine a rectangular pocket. After the cutting tool (an end mill) has been plunged to the pocket s depth (just like a drill), it then machines the rectangular shape in the workpiece. This requires table movement right/left and fore/aft. The machine must, of course, provide the support needed to mill in these directions and as you can see from the previous illustration, knee style milling machines provide good support for all moving components. Machining operation to mill a rectangular pocket We will be discussing hole-machining operations and milling operations in more detail in our next discussion. For now, our intention is simply to show you what CNC machining centers are designed to do: To perform the same kinds of machining operations that can be done on drill presses and milling machines. These include hole-machining operations and milling operations. The next illustration shows a typical CNC machining center. Copyright 2011, CNC Concepts, Inc. Machining Center Setup and Operation Page3

4 Machining operations performed on machining centers Generally speaking, CNC machining centers machine a stationary workpiece with a series of rotating cutting tools. That is, with most machining center operations, the workpiece being machined is securely held by a workholding device like a vise while a rotating cutting tool (like a drill) is driven to contact it. The cutting edges of the cutting tool will scrape material from the workpiece. This scraping of material from the workpiece is called machining and the small pieces of material being scraped from the workpiece are called chips. Any CNC person must understand the machining operations that can be performed on CNC machining centers. This is imperative for programmers, since they must develop programs that perform the machining operations. It is also important for setup people, since they must often make adjustments when new programs are run. And it is important for operators, since they must be able to determine when cutting tools are getting dull and in need of replacement. So the more a person knows about the machining operations a CNC machining center can perform, the easier it will be to become proficient as a programmer, setup person, or operator. Introduction to cutting conditions It is also important for a CNC person especially programmers and setup people to understand the cutting conditions related to the machining operation being performed. Cutting conditions determine how the machining operation will be performed, contributing to the efficiency, surface finish, and quality of the machining operation. The two most common cutting conditions are spindle speed and feedrate (though there are several others). Spindle speed is how fast the cutting tool rotates. Feedrate is how fast the cutting tool (or workpiece) moves during the machining operation. For CNC machining centers, spindle speed is specified in revolutions per minute (rpm). Feedrate is usually specified in per-minute fashion, and is given in either inches per minute (ipm) or millimeters per minute (mmpm), depending upon the measurement system being used. A programmer must be able to determine a workable speed and feed for each machining operation they program. Setup people often modify programmed cutting conditions in order to achieve an optimal machining operation (better surface finish, longer tool life, or optimum cutting time). Operators must be able to determine when cutting tools are getting dull. Cutting conditions are commonly recommended by cutting tool manufacturers based upon the cutting tool to be used, the material to be machined, the material that the cutting tool s cutting edge is made from, and the kind of machining operation to be performed. We ll be discussing how to determine cutting conditions as we present each kind of machining operation. How cutting conditions are recommended Again, machining centers require spindle speed to be specified in revolutions per minute (rpm) and feedrate in per minute fashion (inches or millimeters per minute). Unfortunately, most cutting tool manufacturers do not specify their recommendations in this manner. Speed is recommended surface feet per minute (sfm) if you work with the inch measurement system or meters per minute (mpm) if you work with the metric measurement system. In either case, this is the linear length of material that will pass by each cutting edge of the cutting tool during one minute. If a speed of 80 surface feet per minute is recommended, 80 feet of material will pass by each cutting edge of the tool during one minute. Note that this is based upon the cutting tool s largest diameter. For a 0.5 inch diameter drill, for example, 80 feet of material will pass by the outer-most diameter of the drill (0.5 inch) during one minute. The smaller the diameter of the cutting tool, the higher the speed in rpm will be required in order to achieve a given speed in surface feet per minute. Most cutting tool manufacturers recommend feedrate in either per-tooth (per cutting edge) or per revolution. You ll be left to do the conversion to the appropriate feedrate in inches or millimeters per minute. Some formulae and examples follow. Copyright 2011, CNC Concepts, Inc. Machining Center Setup and Operation Page4

5 Spindle speed: Converting from surface feet per minute (sfm) to revolutions per minute (rpm) It is pretty simple to calculate the required spindle speed in rpm for a cutting tool if you know the recommended speed in surface feet per minute and the diameter of the cutting tool. Speed in rpm is calculated with this formula if you work in the inch measurement system: rpm = sfm times 3.82 divided by tool diameter Say for example, you are going to be using a 0.5 inch diameter high speed steel (hss) twist drill to machine a hole in mild steel. You look in the technical documentation from the drill manufacturer and they recommend that you run this drill at a speed of 80 sfm. For this half inch diameter drill, this means you must use a spindle speed of 611 rpm (80 times 3.82 divided by 0.5 is 611.2). Again, the trick lies in determining the recommended speed in surface feet per minute (sfm). Once you know this speed, calculating rpm is simple. Spindle speed: Converting from meters per minute (mpm) to revolutions per minute (rpm) Here is the rpm calculating formula if you work in the metric measurement system: rpm = mpm times 319 divided by tool diameter Say you are machining mild steel with a 10.0 mm hss twist drill. The drill manufacturer recommends speed of 25 meters per minute. In this case, you must run the drill at 797 rpm (25 times 319 divided by 10.0 is 797.5). Feedrate: Converting inches per tooth (ipt) or inches per revolution (ipr) to inches per minute (ipm) Once you determine a speed in rpm, you can calculate the inches-per-minute feedrate. Depending upon the style of cutting tool, cutting tool manufacturers will recommend feedrate in either per-tooth or per-revolution fashion. Generally speaking, inches per tooth will be specified for milling cutters and inches per revolution will be specified for most other cutting tools. Use this formula if feedrate is specified in per-tooth fashion: ipm = rpm times ipt times number of teeth Say for example, you have already determined the spindle speed for a 1.0 inch diameter end mill that has 4 flutes. Using the rpm formula give earlier, you determine that the end mill should run at 380 rpm. Based upon the material you are machining, the cutting tool manufacturer recommends a feedrate of ipt. In this case, you ll use a feedrate of ipm (380 times times 4 is 3.648). Note that the words per tooth refer to the number of cutting edges for the tool. They could be inserts, flutes, or teeth. Use this formula if feedrate is specified in per-revolution fashion: ipm = rpm times ipr For example, say you will be drilling a 0.5 inch diameter hole in mild steel. You ve already calculated the speed required (611 rpm). The drill s manufacturer recommends a feedrate of ipr. In this case, you ll run the drill at a feedrate of ipm (611 times is 2.444). Feedrate: Converting millimeters per tooth (mmpt) or millimeters per revolution (mmpr) to millimeters per minute (mmpm) Once you determine the required speed in rpm, you simply multiply the required feedrate in millimeters per revolution times the speed in rpm to determine the required feedrate in millimeters per minute: mmpm = rpm times mmpr If feedrate is recommended in per tooth fashion, you must first determine the required feedrate in millimeters per revolution by multiplying the number of teeth (or flutes or inserts) times the recommended feedrate in millimeters per tooth. mmpr = number of teeth times mmpt When working in the inch system, here is a summary of the formulae provided so far: rpm = sfm times 3.82 divided by tool diameter Copyright 2011, CNC Concepts, Inc. Machining Center Setup and Operation Page5

