FANUC SERIES 21i/18i/16i – TA Concise guide Edition 03.
_____________________________________________________________________ 0.1 GENERAL INDEX- CONCISE GUIDE FOR PROGRAMMER PAGE PAR. CONTENTS 7 1.0 FOREWORD 8 2.0 NC MAIN FUNCTIONS AND ADDRESSES 8 2.1 O Program and sub-program number 8 2.2 N Block number 9 2.3 G Preparatory operations 9 2.4 X/Z/B/Y Movement absolute co-ordinates 10 2.5 U/W Movement incremental co-ordinates 12 2.6 F Work feed 12 2.7 S Spindle rotation speed 13 2.8 T Tool selection 15 2.
_____________________________________________________________________ PAGE PAR. CONTENTS 44 3.15 M134/M135 Precise stop 45 3.16 G List of main “G” preparatory functions 47 4.0 FIXED FANUC CYCLES 47 4.1 G71 Material removal by turning 53 4.2 G72 Material removal by facing 57 4.3 G73 Profile repetition 60 4.4 G70 Finishing cycle 63 4.5 G174 Radial grooves rough machining/pre-finishing cycle 67 4.6 G176 Axial grooves rough machining/pre-finishing cycle 72 4.
_____________________________________________________________________ PAGE PAR. CONTENTS 118 7.8 O9103 Front tapping sub-program 121 7.9 O9104 Radial tapping sub-program 124 7.10 G112 Programming in imaginary co-ordinates 127 7.11 G2/G3 Circular interpolation in G112 129 7.12 G41 G42 G40 Milling radius offset in G112 131 7.13 G107 Cylindrical interpolation 135 7.14 Programming with real Y axis 138 8.0 BAR MACHINING 138 8.
_____________________________________________________________________ PAGE PAR. CONTENTS 150 13.12 Creation of a new subprogram 150 13.13 Graphic simulation of a programme 151 13.14 Running of the programme in automatic cycle 151 13.15 Interruption of programme execution 151 13.16 How to start the programme from an intermediate stage 151 13.17 Background editing 152 14.0 TOOL RESET 152 14.1 Manual tool reset 153 14.2 Centre reset 153 14.
_____________________________________________________________________ PAGE PAR. CONTENTS 163 19.0 KEYBOARD AND OPERATOR’S PANEL 163 19.1 Description of keys on the operator’s panel 167 19.2 Description of keys on the MDI panel 170 19.3 Selector switch and keys below the operator’s panel 172 20.0 SERIAL PORT COMMUNICATION 172 20.1 Setting of data transfer parameters 172 20.2 Cable scheme 174 20.3 Transmission programs 176 20.4 How to copy a programme to the serial port 176 20.
_____________________________________________________________________ 1.0 FOREWORD On an NC machine tool the sequence of the instructions programmed to process a workpiece consists of codes which are made up of functions or addresses with a relevant numeric value. When preparing a part program the tool path is imagined referring to a system of co-ordinates, the origin of which ( => zero point to which all the dimensions refer) can be chosen.
_____________________________________________________________________ 2.0 NC MAIN FUNCTIONS AND ADDRESSES The sequence of instructions that make up the program consists of letters and numbers, each of which has a specific significance. 2.1 “O” PROGRAM AND SUB-PROGRAM NUMBER The letter O followed by a number indicate the programs and the sub-programs. The number paired with the letter O can range from 1 to 9999.
_____________________________________________________________________ 2.3 “G” PREPARATORY OPERATIONS The G code prepares the control to carry out certain operations that differ according to the number that follows this code (e.g.: G0, G1, G3, etc.). There are two types of preparatory functions: modal functions and self-deletion functions. The former remain active until they are cancelled by other modal functions, the latter are only active in the block where they are entered. 2.
_____________________________________________________________________ X / Z Co-ordinates Position N5 X0 Z0 N6 X40 (1) N7 Z-20 (2) N8 X80 Z-50 (3) N9 Z-70 (4) 2.5 “U and W” MOVEMENT INCREMENTAL CO-ORDINATES Codes U and W define the incremental co-ordinates referring to the last programmed point. U defines a movement on axis X (diametrical programming); W defines a movement on axis Z. These codes can be programmed with a positive or a negative sign.
_____________________________________________________________________ The first program start value and the first position of each tool must always be programmed in absolute co-ordinates. It is possible to program an absolute co-ordinate and an incremental co-ordinate in the same block, providing they do not refer to the same axis.
_____________________________________________________________________ 2.6 “F” WORK FEED Function F (Feed) defines the work feed and can have two different significances, according to which preparatory G function is active (G95 or G94 see par. 3.6 and par. 3.7): • mm/rev (usually used for turning operations). • mm/min (usually used for milling operations or for work movements with spindle stationary). The programmed feed F can be modified through the axis trimmer with a variable value from 0% to 120%.
_____________________________________________________________________ 2.8 “T” TOOL SELECTION Code T (Tool) defines the tool corrector and the position of the turret to be activated for machining. The tool corrector contains information that identifies the characteristics (length, direction, radius etc.) of the tool. When programming, the tool setting is always composed of 3 or 4 digits.
_____________________________________________________________________ When a tool is called up, the turret rotates so as to follow the shortest path, whether clockwise or anticlockwise. In the machines provided with hydraulic turrets, there are two functions to select the desired turret rotation direction. These functions are M16 and M46. M16 forces the clockwise rotation of the turret disk. M46 forces the anti-clockwise rotation of the turret disk. Example: N3 ……….
_____________________________________________________________________ 2.9 “M” AUXILIARY FUNCTIONS Auxiliary functions are used to send commands to the control and to the machine tool and they are divided between functions that become operational as soon as they are read, and functions that become operative at the end of block (M0, M1, M3, M4).. The list below indicates the most commonly used M auxiliary functions : M0 => Stop program .
_____________________________________________________________________ The M functions listed below are used for many specific applications. Details regarding the use of these functions can be found in the machine documentation.
_____________________________________________________________________ M52 ➪ tailstock release from bench and hooking onto carriage M53 ➪ tailstock release from carriage and hooking onto bench M58 ➪ spindle and reset sensor orientation in work position M62 ➪ workpiece counter increment on display (only active in automatic mode) M63 ➪ external robot call to change workpiece (optional) M64 ➪ workpiece released indication to external robot (optional) M65 ➪ workpiece locked indication to external robot (opt
_____________________________________________________________________ 2.10 “M” OTHER AUXILIARY FUNCTIONS The list below indicates other M functions used for many specific applications. Details regarding the use of these functions can be found in the machine documentation.
_____________________________________________________________________ 2.11 “ / “ SKIPPING A BLOCK This function is used to run or exclude the marked block. To activate or exclude this function use the relevant key on the operator panel (“see paragraph 19.1) - With the key warning light off the barred blocks are run. - With the key warning light on the barred blocks are skipped. Example: N10 /T101 N20 /G54 N30 /G92 S2000 N40 /G96 S180 M4 N50 /G0 X100 Z2 M8 N60 /G1 Z-40 F0.25 2.
_____________________________________________________________________ 3.0 ISO PROGRAMMING ISO language is a unified programming system common to many controls on different types of machine tools of different nature. 3.1 “G0” LINEAR AXES RAPID TRAVERSES The “G0” function controls rapid axis movement (at maximum speed). This function is used to separate from or approach the workpiece at a safe distance. This block must contain one or more destination coordinates (X e Z ). Programming “G0 X… Z...
_____________________________________________________________________ 3.2 “G1” WORK LINEAR INTERPOLATION The “G1” function controls a linear work movement (at a programmed speed). This function is used to carry out machining on the workpiece. With this function it is the programmer who decides the speed (feed “F”) at which the tool is to reach the programmed point. The same block must also contain one or two destination co-ordinates (X and Z) and the feed (F) if this has not been inserted beforehand.
_____________________________________________________________________ The linear movement programmed with G1 can be linked to the movement of the next block by a chamfer (,C) or a connecting radius (R). For two-axis machines (without the axis C option) the chamfer can be identified by just the letter C followed by the value (and not by ,C) Example: N12 ….. N13 G1 X… Z… ,C… Z ,C N14 ….. ,C X Z R N12 ….. N13 G1 X… Z… R… R X N14 ….. These functions can only be programmed in a “G1” block.
