Chapter 9. NC Part Programming: Defining Geometry and Machining Plan (Motion)

Transcription

1 Chapter 9. NC Part Programming: Defining Geometry and Machining Plan (Motion) NC Program Storage Media Punched Card Tape (one inch wide) Magnetic Tape Floppy Disk and CD Transfer data through RS-232 interface from controller to computer using such protocols as Kermit and Xmodem. Also, some machines use local area network (LAN) instead of serial communications. Symbolic Codes Binary-Coded Decimal (BCD): eight-track punched tape is one common input media for NC machines American Standard Code for Information Interchange (ASCII): was formulated in 1979 to standardize the punched codes, but this is also used in computers and telecommunications. Many new NC systems accept both BCD and ASCII codes.

2 Tape Input Format (organization of words within blocks)

3

4 Address: An identifying letter inserted in front of each word. Words: Each item of the program sheet, such as the sequence number, the preparatory (G) function, and the X position, forms one word on the tape. Blocks: A block consists of all the items or words needed to instruct the machine how to perform in any one position of the work piece. The way in which blocks are arranged along the length of the tape is known as the block format.

5 Four tape inputs are used for NC: Fixed sequential format requires each NC block be the same length requiring all values appear even if they are not required. Block address format eliminate the need for specifying redundant information in subsequent NC blocks through a change code. All data must contain a predefined number of digits. Tab sequential format has the words listed in a fixed sequence and separated by the tab key. Each tab will skip the redundant data.

6 Block Address Format and G-code program A block of NC part program consists of several words and a program written in this data format is called NC program (or simply g-code). A NC program can contain any of following word addresses (word = address + value). N,G,X,Y,Z,A,B,C,H,I,J,K,F,S,T,R,M,U,V,W N-code: The N-word specifies the sequence number to identify the block within the program. G-code (preparatory code): prepares the MCU for control functions.

7 X,Y,Z,A,B,C,U,V,W-codes: provide coordinate position of the tool. X,Y,Z are for translational (Cartesian) axes and A,B,C are for rotational axes about X,Y,Z axes. U,V,W are incremental X,Y,Z. Ex. Move the cutter to a new position (1.12, 2.275, 1.0) X1.12 Y2.275 Z1.0

8 G-code [0-9] All G codes listed are for RS-274 compatible CNC controls. Motion Class [G00 G09] G00: rapid traverse code (PTP) G01: linear interpolation G02: CW circular interpolation G03: CCW circular interpolation G04: dwell G08: acceleration G09: deceleration

9 G10-G19 Presets and Plane Selection G-Codes [G10 - G19] G17: X-Y plane G18: Z-X plane G19: Y-Z plane

10 G20-29 Unit Selection G-Codes and Machine Coordinate Motion [G20 - G29]

11 G30-39 Feedrate Control and Threading [G30 G39]

12 G40-49 Tool Compensation Codes [G40 - G49] G40: cutter compensation cancel G41: cutter compensation left G42: cutter compensation right

13 Tool Radius Compensation The tool compensation (sometimes, cutter radius compensation [CRC]) commands will effectively compensate the tool-path along the tool-path direction (the program knows all tool-paths). Start and End of Compensation If G41 or G42 and G01 are in the same block, there will be a gradual effect of compensation (ramp-up block). N0020 G01 G41 X0.500 Y2.000 N0030 G01 X2.500 M96 Note that the tool moves along the hypotenuse of a right triangle in the ramp compensation with right angle at the destination point.

14 If G41 or G42 and G01 are in separate blocks from X and Y, the compensation is effective from the start of the block N0010 G41 N0020 X0.500 Y2.000 N0030 G01 X2.500 G40 also works same way as G41 and G42 in opposite way. N0070 G40 X3.000 Y2.000 M02 N0070 X3.000 Y2.000 N0080 G40 M02

15 Cornering Fadal CNC Controls: Use of M96 and M97 with M96 the controller adds an additional block for circular arc at the corner, while with M97 the cutter moves to machining point. If a step to be machined is smaller than the cutter radius, M97 must be used instead of M96. Note that a fillet is used than sharp corner in design. For a 3D corner, both M96 and M97 produce different results as below.

16 Fanuc CNC Controls: Use of G09 or G61 and G64 Non-modal exact stop check command: G09 Modal exact stop check command: G61 and G64 (to cancel) G01 G09 X40 Note that G09 is effective after the motion to X40. Also, it is non-modal command and works only for one step while G61 is modal command and effective until it is cancelled.