6 ipm = rpm times ipt times number of teeth ipm = rpm times ipr What Does A CNC Machining Center Do? We ll be using these formulae as we look at specific machining operations performed on machining centers. Getting recommendations for cutting conditions The next illustration shows how one end mill manufacturer recommends cutting conditions. In the left-most column, the material is specified. Next, you see the recommended speed in sfm. Finally, feedrate is recommended in inches per tooth format based on the size of the end mill. Again, this chart is typical of cutting tool manufacturer s recommendations for speed and feed for their cutting tools. A partial list of end mill cutting conditions recommendations from a cutting tool manufacturer. Other cutting conditions related to machining operations Spindle speed and feedrate are very important, but they represent only two of many cutting conditions that contribute to successful machining. Here we simply introduce some others. Radial depth of cut For milling operations, this is the amount of material being machined by the periphery (outside diameter) of the milling cutter. Axial depth of cut (commonly referred to as simply depth of cut) For milling operations, this is the amount of material being machined by the end of the milling cutter. Use of coolant Coolant is the liquid that cools and lubricates the cutting tool as it performs its machining operation. Rigidity of setup While not a cutting condition per-se, the success of the machining operation depends upon appropriate rigidity of the workholding device and the cutting tool. Most cutting tool manufacturers assume that the setup securely holds the workpiece and that the cutting tool is strong and rigid when they provide recommendations. Cutting tool materials We already mentioned that cutting conditions are closely related to the material being machined (as the previous chart illustrates). In addition, the material of the cutting tool s cutting edge/s is also an important factor. Generally speaking, the harder the cutting tool material, the faster will be the recommended speed. There are several cutting tool materials available. High speed steel (hss) or cobalt are relatively inexpensive and are commonly used when the entire cutting tool is made from the same material. With a center drill, spot drill, or twist drill, for example, the cutting edges and the shank of the tool are made from the same material so high speed steel or cobalt is commonly used. Copyright 2011, CNC Concepts, Inc. Machining Center Setup and Operation Page6

7 Carbide (or coated carbide) is another popular cutting tool material. It is much harder than high speed steel or cobalt and allows faster cutting speed. But it is also much more expensive. For this reason, cutting tool manufacturers may only provide the cutting edges (commonly called inserts) from carbide. The rest of the tool (called the tool s shank) may be made from steel. Hole-machining operations Hole-machining operations are the most common operations performed on a CNC machining center. Almost every machining center job requires some form of hole-machining. Most CNC machining center control manufacturers provide a series of special canned cycles to help with these very common machining operations. While canned cycles are not addressed in this text (they are in the Machining Center Programming manual), we mention them here to let you know that there are very simple commands available to help with the programming of hole-machining operations. Depending upon the accuracy and finish requirements of the hole to be machined, hole-machining may require as many as three stages starting the hole, rough machining the hole, and finish machining the hole. We ll begin with those machining operations that are performed to start holes. The round holes in this die block have been machined by hole-machining cutting tools Center drilling Center drilling is done to assure that a subsequent drilling operation gets off to a good start. Note that center drilling is only necessary for drills that have a drill point, like twist drills and spade drills (more on these tool types is coming up). If the hole s position is critical, it is always best to center drill for drills with a drill point. The next drawing shows a plain type center drill as well as specifications for its most common sizes. Note that the most common sizes used with CNC machining centers include #3, #4, and #5. Copyright 2011, CNC Concepts, Inc. Machining Center Setup and Operation Page7

8 When a hole has been center drilled, there will be clearance for the web of the drill to follow. And since the drill will come into contact with the workpiece at a very small diameter, the drill will get started into the hole correctly. The next drawing shows this. After center drilling, drill starts contacting the workpiece from here. Generally speaking, if the hole has not been started with a center drill, smaller drills will have the tendency to wander from its desired path. With short, large drills (over in or so in diameter), the drill may be able to overcome this tendency to wander, and will machine the hole correctly. But as stated, if the hole s position is critical, and for smaller diameter drill sizes, it is always best to center drill first. Note that as a center drill plunges deeper into the hole, the diameter of the hole becomes larger. To attain the best results from center drilling, we feel the diameter of the center drilled hole should be just large enough to allow clearance for the subsequent drill web. That is, you should not attempt to center drill the hole to a diameter that will form a chamfer after drilling (though some programmers do). If you attempt this, the drill will still be prone to wander (more on why during our discussion of spot drilling a little later). Additionally, since the very point of a center drill is quite weak, there will be a tendency for the point to break if you try to go too deep. A broken center drill will leave a very hard remnant inside the hole that will be difficult to remove. Copyright 2011, CNC Concepts, Inc. Machining Center Setup and Operation Page8

9 Again, are times when the hole-location is not critical, when the drill is quite rigid, and/or when a certain amount of wandering is acceptable. If you wish to start a hole by forming a chamfer, we recommend that you use a spot drill (discussed next) instead of a center drill. Cutting conditions for center drilling Speed will be recommended in sfm or mpm, depending upon your measurement system. You ll need to calculate speed in rpm based upon the point diameter of the center drill (again, we re assuming that you will only center drill deep enough to make clearance for the drill web). Recommended feedrate will be specified in per-revolution fashion, meaning you ll need to calculate feedrate in inches per minute (ipm). Example: Say you are machining mild steel with a #4 center drill (having a point diameter). The center drill manufacturer recommends a speed of 80 sfm and a feedrate of ipr. In this case you ll use a spindle speed of 2,445 rpm (3.82 times 80 divided by 0.125). You ll use a feedrate of ipm (0.001 times 2445). Dull tool replacement and sharpening Cutting tool manufacturers will sometimes provide approximate tool life for the tools they make based upon the cutting conditions they recommend. But for the most part, CNC people are expected to recognize when a cutting tool is getting dull. Symptoms of dull tools include discoloration in chips (turning more blue or black), excessive smoke from the machining operation, changes in machining sounds (like squealing), and degraded surface finish on machined surfaces. Most companies do not attempt to sharpen their center drills. Spot drilling Another way to start a hole prior to drilling is to use a spot drill. The next drawing shows a common spot drill. A spot drill has a ninety degree point angle which will form a 45 degree chamfer for the hole being machined. By chamfer, we mean a small corner-break on the surface being machined around the rim of the hole. Chamfering is done to remove the sharp edges from the top of the hole. The depth of a spot drilled hole determines the chamfer size, and it is quite easy to calculate. Simply divide the desired chamfer diameter by two to come up with the spot drilling depth. The next drawing shows this. For example, say you are going to drill a hole to a diameter of in. You want a by 45 degree chamfer around the top of the hole. In this case, the desired chamfer diameter is in (0.25 plus plus 0.015). The depth required for the spot drill in this case is (0.280 divided by 2). Copyright 2011, CNC Concepts, Inc. Machining Center Setup and Operation Page9

