Multiple Thread Cutting Cycle G76

Multiple Thread Cutting Cycle G76:-

G76P (m) (r) (a) Q (Δd min) R (d);

G76X (u) _ Z(W) _ R(i) P(k) Q(?d) F(L) ;

m                =        Repetitive Count In Finishing (1 To 99)

r                  =        Chamfering Amount

a                  =        Angle of Tool Tip

P                  =        m, r, and a are specified by address P at the same time.

Δdmin          =        Minimum Cutting Depth (Specified By the Radius Value)

d                 =        Finishing Allowance

I                  =        Difference Of Thread Radius If I = 0, Ordinary Straight       Thread Cutting Can Be Made.

K                 =        Height of Thread

Δd                =        Depth of Cut in 1st Cut (Radius Value)

L                 =        Lead Of Thread (Same as G32).

Example:-

Notes:-

1.   In the blocks where the multiple repetitive cycle are commanded, the addresses P, Q, X, Z, U, W, and R should be specified correctly for each block.

2.    In the blocks in which G70, G71, G72, or G73 are commanded and between the sequence number specified by P and Q, M98 (subprogram call) and M99 (subprogram end) cannot be commanded.

3.   In the blocks between the sequence number specified by P and Q, the following commands cannot be specified.

One shot G code except for G04 (dwell)

01 group G code except for G00, G01, G02, and G03

06 group G code

M98 / M99

4.    When G70, G71, G72, or G73 is executed, the sequence number specified by address P and Q should not be specified twice or more in the same program.

5.    The blocks between the sequence number specified by P and Q on the multiple repetitive cycle must not be programmed by using “Direct Drawing Dimensions Programming”.

6.   The multiple repetitive cycle cannot be executing during DNC operation.

7.   Interruption type custom macro cannot be executed during executing the multiple repetitive cycle.

Alarm:-

1.   In the block which is specified by address P of G71, G72 or G73, G00 or G01 group should be commended. If it is not commanded, P/S alarm No.65 is generated.

2.   In MDI mode, G70, G71, G72, or G73 cannot be commanded. If it is commanded, P/S alarm No. 67 is generated. G74, G75, and G76 can be commanded in MDI mode.

Read More

Transverse Cut-Off Cycle G75 Or Diameter Grooving Cycle:-

Transverse Cut-Off Cycle G75 Or Diameter Grooving Cycle:-

Overview:-

  

          This function is used for smooth disposal of machining chips in transverse cut-off machining. This allows easy disposal of machining chips in face turning as well. Both G74 and G75 which are used for cutting off, grooving or drilling, are a cycle to give the escape of a tool automatically. Four patterns which are symmetrical with each other are available. During single block operation, all the blocks are executed step by step.

Programming Format:-

     

       G75 R (1^st ) ;

    

        G75  x__ Z__ P__ Q__ R__ F__ S__ T__  ;

Description:-

            R        =        Distance of Return

          X        =        Absolute Value / Incremental Value of X-Axis

          Z        =        Absolute Value / Incremental Value of Z Axis

          P        =        X-axis cut depth

          Q       =        Z-Axis Movement Distance

R        =        ( 2^nd R )Tool Escape Distance at the Bottom of Cut

          F        =        Feed Rate

          S        =        S Command

          T        =        T Command

Sample Program:-

            G00 G96 G98 ;

          G28 U0 W0 ;

          X102. Z-20. ;

          G75 R2. ;

          G75 W-15. X70. P6. Q5. F150 S100 M3 ;

          G28 U0 W0 ;

          M30 ;

Read More

Face Grooving Cycle G74 Or Longitudinal Cut-Off Cycle

Face Grooving Cycle G74 Or Longitudinal Cut-Off Cycle

Overview:-

            This function is used for smooth disposal of machining ships in longitudinal cut-off machining. For SS materials which produce hard-to-cut machining chips this function can be managed for easy machining chip disposal. You can use this cycle for drilling

Programming Format:-

            G74 R__;

         G74 X__ Z__ P__ Q__ R__ F__ S__ T__;

 Description:-

            R        =        Distance of Return

          X        =        Absolute Value / Incremental Value of X-Axis

          Z        =        Absolute Value / Incremental Value of Z Axis

          P        =        X-Axis Movement Distance

          Q       =        Z-axis cut depth

R        =        ( 2^nd R )Tool Escape Distance at the Bottom of Cut

          F        =        Feed Rate

          S        =        S Command

          T        =        T Command

Drilling Cycle :-

            

         For drilling X, P and R (2^nd ) are  not required .Omit these dada.

