Inch / Metric Selection G20 & G20

Transcription

1 Inch / Metric Selection G20 & G20 Most current CNC machines allow input in either the inch mode or the metric mode. Generally speaking, once either input is selected, it is maintained throughout the program. That is, seldom will you be required to use both modes in one program. In fact, most companies will use one of these measurement modes for all programs written. If the company comes across a part that happens to have been in the other measurement system, they will simply convert the print s dimensions and tolerances to the measurement system with which they are most familiar and run the workpiece in that mode. Here are the conversion formulae. Inches = millimeters divided by 25.4 Millimeters = inches times 25.4 For example, say you have a dimension of 16 mm on the print, but you are going to write your program in the inch mode. To convert to inch, simply divide 16 by 25.4 to come up with the inch equivalent ( in). Though the metric mode is becoming more popular, the inch mode is still, by far, the more common mode used in the United States. Since our country has been working in the inch mode for two centuries, it has been difficult for us to make the switch to metric. Keep in mind that switching to the metric mode involves more than simply writing programs in metric. There are other considerations when making a switch from one mode to the other that will cost your company money. First, all measuring devices like micrometers, calipers, height gages, and dial indicators must be replaced when switching to the metric mode since most of these tools are designed to show measured dimensions in only one of the two input modes. Second, most manual machines like engine lathes, turret lathes, and milling machines have their hand-wheel scale increments in inch. While most machine tool builders offer replacement scales capable of converting the machine from inch to metric, many companies find this expense to be prohibitive. Third, all shop people must be re-educated to work in metric. For these reasons, we have been extremely reluctant to make this change. On the other hand, more and more European and Pacific rim companies (among others) are opening manufacturing facilities in the United States. These companies work exclusively in the metric mode. As time goes on, more and more American companies will be forced to conform. It is likely that you will have to work in the metric mode at some point in your CNC career. How to select the inch or metric mode Most CNC controls allow the measurement system (inch or metric) to be selected in two ways. First, the operator is usually allowed to select the inch or metric mode manually, through some kind of switch. The switch could be a physical toggle switch on the control panel, or more likely, a switch displayed and set through the display screen. Second, the programmer can usually select inch or metric by a preparatory function (G code). On most controls, a G20 selects the inch mode and a G21 selects the metric mode. By this method, the input mode can be selected from within a program, or by manual data input mode (MDI). 1

2 The machine can usually be manipulated so the desired mode is initialized at power up. If your company works exclusively in inch, the machine can be made to power up in the inch mode. If your company works exclusively in metric, the machine can be made to power up in the metric mode. This will keep the programmer from having to specify a G20 or G21 in the program if the desired mode is used. The control will automatically assume the correct mode when the machine is turned on. You can easily tell which input mode is currently selected by looking at the coordinate positions on the display screen. In the inch mode, almost all CNC machines will display coordinate positions to four places of accuracy (down to.0001 in). In the metric mode, the control will display coordinate positions to three places of accuracy (.001 mm). For example, if the position display page of the control screen shows these values: X Y Z you would know the machine was currently set to the inch mode because four places follow the decimal point. On the other hand, if the position display page of the control screen shows these values: X Y Z you would know the machine was currently in the metric mode because three places follow the decimal point. Do note that some high precision machines (especially turning centers) allow you to program out to five places in the inch mode (five places displayed to the right of the decimal point). These controls allow you to program out to four places in the metric mode. There are companies that utilize their CNC machines in both input modes. It may be possible that about half of this company s workpiece prints are dimensioned in inch and the other half in metric. For this company, it may be best to work in the most convenient input mode. Keep in mind that this means a duplication of measuring devices. If your company is one of the few that runs programs in both modes, we recommend that you include the appropriate G20 (inch mode) or G21(metric mode) at the beginning of all programs to avoid accidentally being in the wrong input mode. If no programmed command tells the control which input mode to use, of course the control will assume the input mode from the most recent program (if one exists) or the mode initialized at power up. If the control assumes the wrong mode, the results can be disastrous. If the program is written in the metric mode, but the machine is set to the inch mode, all coordinate position end points will be greatly enlarged. A value that was supposed to be taken as 5.0 mm ( in) will actually be taken as 5.0 inches. On the other hand, if the program is written in the inch mode but when run, the machine is set to the metric mode, coordinate position end points will be dramatically reduced. A value of 5.0 inches will be taken as 5.0 mm ( in). In either case, the problems 2

