Each of the combinations, 1 and 2, are a group of 3 different colors to distinguish the characters displayed.
2.5. Cancellation of the MONITOR DISPLAY In any of the Modes of Operation of the CNC, it is possible to blank the MONITOR out. First of all, it is necessary to press the key To restore the display just press any key. In this case, the STOP key running of the CNC. , in addition to recovering the last display, stops the possible and then the key.
The display is also recovered when a message is received from the PLC64 or from the PLCI. 2.6. FUNCTION KEYS (SOFT KEYS) The CNC has 7 function keys (F1/F7), placed under the screen, which allow the user to operate with the CNC comfortably and quickly. Their meaning will be displayed on the screen just above the corresponding function keys and will be different in each of the situations and modes of operation. Throughout the manual the meaning of the F1/F7 keys which must be pressed in each case, will be indicated in square brackets [].

3. OPERATING MODES

The CNC has 10 different operating modes: 0. AUTOMATIC : Execution of programs in a continuous cycle. 1. SINGLE BLOCK : Execution of part programs block by block. 2. PLAY-BACK : Creation of a program in memory while the machine is being operated manually. 3. TEACH-IN : - Creation and execution of a block without entering it into memory. - Creation, execution and entering of a block into memory; thus a program is created while being executed block by block. 4. DRY RUN : To check programs before actual execution of the first part. 5. JOG/HOME SEARCH : - Manual movement of the machine. - Machine-reference. (Home search). - Presetting of any value and zero-setting the axes. - Entering and executing of F,S,M. - Setting initial conditions of the tool magazine. - Handwheel operation.
6. EDITING Creation, modification and checking of blocks, programs and subroutines. 7. INPUT-OUTPUT Transferring programs or machine-parameters from/to peripherals. 8. TOOL OFFSETS/ G53-G59 Input, modification and checking of the dimensions (radius and length) of up to 100 tools and of zero offsets (G53-G59). 9. SPECIAL MODES - General testing of the CNC. - Verification of inputs and outputs. - Setting of decoded M functions. - Setting of machine-parameters. - Input of values for leadscrew error compensation. - Operate with the PLC.

If the value 1 is entered in the machine-parameter P610(3), the START input is equivalent to ENTER key in PLAY-BACK operating mode.
3.2.8. Deletion of a block Same as in EDITING mode (6).
3.2.9. Copy a program Same as in EDITING mode (6).

MODE 3: TEACH-IN

This method of programming is basically the same as the EDITING mode, except that the blocks which are written may be executed before being entered into memory. This enables a part to be produced block by block while it is being programmed. The execution of a program requires the following steps:
3.3.1. Selection of the operating mode TEACH-IN (3) - Press OP MODE - Press key 3 The meaning of the function keys to operate in this mode will appear on the screen.
3.3.2. Locking/Unlocking of memory Same as section 3.6.2. in EDITING mode.
3.3.3. Deletion of a complete program Same as section 3.6.3. in EDITING mode.
3.3.4. Change of program number Same as section 3.6.4. in EDITING mode.
3.3.5. Display and search of memorized subroutines Same as section 3.6.5. in EDITING mode.
3.3.6. Selection of a program Same as section 3.6.6. in EDITING mode.
3.3.7. Creation of a program Same as section 3.6.7. in EDITING mode except that the block may be executed before pressing ENTER. To do this: - Press. The CNC executes the block. - If it is correct, it may be recorded in memory by pressing ENTER. - If it is incorrect, press DELETE. - Rewrite the block.
On pressing , the CNC executes the block and the display mode changes to AUTOMATIC mode. By pressing ENTER or DELETE the display returns to the TEACH- IN display mode. When the blocks are executed, the CNC retains the sequence of the completed blocks. Radius compensation cannot be performed in this mode. If a subroutine is called, the CNC will execute all its blocks. In machining centers, when M06 is programmed, the CNC will execute all the movements associated with tool change.
3.3.8. Deletion of a block Same as in EDITING mode (6).
3.3.9.Copy a program. Same as in EDITING mode (6).

MODE 4: DRY RUN

This operating mode is used for testing a program in a dry run before producing the first part.
3.4.1. Execution of a program The execution of a program requires the following steps:
3.4.1.1. Selection of the operating mode DRY RUN (4) - Press OP MODE - Press key 4. The screen will display: DRY RUN
0 - G FUNCTIONS 1 - G,S,T,M FUNCTIONS 2 - MAIN PLANE MOVE 3 - RAPID MOVE 4 - THEORETICAL PATH
0 - G FUNCTIONS The CNC will only execute the programmed G functions. 1 - G,S,T,M FUNCTIONS The CNC will only execute the programmed G,S,T,M functions. 2 - MOVEMENT ON THE MAIN PLANE The CNC will execute the G,S,T,M functions plus the movements on the main plane.

