NUMERICAL CONTROL TECHNOLOGY

NUMERICAL CONTROL TECHNOLOGY
Chapter 3 THE CONTROL PRINCIPLE OF NUMERICAL CONTROL MACHINE TOOLS Electromechanical Engineering College Henan University of Science and Technology 领域：数控技术、CAD/CAM技术、柔性加工技术、集成制造技术、智能制造技术、虚拟制造技术、绿色制造技术趋势：高精度、高效率、自动化、信息化、智能化制造业数控化率年增长率达6%，据预测到2020年，我国制造业数控化率将达到60%，正向制造业大国迈进。

3.3、Velocity Control of CNC System
THE CONTROL PRINCIPLE OF NUMERICAL CONTROL MACHINE TOOLS Chapter 3 . 3.1、Introduction to the Control Principle of Numerical Control Machine Tools 3.2、Interpolation 3.3、Velocity Control of CNC System 3.4、Methods of Cutter Compensation in CNC System

THE CONTROL PRINCIPLE OF NUMERICAL CONTROL MACHINE TOOLS
Chapter 3 . 3.1 Introduction Every CNC machine discussed in this book possesses more than one axis of motion. More often than not, it will be necessary for the programmer to command that two or more axes move simultaneously in a controlled manner. For example, an end mill cutter is used on a machining center to machine a contour around the outside of a shape, This contour involves straight surfaces, angular surfaces, and round surfaces. While some of the movements in this example may involve only one axis, the angular and circular motions must involve at least two axes.

Chapter 3 . 3.1 Introduction In the early days of NC, this presented real problems. Whenever the program was required to produce an angular or circular surface, the motion had to be broken down into a long series of very small one-axis motions to form the angle or circle as closely as possible to the desired shape. this kind of motion normally required the help of a computer to produce. With the advent of a feature called motion interpolation, programming common complex movements became much simpler. With today’s current CNC controls, it is relatively easy to command angular and circular motion.

Chapter 3 What is Interpolation? . 3.2 interpolation
THE CONTROL PRINCIPLE OF NUMERICAL CONTROL MACHINE TOOLS Chapter 3 . 3.2 interpolation What is Interpolation? The one that most applies to CNC is the math-related definition: “To estimate a missing functional values at neighboring points.” When the control interpolates a motion, it is estimating very precisely the programmed path base on a small amount of input date.

Chapter 3 . 3.2 interpolation when the control makes a straight motion in two axes, The control automatically, all that is required is the start point and end point of the motion. The control automatically and instantaneously fills in the missing point between the start point and end point. What really happens is that the control makes a series of very small one-axis movement from the start point to the end point. This series of motions resembles a stairway. Each step along the way is very small, and the end result will appear to be a perfectly straight line.

Chapter 3 . 3.2 interpolation As you can see ,when two or more axes are programmed, the control forms a series of small one-axis movement. The size of each step determines the resolution （分辨率）of the axis. The smaller the step, the better the resolution.

Chapter 3 . 3.2 interpolation Circular interpolation is performed in much the same way. Knowing how a CNC control interpolates motion is not of primary concern to the programmer, though it is nice to know what is going on. What is more important to the programmer is to understand the various interpolation types for the particular CNC machine being programmed and have an understanding of how to make the required motion commands.

Chapter 3 . 3.2 interpolation CNC control manufacturers have designed carious types of interpolation commands around the most common motions the machine tool will be expected to make. The two most commonly used interpolation types are linear interpolation (straight-line motion) and circular interpolation (circular motion). Because they are commonly used, these two motion types are equipped as standard features on almost every kind of CNC machine in existence today.

Chapter 3 . 3.2 interpolation The two most commonly used interpolation types are linear interpolation (straight-line motion) and circular interpolation(circular motion).

Chapter 3 . 3.2 interpolation Other kinds of interpolation have much more specific applications and are only provided as options when required. helical interpolation（螺旋线插补）is used on machining centers to allow two axes to be commanded in a circular motion while a third axis is moving in a linear motion. The main application for helical motion is thread milling.