17 G50-59 Transformation and Coordinate System G-Codes [G50 - G59] G50,51: scaling and mirroring G52: shift the workpiece zero (i.e., part zero) point of the program created in the work coordinate system (G54 - G59)

18 G60-69 Machine Specific G-Codes [G60 - G69] G65,66,67: macro programs G68,69: CS rotation code

19 G70-79 Repetitious Cycle G Codes [G70 - G79] G70: inch format G71: metric format G74: full circle programming off G75: full circle programming on

20 H,T,R-Codes H-code: used for tool length offset Ex. G43 H2 T-code: when automatic tool changer is available, T-code specifies the tool number. Ex. T2 M6 R-code: specifies the clearance height (i.e., R-plane) for cycle parameter such as drilling. Ex. N0020 G81 X1.0 Y2.0 Z0.0 R1.3 N0030 G80

21 M-Code M-code: machine-specific (i.e., vendor-specific) and used for miscellaneous words to control miscellaneous functions such as start on/off, spindle on/off, turn on/off the coolant, laser on/off, change the tool, and rewind the program. Some example codes are M00: program stop M01: Optional stop M02: end of the program M03: spindle CW M04: spindle CCW M06: tool change M07: flood coolant on M08: mist coolant on M09: coolant off M30: end of tape

22 Manual Part Programming (Motion) In manual programming, the machining instructions are recorded on a document called a part-program manuscript by the part programmer. Because a part program records a sequence of tool motions and operations to produce the final part geometry, one must prepare a process plan with setups and fixtures before writing the program where the workpiece location and orientation, features (holes, slots, pockets) to be machined, tools and cutting parameters used need to be determined.

23 Safety Blocks Safety Blocks at Beginning of the NC Code One good practice in writing NC part programs is that all NC programs should start with what are called Safety Blocks of G and M codes at the start of the NC program. Even though some CNC controls set motion and register defaults themselves at program start, not all do and keep using whatever parameters were active last time. One example of the safety block is shown below. N10 G90 G70 G40 G49 G17 G80 G53 G00 Here, G90 programming in absolute coordinates (incremental coordinates G91), G70 defines inch unit (G71 for metric unit), G40 cancels any XY cutter compensation, G49 cancels the tool length compensation [the tool length command is used mostly for multiple tool NC programs so that each tool will cut to the correct depth, regardless of how far it extends out of the holder], G17 sets the plane to the XY plane for arc motion, G80 cancels any canned drill cycles, G53 cancels any work coordinate shift, and add a default motion code by putting a G00 since the initial move is almost always a rapid position move from the home location to the program start point.

24 Program Entry Moves (NIST: National Institute of Standards and Technology) Two pre-entry moves and one entry move are generally required. Two methods, general method and simple method, are used for entry moves. N0010 G1 X1 Y5 (to C) N0020 G1 G41 Y4 (to B) N0030 G3 X2 Y3 I1 (to A)

25 Another case where the entry point is given on the concave arc as below can be handled in same way.

26

27 Ex.1. Part Programming for Laser Cutting The laser machining on a table is basically two-dimensional machining and can be assumed zero cutting width. The laser beam focal radius can be very small less than 1/1000 inch. The following is two-dimensional CAD drawing of a thin part. Make a part program to cut out the part by laser. Exclude the letters in the middle.

28 The following shows the sequence of cutting when a automatic converter software is used to convert the 2D drawing DXF file to NC file. The sequence depends on the order of the way the drawing was created. This is neither efficient nor correct. Keeping in mind that the outline must be machined last, make a program for continuous cutting when possible.

29 Geometries for Program

30 F100 L1 G92X0Y0 M88 G0 X Y M90 G2 X Y I J M91 G0 X Y M90 G1 X Y G1 X Y G1 X Y G1 X Y M91 G0 X Y M90 G1 X Y G1 X Y M91 G0 X Y M90 G1 X Y M91 M89 M30 F100: defines the feed rate 100 in/min G92: set a point as the new origin of coordinates that is referenced by subsequent absolute positioning L1: material selection defined previously M88: shutter open for smoke removal M89: shutter close M90: laser on for cutting M91: laser off Programming Tip 1. Cut the outline last 2. Make continuous cutting if possible

31 Ex.2 Fadal CNC Controls Example [NC Program with Fadal CNC Controls] Make a NC program for the following part with tool compensation. The tool diameter of #1 is 0.5 inch. The spindle speed is 5000 rpm and the federate is 25 ipm for plunging and 50 ipm for interpolation. Starting point is SP. The machining must start from A and then move counterclockwise. At the end of cutting move the tool to the starting point with gradual cancellation of the tool compensation. The retract plane is z=0.5 and the feed plane is z=0.1. Plunge cut to z=-0.3 for the workpiece of thickness 0.2 with top at z=0. The point A is located at (1,1) and SP is the starting point.

