|
|
A.CO-ORDINATE SYSTEM FOR A CNC LATHE
Machining of a work piece by an NC program requires a co-ordinate system to be applied to the machine tools. All machine tools have more than one slide, it is important that each slide is identified idividually. There are three planes in which movement can takes place.
Longitudinal
Vertical
Transverse
Each plane is assigned a letter and is referred to as an axes that is
Axes X
Axes y
Axes Z
The three axes are identified by upper case X, Y,X and a direction of movement along each axes is specifying as either PLUS(+) or MINUS(-). Z-axis is always parallel to the main spindle of the machine. The X-axes is always parallel to the work-holding surface and always at right angles to both Z & X-axes.
B. ZERO POINTS AND REFERENCE POINTS
On CNC machine tool traverses are controlled by co-ordinate system .There accurate position within the machine tool as established by "ZERO POINTS" as shown in figure—
MACHINE ZERO POINT(M):-
Is specified by the manufacturer of the machine.This is the zero point for co-ordinate systems and reference point of the m/c
On turning lathes, the m\c zero point as shown in the figure.The main spindle axes (center line) represents the Z- axes , the face determines the X- axes .The direction of the positive X and Z axes point toward the working area.When the tool traverses in the positive direction, it moves away from the workpiece.
REFERENCE POINT(R): - This point serves for calibrating and for controlling the measuring system of the slides and tool traverses. The position of the reference point is accurately pre determined in every traverse axes by the trip dogs and limit switches .Therefore, the reference point co-ordinates always have the same, precisely known numerical value in relation to the machine zero point.After initiating the control system , the reference point must always be approached from all axes to calibrate the traverse measuring system as, for example, through an electrical failure, the machine must again be positioned to the reference point to re-establish the proper positioning values.
WORKPIECE ZERO POINT (W): - The point determines the workpiece co-ordinate system in relation to the machine zero point. The workpiece zero point is chosen by the programmer and input into the CNC system when setting up the machine. The position of the work piece zero point can be freely chosen by programmer within the workpiece envelope of the machine. It is however, advisable to place the workpiece zero point in such a manner that the dimensions in the work piece drawing can be conveniently converted into co-ordinate values and orientation when clamping/chucking, setting up and checking, the traverse measuring system can be effected easily.
For turned parts, the workpiece zero point should be placed along the spindle axes(center line), in line with the right hand or left hand end face of the finished contour. Occasionally, the workpiece zero point is also called the ‘program zero point’.
TOOL POINT:- When machining a work piece, it is essential to able to control the tool point or the tool cutting edges in precise relationship to the work piece along the machining path.Since tools have different shapes and dimensions, precise tool dimensions have to be established beforehand and input into the control system.The tool dimensions are related to a fixed tool setting point during pre-setting.
NC RELATED DIMENSIONING
Dimensional information in work piece drawing can be started in two ways Absolute Dimension System and Incremental Dimension system
Data in absolute dimension system always refer to a fixed reference point in the drawings as shown. This point has the function of a coordinate zero point. The dimension lines run parallel to the coordinate axes and always start at the reference point . Absolute dimension are also called as ‘Reference dimension.’
ABSOLUTE DIMENSIONS ABSOLUTE CO-ORDINATES
ADVANTAGE OF ABSOLUTE DIMENSION SYSTEM
When using incremental dimension system, every measurement refers to a previously dimensioned position as shown in fig. Incremental dimension are distance between adjacent points. These distances are converted into incremental coordinates by accepting the last dimension point as the coordinate origin for the new point. This may be compared to a small coordinate system, i.e. Shifted consequently from point to point (p1.p2. Through p9) as shown in fig. Incremental dimensions are also frequently called ‘Relative dimension or Chain dimension’.
INCREMENTAL DIMENSIONS INCREMENTAL CO-ORDINATES
ADVANTAGES OF INCREMENTAL DIMENSION SYSTEM
A. MISCELLANEOUS FUNCTION (M-CODES)
M-codes are instructions describing miscellaneous functions like calling the tool, spindle rotation, coolant on etc.
M00 PROGRAM STOP
By inserting M00 in a program, the cutting cycle is stopped after the block containing M00 code. This facility is useful if an inspection check is necessary during an operation. The cycle is then continued by a cycle start.
M01 OPTIONAL STOP
Cycle operation is stopped after a block containing M01 is executed. This code is only effective when the optional stop switch on the machine control panel has been passed.
EXAMPAL M01
M02 PROGRAM END
This code is interested at the end of the program, when encountered the cycle will end. To produce another the system must be reset.
M03 SPINDLE FORWARD
Starts the spindle spinning forward, clockwise or negative direction at the last specified spindle rate.
Example: M03 S 1200
M04 SPINDLE REVERSE
Start the spindle spinning reverse, counter clockwise or positive direction at the last specified spindle rate
Example: M04 S 1000
M05 STOP SPINDLE
Stops the spindle without changing the spindle speed.
Example: M05
M06 TOOL CHANGE
The M06 in conjunction with "T" WORD is used to call up the required tool on an automatic indexing turret machine, and to activate its tool offsets. The left most digit of the "T" ignoring zeros selects the new tool. The tool changes are normally performed with the tool post at a safe position away from the work piece, so the code G28 REFERENCE POINT RETURN would be used in the block prior to M06.
Example: M06 T 0202
M08 COOLENT ON
This makes the coolant ON.
M09 COOLENT OFF
This turns the coolant OFF.
M10 CHUCK OPEN
This opens pneumatic or similar automatic chuck to allow for bar feed.
M11 CHUCK CLOSE
This closes the chuck.
M13 SPINDLE FORWARD COOLENT ON
Sets spindle rotation forward and coolant ON.
Example: M13 S1000
M14 SPINDLE REVERSE, COOLENT ON
Sets spindle rotation reverse and coolant ON.
