Lesson 2 Understanding Turning Center Speeds and Feeds

Lesson 2 Understanding Turning Center Speeds and Feeds Speed and feed selection is one of the most important basic-machining-practice-skills a programmer must possess. Poor selection of spindle speed and feedrate can result in poor surface finish, scrapped parts, and dangerous situations. Even if speeds and feeds do allow acceptable workpieces to be machined if they re not efficient productivity will suffer. As you know, spindle speed is the rotation rate of the machine s spindle (and workpiece). Feedrate is the motion rate of the cutting tool as it machines a workpiece. These two cutting conditions are extremely important to machining good workpieces. You will select a spindle speed and feedrate for every machining operation that must be performed. Cutting tool manufacturers supply technical data including the recommendation of a cutting speed and feedrate for the cutting tools they supply. Recommendations are based on three important factors: 1) The machining operation to be performed 2) The material to be machined 3) The material of the cutting tool s cutting edge The machining operation to be performed This criterion determines the style of cutting tool that must be used to perform the machining operation. As the programmer, you will be the person making this decision. It requires that you draw upon your basic machining practice experience. As stated in the Preface and Lesson One, turning centers can perform a wide variety of machining operations, and specific cutting tools are used to perform each operation. The specified spindle speed and feedrate must be appropriate to the cutting tool selection. Some cutting tools, like rough turning tools, perform very powerful machining operations and can remove a great deal of material from the workpiece per pass while others, like small boring bars, perform lighter machining operations and can only remove a small amount of workpiece material per pass. The material to be machined This criterion determines (among other things) how quickly material can be removed from the workpiece. Soft materials, like aluminum can be machined faster than hard materials, like tool steel. So generally speaking, you ll use faster spindle speeds and feedrates for softer materials. The material of the cutting tool s cutting edge The material used for some cutting tools comprises the entire tool. A standard twist drill or end mill, for example, is made entirely of high speed steel (or cobalt, or some other material). With other tools, like many turning tools, boring bars, grooving tools, and threading tools, the shank of the tool is made from one material (like steel), while the very cutting edge of the tool is made from another material (like carbide or ceramic). This lowers the cost of the cutting tool. With these kinds of cutting tools, only the cutting edge of the cutting tool is made from the (expensive) cutting tool material. The cutting edge component of the tool is called an insert. Figure 1.15 shows this kind of cutting tool. Copyright 2011, CNC Concepts, Inc. CNC Turning Center Programming Page 1

Typical inserted turning tools Clamp Shank Insert Clamp Figure 1.15 Examples of cutting tools that use inserts The cutting tool material also determines how quickly machining can be done. Generally speaking, the harder the cutting tool material, the faster machining can be done. Based upon knowing these three criteria, spindle speed and feedrate selection is usually quite simple. You simply reference the cutting tool manufacturer s recommendations. These recommendations along with other cutting condition recommendations like depth of cut are usually provided in the tooling manufacturer s technical manuals or they may be right in the sales catalog for the cutting tools. Speed will be recommended in surface feet per minute (sfm) if the data is given in inch, or meters per minute if the data is given in metric (most cutting conditions provided in the United States are given in inch). This is the amount of material (in feet or meters) that will pass by the tool s cutting edge in one minute. Feedrate will be recommended in per revolution fashion (either inches or millimeters per revolution ipr or mmpr). Say for example, you must finish turn 1018 cold-drawn steel with a finish turning tool that has a carbide insert. You look in the tooling manufacturer s technical handbook and find they recommend a speed of 700 surface feet per minute and a feedrate of 0.005 inches per revolution. With conventional turning equipment like engine lathes and turret lathes, there is only one way to specify spindle speed (in rpm) and one