G89 Boring cycle

 

                                                    The Gcode G89 Boring canned cycle with dwell is used for boring and reaming operation. The G89 boring cycle is same as G85, but the difference between these two cycles is the G89 will use Dwell at bottom. Some times for boring operations, when the feedrate is required for the IN and the out directions of the machined hole, with a specified dwell at the bottom of the hole G89 is used.

Code line for G89 Boring cycle with dwell:

N100 G98 (G99) G89 X… Y… R… Z… P… F…

Diagram for G89 Boring cycle with dwell:

Steps for the G89 Boring cycle with dwell:

• Rapid motion to XY position of the hole position.
• Rapid motion to the R level, i.e., to the top of the hole position.
• Feedrate motion to the depth in Z.
• Dwell at the depth – in milli seconds (P).
• Feedrate motion to Z depth.
• Rapid retract to the initial level (with G98) or Rapid retract to R level (with G99).

G88 Boring cycle

                                                        The G88 boring is used rare, its use is limited to boring operations with special tools that requires manual interface at the bottom of the hole.  When this operation is completed, the tool is moved out of the hole for safety reasons. This cycle is used by some tool manufactures for certain operations.

Code line for G88 Boring cycle Spindle stop:

N100 G98 (G99) G88 X… Y… R… Z… P… F…

Diagram for G88 Boring cycle Spindle stop:

Steps for the G88 Boring cycle Spindle stop:

 1.       Rapid motion to XY position of the hole position.

       2.       Rapid motion to the R level, i.e., to the top of the hole position.

       3.       Feedrate motion to the depth in Z.

       4.       Dwell at the depth – in milli seconds (P).

       5.       Spindle rotation STOP (Feed hold condition is generated and the CNC operator switch's to manual operation mode and performs a manual task, then switches back to memory mode). CYCLE START will return to normal cycle.

        6.       Rapid retract to the initial level (with G98) or Rapid retract to R level (with G99).

        7.       Spindle rotation ON.

G87 Back Boring cycle

                                                            The G87 Back Boring cycle is a special cycle, its practical usage is limited due to the special tooling and setup requirements. Use the G87 Cycle only if the total costs can be justified economically. The boring bar must be set very carefully, it must be preset to match the diameter required for backboring, its cutting point must be set in the spindle oriented mode, facing the opposite direction than the shift direction.

Code line for G87 Back Boring cycle:

                There are two program formats available for the G87 back boring canned cycle. Unfortunately G99 is never used with the G87 cycle.

First one using the Q, which is commonly used:

N100 G98 G87 X… Y… R… Z… Q… F…

Second one using I and J:

N100 G98 G87 X… Y… R… Z… I… J… F…

Diagram for G87 Back Boring cycle:

Steps for the G87 Back Boring cycle:

 1.       Rapid motion to XY position of the hole position.

       2.       Spindle Rotation Stop.

       3.       Spindle Orientation.

       4.       Shift OUT (OSS) by the Q value or shift by the amount and direction of I and J.  

       5.       Rapid motion to the R level, i.e., to the bottom of the hole position.

       6.       Shift IN (OSS)by the Q value or shift back in the opposite direction of I and J. 

       7.       Spindle rotation ON (M03).

       8.       Feedrate motion to the depth in Z.

       9.       Spindle rotation STOP.

      10.   Spindle orientation.

      11.   Shift OUT (OSS) by the Q value or shift by the amount and direction of I and J. 

      12.   Rapid motion to the Initial level, i.e., to the top of the hole position.

      13.   Shift (OSS) IN by the Q value or shift back in the opposite direction of I and J. 

      14.   Spindle rotation ON.

G76 Precision Boring cycle

                                            The G76 is a very use full cycle for high quality holes. Same as G87 there are two programming formats available for the precision boring canned cycle G76.

Code line for G76 Precision Boring cycle:

                There are two program formats available for the G76 back boring canned cycle.