10 There is one problem with spot drilling if the hole s position is critical, and if the up-coming drill is prone to wander. When the drill first comes into contact with a spot drilled hole (or with a center drilled hole sent so deep that it that chamfers the drilled hole), the first surface of the drill to contact the workpiece will be the outside diameter of the drill, not the drill s point. The next drawing shows this. Most experienced machinists will agree that this will cause a tendency for the drill to wander, especially if the drill is not perfectly sharpened. As stated earlier, we feel it is always better to center drill before drilling if the hole location is critical (center drill just deep enough to provide clearance for the drill s web, drill the hole, and then chamfer with a spot drill). However, if the hole s location is not critical, machining time can be saved by spot drilling prior to drilling. Cutting conditions for spot drilling Speed will be recommended in sfm or mpm, depending upon your measurement system. You ll need to calculate speed in rpm based upon the chamfer diameter the spot drill is machining (the largest diameter machined by the spot drill). Recommended feedrate will be specified in per-revolution fashion, meaning you ll need to calculate feedrate in inches per minute (ipm). Example: Say you are machining mild steel with a 0.5 diameter hss spot drill. You intend to chamfer a 0.25 inch diameter hole, providing a chamfer around the hole. This means you ll be spot drilling to a 0.28 inch diameter the diameter you use to calculate spindle speed in rpm. The spot drill manufacturer recommends a speed of 80 sfm and a feedrate of ipr. Spindle speed will be 1,091 rpm (80 times 3.82 divided by 0.28). Feedrate will be ipm (0.003 times 1091). Dull tool replacement and sharpening As stated, most high speed steel and cobalt cutting tools can be sharpened with relative ease. And only the very end of the cutting tool must be sharpened. With a dull spot drill, for example, the very tip can be sharpened. A skilled machinist may be able to do so with a pedestal grinder. There are tool and cutter grinders that can do so more precisely, and may lower the skill level required of the person that is doing the sharpening. Counter sinking The purpose for counter sinking is to chamfer a previously machined hole. That is, a counter sink is used in an existing hole to form a chamfer around its rim. It does not have the ability to start a hole from a solid surface (as a spot drill does). The next drawing shows a counter sink. Notice the point angle of 82 degrees. Though this tool cannot machine a true 45 degree chamfer, most machinists still use it to chamfer holes, especially larger holes that are too big to spot drill. However, if this tool is used in a program, you must be careful when specifying the depth a countersink must go. Calculating hole-depth is not quite as simple as when using a 90 degree spot drill. Copyright 2011, CNC Concepts, Inc. Machining Center Setup and Operation Page10

11 To determine the depth to send the counter sink, divide 0.53 by (the tangent of 41 degrees). For example, if you have previously machined a 1.0 diameter hole and wish machine a 0.03 chamfer around its rim, the chamfer diameter will be 1.06 (1.0 plus 0.03 plus 0.03). The needed depth for the counter sink will be (0.53 divided by 0.869). Since a counter sink is used only after the hole has been machined, it is possible to position the point of this tool well into the hole and close to the surface that must be chamfered. Doing so minimizes machining time as feed motion can be kept very short (just enough to form the chamfer). Look at the next drawing, for example. Notice how far the point of the tool must travel into the hole before chamfering can begin. To determine the approach position prior to counter sinking (commonly called the rapid plane), we recommend that you first calculate the depth for counter sinking (as described above). Then subtract the chamfer size and the approach distance (normally 0.1 inch) from this depth. Consider the previous example (machining a 0.03 inch chamfer around a 1.0 inch diameter hole). We came up with a counter sinking depth of With our recommended method, the approach position will be at a depth of ( minus 0.03 minus 0.1). If more than one hole must be counter sunk, of course, the tool must be fully retracted from one hole prior to moving to the next. Cutting conditions for counter sinking Speed will be recommended in sfm or mpm, depending upon your measurement system. You ll need to calculate speed in rpm based upon the chamfer diameter the counter sink is machining (the largest diameter machined by the counter sink). Recommended feedrate will be specified in per-revolution fashion, meaning you ll need to calculate feedrate in inches per minute (ipm). Example: Say you are machining mild steel with a 1.5 inch diameter hss counter sink. You intend to chamfer a 1.0 inch diameter hole, providing a 0.03 chamfer around the hole. This means you ll be counter sinking to a 1.06 inch diameter the diameter you use to calculate spindle speed in rpm. The counter sink manufacturer recommends a speed of 80 sfm and a feedrate of ipr. Spindle speed will be 288 rpm (80 times 3.82 divided by 1.06). Feedrate will be ipm (0.004 times 288). Dull tool replacement and sharpening Most companies do not attempt to sharpen their counter sinking tools. Copyright 2011, CNC Concepts, Inc. Machining Center Setup and Operation Page11

12 Drilling with twist drills Here is a common twist drill: For most drilling applications, the twist drill is plunged to its final depth in one pass. The drill is then quickly retracted from the hole. Note that the only surfaces that do any machining are at the very end of the drill (chips are forced out by the drill s flutes). Allowing for the drill point When most design engineers specify the depth of a hole, they mean for the hole to be machined with the specified diameter to the depth given. This means if a twist drill (or any drill with a point angle) is used, the programmer must add the drill point amount (called the lead of the drill) to the depth of the hole specified on the engineering drawing. A hole which does not pass completely through the surface being machined is called a blind hole. A hole which passes completely through the surface being machined is called a through hole. Copyright 2011, CNC Concepts, Inc. Machining Center Setup and Operation Page12

13 A twist drill has a 118 degree point angle, and the amount of drill lead is easy to calculate. Multiply the diameter of the drill times 0.3 to come up with the drill s lead. For example, a 0.50 in diameter twist drill has a 0.15 in lead (0.3 times 0.5). In this case, the value 0.15 must be added to the hole-depth specified on the engineering drawing in order to come up with the hole-depth needed in the CNC program. Calculating the depth of through holes If machining a hole through a surface with a twist drill, the drill lead must be added to the workpiece thickness. Additionally, you must add a small amount of clearance which forces the drill to truly break through the surface. Normally in is sufficient. If you do not add this small amount to your hole-depth, it is likely that the hole will not be completely machined through the surface. This is especially likely if the material is gummy, having the tendency to push away from the cutting edges of the drill. For example, if you are machining through a 1.0 in thick workpiece with a diameter drill, you should program the depth of the hole as at least (1.0 plus 0.15 lead plus 0.030). Peck drilling to break chips The previously described motions (feed to full depth and retract) will sometimes cause a long stringy chip to be formed as the drill machines the hole. This is especially true with malleable materials, like aluminum and some steels. This long chip will be whipped around the drill, and grow longer and longer. If left to grow, it will eventually break and be thrown away from the drill. If the protective guarding around the machine is inadequate, it is quite possible that this chip will be thrown right at the operator. Brittle materials like cast iron will never form this kind of stringy chip. One way to solve the stringy chip problem is to force the chip to break at manageable lengths as the hole is being drilled. In this case, peck drilling can be done to break chips. The drill will be plunged into the hole a short distance (say in). Then the drill will be retracted a very small amount (about in). It is during this small retracting motion that the chip is forced to break. The plunge-and-retract motion will be repeated for the entire hole-depth. When finished, the drill will be retracted from the hole. Since this kind of motion will be somewhat difficult (and quite lengthy) to program, most machining centers provide a special peck drilling canned cycle for the purpose of breaking chips. Peck drilling for deep holes The flutes of a twist drill limit the drill s maximum drilling depth (see the previous drawing of a twist drill to see the flutes). However, you must know that most twist drills cannot machine to this maximum depth in one pass. If this is attempted, the flutes of the twist drill will pack with chips, and these chips will eventually bind up between the flutes and the workpiece. If drilling continues after this binding occurs, the drill will eventually break. For this reason, when deep holes must be machined, the drill must peck into the hole a specified depth, then retract completely out of the hole to clear chips. Then the drill will be sent back into the hole to within a small clearance distance from where it left off. The hole will then be machined to a greater depth. This peck drilling will continue until the final depth is reached, at which time the drill will be retracted from the hole one last time. While cutting tool manufacturers may have more specific recommendations, there is a pretty good rule-ofthumb for determining peck amount per pass. For most materials, the peck depth can be calculated by multiplying the diameter of the drill times three. That is, a twist drill has the ability to machine to a depth of about three times its diameter without fear of the chips packing up. So if the hole-depth is deeper than about three times the drill diameter, you should use peck drilling techniques to clear chips. For example, say you must machine a diameter hole to a depth of 2.5 in. Three times in is 1.5 in. In this case, you will first peck to a 1.5 in depth, then retract the drill to clear chips. You will then send the drill back into the hole to a clearance position just above where the drill left off (into the hole to a depth of 1.4 inch will work nicely for this example). Finally, you must command that the balance of the hole be drilled. Since deep hole peck drilling is often necessary, and since it can be cumbersome to program as just described, most machining centers provide a deep hole peck drilling canned cycle for clearing chips in this manner. Copyright 2011, CNC Concepts, Inc. Machining Center Setup and Operation Page13