Chapter 3 . 3.2 interpolation Another kind of interpolation is parabolic interpolation（抛物线插补）. The motion generated in this interpolation is in the form of a parabola. hypothetical interpolation（双曲线插补）, allows users to define their own special form of motion, determined by the kind of motion they require. These two types of interpolation are seldom used or required.

Chapter 3 . 3.2 interpolation Again, the two most commonly used forms of interpolation are linear interpolation and circular interpolation. there is also another type of motion called rapid motion. Some control builders refer to this motion type as positioning. Rapid motion allows the axis motion to take place very quickly, and is generally used to minimize non-cutting time in the program. However, on most CNC machines, the rapid motion will not occur along a straight line, unless only one axis is commanded, so we do not consider it a true interpolation type.

Chapter 3 . 3.2 interpolation It should be refreshing for beginners to know that there are only three commonly used methods to cause axis motion(G00,G01,G02,G03).Every motion the typical CNC machine makes cab be divided into one of these categories. Once you master these motion commands, you will be able to generate the required motions to machine a work-piece.

Chapter 3 . 3.2 interpolation The usage of these commands remains remarkably similar for the various forms of CNC equipment. While there are some minor variations, mostly related to circular commands once you truly understand the information presented here, you will be able to apply what you know to any form of CNC equipment.

All motion types share five things in common.
THE CONTROL PRINCIPLE OF NUMERICAL CONTROL MACHINE TOOLS Chapter 3 . 3.2 interpolation All motion types share five things in common. First, they are all modal, meaning they remain in effect until changed or canceled. If more than one command of the same type is to be made, the programmer need only include the motion type in the first motion.

THE CONTROL PRINCIPLE OF NUMERICAL CONTROL MACHINE TOOLS Chapter 3 . 3.2 interpolation All motion types share five things in common. Second, each of these commands requires that the program include the point of the motion. The control will assume the axes are at the beginning point of the motion prior to the given motion command. This allows the programmer to think of motion commands as a series of connect-the-dots or point-to-point motions.

THE CONTROL PRINCIPLE OF NUMERICAL CONTROL MACHINE TOOLS Chapter 3 . 3.2 interpolation All motion types share five things in common. Third, all motion commands will be affected by whether or not the programmer decides to work from program zero. In the absolute mode (G90 on the most controls), the motion commands will be relative to the program zero point. In the incremental modl(G91 on most controls), the motion will be taken from the current position.

THE CONTROL PRINCIPLE OF NUMERICAL CONTROL MACHINE TOOLS Chapter 3 . 3.2 interpolation All motion types share five things in common. Fourth, each of these motion commands requires movement only of the axes stated in the command. If commanding a motion in only one axis, you need include only the moving axis letter address (X,Y,Z, etc.) and departure value in the motion command. All other axes’ letter addresses can be left out. The control will not attempt to move an axis unless an axis departure is included in the motion command.

THE CONTROL PRINCIPLE OF NUMERICAL CONTROL MACHINE TOOLS Chapter 3 . 3.2 interpolation All motion types share five things in common. Fifth, current CNC controls allow leading zeros to be left out of all types of commands. This means the actual G codes used to instate the motion types can be programmed in one of two ways.G00and G0 mean essentially the same thing to the control, as do G02 and G2,and G03 and G3.Our text will always include the leading zero to maintain compatibility with older controls.

Chapter 3 . 3.2.2 Linear-Circular Interpolation by the Evaluation Function Method Linear Interpolation by the Evaluation Function Method The approximated straight line OA (Figure 3.4) divides the XY plane into two regions: F>0,where the values of the evaluation function are positive, and F<0,where the values are negative. The straight line OA represents the segment F=0.