First one using the Q, which is commonly used:

N100 G98 (G99) G76 X… Y… R… Z… P… Q… F…

Second one using I and J:

N100 G98 (G99) G76 X… Y… R… Z… P… Q… F…

Diagram for G76 Precision Boring cycle:

Steps for the G76 Precision cycle:

1.       Rapid motion to XY position of the hole position.

      2.       Rapid motion to the R level. I.e., to the top of the hole.

      3.       Feed motion in the Z till the end of the hole.

      4.       Dwell at depth – in Milliseconds (P)

      5.       Spindle Rotation Stop.

      6.       Spindle Orientation.

      7.       Shift OUT (OSS) by the Q value or shift by the amount and direction of I and J. 

      8.       Rapid motion to the R level, i.e., to the top of the hole position.

      9.       Spindle rotation ON (M03).

     10.   Rapid retract to the initial level (with G98) or Rapid retract to R level (with G99).

G86 Boring cycle

                                                          The G86 Boring cycle spindle stop Work similar to the G85 Boring cycle or the G81 Drilling cycle, But the difference is there will be no retract in the feedrate motion. In some cases Using G85 for boring tool may make the finish of the hole worse rather than improving because of removal of material in backward motion. In this G86 cycle the spindle is stopped as the depth of the hole is reached and the tool is retracted in rapid. This cycle is typically used for Roughing and semi finishing of the Holes.

Code line for G86 Boring cycle Spindle stop:

N100 G98 (G99) G86 X… Y… R… Z… F…

Diagram for G86 Boring cycle Spindle stop:

Steps for the G86 Boring cycle Spindle stop:

 1.       Rapid motion to XY position of the hole position.

       2.       Rapid motion to the R level, i.e., to the top of the hole position.

       3.       Feedrate motion to the depth in Z.

       4.       Spindle rotation STOP.

       5.       Rapid retract to the initial level (with G98) or Rapid retract to R level (with G99).

G85 Boring cycle

                                                   The G85 Boring cycle is used for boring and reaming operations. This cycle is used to improve the surface finish of the hole to meet the high dimension tolerance or the concentricity of the hole. This operation carries out the tool in and out of the hole without spindle stop. Point to be noted in this operation is a little amount of material will be removed during the tool is feeded backwards out of the hole, this happens because of the released tool pressure during retract.  This cycle is especially suitable for reaming.

Code line for G85 Boring cycle:

N100 G98 (G99) G85 X… Y… R… Z… F…

Diagram for G85 Boring cycle:

Steps for the G85 Boring cycle:

 1.       Rapid motion to XY position of the hole position.

       2.       Rapid motion to the R level, i.e., to the top of the hole position.

       3.       Feedrate motion to the depth in Z.

       4.       Feedrate motion back to the R level.

       5.       Rapid retract to the initial level (with G98) or Rapid retract to R level (with G99).

G74 Reverse Tapping cycle

                                        The G74 Gcode cycle is the standard reverse tapping cycle used for the Left hand thread in a hole. At the start of the cycle the Reverse spindle rotation M04 must be In effect.  The machine switches on the control panel cannot be accessed until the cycle of thread is completed. As said in G84 the spindle speed and the feed of the lead thread is very important, these relationship must be maintained at all the times of the tapping cycle.

Code line for G74 Tapping cycle:

N100 G98 (G99) G74 X… Y… R… Z… F…

Diagram for G74 Tapping cycle:

The cycle is the standard reverse tapping cycle used for the Left hand thread in a hole. At the start of the cycle the Reverse spindle rotation M04 must be In effect.  The machine switches on the control panel cannot be accessed until the cycle of thread is completed. As said in G84 the spindle speed and the feed of the lead thread is very important, these relationship must be maintained at all the times of the tapping cycle

Steps for the G74 Tapping cycle:

 1.       Rapid motion to XY position of the hole position.

       2.       Rapid motion to the R level, i.e., to the top of the hole position.

       3.       Feedrate motion to the depth of the thread in Z with CCW Spindle rotation (M04).

       4.       Spindle rotation stop in bottom of hole.

       5.       Spindle Clockwise rotation (M03) and back in feedrate to R level.

       6.       Spindle rotation Stop.

       7.       Spindle rotation Reverse (M04) and Rapid retract to the initial level (with G98) or Rapid retract to R            level (with G99).