14 When an extremely deep hole must be drilled, the shear length of the drill will weaken its own integrity. In this case, if the drill is allowed to start from solid material, it may bend and/or break before the hole even gets started (even if the hole has been center drilled). At best, the drill will wander as the hole is started and the hole will not be straight. For this reason, extremely deep holes (over about six times the drill diameter) should be pilot drilled. Pilot drilling involves using a shorter drill of the same diameter to start the hole and machine to a reasonable depth. Then, a longer drill which is capable of machining to the required depth can continue machining to the final depth. We recommend that you make the pilot drill machine to at least four times the drill diameter before the longer drill used is used. Cutting conditions for twist drills Speed will be recommended in sfm or mpm, depending upon your measurement system. You ll need to calculate speed in rpm based upon the drill s diameter. Recommended feedrate will be specified in perrevolution fashion, meaning you ll need to calculate feedrate in inches per minute (ipm). Example: Say you are machining mild steel with a 0.5 inch diameter hss twist drill. The twist drill manufacturer recommends a speed of 80 sfm and a feedrate of ipr. Spindle speed will be 611 rpm (80 times 3.82 divided by 0.5). Feedrate will be ipm (0.005 times 611). Applications for drilling with twist drills As you know, a drill will machine a hole. The diameter of the hole will be close to the diameter of the drill (actually, just slightly larger). Generally speaking, if the overall tolerance for the hole-diameter is greater than about inch, drilling will create an acceptable hole. This is commonly the case when the hole will be used as a clearance hole for a screw or bolt to fit through. If a closer tolerance must be held, another machining operation (like reaming or boring) must be done after the drilling operation. The finish left by a drill will be about 125 rms, which is not considered to be a very fine finish (125 rms is equivalent to about a 200 grit sand paper). If a better finish is required, another machining operation (like reaming or boring) must be done after drilling. Dull tool replacement and sharpening Symptoms of dull drills include discoloration in chips (turning more blue or black), excessive smoke from the machining operation, changes in machining sounds (like squealing), and degraded surface finish on machined surfaces. Most high speed steel and cobalt cutting drills can be easily sharpened. Only the very end of the cutting tool must be sharpened. With a dull twist drill, the very tip can be sharpened by a skilled machinist using a pedestal grinder. There are also tool and cutter grinders available that can do so more precisely, and will lower the skill level required of the person who is doing the sharpening. Other drilling tools Twist drills are very popular for drilling holes up to 1.0 inch in diameter. When holes larger than this must be machined, it becomes quite expensive to make the entire tool out of the cutting tool material (high speed steel or cobalt). Instead, most cutting tool manufactures separate the shank of the tool from the cutting portion of the tool. Spade drills Like a twist drill, a spade drill commonly uses high speed steel or cobalt for it cutting edges. But the shank of the spade drill is made from less expensive steel. The next illustration shows a spade drill. Copyright 2011, CNC Concepts, Inc. Machining Center Setup and Operation Page14

15 Again, only the very end (blade) is made of the cutting tool material. The next illustration shows some typical blades. Since the cutting tool material for most spade drills is high speed steel or cobalt, the cutting speed in rpm will be quite low (since the hole diameter is quite large). And note that most machining centers don t have a great deal of power when it comes to Z axis thrust. A machining center may have a 20 hp spindle drive motor, but only a 2 hp Z axis drive motor. For this reason, and since spade drills require powerful thrust to push them into holes, they aren t commonly used with smaller CNC machining centers. Carbide inserted drills This form of drilling tool is available in many varieties. Since the actual cutting edges are made of carbide (or coated carbide), this kind of drill allows a much faster cutting speeds than hss or cobalt. And in essence, they transfer the power required for drilling from Z axis thrust to spindle power. For this reason, these drills are much more popular for use with CNC machining centers than spade drills. A carbide inserted drill usually has a straight shank with a flat for clamping and is commonly held in an end mill holder. Dull tool replacement and sharpening While most high speed steel and cobalt cutting tools can be sharpened with relative ease, cutting tools that incorporate carbide inserts will not be sharpened. Instead, the insert will be indexed (rotating the insert to a fresh cutting edge) or replaced. Most carbide inserts are clamped into cutting tools with Allen (hex) wrenches. To replace an insert, the setup person or operator will remove the insert, rotate it or replace it, and then clamp the insert back into the cutting tool. Copyright 2011, CNC Concepts, Inc. Machining Center Setup and Operation Page15

16 Counter boring Counter boring is done after a hole has been machined (usually by drilling) to enlarge the diameter of the hole to a specific depth. The bottom of the hole machined by the counter boring tool is flat. Counter bored hole for socket head cap screw As you can see from the previous illustration, the primary purpose for counter boring is to recess a surface for the head of a bolt usually a socket head cap screw. A true counter boring tool has a pilot that locates in the previously machined hole and keeps the counter bore from wandering as the hole is machined. The next illustration shows one, along with another pilot. If a true counter boring tool is used for the counter boring operation, the pilot is sent into the hole until the cutting edge is within the approach distance of the work surface (usually about 0.1 inch). As with a counter sinking tool, you must be concerned with the pilot s position after the hole is machined. If more than one hole must be counter bored, you must confirm that the pilot has cleared the work surface before moving to the next hole. When the surface to be counter bored is flat, most programmers use an end mill for the counter boring operation. In fact, there are many programmers that have never used a true counter boring tool. All end mills allow machining in a plunging direction just as a counter boring tool does. There are even end mills that allow machining into a solid surface (called center cutting end mills). With this kind of tool, a hole need not exist before a flat bottom hole is machined. If the end mill being used for counter boring is not of the center cutting style, and if the end mill is not of the center-cutting type, you must ensure that the previously machined hole is larger than the small hole in the center of the end mill. Copyright 2011, CNC Concepts, Inc. Machining Center Setup and Operation Page16