Example: M14 S1000
M25 QUILL EXTEND
Extends the quill (tailstock)
M26 QUILL RETRACT
Retracts the quill (tailstock)
M30 PROGRAM END
Stops the spindle, Turns the coolant OFF Terminates and resets the CNC program.
M38 DOOR OPEN
Opens the door, waiting until the door is open.1
M39 DOOR CLOSE
Closes the door, waiting until the door is closed.
M62 SET OUT PUT 1 ON
M63 SET OUT PUT 2 ON
M64 SET AUXILIARY OUTPUT 1 OFF
M65 SET AUXILIARY OUTPUT 2 OFF
Codes M62 to M65 are assigned by the machine tool manufacturers to output a signal to a preferential device outside the machine tool. this could be for example, the initial signal to a system controlling a conveyor or robot arm billet loading system, feeding the machine tool as part of an integrated manufacturing system.
M66 WAIT INPUT 1 ON
M67 WAIT INPUT 2 ON
M76 WAIT INPUT 1 OFF
M77 WAIT INPUT 2 OFF
Above codes are assigned by the machine tool manufaturer to wait for a signal input form a preferential device indicating that the machine operation can commence.For example, a robot arm on correctly positioning the billet can signal for the CNC programming to commence.
|
G00 FAST TRAVERSE The rapid traverse instuction is identified by the program word G00. A rapid traverseinstruction traverses the tool to the target point at maximum traverse rate As supplementary functions it will be necessary to input the co-ordinates of the target point. The tool normally takes the shortest path from the starting point to the destination point. The tool path is determined by the non-linear interpolation type positioning. positioning is done separately with each axis. note:- the rapid traverse is used for movements where no tool is in engagement. G01 LINEAR MOTION In accordance with the established standards, the instuction "straight line at feed rate" requires the program word G01. the following supplementory function is also needed: Target point coordinates feed rate, spindle speed or cutting speed. G01 traverses the tool along a linear path to the given target point with the feed rate input as a supplementory function. When giving instructions G01, the coordinates of the distination point can be expressed using either absolute or incremental dimensions. CIRCULAR INTERPOLATION G02/G03 G02-Clockwise Direction G03-Counter clockwise direction Io and Ko can be omitted. If X (U) an Z (W) are both omitted or if the end point is located at the same position as the start point, and when the center is commanded by I and K, an are of 360° (a complete circle) is assumed. If I, K and R are specified simultaneously, the arc specified by address R takes precedence and the others are ignored. |
G04 DWELL
|
A Go4 Causes the program to wait for a specified amount of time. The time can be specified in seconds with the "X" or ‘U" prefixes or in milliseconds with the "P" prefix. During cutter motion, a deceleration at the end of the motion specified by one statement and an acceleration at the start of the specified by the next statement are usually applied by the NC controller. A GO4 code can be inserted between the two statements to make a sharp corner. |
G20 IMPERIAL
A G20 causes position to be as being in imperial units. All the best values are in inches. This can only be at the start of the main program.
G21 METRIC
A G21 causes positions to be interpreted as being in metric inches. All the input values are in mm. This can only be at the start of the main program.
G28 GO TO REFERENCE POINT
|
A G28 causes a fast traverse to the specified position and then to the machine datum. |
G28 X 30 Z15 G28 U 0 W0 |
COMPENSATE FUNCTION
Tool offset is used to compensate for the difference when the tool actually used differs from the imagined tool used in programming (usually, standard tool). During programming, a four digit number is programmed following the letter T, the first two digits represent the Tool number, and the second two digits represents the Tool offset number. Fig.18 illustrate the concept of Tool offsets.
TOOL GEOMETRY OFFSET AND TOOL WEAR OFFSET
With the option of tool geometry and wear compensation, it is possible to divide the tool offset for compensating the tool shape or mounting position to the geometry offset, and tool wear to the wear offset. The total value of the tool geometry offset and tool wear to the wear offset. The total value of the tool geometry offset and tool wear offset are set as the tool offset value if the tool geometry and wear compensation option is not equipped. Figs. 19 and 20 illustrate the method differentiation of tool geometry offset from tool wear offset.
TOOL NOSE RADIUS COMPENSATION (G40-42)
In turning operations on lathe, the positions and cutter path for contouring motion cannot be defined directly on the basis of the dimensions specified on a part drawing. The coordinates of the end position in each contouring motion statement of an NC program must be calculated. This calculation is time consuming and error prone. On modern CNC machines, special calculation functions or cutter-radius compensation codes are provided to allow a user to utilize part-profile coordinates obtainable from the part drawing to program a contouring motion. These are the G41 and G42 codes for tool radius compensation on the left- and right-hand sides of a profile, respectively. A left or right compensation is based on the fact the tool is on the left-or right-hand side when one goes along the part profile in the direction specified by the contouring motion statements in the program. A G40 code is provided to cancel the cutter-radius compensation. The tool nose radius compensation function together with the tool-offset function together with the tool-offset function automatically compensates for the error in cutting due to tool nose roundness. Fig. 21 illustrates the tool nose radius compensation.
The nose of a lathe cutter is only a section of a circle and does not rotate, like an end mill, during the cutting process. Therefore different cutter compensation vectors (or directions) must be applied with different types of cutting tools as shown in FIG. 22, which illustrates the relationship between the tool and the start point. The end of the arrow is the imaginary tool nose. The direction of the imaginary tool nose viewed from the tool nose center is determined by the direction of the tool motion during cutting; this is set in advance with the offset values. Imaginary tool nose numbers 0 and 9 are used when the tool nose center coincides with the start point.
The tools installed on the turret have different relative positions with respect to the turret center. To compensate for these differences, one should set the offsets in the X and Z directions for different tools . The number of pairs of offsets is restricted to the number of tools.