_____________________________________________________________________ Example of how to use the R and ,C functions: 24 12 40 Chamfers 2x45º Ø35 Ø55 Ø75 R4 N5 …… N6 G0 X0 Z3 Approach N7 G1 Z0 F0.2 N8 X35 ,C2 N9 Z-40 R4 Profile description N10 X55 Z-52 F0.
_____________________________________________________________________ 3.3 “G1 A…” PROGRAMMING WITH ANGLES When using G1 instructions as well as the end of movement co-ordinates X and/or Z, besides radii or chamfers on final points (R and ,C) the programmer can indicate the movement angle (A or ,A on machines that have the motor driven back spindle option) When programming the angle, value A can be positive or negative in a range from 0° to 360°.
_____________________________________________________________________ The use of the A angle makes it possible to program just one final point matched to the movement angle instead of two final points ( X e Z), or in certain conditions, to insert only the line angle without any final co-ordinate.
_____________________________________________________________________ Example of programming using the angles: N48 G0 X0 Z2 N49 G1 Z0 F0.
_____________________________________________________________________ Example of programming using the angles: N48 G0 X0 Z2 N49 G1 Z0 F0.25 N50 X40 N51 Z-7.1 ,A130 N52 X80 ,A150 R5 N53 Z-92 R4 N54 X140 ,A130 ,C2.
_____________________________________________________________________ 3.
_____________________________________________________________________ I and K functions trend : R I -K Programming example : 22.4 19 R5 Ø44 Ø34 ø38 22.4 N5 …… N5 ……. N6 G0 X38 Z3 N6 G0 X38 Z3 N7 G1 Z-19 F0.2 Or: N7 G1 Z-19 F0.2 N8 G3 X44 Z-22.4 R5 N8 G3 X44 Z-22.4 1-2 K-3.4 N9 G1 Z-30 N9 G1 Z-30 N10 ……. N10 ……. G2 and G3 are modal functions and are cancelled by programming a linear movement G function (G0, G1).
_____________________________________________________________________ 3.5 “G4” AXIS PAUSE TIME The G4 function controls a machine axes pause during the running of a cycle for a time, indicated in seconds, that can be programmed with address U. The G4 can be thus programmed: N12 ……. N13 G4 U1 N14 ……. Where : Activates the pause of the machine axes. • G4 => • U => Defines the time of the axes pause in seconds. Minimum value 0.001 seconds, maximum value 9999.999 seconds.
_____________________________________________________________________ 3.6 “G95” FEED IN MM/REV The G95 function selects the feed F in mm/rev. When this function is active the feed values will be programmed as follows: F0.05, F0.15, F0.3, F0.5 and so forth. G95 is automatically activated when the machine is switched on, therefore it is not necessary to specify its activation in the program. It is a modal function and can be cancelled by programming code G94. N4 …… N5 G1 Z-30 F0.
_____________________________________________________________________ 3.8 “G97” FIXED REVOLUTIONS SPINDLE ROTATION Function G97 prepares the spindle speed in revs/min (fixed revs) set by the code S. When this function is active the programmed S value represents the actual number of revolutions per minute of the spindle. (e.g.: S50, S160, S500, S1200, S3200, S5000 etc.). G97 is automatically activated when the control is switched on, therefore it is not necessary to specify its activation in the program.
_____________________________________________________________________ 3.9 “G96” CONSTANT CUTTING SPEED G96 sets the spindle rotation indicated by the code S as constant cutting speed (m/min). With this function active the programmed S value is the surface speed in metres per minute (e.g.: S80, S100, S120, S200, S350 etc.), this function continuously updates the actual spindle revolutions according to the work diameter, keeping the cutting speed constant.
_____________________________________________________________________ A block containing G96 is programmed: N4 …… N5 G96 S150 M4 N6 …… Where: • G96 => Spindle speed set Vt [m/min] • S150 => Cutting speed Vt [m/min] • M4 => Spindle direction of rotation 3.10 “G92” SPINDLE REVOLUTION LIMITATIONS Using the constant cutting speed (function G96) it is often necessary for technical reasons and safety (type of collet chuck, size of workpiece, unbalancing, etc.), to set a limit to the spindle maximum rpm.
_____________________________________________________________________ 3.11 “G33” THREAD CUTTING MOVEMENTS Function G33 is used for separate thread cutting movements.
_____________________________________________________________________ M30 x 2 w. 2 threads 25 N1 T1 (Thread cutting) N2 G97 S1300 M3 N3 G0 X29.5 Z10 M8 N4 G33 Z-26 F4 Q0 N5 G0 X32 N6 Z10 N7 X29.5 N8 G33 Z-26 F4 Q180000 N9 G0 X32 N10 Z10 N11 X29.2 N12 G33 Z-26 F4 Q0 N13 G0 X32 N14 Z10 N15 X29.2 N16 G33 Z-26 F4 Q180000 N17 G0 X32 N18 Z10 N19 ….. N20 …..
_____________________________________________________________________ 3.12 “G41”-“G42”- “G40” TOOL RADIUS OFFSET All inserts for turning have the cutter edge rounded to a pre-defined radius, specified by the insert manufacturer (e.g. 0.4; 0.8; 1.2 etc.). With the tool measurement a point is determined for movements that is not on the insert profile, but is the intersection of the horizontal and vertical lines tangent to the insert radius, as can be seen in the figure that follows.
_____________________________________________________________________ To use the Tool Radius Offset therefore means to enable 3 functions from the program: G41 ➨ Activate the Tool Radius Offset for a PIECE ON THE RIGHT as to the tool direction. G42 ➨ Activate the Tool Radius Offset for a PIECE ON THE LEFT as to the tool direction. G40 ➨ Deactivate the tool radius offset. La Tool Radius Offset is usually only used in the finishing stages to obtain the correct profile.
_____________________________________________________________________ When using the Tool Radius Offset it is also necessary to enter the value of the insert radius (R) and tool orientation (T) in the tool table. The radius value is supplied by the insert manufacturer. For the tool orientation see the figure below. To make it simpler we can say that all the external left tools will have orientation T3 whereas all the internal left tools will have orientation T2.
_____________________________________________________________________ Example of workpiece finishing with a tool radius 0.8: N1 T101 (FINISHING) N2 G92 S3000 N3 G96 S180 M4 N4 G0 X-2 Z3 M8 N5 G42 (Activation of Tool Radius Offset) N6 G1 X0 Z0 F0.25 N7 X40 Z0 N8 Z-7.1 ,A130 N9 X80 ,A150 R5 N10 Z-92 R4 N11 X140 ,A130 ,C2.65 N12 Z-130 N13 X160 N14 G40 (Deactivation of tool Radius Offset) N15 G0 X200 Z200 M5 N16 M30 Note: enter radius (R) 0.
_____________________________________________________________________ 3.13 “G54 / G59” WORKPIECE ORIGINS To be able to refer the tool movements to a fixed point on the workpiece to be machined. By means of a certain operation procedure one or more fixed points are defined that allow the operator to have a reference for the movements to be entered in the work program. These points are called “WORKPIECE ORIGINS” (G54, G55, …G59).
_____________________________________________________________________ Origin G53 cannot be written alone in the block. It must always be coupled to X or Z co-ordinates which identify the movement referred to the machine zero. This movement will always be carried out in rapid traverse. In the case of a more “traditional” use of the machine origin it is recommended to use an origin that can be modified (e.g.
_____________________________________________________________________ 3.14 “G52” ORIGIN TRANSFER BY PROGRAM An alternative to the origin transfer by table is the direct origin transfer by program using instruction G52. With the G52 function it is possible to move the reference point by program (e.g.: G54, G55 etc.). G52 operates in absolute mode in relation to the last workpiece origin selected, with the movement values inserted in the characters of address X and/or Z (e.g.: G52 X5 Z-10).
_____________________________________________________________________ 3.15 “M134 / M135” PRECISE STOP The tool passage from a block to another may happen in two ways: - in execution point to point - in continuous execution These two ways of passage from a block to another can be enabled by two functions M, which are: M134 execution point to point with deceleration at end of block. With this function axes between the blocks execute a deceleration to reach the quote and then restart.
