Techniques With Motion Types

Techniques With Motion Types In this lesson we ll look at some motion techniques that are not commonly discussed in basic CNC courses Note that we re still talking about the basic motion types rapid (G00), straight line (G01), and circular (G02-G03) motion In lesson seven, we ll discuss more advanced motion types G00 & G01 rapid and straight line motion for positioning (not cutting) The basic motion types (including G00 and G01) are usually well covered in most basic CNC courses - at least as far as basic usage goes Here we intend to expose some important things not commonly addressed in basic courses As you know, G00 will cause the machine to move as fast as it possibly can in all commanded axes (if more than one axis is commanded, it s likely that the motion will not be in a straight line) The primary function of rapid motion is, of course, to help minimize air cutting time during the program s execution Most instructors teach students that if they re not cutting anything in the motion they should be causing the tool to move at rapid While this is a great rule of thumb, there are times when using G01 for positioning (non-cutting) movements is advantageous - in fact - there is even one time when using G01 is actually faster! What is your maximum feedrate? Most CNC users can quickly state the rapid rates for the various machines they own It s well publicized, and machine tool builders are quite proud of how fast they can make their machines move For smaller machines, it s not uncommon to have rapid rates well in excess of 1,000 inches per minute However, most CNC users cannot as readily state their machines maximum feedrate (the fastest the machine can move in G01 mode) Indeed, you may have to scour your machine tool builder s programming manual to find this specification (if you find it at all) A control parameter setting, the maximum feedrate is commonly set to about half the machine s rapid rate (but confirm this to be sure) If, for instance, the machine has a rapid rate of 1,000 ipm, the maximum feedrate will probably be in the neighborhood of 500 ipm Since it is rare that a cutting operation would require this fast a motion rate (but we ll show one such machining operation a little later), most CNC users are not concerned with maximum feedrate Which is faster, G00 or G01? At first glance, it may seem like a no-brainer that the rapid mode is much faster than the straight line motion mode While rapid motion is commonly your best choice for fast axis motion, there is one time when G01 may be (much) faster than G00 - when making very small movements since the machine will not actually reach its rapid rate How G01 compares to G00 for small movements is also determined by how certain control parameters that are related to axis acceleration and deceleration are set Though a service engineer may take exception with the details this explanation, this presentation should be easy enough for everyone to understand With most controls, acceleration and deceleration parameters for the rapid (G00) mode are set up with exponential methods The left-most drawing shows a graph of exponential accel/decel 1

5 time constants 7 time constants Motion rate 1,200 ipm Motion rate Motion rate 2 time constants 300 ipm Time Time Time Notice that most controls will take about five time constants to complete the acceleration Though variable, let s say the time constant is currently set to 100 milliseconds The same will be true for deceleration This means that the machine will be accelerating for about the first 1/2 second of motion At the end of the command, the machine will be decelerating for the last 1/2 second of the command (again, this is assuming five time constants are required and each time constant is 100 ms) For lengthy motions, there will be ample time to accelerate up to the machine s rapid rate and decelerate down when the machine comes close to the end of the motion The longer the motion, the more distance the machine will truly move at the full rapid rate As you probably know, with short rapid motions the machine will never reach its full rapid rate (in our example, any rapid motion requiring less than one second) It will be right in the middle of the acceleration when it determines that it must start decelerating if it is to stop in the commanded position The middle illustration shows this kind of motion in graph form Notice that the machine never came close to reaching its full rapid rate when it begins slowing down Though this graph is not perfect (there will be lots of variables based upon machine size and how the related parameters will be set), notice that the time required for this motion is about 700 ms (seven time constants) And again, the machine never comes close to its true rapid rate Though it may come as a bit of a surprise, we can commonly speed up the machine s motions during short positioning movements by programming in G01 mode instead of G00 One of the main reasons for this is that acceleration/deceleration is handled differently when G01 is used First of all, it s done in a linear fashion (not exponential) And second, usually only 2-3 time constants (200-300 ms) are required to complete acceleration/deceleration The right-most drawing illustrates this Even though slower feedrates are programmed (we ll be using 300 ipm), the machine will actually respond faster in G01 mode than it will in G00 mode A test It s hard to predict just what kind of improvement you can expect by programming short movements with fast feed G01 commands as opposed to rapid motion commands Factors include the machine size, the rapid rate, the feedrate used, and how acceleration/deceleration parameters are set However, there is a test you can perform to determine just how much you can save with a specific machine This first test program simulates center drilling 50 closely spaced holes Note that the depth of each hole is only 02 (03 actual movement) and the holes are spaced 05 apart) While it s rather long, you can of course use a text editor and copy-and-paste to avoid 2

