Block Delete techniques (also called optional block skip)

Block Delete techniques (also called optional block skip) Many basic courses do at least acquaint novice programmers with the block delete function As you probably know, when the control sees a slash code in a program, it looks at a special on/off switch on the control panel (the block delete switch) If the switch is on, the control will ignore the balance of the command that is programmed after the slash code If the switch is off, the control will execute the balance of the command This function allows the programmer to give the setup person or operator a choice between one of two possibilities Even if this function is introduced in a basic CNC course, most instructors will not describe the various applications for block delete Here, we ll show two advanced capabilities of block delete, and we ll show a variety of applications Using block delete mid-command Though it is not commonly known, most controls will allow you to place the slash code right in the middle of a CNC command - and only what is to the right of the slash code will be affected by the block delete switch Say you are trying to use one program to machine a workpiece that can be made of two materials One material is steel and the other is cast iron For the steel workpiece, you need coolant to flow, but for the cast iron workpiece, you elect not to run coolant You could, of course, start the coolant on a line by itself and place a slash code in the program at the beginning of the command like this: N045 T01 M06 (Tool change) N050 G54 G90 S300 M03 T02 (Select coordinate system, absolute mode, start spindle, get next tool ready) N055 G00 X40 Y30 (Move to first XY position) N060 G43 H01 Z01 (Instate tool length compensation) /N065 M08 (If block delete switch is off, start spindle) With this method, however, the programmer is isolating the coolant on command from other commands in the program While this may not be too bad, if the machine has a fully enclosed guarding system, it may be wiser (and faster) to turn the coolant on in line N060, as the tool approaches in the Z axis Consider the next series of commands N045 T02 M06 (Tool change) N050 G54 G90 S300 M03 T03 (Select coordinate system, absolute mode, start spindle, get next tool ready) N055 G00 X40 Y30 (Move to first XY position) N060 G43 H02 Z01 / M08 (Instate tool length compensation If block delete switch is off, start spindle) 1

Notice that the slash code is now placed in the middle of command line N060 And only what is to the right of the slash code (the M08 in our case) will be affected by the block delete switch While almost all current model CNC controls allow this programming technique, be sure to test it to ensure that it works as we say Conflicting words in a command While the technique we ll show next is a bit obscure, it is sometimes helpful to know what will happen if conflicting words are specified in a command The command N060 G00 X20 X40 for example, probably represents a mistake It is likely that the programmer meant to specify Y40 instead of X40 in the command But believe it or not, most controls will not actually generate an alarm if this command is given (test if you are in doubt) Instead, the control will simply execute the latter of the two conflicting words In this example, the control will move the tool to X40 and ignore the X20 word in the program Understanding how conflicting words are handled by your control can be helpful with block delete In a previous example, we describe how to use the slash code to control whether coolant comes on for the purpose of running the same workpiece in two different materials with but one program If, of course, you want to run the same workpiece in two materials with the same program, it is likely that the feed and speed for each tool must also change from one material to another Intentionally including conflicting words in a command (feed and speed words) in conjunction with block delete will allow you to write one program that will work for both materials Consider these commands N045 T02 M06 (Tool change) N050 G54 G90 M03 T03 S300 / S400 (Select coordinate system, absolute mode, get next tool ready, start spindle at 300 rpm if block delete is turned on, 400 rpm if turned off) N055 G00 X40 Y30 (Move to first XY position) N060 G43 H02 Z01 / M08 (Instate tool length compensation If block delete switch is off, start spindle) N065 G81 R01 Z-05 F35 / F45 (Drill hole, feed at 35 ipm if block delete is turned on or 45 ipm if block delete is turned off) If you are running the cast iron workpiece, turn the block delete switch on In line N050, the S400 word will be skipped and the spindle will start at 300 rpm In line N060, the M08 word will be skipped, keeping coolant off In line N065, the F45 word will be skipped, meaning the feedrate used will be 35 ipm 2