G84 Tapping cycle

                                        The G84 Gcode tapping cycle is the standard tapping cycle used for the right hand thread in a hole. At the start of the cycle the normal spindle rotation M03 must be In effect.  For tapping always R Level must be higher compared to the other cycles. The feedrate and the spindle speed calculation very important for the tapping cycle since there is a direct relationship between the spindle speed and the lead of the tap.

Code line for G84 Tapping cycle:

N100 G98 (G99) G84 X… Y… R… Z… F…

Diagram for G84 Tapping cycle:

Steps for the G84 Tapping cycle:

 1.       Rapid motion to XY position of the hole position.

       2.       Rapid motion to the R level, i.e., to the top of the hole position.

       3.       Feedrate motion to the depth of the thread in Z with Clockwise Spindle rotation (M03).

       4.       Spindle rotation stop in bottom of hole.

       5.       Spindle reverse rotation (M04) and back in feedrate to R level.

       6.       Spindle rotation Stop.

       7.       Spindle rotation normal (M03) and Rapid retract to the initial level (with G98) or Rapid retract to R              level (with G99).

G73 Chip break Drilling cycle

                                             The gcode G73 chip breaking cycle works same as deep hole drilling cycle G83and is also known as peck drilling cycle. But In this cycle the drill will not be retracted to the clearance position of the hole, the drill will retract only to specified height after drilling the certain depth of cut keeping the drill inside the hole. This cycle retracts to the specified height after each peck of drill and repeated until the total depth of the hole is achieved.

                The cycle G73 is used for the long series of the drills where we can expect the vibration of the tool and it can damage the hole and the tool. G73 cycle keeps the tool inside the hole until the drilling operation is completed and saving the time on the cycle.

Code line for G73 Chip break drilling cycle:

N100 G98 (G99) G73 X… Y… R… Z… Q… F…

Diagram for G73 Chip break drilling cycle:

Steps for the G73 Chip break drilling cycle:

 1.       Rapid motion to XY position of the hole position.

       2.       Rapid motion to the R level, i.e., to the top of the hole position.

       3.       Feedrate motion to the depth by the amount of Q value in Z.

       4.       Rapid retract to Clearance value Specified.

       5.       Feedrate motion in Z axis by the Q amount plus the clearance value.

       6.       Point number 4 and 5 repeated until the z depth of the hole is reached.

       7.       Rapid retract to the initial level (with G98) or Rapid retract to R level (with G99).

G83 Deep hole Drilling cycle

                        The deep hole drilling cycle (Standard Peck Drilling) is also known as peck drilling cycle. In this cycle the drill will be retracted to the clearance position of the hole after drilling the certain depth of cut. After retracting to clearance plane, this cycle retracts to the R level after each peck of drill and repeated until the total depth of the hole is achieved.

Code line for G83 Peck drilling cycle:

N100 G98 (G99) G83 X… Y… R… Z… Q… F…

Diagram for G83 peck Drilling cycle:

Steps for the G83 peck drilling cycle:

      1.       Rapid motion to XY position of the hole position.

      2.       Rapid motion to the R level, i.e., to the top of the hole position.

      3.       Feedrate motion to the depth by the amount of Q value in Z.

      4.       Rapid retract to R level.

      5.       Rapid motion to the previous drilled depth with clearance.

      6.       Point number 3, 4 and 5 repeated until the z depth of the hole is reached.

      7.       Rapid retract to the initial level (with G98) or Rapid retract to R level (with G99).

G82 Drilling cycle with dwell

                              The Gcode G82 Drilling cycle is work same as drilling cycle G81 but with dwell. Dwell is used for the some of the improve accuracy of the hole. During drilling with dwell the tool pauses at the hole bottom. These cycle is used for center drilling, spot drilling, spot facing, countersinking etc.