32 What must be done if one wants to move directly to A?

33 N100 G20 N102 G0 G17 G40 G49 G80 G90 [safety block] N104 T1 M6 N106 G0 G90 G54 X0. Y0. A0. S5000 M3 N108 G43 H1 Z0. N110 Z.5 [to retract plane] N112 X-1. Y2. [any point in upper left side of A] N114 Z.1 [to feed plane] N116 G1 Z-.3 F25. N117 G42 X1. Y1. F50. [tool compensation right] N118 X3.8 M96 [modal, default in some machines] N120 Y N122 G2 X Y3. I.3 J N124 G1 X2.2 N126 Y2.8 M97 N128 X1. M96 N130 Y1. N132 Z-.2 F125. [off machining surface, good practice] N134 G0 Z.5 [to retract plane] N136 G40 X0. Y0. [tool compensation cancel] N140 M5 N142 G91 G28 Z0. [to machine zero thru z0] N144 G28 X0. Y0. A0. [to machine zero thru x0,y0,a0] N146 M30

34 Computer-Assisted Part Programming In computer assisted part programming in CAM that has almost replaced standalone APT s, general purpose computers are used as an aid to programming and special-purpose high level programming languages perform the various calculations necessary to prepare the CL data. There are two major part programming languages: Machine-oriented languages create tool paths with all necessary calculations processing the special coordinate-data and coding for speed and feedrate General purpose languages break down the computer processing into two: preprocessing and post-processing. The processing state produces an intermediate data points for cutter location (CL). There are three steps Translate input symbols Arithmetic calculations Cutter offset calculations

35 In computer assisted part programming Machine-oriented languages General purpose languages EIA RS-494B provides a new standard for computer numerical control that allows different machines operate from the same input data. This standard is Standard for 32-Bit Binary CL Exchange (BCL) Input Format for Numerically Controlled Machines. The BCL format represents NC machining input data that are 32-bit binary integer words. The contents of this record closely parallels the contents of CL data record in ANSI Programming Language APT. A BCL file is typically produced by a part-oriented post-processor call a BCL converter. The BCL format appears as: FILE HEADER (optional) PARTNO (optional) UNITS record DATA record (continue) DATA record END OF FILE record

36 EIA-RS-494 EIA-RS-494 is a 1983 Binary Cutter Location (BCL) standard for CNC. [From Wikipedia, 11/13/2012] Here is a list of Electronic Industries Alliance (EIA) Standards. The EIA ceased operations on February 11, 2011, but the former sectors continue to serve the constituencies of EIA. EIA designated ECA to continue to develop standards for interconnect, passive and electro-mechanical (IP&E) electronic components under the ANSI-designation of EIA standards. All other electronic components standards are managed by their respective sectors. ECA is expected to merge with the National Electronic Distributors Association (NEDA) to form the Electronic Components Industry Association (ECIA). However, the EIA standards brand will continue for IP&E standards within ECIA. As currently authorized, any ANSI standard designated at ANSI EIA-xxx is developed and/or managed by ECA (and, in the future, ECIA).

37 Computer-Assisted Part Programming by Pro/Manufacturing > CL Data

38 APT (Automatically Programmed Tool) More than 100 part-programming languages have been developed since 1956 and some have stood the test of time and did not. APT has been the most popular part-programming language and employed by most CAM systems. Summary characteristics of APT is given below Three dimensional unbounded surfaces and points are defined to represent the part Surfaces are defined in a X-Y-Z coordinate system chosen by the part programmer In programming, the tool does all the moving; the part is stationary The tool path is controlled by pairs of three-dimensional surfaces; other motions, not controlled by surfaces, are also possible A series of short straight-line motions are calculated to represent curved tool paths (linear interpolation) The tool path is calculated so as to be within specified tolerances of the controlling surfaces The X, Y, and Z coordinates of successive tool-end positions along the desired tool path are recorded as the general solution to the programming problem Additional processing (postprocessing) of the tool-end coordinates generates the exact tape codes and format for a particular machine

39 An APT processor interprets and computes the cutter path, whereas a post-processor translates the cutter-path to a format acceptable by a specific machine. 1. Identification statements. These define a specific project. 2. Geometry statements. These define a scaler or geometric quantity. 3. Motion statements. These describe a cutter path, such as GOLFT. 4. Postprocessor statements. These define machining parameters such as feed, speed, coolant on/off and so on. 5. Auxiliary statements. These describe auxiliary machine-tool functions to identify the tool, part, tolerances, and so on.

