G00 RAPID POSITIONING MOTION

This G code is used for rapid traverse of the two axes of the machine from one program point to the next program point. The auxiliary (tailstock) B axis, can also be moved in rapid with a G00. This G code is modal so that all following blocks will be in rapid motion until another group 01 G code is specified. Generally, rapid motion done in both X and Z axes will not be in a straight line from one program location to the next program location. All the axes specified are moved at the maximum speed and will not necessarily complete each axis move at the same time. So you need to be careful of any obstructions to avoid with this type of rapid move. The tool will first move from the current position in a straight line along a 45 degree angle to an intermediate location, until one of these axes has completed its move. Then the machine will move parallel to the X or Z axis to complete the rapid move to the final location. These rapid moves may be in ABSOLUTE or INCREMENTAL coordinate command values which will change how those values are interpreted. The "U" letter address relates to X-axis incremental moves and the "W" letter address relates to Z-axis incremental moves. 

G01 LINEAR INTERPOLATION MOTION

This G code provides for straight line (linear) motion from point to point. Motion can occur in 1 or 2 axes. Both axes will start and finish motion at the same time to move the tool along a straight line path parallel to an axis or at a slope (angled) line. The speeds of all axes are controlled so that the feedrate specified is achieved along the actual path. The F (Feedrate) command is modal and may be specified in a previous block. These moves may be made in ABSOLUTE or INCREMENTAL coordinate command values which change how those values are interpreted. The "U" letter address relates to X-axis incremental moves, and the "W" letter address relates to Z-axis incremental moves. Only those axes specified are moved in either absolute X Z, or incremental U W commands. When feeding to a location using G01, it should be using a previously defined tool geometry “Txxyy” offset commanmd. The Txxyy code defines the tool and offset that are being used. This T command differs slightly depending on Setting 33 FANUC or YASNAC coordinate system. Most people set if for FANUC. When set to FANUC, xx is the tool number (any xx leading zero is ommitted); and yy is the tool geometry and wear offset that is being used for that tool. T101 would be recognized as tool 1 offset 1 and T323 would be recognized as tool 3 offset 23.

G02 CIRCULAR INTERPOLATION MOTION CW

Circular interpolation commands are used to move a tool along a circular arc to the commanded end position. Five pieces of information are required for executing a circular interpolation command: Plane selection, arc start position coordinates, rotation direction, arc end position coordinates, and arc center coordinates or arc radius. There are two ways to define a circular interpolation move. The first way is using I and K method, which defines the distance and direction from the start point to the arc center. The R method, is easier to define, and is the actual arc radius value your interpolating. When using I and K, it does not need to be entered in the porgram if either one has a zero value. It will be recognized as zero if it’s not listed in the G02 or G03 line. R: Using an R is the distance from the starting point to the arc center. With a positive R value, the control will generate a circular path of 180 degrees or less, but to generate a circular path of over 180 degrees, you specify a negative R. When feeding to a location using G02 or G03, it should be using a previously defined tool geometry “Txxyy” offset commanmd. The Txxyy code defines the tool and offset that are being used.

G03 CIRCULAR INTERPOLATION MOTION CCW

G03 will generate counterclockwise circular motion but is otherwise defined the same as G02 clockwise circular motion. Circular interpolation commands are used to move a tool along a circular arc to the commanded end position. Five pieces of information are required for executing a circular interpolation command: Plane selection, arc start position coordinates, rotation direction, arc end position coordinates, and arc center coordinates or arc radius. There are two ways to define a circular interpolation move. The first way is using I and K method, which defines the distance and direction from the start point to the arc center. The R method, is easier to define, and is the actual arc radius value your interpolating. When using I and K, it does not need to be entered in the porgram if either one has a zero value. It will be recognized as zero if it’s not listed in the G02 or G03 line. R: Using an R is the distance from the starting point to the arc center. With a positive R value, the control will generate a circular path of 180 degrees or less, but to generate a circular path of over 180 degrees, you specify a negative R. When feeding to a location using G02 or G03, it should be using a previously defined tool geometry “Txxyy” offset commanmd. The Txxyy code defines the tool and offset that are being used.