G50 CO-ORDINATE SETTING
G50 enables tool nose radius compensation to the left of the programmed path. G50 has 2 uses. Coordinate setting block has "X", "Z", "U" OR "W" upon it. A maximum spindle speed block does not.
G50 CLAMP SPINDLE
G50 sets the maximum spindle speed for constant surface control. An "X","Z", "U" or "W" prefix must not be on the block or it will be interpreted as a coordinate setting block.
Example: G50 S2000
G50 creates a new coordinate system in which the tools current position is set to the specified coordinates. The new coordinates can be in absolute or incremental form.
Example: G50 XO ZO
And G50 U-40
G96 CONSTANT SURFACE SPEED
The cutting speed during turning is the peripheral speed of the work. The peripheral speed of a rotating work represents the peripheral path in a given unit time. The peripheral speed or cutting speed is thus the fully stretched chip length produced in one time. The cutting speeds vary in direct relation to the diameters, even if the number of revolutions per minute is the same in all cases.
The correct selection of the cutting speed for turning is very important.
Cutting speed too low: Time loss and low surface finish. With increasing cutting speed the surface speed is improved.
Cutting speed too high: High tool wear.
The advantage of the CONSTANT SURFACE SPEED can be evident through a parting operation. During parting operation, the diameter of the work where cutting is taking place is steadily decreasing. The cutting efficiency can only be maintained if the spindle speed is increased at a corresponding rate so the speed where the cutting is taking place is constant. This operation however may not be critical enough to warrant the need for the C.S.S. facility. A complex component with turned profiles requiring a uniformly high surface finish would demand the use of the C.S.S. facility.
NOTE: When constant surface speed control is used, the work coordinate system must be set so that the center of rotation meet the Z-axis (X=0).
Example: G96 S100
Sets the surface speed to 100 meters a minute.
G97 NORMAL SPINDLE SPEED
G97 cancels constant surface speed. The spindle speed will not change until the next "S" value is reached.
Example: G97
G98 FEED PER MUNUTE
This command coupled with the F word is used to specify federate per minute. This can be in either mm/min or inch/min. This is the default.
Note: The DENFOED FANUC simulation will default to G98 and this is modal and will remain active until G99 (Feed per revolution) is entered.
G99 FEED PER REVOLUTION
This command coupled with the F word is used to specify a federate per revolution. This can be in mm/rev or inch/rev. The feedrates available in the DENFORD FANUC simulation are 0.01-200 mm/min. Recommended federates are published by tool and cutter manufacturers, along with recommended cutting speeds. If the feed rate is expressed as mm/rev. a simple calculation can be used to convert to mm/min.
Feed, mm/min = Feed (mm/rev) X Spindle speed (r.p.m)
PROGRAM FOR SIMPLE FACING OPERATION
DWG NO. 1
(Drawing NO: 1
(CNC program for simple facing
(Material to be removed by facing 2mm.
(GO1 Linear interpolation
01001 Program Number 1001
[BILLET X20 Z60 Defining Billet size Dia: 20mm length 60mm
G21 G40 G98 Initial settings.
G28 UO WO Going to Home Position
M06 T0101 Selecting Tool No. 1
M03 S1200 Setting spindle speed at 1200 rpm
G00 X20 Z1 Tool moving to tool entry point X20 Z1 at rapid traverse
G01 Z-0.5 F45 Giving depth of cut of 0.5mm at a feed rate of 45 mm/min.
G01 X0 Moving the tool to spindle centerline.
G01 Z1 Moving the tool to spindle centerline.
G00 X20 Moving the toll to X20
G00 Z-1 Giving second depth of cut
G01 X0 Moving the tool to spindle centerline.
G01 Z1 Retract back the too.
G00 X20
G00 Z-1.5
G01 X0
G01 Z1
G00 X20
G00 Z-2
G01 X0
G01 Z1
G00 X20
G28 U0 W0 Going to home position
M05 Stop the spindle
M30 Program stop and rewind.
PROGRAM FOR SIMPLE TURNING OPERATION
(Program for simple turning, Reducing the diameter from 20 mm to 14 mm
[BILLET X 20 Z60 Defining Billet size. Dia: 20, length 60 mm
G21G40 G98 Initial settings.
G28 U0W0 Going to home position
M06 T0101 Selecting tool no. 1 with offset no. 1
M03 S1200 Setting spindle speed a t1200 rpm.
G00 X20 Z1 Tool moving to tool entry point.
G00 X 19
G01 Z-30 F45
G01 X20
G00 Z1
G00 X18
G01 Z-30
G01 X20
G00 Z1
G00 X17
G01 Z-30
G01 X20
G00 Z1
G00 X16
G01 Z-30
G01 X20
G00 Z1
G00 X15
G01 Z-30
G00 X20
G00 Z1
G28 U0 W0 Go to home position.
M05 Stop the spindle
M30 Program stop and rewind
PROGRAM FOR LINEAR AND CIRCULAR CONTOUR OPERATION
DWG NO.3
(Drawing No: 3
(Program for linear and circular interpolation
(G01 – Linear interpolation
(G02 – Clockwise circular interpolation
(G03 – Anti-clockwise circular interpolation
01003 Program number 1007
BILLET X 40 Z60 Defining Billet size Dia: 40mm length 60 mm
G21 G40 G98 Initial settings
G28 U0 W0 Going to home position
M06 T0101 Selection Tool No. 1 with offset no. 1
M03 S1200 Setting spindle speed at 1200 rpm
G00 X40 Z1 Tool moving to tool entry point at rapid rate.
G00 X5
G01 X10 Z-10 F45
G01 W-5
G02 X25 Z-25 R10 F25 CLOCKWISE INTERPOLATION – G02
G01 Z-30 F45
G03 U10 Z-37 R10 F25 COUNTER CLOCKWISE INTERPOLATION – G03
G01 Z-42 F45
G01 X40 Z-47
G01 Z-52
G28 U0 W0 Going to home position
M05 Stop the spindle
M30 Program stops and rewind.