Notes:-

1.   During single block operation, all the blocks are executed step by step2.   Omission of address X , P and R( 2^nd ) provides the operation of Z axis alone , resulting in peck drilling cycle.3.   R ( 1^st ) and R ( 2^nd ) are both command values address R. the differentiation is given by whether Z is commanded together . that is ,the command R together with Z results in the flat of R ( 2^nd )4.   Cycle operation is performed in the block where Z is commanded

Sample program:-

            G00 G96 G98 ;

            G28 U0 W0 ;

            X100. Z2.0 ;

            G72 R2. ;

            G72 U-50. Z-40. P5. Q7. F150. S100 M3 ;

            G28 U0 W0 ;

            M30 ;

Read More

Finishing Cycle G70 Fanuc Control CNC Programming

Finishing Cycle G70 Fanuc Control CNC Programming

After roughing have been carried out by the G71 to G73 commands, finishing can be performed by following programming format.

G70 P__ Q__

          P        =        finish shape start sequence number

          Q       =        finish shape end sequence number

Example:-

          O1234 ;

          ;

          ;       

          N100 G70 P200 Q300 ;

          ;

          ;

          M30;

Read More

Contour –Parallel Roughing Cycle G73 Or Profile Turning Cycle Or Copy Turning Cycle

Contour –Parallel Roughing Cycle G73 Or Profile Turning Cycle Or Copy Turning Cycle

Profile Turning Cycle:-

          This function will allow efficient execution in roughing when cast or forged parts are to be cut along finish shape.

Programming Format:-

          G73 U___ W__ R__ ;

          G73 p__ Q__ U__ W__ F__ S__ T__ ;

          U       =        escape distance and direction in the X-axis direction ( radial value )

          W       =        escape distance and direction in the Z-axis direction

          R        =        times of divisions

          * Other Addresses Are As With G71

Tool Nose Radius Compensation:-

          When this cycle is commanded in the tool nose radius compensation mode, tool nose radius compensation is applied to the finishing shape sequence for this cycle and cycle is executed for this shape.

         

           However, when this cycle is commanded in the tool nose radius compensation mode, the compensation is temporarily cancelled immediately before this cycle and started at the head block of the finishing shape sequence.

Sample Program:-

N10     G00 G96 G98

N11     G28 U0 W0

N12     T0101

N13     X150. Z5.

N14     G73 U8. W6. R3.

N15     G73 P16 Q20 U4. W2. F150 S100 M3 ;

N16     G00 X50. ;

N17     G01 Z-30.;

N18     X80. Z-50. ;

N19     Z-75. ;

N20     X120. Z-90.0 ;

N21     G70 P16 Q20 ;

N22     G28 U0 W0 M5 ;

N23     M30 ;

Read More

Facing Cycle For Fanuc Control G72 or Transverse Roughing Cycle

Facing Cycle in Fanuc Control G72 or Transverse Roughing Cycle

Programming format:-

G72 W__ R__ ;

G72 P__ @__ U__ W__ F__ S___ T__ ;

W       =        Cutting Depth

R        =        Escape Distance

P        =        Head Sequence No. For Finishing Shape

Q       =        End Sequence No. For Finishing Shape

U       =        Finishing Allowance and Direction In X Axis Direction (Diametric Vale)

W       =        Finishing Allowance and Direction in Z Axis Direction

F        =        Feed Rate

S        =        Cutting Speed

T        =        Tool Number

Note:-

         If F and S commands exist in blocks defined by p and Q, they will be ignored during roughing cycle because they are considered for finishing cycle.

Sample program:-

N01     G00 G96 G98 ;

N02     G28 U0 W0 ;

N03     T0101

N04     X176. Z2.  ;

N05     G72 W7. R1.