_____________________________________________________________________ 3.16 LIST OF MAIN “G” PREPARATORY FUNCTIONS The list below indicates the main G preparatory functions used to program the FANUC numeric control. G0 ➪ rapid axis linear movement. G1 ➪ axis linear movement in work mode. G2 ➪ clockwise circular interpolation. G3 ➪ anticlockwise circular interpolation. G4 ➪ stand-by. G10 ➪ data entry from program. G11 ➪ deletes the data entry from program mode G17 ➪ selection of working surface X Y.
_____________________________________________________________________ G84 ➪ fixed front tapping cycle (cannot be used with rotating tools). G85 ➪ fixed cycle of frontal boring. G87 ➪ fixed side drilling cycle. G89 ➪ fixed side of lateral boring. G90 ➪ programming with absolute co-ordinates. G91 ➪ programming with incremental co-ordinates. G92 ➪ spindle speed limitation. G94 ➪ feed programming in mm/min. G95 ➪ feed programming in mm/rev.. G96 ➪ constant cutting speed programming in m/min.
_____________________________________________________________________ 4.0 FIXED FANUC CYCLES Fixed cycles are functions that simplify the ISO programming. The most commonly used fixed cycles are described below. 4.1 “G71” MATERIAL REMOVAL BY TURNING The “G71” function activates the material removal by turning cycle. With this function the tool makes increments on axis X and turning on axis Z. The material removal cycle in turning is always composed of two program blocks. Example: N17 ……. N18 G0 X.. Z.. .
_____________________________________________________________________ • U => Diametric machining allowance on axis X value indicated with sign • W => Machining allowance on axis Z value indicated with sign • F => Work feed in rough machining In rapid traverse the tool reaches the X and Z values indicated in the block before the first G71 (these values therefore determine the point where the tool will start to machine: X will be equal to the diameter of the blank workpiece, Z will be the safety dist
_____________________________________________________________________ For overmetal U and W situation see the scheme below: _____________________________________________________________________ CONCISE GUIDE FANUC 49
_____________________________________________________________________ Example of how to use the G71 cycle: CHAMFERS 1.5 x 45° O3434 (REMOVAL OF MATERIAL BY TURNING) N1 T101 N2 G54 N3 G92 S3000 N4 G96 S200 M4 N5 G0 X140 Z3 M8 N6 G71 U3 R1 N7 G71 P8 Q19 U0 W0 F0.35 N8 G0 X26 N9 G1 Z0 N10 X30 ,C1.5 N11 Z-20 R2 N12 X50 ,A120 R3 N13 Z-78.5 R2 N14 X65 ,C1.5 N15 Z-110 R1.5 N16 X120 ,C1.5 N17 Z-130 R1.5 N18 X140 ,C1.
_____________________________________________________________________ N19 Z-132 N20 G0 X200 Z200 M5 N21 M30 If in the profile there are shaded parts (decreasing profiles) proceed as follows: - describe the shaded parts using the same functions as for monotone profiles, angles included - the shaded parts cannot be more than 10 - the first profile description block (block after the second G71) must contain both X and Z - remember that CNC, in machining of shaded parts, doesn’t consider the tool radius compens
_____________________________________________________________________ Example of how to use the G71 cycle with shaded parts : O3435 (MATERIAL REMOVAL IN TURNING WITH SHADED PARTS) N1 T606 N2 G54 N3 G92 S3000 N4 G96 S200 M4 N5 G0 X82 Z3 M8 N6 G71 U2 R1 N7 G71 P8 Q16 U0 W0 F0.
_____________________________________________________________________ 4.2 “G72” MATERIAL REMOVAL BY FACING Function “G72” activates the material removal by facing cycle. With this function the tool makes increments on axis Z and turning on axis X. The material removal by facing cycle is always composed of two program blacks. Example: N17 ……. N18 G0 X.. Z.. .
_____________________________________________________________________ The tool, in rapid traverse, reaches the X and Z values indicated in the block before the first G72 (these values thus determine the point where the tool will start machining: X will be equal to the rough workpiece diameter plus a small safety margin that facilitates the cut increment, Z will be 0 if the workpiece is already faced, or 1 or 2 if there is a machining allowance).
_____________________________________________________________________ Example of how to use cycle G72: CHAMFERS 2 x 45° O3435 (REMOVAL OF MATERIAL BY FACING) N1 T101 N2 G54 N3 G92 S3000 N4 G96 S200 M4 N5 G0 X122 Z0 M8 N6 G72 W2.5 R1 N7 G72 P8 Q18 F0.35 N8 G0 Z-47 N9 G1 X120 N10 Z-45 ,C2 N11 X80 N12 Z-25 ,C1.
_____________________________________________________________________ N15 Z-10 ,A-60 N16 X30 R1.5 N17 Z0 ,C1.
_____________________________________________________________________ 4.3 “G73” PROFILE REPETITION The “G73” function activates the profile repetition cycle. With this function the defined profile can be repeated several times, moving it each time by a certain distance. This cycle is most useful to work on workpieces coming from stamping, casting or a previous rough machining. The profile repetition cycle is always composed of two program blocks. Example: N17 ……. N18 G0 X.. Z.. .
_____________________________________________________________________ In rapid traverse the tool reaches the values of X and Z set in the block before the first G73 (thus these values determine the point where the tool will start to work). An increment takes place which is equal to the values set in parameters U and W of the first G73 and the number of profile repetitions expressed in parameter R. The tool makes a series of cuts going from the point set in block P up to the point set in block Q.
_____________________________________________________________________ Example of how to use cycle G73 : O3436 (PROFILE REPETITION) N1 T101 N2 G54 N3 G92 S3000 N4 G96 S200 M4 N5 G0 X120 Z10 M8 N6 G73 U3 W3 R4 N7 G73 P8 Q12 F0.
_____________________________________________________________________ 4.4 “G70” FINISHING CYCLE The “G70” function activates the finishing cycle. This function can be used after the three rough machining cycles G71, G72 and G73. The finishing cycle consists of just one block and can contain these codes: • P => Number of first block of the profile to be finished. • Q => Number of the last block of the profile to be finished. • F => Finish feed.
_____________________________________________________________________ Example of how to use cycle G70: CHAMFERS 1.5 x 45° O3437 (PROFILE ROUGH MACHINING AND FINISHING) N1 T101 N2 G54 N3 G92 S3000 N4 G96 S200 M4 N5 G0 X140 Z3 M8 N6 G71 U3 R1 N7 G71 P8 Q19 U0.5 W0.1 F0.35 N8 G0 X26 N9 G1 Z0 N10 X30 ,C1.
_____________________________________________________________________ N13 Z-78.5 R2 N14 X65 ,C1.5 N15 Z-110 R1.5 N16 X120 ,C1.5 N17 Z-130 R1.5 N18 X140 ,C1.5 N19 Z-132 N20 G0 X200 Z200 N21 T202 N22 G54 N23 G92 S3000 N24 G96 S200 M4 N25 G0 X140 Z3 M8 N26 G70 P8 Q19 F0.
_____________________________________________________________________ 4.5 “G174” RADIAL GROOVES ROUGH MACHINING/PRE-FINISHING CYCLE Function G174 activates the rough machining and pre-finishing cycle for grooves on outer and inner diameters, performed by a parting tool with less width at the bottom of the groove. To run a G174 cycle the tool must be positioned with the reference edge on the start cycle point (tool reset on left edge), at a distance of a diametrical millimetre from the part to be machined.
_____________________________________________________________________ C R TOOL RESET The insert radius of the tool used must be specified in the correctors table. G174 must be programmed as follows: N...G174 A.. B.. C.. U/X.. W/Z.. Y.. H.. K.. Q.. D.. (F..) (L..) (P..) (R..) (S..) Where: G174 = Activates the rough machining and pre-finishing cycle for the outer and inner radial grooves. A.. = Angle of groove right-hand wall (in positive direction of axis Z) B.. = Angle of groove left-hand wall.