3.5.5.1. Entering an F value - Press the F key - Key in the required value - Press
3.5.5.2. Entering an S value - Press the S key - Key in the required value - Press 3.5.5.3. Entering an M value - Press the M key - Key in the required value - Press
Except for M41,M42,M43 and M44 which are automatically generated by the CNC when an S value requiring range change is programmed.
3.5.6. Operation of the CNC as a readout Once the JOG operating mode is selected, if the external MANUAL input is activated, the CNC acts as a readout. In this case, the machine has to be moved by means of external controls and the analog signals must be generated outside the CNC.The S and M functions may be entered in this form of operation. If when operating in this mode, the software travel limits (set via machine-parameters) are overrun, the CNC will send the relevant error code and will only allow the machine to be moved to bring it back to the permitted zone.
3.5.7. Change of measurement units Every time the key I is pressed the measurement units change from mm to inches and viceversa. 3.5.8. Handwheel operation When an electronic handwheel is fitted, with this option the axes can, one at a time, be moved manually. For this: - Select the JOG operation mode. - Turn the front knob to one of the positions.
- Press any of the two JOG keys which correspond to the axis to be moved by the Handwheel. If a FAGOR Handwheel (mod 100 P) is used, the axis can also be selected by means of the built-in selector button; the relevant axis will be displayed in reverse video on the CRT. - Turn the Handwheel, the axis will move according to the setting of the relevant machineparameter multiplied by the factor selected with the switch (X1,X10,X100). It should be borne in mind that if we wish to move an axis at a speed of over G00 corresponding to this axis, the CNC will assume this as maximum, ignoring additional pulses. In this way the generation of following errors is avoided. To change the axis being jogged: - Press any of the two JOG keys of the new axis or the axis selector button if a FAGOR Handwheel (mod 100 P) is used. - Turn the Handwheel. To end the Handwheel operation. - Turn the M.F.O. switch to any other position or press the STOP key or keep the axis selector button pressed until the CRT stops blinking the selected axis, if a FAGOR Handwheel (mod 100 P) is used.

G01 G90 X650 Y400 F150

The knob on the front panel of the CNC (M.F.O.) can be used to vary the programmed feedrate F between 0% and 120% or between 0% and 100%, according to parameter P606(2). If, during a G01 movement, the RAPID FEED key is pressed, the movement will be performed at twice the programmed feedrate if P606(2) is zero. The same thing will happen when the external START input is activated if P609(7) is one. Function G01 is modal and incompatible with G00,G02,G03 and G33. Function G01 can be programmed as G1. 6.2.3. G02/G03. Circular helical interpolation G02: Clockwise circular helical interpolation. G03: Counter-clockwise circular helical interpolation.
6.2.3.1. Circular interpolation The movements programmed following G02/G03 are performed in a circular path at the programmed feedrate F. The definitions of clockwise (G02) and counter-clockwise (G03) have been fixed according to the system of coordinates depicted below (right-hand or dextrogyratory system).
This system of coordinates is referred to the movement of the tool over the part.
The direction of G02 and G03 on the XZ plane can be changed by means of parameter P605(4). If the system of left-hand coordinates is used, the directions of G02 and G03 are reversed. Circular interpolation can only be carried out in the plane. The method of defining circular interpolation is as follows: Cartesian coordinates XY plane G17 G02 (G03) X+/-4.3 Y+/-4.3 I+/-4.3 J+/-4.3 F5.4 XZ plane G18 G02 (G03) X+/-4.3 Z+/-4.3 I+/-4.3 K+/-4.3 F5.4 YZ plane G19 G02 (G03) Y+/-4.3 Z+/-4.3 J+/-4.3 K+/-4.3 F5.4 In the case of four-axis machines: a) If the fourth axis (W) is incompatible with the X axis. WY plane G17 G02 (G03) W+/-4.3 Y+/-4.3 I+/-4.3 J+/-4.3 F5.4 WZ plane G18 G02 (G03) W+/-4.3 Z+/-4.3 I+/-4.3 K+/-4.3 F5.4 b) If the fourth axis (W) is incompatible with the Y axis. WX plane G17 G02 (G03) W+/-4.3 X+/-4.3 I+/-4.3 J+/-4.3 F5.4 WZ plane G19 G02 (G03) W+/-4.3 Z+/-4.3 J+/-4.3 K+/-4.3 F5.4 c) If the fourth axis is incompatible with the Z axis. WX plane G18 G02 (G03) W+/-4.3 X+/-4.3 I+/-4.3 K+/-4.3 F5.4 WY plane G19 G02 (G03) W+/-4.3 Y+/-4.3 J+/-4.3 K+/-4.3 F5.4
16 8025/8030 CNC PROGRAMMING MANUAL
Polar coordinates XY plane G17 G02 (G03) A+/-3.3 I+/-4.3 J+/-4.3 F5.4 XZ plane G18 G02 (G03) A+/-3.3 I+/-4.3 K+/-4.3 F5.4 YZ plane G19 G02 (G03) A+/-3.3 J+/-4.3 K+/-4.3 F5.4 In the case of four-axis machines: a) If the fourth axis (W) is incompatible with the X axis. WY plane G17 G02 (G03) A+/-3.3 I+/-4.3 J+/-4.3 F5.4 WZ plane G18 G02 (G03) A+/-3.2 I+/-4.3 K+/-4.3 F5.4 b) If the fourth axis (W) is incompatible with the Y axis. WX plane G17 G02 (G03) A+/-3.3 I+/-4.3 J+/-4.3 F5.4 WZ plane G19 G02 (G03) A+/-3.3 J+/-4.3 K+/-4.3 F5.4 c) If the fourth axis is incompatible with the Z axis. WX plane G18 G02 (G03) A+/-3.3 I+/-4.3 K+/-4.3 F5.4 WY plane G19 G02 (G03) A+/-3.3 J+/-4.3 K+/-4.3 F5.4