Code line for G82 Drilling cycle:

N100 G98 (G99) G82 X… Y… R… Z… P… F…

Diagram for G82 Drilling cycle with Dwell:

Steps for the G82 drilling cycle:

        1.       Rapid motion to XY position of the hole position.

        2.       Rapid motion to the R level, i.e., to the top of the hole position.

        3.       Feedrate motion to the depth of the hole in Z.

        4.       Dwell at the bottom of the hole. In milliseconds (P).

        5.       Rapid retract to the initial level (with G98) or Rapid retract to R level (with G99).

G81 Drilling cycle

                  The drilling cycle gcode G81 is canned cycle and is a simple drilling cycle used for drilling the hole without the dwell at the depth of the hole is not required. Mainly this cycle is used for the center drilling and the holes with small depth.

Code line for G81 Drilling cycle:

 N100 G98 (G99) G81 X... Y... R... Z... F...

Diagram for G81 Drilling cycle:

Steps for the G81 drilling cycle:

 1.       Rapid motion to the XY position of the hole position.

       2.       Rapid motion to the R level, i.e., to the top of the hole position.

       3.       Feedrate motion to the depth of the hole in Z

       4.       Rapid retract to the initial level (with G98) or Rapid retract to R level (with G99).

Fixed Cycles or canned cycles

                                  On the CNC Milling and machining centers the most common operation done is the drilling, tapping and boring the holes. The standard center drilling, spot drilling and drilling are used together with related operations such as reaming, tapping, single point boring, countersinking and counter boring operations. Always machining a simple hole requires only a single drill but the complex hole may require several tools to be completed.   All CNC control manufacturers have incorporated the programming methods for machining holes in their control systems. These methods are called canned cycles or fixed cycles. Machining holes are operated with point to point machining; the detailed of Point to point machining is explained as below:

POINT-TO-POINT Machining:

                While machining the holes actual cutting takes place is along a single axis i.e., the Z=axis. This type of machining is commonly called as point-to-point machining. This method involves the rapid motion in X and Y-axis for positioning to centre of hole and then the cutting take place in Z-Axis with machining federate.  Some motions along Z axis may also include rapid motion till the tool reaches the part for machining hole. The programming structure for point to point machining can be grouped into four general steps as shown below:

Step1: Rapid motion to the hole position along X and/or Y-axis.

Step2: Rapid motion to the starting point of the cut along the Z axis.

Step3: Feedrate motion to the specified depth along Z axis

Step4: Return to a clear position along the Z axis.

                These four steps represent the minimum number of blocks required to program a drilling for a single hole using manual programming method, without using fixed cycles or canned cycles. If you have one or two holes in a part with same diameter then the program is very simple with the minimum tool. Suppose you have a more holes with different diameter then we may have to call more tools  to finish all the holes.

Fixed Cycles or canned cycles:

                Most of the time consuming task in programming point to point operation is the repetitive information written in the program, this can be overcome by using the fixed cycles, here once the drilling cycle is called and the next the inputting the  position of holes is enough, the controller repeats the drilling cycle until it is cancelled by the G-code. This method is called the canned or fixed cycle.

                The canned cycle is designed by the control manufacturers to eliminate the repeated data in manual programming and allow an easy program data changes at the machine. A number of identical holes may share the same starting point, same feedrate and the same depth, only the X and Y coordinates are different for each hole on the part. The specified values become modal for the duration of the cycle and do not have to be repeated, unless there is a change in them.

These canned cycles are called in the program by a G command as following canned or fixed cycles.

 G73 = High speed peck drilling cycle.

G74 = Left hand Tapping cycle.

G76 = Boring cycle

G80 = cancel of any kind of canned cycles.

G81 = general drilling or simple drilling cycle.

G83 = Peck drilling cycle.

G84 = Right hand tapping cycle.

G85 = Simple Boring Cycle.

G86 = Boring cycle with spindle stop

G87 = Back boring cycle.