way to select feedrate (in per revolution fashion). Since the speed for conventional lathes must be specified in rpm, a machinist must to convert the 700 sfm to the appropriate speed in rpm based on the diameter of the workpiece that is being machined. Here is the formula to do so: Rpm = sfm times 3.82 divided by the diameter to be machined If, for example, the workpiece diameter to be machined is 4.0 inches, the necessary speed for 1018 colddrawn steel (if it is to be run at 700 sfm) will be 668 rpm (700 times 3.82 divided by 4.0). As you can imagine, calculating spindle speed in rpm can be pretty cumbersome, especially if several diameters must be machined by the same tool. And consider a facing operation. As soon as a facing tool begins moving, the diameter it is machining will change. The two ways to select spindle speed CNC turning centers allow you to specify spindle speed in two ways. You can do so in rpm, or you can specify spindle speed directly in surface feet per minute (or meters per minute if you are working in the metric mode). In our previous turning example, this means you can specify the spindle speed to be used as 700 sfm eliminating the rpm calculation. This second method of selecting spindle speed for CNC turning centers is called constant surface speed (css). As the name implies, constant surface speed will cause the machine to constantly update (change) the spindle speed in rpm to maintain the specified speed in surface feet per minute (or meters per minute if you work in Copyright 2011, CNC Concepts, Inc. CNC Turning Center Programming Page 2

the metric mode). As a cutting tool moves in the X axis (changing diameter), spindle speed in rpm will also change. As the cutting tool moves to a smaller diameter, speed in rpm will increase. As it moves to a larger diameter, spindle speed in rpm will decrease. Two preparatory functions (G codes) specify which of the spindle speed modes (rpm or css) you want to use for speed selection. G96 select constant surface speed mode G97 select rpm mode An S word specifies the actual speed. Three M codes are used for spindle activation. M03 - Spindle on forward (right hand tools) M04 - Spindle on reverse (left hand tools) M05 - Spindle off Here are two examples (working in the inch mode): N050 G96 S500 M03 (Turn spindle on forward at 500 sfm) N050 G97 S500 M04 (Turn spindle on reverse at 500 rpm) As stated, constant surface speed mode (G96) will cause the machine to constantly and automatically update the spindle speed in rpm based on the current diameter the cutting tool is machining. If for example, you have selected a speed of 500 sfm and the tool is currently machining a 3.5 in diameter, the machine will run the spindle at 546 rpm (3.82 times 500 divided by 3.5). There will be no need for you to perform the spindle rpm calculation the machine does this for you. If facing a workpiece (machining direction is X minus), the machine will constantly increase the spindle rpm as the facing operation occurs. See Figure 1.16 for a graphic illustration of how the diameter being machined changes during a facing pass and the impact this has on spindle speed in rpm. Constant surface speed automatically determines speed in rpm Using a speed of 500 sfm... (G96 S500 M03) 2.0 dia. 955 rpm 4.0 dia. 477 rpm 6.0 dia. 318 rpm When the facing tool reaches center (diameter of zero), the spindle will be running at its maximum speed in rpm Figure 1.16 Drawing illustrates a facing tool that is machining to the center of a workpiece When to use constant surface speed mode You should use constant surface speed mode (G96) whenever a single point cutting tool will be machining more than one diameter on the workpiece. Examples include rough and finish facing, rough and finish turning, rough and finish boring, necking (grooving), and cutting off (parting). Copyright 2011, CNC Concepts, Inc. CNC Turning Center Programming Page 3

For these kinds of operations, constant surface speed provides three important benefits: 1) Constant surface speed simplifies programming. As you have seen, it eliminates the need for rpm calculations. 2) Since the appropriate rpm will be used as machined diameters change, the witness marks (finish) on the workpiece will be consistent from one surface to another. This is also related to the fact that feedrate will be specified in inches per revolution (ipr) or millimeters per revolution (mmpr). As the spindle speed changes, so does the feedrate per minute (feedrate selection is presented later in this lesson). 