6.4. TRANSITION BETWEEN BLOCKS 6.4.1. G05. Round corner (Does not wait for in position) When operating on G05, the CNC starts to execute the next block of the program as soon as the deceleration of the axes programmed in the previous block begins (it does not wait for in-position). In other words, the movements programmed in the next block are executed before the machine has reached the exact position programmed in the previous block. Example:
N1 G91 G01 G05 Y70 F100 N10 X90 As can be seen in the example, the edges would remain rounded in the case of two mutually perpendicular movements. The difference between the theoretical and actual profiles is a function of the feedrate value. The faster the feedrate, the greater the difference between theoretical and actual profiles. Function G05 is modal and incompatible with G07. Function G05 can be programmed as G5.
6.4.2. G07. Square corner When operating on G07, the CNC does not execute the next block of the program until the exact position presently programmed has been reached. Example:
N5 G91 G01 G07 Y70 F100 N10 X90 The theoretical and actual profiles coincide. Function G07 is modal and incompatible with G05. Function G07 can be programmed as G7. When turned ON and after M02,M30, EMERGENCY or RESET if machine parameter, the CNC assumes function G07 or G05 depending on the value assigned to machine parameter P613(5), i.e.,. With P613(5) = 0, it assumes G07. With P613(5) = 1, it assumes G05
6.5. G08. ARC TANGENT TO PREVIOUS PATH An arc tangent to the previous path can be programmed by means of G08. Center coordinates (I,J,K) are not required. Cartesian coordinates (XY plane) N4 G08 X+/-4.3 Y+/-4.3 N4 G08 X+/-4.3 Y+/-4.3 : Block number : Code defining circular interpolation tangent to previous path : Coordinate values of the arcs final point : Coordinate values of the arcs final point
Polar coordinates: N4 G08 R+/-4.3 A+/-4.3 N4 G08 R+/-4.3 A+/-4.3 : Block number. : Code defining circular interpolation tangent to previous path. : Radius (referred to polar origin) of the arcs final point. : Angle of the arcs final point.
Example: The starting point being X0 Y40 the programming of the following path is described: - Straight line - Arc tangent to the previous line - Arc tangent to the previous arc N0 G90 G01 X70 F100 N5 G08 X90 Y60 N10 G08 X110 Y60
An alternative way of programming (using I,J) would be the following: N0 G90 G01 X70 F100 N5 G03 X90 Y60 I0 J20 N10 G02 X110 Y60 I10 J0 The function G08 is not modal. It replaces G00,G01,G02 or G03 only in the block in which it is written. The previous path can be a straight line or an arc. G08 replaces G02 and G03 only in the block in which it is written.
A circle cannot be executed with G08 function, as there are infinite solutions. The CNC will display the error code 47.
6.6. G09. ARC PROGRAMMED BY THREE POINTS Two points (the final plus one intermediate point) are sufficient to program an arc provided that the actual position is the starting point. In other words, an intermediate point is programmed instead of the center. This feature can be useful when a part is programmed in PLAY BACK and after writing G09 in the block the machine can be manually shifted to the intermediate point of the arc and press ENTER. Then to the final point and press ENTER. In this way, the block will be stored in the memory. Cartesian coordinates (XY plane) N4 G09 X+/-4.3 Y+/-4.3 I+/-4.3 J+/-4.3 N4 G09 X+/-4.3 Y+/-4.3 I+/-4.3 J+/-4.3 : Block number. : Code identifying 3 point arc definition. : X value of the arcs final point. : Y value of the arcs final point. : X value of the intermediate point. : Y value of the intermediate point.