3 created by being in the wrong input mode sets up potentially dangerous situations. The inclusion of the proper input mode G code at the beginning of all programs will let you avoid this possibility for disaster. Other considerations when switching to metric mode As you have seen, switching from one input mode to the other is not as simple as throwing a switch. Though the machine will assume the correct mode in this manner, your company s measuring devices, manual machine tools, and even the attitude of its employees also affects the change from inch to metric and vice versa. There are yet other considerations. When working in one input mode or the other, you must work exclusively in the selected mode. For example, the measurement of the program zero point must be made in the selected mode. If working in metric, the distance from program zero to the machine s starting point must be entered in the metric mode. Tool offsets must also be entered in the selected mode. Say you intend to work in metric. For machining centers, tool length offsets and cutter radius offsets must be entered in metric. For turning centers, offsets to control machining size as well as tool nose radius offsets must be entered in metric. Note that most types of cutting tools must also be supplied in the selected input mode. For example, if the design engineer dimensions a hole to be 10 mm in diameter, a 10 mm drill must be used. Though there are times when you will find tooling in inch equivalents that happen to match the metric tool requirements, these occurrences are purely coincidental. The advantage of the metric mode If your company is currently working exclusively in the inch mode, you may see little reason to change to metric. Surely, nothing presented to this point will have changed your mind. It would take quite an investment of time and money to switch to metric. You will probably want to continue machining workpieces in the Inch mode and convert those few metric prints you come across to inch and run the parts in the inch mode. However, there is one advantage to of working in the metric mode that is not very obvious. It has to do with the least input increment of the machine tool in the selected input mode. The least input increment is the smallest departure movement possible on the CNC machine. For most CNC machines, the least input increment in the inch mode is in. In the metric mode, the least input increment is mm. When converted to the inch mode, mm is equal to in (.001 divided by 25.4), so mm is less than half of in. This means the machine has a much finer resolution or movement grid when you are working in the metric mode. You can target the end point of each movement command to a more precise position when working in the metric input system. The next illustration shows the grid for the inch mode as it compares to the grid for the metric mode ( grid as compared to mm grid). This is a graphic illustration of how much more precise you can be with the specification of end points in the metric mode. As you can see, the machine s resolution (set of possible end points for each command) is much finer in the metric mode. 3

4 in mm Resolution of inch mode Resolution of metric mode Drawing shows the difference between the inch and metric modes We are not saying that the machine is more accurate in the metric mode. The CNC machine will perform to its quoted specifications in either mode. In the metric mode, you can simply target your end points to with a finer precision. We compare this to indexing devices. A five degree indexer has 72 positions. A one degree indexer has 360 positions. This doesn t make the one degree indexer more accurate than the five degree indexer; it simply has more programmable positions. When you think about it, working in the inch mode when the metric mode is available is kind of like have a one degree indexer but never programming it to less than two degree increments. In a similar way, the metric mode will allow the possible end points along a linear axis to be more than doubled. Actually there will be 2.54 times the number of end points for any linear axis in the metric mode than in the inch mode. For a linear axis that is ten inches long, there are 100,000 possible programmable positions in the inch mode. For the same linear axes, there are 254,000 possible programmable positions in the metric mode. Note that the metric advantage does not apply to a rotary axis. Since all true rotary axes are commanded in angular increments, there is no difference in the number of possible end points from the inch mode to the metric mode. A position of 45 degrees is commanded the same in both modes. 4

