Coordinate System Techniques

Transcription

1 Coordinate System Techniques In this lesson, we ll show some advanced implications of what can be done with coordinate systems. For the most part, this lesson applies to machining centers. But there are some points we ll make about turning center coordinate systems as well. G52 - temporary shift of program zero on machining centers As you know, all coordinates going into your programs are taken from program zero if you work in the absolute mode. In most cases, this makes programming simpler. However, there is one time when specifying coordinates from one centralized program zero point is rather cumbersome. If, for example, you have multiple identical machining operations to perform, it can be helpful for manual programmers to develop a subprogram that machines but one of the operations. This subprogram can be recalled and executed for as many operations as are required. However, if the subprogram is written in the absolute mode from the centralized program zero point, when it is repeated, it will perform the same operation in the same location (not machining in a different location). For this reason, many programmers will develop the subprogram in the incremental mode, ensuring that the machining operation will take place in different locations. Developing any series of motions in the incremental mode is tedious and error prone. Though it s only available on newer Fanuc controls, G52 will allow you to temporarily shift the program zero position from the centralized location to a more convenient position relative to the machining operation being performed. When this command is given N060 G52 X4.0 Y3.0 the control will shift the program zero point from the centralized location (specified in the currently instated fixture offset) to a location of X4.0 and Y3.0. If you wish to switch again, the command N175 G52 X7.0 Y5.0 will shift program zero again. Note that these values are not accumulative. This command will still shift from the centralized program zero point (not from the last shifted location). When you re finished using this technique, you must remember to shift the program zero point back to its original position. The command N250 G52 X0 Y0 will do just that. Here is an example that stresses the use of G52. The next drawing shows the workpiece to be machined. 1

2 Drawing shows workpiece for G52 example. Note multiple pockets must be machined. Here is the main program: O0006 (Main program number) N005 G54 G90 S600 M03 (Select coordinate system, absolute mode, turn the spindle on) N010 G00 X0.75 Y0.75 (Move to beginning point of left most slot) N015 G43 H01 Z.1 (Instate tool length compensation) N020 G52 X0.75 Y0.75 (Shift program zero to lower side of left-most slot) N025 M98 P1006 (Execute program O1006 to machine the first slot) N030 G52 X1.625 Y0.5 (Shift program zero to lower side of second slot) N035 M98 P1006 (Execute program O1006 to machine second slot) N040 G52 X2.5 Y0.75 (Shift program zero to lower side of third slot) N045 M98 P1006 (Execute program O1006 to machine third slot) N050 G52 X3.375 Y0.5 (Shift program zero to lower side of fourth slot) N055 M98 P1006 (Execute program O1006 to machine fourth slot) N060 G52 X4.25 Y0.5 (Shift program zero to lower side of fifth slot) N065 M98 P1006 (Execute program O1006 to machine fifth slot) N070 G52 X0 Y0 (Shift coordinate system back to normal position) 2

3 N075 G91 G28 Z0 M19 (Return to tool change position) N080 M30 (End of program) Note that each G52 shifts the program zero point to the lower Y axis center of the slot (point 1 in the tool path drawing). This becomes the point of reference (program zero) for the subprogram s movements. Here is the subprogram written in the absolute mode. All coordinates programmed after a G52 are shifted to the temporary coordinate systems. Note that you must remember to shift back to the original coordinate system (done in line N070) when you re finished. Now, here is the subprogram being called that machines one slot. Note that it is written in the absolute mode. O1006 (Subprogram to machine one slot) N1 G00 X0 Y0 (Move to point 1) N2 G01 Z-0.25 F2.5 (Plunge into slot) N3 Y1.75 F5.0 (Mill to point 2) N4 G41 D31 X-0.25 (Instate cutter radius comp, move to point three) N5 Y0 (Mill to point 4) N6 G03 X0.25 R0.25 (Circular mill to point 5) N7 G01 Y1.75 (Mill to point 6) N8 G03 X-0.25 R0.25 (Circular mill to point 7) N9 G1 G40 X0 (Move away to point 8) N10 G00 Z0.1 (Rapid out of slot) N11 M99 (End of subprogram) Once again, notice that all coordinates in this subprogram are taken from the center of the slot in X and the center of the lower radius in Y. This is made possible by the G52 commands in the main program. G53 - rapid movement relative to the machine s zero return position Almost all of the movements you make in a CNC program are specified from the program zero point (if you work in the absolute mode). And in general, the program zero point makes an excellent origin for the various cutting movements needed in your program. However, there are certain times when causing motion relative to the machine s zero return position can be very helpful. Note that with most machine s, and especially with machining centers, the zero return position is very close the plus over-travel limits. If this is the case, any coordinate specified in the G53 command will be negative. Also, G53 automatically invokes the rapid mode, meaning you can only make positioning movements (not cutting movements) with G53. The command N050 G53 X-2.0 Y-3.0 will rapid the machine to a location two inches to the negative side of the zero return position in X and three inches negative of the zero return position in Y. Another way to send the machine to the zero return position You were probably taught to use a G28 command to send the machine to its zero return position. The command N080 G91 G28 X0 Y0 Z0 3