Chapter 3 . 3.2.2 Linear-Circular Interpolation by the Evaluation Function Method Linear Interpolation by the Evaluation Function Method Y X F<0 F>0 Pi (Xi,Yi) Ae (Xe,Ye) O X/Y = Xe/Ye

Chapter 3 . Fi>=0， +X Xi+1 = Xi +1 Fi+1 = XeYi –Ye(Xi+1) =Fi -Ye
THE CONTROL PRINCIPLE OF NUMERICAL CONTROL MACHINE TOOLS Chapter 3 . 3.2.2 Linear-Circular Interpolation by the Evaluation Function Method Linear Interpolation by the Evaluation Function Method Y X F<0 F>0 Pi (Xi,Yi) Ae (Xe,Ye) O Fi>=0， +X Xi+1 = Xi +1 Fi+1 = XeYi –Ye(Xi+1) =Fi -Ye Fi<0， +Y Yi+1 = Yi +1 Fi+1 = Xe(Yi +1)-YeXi =Fi +Xe

Chapter 3 . Linear Interpolation by the Evaluation Function Method If an intermediate point, say, the X1 Y1 point, is in the upper region F>0,the next step is taken along the X axis. If an intermediate point, say, the X2 Y1 point, lies in the lower region F<0,the next step is taken along the Y axis. Since we specify the path by incremental measurement, each endpoint of the last location lies in the origin of coordinates, F=0,X0=0,and Y0 =0.

Chapter 3 . Linear Interpolation by the Evaluation Function Method Since the start point is in the region F=0,we make the first step along the X axis to the point with coordinates X1 =1and Y0 =0.This point is in the region F<0,so the nest step is along the Y axis to the point with coordinates X1 =1 and Y1 =1.This point is in the region F>0,and so the nest move is along X to the X2 Y1 point. The step-by-step procedure at a rate specified by the NC speed program until the path of interpolation reaches the endpoint Xe ,Ye .

Chapter 3 . Linear Interpolation by the Evaluation Function Method If the interpolated section coincides with the X axis (Ye =0),the path of interpolation runs along this section and does not move beyond the region F=0.If the interpolated section lies on the Y axis, the first step which must always be laid off on the X axis is not taken

Chapter 3 . Linear Interpolation by the Evaluation Function Method The value and sign of the evaluation function are computed by an interpolator. As regards each intermediate point (Xi ,Yj )the function Fij depends both on the endpoint coordinates Xe ,Ye read from the program and on the current coordinates Xi ,Yj :Fij =YjXe-XiYe .As noted above, the start point of the path of interpolation lies at the origin, and so F00 =0.

Chapter 3 . Linear Interpolation by the Evaluation Function Method The current values of the function F are defined in the following way: after completing one step along the X axis, the coordinate Y of the current point dose not change, while the coordinate X increases by unity:Xi+1=Xi+1. The next step along the Y axis dose not change the X coordinate, but increase the Y coordinate by one:Yj+1=Yj+1.After completing the step from the XiYj point to the Xi+1Yj point, the function becomes Fi+1j=YiXe-Xi+1Ye=YjXe-(Xi+1)Ye=YjXe-XiYe-Ye. But YiXe-XiYe=Fij, and so Fi+1j=Fij-Ye. After moving for one step along the Y axis,the function becomes Fij+1=Fij+Xe.

Chapter 3 . Linear Interpolation by the Evaluation Function Method So, each endpoint becomes the origin for the next move. At these points the evaluation function is always zero, so all the successive of Xe and Ye determine this function. The sign of function that has resulted from the last step is the indication of the next step.

Mode 1 (F>=0) Mode 2 (F<0) a) X step a)Y step
THE CONTROL PRINCIPLE OF NUMERICAL CONTROL MACHINE TOOLS Chapter 3 . Linear Interpolation by the Evaluation Function Method Linear interpolation Mode 1 (F>=0) Mode 2 (F<0) a) X step a)Y step b)Fi+1j=Fij-Ye b) Fi+1j=Fij+Xe c)Xi+1=Xi+1 c) Yi+1=Yi+1 d) Xe = Xi+1 d) Ye = Yi+1

e.g . Line: OA， final point: Xe=6 ,Ye=4，start point :O
THE CONTROL PRINCIPLE OF NUMERICAL CONTROL MACHINE TOOLS Chapter 3 . Linear Interpolation by the Evaluation Function Method e.g . Line: OA， final point: Xe=6 ,Ye=4，start point :O O A 9 8 7 5 4 3 2 1 6 10 Y X