G94 FACING CYCLE
|
Facing Cycle – G94 |
Command |
|
A G94 a ‘BOX Type’ cutting cycle. This cycle is used for stock removal either parallel or at an angle to work peace. It is the equivalent of rapid to Z position, feed to X position, feed to start Z position, and rapid to start X position. If an "R" value is specified tapering will be performed. The sign of ‘R’ depends on direction of the taper. The initial rapid move will be to the Z position plus "R" value. As canned cycles are modal, to repeat the cycle for removing further material only the value in the axis to be moved needs to be changed. |
G94 X (U) Z(W) F G94 X(U) Z(W) R – F G94 X(U) Z (W) R+F Where X = Dieameter to which the movement is being made. U = The incremental distance form the current tool position to the required final diam Z = The Z co-ordinate to which the movement is being made. W = The incremental distance from the current tool position to the required Z axis position. R = The difference in incremental of the cut start radius value and the cut finish radius value. Example: G94 U-40 W-2.0 R-8 F1400 W-3.0 W-4.8 |
PROGRAM FOR BOX FACING OPERATION
(Drawing No: 4
(Program for facing Cycle
(G94 – Box facing cycle
01004 Program number 1005
[Billet X20 Z60 Defining Billet size Dia: 20 mm length 75 mm
G21 G40 G98 Initial settings.
G28 U0 W0 Selecting tool no. 1 with offset no.1
M06 T0101 Selecting spindle speed at 1200 rpm
G00 X21 Z0 Tool moving to tool entry point at rapid rate
G94 X10 Z-0.5 F35 G94 BOX FACING CYCLE
G94 CODE SYNTAX. G94 X Z F
Z-1
Z-1.5
Z-2
Z-2.5
Z-3
Z-2.5
Z-3
Z-3.5
Z-4
Z-4.5
Z-5
G00 Z21 Z-5
G94 X14 Z-5.5 F35 G94 BOX FACING CYCLE
Z-6
Z-6.5
Z-7
Z-7.5
Z-8
Z-8.5
Z-9
Z-9.5
Z-10
G28 U0 W0 Going to home position
M05 Stop the spindle
M30 Program stops and rewind
PROGRAN FOR TAPER FACING OPERATION
DWG NO. 5
(Drawing no: 5
(Program for Taper Facing Cycle: G94 R-
01005 Program number 1005
(Billet X20 Z60 Defining Billet size Dia: 20mm length 60 mm
G21 G40 G98 Initial settings
G28 U0 W0 Going to home position
M06 To 101 Selecting tool no.1 with offset no.1
M03 S1200 Setting spindle speed at 1200 rpm.
G00 X21 Z0 Tool moving to tool entry point at rapid rate
G94 X 10 Z-0.5 F35 G94 FOR FACING CYCLE
Z-1
Z-1.5
Z-2
Z-2.5
Z-3
Z-3.5
Z-4
Z-4.5
Z-5
Z-5.5
Z-6
Z-6.5
Z-7
Z-7.5
Z-8
Z-8.5
Z-9
Z-9.5
Z-10
G28 U0 W0
M06 T0202 USING LEFT HAND TOOL
M03 S1000
G00 X21 Z-5
C94 X20 Z-10 R-10 F30 TAPER FACING CYCLE G94 R-
X18
X17
X16
X15
X14
X13
X12
X11
X10
G28 U0 W0 Going to home position
M05 Stop the spindle.
M30 program stop and rewind.
72 MULTIPLE FACING
|
This Multiple Facing cycle is used when the major direction of cut is along the – ‘X’- axis. This cycle causes the profile to be roughed out by facing Control passes on to after the last block of the profile. Two G72 blocks are needed to specify all the values. Example: G72 W2.0 R1.5 G72 P10 Q20 U1.0 W1.0 |
G72 W (*w1) R (*r) G72 P (*p) Q (*q) U (*u2) W (*w2) F (*f) S (*s) T (*t) Where, (w1 = depth of cut in the Z axis *r = escape or relief amount *p= the line number in the program marking the start of the finished form required. *q = the line number in the program marking the end of the finished form required. *u2 = the amount and direction of the finishing allowance left in the X-axis. *w2 = the amount and direction of the finishing allowance left in the Z-axis. *f = feed rate, *s = speed, *t = tool number |
NOTE: The values of F, S or T contained in the data blocks for the profile are ignored when G72 line read and the F, S or T in that line is acted upon.
PROGRAM FOR MULTIPLE FACING OPERATION
(Drawing No. 6
(Program for multiple facing
(Multiple facing cycle – G72
01006 Program number 1006
[Billet X40 Z60 Defining Billet size Dia:40mm length 60 mm
G21 G40 G98 Initial settings
G28 U0 W0 Going to home position
M06 To 101 Using RH Roughing Tool
Selecting tool no.1 with offset no. 1
M03 S1200 Setting spindle speed at 1200 rpm.
G00 X 40 Z1 Tool moving to tool entry point at rapid rate
(Multiple facing cycle – G72
(Depth of cut for each pass W 0.5 mm
(Relief amount R = 0.5 mm
(Allowances on X and Z axes = 0.1 mm respectively.
(P and Q: Beginning and end of cycle sequence Nos.
(Feedrate F – 35 mm/min.
G72 W0.5 R0.5
G72 P10 Q20 U0.1 W0.1 F35
N10 G01 Z-52
G01 X40
G01 Z- 47
G01 X35 Z-42
G01 Z-37
G02 X25 Z-30 R10 F25
G01 Z-25 Z-30 R10 F25
G01 X10 Z-15 F35
N20 G01 X5 Z0
G28 U0 W0
M06 T0202 Using LII Finishing Tool
M03S1450
G00 X21 Z1
G70 P10 Q20 F25 Finishing cycle
G28 U0 W0 Going to home position
M05 Stop the spindle
M30 Program stop and rewind.