Programming Format for the canned cycle:

General format for the canned cycle is a series of values specified by the unique address. The format is as shown below:

N... G... X...Y... R... Z... P... Q... I... J... F... K…

Whereas,

N = Block Number

G= Cycle Number eg: G81, G83 etc.

X = Hole position in X-axis

Y= Hole position in Y-Axis

R = Start position or the return Level

Z= depth of the hole

P= Dwell time (1s=1000ms)

Q = Depth of the peck drill

I = shift amount in X-direction for boring cycles.

J= shift amount in Y-direction for boring cycles.

F= Feed rate

K = number of repetitions.

Programming example for Point to point position and canned cycles:

Manual Programming with Points:                                    Programming with Fixed cycles or canned cycles:

O1000                                                                           O1000

N100 G20 G17 G40 G80                                               N100 G20 G17 G40 G80

N101 G90 G54 G00 X5.9 Y1.89 S1000 M03                N101 G90 G54 G00 X5.9 Y1.89 S1000 M03

N102 G43 Z1 H01 M08                                                 N102 G43 Z1 H01 M08

N103 Z0.5                                                                     N103 G99 G81 R0.5 Z-2 P300 F5

N104 G01 Z-2 F5                                                          N104 X3.87 Y3.4

N105 G04 P300                                                            N105 X2.047

N106 G00 Z0.5                                                             N106 G80 G28 Z0 M09

N107 X3.87 Y3.4                                                          N107 M30

N108 G01 Z-2 F5

N109 G04 P300                                                                                 

N110 G00 Z0.5

N111 X 2.047

N112 G01 Z-2 F5

N113 G04 P300 

N114 G00 Z0.5 M09

N115 G28 Z0

N116 M30

General rules to be followed by the fixed cycles or canned cycles:

è Absolute or incremental mode can be programmed anytime in the fixed cycle or before the fixed cycle. i.e., G90 for absolute mode and the G91 for Incremental mode

è If both X and the Y-axis Omitted in the canned cycle mode then the cycle will be executed at the current position of the tool. If one of the axis is omitted, the cycle will be executed in the specified location of one axis, without changing the other axis.

è If you miss to select G98 or G99, the control system will select the default command set ny a system parameter, usually G98 is default command.

è Address P for the dwell cannot be used with the decimal points, dwell is always programmed in milliseconds.

è The command G80 should be always used to cancel the canned cycles, no any other canned cycles can be called in the same line. 

Canned or fixed cycle cancellation

Any canned or the fixed cycle that is active can be cancelled with the G80 Gcode command. When the machine calls the G80 Gcode the control mode is automatically transferred to the rapid motion mode G00.

Code line for G81 Drilling cycle:

N100 G98 (G99) G81 X... Y... R... Z... F...

N110 G80      (Canned cycle cancel)

N120 G0 Z…   (To the safety plane) 

CNC MACHINING CENTERS

                    The machining centre is a machine tool which is capable of doing multiple machining operations on a work part in a single setup. Recent CNC machining centers are equipped with lot of feature which can increase the production and time saving. Time saving on CNC is a huge profit for the company.

The machining center designation refers to the orientation of the machine spindle, and is classified as below:

1. Vertical Machining centers (VMC).
2. Horizontal Machining centers (HMC).
3. Universal Machining centers (UMC).

1. Vertical machining centre (VMC):

These machines have its spindle on a vertical axis relative to the work table and always perpendicular to the machining bed. A vertical machining centre (VMC) is typically used for flat work that requires tool access from top. E.g. mould and die cavities, large components of aircraft. Vertical machining centers are limited for the small type of components. These machines are less expensive compared to the other machining centers.

Axes Designation in vertical machining centers is as shown below:

    2. Horizontal machining centre (HMC):

This type of machines have the Z axis in the horizontal position and the part is loaded on the table vertically in X and Y direction. Horizontal machining centers are used for machining the cube shaped parts where tool access can be best achieved on the sides of the cube. The number of setups can be reduced compared to the Vertical machining centers.  Some horizontal machining centers have their bed in X and Y axis perpendicular to the spindle and some have in X and Z axis parallel to the spindle.