8. 9. 10.

Real Theoretical
Once the cycle is finished, the parameter table will show: P90 = Measured X value P91 = Measured Y value P92 = Measured Z value P93 = Real value minus theoretical value on the X axis (P90-P0) P94 = Real value minus theoretical value on the Y axis (P91-P1) P95 = Real value minus theoretical value on the Z axis (P92-P2) Parameters P93, P94 and P95 will indicate the offset value to be added to the parts datum point so the theoretical values will be the same as the parts realvalues. To do so, a function of the following type may be used: G53/59 I P93 J P94 K P95
N05. Inside edge measuring cycle Programming format: G75 N05 P0=K P1=K P2=K P3=K P4=K G75 N05 = Inside edge measuring cycle code. P0 = Theoretical X value of the point to be measured. P1 = Theoretical Y value of the point to be measured. P2 = Theoretical Z value of the point to be measured. P3 = Safety distance. P4 = Probing feedrate. In this cycle two probings will be performed. The first one on the abscissa of the main plane, that is:. On the X axis for the XY plane (G17). On the X axis for the XZ plane (G18). On the Y axis for the YZ plane (G19) The second probing will be performed on the ordinate of the main plane, that is:. On the Y axis for the XY plane (G17). On the Z axis for the XZ plane (G18). On the Z axis for the YZ plane (G19) The probe must be located inside the pocket before calling for the cycle.
The probes movements will be the following: Let us suppose that the main plain is XY and the edge to be measured is the upper righthand edge of the part (see fig.). 1. The probe will be positioned in rapid at a distance P3 of the first side to be measured. 2. The axis perpendicular to the main plane, in this case Z, will move in rapid to a coordinate value defined by P2. 3. The first probing will be performed by moving the X axis a maximum distance of 2P3 at a feedrate defined by P4 until the probes signal is received. If, afterreaching the maximum distance 2P3, the CNC has not received the probes signal, error 65 will be displayed. 4. Once the first probing is done, the measured value will be loaded and then the X axis will return in rapid. Next, the probe will be positioned in rapid at a distance P3 of the other side to be measured as shown by the diagram. 5. The second probing will be performed by moving the Y axis a maximum distance of 2P3 at a feedrate defined by P4 until the probes signal is received. If, after moving the maximum distance, the CNC has not received the probes signal, error 65 will be displayed. 6. Once the second probing is done, the measured value will be loaded and then the Y axis will return in rapid. 7. The Z axis will move in rapid up to the Z value of the cycles starting point. 8. X and Y axes will return in rapid to the cycles starting point.