17 Since an end mill does not have a pilot, there is no need to be concerned with clearing a pilot between holes, as you must with a true counter boring tool. Cutting conditions for counter boring tools Speed will be recommended in sfm or mpm, depending upon your measurement system. You ll need to calculate speed in rpm based upon the counter boring tool s diameter. Recommended feedrate will be specified in per-revolution fashion, meaning you ll need to calculate feedrate in inches per minute (ipm). Example: Say you are machining mild steel with a 0.75 inch diameter hss counter boring tool. The manufacturer of the counter boring tool recommends a speed of 80 sfm and a feedrate of ipr. Spindle speed will be 407 rpm (80 times 3.82 divided by 0.75). Feedrate will be ipm (0.008 times 407). Dull tool replacement and sharpening A dull counter boring tool must usually be sharpened with a tool and cutter grinder. Reaming Reaming is done to improve the surface finish and size accuracy of a previously machined hole. Prior to reaming, the hole is machined very close to the finish size by some other tool (usually a drill). For holes up to about 0.5 inch in diameter, most programmers will drill about 1/64 (0.0156) under the reamed size. For holes over about 0.5 inch, they will drill about 1/32 (0.0316) under the reamed size. So a reamer is not intended to machine a great deal of stock. The next drawing shows a straight reamer. The surface finish and diameter accuracy machined by a reamer will be much better than that machined by a drill. However, a reamer will follow the previously machined hole. If the drill wandered as it machined the hole, so will the reamer. All reamers have a small chamfer on the very end of the reamer. It is this chamfer that actually machines the material from the hole being reamed. For this reason, the size of the chamfer controls the amount of material that can be machined from the hole. Again, reamers up to 0.5 inch in diameter have at least a 1/64 inch chamfer. It is important to consider the size of the chamfer when calculating the depth for through holes. The reamer s chamfer size must be added to the workpiece thickness. Most programmers will add another 0.03 (in addition to the chamfer size on the reamer) inch or so to ensure that the reamer truly breaks though the bottom surface of the through hole. Cutting conditions for reamers Speed will be recommended in sfm or mpm, depending upon your measurement system. You ll need to calculate speed in rpm based upon the reamer s diameter. Recommended feedrate will be specified in perrevolution fashion, meaning you ll need to calculate feedrate in inches per minute (ipm). Copyright 2011, CNC Concepts, Inc. Machining Center Setup and Operation Page17

18 Example: Say you are machining mild steel with a 0.5 inch diameter hss reamer. The reamer manufacturer recommends a speed of 60 sfm and a feedrate of ipr. Spindle speed will be 458 rpm (80 times 3.82 divided by 0.5). Feedrate will be 2.25 ipm (0.005 times 458). Applications for reaming As mentioned, reaming will improve upon the sizing and surface finish machined by drilling. While there is no way to control the diameter machined by a given reamer (a reamer will machine only a diameter hole), a reamer will allow you to hold much closer tolerances than when drilling. A tolerance of plus or minus inch can be easily held with reamers. When it comes to surface finish, a reamer can machine the hole to a surface finish of about rms, much better than a drill. Reamers are used to machine holes that accept pins. They can easily provide a slip fit or a press fit. Boring with boring bars Like reaming, boring is done to improve the quality of finish and size-accuracy for a previously machined hole. And just as for reaming, the hole before boring must be machined to a diameter very close to the size of the hole to be finish bored (usually about 1/64 th to 1/32 nd inch smaller). But unlike reaming, a boring bar does not have the tendency to follow the previously machined hole. If cutting conditions are correct, the boring bar will make its own path. For this reason, boring is often preferred over reaming if there is any tendency for the previously machined hole to have wandered. The actual cutting edge of most boring bars used in CNC machining centers is made of carbide or coated carbide. This allows faster cutting speeds and the cutting edge will last for a longer period of time. Boring bars used on CNC machining centers must be adjustable. The diameters each can machine fall into a specific range. Some form of mechanical device (commonly a set screw) is used to make precise adjustments. Again, a boring bar will machine a perfectly straight hole to a precise diameter (usually to within less than inch) and provide a very good surface finish inside the hole (usually less than 32 rms). As the illustration above shows, boring bars usually have but one cutting edge (tip, or insert). It can be quite difficult (nearly impossible) to precisely set the diameter that a boring bar will machine before it actually machines in a hole. For this reason, CNC setup people must commonly trial machine (test cut and then adjust). They will intentionally set the boring bar so that it will machine slightly undersize (by about inch or so). This ensures that the boring bar will not machine the hole too big on the first try. They will allow the boring bar to machine deep enough into the hole so they can take a measurement. They will then stop the machine, measure the hole-diameter, and adjust the boring bar accordingly. Depending upon the skill of the setup person and the quality of the boring bar, they may have to repeat this process until the hole is being machined to the appropriate diameter. Boring bars can be used for rough boring (straightening out a hole prior to finish boring) or for finish boring (machining a hole to its finished diameter). Cutting conditions for boring bars Copyright 2011, CNC Concepts, Inc. Machining Center Setup and Operation Page18

19 Speed will be recommended in sfm or mpm, depending upon your measurement system. You ll need to calculate speed in rpm based upon the boring bar s diameter. Recommended feedrate will be specified in perrevolution fashion (this may also be considered a per-tooth feedrate, since most boring bars have but one cutting edge). You ll need to calculate feedrate in inches per minute (ipm). Example: Say you are machining mild steel with a 1.5 inch diameter boring bar that has a carbide cutting edge (insert). The boring bar (or insert) manufacturer recommends a speed of 350 sfm and a feedrate of ipr. Spindle speed will be 891 rpm (350 times 3.82 divided by 1.5). Feedrate will be ipm ( times 891). Dull tool replacement and sharpening Note that most boring bars used on CNC machining centers incorporate a carbide insert for the cutting edge. While most high speed steel and cobalt cutting tools can be sharpened with relative ease, cutting tools that incorporate carbide inserts will not be sharpened. Instead, the insert will be indexed (rotating the insert to a fresh cutting edge) or replaced. Some boring bars use a cartridge system. When the boring bar gets dull, the entire cartridge is replaced. Note that if trial machining is necessary during the initial setup, it will also have to be done when dull boring bar inserts/cartridges are replaced. Tapping Tapping is done to machine threads on the inside of a hole that has been previously machined (normally by drilling). Generally speaking, a screw or bolt will be used in the tapped hole, allowing the workpiece being tapped to be fastened to some other component. Notice that while a tap has a round shank, there is a square machined at the end of the shank. This helps the cutting tool holder (a special tap holder) overcome the torque from the tapping operation. In the tap drawing, notice that there are a series of imperfect threads at the very tip of the tap. This means the tap must go deeper to provide full threads in a hole. The number of imperfect threads will be specified by the tap manufacturer. Most taps have at least three imperfect threads. Finally, notice that the distance between each crest of the thread is called the pitch (also called the lead of the thread). The thread s designation will include (or imply this pitch). Internal threads specified in the inch measurement system, for example, are specified with the thread s largest diameter, called its major diameter, and the number of threads per inch. This thread: Copyright 2011, CNC Concepts, Inc. Machining Center Setup and Operation Page19