3) Since spindle speed in rpm will be correct during all machining operations, tool life will be extended to its maximum. When to use rpm mode There are three times when constant surface speed cannot be used so spindle speed in rpm must be calculated and specified in the rpm mode (G97). First, you must specify spindle speed in rpm for any cutting tool that machines right on the spindle s centerline. We call these tools center-cutting tools. Examples include drills, taps, and reamers. These tools machine a hole right in the center of the workpiece. Again, these tools are sent right to the spindle s centerline (a diameter of zero). If you specify speed in the constant surface speed mode (G96) for a center cutting tool even as just one surface foot per minute the spindle will run at its maximum speed in rpm when a cutting tool is sent to a diameter of zero. (3.82 times one divided by zero is infinity). When you machine with a center cutting tool, you must calculate and specify spindle speed in rpm. If for example, you must drill a 0.75 diameter hole and the drill manufacturer recommends a speed of 80 sfm based upon the material you are machining, the required speed will be 407 rpm (3.82 times 80 divided by 0.75). Second, rpm mode must be used when chasing threads. The machine must perfectly synchronize the spindle speed with the feedrate motion during the multiple thread-passes required for machining a thread. With most machines, this cannot be done in the constant surface speed mode. And third, if your machine has live tooling (introduced in Lesson One), spindle speed must always be specified in rpm when live tool are being used. We ll mention one more time that some programmers elect to use the rpm mode even though constant surface speed could be used. When a turning tool or boring bar is machining but one diameter (or even several diameters that are close together), there is not much of an advantage to using constant surface speed other than eliminating the need for the rpm calculation. So some programmers will calculate an rpm based upon the largest diameter being machined and program the operation in the rpm mode. See Figure 1.17 for an example. Copyright 2011, CNC Concepts, Inc. CNC Turning Center Programming Page 4

Rpm change will be small, so some programmers use rpm mode At 500 sfm: 2.0 995 rpm required 1.875 1,086 rpm required 1.75 1,091 rpm required Since the rpm change from the smallest diameter to the largest diameter is small (under 100 rpm), some programmers will use the rpm mode and specify the speed for the larges t diameter to be machined (995 rpm in this case). Figure 1.17 With small diameter changes, rpm changes will also be small How fast will the spindle be running when constant surface speed is used? Say you re going to be rough turning a mild steel workpiece with a cutting tool that has a carbide insert. The cutting tool manufacturer recommends that you run the spindle at 500 sfm. In the program at the beginning of the tool, you give this command: N050 G96 S500 M03 This command will start the spindle at 500 sfm (assuming the inch mode is being used) in the forward direction. But when the spindle starts, how fast will it be running in rpm? Based upon the information just provided, you cannot answer this question. Prior to answering, you must know the diameter at which the cutting tool is currently positioned. And even then, you must perform the rpm calculation (3.82 times sfm divided by diameter). For people that have experience running a conventional lathe, this can be a little unnerving. Machinists are accustomed to specifying spindle speed directly in rpm so when the spindle starts on a conventional lathe, they will know precisely how fast the spindle will run in rpm. If you want to know the precise rpm at which the spindle will start with CNC turning centers (when specifying speed in the constant surface speed mode), you must perform the rpm calculation and you must know the diameter position of the cutting tool in order to perform this calculation. How fast can the spindle rotate? As stated in Lesson One, you must reference the machine tool builder s documentation (commonly the programming manual) in order to determine your machine s spindle characteristics. Say, for example, you find that your turning center has two spindle ranges. The low range runs from 0 1,500 rpm. The high range runs from 0 5,000 rpm. This means, of course, that when the spindle is in the low range, it cannot run any faster than 1,500 rpm. When it is in the high range, it cannot run faster than 5,000 rpm. When you specify spindle speed in the constant surface speed mode, the current spindle range (low or high) will determine the maximum spindle speed. Using the rpm calculation, the machine will attempt to run the spindle at the appropriate rpm. If the rpm calculation renders a speed in rpm that is higher than the maximum speed allowed in the current spindle range, the spindle will simply peak out at the maximum rpm of the spindle range and run at this speed. Consider these scenarios for the machine just described. Scenario number one: Say you are rough turning a workpiece from an 8.0 diameter down to a 1.0 diameter. Based upon the cutting tool being used and workpiece material being machines, the cutting tool manufacturer recommends a speed of 800 sfm. Since this is a powerful machining operation, you select the low spindle range. Copyright 2011, CNC Concepts, Inc. CNC Turning Center Programming Page 5