6.30.3. Preparation of a digitizing operation and later execution at the machine. CONCEPTION OF THE SYSTEM. THE PROBE. The probe can be fastened to the toolholder of the milling machine or machining center, as if it were a tool, converting the machine tool into an automatic digitizing system. The tip (interchangeable) of the needle of the probe isprovided with a ball which is threaded to the probe and follows the surface of the pattern during digitizing. Each probe involves a family of tips with different ball radii for multiple applications. The diameter of the ball of the needle or tip should be the same as the tool used in subsequent machining. The corrections of radii for other tools are also possible but another treatment of the digitized program is required (G41, G42, G43). The different probe needles have variable weights. In fact, in the probe system, needles must have a maximum weight of 200 gm approximately to avoid possible errors of interpretation of contact.
. CALIBRATING THE PROBE For this, we use the N01 cycle with which we determine the offset values for the probe, which will be entered by the CNC in the corresponding corrector, which we have chosen previously. (T00 by default.) The offset values are the error which may exist in the axes of the main plane between the axis of the toolholder and the center of the measurement probe ball. In order to execute this cycle it is necessary to machine a hole beforehand, inside which we will carry out the probings. Once the hole has been made, the diameter and X,Y,Z coordinates of which we know (this is due to that fact that we have chosen the place previously and moved to it with the CNC jog controls) we change the tool for the probe and move in Z until we are inside the hole. Next, we execute the N01 probe calibration cycle. Previously the programming format is completed and the tool corrector is chosen where we want offset I,K to appear. T00 corrector is taken by default. All these operations can be done in TEACH-IN. On exiting from the cycle the control automatically updates the I,K offset of the table and the probe goes back to the starting point. Next we complete the rest of the information on the table: R : Radius of the ball L : Length of the probe (depends on the zero part). If zero part is on the surface of part, L will be zero also. This type of probe placed on the toolholder of the spindle will be used to carry out the remaining probingcycles. If we change the probe for another, we must repeat the entire process. Once the probe has been calibrated we can proceed with the probing of the surface chosen.
. DIGITIZING OF THE PATTERN Digitizing consists of the reading of points on a surface with a measurement probe. Points are read with the combination of the preparatory functions of the CNC: - Function G75 allows the reading and acceptance of the points by the CNC. - The G76 function allows these to be stored in the CNC itself, if the contents are less than 32 Kb, or in a computer. The program obtained in this way allows the reproduction of the points and the generation of the surface which has been digitized previously in two ways: - From the CNC itself, if the contents are less than 32 Kb. - Of from a computer by means of the FAGORDNC application using the option: EXECUTION OF THE INFINITE PROGRAM. 1-Sampling program This is a CNC program which guides the probe along the surface to be digitized in a succession of points which is as extensive and dense as the computer systems available permit. The probe travels over the surface of the model at defined intervals of space, defined in the sample program. The coordinates of these points will be read and the different blocks of the machining program will be generated. By observing the model to be digitized and depending on its geometry we can choose different types of sampling: -Rectangular probing according to the X axis. -Rectangular probing according to the Y axis. -Circular probing. -Diametric probing. -Profile monitoring probing. -Combinations of these. -Etc. Later, examples of these sampling programs will be seen.

6.32.5.2. G82. Drilling canned cycle with dwell The operations and movements of the tool (Z axis) are as follows:. If the spindle was previously running, it continues rotating in the same direction. If it was not running, it starts clockwise (M03). Rapid movement of the Z axis from the starting plane to the reference (approach) plane. Movement at the working feedrate of the Z axis to the full machining depth. Dwell. Any time between 0.00 and 99.99 seconds may be programmed, unless it is programmed using a parameter (KP3) in which case the limits are 0.00 and 255. In this cycle the programming of K dwell is obligatory. Rapid withdrawal of the Z axis to the reference plane if G99 is programmed. Rapid withdrawal of the Z axis to the starting plane if G98 is programmed.
(G82) DRILLING WITH DWELL

R=Reference plane

G01 Feed G00 Feed K=Programmable dwell
Example G82: Drilling four holes 20 mm deep. Let us suppose that:. The distance between the reference plane and the parts surface is 2 mm. The starting point is X0, Y0, Z0 and the spindle is not running. N0 G82 G99 G00 G91 X50 Y50 Z-98 I-22 K1.5 F100 S500 N3 N5 G98 G90 G00 X500 Y500 N1 N10 G80 G00 X0 Y0 N15 M30
First block (N0) G82 : Defines the drilling canned cycle with dwell. G99 : Defines the withdrawal of the tool (Z axis) to the reference plane. G00 : Defines the movement of X and Y axes as being rapid. G91 : Defines the X,Y,Z,I dimensions as being incremental. X( ) : Movement in millimeters of these axes. Y( ) Z( ) : Movement in millimeters of the tool (Z axis) from the starting plane to the reference one. I( ) : Movement in millimeters from the reference plane to the full machining depth.
K( ) : Defines the dwell in seconds. F( ) : Working feedrate in millimeters/min. S( ) : Spindle rotation speed in rev/min. N( ) : Number of times the block is repeated.
Second block (N5) G98 : Defines the withdrawal of the tool (Z axis) to the starting plane. G00 : Defines the X and Y axes movement as being in rapid. G90 : Defines the X and Y dimensions as being absolute. X( ) : Absolute coordinates of these axes. Y( )
Third block (N10) G80 : Canned cycle cancellation. G00 : Defines the X and Y axes movement as being in rapid. X( ): Absolute coordinates of these values. Y( )
Fourth block (N15) M30 : End of program and return to the first block.
Starting plane Reference plane
Sequence and explanation of the operations 1. The X and Y axes move 50 mm in rapid to point X50,Y50. 2. The spindle starts rotating clockwise (M03) at a speed of 500 rev/min. 3. The Z axis moves 98 mm in rapid to Z-98 (reference plane). 4. The Z axis moves a further 22 mm in working feedrate (F100) to point Z-120 (full drilling depth). 5. Dwell 1.5 seconds. 6. The Z axis withdraws 22 mm in rapid to the reference plane (Z-98). 7. The X and Y axes move 500 mm in rapid to point X100, Y100. 8. Operations 4,5 and 6 are repeated. 9. The X and Y axes move 5 mm in rapid to point X150, Y150. 10. Operations 4,5 and 6 are repeated. 11. The X and Y axes move in rapid to point X500,Y500. 12. Operation 4 repeated. 13. The Z axis withdraws 120 mm in rapid to the starting plane (Z0). 14. The X and Y axes move in rapid to point X0,Y0. 15. End of program. The spindle stops running.