G90 Single Turning Cycle
This cycle can be used to produce either a parallel or tapered tool path. This cycle perform four distinct moves with one line of information and. It is the equivalent of
|
Parallel Turning – G90 |
Command |
|
With the above command, the cycle will execute removing material to the required diameter and length. To repeat this cycle to reduce the diameter but maintain the same length, only the value to be changed needs to be programmed. |
G90 X(U) Z(W) F(*f) Where, X= Diameter to which the movement is being made. U = The incremental distance from the current tool position to the required final diameter. Z = The Z axis Co-ordinate to which the movement is being made. W = The incremental distance from the current tool position to the required Z axis position. F = feed Example: G90 X30 Z-25 F0.4 X25 X20 |
PROGRAM FOR STEP TURNING OPERATION USING G90 CYCLE
20 15 15
DWG NO. 7
(Drawing No: 7
(Program for step Turning
(G90 – Box Turning cycle
O0007 Program number 1003
[Billet X20 Z60 Defining Billet size Dia: 20 mm length 60 mm
G21 G40 G99 Initial settings
G28 U0W0 Going to home position.
M06 To 101 Selecting Tool no.1 with offset no.1
M03 S1200 Setting spindle speed at 1200 rpm
G96G00 X20 Z1 Using constant surface speed – G96
Tool moving to tool entry point at rapid rate
G90 X19 Z-30 F30 G90 Box turning cycle code syntax : G90 X Z F
X18
X17
X16
X15
X14
G00 X14 Z1
G90 X13 Z-15
X12
X11
X10
G28 U0 W0 Going to home position
M05 Stop the spindle
M30 Program stop and rewind
G90 TAPER TURNING
|
If an "R" value is specified in the command format of G90 cycle, tapering will be performed. The sign of ‘R’ will depend on the direction of the taper. The initial rapid move will be to the X position plus the "R" value. |
G90(U) Z(W) R F Where, X= Diameter to which the movement is being made U= The incremental distance from the current tool position to the required final diameter. Z = The Z axis co-ordinate to which the movement being made. W = The incremental distance from the current tool position to the required Z-axis position. R = The difference in incremental of the cut start radius value and the cut finish radius value. Example: N100 G00 X44 Z2 N110 G90 X36 Z-20 R-2 F3 |
NOTE: When programming in incremental ‘U’ and ‘W’ must be signed always, in either absolute or incremental.
PROGRAM FOR TAPER TURNING OPERATION
54
DWG NO.8
(Drawing No: 8
(Program for Taper turning G90 R & G90 R+
O100 8 Program Number 1008
[Billet X20 Z75 Defining Billet size
Dia: 20 mm length 75 mm
G21 G40 G98 Initial setting
G28 U0W0 Going to Home position
M06 To 101 Selecting spindle speed at 1200 rpm
G00 X 20 Z1 Tool moving to tool entry point at rapid rate
G90 X 19 Z-9.5 F35 Step Turning Using G90
X18
X17 Z-6
X16
X15
X14
X13
X12
X11
X10
X9
G00 X 18 Z
G90 X 18 Z-21 R0 F30
X18 R-0.5
X18 R-1
X18 R-1.5
X18 R-2 R = (D1 – DF) / 2
X18 R-2.5 D1-Intial Diameter
X18 R-3 DF – Final Diameter
X18 R-3.5
X18 R-4
X18 R-4.5
G01 X18 Z-33
G90 X18 Z-48 R0 F30 Taper Turning – G90 R +
X17 R0.5
X16 R1
X15 R1.5
X14 R2
X13 R2.5
X12 R3
X11 R3.5
X10 R4
X9 R4.5
G00 X18 Z-48
G90 X18 Z-54 F30 Box Turning Using G90
X17
X16
X15
X14
X13
X12
X11
X10
X9
G28 U0 W0 Going to home position
M05 Stop the spindle
M30 Program stop and rewind.
G70 FINISHING CYCLE
|
On completion of roughing out operation using cycles G71, G72 or G76, the material left as a finishing allowance is removed using the finishing cycle is the same programming lines that the roughing cycle is based on. A G70 cycle causes a range of blocks to e executed, and then control passes to the block after the G70. |
N40 G71 U(*u)1 R(*r1) N50 G71 P60 Q120 U(*u2) W(*w2) F(*f) S(*s) N130 G70 P60 Q120 The ‘P" and ‘Q’ values specifies the ‘N’ block numbers at the start and end of the profile. |
G71 MULTIPLE TURNING
|
This multiple turning cycle is used when the major direction of cut is along the ‘Z’ axis. This cycle causes the profile to be roughed out by turning. Control passes on to after the last block of the profile. Two G71 blocks are needed to specify all the values. |
G71 U (*ul) R (*r) G71 P (*p) Q (*q) U (*u2) W (*w2) F (*f) S (*s) T (*t) Where, *ul = depth of cut (Radios designation) *R = relief amount *p = Line or block number of the start of the final profile *q = Line or block number of the end point of the final profile *u2 = Finishing allowance in the X axis *w2 = finishing allowance in the Z axis *f = feed rate *s = speed *t = tool number |
Note: The values of F, S or T contained in the data clocks for the profile are ignored when G71 line read and the F,S or T in that line is acted upon.
PROGRAM FOR MULTIPLE TURNING OPERATION
5 5 5 7 5 10 5 10
DWG NO. 9
(Drawing No. 9
(Program for multiple turning operation – G71
(G70-Finishing Cycle
O1009 Program Number 1009
[Billet X40 Z60 Defining Billet size Dia: 40 mm length 60 mm
G21 G40 G98 Initial settings
G28 U0 W0 Going to Home position
M06 To 101 (Using RH Roughing Tool
Selecting Tool No. 1 with offset No.1
M03 S1200 Setting spindle speed at 1200 rpm
G00 X40 Z1 Tool moving to tool entry point at rapid rate
(G71 Multiple Turning
(Depth of cut for each pass U = 0.5 mm
(Relief amount R = 1.0 mm
(P and Q: Beginning and end of cycle sequence Nos.
