Automatic Generation of Nc-code for Hole Cutting with In-process Metrology

A new method to mill flat-bottomed circular holes with more accurate diameters has been added to the data preparation software for the Vertical Workstation of the Automated Manufacturing Research Facility at the National Institute of Standards and Technology. This software already had the capability to generate NC-programs automatically for cutting two-and-a-half dimensional parts. Additional design functions, a new process planning function and a new NC-code generating function have been added to the software to implement the new method. The new cutting algorithm uses a touch probe to measure the diameter of the semi-finished hole during the cutting process. The radius used to finish cut the hole is then changed from its nominal value by an amount equal to the difference between the nominal and measured values of the radius of the semi-finished hole. The new hole milling process corrects errors caused either by tool deflection or by using a tool whose actual radius differs from its nominal radius. With the new process, errors in the diameter of a hole cut with an end mill have been reduced from roughly five mils (plus tool diameter error) to about one mil (regardless of tool diameter error), as compared with a process which does not measure during cutting. The new process is integrated into the Vertical Workstation system by allowing the user to specify the diameter tolerance of the hole during the design process. The automatic process planner then selects the new process for high tolerance holes. BACKGROUND Nature of the Problem For small batch production, the inability to produce a high-tolerance hole without special tooling is an important practical problem. A hole with very high diameter tolerance must be finished with a tool (end mill, ream, or boring tool) whose cutting diameter is the same as the diameter of the hole. However, for a certain tolerance range, roughly 0.5 to 5 mils (1 mil = 0.001 inch), exact sized tools may not be required if good enough machining techniques are available. It is desirable to avoid having to use exact sized tools in order to save time and money. If a hole is an odd size, a tool of exact size may not be on hand, and will have to be obtained by purchase or manufacture. There are 1000 exact sizes less than an inch if 1 mil accuracy is required. Having a tool inventory of that order of magnitude is very costly. Even if a tool is available, it may not be in the tool carousel of the machining center when it is time to cut the hole. The setup time to put it in and take it out is costly. If a small set of standard sized end mills can be used to make most milled holes, a good deal of money might be saved, particularly where only one or a few parts of a given design are to be made. Description of the Vertical Workstation The Automated Manufacturing Research Facility (AMRF) at the National Institute for Standards and Technology (NIST) formerly the National Bureau of Standards serves as a testbed for developing techniques and standards for automated manufacturing [13]. Small batch production is emphasized in the AMRF. The AMRF includes three machining workstations. One of these is the Vertical Workstation (VWS), which contains a Monarch VMC-75 Vertical Machining Center with a GE2000 controller. The VMC-75 is a 3-axis machine. It is equipped with a Renishaw touch probe. Software has been developed for the Vertical Workstation, called the VWS2 system, which supports the automatic machining of a family of two-and-a-half dimensional parts [3]. The VWS was used as the testbed for the research reported here, and the techniques developed were embodied in software which was integrated in the VWS2 system. This work was done in conjunction with the Quality in Automation project being carried out in the AMRF [14]. Three types of documents: designs, process plans, and equipment control programs, are of key importance in the VWS2 system. A design may be created as a feature-based design using the VWS2 design editor [4]. For a more limited range of parts, a boundary representation design in PDES/STEP format may be parsed automatically into a feature-based design [7]. A process plan for machining is prepared automatically from the feature-based design [8], and then an NC-program for the GE2000 controller is prepared automatically from the design and the process plan [6]. Producing Holes In the VWS2 design protocol, a hole is defined as a depression with a circular outline that has a flat or conical bottom, or goes all the way through the part. The parametric representation of a hole includes x and y coordinates of the center of the hole, plus diameter, depth, and bottom-type. In enhancements not previously documented, centertolerance and diameter-tolerance have been added as parameters. Holes may be made by many methods, of course. Process plan work elements and automatic NC-code generators are in place in the VWS2 system for drilling, milling, and counterboring. In this paper