6.32.5.3. G84. Tapping canned cycle The operations and movements of the tool (Z axis) are as follows:. If the spindle was previously running, it continues to rotate in the same direction. If it was not running, it starts clockwise (M03). Rapid movement of the Z axis from the starting plane to the reference (approach) plane. Movement at the working feedrate of the Z axis to the full machining depth. Whether the spindle stops running or not (M05), depends on the value given to the machine-parameter P607(2). Dwell. Any time between 0.00 and 99.99 seconds may be programmed unless it is programmed using e parameter (KP3) in which case the limits are 0.00 and 655.35 seconds. Reversal of spindle rotation. The Z axis withdraws at the working feedrate to the reference plane. The spindle stops running or not (M05), depending on the value given to the machine parameter P607(2). Dwell (same value as programmed above). Reversal of spindle rotation. Rapid withdrawal of the Z axis to the starting plane if G98 is programmed.

(G84) TAPPING

During the tapping canned cycle (G84), the feedrate is 100% regardless of the position of the FEEDRATE knob. also, the spindle speed (S) cannot be changed from the front panel keys during the movement of the axis perpendicular to the main plane.
Example Tapping four holes, 20 mm deep. Let us suppose that:. The working plane is the one formed by X and Y axes. The distance between the reference plane and the surface of the part is 2 mm. The starting point is X0,Y0,Z0 and the spindle is not running. N0 G84 G99 G00 G91 X50 Y50 Z-98 I-22 K1.5 F350 S500 N3 N5 G98 G90 G00 X500 Y500 N1 N10 G80 G00 X0 Y0 N15 M30
Sequence and explanation of operations 1. The X and Y axes move 50 mm in rapid to point X50,Y50. 2. The spindle starts rotating clockwise (M03) at 500 rev/min. 3. The Z axis moves 98 mm in rapid to the reference plane (Z-98). 4. The Z axis moves at the working feedrate (F350) to point Z-120 (full machining depth). 5. The spindle stops running (M05). 6. Dwell of 1.5 seconds. 7. Reversal of spindle rotation. 8. The Z axis withdraws 22 mm at the working feedrate to the reference plane (Z-98). 9. The spindle stops running. 10. Dwell of 1.5 seconds. 11. Reversal of spindle rotation. 12. The X and Y axes move 50 mm in rapid to point X100,Y100. 13. Operations 4 to 11 are repeated. 14. The X and Y axes move 50 mm in rapid to point X150 Y150. 15. Operations 4 to 11 are repeated. 16. The X and Y axes move in rapid to point X500,Y500. 17. Operations 4 to 11 are repeated. 18. The Z axis withdraws 98 mm in rapid to the starting plane (Z0). 19. The X and Y axes move in rapid to X0,Y0. 20. End of program (spindle stops running).