When rough turning begins, the spindle will be running at about 334 rpm (3.82 times 800 divided by 8.0). As the rough turning tool makes roughing passes, the spindle speed in rpm will increase. When the rough turning tool reaches 2.0 in diameter, the spindle will attempt to run at 1,528 rpm (3.82 times 800 divided by 2.0). Since the maximum rpm in the low spindle range for this machine is 1,500 rpm, the machine will not be able to achieve the appropriate rpm. It will peak out at 1,500 rpm. If you continue to rough turn the workpiece in the low spindle range, this rough turning pass as well as the rest of the roughing passes will be performed at 1,500 rpm. Scenario number two: Whenever you face a workpiece to center (a common machining operation), the spindle will run up to the maximum speed of the current spindle range. For our example machine, this means it will run up to 1,500 rpm if the low range is selected or 5,000 rpm if the high range is selected. For small, perfectly round workpieces, this will be acceptable. The workpiece will run true in the spindle all the way up to the machine s maximum speed even in the high range. But you must exercise extreme caution when workpieces are larger and especially when they are not perfectly round. Castings, for example, are notorious for being out-of-round. An out-of-round workpiece will wobble in the workholding device when the spindle rotates. The faster the spindle runs, the more machine vibration this wobbling will cause. Of course, wobbling is caused by the fact that the workpiece is not truly concentric with the spindle and it will place stress on the workholding device used to secure the workpiece. If this stress is excessive, the workpiece will actually be released by the workholding device. This makes for a very dangerous situation. A workpiece that is rotating at a very high rate will be bouncing around inside the machine and could actually come right through the door of the machine. When you must machine large workpieces that are not truly round, you must be very careful not to allow the spindle to reach a speed in rpm that causes the machine to vibrate. A test can be made during the machine s setup to determine this maximum spindle speed. Once you know how fast the spindle/workpiece can safely rotate, you can specify a spindle limiting command in the program that will keep the spindle from exceeding this speed. The maximum spindle speed test: The setup person will load a workpiece and start the spindle at a very slow rpm. They will continue to increase the spindle speed in small increments until they start to feel vibration. The speed at which the machine begins to vibrate will be reduced by about twenty percent and will be the maximum speed for this workpiece while it is in its rough state. How to specify a maximum speed for the constant surface speed mode Here is a way to limit the maximum speed in rpm that the spindle can achieve. In essence, you will be superseding the maximum rpm of each spindle range. The spindle limiter is specified with a G50 command. The command N055 G50 S2000 (Limit spindle speed to 2,000 rpm) specifies that the spindle will not be allowed to exceed 2,000 rpm, even if the constant surface speed mode is being used and the machine has calculated a speed that is greater than 2,000 rpm. If this command is specified at the beginning of the program for our example machine (maximum speed in the high range is 5,000 rpm), the spindle will not be allowed to run faster than 2,000 rpm, even if the high range is selected. If, after specifying the spindle limiter shown above in line N055, you program a facing tool to face to center (zero diameter) in the high spindle range, the spindle will peak out when it reaches 2,000 rpm. A potential limitation of constant surface speed While constant surface speed is an extremely important programming feature, we must point one potential limitation. If it is not efficiently programmed, it can increase program execution (cycle) time. The reason for this has to do with the fact that a turning center s spindle cannot instantaneously respond to speed changes in rpm. It takes time for the machine to respond to spindle rpm changes. How much time rpm changes take for a given turning center is based on several factors, including machine size, horsepower, size & weight of the work holding device, and weight of the workpiece being machined. Copyright 2011, CNC Concepts, Inc. CNC Turning Center Programming Page 6