Axes Designation in vertical machining centers is as shown below:

               3.  Universal machining centre (UMC):

These machines are the machines which has 5 or more axis. It has a work head that swivels its spindle axis to any angle between horizontal and vertical making this a very flexible machine tool.  The complex parts like Aerofoil shapes, curvilinear geometries can be machined using these universal machining centers. These machines works on the swivels spindle axis which is called pivot point. Most of these machines are used for finishing of parts due to achieving of high accuracy. 

Advantages of machining centers:

·         Reduced setups which gains the time and saves the machining cost.

·         Reduced part handling by the operator, due to reduced setups.

·         The parts utilize the same fixture throughout their processing which Increases the accuracy and repeatability.

·         Faster process and faster delivery of parts in small lot sizes.

Disadvantages of machining centers:

·         These machines are more expensive compared to other conventional machines.

·         Need highly skilled and trained labors to operate these machines.

·         Needs software’s for DNC, Simulation and CAM programming, which makes the cost higher to use these machines.

Features of CNC machining centers:

Usually the CNC machining centers are designed with many features to reduce non productive time. Some of the features are:

                      1.       Automatic tool changer (ATC).
                2.       Automatic work part positioned.
                3.       Automatic pallet changer.

       1.       Automatic tool changer (ATC):

                        The Cutting tools are stored in the storage unit called the “tool magazine” which is integrated with the machine tool and named with the tool numbers. When a tool number is called by the tool number the magazine rotates to the proper position and an automatic tool changer (ATC) with the program control, exchanges the tool in the spindle for the tool in the tool storage unit. The Capacities of tool magazine commonly range from 16 to 80 cutting tools. These Automatic tool changes save the manual tool changing and the big save on the cycle time or the operation time.

      2.       Automatic work part positioned:

                      Automatic work part positioning acts as rotary axis rotating the part and give access to the cutting to machine, many horizontal and vertical machining centers have the capability to orient the work part relative to the spindle. The table can be oriented at any angle about a vertical axis to permit the cutting tool to access almost the entire surface of the part in a single setup. These automatic work part positions are programmed by the programmer. The positioning of the rotation is very important the tool need to move to safety plane when there is a big rotation in the rapid. With these features we can reduce the number of setups and save huge time and gain increase in productivity.

       3.       Automatic pallet changer:

                    Recent modern Machining centers are equipped with two (or more) separate pallets that can be changed using an automatic pallet changer. While machining is performed with one pallet in position at the machine, the other pallet is in a safe location out of the machine. The operator can unload the finished part and then fixture the raw work part for next cycle with the pallet outside the machine. Using these automatic pallet changers the time of loading and unloading the part can be saved and the machine will be loaded continuously. These featured machines are very helpful in mass production activity.

Enjoy learning CNC Programming.

Classification of CNC control systems

            The CNC control systems can be classified based on below types:

1.      Motion type CNC

1.1.   Contouring systems

1.2.   Point to point systems

2.      Control  loop CNC

2.1.   Closed loop system

2.2.   Open loop system

3.      Number of axis type CNC

3.1.   2-axis machines

3.2.   2.5 axis machines

3.3.   3 axis machines

3.4.   4 axis machines

3.5.   5 axis machines and above.

1.     Motion type CNC Control:

            Based on the basic difference of the machine to be controlled there are two types of machine tools and control system. “Contouring systems” and “Point to point control system”.

1.1   Contouring system:

This type of machine tools works in a continuous path by cutting the material and following a contour of the part.  These machine tools are known as contouring machines which includes Milling, lathe and routing machines. These contouring machines are also capable of doing the work same as point to point system. These contouring system machines require simulations movement of the tool and the work piece i.e., the positions of the work piece and the tool are simultaneously controlled by a control system. These machines are uneconomical if it’s used as only point to control without continuous motions.  The contouring motion works as below shown in figure.