If you are running the steel workpiece, turn the block delete switch off In line N050, both S300 and S400 will be read by the control But since it is the latter of the two conflicting words, only the S400 word will be executed (the speed fro the steel workpiece) The same technique is used for feedrate in line N065 In line N060, the M08 word will be executed and coolant will come on Similar techniques will, of course, be required for all tools in the program While this is a unique technique that helps you use the same program for two workpieces in a family, it just scratches the surface of what can be done for part families with a function called parametric programming If you have part family applications, you ll really want to learn more about parametric programming (we offer another online course for parametric programming) Trial machining You know from basic CNC courses that trial machining is done to help ensure that a tool will not machine too much material the first time it cuts It is commonly required when running the first workpiece in the production run for dimensions that have critical tolerances It may also be required during the production run when dull tools are replaced The most common method of trial machining involves several steps First, the setup person makes an adjustment of some kind (possibly to the tool itself or more likely to a tool offset) that will ensure that excess stock is left on the workpiece Second, the tool is allowed to machine in its normal fashion Third, the machine is stopped and the setup person measures the surface machined by the tool (if the entire tool is run, most setup people and operators use the optional stop function to actually stop the machine) Fourth, the setup person makes an adjustment (again, to the tool or an offset) based on the measurement just taken And fifth, the setup person reruns the tool While this method of trial machining is almost failsafe (the surface will come out some where within its tolerance band), there are three potential problems First, this method assumes that the workholding setup, workpiece, and cutting tool are pretty rigid If there is any flexing, and since the material machined on the second try will be much less than it will be in production, it is possible that the surface will not be within its tolerance band if the tolerance is very small Second, this method requires that the tool be run in its entirety twice (once when trial machining and once after the measurement) If the tool s machining operation is very long, production time will suffer And third, trial machining requires much manual intervention The setup person or operator will be highly involved with the entire process, requiring a high level of skill on their part One of the programmer s primary goals should always be to make their CNC programs as easy to run as possible And when it comes to trial machining, a programmer can almost always make it easier to trial machine with block delete In all cases, if trial machining is required, the setup person or operator will turn off the block delete switch to have the control execute the trial machining commands If they don t wish to trial machine (the 3

machine is in normal production), they turn on the block delete switch and the trial machining commands will be ignored Here we show a few example machining operations that can benefit from the programming of trial machining the most However, what we show is not in any way the limit of what you can accomplish If you see setup people and operators struggling to perform trial machining (or taking much time to do so), it s likely that you can do something to help them with block delete Trial boring on a machining center Most boring bars used on machining centers require manual adjustment And they vary when it comes to how easily and precisely they can be adjusted Ideally, it would be great if the boring bar could be perfectly adjusted prior to being placed in the machine (and some companies go to great lengths to do so) But for most companies, it is not feasible to purchase the expensive presetting devices it takes to perfectly set boring bars And the tighter the diameter tolerance you expect the boring bar to hold, the harder it is to adjust it up front (tool pressure will, of course, also affect the diameter the boring bar will cut) Most machining center using companies are resigned to intentionally setting the boring bar undersize by a small amount and then having the setup person trial machining for the first workpiece The setup person will allow the boring bar to enter the hole by a small amount (some people let the boring bar machine to its final depth if tolerance is especially small) While the bar is still in the hole, they ll manually stop the cycle, manually retract the boring bar, manually move the machine into a position that allows a measurement of the hole, manually measure the hole, manually adjust the boring bar, and finally, they will manually rerun the tool Depending upon the quality of the boring bar, the skill of the setup person, and the tolerance to be held, the setup person may have to repeat the process several times to get the boring bar to cut on size Note that if trial machining is needed during setup, it will also be needed whenever the tool is replaced during the production run, meaning operators will also be required to trial machine when dull tools are replaced Techniques Saving time with and block effort: delete Trial boring on a machining center: Commonly taught in basic CNC Trial boring courses: subprogram Use block delete to help with trial machining Slash code in program O1000 (/) Works If off, with trial block machining delete N1 will G91 switch take G86 R0 place Z-03 If on, If on, block trial skippedif machining N2 off, will G80 be M09 block skipped executed N3 G00 Z30 N4 X40 Y40 Not With always a little taught ingenuity, basic N5 you courses: M00 can streamline Mid almost command any trial machining N6 G00 X-40 Another operation! Y40 M03 optional stop N7 Z-30 M08 Conflicting words with Multiple N8 G90 block deletes Trial machining N9 M99 With 2) Allow unexpected boring stock bar to partially machine hole 4