40 ANSI INCITS Programming Language APT (revision, redesignation and consolidation of ANSI X , ANSI X /AM , ANSI X /AM ) (formerly ANSI INCITS ) Establishes the form for, and the interpretation of,programs expressed in the Automatically Programmed Tools (APT) language and of the System-Neutral CLFILE (SCL), which can be generated by processors, such as APT, or by graphical systems. The purpose is to promote portability of these input language programs to a wide variety of computers. In addition, the SCL permits commonality and portability, regardless of the source that produces it, to a wide variety of manufacturing equipment. APT is an English-like language for describing operations for numerically controlled machines. An APT language input program is converted by a computer processor and, probably, subsequently by a postprocessor into an ordered set of instructions for numerically controlled machines.

41 APT: Part Definition (Geometry) Geometry Statements Creating entities such as points, lines, circles, planes, cylinders, cones, and spheres structure variable = function name / function description

42 Point Definitions PT=POINT/X,Y,Z PT=POINT/INTOF,LINE1,LINE2 PT=POINT/MODIFIER,INTOF,LINE1,CIRCLE1 where Modifier options are {xlarge,xsmall,ylarge,ysmall} PT=POINT/MODIFIER,INTOF,C1,C2 PT=POINT/CIRCLE,ATANGL (in degrees) PT=POINT/CENTER,CIRCLE PT=POINT/MODIFIER,INTOF,LINE,CONE (intersection of a line with a cone) PT=POINT/INTOF,PLANE1,PLANE2,PLANE3(intersection of three planes PT=POINT/RTHETA,XYPLAN,RADIUS,ANGLE (polar coordinates) PT=POINT/INTOF,LINE,TABCYL,TABC1 (Intersection of a line and a tabulated cylinder) PT=POINT/PATTERN,N (Point as Nth location of a pattern)

43 Line Definitions Ln=Line/x1,y1,z1,x2.y2.z2 (Line thru a pt and tangent to a circle) Ln=Line/point,modifier,tanto,circle (Line tangent to two circles) Ln=Line/modifier,tanto,circle1, modifier,tanto,circle2 (Line tangent to two circles) Ln=Line/point,atangl,axis (Line thru a pt and making an angle w/axis ) Ln=Line/point,slope,value(Line thru a pt and having a slope ) Ln=Line/xaxis (or yaxis) (Line on a axis) Ln=Line/point,slope,value,line2(Line thru a pt and having a slope wrt another line) Ln=Line/point,parlel,line(Line thru a pt and parallel to another line) Ln=Line/point,perpto,line(Line thru a pt and perpendicular to another line) Ln=Line/parlel,line,modifier,offset value(line parellel to another line given offset distance)

44 Ln=Line/intof,plane1,plane2 (Line given by intersection of two planes) Ln=Line/atangl,value,interc,modifier,value Ln=Line/point,tanto,tabcyl (Line in x-y plane passing thru a pt and tangent to a tabulated cylinder) Ln=Line/point,perpto,tabcyl (Line thru a pt and perpendicular to a tabulated cylinder)

45 Ex.3 (programming for geometry) Introduce a coordinate and label geometric entities and define the geometries that can form the part. Define all points and then lines using the points defined before.

46 Planes Definitions Plane requires three points for complete definition. Plane by equation: PL=plane/a,b,c,d in equation ax+by+cz-d=0 Plane by 3 pts: PL=plane/pt1,pt2,pt3 Plane thru a pt and parallel to another plane: PL=plane/pt,parlel,pl2 Plane parallel to another plane at a distance: PL=parlel,pl2,modifier,value, modifier={xsmall,xlarge,ysmall,ylarge,zsmall,zlarge} Plane thru a point and perpendicular to a vector: PL=plane/pt,perpto,vector1 Plane thru two pts and perpendicular to another plane: PL=plane/pt1,pt2,perpto,pl1 Plane perpendicular to two planes and thru a pt: PL=plane/pt,perpto,pl1,pl2