Generally speaking, the bigger the machine, the more the time it takes for the spindle to respond to rpm changes. One way to determine spindle response time is to actually measure it with a stop-watch. Say you do so and find these characteristics for one of your machines: 0-1,000 rpm takes 2 seconds 0-2,000 rpm takes 4 seconds 0-3,000 rpm takes 6 seconds 0-4,000 rpm takes 8 seconds Say your program has a turret index position of 8.0 inches in diameter (the X axis). This position provides ample clearance for safely indexing the turret. When each tool is finished machining, it is sent to this position. If the machine is in the constant surface speed mode (and assuming the workpiece is smaller than 8.0 inches in diameter), the spindle will slow down during this motion. If the speed is 600 sfm, for example, the spindle will be running at 286 rpm whenever a cutting tool is at this 8.0 inch diameter turret index position. When you command a cutting tool to approach a workpiece in the X axis, the spindle speed in rpm will increase accordingly. Say the tool is approaching to a 0.75 in diameter. At 600 sfm, the spindle will increase to 3,056 rpm. For the example machine just shown, this will take six seconds. It s likely that the approach movement will occur much faster than the spindle response, meaning the machine will pause for about five seconds, while the spindle gets up to speed. The reverse will happen during each tool s retract to the 8.0 inch diameter turret index position (slowing back to 286 rpm). For each of these approach/retract motions, about five seconds will be added to program execution time (for our example machine). This is the reason why constant surface speed can waste cycle time if not efficiently programmed. We ll show how to efficiently program constant surface speed in Lesson Twelve. The two ways to specify feedrate As with spindle speed, there are two ways to specify feedrate for CNC turning centers. As mentioned in Lesson One, feedrate can be specified in per revolution fashion (inches or millimeters per revolution) or in per minute fashion (inches or millimeters per minute). Again, two G codes are used to specify which feedrate mode will be used. G98 feed per minute G99 feed per revolution When you power up on a CNC turning center, the feed per revolution mode (G99) is automatically selected. (By the way, CNC words that are automatically selected at power-up are called initialized words.) This means that if you do not include a feedrate mode specifying G code in a program, the machine will assume the feed per revolution mode. You ll notice that many of the example programs provided in this text make this assumption (they don t include a G99). Also as mentioned in Lesson One, an F word actually specifies feedrate. Here are two examples (assuming you are working in the inch mode). N060 G98 F30.0 (Feedrate of 30.0 ipm) N060 G99 F0.012 (Feedrate of 0.012 ipr) When to use the feed per revolution mode We recommend using the feed per revolution feedrate mode (G99) for almost all machining operations you perform on CNC turning centers. In the per revolution feedrate mode, feedrate specifies how far the cutting tool will move during one spindle revolution. Per revolution feedrate mode is especially helpful with cutting tools that use the constant surface speed mode (like rough and finish turning tools, rough and finish facing tools, rough and finish boring tools, and grooving tools). As the spindle changes speed in rpm based upon the current diameter position of the cutting tool, the Copyright 2011, CNC Concepts, Inc. CNC Turning Center Programming Page 7