Our first example of trial machining with block delete will dramatically reduce the manual intervention The setup person must still manually measure the hole and manually adjust the boring bar, but just about everything else will be done by the program Additionally, we re using a special subprogram written in the incremental mode that will work for any hole diameter in any location, meaning this subprogram can be kept in the controls memory permanently and will be available whenever trial boring is required This, of course, minimizes programming effort and verification effort once the subprogram is proven Main program: O0001 (Program number) (Machining prior to boring bar) N255 T04 M06 (23750 boring bar) N260 G54 G90 S450 M03 T05 (Select coordinate system, absolute mode, start spindle, get next tool ready) N265 G00 X40 Y40 (Move to first hole location) N270 G43 H04 Z01 M08 (Instate tool length compensation, move to Z position, start coolant) N275 F25 (Ensure that trial boring program uses desired feedrate) /N280 M98 P1000 (Jump to trial boring sub program) /N285 M98 P1000 (Give second trial boring try) /N290 M98 P1000 (Give third trial boring try) /N295 M98 P1000 (Give fourth trial boring try) N300 G86 R01 Z-10 F25 (Bore hole to depth) Now here s the subprogram that will work for any hole diameter in any location O1000 (Subprogram number) N1 G91 G86 R0 Z-03 (Bore just deep enough to take measurement) N2 G80 M09 (Cancel cycle, turn off coolant) 5

N3 G00 Z30 (Retract in Z to clear all obstructions) N4 X40 Y40 (Move far enough to allow measurement) N5 M00 (Program stop to allow measurement) N6 G00 X-40 Y40 M03 (Move back to hole, restart spindle) N7 Z-30 M08 (Move back to just above hole, restart coolant) N8 G90 (Reselect absolute mode) N9 M99 (End of subprogram) In the main program, notice that line N275 selects the feedrate needed for boring Since we want the subprogram to work for any hole diameter, the subprogram does not actually include a cutting feedrate in the boring cycle Also, the entire subprogram is written incrementally to allow it to function properly regardless of the hole s location We are assuming that, in line N3 of the subprogram, the tool will be high enough to clear all obstructions for all times you use the routine You may have to retract to a higher position We re also assuming that the XY movement in line N4 is a convenient location for measurement You can, of course, modify these values to work for your setup people And finally, we re assuming you run coolant for the boring bar It s being restarted in line N7 of the sub program In the main program, we re giving the setup person four tries to get the boring bar sized (you can easily add M98 commands for more tries) Again, they ll turn off the block delete switch and run the program When the control gets to line N280, it will execute subprogram O1000 and trial bore 0200 deep (just deep enough to take a measurement) The tool will then retract and move to a convenient measuring position and stop (M00 in line N5) At this point the setup person simply measures the hole and adjusts the boring bar (since it is not to size, they leave off the block delete switch) When they press cycle start, the tool will be brought back to the hole location The subprogram ends by reselecting the absolute mode When back in the main program the control will also execute line N290 and the machine will trial bore a second time, since the setup person has left off the block delete switch At the M00 in the subprogram, the setup person will measure again If the hole is to size, they will turn on the block delete switch and the balance of the trial machining passes will be skipped If not, they ll adjust the boring bar again, leaving off the block delete switch This process is repeated until the hole is sized, at which time, they will turn on the block delete switch Of course, once the hole is sized and block delete is turned on, the machine will continue to ignore the trial machining commands during the production run But if the boring bar dulls and the insert/cartridge is replaced, trial machining can be easily done again (this technique will help during both the setup and the production run) Trial turning on a turning center In the previous machining center trial boring example, the reason for programming the trial boring operation is to provide assistance to the setup person, minimizing the amount of manual intervention required This, in turn, reduces the time it takes to trial machine and minimizes the potential for mistakes Note also, that since the boring bar is only allowed to enter the hole a small amount (just enough to get a measurement), machining time for trial machining is also reduced While the time saved may be minimal 6