_____________________________________________________________________ W/Z.. = W groove width, Z last point of groove – specify one or the other -: If W<0 the groove machining is made from right to left of the workpiece. If W>0 the groove machining is made from left to right of the workpiece. If Z < the starting point value, machining is made from right to left of the workpiece (toward Z negative). If Z > the starting point value, machining is made from left to right of the workpiece (toward Z positive).
_____________________________________________________________________ L.. = overmetal on groove’s sides value expressed in mm. NOTE: if only one of the two variables (F or L) is specified, the other variable will be assigned the same value. If they are omitted both are considered null. P.. = Depth of cut (it must always be more than 0, radial value expressed in mm.).The distance between on cut and another is 0.2 mm.If omitted the machining is executed in one cut. R..
_____________________________________________________________________ 4.6 “G176” AXIAL GROOVES ROUGH MACHINING/PRE-FINISHING CYCLE The G176 function activates the rough machining and pre-finishing cycle for axial grooves, working from the right or the left (see fig. 1) with a parting tool having a width less than the bottom of the groove To run a G176 cycle, position the tool with the reference edge (tool reset on the bottom edge)on the start cycle point, at a distance of 0.5 millimetres from the workpiece.
_____________________________________________________________________ Radius specified in the correctors table for the tool used. C R Tool reset Function G176 has to be programmed as follows: N...G176 A.. B.. C.. U/X.. W/Z.. Y.. H.. K.. Q.. D.. (F..) (L..) (P..) (R..) (S..) Where: G176 = Activates the rough machining and pre-finish cycle for right and left axial grooves.
_____________________________________________________________________ A.. = Angle of groove high wall (in axis X positive direction) B.. = Angle of groove low wall. These angles are always positive and have a value from 0 to 89.999 degrees. When the assigned value is 0 , this means the walls are horizontal. C.. = Tool width, always positive value,(r radius and orientation T3 must be specified on table offset as it’s automatically activated the radius compensation). U/X..
_____________________________________________________________________ D can have a value from 0 to 15 according to the elements (chamfers/radii) that constitute the groove, and their arrangement.
_____________________________________________________________________ Example of rough machining and pre-finish of an axial groove using a tool 3 mm wide: N18 T909 (TOOL FOR AXIAL GROOVES) N19 G54 N20 G92 S1500 N21 G96 S100 M4 N22 G0 X30 Z0.5 M8 F0.12 N23 G176 A5 B8 C3 X80 Z-20 Y1 Q1 H1.5 K1.
_____________________________________________________________________ 4.7 “G175” / “G177” FINISHING CYCLE FOR RADIAL/AXIAL GROOVES Functions G175 and G177 activate the finishing cycle for radial grooves (on outer and inner diameters) and axial grooves (cut from right to left of the workpiece). Only function G175 is described here; the description is also valid for cycle G177 (for which the rough machining cycle is G176).
_____________________________________________________________________ Example of rough machining and finish on a radial groove with a tool 3 mm wide: N18 T303 (TOOL FOR RADIAL GROOVES) N19 G54 N20 G92 S1500 N21 G96 S100 M4 N22 G0 X101 Z-30 M8 F0.12 N23 G174 A5 B8 C3 X60 Z-80 Y1 Q1 H1.5 K1.5 D6 F0.4 L0.
_____________________________________________________________________ If the grooves cycle is not programmed correctly, the following alarms may be generated: All 3000: Parameter X or U missing: The value for parameter X or U has been omitted. All 3001: Parameter Z or W missing: The value for parameter Z or W has been omitted. All 3002: Parameter C not correct: The value for parameter C has been omitted or the value is less than or equal to 0.
_____________________________________________________________________ *All 3015: Upper left chamfer error: Upper left chamfer too small in relation to programmed tool radius (right groove bore). *All 3016: Upper right chamfer error: Upper right chamfer too small in relation to programmed tool radius (left groove bore). *All 3017: Lower left chamfer error: Lower left chamfer too small in relation to programmed tool radius (only external grooves).
_____________________________________________________________________ 4.8 “G76” THREAD CUTTING CYCLE IN SEVERAL CUTS Function “G76” activates the thread cutting cycle in several cuts. This function can be used for external and internal thread cutting. The thread cutting cycle in several cuts is always composed of two program blocks. Example: N17 ……. N18 G0 X.. Z.. .
_____________________________________________________________________ rd 3 pair : thread cut angle (value of two digits, only 6 selections 00,29,30,55,60,80) E.g. 00 for square thread cutting 55 for Whitworth thread cutting 60 for metric thread cutting If threads are to be cut with an angle that differs from the 6 selections available, use value 00 In brief : P010060 (1 idle traverse, vertical exit at end of thread , thread with angle of 60°) • Q => Minimum cut depth (in thousandths) E.g. • Q100=0.
_____________________________________________________________________ Example of external metric thread cutting : N17 T101 (External thread cut) N18 G54 N19 G97 S800 M3 N20 G0 X32 Z6 M8 N21 G76 P010060 Q100 R0.02 N22 G76 X28.161 Z-50 P919 Q250 F1.
_____________________________________________________________________ Example of internal metric thread cut : N17 T101 (Internal thread cut) N18 G54 N19 G97 S800 M3 N20 G0 X25 Z6 M8 N21 G76 P010060 Q100 R0.02 N22 G76 X30 Z-40 P919 Q250 F1.
_____________________________________________________________________ Example of external tapered thread cut 1” NPT (pitch 14 threads / inch) : N17 T101 (Taper thread cut) N18 G54 N19 G97 S800 M3 N20 G0 X33 Z6 M8 N21 G76 P010060 Q100 R0.02 N22 G76 X29.588 Z-17.343 P1161 Q250 F1.814 R-0..729 N23 G0 X150 Z100 To machine the tapered thread cut it is important to remember: - Pitch F = 25.4 (comparison between mm and inches) / 14 (n° threads / inch) = 1.
_____________________________________________________________________ 4.9 “G83” FRONT DRILLING CYCLE Function “G83” activates the front drilling cycle. With this function the bit makes a series of cuts, of the required size, undercutting or breaking the chip and returning, at the end of cycle, in rapid traverse to the starting point. The front drilling cycle can contain these codes: • Z => End of drilling absolute value • F => Drilling feed ( in mm/rev.
_____________________________________________________________________ It should also be remembered that parameter 5114 determines: - with chip undercutting: the distance at which the drill is to stop in relation to the last point reached, when re-entering the hole after undercutting.
_____________________________________________________________________ 4.10 “G84” FRONT TAPPING CYCLE THIS CYCLE IS NOT VALID FOR TAPPING WITH MOTOR DRIVEN TOOLS FOR TAPPING WITH MOTOR DRIVEN TOOLS SEE FUNCTIONS P9103 AND P9104 Function “G84” activates the front tapping cycle.
_____________________________________________________________________ This cycle can only be used for right-hand tapping, therefore with entry in direction M3 and coming out in direction M4.
_____________________________________________________________________ 5.0 SUB-PROGRAMS / PARAMETRIC PROGRAMMING Sub-programs are useful to repeat the same operation several times, using inside the program the same functions and co-ordinates already known to the operator With parametric programming, variable values (parameters or variables #) can be attributed to the program codes instead of fixed values (numeric values).
_____________________________________________________________________ MAIN PROGRAM O1 … … … … … M98 P8001 … … … … M30 SUBPROGRAM O8001 … … … … … M98 P8002 … … … … M99 Level 1 SUBPROGRAM O8002 … … … … … M98 P8003 … … … … M99 Level 2 SUBPROGRAM O8003 … … … … … … … … … … M99 Level 3 A sub-program is a normal program that ends with function M99. The same functions can be used inside the sub-program as used in main programs (e.g. fixed cycles, geometric functions etc.
_____________________________________________________________________ If it is required to return from the sub-program to a pre-defined block and not to the block that immediately follows the one in which it has been run, add the pre-defined block to M99, preceded by the letter P.