Chapter 3 . THE CONTROL PRINCIPLE OF NUMERICAL CONTROL MACHINE TOOLS
Linear Interpolation by the Evaluation Function Method 步数判别坐标进给偏差计算终点判别 F0=0 ∑=10 1 F=0 +X F1=F0-ye=0-4=-4 ∑=10-1=9 2 F<0 +Y F2=F1+xe=-4+6=2 ∑=9-1=8 3 F>0 F3=F2-ye=2-4=-2 ∑=8-1=7 4 F4=F3+xe=-2+6=4 ∑=7-1=6 5 F5=F4-ye=4-4=0 ∑=6-1=5 6 F6=F5-ye=0-4=-4 ∑=5-1=4 7 F7=F6+xe=-4+6=2 ∑=4-1=3 8 F8=F7-ye=2-4=-2 ∑=3-1=2 9 F9=F8+xe=-2+6=4 ∑=2-1=1 10 F10=F9-ye=4-4=0 ∑=1-1=0

Chapter 3 . Circular Interpolation by the Evaluation Function Method The approximation of a curved path consists in the following. The arc of the circle (Figure 3.5)divides the XY plane into two regions :F>0,on the outside of the curve, and F<0,on the inside of the curve. The curve itself represents the segment where F=0.The interpolated section of the arc has the start point with coordinates X0 ,Y0 and the endpoint with coordinates Xe, Ye. The origin of coordinates lies at the enter of the circle of radius R.

Chapter 3 . Circular Interpolation by the Evaluation Function Method If an intermediate point, say, the X1Y3 point, is in the region F>0,the next step is taken along the X axis. If an intermediate point,say,X2Y3,in the region F<0,the next step is taken along the Y axis.

Chapter 3 . 1） CCW F≥0， -X Fi<0， +Y
THE CONTROL PRINCIPLE OF NUMERICAL CONTROL MACHINE TOOLS Chapter 3 . Circular Interpolation by the Evaluation Function Method X Y Pi（Xi，Yi） A B F > 0 F < 0 1） CCW F≥0， -X Fi<0， +Y

Chapter 3 . 2） CW F≥0， -Y Fi<0， +X
THE CONTROL PRINCIPLE OF NUMERICAL CONTROL MACHINE TOOLS Chapter 3 . Circular Interpolation by the Evaluation Function Method X Y Pi（Xi，Yi） A B F > 0 F < 0 2） CW F≥0， -Y Fi<0， +X

Chapter 3 . Circular Interpolation by the Evaluation Function Method In interpolating the arc by the way of movement from the XiYj point to the Xi+1Yj point, we have Xi+1=Xi-1.With the step completed along the Y axis from the XiYi point to the XiYi+1 point, we have Yj+1=Yj+1. The start point of the curve (X0,Y0)is given by the formula X02+Y02=R2.The evaluation function at the start point is F=0,and at an intermediate point it is Fij=Xi2+Yj2-R2.

Chapter 3 . Circular Interpolation by the Evaluation Function Method The X step from the XiYj point to the Xi+1Yj point gives Fi+1j=Fij-2Xi+1;the step from the XiYj point to the XiYj+1 yields Fij+1=Fij+2Yi+1. Since the initial value of F is zero, all the subsequence values of the function will be find by the current values of the endpoints.

b) Fi+1j=Fij-2Xi+1 b) Fij+1=Fij+2Yj+1 c)Xi+1=Xi-1 c) Yi+1=Yi+1
THE CONTROL PRINCIPLE OF NUMERICAL CONTROL MACHINE TOOLS Chapter 3 . Circular Interpolation by the Evaluation Function Method Mode 1 (F>=0) Mode 2 (F<0) a) X step a) Y step b) Fi+1j=Fij-2Xi+1 b) Fij+1=Fij+2Yj+1 c)Xi+1=Xi-1 c) Yi+1=Yi+1 d)Xe = Xi+1 d) Ye = Yi+1

e.g . CCW circle: start point : A（4，0 )final point: B（0，4）
THE CONTROL PRINCIPLE OF NUMERICAL CONTROL MACHINE TOOLS Chapter 3 . Circular Interpolation by the Evaluation Function Method e.g . CCW circle: start point : A（4，0 )final point: B（0，4） A B Y X 4