depending upon the hole s depth, there are times when the primary goal of providing trial machining help is primarily to reduce machining time during setup Techniques Saving time with and block effort: delete Trial rough turning (minimize trial machining time): Commonly taught in basic O0003 Use block delete to help with CNC trial courses: machining N005 T0101 M41 Slash code in program N010 (/) G96 S400 M03 N015 G00 X60 Z1 Works If off, with trial block machining delete will /N020 switch take X55 place /N025 G01 Z-3 F0020 If on, If on, block trial skippedif machining off, will be block skipped /N030 X60 executed /N035 G00 X80 Z3 /N040 M00 (DIAMETER 550 IN) Not With always a little taught ingenuity, basic you courses: can streamline /N045 T0101 M03 Mid almost command any trial machining /N050 G00 Another operation! X6 Z1 optional stop Conflicting words with Multiple N060 block deletes Trial machining Rough turning time: 18 minutes With unexpected stock N055 G71 P060 Q160 D2500 Consider a large workpiece to be machined on a turning center The rough turning (or boring) operation may take over fifteen minutes If traditional trial machining techniques are used to ensure that the roughing tool leaves the proper amount of finishing stock, the entire rough turning operation will have to be repeated (after the initial offset adjustment and measurement) Fifteen minutes of program verification time will be wasted By using our recommended method, the setup person will be able to set the rough turning tool s offset before the first workpiece is completely rough turned Since the amount of time needed to actually set the offset will remain essentially the same with our given method, the amount of program verification time that will be saved will be the time it takes to perform the roughing operation (almost fifteen minutes in our case) A programmer can program a short rough turning pass under the influence of block delete To ensure that tool pressure will remain consistent, this roughing pass must be at the same depth of cut as is used for the normal rough turning operation Note that this rough turning pass only needs to go far enough into the workpiece to allow a measurement to be taken Our example program provides 03 in for this purpose Here is a portion of the program showing the trial rough turning operation O0003 (Program number) N005 T0101 M41(Select rough turning tool, offset, and spindle range) N010 G96 S400 M03 (Start spindle CW at 400 SFM) N015 G00 X60 Z1 (Rapid up to the workpiece) /N020 X55 (Begin trial machining operation) /N025 G01 Z-3 F0020 (Trial machine) /N030 X60 (Feed up face) /N035 G00 X80 Z3 (Rapid to convenient measuring position) /N040 M00 (Stop for measurement, DIAMETER SHOULD BE 550 IN) /N045 T0101 M03 (Reinstate offset, restart spindle) /N050 G00 X6 Z1 (Rapid back to starting point) 7