20 1/2-13 What Does A CNC Machining Center Do? for example, specifies a 0.5 inch major diameter thread having thirteen threads per inch. The pitch for threads specified with number of threads per inch is: pitch = 1 divided by number of threads per inch For the 1/2-13 thread, for example, the pitch is inch. The tap s pitch is important when determining the required feedrate for tapping (more on why a little later). In the metric measurement system, a thread is specified with its major diameter and pitch. That is, the thread s pitch is specifies directly as part of the thread s designation. Here is an example of a thread specified in the metric system: This thread has a twelve millimeter major diameter and a 1.5 millimeter pitch. The hole before tapping Prior to tapping, the hole is machined slightly smaller than the major (largest) diameter of the thread to be tapped. How much smaller than the thread s major diameter determines the class of fit for the thread as well as how difficult the thread will be to tap. The smaller the diameter of the start hole, the tighter the fit will be, but the more difficult the hole will be to tap. The hole prior to tapping must be larger than the thread s smallest diameter (its minor diameter). Tap manufacturers provide charts to show you the recommended tap drill diameter based upon the required class of fit. Some taps have lengthy leads (imperfect threads and/or chamfer length). This requires that the hole be machined much deeper than the tapping depth. Other taps have very short leads (called bottoming taps), and require very little extra hole-depth. The lead of any tap can be calculated by multiplying the pitch of the thread (again, one divided by the number of threads per inch) times the number of imperfect threads. The tap s lead must, of course, be added to the depth required of the tapped hole. For blind holes, this means the tap drill depth must be increased accordingly. Generally speaking, through holes are best machined with plug taps. The next illustration shows a plug tap. As the thread is tapped, a plug tap will tend to push the chips machined by the tap further into the hole. Since a through hole is being machined, these chips will be sent though the hole and not interfere with the machining action. Since the chips produced by a plug tap are pushed further into the hole, a plug tap makes a poor choice for tapping blind holes. If the chip is pushed further into a blind hole, it will have nowhere to go, and eventually interfere with the machining action. In this case, a spiral flute tap should be used. The spiral flute tap (shown in the next illustration) is designed to draw the chip out of the hole along the flutes of the tap. Copyright 2011, CNC Concepts, Inc. Machining Center Setup and Operation Page20

21 Actions required for tapping The actual motions required during tapping are as follows: With the spindle running in the forward direction (assuming a right-hand thread is being machined), the tap is fed into the hole to the hole-bottom position. At the hole-bottom, the spindle direction is reversed and the tap feeds back out of the hole. Once the tap is out of the hole, the spindle reverses again (back to forward) to get ready to tap the next hole. During these motions, it is mandatory that the motion rate (feedrate) and spindle speed be perfectly synchronized. If there is any deviation in speed of feedrate during tapping, the tool will have the tendency to rise or fall relative to the tapping axis (usually the Z axis). Also, as the spindle slows down and speeds up during its change in direction at the hole-bottom, the tapping feedrate must be kept perfectly aligned with this change in spindle speed. Cutting conditions for taps As mentioned, the spindle speed and feedrate must be synchronized during the tapping cycle. The rpm for any tap can be calculated as for any tool, with the following formula: rpm = 3.82 times sfm divided by tap diameter And again, tap manufacturers will recommend the speed in surface feet per minute for the taps they make. Once the rpm is determined, the feedrate must be made to synchronize with calculated rpm. If the machining center allows feedrate to be specified in per-revolution fashion (most current machines allow this for tapping operations), you can simply specify the thread s pitch as the feedrate. When tapping, of course, the tool must move by an amount of one pitch per spindle revolution. And again, pitch for threads specified in the inch measurement system can be calculated by dividing one by the number of threads per inch. Unfortunately, feedrate for older machining centers cannot be specified in per-revolution fashion. For these machines, feedrate must be specified in per-minute fashion. This means a calculation must be done in order to determine the per-minute feedrate needed for tapping. Multiply the previously calculated rpm times the tap s pitch to come up with the per-minute feedrate. For example, consider a 3/8-16 tap. Say the tap manufacturer recommends a spindle speed of 30 sfm for tapping based upon the material you will be machining. You ll need a spindle speed of 305 rpm (30 times 3.82 divided by 0.375). The pitch for a 16 threads per inch thread is in (1 divided by 16). To come up with the feedrate for this operation, multiply in times 305 rpm. The result is inches per minute. Dull tool replacement and sharpening Most companies will not attempt to sharpen their taps. Copyright 2011, CNC Concepts, Inc. Machining Center Setup and Operation Page21

22 Milling operations You know that most hole-machining tools (like twist drills) can only machine in a plunging fashion (along the length of the tool). That is, they can only machine when they re being pushed into a hole. Once in a hole, they cannot be moved side-to-side. If they are, the tool will break. You can think of most milling cutters as being like hole-machining tools that have the additional ability to machine perpendicular to their lengthwise axis (milling on the side or periphery of the milling cutter). Some milling cutters, like center cutting end mills, can actually perform just like hole-machining tools, plunging into solid material. Here is another way to compare milling tools to the hole machining tools we ve presented so far. As you know, the only part of a hole-machining tool (like a twist drill) that is designed to do any machining is at the very end of the tool (the lips of a drill). The flutes of the drill are not designed to do any machining. By comparison, the flutes of most milling cutters (like end mills and shell mills) are designed to machine. The next illustration shows an end mill machining along in this fashion (on the side of the cutter). This kind of milling is commonly referred to as side milling (also called peripheral milling). The next illustration shows the machining operation from the perspective of the spindle. And it better illustrates that the flutes of the milling cutter are designed to machine material from the workpiece. Copyright 2011, CNC Concepts, Inc. Machining Center Setup and Operation Page22

23 Milling cutters that can plunge like hole machining tools Since hole-machining has just been presented, let s begin by looking at some milling cutters that also have the ability to machine in a plunging fashion. During the presentation of counter boring, we mentioned that end mills have the ability to counter bore a hole. All end mills have this ability, but whether or not they can plunge into solid material is based upon whether the end mill is a center cutting end mill. The next illustration shows a center cutting end mill. Though it may be a little difficult to see from this illustration, the flutes of a center cutting end mill extend to the very center of the milling cutter. This allows the milling cutter to machine a hole from solid material much like a twist drill. The bottom of the hole, of course, will be flat. Here is another illustration that may better help you understand. In the lower left corner of this illustration, you can see a cross-section of the end mill very close to its end. Again, notice that the vertical flutes come to the very center of the end mill. By comparison, end mills that are not of the center-cutting variety have a hole in the center. This hole keeps them from plunging into solid material. They can still be used for counter boring, as long as the existing hole to be counter bored is larger than the hole in the end mill. The next illustration shows an end mill that does not have center cutting abilities. Copyright 2011, CNC Concepts, Inc. Machining Center Setup and Operation Page23