G28 FANUC RETURN TO MACHINE ZERO THROUGH REFERENCE POINT

The G28 code is used to return to the machine zero position on all axes. If an X or Z axis is specified on the same block, only those axes will move and return to the machines’ zero point. If X or Z specifies a different location than the current position, then the movement to machine zero will be through the specified point. If no X or Z is specified, all axes will be moved directly to machine zero, along with the tailstock, B axis (for the machines that have a tailstock). If you do not want to position through an intermediate point while specifying an X or Z axis to position to machine home, than use an incremental U0 and/or W0 command for the specific axis that you want to send to machine zero. This will command those axis specified to position incrementally to a zero distance as an intermediate point, and then those axes specified will go directly to machine zero. G28 will not recognize any tool length offsets in this move, though the offset is not cleared. The tool offsets will not be cleared until a T0, M30, Reset, or a new offset is called up. The G28 command will send turret in the X and Z axes to machine home along with tailstock. If the tailstock is home not being used, then this is not a problem. If tailstock is being used, and is in holding a part, you may not want to send the tailstock home when a G28 is on a line in a program. To command only the turret to go home, and not the tailstock, program in G28 U0 W0 to send only the X and Z axes home and the tailstock will remain in place.

G40 TOOL NOSE COMPENSATION CANCEL

G40 cancels G41 or G42. Programming Txx00 or just T0 will also cancel tool nose compensation. You must always cancel tool nose compensation before the end of a program. The G40 departure move, off of the part, usually does not correspond with any point on the part. In many cases overcutting or undercutting could occur if tool is still on the part when you cancel cutter compensation. 

G41 TOOL NOSE COMPENSATION LEFT

G41 will select tool nose compensation left; that is, the tool is programmed to the left of a tool path part line, to compensate for the tool tip radius. A tool offset must be selected with a Tnnxx code, where xx corresponds to the offsets that are to be used for the nn tool turret location.

G42 TOOL NOSE COMPENSATION RIGHT

G42 will select tool nose compensation right; that is, the tool is programmed to the right of a tool path part line, to compensate for the tool tip radius. A tool offset must be selected with a Tnnxx code, where xx corresponds to the offsets that are to be used for the nn tool turret location.

G50 SPINDLE SPEED CLAMP

Spindle speed, on any CNC lathe, is limited by the maximum permissible speed of the power chuck. The effects of centrifugal force on its gripping force, unbalanced condition of the workpiece causing machine vibration, and so on, can be constrained by programming a G50 code at the start of each tool. G50 can be used to clamp the maximum spindle speed. The control will not allow the spindle to exceed the S address value specified in the most recent G50 command. This is most often used in constant surface feed mode G96. N1 G50 S2500 ; (SPINDLE RPM WILL NOT EXCEED 2500 RPM) N2 G96 S390 M03 ; (ENTER CONSTANT SURFACE SPEED MODE, SPINDLE ON) The MAXIMUM spindle speed is designated by the "S" word along with the preparatory G50 command with the "S" word in the same block with no other commands. Once the MAXIMUM spindle speed is established, any direct RPM programmed in G97 (direct revolution per minute) or control calculated RPM from the G96 (constant surface footage mode) that exceeds the RPM established by the G50 block, is ignored and the G50 S word spindle speed is used. The second use of G50 is for older equipment that does not have work zero and geometry offset capabilities. This will not be covered in this workbook because it’s not desirable anymore because it’s not as easy to use as what is now available. 