R(0.000/500): Factor which decreases or increases the value of incremental penetration B. If R=1, all the penetrations B are equal. If R is different from 1, the first penetration will be B=B, the second B=RB, the third B=R(RB) and so on. If this parameter either is not programmed or is set to 0, the CNC will consider it as value 1.
: Identifies the number of times the block execution is required to be repeated. A value within N0 and N99 can be programmed, although, if it is programmed with a parameter (N P2), the latter can have a value within 0 and 255. If the parameter N is not programmed, CNC assumes the value N1. Obviously, the programming of values of Nhigher than 1 makes sense if operating on G91, in other words, the values of movement of the axes are incremental, since otherwise, the machinings will be repeated at the same point. When programming the same canned cycle a number of times, only the functions F,S and M will be executed in the cycle calling block.
Movements of the axis perpendicular to the main plane, on the deep drilling cycle G83, programmed in format b).
Reference plane Part surface
Working direction G01 Rapid Feed G00
Sequences and explanation of operation: 1. If the spindle was previously running, it keeps on rotating in the same direction. If it was not running, it start clockwise (M03). 2. Movement from the starting plane to the reference plane in rapid G00. 3. Movement at the working feedrate of a distance equal to B+D. 4. Dwell K in seconds, if it has been programmed. 5. Withdraws in G00 either a distance equal to H or to the reference plane according to the value given to J. 6. Movement in rapid to a distance C, before the previous penetration. 7. Movement at the working feedrate of a distance equal to B+C. 8. Dwell K in seconds if it has been programmed. 9. Operations 5 to 8 are repeated, until reaching the penetration I. 10. Depending on the function programmed G98 or G99, the tool withdraws either to the starting plane or the reference plane in rapid.
If the value given to parameter R is equal to 1, all the incremental penetrations B are equal (B1=B2=B3=B4). If the mentioned parameter is different from 1, the different penetrations will be: B1=B; B2=RB1; B3=RB2; B4=RB3. In both cases, the last penetration will be determined by the CNC, according to the value of the total penetration I. If we program for instance, B=12 L=9 R=0.9; the incremental penetrations B will be: B1=12 B2=0.9X12=10.8 B3=0.9X10.8=9.72 B4=0.9X9.72=8.748 As B4 is smaller than the minimum penetration L, from B4 on, it included, every subsequent penetration will have a value equal to L, that means equal to 9.
6.32.7. Pocket milling canned cycle definition (G87,G88) When operation on cartesian coordinates, the basic structure of the block in which a cycle is defined is: N4 (G87 or G88) (G98 or G99) (W+/-4.3) (V+/-4.3) X+/- 4.3 Y+/-4.3 Z+/-4.3 I+/-4.3 J+/-4.3 K4.3 (for G87 only) B4.3 C4.3 D+/-4.3 H4 L4.3 N2 N4 : Block number (0-9999).

Polar origin

In block N0, the point X200 Y0 has been defined as polar origin. In block N5 a linear interpolation (G01) up to point R150 A90 (X200 Y150) has been programmed.
2) Let us again suppose that the tool is at X0 Y0. N0 G93 G01 R200 A135 F500 N5 R100 A90
On reading block N0, the CNC takes the point where the tool is located at that moment (X0,Y0) as the polar origin in order to continue by executing a linear interpolation movement (G01) to the point defined by R200 A135. N5 then defines another linear interpolation movement to R100 A90.
When turned on or after M02,M30, EMERGENCY or RESET, the CNC takes the point (X0,Y0) as the polar origin. When changing of main plane, it takes the cartesian coordinate origin of that plane as the polar origin. When changing to G18 it takes X0 Z0. When changing to G19 it takes Y0 Z0. When changing to G17 it takes X0 Y0.
6.36. G94. FEEDRATE F IN mm/min. (inches/min.) When the code G94 is programmed the CNC assumes that the values entered by F are in mm/min.(0.1 inches/min) or 0.1mm/min (0.01 inch/min) depending on the value of machine parameter P611(5). G94 is modal, i.e. it remains active until G95, is programmed when turning on or after M02,M30, EMERGENCY or RESET the CNC assumes G94.
6.37. G95. FEEDRATE F IN mm/rev. (inches/rev.) When the code G95 is programmed the CNC assumes that the values entered by F3.4 are in mm/rev. the maximum value in mm is F500 (500mm/rev). In inches the format is F2.4 (F1=1inch/rev) and the maximum value is 19.6850 inch/rev. G95 is modal, i.e. it remains active until G94,M02 or M30 are programmed. This feature requires an encoder on the spindle.
The meaning of F (feed programming) differs, according to whether we are working in G94 or G95, from the value of machine parameter P611 (5) when we are working in G94 and from the system used in programming either in mm or inches. All this will be dealt with later in the section FEED PROGRAMMING.
6.38. G96. CONSTANT SURFACE SPEED When G96 is programmed, the CNC assumes that values F refer to the feed at the tools cutting edge. The feed at the center of the tool will vary when machining around corners so that the feed at the cutting edge remains constant. This feature enables a better finishing of the part especially on inside corners. G96 is modal and is cancelled by G97,M02 or M30. When operating in G96 the tool centers speed will varyaround corners, so that the cutting edges speed remains constant.