24 Climb versus conventional milling Again, milling cutters have the additional ability to perform side milling operations. There are two types of side milling, based upon which way the cutter is moving as it machines. They are called climb milling and conventional milling. See the next illustration to see how climb milling is done. Climb milling In this illustration, the spindle is running in the forward direction (we re using a right-hand end mill almost all milling cutters are of the right-hand style). The milling cutter will be moving from right to left. As the cutter machines in this direction, notice that the flutes of the end mill will have a tendency to pull the end mill along the workpiece. Again, this style of side milling is called climb milling (also referred to as downhill milling). Now look at the next illustration to see conventional milling. Conventional milling The spindle is still running in the forward direction. As the cutter moves from left to right, notice that the flutes will have the tendency to push the milling cutter from the workpiece. This type of side milling is called conventional milling (also referred to as uphill milling). Climb milling tends to be less stable than conventional milling and it requires much more rigidity from the machine tool being used to perform the milling operation. Indeed, there are machine tools that cannot perform climb milling operations. Any machinist that has run a knee style milling machine (like a Bridgeport mill) knows that if climb milling is attempted, the results can be disastrous. The milling cutter will pull itself along with the cut, eliminating the machinist s ability to control the cutting motion with the machine s handwheels. Do note however, that when the machine tool provides enough stability (as most CNC machining centers do), climb milling will leave a much better finish than conventional milling. For this reason, we recommend climb milling if you have a machining center with sufficient rigidity and strength. Copyright 2011, CNC Concepts, Inc. Machining Center Setup and Operation Page24

25 Radial and axial depth of cut Since milling cutters can perform side milling operations, there are two more important cutting conditions related to milling: radial depth-of-cut and axial depth-of-cut. As the next illustration shows, radial depth-ofcut is the amount of material being machined by the periphery of the cutter. The axial depth-of-cut is the depth the cutter is milling along its lengthwise axis. Most cutting tool manufacturers will provide recommendations related to the maximum radial and axial depths-of-cut a given milling cutter can machine. They may say something like radial depth of cut should not exceed 30% of the cutter s diameter and axial depth of cut should not exceed the cutter s diameter. Left end view Top view Axial depth of cut Radial depth of cut Front view Rough milling versus finish milling Depending upon the surface finish and size requirements for a given milling operation, it may be necessary to rough machine the surface close to its finish size and then finish mill the surface. In some cases, the same milling cutter is used to both rough and finish mill. But it is almost always better to use two separate milling cutters, one to rough mill and the other to finish mill. This is especially true when many workpieces must be produced, since a milling cutter used solely for finishing will last much longer than one used for both rough and finish milling. For rough milling operations, some milling cutter manufactures will recommend the amount of material to be left for finish milling (called finishing stock), but most will assume the person using the milling cutter will know how much stock should be left for finishing. Generally speaking, stock left on the side (radial depth of cut for the finishing end mill) will range between and inch. Stock left on the top surface (the axial depth of cut for finish milling) is usually between and 020 inch. As mentioned, it is usually best to use two different milling cutters when rough and finish milling must be done. Indeed, there are special milling cutters that have been specifically designed to perform rough milling operations. These milling cutters cannot perform finish milling operations (they leave a very poor surface finish). They are designed to remove a large amount of material as quickly as possible without much concern for the surface finish they leave. The next illustration shows one. These cutters are commonly referred to as hog mills. Copyright 2011, CNC Concepts, Inc. Machining Center Setup and Operation Page25

26 Notice the serrated flutes of this end mill. It actually looks like a tap but again this is an end mill that has been specifically designed for rough milling. Cutting tool material Like many hole-machining cutting tools, milling cutters are available with different cutting-edge materials. Also like hole-machining cutting tools, some milling cutters are comprised solely one material (like high speed steel, cobalt, or even carbide). With other milling cutters, the shank is made from one material and the cutting edges (inserts) are made from another material like carbide or coated carbide. As an example, here are some end mills that are entirely made from one material. Sometimes an end mill is made from one material like high speed steel or cobalt and then coated with a much harder material. This is done to prolong the life of the milling cutter. In the next illustration, the end mill second from the left is coated with such a material (though it is not possible to see from the illustration, it has a gold-colored coating). The next illustration shows an inserted end mill. With this milling cutter, the shank is made of steel and only the cutting edges (inserts) are made of the cutting tool material like carbide or coated carbide. Copyright 2011, CNC Concepts, Inc. Machining Center Setup and Operation Page26

27 Insert placement is critical with inserted milling cutters. When placed in the milling cutter body, the seat area must be clean free of chips and other debris. The screw holding the insert must be secure, but not too tight. Carbide inserts are brittle and will shatter if there is any debris in the seat or if too much clamping pressure is applied. Cutting conditions for milling operations As with hole-machining operations, the two primary cutting conditions for milling operations are spindle speed and feedrate. And like recommendations for hole-machining tools, spindle speed will be recommended in sfm or mpm, depending upon your measurement system. You will need to calculate speed in rpm based upon the milling cutter s diameter, just as you do for hole-machining tools. Recommended feedrate will be specified in per-tooth fashion. (Some milling cutter manufacturers refer to the per-tooth feedrate as chip load.) Per-tooth actually means per-flute or per-insert. You ll first need to calculate the per revolution feedrate which is easy to do: per revolution feedrate = per-tooth feedrate times the number of teeth (flutes, or inserts) Once you know the per-revolution feedrate, you can calculate the per-minute feedrate by multiplying the previously determined spindle speed in rpm times the per-revolution feedrate. There are at least two additional cutting condition criteria for milling operations. First, the depth of cut (both radial and axial) will dramatically affect optimum cutting conditions for the milling operation. The more material being removed, the slower will be the cutting conditions (at least for feedrate). Though some milling cutter manufacturers will consider both radial and axial depth of cut in their recommendations, many do not. You will probably be expected to adjust the feedrate recommendations they provide based on the amount of material the milling cutter will be removing. Second, most milling cutter manufacturers will base recommendations on whether the milling cutter will be performing a rough milling or finish milling operation. Generally speaking, finish milling is done with a faster cutting speed, but with a slower feedrate (per-tooth). The next illustration shows one end mill manufacturer s method for recommending cutting conditions. Copyright 2011, CNC Concepts, Inc. Machining Center Setup and Operation Page27