N06     G72 P06 Q13 U4. W2. F100 S100 M3

N07     G00 Z-80. S150 ;

N08     G01 X120. W8. F100;

N09     W10.;

N10     X82. W11. ;

N11     W20. ;

N12     X35. W21. ;

N13     W12. ;

N14     G70 P06 Q13 ;

N15     G28 U0 W0 M5 ;

N16     M30;

Read More

Subprogram Call: M98, M99

Subprogram Call: M98, M99

Function and Purpose

          Fixed sequences or repeatedly used program can be stored in the memory as subprograms which can then be called from the main program when required.M98 serves to call sub programs and M99 serves to return from the subprogram. Furthermore, it is possible to call other subprograms from particular subprograms and the nesting depth can include as many as 8 levels.

Programming Format:-

          Subprogram call

          M98 P__ Q__ L__ ;

          P        =        program number

          Q       =        sequence number in subprogram to be called

          L        =        number of sub program repetitions

Return to Main Program from Subprogram:-

          M99 P__ L__ ;

          P        =        sequence number of return destination

          L        =        number of times after repetition number has been changed

Example:-

          O1234 ;

          0000000;

          ;

          ;

          M99;

          %

Notes:-

          Main programs can be used during memory and tape operation but subprograms must have been entered in the memory.

          The following commands are not the object of subprograms nesting and can be called even beyond the 8^th nesting level

Subprogram Execution

M98 : subprogram call command

M99 : subprogram return command

Read More

Mirror Image On / Off G15.1 / G50.1

Mirror Image On / Off: G15.1 / G50.1

Function and Purpose:-

          Mirror image mode can be turned on and off for each axis using G-codes. Higher priority is given to the mirror image setting with the G-codes over setting by any other methods.

 Programming Format

          G51.1 X__ Y__ Z__                    Mirror image ON

          G50.1 X__ Y__ Z__           Mirror image OFF

Detailed:-

          Use the address and coordinates in a G51.1 block to specify the mirroring axis and mirroring center (using absolute or incremental data), respectively

          If the coordinate word is designated in G50.1, then this denotes the axis for which the mirror image is to be cancelled .Coordinate data, even if specified, is ignored in that case.

          After mirror image processing has been performed for only one of the axes forming a plane, the rotational direction and the offset direction become reverse during arc interpolation, tool diameter offsetting, or coordinate rotation.

          Since the mirror image processing function is valid only for local coordinate systems, the center of mirror image processing moves according to the particular counter preset data or workpiece coordinate offsetting data.

Sample Programs:-

          G00 G90 G40 G49 G80

          M98 P100

          G51.1 X0.0

          M98 P100

          G51.1 Y0.0

          M98 P100

          G50.1 X0.0

          M98 P100

G50.1 Y0.0

M30.

(SUB PROGRAM O100)

O0100

G91 G28 X0.0 Y0.0

G90 G00 X20.0 Y20.0

G42 G01 X40. D.01F120

Y40.

X20.

Y20.

G40 X0.0 Y0.0

M99

Read More

Programmed Data Setting G10

Function Purpose:-

                The G10 command allows tool offset data, work offset data and parameter data to be set or modified in the flow of program.

Programming Formats

Programming Workpiece Offsets

          Programming format for the workpiece origin data

          G10 L2 P__ X__ Y__ Z__ ……. (Additional axis)

          P :      0 = Coordinate shift (Added Feature)

                   1 = G54       

                   2 = G55

3 = G56

4 = G57       

                   5 = G58

6 = G59

Data of P-commands other than those listed above are handled as P = 1.

If P-command setting is omitted, the workpiece offsets will be handled as currently effective ones.

Programming Tool Offsets:-

          Programming format for the tool offset data of Type A

          G10 L10 P__ R__

          P : Offset number

          R : offset amount

Programmable Parameter Data Input:-

          G10 L50 …………….. Parameter input mode ON

          N__ P__ R__

          N__ R__

          G11…………………… Parameter input mode OFF

                   N : Parameter number

                   P : Axis number (for axis type parameter)

                   R : Data of parameter

Notes:-

1.   Do not use the G10 command in the same block with a fixed cycle command or a subprogram call command. This will cause a malfunctioning or a program error

Example:-   

          G10 L2 P1 X-100 Y-1000 Z-100 B-1000

Read More