4 for, example, will send the machine straight to its zero return position. In our basic courses we recommend using G28 for two reasons. First, it is universal (older controls do not have G53). Second, the axis origin lights will come on at the completion of a G28. However, many programmers don t like the G28 command. It s hard to understand (due to the intermediate movement made), it requires you to switch to the incremental mode (if you use our recommended method), and you must remember to re-select the absolute mode at the beginning of the next tool. As long as you have a newer control (that has G53) and don t care about the axis origin lights coming on, the command N080 G53 X0 Y0 Z0 will send the machine to its zero return position. Simply replace all of your G28 commands with G53. Use with manual pallet changers Some CNC users place after-market manual pallet changers on their vertical machining centers. These devices require that (at least) the axis be sent to a precise location in order for the pallet change to occur. If you try to program this position using the program zero point as the origin, the positioning command will change for every program (and even for every setup if you don t make qualified setups. On the other hand, the position of the pallet change in X is constant as it relates to the zero return position. Once you determine its position (by measuring it once), you can use the same G53 command to send the X axis to the appropriate position. If for example, you measure this position as being negative from the zero return position, use the command N050 G53 X any time you wish to send the machine to its pallet change position. Common turret index position on turning centers With geometry offsets, you can have the turning center index the turret just about anywhere. The control will constantly keep track of where the program zero point is, even if you have a different tool change position for every tool. This makes for very easy, safe, and efficient tool changing. Even with all the benefits of geometry offsets, some turning programmers like to index the at a common position - and this position will be different for every tool relative to the program zero point. However, it will be a consistent distance from the machine s zero return position. Say for example, a setup person moves the turret to a safe index position that is 5 inches to the left (negative) of the Z axis zero return position and determines (by indexing the turret) that this is a good safe index position. In this case, the command N060 G53 X0 Z-5.0 will can be included before every turret index and the turret will be positioned to the common turret index position. 4

5 G54-G59 - fixture offsets Most basic course stress the use of fixture offsets for assigning but one program zero point per program. They also assume that you will be using the machine s zero return position as the point of reference for program zero entries. To actually determine program zero assignment values, many teach beginners to actually measure them during the setup, right on the CNC machining center. While these basics are important, and they truly help a beginner understand how fixture offsets work, they aren t very efficient, especially if you make a lot of repeated qualified setups. (By qualified setups, we mean setups that can be repeated in exactly the same manner time after time. If a setup is truly qualified, the program zero assignment values will be the same every time the setup is made.) The two ways to use fixture offsets As stated, basic CNC courses commonly teach but one of the ways to use fixture offsets (using the machine s zero return position as the point of reference for fixture offset entry). But there is another way to assign fixture offset values that may be more appropriate to your needs. Regardless of which method you use to assign fixture offsets, programming remains exactly the same, meaning you can easily switch methods without having to change your programs. Using the machine s zero return position as the point of reference Again, this is the method commonly taught in basic CNC courses. With this method, the setup person enters the distances from the machine s zero return position (spindle center in X and Y and spindle nose in Z) to each program zero point in the appropriate fixture offset registers. Since the zero return position is commonly located close to the machine s plus over-travel limits, these values will commonly be negative. If multiple program zero points must be assigned (two or more workpieces in the setup, for example), these techniques are simply repeated for each program zero point. Shifting the point of reference for program zero assignment value entries Using the machine s zero return position as the point of reference is somewhat cumbersome. The actual values will be rather random, and might be very difficult to predict. Believe it or not, with Fanuc and Fanuc-compatible controls, you can actually shift the point of reference for program zero assignment values to a location that makes more sense. Program zero assignment values will make sense and it may be quite easy to determine them without measuring. You ve probably noticed fixture offset number zero on the fixture offset page of the display screen. If you ve been working from the machine s zero return position, the values in fixture offset number zero s registers are zero. This fixture offset actually lets you shift the point of reference. If the registers in fixture offset number zero are all zero, the amount of shift from the zero return position is nothing (you re working with the zero return position as the point of reference). Shifting the point of reference for sub-plates Look at the next drawing. A special sub-plate is mounted on the table. Note that every four inches, a precise reamed hole is machined. Every other four inches, there s a 1 / 2-13 tapped hole. So every two inches there is either a location hole (reamed) or a mounting hole (tapped). Ideally, this sub-plate will be located on the machine table with 5