Chapter 3 . THE CONTROL PRINCIPLE OF NUMERICAL CONTROL MACHINE TOOLS
Circular Interpolation by the Evaluation Function Method 步数偏差判别坐标进给偏差计算坐标计算终点判别起点 F0=0 x0=4, y0=0 Σ=4+4=8 1 -x F1=F0-2x0+1 =0-2*4+1=-7 x1=4-1=3 y1=0 Σ=8-1=7 2 F1<0 +y F2=F1+2y1+1 =-7+2*0+1=-6 x2=3 y2=y1+1=1 Σ=7-1=6 3 F2<0 F3=F2+2y2+1=-3 x3=4, y3=2 Σ=5 4 F3<0 F4=F3+2y3+1=2 x4=3, y4=3 Σ=4 5 F4>0 F5=F4-2x4+1=-3 x5=4, y5=0 Σ=3 6 F5<0 F6=F5+2y5+1=4 x6=4, y6=0 Σ=2 7 F6>0 F7=F6-2x6+1=1 x7=4, y7=0 Σ=1 8 F7<0 F8=F7-2x7+1=0 x8=4, y8=0 Σ=0

Chapter 3 . 3．3 Forms of Compensation Now we begin our discussions of the specific types of compensation available for different CNC machine tools．If you are a beginner to CNC，it is necessary that you understand the reasons why the various forms of compensation work as they do．In fact，we say it is as important to understand why you need compensation for the various purposes，at least at first，as it is to know the commands to use it．Knowing the reasons why compensation is needed will help you understand how to use it．

Chapter 3 . 3．3 Forms of Compensation Also along these lines，you will find that the actual programming commands related to the various forms of compensation will vary dramatically from one CNC control to the next，yet the basic reason for its use will not．That is，why tool length compensation is needed will stay the same from one machining center to the next，but its usage will vary．If you understand why you need the compensation type，you are well on your way to understanding how to use it．Also，knowing why compensation is used for its various purposes will allow you to easily adapt to any one version of its use.

Chapter 3 . 3．3 Forms of Compensation Here is a list of the compensation types we will only discuss the cutter radius compensation and the CNC machine tools related to the compensation： Compensation Related Tool length compensation Machining centers Cutter radius compensation Machining centers Fixture offsets Machining centers Dimensional tool offsets Turning center tool nose radius compensation Turning centers Wire radius compensation Wire EDM machines Wire taper compensation Wire EDM machines

Chapter 3 . 3．3．1 Cutter Radius Compensation Cutter radius compensation (also called cutter diameter compensation) is used on machining centers and similar CNC machines．This feature allows the programmer to forget about the cutting tool’s radius or diameter during programming．Like all forms of compensation, it makes programming easier，since the programmer need not be concerned about the exact cutter diameter while the program is being prepared．Cutter radius compensation also allows the radius 0t the cutting tool to vary without modification to the Program．

Chapter 3 . 3．3．1 Cutter Radius Compensation Cutter radius compensation is not applied to all forms of cutting tools．It is needed only for cutting tools that have the ability to machine on the periphery of the cutter，and only when machining the periphery of the cutter．Tools like end mill,，shell mills，and some face mills have this ability．Drills，reamers，taps，boring bars，and other center cutting tools have absolutely no use for cutter radius compensation．

Chapter 3 . 3．3．1 Cutter Radius Compensation One way to program the milling cutter’s path is to program the motions by the centerline of the milling cutter．In this case，the programmer must take into consideration the diameter of the milling cutter．For example，if the milling cutter is 1 inch in diameter，all motions programmed must be kept precisely 0．5 inch away from the surfaces to be milled．Even this assumes that there is no tool pressure pushing the cutting tool away from its programmed path．Tool pressure will be discussed further later．

Chapter 3 . 3．3．1 Cutter Radius Compensation
THE CONTROL PRINCIPLE OF NUMERICAL CONTROL MACHINE TOOLS Chapter 3 print． . 3．3．1 Cutter Radius Compensation