N055 G71 P060 Q160 D2500 U0040 W0005 F0020 (Rough turn) N060 In line N020, we begin the trial turning operation In lines N025, N030, and N035, the tool makes the trial turning pass and rapids to a convenient measuring position At this position the setup person can easily measure the workpiece In line N040, the machine stops due to the M00 We strongly recommend that you include a message in the program at this point telling the setup person what the diameter (and if necessary, the Z face position) the workpiece should currently be The setup person measures the workpiece and adjusts the offset accordingly Line N045 reinstates the offset, based on the setup person s offset change In line N050, the tool rapids back to its starting point From line N055, the program continues in its normal manner After setting the offset, the operator turns on the block delete switch so the roughing tool won t trial machine on the next workpiece The block delete switch can be turned off whenever the setup person wishes to use the trial machining sequence, meaning the CNC operator will also have this sequence available should it be needed when changing (or indexing) the rough turning tool s insert during the production run Any lengthy roughing operation can be handled in much the same manner For rough boring on a turning center, the only difference will be that the programmer may have to move the boring bar further away from the workpiece to allow a measurement to be taken Eliminating tool pressure when finishing on turning centers The turning center programmer can also facilitate the setup person s ability to size for the finishing tool before the finishing operation even takes place By incorporating this technique, any tool pressure related problems caused by using more conventional trial machining processes can be eliminated While we use the same large turned workpiece for this example program, keep in mind that this technique can also be used when the rough turning operation is quite short If the goal now is to perfectly size the finishing tool, and may have nothing to do with reducing roughing time However, you must still use a trial roughing operation to confirm that the roughing tool leaves the proper amount of stock for finishing With this technique, we simply include another set of commands under the influence of block delete for finish turning right after the trial rough turning commands (in the rough turning tool portion of the program) These commands will first re-machine with the rough turning tool to ensure that the rough turning tool has left the correct amount of finishing stock Then the program will index the turret to the finishing tool and continue machining on our practice surface It is important to program the same depth-of-cut during the trial finishing operation as will be used for the actual finishing operation It is also important that the setup person initially adjusts the roughing tool s offset in a way that allows excess stock prior to trial machining This ensures that the roughing tool won t machine too much stock, not leaving the proper amount for finishing After 8

cutting, the machine will move to the convenient measuring position and stop again At this point the setup person measures the surface/s and adjusts offset/s accordingly After this technique is used, the setup person can rest assured that the finishing tool will machine perfectly to size, even on the very first workpiece Here is the example program O0003 (Program number) N005 T0101 M41(Select rough turning tool, offset, and spindle range) N010 G96 S400 M03 (Start spindle CW at 400 SFM) N015 G00 X60 Z1 (Rapid up to the workpiece) /N020 X55 (Begin trial machining operation) /N025 G01 Z-3 F0020 (Trial machine) /N030 X60 (Feed up face) /N035 G00 X80 Z3 (Rapid to convenient measuring position) /N040 M00 (Stop for measurement, DIAMETER SHOULD BE 550 IN) /N045 T0101 M03 (Reinstate offset, restart spindle) /N055 G00 X55 Z1 (Rapid back to rough turned diameter) /N060 G01 Z-3 F0020 (Ensure correct diameter) /N065 X60 (Feed up face) /N070 G00 X80 Z60 (Rapid to tool change position) /N075 T0202 M42 (Index to finish turning tool, select range) /N080 G96 S700 M03 (Select finish turning speed) /N085 G00 X542 Z1 (Rapid to trial diameter, 0040 cut depth) /N090 G01 Z-03 F0008 (Trial machine) /N095 X60 (Feed up face) /N100 G00 X8 Z5 (Rapid to tool change position) /N105 M00 (DIAMETER SHOULD BE 54200) /N110 T0101 M41 (Re-select rough turning tool) /N115 G96 S400 M03 (Re-select roughing speed) /N120 G00 X6 Z1 (Rapid back to starting point) N125 G71 P130 Q230 D2500 U0040 W0005 F0020 (Rough turn) N130 With this technique, the setup person must confirm that the rough turning tool will not cut undersize with its first pass, meaning an offset adjustment must be made to offset number one to force some excess stock to be left Additionally, the proper speed and feedrate for actual finish turning must be used when trial finish turning In line N105 the setup person measures the diameter and adjusts the finishing offset accordingly The program then indexes back to the rough turning tool and begins the actual rough turning operation After the trial machining operation has been completed and the setup person is sure that roughing and finishing will be done correctly, the block delete switch can be turned on to skip the trial machining operations in production Whenever changing inserts (at least for the finisher), these same techniques can be used again 9