(Allowances on X(U) and Z(W) axes = 0.1 mm respectively.
(Feedrate = 35 mm/min.
G71 U0.5 R1
G71 P10 Q20 U0.1 W0.1 F35
N10 G01 X5
G01 Z0
G01 X10 Z-10
G01 Z-15
G02 X25 Z-25 R10
G01 Z-30
G03 X35 Z-37 R10
G01 X40 Z-47
N20 G01 Z-52
G28 U0 W0
M06 T0202 Using RH Finishing Tool
M03 1450
G00 X20 Z1
G70 P10 Q20 F25 Finishing cycle
G28 U0 W0 Going to home position
M05 Stop the spindle
M30 Program stop and rewind
G73 PATTERN REPEATING
|
This cycle provides for roughing out of a form by repeating the desired tool path a set number of times, the too path being incremented into the workpiece until the full form is completed. This cycle is particularly useful which machining castings or forgin, which are already formed to the basic shape, required. Two G73 blocks are needed to specify all the values. Example: G73 U3 W4 R5 G73 P1 Q2 U3 W4 F0.1 S1500 |
G73 U(*u1) W(*w1) R(*r1) G73 P(*p) Q(*q) U(*u2) W(*w2) F(*f) S(*s) T(8t) *u1 = d of relief amount in the X axis *w1 = distance and direction of relief amount in the Z-axis the number of divisions. *p, *q = the line numbers in the program marking the start and finish of the finished form required. (u2 = the amount and direction of the finishing allowance in the X axis *w2 = the amount and direction of the finishing allowance in the Z axis *f = feed rate *s = speed *t = tool number |
Note: The values of F, S or T values can be different than the F,S and T values set in the profile line P and Q.
PROGRAM FOR SIMPLE FACING OPERATION(PATTERN REPETING CYCLE)
R30
10 20 20 10
DWG NO. 10
(Drawing No:10
(Program for pattern repeating cycle – G73
O1010 Program Number 1010
[Billet X34 Z70 Defining Billet: size Dia: 34 mm length 70 mm
G21 G40 G98 Initial settings
G28 U0 W0 Going to home position
M06 T0101 Using RH Roughing Tool
Selecting Tool No. 1 with offset no.1
M03 S1200 Setting spindle speed at 1200 rpm.
G00 X34 Z1 Tool moving to tool entry point at rapid rate
G71 P10 Q20 U0 W0 F35 Which pattern repeating cycle is used
N10 G01 X10
Z-10
X26 Z-30
G02 X32 Z-50 R30
N20 Z-60
G28 U0 W0
M06 T0202
M03 S1450
G00 X15 Z1
G73 U0.75 W0.0 R4 PATTERN REPEATING CYCLE
G73 P100 Q200 U0.1 F35
(Distance and direction of relief along X and Z axes, U and W: 0.75 and 0mm resp.
(No. of divisions, R = 4
(Allowances on X and Z axes U, W = 0.1 mm respectively.
(P and Q : Beginning and end of cycle sequence Nos.
G01 X8
Z-10
X24 Z-30
G02 X30 Z-50 R30
N200 Z-60
S1450
G00 X15 Z1
G70 P100 Q200 F25 Finishing Cycle
G28 U0 W0 Going to home position
M05 Stop the spindle
M30 Program stop and rewind.
G74 GROOVING IN AXIS
|
This cycle is designed for outer Diameter/Inner diameter drilling, The drill entering the workpiece By a predetermined amount then Backing off by another set amount to provide breaking and Allowing war clear the drill flutes. Two distinet lines of data command the cycle. |
G75 R(*r) G75 X(u) Q(8q) F(*f) Where, *r1 = return amount x = total depth along X axis (absolute) u = total depth along X-axis (incremental) (q = depth of cut (incremental unsigned) *f = feedrate. Example: G75 R1.0 G75 X0 Q5000 F100 |
PROGRAM FOR EXTERNAL GROOVING OPERATION
38
10
3
2 5 2 22
DWG NO. 11
(Drawing No:11
(Program for Grooving
(G codes used G81 & G75
(Diameter Drilling cycles
O1011 Program number 1011
Billet X20 Z60 Defining Billet size Dia: 20mm length 60 mm
G21 G40 G98 Initial settings
G28 U0 W0 Going to home position
M06 T0101 (Using RH roughing tool
Selecting tool no.1 with offset no.1
M03 S1200 Setting spindle speed at 1200 rpm
G00 X20 Z1 Tool moving to tool entry point at rapid rate
G71 U.5 R1 Multiple Turning
G71 P10 Q20 U.1 W.1 F45
N10 G01 X9
X10 Z-1
Z-22
X18 Z-29
N20 Z-45
G28 U0 W0
M06 T0202
M03 S1450
G00 X19 Z-22
G70 P10 Q20 F25 Calling Finishing Cycle
G28U0W0 Grooving operation using G81 cycle
M06 T0505 Calling 2mm grooving tool.
M03 S750
G00 X19 Z-22
G81 X18.5 F15
X18
X17.5
X17
X16.5
X15
X14.5
X14
X13.5
X13
X12.5
X12
X11.5
X10
X10.50
X9.5
X9
X8.5
X8
G00 X18
G00 X18 Z-33
G75 R1 GROOVING USING G75 CYCLE
G75 X8 W-5.0 P1500 Q250 R0 F15
(Relief amount, R = 1.0 mm
(Depth of Groove, X = 5mm
(Width of groove, W = 5.0 mm
(Stepping distance along Z axis Q = 0.25 mm
G28 U0 W0 Going to home position
M05 Stop the spindle
M30 Program stop and rewind.