_____________________________________________________________________ Or to repeat continually a part of the program O2 (MAIN PROGRAM) N10 N20 N30 N40 N50 N60 N70 N80 N90 M99 (SKIP TO FIRST BLOCK AND CONTINUE REPEATING THE PROGRAM) N100 M30 _____________________________________________________________________ CONCISE GUIDE FANUC 88
_____________________________________________________________________ 5.2 PARAMETRIC PROGRAMMING Parametric programming uses variables, arithmetical instructions and conditioned skip instructions. In this way programs for general use can be developed, or they can be personalised for specific customer requirements. VARIABLES There are four types of variables: From #1 to #33 LOCAL VARIABLES These can only be used inside a macro and not shared with other macros.
_____________________________________________________________________ ARITHMETIC OPERATIONS There are ten types of arithmetical operations available: 1 Variable definition and replacement Example: #101=1005 #101=#110 #101=-#112 2 addition Example: #101=#110+#111 3 subtraction Example: #101=#110-#111 4 multiplication Example: #101=#110*#111 or #101=#110*7 5 division Example: #101=#110/#111 or #101=#110/7 6 square root Example: #101=SQRT[#110] or #101=SQRT[5] _________________________________________________
_____________________________________________________________________ 7 sine Example : #101=SIN[#110] or #101=SIN[30] 8 cosine Example: #101=COS[#110] or #101=COS[30] 9 tangent Example: #101=TAN[#110] or #101=TAN[30] 10 arc. cot.
_____________________________________________________________________ 3 conditioned skip if different Example: IF[#101 NE #102] GOTO1000 (skip to block N1000 if parameter #101 is different from parameter #102, if the two parameters are the same the program passes to the next block) 4 conditioned skip if greater than Example: IF[#101 GT #102] GOTO1000 (skips to block N1000 if parameter #101 is greater than parameter #102, if parameter #102 is greater or equal to parameter #101 the program continues with the
_____________________________________________________________________ 6.0 BACK SPINDLE MACHINING The back spindle option is an additional spindle opposite and co-axial to the main one, which makes it possible to machine on the rear part of the workpiece after taking it from the first spindle. The back spindle is useful when working on parts machined from bars, since in most cases, it is possible to obtain complete items regarding the turning operations.
_____________________________________________________________________ Where: • M203 => Back spindle clockwise rotation • M204 => Back spindle anti-clockwise rotation • M205 => Back spindle rotation stop • B => Back spindle axis movement co-ordinate 6.2 “M” AUXILIARY FUNCTIONS The list below contains all the M functions used with the back-spindle option for many specific applications. For details on how to use these functions, consult the machine documentation.
_____________________________________________________________________ 6.3 EXAMPLE OF MACHINING WITH BACK SPINDLE Example of machine the part shown below with a back spindle: 50 15 R2 5 10 20 R2 T1 ∅90 ∅92 N1 G0 B0 ; Back spindle re-positioning N2 T101 ; Tool call-up N3 G54 ; Origin activation N4 G92 S2500 ; Main spindle revs limitation N5 G96 S150 M4 ; Main spindle cutting speed ∅100 N6 G0 X103 Z0 M8 N7 G1 X-0.5 F0.25 N8 G0 X88 Z2 N9 G1 Z0 N10 X90 Z-1 F0.
_____________________________________________________________________ N20 G92 S2500 ; Back spindle revs limitation N21 G96 S150 M204 ; Back spindle cutting speed N22 G0 X103 Z0 M8 N23 G1 X-0.5 F0.25 N24 G0 X90 Z-2 N25 G1 Z0 ; Machining on back spindle side N26 X92 Z1 F0.3 N27 Z15 R2 N28 X100 Z20 F0.15 N29 G0 X200 Z-200 M205 N30 M30 Machining with the back spindle is exactly the same as with the main spindle ; the same ISO functions, same Fixed Cycles.
_____________________________________________________________________ EXAMPLEOF PIECE EXCHANGE WITH COUPLE REDUCTION ….
_____________________________________________________________________ 6.4 “O9100” - WORKPIECE EXCHANGE WITH PARTING OFF This is a sub-program that manages the workpiece change-over between spindles machining from bars. For this reason the cutting is performed with a parting off tool. This sub-program is used when, machining the bar, the workpiece is taken up on the back spindle to machine the second part. At the end of the cycle the workpiece with the useful length will remain on the main spindle .
_____________________________________________________________________ Description: The sub-program is run as follows: The spindles start to rotate in synchronism (M70) at approx. 50 rpm in the direction defined by variable “M”, the parting off tool defined in variable “T” is brought to working position.
_____________________________________________________________________ It is also possible to recover any backlash caused by the use of double cone collet chucks, by inserting a value in mm from 0 to 1 in “R” , which is recovered before parting off with the bar gripped between the two spindles. Separation takes place first along axis X at the value defined in variable “X” then axes B and Z simultaneously at the values at which turret rotation took place.
_____________________________________________________________________ 6.5 “ O9101” - WORKPIECE CHANGE-OVER WITH PARTING OFF, WITHOUT EXTRACTION This is a sub-program that manages the workpiece change-over between spindles working from a bar, for this reason the cut is made with a parting off tool. This sub-program is used when, working on a bar, the workpiece is taken onto the back spindle to work on the second part.
_____________________________________________________________________ Description: The sub-program is run as follows: The spindles start to rotate in synchronism (M70) at approx. 50 rpm in the direction defined by variable “M”, the parting off tool defined in variable “T” is brought to working position . The origin used is that which was active before entering the sub-program.
_____________________________________________________________________ It is also possible to recover any backlash caused by the use of double cone collet chucks, by inserting a value in mm from 0 to 1 in “R” , which is recovered before parting off with the bar gripped between the two spindles. Separation takes place first along axis X at the value defined in variable “X” then axes B and Z simultaneously at the values at which turret rotation took place.
_____________________________________________________________________ 6.6 “ O9102” - WORKPIECE CHANGE-OVER WITHOUT PARTING OFF This is a sub-program that manages workpiece changeover between spindles working from a bar section. Therefore there is no parting off operation.
_____________________________________________________________________ monitor. This value is to be entered in variable “B”. If the rest on mechanical stop is used the value found (using the same method as described above – bringing the back spindle manually onto the mechanical stop) must be increased by 1 or 2 mm before being inserted in variable “B” (E.g.: Value read on monitor B-255.5; Value inserted in variable “B”=-254.5).
_____________________________________________________________________ 7.0 MACHINING WITH “AXIS C” AND MOTOR DRIVEN TOOLS Axis C is an option used to program spindle movements intended as angle movements made with programmable feed. This means that the spindle no longer responds to S functions (rpm.) or M functions (direction of rotation) but becomes an axis to all effects, programmed with address “C” (or “A” in machines fitted with back spindle option).
_____________________________________________________________________ N17 ……. N18 T101 ; Call up for turning tool N19 ……. N20 ……. ; Turning N21 ……. N22 T202 ; Call up for milling tool N23 G54 ; Origin activation N24 M303 S1000 ; Module rpm and direction of rotation N25 G94 F500 ; Feed mm/min set. N26 ……. N27 ……. ; Machining with motor driven module N28 ……. N29 M305 ; Stop module rotation N30 T303 ; Call up for turning tool N31 G95 ; Feed mm/rev. set N32 …….
_____________________________________________________________________ 7.2 MOTOR DRIVEN TOOLS RESET All the tools mounted on motor driven modules (cutters, bits, tapping bits etc.) reset with the same procedure used for normal turning tools. Axial motor driven modules => They reset only along axis Z, the tool length along axis X must be zero (X0) because these tools are co-axial with the turret “zero” position. The reset procedure is described in the Concise Guide for Operator, chapter 14 – TOOL RESET.
_____________________________________________________________________ 7.3 AXIS C The axis C option is activated by functions M37 and G28 C0 (M237 and G28 A0 in the case of back spindle option) whereas to leave this option and return to turning mode it is sufficient to program function M36 (M236 for back spindle option ). Example: N26 …….
_____________________________________________________________________ 7.4 PROGRAMMING IN REAL CO-ORDINATES When functions M37 and G28 C0 (M237 and G28 A0 on machines with back spindle option) the machine prepares to work in “real co-ordinates”. X….. Z…… C (A)…… C+ X+ Z+ Where : • X => Absolute co-ordinate of axis X, is to be programmed with a diametrical value. • Z => Absolute co-ordinate of axis Z. • C => Co-ordinate for axis C positioning on main spindle.