typing the whole program out longhand Note also that this program is using G00, even though motions are quite small Ensuring that rapid override and feedrate override are set to 100%, run and time this program It requires about 25 inches of X axis travel, so move the machine at least 25 inches to the negative side of the plus over-travel limit prior to running O0001 (Test program with G00) G91 F80 (Repeated 40 more holes) M30 Here is the second test program that uses G01 for positioning movements Run and time this program and compare it to the first one O0002 (Test program using G01 for all motions) G91 F80 3

Z03 F300 (Repeated 40 more holes) M30 What were your results? You may be quite surprised at the results of this test We d be interested in hearing them so we can relate more specific information based upon machine sizes If you will let us know the differences in cycle time (you can email us at lynch@cnccicom) We make one last point about G00 versus G01 for short positioning movements According to GE Fanuc Automation, you ll put much less stress and strain on the machine if you use G01 for short positioning movements With G00, the axis drive system is constantly chasing its tail trying to determine the proper rate of motion (again, look at the middle drawing) No sooner than a drive motor begins to speed up, it has to begin slowing down This causes spikes in power consumption and places undue wear and tear on the servo drive system 4

How do canned cycles work? Of course that there are several canned cycles to help perform hole machining operations When it comes to the points just made about short positioning movements, you must understand that most controls use G00 (internal to the canned cycle) on a regular basis The G81 drilling cycle, for example, uses G00 to retract from the hole and to move to hole locations You might add this short program to your series of tests O0001 (Program number) G91 G81 R0 L25 (Drill 25 holes along a line) M30 This time we re drilling with G81 (feed to depth retract at rapid) Since the command is given in incremental mode, we can include the and the L25 to make the machine drill 25 equally spaced holes When you time the execution of this program, you will likely find that it takes the same amount of time as the G00 test (again, G81 uses G00 internal to the cycle) You might even find it takes a little longer since, depending upon control model, canned cycles can take longer to execute than straight forward motion commands Using G01 for fast feed approach As stated, machines are coming with faster and faster rapid rates It is not unusual for a new machine to have a rapid rate in excess of 1,500 inches per minute But with many machines, the rapid override function has not been improved sufficiently to provide adequate control of the machine while it s making rapid movements - especially when approaching to within a small distance away from the workpiece (most programmers rapid to within no more than 01 inch from the surface to be machined) Note that it is the machine tool builder that provides the rapid override function (not only Fanuc) and machine tool builders vary with regard to how much control they provide The best control of rapid override we ve seen is tied to the single block switch If single block is on, the rapid override function is automatically activated and a multi-position switch (commonly feedrate override) is used to control the rate of motion In its lowest position, rapid motion occurs at but a crawl With this much control of rapid motion, even verifying very tiny rapid approach distances is safe and easy But as stated, not all machine tool builders provide this much control of their rapid rate With some rather crude rapid override functions, you have a four-position rapid override switch (100%,50%, 25%, and 10%) In its lowest position (10%), a machine having a rapid rate of 1,500 inches per minute will still be moving at 150 inches per minute Worse, some builders give but a simple on/off switch for rapid override If turned on, rapid motion will occur at 25% of its normal rate Some machines provide additional control of rapid rate with the dry run function When dry run is turned on, the jog feed or feedrate override switch is used to more adequately control rapid rate - and you can still slow motion to a crawl But since you should not let the machine cut under the influence of dry run (dry run slows rapid motion but it speeds up cutting motions), having to deal with dry run for the purpose of verifying approach movements can be cumbersome 5