47 Definition of Circle By a center and a radius: C=circle/center,pt1,radius,value By a center and tangent to a line: C=circle/center,pt,tanto,line By a center and a pt on its circumference: C=circle/center,pt1,pt2 on circumference By three pts: C=circle/pt1,pt2,pt3 By a center and a tangent to another circle: C=circle/center,pt1,modifier (large or small) By a radius and two intersecting lines: C=circle/tanto,line,modifier,pt,radius,value By a radius tangent to a line and thru a pt: C=circle/tanto,line,modifier,pt,radius,value By a radius tangent to a line and another circle: C=circle/ modifier,line, modifier,in/out,c2,radius,value By a radius and tangent to two circles: C=circle/ modifier,in/out,c2,in/out,c3,radius,value By a radius tangent to a line and a tabulated cylinder: C=circle/tanto,line1,modifier,tabcyl, modifier,point (closest pt), radius, value

48 Definition of Cylinders cy=cylinder/x,y,z,a,b,c,radius cy=cylinder/center_pt,axix_vector,radius tc=tabcyl/modifier1,modifer2,[trform,m],data where modifiere={nox,noy,noz,rtheta,thetar} and tabulated cylinder is a surface created by a curve and a vector Suf=rldsuf/suf1,p1,p2,p3,suf2,p4,p5,p6 A ruled surface is created blending two curves.

49 Ex.4 (cylinder) Introduce a coordinate and label geometric entities and define the geometries that can form the part. Start with lines if possible to define entities.

50 Ex.5 (surfaces) Introduce a coordinate and label geometric entities and define the geometries that can form the part. Start with lines if possible to define entities.

51 Additional Definitions Elips = ellipse/center,pt,semi-major axix length, semi-minor axis length, semi-major axis angle. Hyp = hyperb/center, pt, length of half transverse axis, angle of transverse axis Cn = cone/x,y,z,a,b,c,angle where x,y,z and a,b,c are vertex and base center coordinates Cn = cone/point,vector,angle Vc = vector/ x, y, z Vc = vector/pt1,pt2 Vc = vector/perpto,plane,modifier where modifier = {posx,posyposz} Vc = vector/vec1,cross,vec2 Ptrn = pattern/linear,pt1,pt2,no_of_pts Ptrn = pattern/linear,pt,vec,incr,no_of_incr,at,d Ptrn = pattern/linear,pt,vec,incr1,incr2,incr3,,incrn Ptrn = pattern/radial,incr_angle,total_angle,ccw,n

52 Ex.6 (part) Introduce a coordinate and label geometric entities and define the geometries that can form the part. Start with lines if possible to define entities.

53 Motion Statement Basic motion statements are based on three surfaces that guide the tool in three-dimensional space. They are Drive Surface Part Surface Check Surface

54 There are two types of motion; point-to-point (PTP) motion for rapid traversing without cutting contouring for continuous material removal in three-dimensional space.

55 GOTO and FROM Statement GOTO / a point This is a PTP statement for rapid motion. FROM / a point This is to start a motion from.

56 GO Statement This is for contouring. TO TO TO GO / ON, Drive Surface, ON, Part Surface, ON, Check Surface PAST PAST PAST TANTO The modifier TANTO is only used by check surface. CS CS CS DS DS DS DS CS On PS On PS On PS On PS GO/TO,DS,TO,PS,TO,CS GO/TO,DS,TO,PS,ON,CS GO/TO,DS,TO,PS,PAST,CS GO/TO,DS,TO,PS,TANTO,CS

57 Ex.7 Example [Part Program] Make an APT program for the following part with tool compensation using APT. Use POINT, LINE, CIRCLE to define geometry first, and then use motion statements such as FROM, GOTO, GO. Starting point is SP from which move to the point A and then move counterclockwise. At the end of cutting move the tool to the starting point. Ignore all other commands. The point A is located at (1,1) and SP is at the origin. The cutting precision of machine is 1/1000 in. Assume the tool moves tangent to the part surface PL1 that is positioned at z = 0.