28 Notice that they provide speed and feedrate (per tooth) based upon the material being machined. They also consider the milling cutter s diameter in the feedrate recommendation. But they do not address roughing or finishing in the chart. They do mention radial and axial depth-of-cut in the notes preceding the chart (axial depth of cut not to exceed one times the diameter and radial depth of cut not to exceed 30% of the diameter). They also mention what to do if the milling cutter will be used to machine a slot (doc stands for depth-of-cut). But do note that this manufacturer makes no special recommendations based upon whether the milling cutter is rough milling or finish milling (other than the rather cryptic note about using standard milling practices ). Example: Say you are finish a surface in mild steel with a 0.5 inch diameter high speed steel (hss) end mill that has four flutes. The end mill manufacturer recommends a speed of 80 sfm and a feedrate of ipt. Spindle speed will be 611 rpm (80 times 3.82 divided by 0.5). Feedrate will be ipm ( times 4 times 611). Types of milling cutters With the basics of milling operations understood, let s look at the specific types of milling cutters available. End mills We ve presented much about end mills during the previous introduction to milling operations. Here is a quick summary of the key points we ve made:? End mills can be made of one material (like high speed steel).? End mills can be inserted the shank is made of one material (like steel) while the cutting edges (inserts) are made of a much harder material (like carbide).? Radial depth-of-cut is the amount of material being removed by the periphery of the end mill.? Axial depth-of-cut is the amount of material being removed along the lengthwise axis of the end mill.? There are two different ways to side mill, climb milling and conventional milling.? Center cutting end mills can plunge into solid material, just like a drill.? End mills that are not center cutting can still plunge, but the existing hole in the workpiece must be larger than the hole in the center of the end mill.? End mills can be used to rough mill and finish mill and there are end mills that have been specifically designed to perform roughing operations (commonly called hog mills). Copyright 2011, CNC Concepts, Inc. Machining Center Setup and Operation Page28

29 ? Speed and feedrate recommendations are based upon the size of the end mill, the end mill s cutting material, the workpiece material, the radial and axial depth of cut, and whether the end mill is rough machining or finish machining. End mills can be used to perform a variety of milling operations. Here are a few of the countless milling operations that can be performed by end mills. Circle milling a counter bored hole The larger a counter bored hole, the larger the counter boring tool must be. In many cases, it makes more sense to mill the counter bored hole using a circular motion than it does to use a very large (expensive) counter boring tool. Additionally, one milling cutter can be used to mill any number of different sized holes. The next illustration shows a hole that has been counter bored by an end mill in this fashion. It is likely that the hole being milled in this illustration has been rough milled and finish milled. Pocket milling End mills are commonly used to machine the material out of pockets. Pockets can be round, square, rectangular, or just about any shape. A center cutting end mill must be used if the end mill must plunge into the pocket prior to opening it up in the X and Y axes. It is also possible to start a pocket by drilling a hole at the location where the end mill will begin machining. The next illustration shows the machining of an irregularly shaped pocket. Keyway and slot milling An end mill can be used to mill a slot equal to or greater than its diameter. The next illustration shows a keyway milling operation. Copyright 2011, CNC Concepts, Inc. Machining Center Setup and Operation Page29

30 Face milling For small workpieces, an end mill can be used to machine the top surface of the workpiece in a face milling manner. However, there are special cutting tools (called face mills) that are designed specifically for this operation. Face mills allow a large surface to be milled. (We will show face mills next.) Exterior peripheral milling End mills can be used to machine exterior surfaces from a workpiece. They can mill any side of the workpiece (front, back, left, or right sides). And they can machine an entire exterior contour. The next illustration shows an example. Face mills Though an end mill can perform a face milling operation, a face mill is specifically designed for this purpose. The next illustration shows one. As the name implies, a face mill is used to machine an upper surface (face) of a workpiece, as the next illustration shows. Face milling is usually done early in the CNC machining center process to make a nice flat surface into which other machining operations (like drilling and tapping) will be done. Copyright 2011, CNC Concepts, Inc. Machining Center Setup and Operation Page30

31 Like end mills, face mills are specifically designed for both roughing and finishing operations. Actually, the same face mill cutter body is often used for both roughing and finishing, but the inserts will be different for rough face milling versus finish face milling. Generally speaking, spindle speed will be faster for finishing, yet feedrate will usually be slower (per tooth). The depth of cut for rough face milling can be up to 0.25 inch (or more) as long as the CNC machining center has the ability to make such a heavy cut. When rough face milling, most programmers will leave between and inch of material for finishing. As you can see by a previous illustration, face milling cutters have several inserts. Generally speaking, the larger the face mill, the more inserts it will have. Other milling cutters There are some milling cutters that have a very specific application. Here we list a few. Copyright 2011, CNC Concepts, Inc. Machining Center Setup and Operation Page31

32 Ball and bull end mills Ball end mills can be used to machine a fillet radius on a workpiece. As you can see, the end of a ball end mill is in the form a complete radius. They provide the ability to machine a fillet radius. A bull end mill will also allow a fillet radius to be machined. As you can see, the radius on the end of the bull end mill is not a full radius that is it doesn t extend all the way to the center of the end mill. Ball and bull end mills are often used when three dimensional shapes must be machined. A computer aided manufacturing (CAM) system is required to prepare the program for three dimensional machining. After importing a drawing of the workpiece to be machined (usually from a computer aided design or CAD system, the programmer will tell the cam system to machine as much of the workpiece as possible with a relatively large ball or bull end mill. This will cause the CAM system to rough as much of the workpiece as possible. Copyright 2011, CNC Concepts, Inc. Machining Center Setup and Operation Page32

33 But there will be workpiece attributes that cannot be machined by the large ball or bull end mill. So the programmer will then specify a new (smaller) cutter and have the CAM system repeat the process. Now the CAM system will generate programmed movements to continue machining the workpiece. This process (choosing smaller and smaller ball or bull end mills) will be repeated until the all surfaces of the workpiece have been machined. Slotting cutters We mentioned that end mills can machine slots, but there is a milling cutter specially designed to do so the slot milling cutter. From the next illustration, notice how much this cutter resembles a circular saw blade. The tool holder for this kind of cutter provides an arbor to which the milling cutter is clamped. Copyright 2011, CNC Concepts, Inc. Machining Center Setup and Operation Page33

34 Thread milling cutters During the presentation of hole-machining operations, you learned that one way to machine threads inside a hole is to use a tap. But as you know, a tap requires a great deal of torque. The larger the tap, the more torque will be required. Additionally, there is no way to control the diameter of a tapped hole diameter is part of the tap design. When holes are too large to be tapped and/or when you need better control of the major diameter being threaded in the hole, you can use a thread milling cutter to machine the thread. Note that an additional benefit of thread milling cutters is that they can machine external (male) threads as well as internal threads (female). Motions needed for thread milling The motions needed for thread milling may be a little tough to visualize. The thread milling cutter will be moving in three axes (X, Y, and Z) when milling a thread. Two of the axes (X and Y) will move in a circular fashion while the third axis (Z) will be moving in a linear fashion. The motion resembles a spiraling motion, but the radius of the spiral remains constant. The next illustration shows the motion The illustration includes the approach motion (arc-in), the milling around the thread, and the escape motion (arc-out). Note that the amount of Z axis motion will be related to the thread pitch being machined. If making a half circle motion around half the thread, the tool will have to move by a value of half the pitch in the Z axis. Machining the entire thread in one pass There are actually three different styles of thread milling cutters being used on CNC machining centers. Two of them have the ability to machine the entire thread in one pass. The first resembles a tap. The next illustration shows it. Copyright 2011, CNC Concepts, Inc. Machining Center Setup and Operation Page34