Again note that with some machines, the only control you ll have of rapid rate is the rapid override function (dry run may not even affect rapid motions) With these machines, verifying approach movements when small approach distances are used can be very dangerous For machines that have inadequate control of rapid, and even with those that force you to use dry run to fully control rapid rate, you can facilitate the task of verifying approach movements by keeping the initial movement a tool makes in an approach (at rapid) a large distance from the surface to be machined - a distance that can be easily spotted at ten percent of the machine s rapid rate Usually 20 inches is sufficient For the balance of the approach, switch to the G01 straight line cutting mode and feed at a fast feedrate To minimize air cutting time, we recommend using the machine s fastest programmable feedrate, which is normally half the rapid rate Example: N015 G00 X10 Y10 N020 G43 H01 Z20 N025 G01 Z01 F2000 N030 G81 R01 Z-05 F45 With this approach, the machine will stop two inches above the work surface in line N020 The machine will still be moving at rapid during this movement, but the setup person should be able to catch any mistake if the tool comes closer than this distance In line N025, the feedrate override switch will control the balance of the approach motion, giving the setup person the ability to completely manipulate the approach motion rate Which is initialized, G00 or G01? It may be helpful to know that you have control of whether the machine powers up in the G00 or G01 mode (a parameter controls this choice) If your setup people and operators do quite a bit of manual data input (MDI) functions, and if these actions include actually causing axis motion, it may be wise to ensure that the machine powers up in the G01 mode to minimize the potential for undesirable rapid motion during their first MDI motion command Reducing rapid approach distance Most basic CNC courses teach beginners to rapid within 01 inch (or 25 mm) of qualified surfaces to be machined By qualified, we mean surfaces that are not varying from one workpiece to another For unqualified surfaces (like many castings and forgings), beginners are taught to keep the approach distance even greater While 01 inch is a safe approach distance, consider its effect on cycle time Say you must center drill (or spot drill) and drill fifty holes If you stay 01 inch away from the surface, the machine will be air cutting for a distance of 01 before it comes into contact with each hole Times fifty holes, that s five inches of air cutting At five inches per minute (not an unreasonable feedrate for center drilling or spot drilling), this equates to one minute of cycle time If you reduce the rapid approach distance to 005 inch, you ll cut thirty seconds from the cycle! Note that since you will still use verification functions like single block, dry run, and jog feedrate to control each tool s approach motion, this should be no more dangerous than having an approach distance of 01 inch (as long as the surface is truly 6

qualified) In fact, we contend that if you would have been taught in basic CNC courses to make your rapid approach distance 005 inch, you wouldn t have had any problems you haven t had staying 01 inch away! Note that this technique does assume that you are using a relatively accurate method of determining tool length compensation values (measuring tool lengths with a tool length measuring fixture, measuring tools on the machine, etc) What is your rapid approach distance after center drilling or spot drilling? The center drill actually makes a certain amount of clearance for the subsequent drill The larger the center drilled hole, the more clearance you ll have Look at the next drawing Rapid To Work Surface! Drawing shows how you can rapid the drill tip right to work surface after center drilling Believe it or not, you ll have ample clearance for the drill after center drilling to rapid the drill tip right down to the work surface Here is an example of how much clearance you ll have If you center drill to a 025 inch diameter, and if you use a 118 degree twist drill, the drill will still have to move about 007 inch before it starts cutting If you stay 01 away from the work surface, the tool will have to move 017 inch before it starts cutting! If you spot drill to a diameter bigger than the drill diameter (to make a chamfer for the hole to be drilled), you can actually send the drill into the hole by the drill lead amount (03 times the drill diameter for a 118 degree twist drill) and still have the chamfer amount for clearance Before you are too quick to discount this technique (many programmers are a little nervous when they hear this for the first time), go out to your machine with a stop-watch During the machining cycle use the stop-watch to determine just how much air cutting time there is in the program that s running In some cases, you can reduce the program execution time by over 20% by applying this technique! This savings will likely justify whatever effort and precautions you must take in order to safely implement it 7