5 Selecting the mean value for a dimension There are times when having the ability to select finer increments of motion will make the difference between success and failure with a program. For example, when you are trying to hold extremely critical tolerances on a workpiece, it may be helpful (if not mandatory) to target each motion as precisely as possible. When programming any workpiece, most programmers will select the mean dimension of the tolerance for use as the programmed coordinate. This allows any cutting condition problems to slightly affect machining yet be within the given tolerance. For example, for the dimension in plus minus the programmer would use as the programmed coordinate, since it represents the mean value of the specified tolerance ( plus minus half the overall tolerance ). However, there are times when the programmer cannot specify the precise value of the mean tolerance in the inch mode due to the resolution grid limitations discussed earlier. For example, for the dimension plus minus nothing the mean value of this dimension is in. Since the least input increment in the inch mode is in, the desired end point of the motion command cannot be commanded in the Inch mode. In this mode, either the dimension would have to be rounded up to in or rounded down to in. Either way, the programmed value would be from the needed program value. However, if the dimension is converted to metric the mean dimension end point programmed can be much more precise. The value in metric is mm ( times 25.4), which can be rounded to mm. This coordinate is within mm (or in) of being precisely the desired mean value coordinate. When compared to the best possible inch mode value (within in), you can see how much better the metric mode lets you target end points. Offset considerations Another time when using the metric mode will help with critical tolerances is when offsetting. When an operator is trying to adjust the size of the workpiece with tool offsets, the machine s least input increment will again be the limitation. If in the Inch mode, the operator will be limited to making offset adjustments in increments of in. In the metric mode, the operator is allowed to make much finer adjustments in mm ( in) increments. This can sometimes mean the difference between being able to hold size or not being able to hold size for critical tolerances. Though the points made here are true for all kinds of CNC machines, the most common time when you will have this kind of tolerance problem is on turning centers when trying to hold close diameter tolerances. For example, say this Inch input mode diameter and tolerance must be held on a turning center in plus.0001 in minus nothing 5

6 In this case, the operator would have little or no chance to adjust the offset perfectly if working in the Inch mode. Also note that the programmer would have to program the value as either or In either case, the programmed coordinate would be on a tolerance limit. The best the operator could hope for is to be very lucky when adjusting the offset. By luck alone will the dimension come out to the mean dimension of the tolerance. However, when converted to the metric mode, inch is mm. The tolerance band of inch is mm when converted. This means the mean dimension of the tolerance would be mm ( times 25.4 rounded down to the next mm). If run in the metric mode, the operator will have a much better chance of adjusting the offset to conform to this dimension. Admittedly, the tolerances we have been discussing are minute indeed, and in reality, most companies will not have to work to such close tolerances. But when faced with the task of handling such close tolerances, it is good to know the implications of working in the metric mode. In these cases, you can convert the dimensions on the drawing to metric and machine the workpiece in the metric mode. How the control generates axis departure (inch versus metric mode) Depending on the control manufacturer, the resolution of the CNC control will sometimes determine how smoothly motion will occur. By resolution, we mean the size of the smallest single axis departure when a movement of more than one axis is commanded. When linear and circular commands (G01, G02, and G03), are given, the actual motion occurs is along a series of tiny single axis motions. For most applications, these motions will be so tiny that the end result will appear to be a perfectly straight line or a perfectly round circle. But in reality, these motions are actually generated by a series of tiny single axis motions as shown in the next drawing. The size of each step is the determined by the control s resolution. The better the resolution, the smaller the step, hence the smoother the motion will be. Drawing shows the steps generated by any motion command 6

7 For some current CNC controls, the control s resolution is exactly the same (and the best it can be) no matter which input mode is selected (inch or metric). However, the resolution of some (especially older CNC controls) is dramatically affected by which input mode is selected. In fact, many times the least input increment is the actual step value determined by the control s resolution. If this is the case, the control s motion capabilities will be directly affected by whether the control is in the inch or the metric mode. That is, in the inch mode the resolution (step size) will be in. In the metric mode, the resolution will be mm (or in). This means the control can make smoother movements in the metric mode than in the inch mode. For most applications, there would be no indication of this limitation in the Inch mode. The tiny in steps would seldom be detectable. Also, newer controls have the same resolution in either mode, meaning you would never be faced with any problems stemming from resolution differences based on the input mode.but there is one kind of problem you may come across at some point in your career we wish to warn you about. The next drawing shows a workpiece to be machined on a turning center that requires a very tiny taper on the face of the part (though not to scale). If this part is to be programmed in inch mode, and if the resolution of the control is set by the least input increment ( in in this case), the desired motion could not be generated. Drawing shows workpiece with small taper on face The next drawing shows what will happen. Notice that since only taper is generated on the face in the Z axis, the control would simply divide this motion by the least input increment ( divided by is 1) and break the command down into two steps. No true taper could be generated. 7

8 Drawing shows what will happen on face of workpiece in inch mode In the metric mode, since the least departure increment is less than half of that in the inch mode, the motion would be much better, though still not perfect. The next drawing shows the same motion if made in the metric mode. Drawing shows what will happen on face in metric mode 8

9 Keep in mind that some (especially newer) CNC controls do not base the control s resolution on the least input increment. With this kind of control, the resolution (step size) is even smaller than the least input increment, even in the metric mode. This means the above mentioned problem may never occur. 9