58 Solution SP = POINT / 0,0,0 PTA = POINT / 1,1,0 PTB = POINT / 3.8,1,0 PTC = PONT / 3.8,1.735,0 PTD = POINT / 2.815,2.8,0 PTE = POINT / 2.2,2.8,0 PTF = POINT /2.2,2.6,0 PTG = POINT / 1,2.6,0 LNAB = LINE / PTA,PTB LNBC = LINE / PTB,PTC CIRCLECD = CIRCLE / POINT(4.1,3.2,0),PTB,PTC LNDE = LINE / PTD,PTE LNEF = LINE / PTE,PTF LNFG = LINE / PTF,PTG LNGA = LINE / PTG,PTA FROM / SP GO / TO,LNAB,TO,PL1,ON,LNAG GO / TO,LNAB,TO,PL1,PAST,LNBC GO / TO,LNBC,TO,PL1,PAST,CIRCLECD GO / TO,CIRCLECD,TO,PL1,PAST,LNDE GO / TO,LNDE,TO,PL1,PAST,LNEF GO / TO,LNEF,TO,PL1,TO,LNFG GO / TO,LNFG,TO,PL1,PAST,LNGA GO / TO,LNGA,TO,PL1,ON,LNAB GOTO / SP

59 Relative Motion Statement Point-To-Point (PTP) Motion GODLTA / coordinate increment Contouring Motion COMMAND / (TO) Drive Surface, TO/ON/PAST/TANTO, Check Surface Here, the command can be any one of the followings GOLFT GORGT GOUP GODOWN GOFWD GOBACK move left along the drive surface move right along the drive surface move up along the drive surface move down along the drive surface move forward from a tangent position move backward from a tangent position

60 Ex.8 Example. Assuming all geometric entities have been defined as shown in the figure and the hypothetical part plane is PL1, make a possible APT motion program to cut the part.

61 Solution. FROM / START GO / TO,L1,TO,PL1,ON,L3 GORGT / L1,TANTO,C1 GOFWD / C1,TANTO,L2 GOFWD / L2,PAST,L3 GOLEFT / L3,PAST,L1 GOTO / START Note: GOLFT and GORGT for next motion are relative to the direction of the current motion.

62 Miscellaneous Statements Macro is a set of instruction that can be repeatedly used. (i.e., subroutine in Fortran or function in C language) Ex. DRILL = MACRO GODLTA/0,0,-0.5 GODLTA/0,0,+0.5 TERMAC Looping can be programmed just like any other structured programming using LOOPST and LOOPND. PATTERN command defines a set of points and CYCLE command can perform manufacturing operations at those points Ex. Suppose a pattern of points has been defined in PTN2. Then, CYCLE/DRILL(, list of parameters) GOTO/PTN2 CYCLE/OFF

63 Ex.9 The following program shows how to drill holes in a certain pattern. RESERVE/PNT,6 LOOPST STARTY=3 (2,4) J=1 (2,3) (4,3) 4 I =1 STARTX=2 y 5 PNT(I)=POINT/STARTX,STARTY,1 (1,2) IF(I-3) 6,8,8 Hole depths are 0.5 x 6 I = I + 1 STARTX = STARTX + 2 JUMPTO/5 8 IF(J-2) 9,10,10 9 J = J + 1 STARTY = STARTY + 1 JUMPTO/4 10 LOOPND

64 Ex.10 Motion Commands for Milling The following part is to be machined by milling. The work piece is 4 x 5 x 1.6 inches and low-carbon steel. Assume the milling machine is 3-axis CNC.

65 Process Plan: 1.Set the lower left corner of the part as the machine zero-point. 2.Clamp the work piece in a vise. 3.Mill the slot with a ½ in four-flute flat end mill made of carbide. From the Machinability Data Handbook, the recommended feed is in/tooth/rev and recommended cutting speed is 100 fpm 4.Drill four holes with a 0.5-in-diameter twist drill. Use 0.18 ipr feed and 100 fpm speed.

66 Machining Specifications Despite the great deal of standardization through programming languages like APT and computer-assisted part programs, these standards are not so apparent in hardware as in software. As a result, the APT program has to be post-processed for a particular machine. Typical post-processor commands include: MACHIN/ calls a machine tool COOLNT/ coolant fluid can be turned on and off. FEDRAT/ feed rate is specified SPINDL/ spindle speed is specified TURRET/ call a specific tool from tool changer END forces to stop the machine so that the operator can change a tool manually or inspect the part.

67 Tolerance Setting Nonlinear motion along a curve is achieved by a set of continuous straight line segments. The tolerance statements dictate how many line segments to be generated for contouring motion. Either one or both may be specified. OUTTOL / INTOL / 0.001

68 CL Data to MCD CAD/CAM system effectively creates geometry (i.e., modeling) adds PMI (product manufacturing information) produces engineering drawings produces CL data in tool-path simulation by CAP programming like APT helps to convert CL data to machine control data (MCD) for machining in post-processing. MCD = NC control codes