IDENTIFICATION OF A STANDARD SUBROUTINE
A standard (non-parametric) subroutine always begins with a block which contains function G22. The structure of the subroutine opening block is: N4 G22 N2 N4 : Block number G22: Defines the beginning of a subroutine N2 : Identifies the subroutine (may be any number between N0 and N99) This block cannot contain additional information.
Two standard subroutines having the same identification number but belonging to different programs cannot be present at the same time in the memory of the CNC, although a standard subroutine and a parametric subroutine may be identified by the same number. The subroutine opening block is followed by programming the blocks required. A standard subroutine can contain parametric blocks. Example: N0 G22 N25 N10 X20 N15 P0=P0 F1 P1 N20 G24 A subroutine must always end with a block of the form: N4 G24. N4 : Block number G24: End of subroutine No other additional information can be programmed in that block.
CALLING IN A STANDARD SUBROUTINE
A standard subroutine may be called in from any program or other subroutine (standard or parametric). Calling in a standard subroutine is achieved by function G20. The structure of a call block is: N4 G20 N2.2 N4 : Block number
G20 : Subroutine call N2.2 : The two figures to the left of the decimal point identify the number of the subroutine called in (00-99).The two figures on the right of the decimal point indicate the number of times the subroutine is to be repeated (00- 99). Unless it is programmed by a parameter, in which case the limits are 0 and 255. However, when no number is indicated, the subroutine will be executed only once. No other additional information can be programmed in the block calling in a standard subroutine.
12.3. IDENTIFICATION OF A PARAMETRIC SUBROUTINE A parametric subroutine always begins with function G23. The structure of the first block of a parametricsubroutine is: N4 G23 N2 N4 : Block number G23 : Defines the beginning of a parametric subroutine. N2 : Identifies the parametric subroutine (may be any number between N00 and N99).
Two parametric subroutines having the same number but belonging to different programs cannot be present at the same time in the memory of the CNC, although it is possible for a normal subroutine and a parametric subroutine to be identified by the same number. The above block is followed by programming the blocks required. A parametric subroutine must always end with a block of the form N4 G24. N4 : Block number G24 : Defines the end of a subroutine (standard or parametric). No other additional information can be programmed in that block.

If it is not required for the CNC error code comment to be displayed, the number of the code after G30 must be greater than those used by the CNC. Remember also that the user can write comments in the program which will be displayed when the corresponding block is executed.
EXAMPLE OF PROGRAM OF AN ARC WHOSE RADIUS IS GREATER THAN 8388.607 mm If starting point is X3000 Y2000 and the following arc is programmed: G03 X1000 Y3774.964 I-8000 J-7000 The CNC will generate error 33 because the radius is greater than 8388 mm. Parametric programming can be used to overcome this limitation.
MEANING OF PARAMETERS Call parameters P0: X value of the final point P1: Y value of the final point P2: Distance from the starting point to the center, along X axis P3: Distance from the starting point to the center, along Y axis P4: Feedrate P5: Increment of the angle with its sign (Clockwise = negative, counterclockwise = positive). Parameters used in the subroutine P90: X value of the starting point P91: Y value of the starting point P92: Radius P93: Initial angle P94: Final angle P95: Working or movement angle P96: Arcs centers X value P97: Arcs centers Y value P98: Calculations P99: Calculations

Subroutines flow chart:

SUBROUTINE N98 N00 G23 N98 N01 P90=X P91=Y.. (Takes point values) P96=P90 F1 P2 P97=P91 F1 P3.. (Calculates center) P92=P2 F6 P3... (Calculates radius) P98=P3 F4 P2 P93=F10 P98.. (Calculates angle ) P98=P90 F2 P96 P98=F11 K0 N02 G29 N4 N03 P93=P93 F1 K180 N04 P98=P0 F2 P96 P99=P1 F2 P97.. (Calculates angle ) N05 P94=P99 F4 P98 P94=F10 P94 P98=F11 K0 N06 G29 N8 N07 P94=P94 F1 K180 N08 P5=F11 K0 N09 G29 N16 N10 P93=F11 K0 N11 G29 N2... (Adjusts values of N12 P94=F11 K0 and if the N13 G28 N21 arc spares 3rd and 4th N14 P93=P93 F1 K360 quadrants) N15 G25 N21 N16 P94=F11 K0 N17 G29 N21 N18 P93=F11 K0 N19 G28 N2 N20 P94=P94 F1 K360 N21 P95=P93 F1 P5... (angle = + P5) N22 P98=F8 P95 P98=P98 F3 P92 P98=P98 F1 P96.. X value of point) P99=F7 P95 P99=P99 F3 P92 P99=P99 F1 P97.. (Y value of point) N23 G1 XP98 YP99 FP4... (Go to point) N24 P95=F11 P94.. (End of arc?) N25 G26 N37 N26 P94=F11 P93.. (Compare and ) N27 G26 N37... (If = end ) N28 G28 N33 N29 P95=P95 F1 P5 P95=F11 P94.. (If > increment of ... and check whether = ) N30 G28 N32 N31 P95=P94... (If = has been reached or surpassed) N32 G25 N22... (calculates new point) N33 P95=P95 F1 P5 P94=F11 P95.. (If > decrement of and... check whether = ) N34 G28 N36 N35 P95=P94... (If = has been reached or surpassed) N36 G25 N22... (calculates new point) N37 G24