You may be questioning the wisdom of including the actual trial machining commands in the program that machines the workpiece Admittedly, if these techniques are used often, the CNC programmer may be cluttering the program with a great number of commands that are seldom used Keep in mind that the trial machining commands can be easily stored in a separate subprogram or parametric program, and invoked with one simple command from the main program Here is an example that shows how a subprogram can be used for trial machining However, it is not nearly a flexible as the subprogram shown for trial boring on a machining center This subprogram will only work for one specific workpiece If you have need of this technique for a variety of workpieces, a parametric program can be created that would work for all workpieces Parametric programming is presented in a future module of this course O0003 (Main program) N005 T0101 M41(Select rough turning tool, offset, and spindle range) N010 G96 S400 M03 (Start spindle CW at 400 SFM) N015 G00 X60 Z1 (Rapid up to the workpiece) /N020 M98 P1000 (Call trial machining subprogram) N025 G71 P130 Q230 D2500 U0040 W0005 F0020 (Rough turn) N030 O1000 (Sub program) N001 X55 (Begin trial machining operation) N002 G01 Z-3 F0020 (Trial machine) N003 X60 (Feed up face) N004 G00 X80 Z3 (Rapid to convenient measuring position) N005 M00 (Stop for measurement, DIAMETER SHOULD BE 550 IN) N006 T0101 M03 (Reinstate offset, restart spindle) N007 G00 X55 Z1 (Rapid back to rough turned diameter) N008 G01 Z-3 F0020 (Ensure correct diameter) N009 X60 (Feed up face) N010 G00 X80 Z60 (Rapid to tool change position) N075 T0202 M42 (Index to finish turning tool, select range) N011 G96 S700 M03 (Select finish turning speed) N012 G00 X542 Z1 (Rapid to trial diameter, 0040 cut depth) N013 G01 Z-03 F0008 (Trial machine) N014 X60 (Feed up face) N015 G00 X8 Z5 (Rapid to tool change position) N016 M00 (DIAMETER SHOULD BE 54200) N017 T0101 M41 (Re-select rough turning tool) N018 G96 S400 M03 (Re-select roughing speed) N019 G00 X6 Z1 (Rapid back to starting point) N020 M99 (End of subprogram) 10

Trial threading on a turning center Many threads take very little time to machine A very fine pitch, single start, short thread on a small diameter, for example, may not require more than about ten or twenty seconds to machine In this case, use conventional trial machining techniques to size the thread However, the longer the thread takes to machine, the more time it will take to use conventional trial machining techniques Coarser threads, for example, require more passes (and more time) to machine Multiple start threads require even more passes, meaning even more time A lengthy four-start ACME thread on a large diameter, for instance, may take twenty to thirty minutes to machine If conventional trial machining techniques are used, the entire thread must be run twice (once to trial machine, once to bring on size), meaning from twenty to thirty minutes of wasted program verification time The same block delete techniques just shown can be used to minimize trial machining time for lengthy threading operations However, keep in mind that some CNC controls make it very easy to specify how threads are to be machined within their standard canned cycles If this is the case, it may be quite easy for the setup person to simply modify the (one) threading command to minimize the number of threading passes needed to finish the thread after offset adjustment Once the first thread has been machined to size, of course, the threading command must be changed back to its original state Unfortunately, modifying the CNC program to minimize the number of threading passes requires the setup person to thoroughly understand the threading command Mistake can result in disaster for the threading tool For this reason, and since not all companies use standard threading canned cycles, if you wish to minimize program verification time, it may be necessary to size threads using block delete techniques Conclusion to trial machining with block delete Note that we have but scratched the surface when it comes to the kind of assistance you can provide setup people and operators when it comes to trial machining Again, as you watch setup people running the first workpiece (or as you do so yourself), constantly ask yourself what can be done to make the process easier Since trial machining is done on such a regular basis (and remember what we said in module one about the ease of justifying improvements to repeated tasks), programmers should be anxious to provide as much help as possible Other examples of using block delete to help with trial machining that you may find useful include lengthy trial milling on machining centers, trial thread milling, trial grooving on turning centers, and just about any other kind of machining operation Again, what kinds of machining operations are your setup people having problems getting to size? Using block delete with unexpected rough stock There are many times when the CNC machining operation is not the first machining operation to be performed on a workpiece If previous machining operations must be performed prior to the CNC operation, it is important that those operation/s be performed consistently For example, if a part is to be run on a CNC turning center is made from round bar stock, the stock is usually be cut to length on a cut off saw of some kind In this case, it is important that the cut off saw cut each piece of raw material to the same length While the CNC turning center can deal with a small amount of length variance from one part to the next, if the overall length is much greater than planned, it can present 11