G01 - Straight line cutting motion (also called linear interpolation) Because it is such a needed motion type, G01 is usually well covered in basic CNC courses Of course, G01 can be used to machine any straight surface - and a feedrate (F word) specifies the rate of motion Drilling holes, milling straight surface, and turning straight diameters, tapers and chamfers are among the many machining operations that can be done with G01 We have but a few points to make Efficiency of basic motion types Throughout your CNC career, you re going to be exposed to lots of fancy programming features that simplify programming (in module number one, we called them convenience features) While many of these higher level programming features are quite helpful, you must understand that the control can always follow a series of straight forward motion commands (G00, G01, G02, & G03) faster than it can interpret and execute a canned cycle that causes the same motions We say Any time you make the control think, it takes time From a purely cycle time related standpoint, straight forward motion commands will always make the control execute as quickly as possible Minimizing corner rounding All CNC controls have a look ahead buffer to keep the machine from having to come to a complete stop between commands This minimizes the tendency for tools to leave dwell marks on the workpiece as it is being machined However, to keep the machine from stopping during a transition from one straight line motion to another (G01 to G01), the control will actually cause the tool to begin the second motion command before it completely finishes the first For outside corners, this has the effect of creating a small radius on the corner (actually the motion generated is not a perfect radius) The larger the machine and the faster the feedrate, the more likely the control s tendency will be to have the tool to round corners For most applications, the amount of corner rounding is unnoticeable Either the machine is light enough or the feedrate is slow enough that the amount of corner rounding is immeasurable But consider milling a free machining material like aluminum with a larger machining center It is quite likely that outside corners (corners that are supposed to be sharp) will have a noticeable rounding which may cause the workpiece to be out of tolerance Fanuc and Fanuc-compatible control manufacturers offer two ways to program around this problem A G04 dwell command can be placed between the two G01 motions to cause the machine to come to a complete stop and pause for a specified length of time Or the exact stop check command (G09 or G61) can be used Either will have the effect of forcing the machine to leave a sharp corner Both the dwell command and the exact stop check commands are discussed later in this course If you have this problem on a regular basis, you should consult your machine tool builder While you can use the methods just introduced to program around this machine problem, your machine tool builder may be able to improve the way your machine s axes respond during transitions from one G01 command to another In essence, they may be able to tighten up the response of the axis drives These modifications are made through parameter changes 8

G02 & G03 - circular motion commands Since all machining and turning centers are equipped with these two motion types, they are also well covered in most basic CNC courses, While it is still a simple motion to understand, circular motion tends the be the hardest of the three basic motion types to master (rapid motion, straight line motion, and circular motion) Also note that with most controls, G02 and G03 are not only used to generate circular motion, they are also used to generate helical motion for milling threads on a machining center In this discussion, we ll only discuss G02 and G03 as they apply to circular motion Helical motion will be presented in the next module Which way is clockwise? In basic CNC courses, beginners are taught that G02 is clockwise circular motion and G03 is counterclockwise circular motion While this is generally correct, there is a better definition for determining arc direction For machines with more than two axes (like machining centers) you must determine clockwise versus counterclockwise by viewing the motion from the plus side of the uninvolved axis It just so happens that when you view XY circular motion on for a machining center, you re always doing so from the plus side of the Z axis However, if you even intend to program circular motion in the XZ, you must view the motion from the plus side of the Y axis (the column side of a vertical machining center) If you intend to program circular motion in the YZ plane, you must view the motion from the plus side of the X axis (right side of a vertical machining center) Look at the drawing Notice that since this is an XZ motion on a vertical machining center, you must view the motion from the plus side (column side) of the Y axis Z G02! X Additionally, if you do intend to make circular motion in any plane other than XY (XZ or YZ), you must first command the proper plane selection (see G17, G18, and G19 later in this module) It just so happens that G17 is initialized, meaning you never have to program plane selection if you work exclusively in the XY plane (as most programmers do) Limitation of the R word 9