we deal only with milling. Before the research reported here was done, a holemilling algorithm was already in place in the VWS2 system. We will call it the "old algorithm", and we will call the one reported here the "new algorithm". Both algorithms use an end mill. The old algorithm starts the hole by one of three methods: cutting a slot down the middle, spiralling in, or plunge cutting, depending on the amount of room available for the tool in the hole. Next, material is removed by peripheral milling, if necessary, to make a hole whose depth is that of the designed hole but whose radius is 10 mils less. Finally, the old algorithm performs a finish cut on the sides of the hole to remove the last 10 mils and achieve the designed diameter. In calculating the tool path, the system uses the value of the diameter of the end mill stored in a database of current tooling. Automatic Generation of NC-Programs Computer systems for the semi-automatic (user-interactive) generation of NC-programs are widely used. At least 40 such systems are commercially available [9], and more exist in university, government, and private research laboratories. A few systems do not require user interaction once a design and process plan have been prepared [1]. Fully automatic generation of NC-programs which use probing for in-process metrology is extremely rare. OBJECTIVES The objectives of the work reported here were: 1. to develop an algorithm for making holes with a tighter diameter tolerance than was being achieved with the old algorithm, without requiring the use of a tool with the same diameter as the hole. 2. to integrate the algorithm into an automatic machining system, so that its use would be triggered by the tolerance requirements given in a design, with process planning and NC-programming handled automatically. SOURCES OF ERROR There are many ways for error to creep into machining a hole with an end mill. We will omit detailed discussion of novice-level errors such as using a 4-flute end mill in aluminum (or other tool-workpiece mismatches), plunge cutting with a non-center-cutting end mill, or using a dull tool. Several less elementary errors are discussed below. Methods of correction are discussed for each error type. Geometric analyses of control algorithm error and small tool path radius error are given in the appendix to this paper. Tool Diameter An end mill may have a spinning volume which is a nicely shaped cylinder, but have a cutting diameter (the diameter of the cylinder) which is different from the tool’s nominal diameter or last measured diameter. Tool wear might account for this. A tool may have been resharpened (a common practice) and be slightly undersized as a result. It is much more common for an end mill to be undersized than oversized, since wear and sharpening remove material. Some machining centers, including the Monarch VMC-75, have cutter radius compensation. To use it, the tool must be measured, a parameter set in the machine tool controller, and an instruction issued in the NC-program. In the VWS2 system, another correction method is to use the exact cutter diameter in the current tooling database. This also requires measuring the tool. Tool Deflection Even if the spindle of the machine tool is following a correctly defined tool path exactly, the tip of the tool may not follow the correct path because cutting forces bend the tool to the side. In milling a hole, the last cut is normally a circular cut around the surface of the hole. For this type of cut, tool deflection will make a hole that is too small, and the sides of the hole may taper, so that the diameter is smaller at the bottom than at the top. Tool deflection may be corrected by taking very light cuts to minimize the bending force on the tool, by reducing the feed rate (also to reduce bending force), or by enlarging the tool path slightly to compensate for bending. Chatter The tool may vibrate rapidly while cutting, making a loud noise called chatter. When a tool chatters it bangs against the workpiece. This results in a rough surface and large errors in surface location. It is hard to predict when chatter will occur, but it may usually be eliminated by reducing the feed rate, taking lighter cuts, or changing the spindle speed. The workpiece may also vibrate, typically if the ratio of the thickness of the part to the distance from where it is being machined to the nearest fixturing point is small. This problem is harder to deal with, and may require refixturing or changing the tool path. Chip Interference If chips of material cut by an end mill are not removed promptly from the vicinity of the end mill, the end mill may grab them and drag them against the workpiece. This results in a rough surface. The cure for this is to clear chips away as soon as they are formed. If this is not feasible, periodic chip clearing (especially just before finish cuts) will help. Position Measurement Error NC machining centers perform machining by repeating a simple sequence of operations at a fixed rate of repetition [10]. Typically, a cycle lasts a few milliseconds. The operations are: measure the spindle position, calculate where it should be at the end of the next cycle, and issue the control signals required to move the spindle in a straight line to get it there at the right time. If the position measurement system of the machine tool is not accurate, holes made by the machine tool will not be correctly made. Repeatable position errors may be compensated by mapping them and putting corrections into NC-programs. Control Algorithm Error In making a circular arc, the machine tool control system makes a series of straight line segments to approximate the arc. If the control algorithm makes segments whose endpoints are on the arc, the average diameter of the hole will be slightly too small. If the control algorithm makes segments that are tangent to the arc and whose endpoints lie outside the arc, the average diameter will be slightly too large. Other algorithms are likely to make segments that lie between those two extremes. As shown in the appendix, the maximum difference is approximately d2 / (2 r) , where d is the length of a segment, and r is the radius of the hole. Although it is not clear whether control algorithm error will ever be significant, the worst it can get is when the radius of the arc is very small, since the difference is inversely proportional to the radius. A circular tool path 10 mils in radius made at a feed rate of 15 inches per minute will take about 0.25 second to make. If one segment is made each millisecond, so that there are 250 segments, the difference described above is about 0.003 mil. If it takes ten milliseconds to make a segment, so that there are 25 segments, the difference is about 0.3 mils. Control algorithm error might be reduced by reducing the feed rate of the tool, so that d is small. Since feed rate is normally adjusted to make chips of a certain size, reducing it may cause problems in machining some (but not many) materials. Handling the adjustment automatically would require special test and correction routines in the Process Planning module. Control Execution Error There is always some error in the execution of an NC-code instruction to move the tool. The largest error usually results from overshoot or undershoot in the direction of tool movement. The error becomes noticeable when there is a large change in the direction of successive tool movements. The simplest method of reducing control execution error is to reduce the feed rate, so that smaller movements are required in each clock cycle. Overshoot and undershoot may also be reduced by using a special machine code provided for that purpose [12] or by avoiding large changes in the direction of tool movement. Large changes in direction are avoided by having each programmed linear or circular move start out in the same direction in which the last one finished (i.e. successive motions have a common tangent). Dwell Error If an end mill is allowed to dwell in one place against the wall of a hole it is cutting while it is spinning, for even a fraction of a second, it will make a slight depression in the wall [10]. This seems to be caused in part by the tool unbending after being subjected to cutting forces, but a depression will be made after even the lightest of cuts. Dwelling often occurs during the execution of an NC-program, even if it is not part of the program. If the spindle is to be retracted after a cut, for example, there is usually a brief dwell between the end of the cut and the retraction. Dwell error is eliminated by not dwelling during a finish cut. This requires knowing what sequences of NC-program steps may result in unintentional dwell and avoiding them. Small-Circle Tool Path Error If the radius of a circular tool path is very small, another interesting type of error crops up. The shape of the cross section of the swept volume of the tool becomes significantly different from a circle. This is because the tool revolves only few times as it travels around the tool path. The appendix gives a geometric analysis of this error. As with control algorithm error, decreasing the feed rate should solve the problem, but may not be the most desirable solution. NEW PROCEDURE General Approach The general approach taken in the new algorithm is: 1. Rough-cut the hole using the old techniques. 