G92 SINGLE THREADING CYCLE
|
This is a Box Type cycle producing a single pass of the threading tool. The position specified is that of the end of the thread. The ‘F’ value specifies the pitch, NOT the feed. |
G92 X(*u1) Z (*w1) F(*f) Where, X = Depth of cut (absolute) *u1 = Depth of cut (incremental) Z = Length of thread (absolute) *w1 = Length of thread (incremental) *f = Lead or pitch of thread. Example: G00 X32 Z5 G92 X20.977 Z-20 F2.5 X19.955 X18.932 |
PROGRAM FOR EXTERNAL SIMPLE THREADING OPERATION
60
M12*
1.25P
19
10 10 10 10 20
DWG NO. 12
(Drawing No:12
(Program for Threading
(G92-Box Threading Cycle
O1012 Program Number 1012
[Billet X20 Z60 Defining Billet size Dia:20 mm length 60 mm
G21 G40 G98 Initial settings
G28 U0 W0 Going to home position
M06 T0101 (Using RH Roughing Tool selecting Tool No.1 with offset No.1
M03 S1200 Setting spindle speed at 1200 rpm
G00 X20 Z1 Tool moving to tool entry point at rapid rate.
G71 P10 Q20 U0.1 W0.1 F35
N10 G01 X11
X12 Z-1
Z-20
G02 X16 Z-30 R15
G01 Z-40
G03 X20 Z-50 R15
N20 G01 Z-60
G28 U0 W0
M06 T0202
M03 S1450
G00 X21 Z1
G70 P100 Q200 F25
G28 U0 W0
M06 T0505 Calling 2mm width grooving tool
M03 S800
G00 X12 Z-20
G81 X11.5 F30 Grooving operation
X11
X10.5
X10
X9.5
G28 U15 W0 Box threading cycle – G92
M06 T0707 Calling Threading Tool
G00 X12 Z2
G92 X11.5 Z-19 F1.75
(Successive core diameter X = 11.5mm
(Length of thread, Z= 19mm, Pitch of thread, F = 1.75 mm
X11
X10.5
X10
X9.83
G28 U0 W0 Going to home position
M05 Stop the spindle
M30 Program stop and rewind.
G76 MULTIPLE THREADING CYCLE
|
This is a ‘BOX TYPE’ cycle that is repeated a given number of times. After the first pass subsequent passes cut with one edge of the threading tool only to reduce the load at the tool tip. This cycle requires two distinct blocks of data. When the cutting depth of one cycle becomes smaller than the limit, the actual amount of cut is clamped at the minimum cut depth. |
G76 P(m) (-r) (a0 Q(*q1) R(8r1) G76 X(*x) Z(*z) P(*p2) Q(*q2) F(*f) Where, M = Repetitive count in finishing (1 to 99) R = Chamfering amount (0.01 to 9.91, where 1 is the thread’s lead) A = Angle of tool tip (80° , 60° , 55° , 30° , 29° and 0° ) *x = Finished Depth of Thread *z = End position of thread *p2 = Height of the thread as a radius value x 1000, as the controller accepts this value in microns. e.g. lead 1.5 – F1.5 *q1 = Min cutting depth, *u = Finishing allowance Example: G76 P031560 Q150 R0.5 G76 X17.96 Z-50 P1020 Q250 F1.5 |
PROGRAM FOR EXTERNAL THREADING(MULTIPLE)
60
M12*1.25P
10 10 10 10 20
DWG NO. 13
(Drawing No: 13
(Program for Multiple Threading
(G76 – Multiple threading cycle
O1013 Program number 1013
[Billet X20 Z60 Defining Billet size Dia: 20mm length 60mm
G21 G40 G98 Initial settings
M06 T0101 Going to home position
M0 T0101 Using RH Roughing tool,
Selecting tool no.1 with offset no.1
M03 S1200 Setting spindle speed at 1200 rpm
G00 X20 Z1 Multiple Turning
G71 P10 Q20 U0.1 W0.1 F35
N10 G01 X11
X12 Z-1
Z-20
G02 X16 Z-30 R15
G01 Z-40
G03 X20 Z-50 R15
N20 G01 Z-60
G28 U0 W0
M06 T0202 Calling RH Finishing tool
M03 S1450
G00 X21 Z1
G70 P100 Q200 F25 Finishing Operation
G28 U0 W0
M06 T0505 Calling 2mm width grooving tool
M03 S650
G00 X12 Z-20
G81 X11 F25 Grooving operation – G81
X10
X9
G28 U10 W0
M06 T0707 Calling threading tool
G00 X12 Z3
G76 P031560 Q250 R0.15 G76 –Multiple threading cycle
G76 X9.853 Z-19 P1073 Q300 F1.75
(03 = Number of passes for finishing operation
(15 = Chamfer amount in microns
(60 = Angle of the thread, deg.
(Q = minimum cutting depth = 0.25 mm, R = Finishing allowance = 0.15 mm
(X = Core diameter = 9.853 mm for M12, Z = Length of thread = 19 mm
(P = Height of thread = 1.073 mm ,Q = Depth of cut for first pass = 0.3 mm
(F = Pitch of the thread = 1.75mm
G28 U0 W0 Going to home position
M05 Stop the spindle
M30 Program stop and rewind.