Most instructors limit their presentations in basic CNC courses to the use of the R word to specify the size (radius) of the arc being generated While the R word works just fine, you should be aware of its limitation Generally speaking, the R word tends to be too forgiving That is, the control will respond by doing something regardless of whether the R word is correctly specified The major point: If you intend to use the letter address R to specify the radius of a circular motion, you better be sure that you specify it correctly If you specify a value that is too large or too small, it s likely that the arc machined will not be what you expect If, for example, you specify a too large a radius for an arc that s supposed to be tangent to both adjacent entities, it s likely that the arc will not be tangent to at least one of the entities This problem can be most troublesome when the amount of error is very small You probably won t catch it during a dry run Only when you machine (and scrap) your first workpiece will it be evident that something is wrong Directional vectors Commonly thought of as the old way to specify arc size for circular motions, directional vectors can still be used to specify the arc size Admittedly, they are more difficult to master than the simple R word But they also overcome the limitation just mentioned If you are off by as little as 00001 inch with your specification of directional vectors, most current model controls will generate an alarm - not allowing the program to cut (and scrap) a workpiece Three letter addresses are used (for two axis turning centers, only I and K are used): I - distance and direction from start point of arc to center of arc in X J - distance and direction from start point of arc to center of arc in Y K - distance and direction from start point of arc to center of arc in Z To determine which of I, J, and/or K you must use, first imagine arrow/s drawn from the start point of the arc to the center of the arc If that arrow or arrows can be drawn along the X axis, you ll be using an I in the circular motion command If you can draw an arrow along the Y axis, you ll be including a J And if you can draw an arrow along the Z axis (commonly on turning centers), you ll be including a K in the circular motion command You must also be concerned with polarity of directional vectors If the arrow/s point in the plus direction, the polarity of the related I, J, and/or K values will be positive If they point in the negative direction, the related polarity will be negative Admittedly, directional vectors are much more difficult to program than the simple R word However, since they tend to be more failsafe, we recommend using them, especially if you have a computer aided manufacturing (CAM) system that is generating your CNC programs for you (A CAM system can output directional vectors for circular motion as easily as it does the R word) Here is an example program that uses directional vectors for circular motions 10

Program: O0005 (Program number) N010 G54 G90 S350 M03 (Select coordinate system number one, absolute mode, and start spindle CW at 350 RPM) N015 G00 X-0625 Y-025 (Rapid to point 1) N020 G43 H01 Z-025 (Instate tool length compensation, bring tool down to work surface) N025 G01 X525 F35 (Feed to point 2) N030 G03 X625 Y075 J10 (CCW circular motion to point 3) N035 G01 Y325 (Feed to point 4) N040 G03 X525 Y425 I-10 (CCW circular motion to point 5) N045 G01 X075 (Feed to point 6) N050 G03 X-025 Y325 J-10 (CCW circular motion to point 7) N055 G01 Y075 (Feed to point 8) N060 G03 X75 Y-025 I10 (CCW circular motion to point 9) N065 G00 Z01 (Rapid away from workpiece) N070 G91 G28 Z0 (Return to tool change position) N075 G28 X0 Y0 (Return to starting point in X and Y) N080 M30 (End of program) Notice that since all of these arcs are full 90 degree arcs, only one or the other of I and J are required in each command Arc limitations Many basic CNC courses do not acquaint novice programmers with limitations related to how large an arc can be The limitation has to do with how many quadrant lines your 11

motion can cross A quadrant line is simply a centerline (vertical or horizontal) of the arc With most current model controls your motion is allowed to cross one quadrant line per circular command If your circular motion must go further, you must break the motion into two or more consecutive commands The only exception to this statement is that most current model controls do let you generate a complete circle in one command, as long as you start/end on a quadrant line For most controls, this means you can generate a circular motion of up to 180 degrees, assuming you start or end on a quadrant line Though this motion starts and ends on a quadrant line, it crosses but one quadrant line Full circle in one command As stated, most controls allow you to specify a complete circle motion in one command, as long as you start and end on a quadrant line To do so (with most controls), you must specify the motion with directional vectors (not with the R word) If you work exclusively with the R word for circular motion arc size, you may find it just as easy to break the full circle motion into two half circles and continue using the R word The command N055 G02 J-10 F50 will cause the machine to make a full circle in the clockwise direction with a 10 radius starting from the twelve o clock position (center of the arc is one inch minus of the start point along the Y axis) Arc in and out techniques For machining center contour milling applications, there will be times when you must approach to and escape from actual surfaces of the workpiece being machined If you move the tool directly to the surface (on axis only), it s likely that the tool will leave a nasty witness mark on the surface being machined See the drawing Witness mark here! Drawing shows tendency for leaving witness mark if end mill approaches right to surface To correct this problem, most programmers will have the tool arc in to approach and arc out to escape from the surface being machined The next drawing shows the motion 12

Minimize witness mark Drawing shows arc in and out to approach to and escape from machined surfaces 13