G70 FINISHING CYCLE

P Starting block number of the part geometry to machine Q Ending block number of the part geometry to machine The G70 Finishing cycle can be used to finish cut paths that are defined and roughed out with stock removal cycles G71, G72 and G73. The G70 requires that a beginning block number (P code) and an ending block number (Q code) be specified for the machine code that defines the part geometry to be machined. The G70 cycle is usually used after a G71, G72 or G73 has been performed using the blocks specified by P and Q. All codes in the block defined by P and Q are executed. Any F, S or T codes between the P and Q block are effective. The PQ sequence is searched for in the current program starting from the beginning of the program. The current machine position is saved and remembered as the start position. Then the block starting at P is executed. Processing continues in a normal fashion with blocks following P until a block is found and executed that contains an N code that matches the Q code in the G70 calling block. After execution of the Q block, a rapid (G00) is executed returning the machine to the start position that was saved earlier during G70 initialization. The program then returns to the block following the G70 call. 

G71 O.D./I.D. STOCK REMOVAL CYCLE

This canned cycle will rough out material on a part defining the finished part shape. All a programmer needs to do is to define the shape of a part by programming the finished tool path and then submitting the part path definition to the G71 call by means of a PQ block designation. Any feeds, spindle speed, or tool offset commands on the blocks defining the path are ignored by the G71 call. Any F, S or T commands on the G71 line, or the active ones at that time of the G71 call, are used throughout the G71 roughing cycle. A call to the same PQ block using a G70 will finish the part path with the programmed feeds, speed and offsets that are defined within the PQ block definition. 

G72 END FACE STOCK REMOVAL CYCLE

This canned cycle will rough out material on a part given the finished part shape. It is similar to G71 but roughs out material along the face of a part. All a programmer needs to do is to define the shape of a part by programming the finished tool path and then submitting the path definition to the G72 call by means of a PQ block designation. Any feeds, spindle speeds or tools within the block defining the path are ignored by the G72 call. Any F,S or T commands on the G72 line or in effect at the time of the G72 is used throughout the G72 roughing cycle. Usually a G70 call to the same PQ block definition is used to finish the shape using the programmed feeds, speeds tools and offsets. 

G76 O.D./I.D. THREAD CUTTING CYCLE, MULTIPLE PASS

The G76 canned cycle can be used for threading both straight or tapered (pipe) threads. With G76 a programmer can easily command multiple cutting passes along the length of a thread.

G80 CANNED CYCLE CANCEL

This G code is modal in that it deactivates all canned cycles until a new one is selected.

Note: The use of a G00 or G01 will also cancel a canned cycle.

G96 CONSTANT SURFACE SPEED ON

A G96 commands the control to maintain a constant surface speed, with the spindle speed and where the tool tip is relative to the part diameter. Surface speed is based on the distance of the tool tip to the spindle centerline. This is the radius of cut. Surface speed is maintained by adjusting the spindle speed based on the radius of cut. The current S code is used to determine the surface speed. G96 is modal. 

The formula the machine performs while machining up or down a diameter with G96 on a part is calculating this formula: (SFM x 3.82) Dia. = RPM Example on a 3/4 part diameter: (225 x 3.82) .750 = 1146

G97 CONSTANT SURFACE SPEED OFF / REVOLUTION PER MINUTE ON

A G97 commands the control to not adjust the spindle speed based on the radius of cut. This command will cause the spindle to be at a constant speed. It will cancel any current G96 command. When G97 is actively on, any S command is in revolution per minute (RPM). G97 is modal. 

The formula to find out what surface speed when machining on a part diameter, when the machine is at a constant spindle speed: Diameter x .2618 x RPM = SFM The surface speed for a 5/8 drill at a 1400 spindle speed is: .625 x .2618 x 1400 = 229.075 

G98 FEED PER MINUTE

This command changes how the F address code is interpreted. The value of F indicates inches per minute when Setting 9 is set to INCH, and F indicates millimeters per minute when Setting 9 is set to METRIC. This code is modal. IPM = CURRENT RPM x IPR

G99 FEED PER REVOLUTION

This command changes how the F address is interpreted. The value of F indicates inches per revolution of the spindle when Setting 9 is set to INCH, while F indicates millimeters per revolution of the spindle when Setting 9 is set to METRIC. This code is modal, and is the default feed mode. IPR = IPM : CURRENT RPM