G74 END FACK PECK DRILLING
|
This cycle is designed for deep hole drilling the drill entering the work piece by a predetermined amount then backing off by another set amount to provide breaking and allowing swarf to clear the drill flutes. The cycle is commanded by two distinct lines of data. |
G74 Z(W) Q*q) R(*r2) E(*f) Where, *r1 = Return amount Z = Total depth (absolute) W = Total depth (incremental) *q = Depth of cut (incremental) *q = Depth of cut (incremental, unsigned) *r2 = Relief amount of tool at the bottom of the hole produced, for drilling this value is ZERO. *f = Feedrate Example: G74 R1.0 G74 Z – 40 Q5000 R0.5 F100 |
PROGRAM FOR PEAK DRILLING OPERATION
35
40
DWG NO.14
(Drawing No: 14
(Program for drilling operation – G74 cycle
O1014 Program number 1014
[Billet X30 Z60 Defining Billet size Dia:30mm length 60mm
G21 G40 G98 Initial settings
G28 U0 W0 Going to home position
M06 T0808 Using 12 mm drill with toll No.8 and offset No.8
M03 S500 Setting spindle speed at 500 rpm
G00 X0 Z2 Tool moving to tool entry point at rapid rate.
G74 R1.0
G74 X0.0 Z-35 P0 Q500 R0 F20
(R = Relief amount = 1.0 mm
(X,Z = Position of the bottom of the hole 0,-35
(P = Stepping distance in X axis = 0 , Q = Depth of cut for each pass = 0.5 mm
(R = Relief amount for the tool at the bottom of the
G28 U0 W0 Going to home position
M05 Stop the spindle
M30 Program stop and rewind
PROGRAM FOR STEP BOARING OPERATION
DWG NO. 15
(Drawing No: 15
(Program for internal operation
(G74- Face Drilling Cycle
(G90- For step Boring
O1015 Program Number 1015
[Billet X30 Z50 Defining Billet size Dia: 30mm length 50mm.
G21 G40 G98 Initial settings
G28 U0 W0 Going to Home position
M06 T0808 Using 12 mm drill with tool No. 8 and offset No. 8
M03 S700 Setting spindle speed at 700 rpm
G00 X0Z0 Tool moving to tool entry point at rapid rate
G74 X0 Z-35 P0 Q500 R0 F15
(R = Relief amount = 1.0 mm
(X,Z = Position of the bottom of the hole (0.35)
(P = Stepping distance in X axis = 0
(Q = Depth of cut for each pass = 0.5 mm
(R = Relief amount for the tool at the bottom of the hole. = 0.0 mm
G28 U0 W0
M06 T0101 Calling 10 mm Dia: Boring Tool
M03 S800
G00 X12Z1
G90 X13 Z-30 F20 Internal boring using G90
X14
X15
X16 Z – 20
X17
X18
X19
X20
G28 U0 W0 Going to home position
M05 Stop the spindle
M30 program stop and rewind.
PROGRAM FOR BOARING OPERATION
9 25 20 5 12 8
DWG NO.16
(Drawing No;16
(Program for internal operation
(G71- For Boring operation
O1016 Program number 1016
[Billet X50 Z100 Defining Billet size Dia: 50mm length 100
G21 G40 G98 Initial settings
G28 U0 W0 Going to home position
M06 T0808 Using 12 mm drill with tool No.8 and offset no.8
M03 S700 setting spindle speed at 700 rpm
G0-0 X0 Z0 Tool moving to tool entry point at rapid rate
G74 R1 Calling peck drilling cycle – G74
G74 X0 Z-19 P0 Q500 R0 F15
(R – Relief amount = 1.0mm
(X,Z = Position of the bottom of the hole 0,-79
(P = Stepping distance in X axis = 0
(Q = Depth of cut for each pas 0.5 mm
(R = Relief amount for the bottom
G28 U0 W0 Go to home position
M06 T0101 Boring tool 10 mm Diameter
M03 S800
G00 X12 Z1
G71 U.5 R1
G71 P10 Q20 U0 W0 F20
N10 G01 X50
G02 X40 Z-8 F15
G01 Z20 F20
G03 X30 Z-25 F15
G01 X22 Z-45 F20
G01 Z-70
N20 X12
G70 P10Q 20 Calling finishing cycle
G28 U0 W0 Going to home position
M05 Stop the spindle
M30 Program stop and rewind.
SUBPROGRAM CALL/EXIT –M98/M99
|
Main Program |
Subprogram |
|
A program is divided into a main program and subprogram. Normally the CNC operates according to the main program but when a command calling a subprogram is encountered in the main program control is passed to the subprogram. When a command indicating to return to the main program is encountered in the subprogram control is returned to the main program. The first block of program subroutine must contain a program number "O". |
When a program contains certain certain fixed sequences or frequently repeated patterns, these sequences or patterns may be entered into memory as a subprogram to simply programming. A subprogram can call another subprogram. When the main program call a subprogram. It is regarded as a one-loop subprogram call. Format: O0001: |
PROGRAM USING SUB ROUTINE
20
14
10
20 15 15
(Drawing No:17
(Parting off operation
(M98 – Subprogram Call , M99 – Subprogram Exit
O1017 Program number 1017
[Billet X20 Z60 Defining Billet size Dia: 20 mm length 60 mm
G21 G40 G98 Initial settings
G28 U0 W0 Going RH Roughing tool
M06 T0101 Using RH Roughing tool
M03 S1000 Selecting tool no.1 with offset no.1
G00 X20 Z1 Setting spindle speed at 1200 rpm
Tool moving to tool entry point at rapid rate
M98 P0101000 Calling subprogram for turning
G00 X20 Z15
M98 P0061000
Parting – off operation
G28 U0 W0
M06 T0505
M03 S750 Calling grooving tool with 2mm width
G00 X21 Z1
M98 P421001 Subprogram ‘1001’ 42 times.
G28 U20 W0 Going to home position
M05 Stop the spindle
M30 Program stop and rewind
O1000
G90 U-1 W-15 F45 Subprogram for turning
G01 U-1
M99
O1001
G01 U-1 F25 Subprogram for parting
M99
REFERENCES
1. M-TAB DENFORD
2.CNC PROGRAMING
BY: KRAR