6 keys, so it can be removed and replaced without a change in position. (Note that several tooling suppliers offer this kind of sub-plate, or you could make your own.) Gray reamed holes Black ½-13 tapped holes Machine at zero return position 2 centers Sub-plate Drawing shows a sub-plate mounted on the table of a vertical machining center. Notice that each row of holes is marked (stamped or etched) with a number and each column is marked with a letter. This makes it very easy to designate specific holes. For the previous drawing, hole C3 is a reamed hole, three holes from the left and three holes up. With this location device, you can easily shift the point of reference for program zero assignment value entries. Say you wish to work from the lower left hole in X and Y and the top surface of the workpiece in Z. With the sub-plate mounted on the table, measure the distance in X and Y from the zero return position (center of spindle) to the lower left hole. For Z, measure the distance from the spindle nose (at zero return) to the top of the sub-plate. For most machines, these will be very large negative values. When you enter these values into fixture offset number zero, you effectively shift the point of reference for program zero assignment values to the lower left hole in X and Y, and the top of the sup-plate in Z. From this point on, all program zero assignment values will be taken from the lower left hole in XY and the top of the sub-plate in Z. Look at the next drawing that shows some simple component location tooling. (Again, many tooling suppliers offer this kind of component tooling. If you do make your own sub-plate, you may want to match the design of the most popular tooling suppliers so you can still use standard, and readily available, component tooling.) 6

7 Drawing shows component tooling used with sub-plate With this corner locator, the edge being located will be precisely in line with the left-most location hole in the sub-plate, making it very easy to calculate the distance from the lower left hole to the location surfaces on the corner locator. Look at the next drawing. Hole C A B C D E F G H I J K L M N O P Q Drawing shows simple setup made with corner locator. Sub-plate 7

8 The setup person is told to place the corner locator in holes E5 & G5 (for location) and hole F4 (for clamping). In this case, the X location surface (program zero in X) is precisely eight inches from the left hole in X. The Y location surface is precisely eight inches from the lower hole in Y. With fixture offset number one appropriately set (shifting the point of reference to the lower left hole), the program zero assignment values in X and Y for this setup will be 8.0 in X, and 8.0 inches in Y. Though the drawing doesn t show it, if program zero in Z is the top of the workpiece, the program zero assignment value in Z will be the distance from the top of the sub-plate to the location surface in Z (1.0 in this case) plus the thickness of the workpiece. If the workpiece is 0.75 thick, the Z axis fixture offset value will be Notice how simple the sub-plate and component tooling make it to calculate program zero assignment values (of course, they also make it quite easy to physically make setups). And, knowing which location holes will be used, the programmer can include a G10 in the program to keep the setup person from even having to enter it. For the previous example, the command N005 G90 G10 L2 P1 X8.0 Y8.0 Z1.75 will enter the values into fixture offset number one (note that the L word value for fixture offset setting does vary from one control model to another). In this way, the setup person does not have to do anything when it comes to program zero assignment during setup. We have effectively eliminated program zero assignment tasks from setup. Shifting the point of reference for horizontal machining centers Most horizontal machining centers incorporate a rotary device (indexer or rotary axis) inside the table. This allows the machine to expose several surfaces of the workpiece (or several workpieces) to the spindle for machining during the cycle. Many horizontal machining centers also incorporate two-pallet pallet changing devices to allow the operator to be loading one pallet while the other is being machined. When designing fixtures, most tool designers will dimension the locators from the center of rotation. In this case, the programmer will know the position of all location surfaces (which correspond to program zero positions for X and Z) from the center of rotation as the program is written. If you shift the point of reference from the machine s zero return position to the center of rotation in X and Z, you can easily specify program zero assignment values right in your program with G10 commands. The next illustration shows a horizontal machining center from above (X and Z). 8

9 Machine at zero return Z shift X shift Center of rotation Drawing of a horizontal machining center from above, showing X and Z shift values For the Y axis, it may be best to shift the point of reference to the machine table top. The next drawing shows the value as viewed from the front of a horizontal machining center. 9