_____________________________________________________________________ 7.5 USE OF SPINDLE BRAKE The machines with the axis C option have a brake which acts on a disk integral with the spindle, preventing rotation due to any machining stress.
_____________________________________________________________________ 7.6 “G83” FRONT DRILLING CYCLE Function “G83” activates the front drilling cycle with motor drivel tools. With this function the bit makes a series of cuts, of the required size, undercutting or breaking the chips and returning at the end of the cycle, in rapid transverse, to the starting point or to point R.
_____________________________________________________________________ Example: drilling of 4 axial holes, depth 20 mm. diameter 50 nr. 4 holes at 90° N34 ….TURNING N35 M37 N36 G28 C0 N37 T101 (AXIAL BIT) N38 G54 N39 M303 S2000 N40 G94 N41 G0 X50 Z5 M8 N42 C0 M20 N43 G83 Z-20 F100 N44 C90 M20 N45 C180 M20 N46 C270 M20 N47 G80 N48 G0 X200 Z200 M21 N49 M305 N50 M36 N51 G95 N52 M30 NOTE. FUNCTIONS M20/M21 FOR THE USE OF THE SPINDLE BRAKE ARE OPTIONAL.
_____________________________________________________________________ Codes Q, P and R , if not used, need not be written. This cycle can be used with chip breakage or undercutting, depending on the value of parameter 5101 bit 2 (if it is 0 chip breakage, if it is 1 chip undercutting) by default this bit is set to 1 for chip undercutting.
_____________________________________________________________________ 7.7 “G87” RADIAL DRILLING CYCLE Function “G87” activates the side radial cycle with motor driven tools. With this function the bit makes a series of cuts, of the required size, undercutting or breaking the chip and returning with a rapid traverse at the end of cycle to the starting point or to point R.
_____________________________________________________________________ Example: 4 radial holes at 20 mm from the workpiece zero N34 ….TURNING N35 M37 N36 G28 C0 N37 T101 (RADIAL BIT) N38 G54 N39 M303 S2000 N40 G94 N41 G0 X55 Z5 N42 Z-20 M8 N43 C0 M20 N44 G87 X40 F100 N45 C90 M20 N46 C180 M20 N47 C270 M20 N48 G80 N49 G0 X200 Z200 M21 N50 M305 N51 M36 N52 G95 N53 M30 NOTE: FUNCTIONS M20/M21 TO USE THE SPINDLE BRAKE ARE OPTIONAL.
_____________________________________________________________________ If not used, codes Q, P and R need not be written. This cycle can be used with chip breakage or undercutting, depending on the value of parameter 5101 bit 2 (if it is 0 chip breakage, if it is 1 chip undercutting) by default this bit is set to 1 for chip undercutting.
_____________________________________________________________________ 7.8 “O9103” FRONT TAPPING SUB-PROGRAM Sub-program “9103” activates the axial tapping cycle. With this function the tapping tool enters with a feed equal to the tapping pitch, reverses the module rotation, followed by simultaneous acceleration of the motor driven tool and the axis then the return to starting point The axial tapping cycle contains these codes: • Z => End of tapping absolute value • F => Tapping pitch ( in mm/rev.
_____________________________________________________________________ Example of single call-up (tapping of one hole only): N15 …. TURNING N16 M37 N17 G28 C0 N18 T606 (AXIAL TAPPING M8) N19 G54 N20 M341 (only for axial disks) N21 G94 N22 G0 X30 Z5 M7 N23 C0 M20 N24 G65 P9103 Z-20 M303 F1.25 S200 N25 M340 (only for axial disks) N26 G0 X150 Z50 M21 N27 M36 N28 G95 M9 N29 M30 NOTE: FUNCTIONS M20/M21 FOR USE OF THE SPINDLE BRAKE ARE OPTIONAL..
_____________________________________________________________________ Example of modal call-up (tapping of several holes): nr. 4 M8 at 90° N15 …. TURNING N16 M37 N17 G28 C0 N18 T606 (AXIAL TAPPING M8) N19 G54 N20 M341 (only for axial disks) N21 G94 N22 G0 X50 Z5 M7 N23 G66 P9103 Z-20 M303 F1.25 S200 N24 C0 M20 N25 C90 M20 N26 C180 M20 N27 C270 M20 N28 G67 N29 M340 (only for axial disks) N30 G0 X150 Z50 M21 N31 M36 N32 G95 M9 N33 M30 NOTE: FUNCTIONS M20/M21 TO USE THE SPINDLE BRAKE ARE OPTIONAL.
_____________________________________________________________________ 7.9 “O9104” RADIAL TAPPING SUB-PROGRAM Sub-program “9104” activates the radial tapping cycle. With this function the tapping tool enters with a feed equal to the tapping pitch, reverses the module rotation, followed by simultaneous acceleration of the motor driven tool and the axis then the returns to starting point. The axial tapping cycle contains these codes: • X => End of tapping absolute value • F => Tapping pitch ( in mm/rev.
_____________________________________________________________________ Example of single call-up (tapping of one hole only)(: N15 …. TURNING N16 M37 N17 G28 C0 N18 T707 (RADIAL TAPPING M8) N19 G54 N20 M341 (only for axial disks) N21 G94 N22 G0 X35 Z-15 M7 N23 C0 M20 N24 G65 P9104 X16 M303 F1.25 S200 N25 M340 (only for axial disks) N26 G0 X150 Z50 M21 N27 M36 N28 G95 M9 N29 M30 NOTE: FUNCTIONS M20/M21 TO USE THE SPINDLE BRAKE ARE OPTIONAL.
_____________________________________________________________________ Example of modal call-up (tapping several holes): N15 …. TURNING N16 M37 N17 G28 C0 N18 T707 (RADIAL TAPPING M8) N19 G54 N20 M341 (only for axial disks) N21 G94 N22 G0 X55 Z-15 M7 N23 G66 P9104 X37 M303 F1.25 S200 N24 C0 M20 N25 C90 M20 N26 C180 M20 N27 C270 M20 N28 G67 N29 M340 (only for axial disks) N30 G0 X150 Z50 M21 N31 M36 N32 G95 M9 N33 M30 NOTE: FUNCTIONS M20/M21 TO USE THE SPINDLE BRAKE ARE OPTIONAL.
_____________________________________________________________________ 7.10 G112 PROGRAMMING IN IMAGINARY CO-ORDINATES Function G112, used to program on the front surface, transforms the real co-ordinates into imaginary coordinates. C+ X+ X- CThe imaginary axes are obtained by interpolating real axes X and C. Therefore with G112 active, the control calculates the feed and the points needed to move the real axes along the imaginary components X C.
_____________________________________________________________________ The activation of function G112 does not involve movement of the machine axes, and the monitor shows the addresses of the new co-ordinates. The activation and deactivation functions of the milling radius offset (G41, G42 e G40) are only allowed after function G112 has been activated.
_____________________________________________________________________ Inside the G112 interpolation no fixed drilling or tapping cycles can be used. Example: Milling operation without using radius offset in G112: 60 60 10 N15 …. (TURNING OPERATION) N16 ….
_____________________________________________________________________ 7.11 CIRCULAR INTERPOLATION IN G112 The circular interpolations G2/G3 on the front surface (G112 active) can be programmed in two ways : - Coupling the value of radius R to the co-ordinates of end of interpolation X and C (method most commonly used).
_____________________________________________________________________ Where: • G2 / G3 => Circular interpolation direction clockwise/anti-clockwise • X => Co-ordinate of final point along axis X • C => Co-ordinate of final point along axis C • R => Radius of circular interpolation • I => Incremental co-ordinate along axis X • J => Incremental co-ordinate along axis C _____________________________________________________________________ CONCISE GUIDE FANUC 128
_____________________________________________________________________ 7.12 G41 G42 G40 MILLING RADIUS OFFSET IN G112 Also in milling, as for turning, the tool radius offset can be used . To do so, it is necessary to enter in the tool table the cutter radius (R) and the tool orientation (T), The value of this orientation can be either T0 or T9 (for the procedure to enter this data see the Concise Guide for Operator ).