catastrophic problems for the CNC turning center operation This statement is true of all kinds of CNC machines The condition of the rough stock to be machined by the CNC machine must be consistent from one workpiece to the next for the CNC machine to perform properly Castings and forgings are notorious for this kind of raw material variation that wreaks havoc with CNC operations Techniques with block delete Block delete can be used to help Commonly rough taught machine basic varying CNC stock courses: Slash code in program (/) 01 Works with block delete switch Stock as it If on, block skippedif off, block executed should be: Not always taught in basic courses: 05 Mid command Another optional stop Conflicting Worst case words with Multiple block deletes Trial stock machining condition: With unexpected stock The illustration shows an example of when the rough stock coming to a turning center is not consistent As you can see, the programmer expects there to be only 0100 in of facing stock on the end of the workpiece But the cut off saw operator made a mistake Instead of all pieces of rough stock allowing 0100 in roughing stock, the stock lengths vary In the worst condition, 0500 in stock is left on the face of the part to be machined If machining a workpiece with 0100 in stock, the program will perform just fine But if the operator tried to use the same program for the parts with excess stock, the facing tool will would try to remove much more stock than it was intended to machine, resulting in damage to the workpiece, the tool, and possibly even the machine In extreme cases such as this one, the workpiece would probably be thrown from the chuck, possibly causing injury to the operator This is but one example of when the consistency of the rough stock to be machined on a CNC machine is less than desirable The programmer must constantly be on the lookout for this kind of rough stock problem Even when no previous machining operations are performed prior to the CNC operation, the rough stock could still vary enough to cause problems and must be cautiously checked Castings or all kinds, for example, are notorious for their inconsistency This variation from one workpiece to the next can raise havoc during machining Block delete can be used to allow for the undesirable variance related to the amount of rough stock The program can be written to behave in one of two ways, depending on the rough stock situation A series of extra roughing passes can be included under the influence of a slash codes to machine the undesirable extra stock Then the normal roughing pass can be programmed without the slash code/s If the workpiece has excess 12

stock, the operator will turn off the block delete switch to run the part The control will execute the extra roughing passes to machine the rough stock If the part has the proper amount of rough stock (no excess stock), the part will be run with the block delete switch on In this case, the control will skip the extra passes and only make the roughing pass/es as originally planned WARNING! This brings up a safety related point Whenever you are considering the use of block delete for any application, always ask yourself What s the worst thing that can happen if the operator has the block delete switch in the wrong position? In this case, if the switch is in the on position when a workpiece with excess stock is machined, the tool would attempt to remove all stock in one pass, causing damage to the tool, workpiece, and possibly the machine Knowing this, the operator must exercise extra caution while running the job Due to this potentially dangerous situation, some shop people will elect not to use block delete for this purpose They will treat the job as two different jobs, separating those parts that have excess stock from those that do not Then they will create two programs, one for workpieces with excess stock and one for workpieces without, and run the parts separately One program machines the workpieces with the excess stock, making the needed extra passes The other program machines the workpieces that have the correct amount of rough stock in the normal manner This keeps them from having to risk the possibility of having the operator position the block delete switch incorrectly Here is an example program that incorporates the block delete feature for the purpose of removing unexpected rough stock Though this is a turning center example, the same principles will apply to machining center applications If the workpiece is as it should be, only 0100 in stock will be on the face to be removed In its worst condition, the workpiece has 05 in of stock on the face, meaning five passes are necessary It is this worst condition for which you must plan That is, as you decide how many rough passes to make, you must know the worst possible condition of the rough stock Remember, you can only give the operator two choices Either the rough stock is to the proper length and the block delete switch will be turned on, or the part has excess stock and the block delete switch will be turned off If turned off, the machine must make enough rough passes to allow for the worst case condition (Note that with parametric programming techniques, a program can be developed that will let the operator specify how much stock is on the workpiece and an appropriate number of passes will be made) The program will show only the rough facing tool as it rough faces the part to within 0005 in of the finished surface Here s the program: O0004 (Program number) N005 G96 S600 M03 (Start spindle cw at 600 sfm) N010 G00 T0101 M41 (Index turret, select low spindle range) N015 G00 X42 Z4 M08 (Rapid to position, turn coolant on) /N020 G01 X-06 F012 (Face passed center, 1st pass) /N025 G00 Z5 (Rapid away in Z) /N030 X42 (Rapid back up in X) 13