10 Y shift Drawing shows Y shift amount. Whether you are using a sub-plate on a vertical machining center or a horizontal machining center, and as long as you make qualified setups, these techniques virtually eliminate all program zero assignment-related tasks from setups. This can mean a great reduction in setup time! Dealing with alignment problems after a crash If you are making qualified setups and including G10 commands in your program to enter program zero assignment values, the machine must, of course, stay in alignment. This is true regardless of whether you are using the machine s zero return position for the point of reference for fixture offset entries or you have shifted the point of reference. If you have a crash or other mishap, part of fixing the machine should include recalibrating each axis to make sure the zero return position is in the same location it was before the crash. However, not all companies do so. If, of course, the zero return position has shifted, the G10 commands in all programs will no longer be correct. This is yet another application for the common fixture offset (fixture offset number zero). It can be used to specify the amount of misalignment so all G10 commands will be correct. It may be easiest to visualize how the common offset can be used for this purpose by considering the sub-plate example shown earlier. After a crash, and if the machine is not perfectly re-aligned, simply re-measure and re-enter the distances from the zero return position to the lower-left hole in XY and the top of the sub-plate in Z. Since the sub-plate hasn t changed, all G10s used prior to the mishap will now be correct. 10

11 The same is true for shifting the point of reference to the center of rotation on horizontal machining centers. Simply re-measure and re-enter the shift amounts, and your G10 commands will be back on track. If you are using the zero return position as the point of reference, the common offset will include but a small value in each axis (just the amount of misalignment). To determine these small values, simply re-measure the program zero assignment values for the current setup. Compare your measurement to the values in the G10 command. The difference in each axis will be the amount of the each register in the common fixture offset. Using the common offset to handle machine differences As you know, one way to use tool length compensation is to store the length of each tool in the tool length compensation offsets. One benefit of this method is that tool length compensation values can be measured off line, while the machine is running production for another job. The time the machine is down between production runs can be reduced if tools are assembled and measured while the machine is still in production. If no regard is given to the common offset, the device used to hold each tool as it is being measured must match the spindle of the machine that will be using the tool. And if you have two or more identical machines that have slightly different spindle bores, your tool setter is probably compensating for this machine difference as tools are measured. A given tool will have a different tool length compensation value for each machine. Say you wish to set up a series of commonly used tools that will be readily available for whichever machine needs them first. In this case, the tool length compensation value must work for all machines. One way to accomplish this is to store the deviation from one machine to the next in the Z axis register of the common offset. 48 fixture offset option Fanuc controls come with but six fixture offsets which for most applications is more than enough. However, there are times when more are required. Consider, for example, a horizontal machining center that has a pallet changer. You may, for example, want to assign one program zero point for each side of each pallet. In this case, you will need eight fixture offsets (four sides times two pallets). Fanuc offers an option when it comes to fixture offsets. When this option is purchased, you ll have forty-eight fixture offsets available, but programming is slightly different. With this option the G code G54.1 is used to invoke fixture offsets. An H word in the G54.1 command specifies which fixture offset is being invoked. The command N005 G54.1 H25 for example, invokes fixture offset number twenty-five. What can a spindle probe do for you? We have been stressing the importance of minimizing, if not eliminating, the tasks related to program zero assignment that must be done during setup. This in turn, reduces setup time. However, if you cannot justify making qualified setups, the task of measuring and entering fixture offset values must be done during setup right on the machine, while the machine is down between production runs. In this case, you must do everything possible to make these tasks as easy (and quick) as possible. 11

12 This is a great application for a spindle probe. The spindle probe will automatically measure and enter fixture offset values in less than one minute. If you rarely make qualified setups and must measure program zero assignment values on the machine on a regular basis, a spindle probe makes the best alternative for assisting with program zero assignment. Running out of fixture offsets? As stated, Fanuc controls come standard with six fixture offsets. If you need more on a regular basis, you should purchase the 48 fixture offset option. However, if you seldom need more than six fixture offsets, there is a way of handling this problem. In fact, you ll only need one fixture offset! We point out right away, however, that this technique eliminates one of the main advantages of fixture offsets. When you use fixture offsets, of course, you separate the task of program zero assignment from the program itself. With this technique, program zero assignment values must be entered into programs. With this technique, you ll be using a series of sub-programs (one subprogram for each program zero assignment). It s helpful to make the subprogram numbers in a special series (say the 6000 series). When you invoke subprogram number O6001, for example, you ll be changing to coordinate system number one. When you invoke O6002, you be changing to coordinate system number two, and so on. In each subprogram there will be a G10 command that enters the appropriate program zero assignment values into fixture offset number one. Right in the subprogram, we ll invoke fixture offset number one (with G54) to ensure that the coordinate system is selected. Here are two sample subprograms. You can, of course, have as many subprograms as your control allows (most controls allow at least 100 programs to be stored). O6001 (Coordinate system number one) G90 G10 L2 P1 X Y Z G54 M99 O6002 (Coordinate system number two) G90 G10 L2 P1 X Y Z G54 M99 To invoke the appropriate coordinate system, simply include an M98 command in the main program. For example, the command N010 M98 P6001 invokes coordinate system number one. 12