_____________________________________________________________________ Example of milling operation with radius offset in G112: 80 80 6 N16 ….
_____________________________________________________________________ 7.13 “G107” CYLINDRICAL INTERPOLATION The cylindrical interpolation function G107 allows programming taking into consideration the total length of the plane of the side surface of a cylinder; therefore, this is very useful to program splines of cylindrical cams performed on the skirt of the workpiece (interpolating axes Z and C) and using a radial motor driven module.
_____________________________________________________________________ G107 C0 Cancels the cylindrical interpolation G107 The working plane is transformed in this way: - Functions G107C… and G107 C0 must be written in a block on their own - After instruction G107C… only functions G1 G2 G3 can be used, direct programming functions ,A ,C etc .
_____________________________________________________________________ Example of how to use function G107 (working a piece with diameter 55) N16 …. (TURNING OPERATION) N17 M37 (M237 for back spindle) N18 G28 C0 (G28 A0 for back spindle) N19 T101 N20 G54 (G55 for back spindle) N21 M303 S1500 N22 G94 F1000 N23 G1 G18 W0 H0 (G91 G18 Z0 A0 / G90 for back spindle) N24 G0 X 70 Z10 C0 M8 (A0 for back spindle) N25 G107 C27.
_____________________________________________________________________ N32 Z2 N33 G 107 C0 N34 G18 N35 G0 X200 Z100 N36 M305 N37 M36 (M236 for back spindle) N38 M95 N39 M30 _____________________________________________________________________ CONCISE GUIDE FANUC 134
_____________________________________________________________________ 7.14 PROGRAMMING WITH REAL Y AXIS Machines that have the axis Y option can make transverse movements of the turret of 64 mm (from –32 to +32). Through this option it is therefore possible to make radial machining that is not perpendicular to the centre of the workpiece (out of axis), for example drilling and tapping out of axis in relation to the centre of the workpiece.
_____________________________________________________________________ Example of how to use axis Y N15 ….
_____________________________________________________________________ N34 G1 Z-17 (P7) N35 G3 Z-10 Y-7 R7 (P8) N36 G1 Y-23 (P9) N37 G3 Z-17 Y-30 R7 (P10) N38 G1 Z-61 (P11) N39 G3 Z-68 Y-23 R7 (P12) N40 G1 Y-9 (P13) N41 G2 Z-77 Y0 R9 (P14) N42 G1 Z-83 (P15) N43 G3 Z-90 Y7 R7 (P16) N44 G1 Y23 (P17) N45 G3 Z-83 Y30 R7 (P18) N46 G1 Z-50 (P2) N47 G3 Z-43 Y23 R7 (P19) N48 G1 G40 Z-50 Y18 (P0) N49 G0 X80 N50 G18 N51 G0 Y0 Z100 N52 M305 N53 M36 N54 G95 N55 M30 ______________________________________________________
_____________________________________________________________________ 8.0 BAR MACHINING We have included in this chapter some examples of programs that use loaders, push bar conveyors, and an example using a pull-bar conveyor in a cycle for machine with and without back spindle. 8.
_____________________________________________________________________ T101 (TOOL FOR NEW BAR REFERENCE) G54 G97 M3 S50 M10 (ENABLE SPINDLE ROTATION WITH JAWS OPEN) G0 X0 Z5 M9 Z-47 M69 (OPEN SELF-CENTRING CHUCK/COLLET CHUCK) M67 (STAND-BY FOR LOADING NEW BAR SIGNAL) M68 (CLOSE SELF-CENTRING CHUCK/COLLET CHUCK) G4 U1 M11 (DISABLE SPINDLE ROTATION WITH JAWS OPEN) G0 X200 Z100 T505 (TOOL FOR NEW BAR FACING/PARTING OFF) G54 G92 S2500 G96 S120 M4 G0 X42 Z0.2 M8 G1 X-1 F0.
_____________________________________________________________________ 8.
_____________________________________________________________________ G4 U1 M11 (DISABLE SPINDLE ROTATION WITH JAWS OPEN) G0 X200 Z200 T505 (TOOL FOR FACING / PARTING OFF NEW BAR) G54 G92 S2500 G96 S120 M4 G0 X42 Z0.2 M8 G1 X-1 F0.
_____________________________________________________________________ 8.3 EXAMPLE OF MACHINE TOOL BAR-FEEDER CONVEYOR USE WITH BACK SPINDLE The example below shows the use of a single pipe push-bar conveyor for machine with back spindle.
_____________________________________________________________________ 8.4 EXAMPLE OF MACHINE TOOL BAR-FEEDER CONVEYOR USE WITHOUT BACK SPINDLE The example below shows the use of a single pipe push-bar conveyor for machine without back spindle..
_____________________________________________________________________ 8.5 EXAMPLE OF PULL-BAR CONVEYOR USE It is possible to carry out work from bars without using a bar loading system, using a special tool to extract the bar using the spindle axis Z . The example below shows how this tool can be used: N1 T202 (COMPLETE MACHINING OF ITEM) G54 G92 S2500 G96 S180 M4 G0 X32 Z0 M8 ……… G0 X200 Z100 T505 (PARTING OFF) G54 G92 S2500 G96 S120 M4 G0 X34 Z-32 M8 G1 X3 F0.
_____________________________________________________________________ G1 Z5 F1000 G0 X100 Z100 G95 M62 (INCREASE PIECE COUNTER) GOT01 M30 All tools, including the pull-bar conveyor have to be referred to the same point ( workpiece zero.
_____________________________________________________________________ 12.0 MACHINE START-UP Machine start-up consists in switching on and re-positioning axes, if required. 12.1 POWER-ON To switch on the machine, follow this procedure: 1 - Turn the main switch, on the front panel of the machine, to 1. 2 - Make sure that the two emergency red keys ("mushroom") have been raised.
_____________________________________________________________________ 13.0 PROGRAMME MANAGEMENT This chapter describes management of machining programmes. Management includes insertion, change and deletion of programme blocks as well as deletion, copying and renaming of programmes. 13.
_____________________________________________________________________ 13.5 HOW TO DELETE A CODE To delete a code in a programme, follow this procedure: 1 - By means of the arrow keys, position the cursor on the code to be deleted. 2 - Press the key DELETE 13.6 HOW TO DELETE A BLOCK To delete a block in a programme, follow this procedure: 1 - By means of the arrow keys, position the cursor on the block to be deleted. 2 - Press the key EOB 3 - Press the key DELETE 13.
_____________________________________________________________________ 7 - Press the soft key COPY. 8 - Press the soft key ALL. 9 - Type in the new programme number (without the character O) 10 – Press the key INPUT 11 - Press the soft key EXEC . 13.
_____________________________________________________________________ 13.12 HOW TO CREATE A NEW SUBPROGRAM The procedure followed when creating a subroutine is similar to the one used to create a programme. Subroutines and programmes are stored in the same memory. To make management easier, values should be included between O8001 and O9000 (main programmes range from O1 to O8000). Please note that all our subroutines end up with the function M99.
_____________________________________________________________________ 13.14 RUNNING OF THE PROGRAMME IN CYCLE To run a selected programme in cycle, press the key AUTOMATIC MODE placed on the operator’s panel, then press the key RESET if the programme has not been rewound; finally press START to start machining. For further details on how to run a programme in automatic mode, and on the function keys placed on the operator’s panel, read paragraph 19.1 13.
_____________________________________________________________________ 6 - Press the soft key FIN - BG 14.0 TOOL RESET Tool reset can be carried out following two different procedures described in this manual or by means of a tool-measuring probe in the machines equipped with this option. 14.1 MANUAL TOOL RESET 1 - Fix the rough piece on the chuck 2 - Press the key MDI MODE placed on the operator’s panel 3 - Press the key PROGRAM PAGE 4 - Enable the first external tool to be reset followed by its offset.
_____________________________________________________________________ 24- Position with the cursor on the corrector to reset 25- Write Z followed by the required value 26- press soft key MEASURE To reset the remaining tools for external machining, repeat the procedure described above touching the previously turned diameter or stop. 14.2 CENTRE RESET. The reset procedure in Z is similar to that used for turning tools. As to the X-axis, reset is not performed.