/N035 Z3 (Rapid to new Z position) /N040 G01 X-06 (Face passed center, 2nd pass) /N045 G00 Z4 (Rapid away in Z) /N050 X42 (Rapid back up in X) /N055 Z2 (Rapid to new X position) /N060 G01 X-06 (Face passed center (3rd pass) /N065 G00 Z3 (Rapid away in Z) /N070 X42 (Rapid back up in X) /N075 Z1 (Rapid to new Z position) /N080 G01 X-06 (Face passed center, 4th pass) /N085 X42 N090 Z005 (Rapid to final Z position) N095 G01 X-06 F012 (Face to within 005 of finished surface) N100 G00 Z1 (Rapid away in Z) N105 X42 (Rapid up in X) N110 G00 X60 Z50 (Go back to tool change position) Notice in line N015, the tool is sent to the first roughing Z position (0400 in away from the finished face) If the block delete switch is off, line N020 will be executed, starting the series of rough facing passes from this point If the block delete switch is on, the next command to be executed will be line N090, which sends the tool over to the 0005 position in Z In this case, only one rough facing pass is made Another optional stop You know that the optional stop word (M01) works in conjunction with a switch on the control panel (the optional stop switch) If the switch is on when the control executes an M01, the machine will stop (just like a program stop M00 in this case) If the optional stop switch is off, the control will continue with the program, ignoring the M01 Most programmers get in the habit of including an M01 at the end of each tool to allow the setup person or operator to check and see what the tool has done In this case, if the optional stop switch is on, the machine will stop at the end of every tool This makes program verification and rerunning tools easier However, if an M01 is programmed at the end of every tool, the optional stop function cannot be used for any other purpose If, for example, the programmer wants to provide the operator with an easy way of stopping the machine for the purpose of taking a measurement on every fifth workpiece (right in the middle of the cycle), optional stop cannot be used, since it s already being used at the end of every tool Block delete can actually be used to provide a second optional stop Consider this command /N050 M00 14

Now, the block delete switch will control whether or not the machine will stop at line N050, though it will work in just the opposite fashion compared to M01 (when the block delete switch is off, the machine will stop) This will allow the operator to make the machine stop after every five workpieces (they ll turn the block delete switch off) and the programmer can still program an optional stop (M01) at the end of every tool Special note about multiple applications While we ve shown some excellent applications for block delete, with most controls you ll be limited to but one application per program since there is only one block delete switch Note that some controls do offer an optional feature allowing up to nine block delete functions You ll actually have nine block delete switches labeled one through nine In the program the slash code will include a number to specify which block delete switch controls the function For example, with the command /2 M00 block delete switch number two will control whether or not the machine will stop or not at this point in the program While having the multiple block delete function is nice, if you find yourself wishing you had more than one block delete switch on a regular basis, it should be taken as a signal that you have some excellent applications for parametric programming The multiple block delete function barely scratches the surface of what can be done with parametric programming when it comes to making decisions as to how the machine will behave during the execution of a CNC program Again, we offer another on-line course for parametric programming 15