Chapter 3 . 3．3．1 Cutter Radius Compensation While using the centerline coordinates of the tool path is a popular way of programming，it has several disadvantages and limitation． Here we list and explain them．Each of these limitations presented real problems before cutter radius compensation became available．Fig 3．16 shows the difference between the cutter radius tool's centerline coordinates and part coordinates．Notice that the tool's centerline coordinates require at least one extra calculation to be made for each axis in the coordinate system．On the other hand，part coordinates are usually taken right from the print．

Chapter 3 . 3．3．2．1 Reasons for Cutter Radius Compensation There are several reasons why cutter radius compensation is so helpful．It relieves several programming burdens．Here we list and explain why it is so important to use this feature when you have reason to do so．

Chapter 3 . 3．3．2．1 Reasons for Cutter Radius Compensation Changes in tool diameter．Using a 1-inch diameter end mill to machine the right side of a rectangular work—piece being held In a vise would be considered a simple operation by most experienced programmers．If a programmer prepares the program on the basis of the tool’s centerline coordinates--not using cutter radius compensation, the end mill must be kept away from the right side of the rectangular work—piece by precisely inch throughout its motions．

Changes in tool diameter．
THE CONTROL PRINCIPLE OF NUMERICAL CONTROL MACHINE TOOLS Chapter 3 . 3．3．2．1 Reasons for Cutter Radius Compensation Changes in tool diameter． Imagine that the operator 1s making the setup and discovers the company is out of 1-inch end mills．There are inch—diameter end mills and 1.25-inch-diameter end mills，but no end mills left in 1-inch diameter．In this case，the programmer would have to change the program in order to use an end mill diameter other than the one programmed．

Chapter 3 . 3．3．2．1 Reasons for Cutter Radius Compensation Tool pressure．Most machinists will agree that the cutting tool will seldom machine the work piece as desired on the first try．The cutting tool，work—piece，and even the machine tool itself are under a great deal of pressure during machining．the more powerful the machining operation is，the greater the pressure．Even when a milling cutter is kept quite rigid (sturdy end mill holder and short overall length)，there will be some deflection of the tool during machining．This is because the cutting edge of the tool will have a tendency to push away from the surface being machined．

Chapter 3 . 3．3．2．1 Reasons for Cutter Radius Compensation If you have ever scraped paint from the wall of a room，you have experienced this kind of deflection．When scraping paint，you do your best to push the scraper in a way that will remove the paint，but many times your scraper will be deflected from the surface to be scraped．In machining terms，this tendency to deflect is called tool pressure． Generally speaking，the weaker the machine tool and cutting tool are，the more potential for deflection．While the small deflection may not be substantial enough to cause problems， there are times when it will. This is especially true when the accuracy required of the part is demanding．

Chapter 3 . 3．3．2．1 Reasons for Cutter Radius Compensation In the previously discussed example related to milling the right side of a work—piece，even if an end mill precisely 1 inch in diameter is used，there is still the potential for deflection of the tool during machining．Depending on the expected tolerance for this surface，the amount of deflection may be enough to cause the part to be out of tolerance．If this were the case，and if fixed centerline coordinates were used，it would mean having to reprogram the milling cutter to allow for deflection．

Chapter 3 . 3．3．2．1 Reasons for Cutter Radius Compensation Also note that，as the cutter dulls，deflection will increase．This means a sharp cutter will have less deflection than a dull one. This change in deflection amount during the life of a cut ting tool can present real headaches While machining if fixed centerline coordinates are used in the program．

The class is over Have a nice meal !

NUMERICAL CONTROL TECHNOLOGY

Similar presentations

Presentation on theme: "NUMERICAL CONTROL TECHNOLOGY"— Presentation transcript:

Similar presentations

About project

Feedback

Log in

Auth with social network:

NUMERICAL CONTROL TECHNOLOGY

Similar presentations

Presentation on theme: "NUMERICAL CONTROL TECHNOLOGY"— Presentation transcript:

Similar presentations

About project

Feedback