_____________________________________________________________________ (If a Manual Probe has been chosen extract the probe arm manually) When the probe is enabled, the CNC displays the correctors’ table automatically 5 – By means of the keys JOG Z- Z+ X- X+ and checking with the axes potentiometer, position the tool near the measuring probe 6 – Reduce the potentiometer to 1 or 2 % 7 – Lean on the desired probe X+ X- Z+ ZOnce contact has been achieved, the axis will stop automatically 8 – Move away from the
_____________________________________________________________________ 20 After the facing off of piece, move only with X axis staying on Z facing off co-ordinate 21 Stop the spindle with M5 and press EOB INSERT START 22 Press SETTING PAGE until compens.
_____________________________________________________________________ 6 - Press the soft key ENTER 14.10 ENTRY OF TOOL ORIENTATION Entry of tool orientation is required whenever radius offset is being used (G41, G42, G40).
_____________________________________________________________________ 15.0 ORIGIN MANAGEMENT This procedure is used to establish one or multiple reference points, thus allowing operators to have references for the movements to be entered in the machining programme. Such references are defined as piece origin. 15.1 ORIGIN MEASUREMENT This procedure is used to establish the piece origin when tools are reset on the probe or with an external measuring system.
_____________________________________________________________________ NB: by ABSOLUTE shift we mean the insertion of a new value, whereas ADDITIONAL shift refers to a value to be added to an existing one. 16.0 MACHINE PARAMETERS Machine parameters are used to fully represent the characteristics of servo-motors, as well as the specifications and the functions of the machine tool 16.
_____________________________________________________________________ 17.0 SETTING OF GT 300 TAILSTOCK This procedure only refers to the GT300 with tailstock option, since tailstock are moved differently in the other models.
_____________________________________________________________________ Press any page (EDITING, POSITION, SETTING etc.) to exit the TAILSTOCK SETTING macro NOTE: For further details on how to adjust the thrust pressure and the feed speed of the tailstock, see USER’S AND MAINTENANCE MANUAL included in the machine documents. 17.
_____________________________________________________________________ 18.0 TAILSTOCK AND REST MANAGEMENT ON MACHINES CTX Some machines CTX (400,500,700) are provided with option “tailstock with automatic clamping” and option “positionnable rest”. These options management may happen manually (trough selectors set on operator’s panel or with use of foot switches) or in working cycle ( with functions M). 18.
_____________________________________________________________________ REST M32 rest unclamping from the bed and clamp to the carriage M33 rest unclamping from the carriage and clamp to the bed M84 opening rest arms M85 closing rest arms In machines with option “positionnable retractable rest” you can use also the following functions: M86 retractable rest in working position M87 retractable rest in home position _____________________________________________________________________ CONCISE GUIDE FANUC 162
_____________________________________________________________________ 19.0 KEYBOARD AND OPERATOR’S PANEL The CNC keys can be divided into three categories: - Keys on the operator’s panel - Keys on the editing keyboard - Selector switches (on the operator’s panel) 19.
_____________________________________________________________________ STEP X1 (A6) Incremental movement 1/1000 STEP X10 (A7) Incremental movement 1/100 N.B. By pressing STEP X1 (A6) and STEP X10 (A7) simultaneously, you can obtain incremental movement 1/10 HOME (A8) Pressing this key, axes are positioned in the reference point (see paragraph 1.2).
_____________________________________________________________________ OPT STOP (B10) By pressing this key, you can enable or disable execution of the optional stop during machining. If this control is enabled, the machine will stop the machining process in the blocks of the programme where the M1 function has been entered. By pressing the key START the machine will start the machining process from the following block.
_____________________________________________________________________ COOL OFF (E5) By pressing this key, coolant is no longer supplied to tools COOL ON (E6) By keeping the key pressed, coolant will be supplied to tools. This key is used during machine tooling, to make sure that outlet nozzles are correctly oriented COOL AUTO (E7) By pressing this key you can enable or disable coolant supply to tools. Of course, M7 and M8 must be entered in the current programme.
_____________________________________________________________________ 19.
_____________________________________________________________________ RESET KEY Press this key to reset the CNC or to cancel alarms HELP KEY Press this key whenever you have doubts on one of the keys on the MDI panel or on the meaning of a CNC alarm. SOFT KEYS Soft keys may have different functions, depending on the applications. Their function is displayed at the bottom of the screen ADDRESS KEYS AND NUMBER KEYS Press these keys to enter alphanumeric characters or special characters.
_____________________________________________________________________ FUNCTION KEYS There are seven function keys referred to as pages: POSITION PAGE: This page is used to display absolute, relative and machining dimensions of the current machining process and of the manual shift. PROGRAMME PAGE : This page is used to manage programmes in EDIT MODE (i.e. you can write, modify or delete programmes) and to write the codes for the MDI MODE execution.
_____________________________________________________________________ 19.3 SELECTOR SWITCHES AND KEYS BELOW THE OPERATOR’S PANEL These keys are located below the operator’s panel; you can use them to enable or disable (depending on the options) different machine functions. MANUAL CONTROLS ENABLED By keeping this key pressed, machining can be carried out in JOG MODE or in MDI MODE even if the sliding guard is open (500 spindle revolutions max. and rapid speed at 20%).
_____________________________________________________________________ LAMP This selector switch is used to choose whether the tooling zone of the machine is to be lit up or not MACHINE POWER ON This key is used to turn on the machine (see Par. 12.
_____________________________________________________________________ 20.0 COMMUNICATION ON SERIAL PORT FANUC is equipped with a serial port complying with the RS232C standards. It can be used to communicate both with “intelligent” peripherals (e.g. computers) and with “dummy” devices (such as printers, tape recorders etc.). The parameters of the serial port and the connection diagram is described below. 20.
_____________________________________________________________________ COMPLETE CABLE CONNECTION (7wires) CONNECTOR SIDE PC CONNECTOR SIDE CNC 9 places female 25 places male RxD 2 ………………………………………………………………..2 TxD TxD 3…………………………………………………………………3 RxD DTR 4 ……………………………………………………………….6 DSR GND 5 ……………………………………………………………….7 GND DSR 6………………………………………………………………20 DTR RTS 7………………………………………………………………..5 CTS CTS 8……………………………………………………………….
_____________________________________________________________________ 20.3 TRANSFER PROGRAMS Here are some transfer programs tested on Graziano SPA machines with CN Fanuc. Suggested devices have been tested with a Graziano machine with PC Windows 95 have been tested many types of software of communication, with cable long 10 meters. Bigger distances are often possible but they are connected to the cable quality, connectors quality,and serial port of PC used.
_____________________________________________________________________ CONNECTION WITH CDS SOFTWARE This software is the program of communication standard for Graziano controls producted by PHILIPS /HEIDENHAIN (432,532,Pilot 1150) NAME = FANUC PORT = 1 PROTOCOL = PUN SPEED = 9600 CODE CHARACTER = ASCII TIME DELAY = 10 CNC VERSION = V200 NOTIFY = N NOTE: Press CTRL +PAUSE to interrupt the program at the end of reception and transmission.
_____________________________________________________________________ 20.4 HOW TO COPY A PROGRAMME ON MEMORY CARD To transfer a programme from the CNC memory to the RS 232C serial port, proceed as follows: 1 - Connect the memory card to that of Pc 2 - Press the key EDITING MODE on the operator’s panel 3 - Press PROGRAM PAGE 4 - Write the code 0 followed by desired program number (ex. 08000) 5 - Press the soft key + 6 - Press soft key WRITE 7 - Press the soft key EXEC 20..
_____________________________________________________________________ 20.7 HOW TO COPY A PROGRAMME FROM THE MEMORY CARD If you want to use the Memory Card to transfer and receive programmes, you first need to configure machine parameter n. 20 a 4 ( to modify a parameter see chap. 5) 1 - Insert the MEMORY CARD in the opening on left side of monitor 2 - Press the key EDITING MODE on the operator’s panel 3 - Press key PROGRAM PAGE 4 - Write code O followed by desired program number (ex.