feedrate in inches or millimeters per minute will also change. This will cause witness marks (finish) to be consistent for all surfaces being machined. Even if you re using the rpm mode (possibly for a drill that machines a hole in the center of the workpiece), it is always easier to specify feedrate in per revolution fashion. Again, most cutting tool manufacturers recommend feedrates for their cutting tools in per revolution fashion. When to use the feed per minute feedrate mode Frankly speaking, about the only time we recommend using the feed per minute mode is when you must cause a controlled motion with the spindle stopped. If the spindle is stopped, of course, the axes will not move regardless of how large a feedrate is specified in the per revolution mode. If your turning center has a bar feeder, for example, and if the bar feed operation requires the spindle to be stopped prior to feeding a bar, the feed per minute mode must be used for the bar advance motion (bar feeder programming is shown in Lesson Nineteen. If your turning center is equipped with live tooling, operations performed with live tools require that the machine be in the live tooling mode (not the normal turning mode). In live tooling mode, the machine s main spindle is off (at least from a turning operation standpoint), meaning that feedrate for live tools must be programmed in per minute fashion. Calculating feedrate per minute To calculate feedrate in per minute fashion, multiply the desired feedrate per revolution times the previously calculated spindle speed in rpm. For example, say you must use the live tooling mode and drill a 0.5 diameter hole. For the material you must machine, the drill manufacturer recommends a speed of 80 sfm and a feedrate of 0.008 ipr. First, calculate the speed in rpm 3.82 times 80 divided by 0.5 or 611 rpm. Now multiply 611 times 0.008 which renders a per-minute feedrate of 4.88 ipm. Again, any time you must cause a feedrate motion when the spindle is stopped, you must use the feed per minute mode. One other example is when performing a light broaching operation. Some programmers do prefer to use the feed per minute mode for operations when the feedrate will remain consistent in feed per minute for the entire machining operation (even though feed per revolution could be used). When drilling a hole, for example, once the feed per minute is calculated, it will work for the entire drilling operation. An example of speed and feed usage Figure 1.18 provides an illustration of what happens when you use the constant surface speed spindle mode with the per revolution feedrate mode to perform machining operations. Notice that spindle rpm changes with workpiece diameter. So does feedrate in inches per minute change with changes in spindle rpm. How sfm and ipr selection affect rpm and ipm during machining 4.0 dia 477 rpm 3.34 ipm 2.75 dia 694 rpm 4.86 ipm Turret index position 8.0 238 rpm 1.0 dia 1910 rpm 13.37 ipm For this finish turning operation, you have specified a speed of 500 sfm and a feedrate of 0.007 ipr. Figure 1.18 How spindle speeds and feedrates change as a workpiece is machined Copyright 2011, CNC Concepts, Inc. CNC Turning Center Programming Page 8

As you study Figure 1.18, notice how many speed and feed calculations the machine is making all based upon your spindle speed selection in surface feet per minute and feedrate selection in inches per revolution. Key points for Lesson Two: With CNC turning centers, there are two ways to specify spindle speed (constant surface speed and rpm) and two ways to specify feedrate (feed per revolution and feed per minute). Constant surface speed mode (G96) should be used with single point turning tools that machine more than one diameter during the machining operation. Rpm mode (G97) must be used for tools that machine on center (like drills) and for threading operations. Constant surface speed mode will cause the machine to automatically select the appropriate spindle rpm based upon the specified speed in surface feet/meters per minute and the current diameter position of the cutting tool. Per revolution feedrate mode (G99) is initialized (automatically selected at power-up) and should be used for almost all machining operations. Feed per minute mode (G98) should only be used for feedrate movements when the main spindle is stopped. Using per revolution feedrate mode will ensure that witness marks (surface finish) on the workpiece will be consistent for all surfaces being machined. Rpm = 3.82 times sfm divided by the diameter being machined. Ipm = previously calculated rpm times feedrate per revolution. 1) Which spindle speed mode should you select for cutting tools that machine more than one diameter? A) Constant surface speed mode B) Rpm mode 2) Which feedrate mode should you use for almost all machining operations? A) Per revolution mode B) Per minute mode Quiz 3) Provide a CNC command that will start the spindle at 400 sfm in the forward direction. 4) Provide a CNC command that will start the spindle at 500 rpm in the reverse direction. Answers: 1: A, 2: A, 3: G96 S400 M03, 4: G97 S500 M04 Copyright 2011, CNC Concepts, Inc. CNC Turning Center Programming Page 9