2. Make a circular semi-finish cut using a control radius 10 mils smaller than the radius that should nominally be required to cut the final hole. 3. Measure the diameter of the semi-finished hole and calculate the error in the radius of the semi-finished hole. 4. Make a circular final finish cut whose control radius has been adjusted by the error factor found in step 3. If the measured radius of the semi-finished hole was smaller than its nominal value, make the control radius of the finish cut larger by this amount. If the error was in the other direction, make the adjustment in the other direction. The assumption behind this approach is that if the semi-finished hole and the finished hole (which are nominally identical holes except that the radius of the semi-finished hole is 10 mils smaller) are cut in the same manner, the errors made in cutting them will be essentially the same. Because of the several undesirable side effects of tool paths with small radii (which were observed in early experiments), the tool used in the new algorithm is chosen to be significantly smaller than the hole being cut. To avoid dwell marks on the side of the hole, the tool is not allowed to dwell against the side of the hole. To avoid radial overshoot on starting the hole, the tool is brought into its cutting path on an arc tangential to the path. Tool Path The tool path for the initial rough cut is not critical. The rough-cut hole is nominally made 20 mils smaller in radius than the final hole. The semi-finish cut removes a layer 10 mils thick around the inside of the hole, and then makes another trip around (nominally cutting nothing) to clean it up well under minimal cutting forces. A picture of the path is shown in Figure 1. Next, machining comes to a halt, and a comment in the program appears on the console of the controller, reading: Changing tool to probe for measuring hole. Please clean chips and coolant out of the hole. Then press cycle start. The console operator follows these instructions. When the machine is restarted, the tool is changed to the probe, and the hole-measuring subroutine provided with the Monarch is run to find the diameter of the semi-finished hole. The subroutine automatically sets a parameter in the GE2000 controller to the value of the diameter. The new algorithm sets another parameter to the nominal value of the radius of the final cut plus the difference between the nominal and measured values of the semi-finished hole. This last parameter is used for the radius of the tool path of the finish cut. Finally, the tool is changed again, so that the end mill is in the spindle, and the finish cut is made as shown in Figure 1. Figure 1. Tool Path for Finish Cut start end go around the circle twice Probing Measurement Method The probing subroutine provided with the Monarch [11] is used in the new algorithm. The main NC-program provides the subroutine with approximate-x and approximate-y for the center of the hole and the approximate diameter of the hole. The tool path used by the subroutine is shown in Figure 2, and is as follows. Numbered items below correspond to numbers on the figure. 1. Probe the surface of the part outside the hole to find the zlocation of the hole. 2. Insert the probe in the hole at the approximate center. 3. Move the probe parallel to the x-axis back and forth to opposite sides of the hole, touching at A and B. Let good-x be the average of the x-values at A and B. Good-x will be very close to the x-value of the center of the hole, if the hole is round. 4. Move the probe to (good-x, approximate-y). 5. Move the probe back and forth parallel to the y-axis to opposite sides of the hole, touching at C and D. Let best-y be the average of the y-values at C and D. Store best-y as the y-value of the center of the hole. Store the length of CD as a value for the diameter of the hole. 6. Move the probe to (good-x, best-y). 7. Move the probe parallel to the x-axis back and forth to opposite sides of the hole, touching at E and F. Let best-x (not shown on the figure) be the average of the x-values at E and F. Store best-x as the x-value of the center of the hole. Store the length of EF as another value for the diameter of the hole. The average of the two values of the diameter is stored in a parameter of the controller as the diameter of the hole. The depth of insertion into the hole must be set in the NC-program. The new algorithm uses a quarter inch or 0.02 inches less than the depth of the hole, whichever is less. Error Sources Compensated The new algorithm compensates principally for tool deflection error and tool size error. It is designed to avoid other errors to the extent that can be done in NC-code. To the extent other errors cause a hole to be the wrong size without throwing it out of round, the algorithm will compensate for them (but it is hard to show there are any such errors). EXPERIMENTAL RESULTS To test the new procedure, three pairs of holes were made using tools which were already in the tool carousel of the machining center. Both holes in a pair were the same nominal size and were made with the same tool. Three different end mills were used. The largest hole was made with an 0.625 inch diameter end mill that had been used a long time, and, judging from the results of cutting with it, may have been resharpened at some time, so that its actual diameter is significantly smaller than the diameter listed in the current tooling database. The data are shown in Table 1. These data were taken on July 28, 1988 by the author with a hand-held dial caliper, accurate to about 1 mil. Separate measurements were taken by Mr. David Caparelli of the NIST Precision Metrology Group using a Mitotoyo coordinate Figure 2. Tool Path for Probing