1.2   Point to point control system:

The work piece and the tool are placed in the position and the tool does its work. These types of machines are called point to point systems.  The drilling, tapping and boring machines are characterized under these types. The work piece is not moved until the tool finishes the job and retracts to the safety.  The point to point control system works as shown in the below figure.

2.     Loop control CNC systems:

Based on the looping system the CNC systems are classified into two categories, “Open loop system” and “closed loop system”.

2.1   Closed Loop system:

Since this type of system has feedback from the control system to the actual and the programmed input we call it as closed loop system. The CNC systems works on servo mechanism and it’s a closed loop principle. The feedback can be measured by analog or the digital systems. The analog systems measure the physical variables such as position and velocity in terms of voltage levels and digital systems monitor by electrical pulses.  These closed loop systems are accurate and powerful because of their capability of monitoring operational condition through feedback systems and automatically adjusting the variations in real time.

2.2   Open Loop system:

Open loop system are the systems in which instructions of program are sent into the controller through the input device and then these instructions are converted to the signals by the controller and sent to the servo amplifiers to energize the servo motors. The open loop systems are usually used in the point to point control systems where the accuracy doesn’t matter much and in few continuous path control system since there is no feedback from the system the result may deviate from the actual.

3.     Number of axis type CNC Control:

3.1   Two axis control system:

Two axis control system is a machine which give access to only two axis. The best example is the lathe machine.  The machine driven with the servo motor allows you only 2 axis, i.e., X and the z Axis.  Here in lathe the job will be rotating and the tool will be moving in 2 directions, indicating the depth Z and the cut in X direction.  So the program is done with x and the Z direction, where as in lathe universally use U and V which is implies same as X and Y.

3.2   Two and half axis control system:

Two and half axis control system  is also a three axis machine but the movement will not be 3 dimensional. These are the best example for drilling and tapping machines. First the X and the Y axis are moved to the position and then the third axis comes to effect.  In some of the machines the first X movement is made and the Y movement to reach the XY destination when it is in rapid, But while in feed or machining mode it does its work with 2 dimensional moving along x and y simultaneously, These type of machines may also called as two and half axis machines or 2.5 axis machine.

3.3   Three axis control system:

Three axis control systems are the machines which moves in three dimensional i.e., X, Y and Z axis move simultaneously. These are the most popular machines which can produce high accurate precision parts with three axis machines. The servo motor control the movements as per the instructions are given.  The three axis has verity of machines based on their bed lengths.  As the bed length increases the cost of the machine increases.  The number of setups increases and the cost also increases, three axis machines are limited for simple jobs and straight forward 3 axis jobs.

3.4   Four axis control system:

In Four axis control system is a three axis machine with an extra rotation on B-axis, four axis can be a vertical machine or an horizontal machine.

In vertical CNC machine the rotary head is added on the side of the machine bed. The machine works as the three axis machine but it has a rotary head for example if the holes have be machined on the tube, the tube can be mounted on the rotary B-axis and the drilling in the required angle. But vertical 4-axis machines are limited for the small jobs.

Horizontal 4-axis machines are used worldwide for successful machining of big parts in a single setup, where it takes 2-3 setups in a 3-axis machine. The part is mounted on the bed which has 360 rotations around Y direction i.e., B-Axis giving chance for the tool to cut on the angled faces in a single setup.

3.5   Five axis control system:

Five axis control system are the three axis machines with an extra rotation along Y and Z directions which are called B-axis and A-axis. As in Four axis machines B rotation is given by the bed and the A-axis rotation is given by the spindle movement called PIVOT point.  Using a five axis machine reduces the cycle time by machining the complex parts in a single setup and improves the accuracy on the positional errors by eliminating the setups.

                Five axis machining gives improved access to the under cuts and deep pockets by tilting the tool and also gives good surface finish and the tool life by tilting the tool to maintain optimum tool to part contact all the times.  

There are more than five axis control systems in the world making aerospace and automobile industries to achieve their accuracy and meet the requirements.