Century Star Turning CNC System. Programming Guide (V3.5 April, 2015)

3. Interpolation Function

3.2 Linear Interpolation (G01)

Programming

G01 X(U)… Z(W)… F…

Explanation of the parameters

X, Z

Coordinate value of the end point in the absolute command

U, W Coordinate value of the end point in the incremental command

Feedrate. It is effective until a new value is specified.

Function

The tool is moved along the straight line at the specified feedrate.

3. Interpolation Function

Example 1

Use G01 command to rough machining and finish machining the simple cylinder part.





Figure 3.2 Linear Interpolation - Example 1

%3306（Absolute command）

%3306（Incremental command）

N1 T0106

N1 T0101

N2 M03 S460

N3 G00 X90Z20

N4 G00 X31Z3

N5 G01 Z-50 F100

N5 G01 W-53 F100

N6 G00 X36

N6 G00 U5

N7 Z3

N7 W53

N8 X30

N8 U-6

N9 G01 Z-50 F80

N10 G00 X36

N11 X90 Z20

N12 M05

N13 M30

3. Interpolation Function

Example 2

Use G01 command to rough machining and finish machining simple conical part.







Figure 3.3 Linear Interpolation - Example 2

%3307

N1 T0101

N2 M03 S460

N3 G00 X100Z40

N4 G00 X26.6 Z5

N5 G01 X31 Z-50 F100

N6 G00 X36

N7 X100 Z40

N8 T0202

N9 G00 X25.6 Z5

N10 G01 X30 Z-50 F80

N11 G00 X36

N12 X100 Z40

N13 M05

N14 M30

3. Interpolation Function

Example 3

Use G01 command to rough machining and finish machining the part.

2×45°









Figure 3.4 Linear Interpolation - Example 3

%3308

N1 T0101

N2 M03 S450

N3 G00 X100 Z40

N4 G00 X31 Z3

N5 G01 Z-50 F100

N6 G00 X36

N7 Z3

N8 X25

N9 G01 Z-20 F100

N10 G00 X36

N11 Z3

N12 X15

N13 G01 U14 W-7 F100

N14 G00 X36

N15 X100 Z40

N16 T0202

N17 G00 X100Z40

N18 G00 X14 Z3

N19 G01 X24 Z-2 F80

N20 Z-20

N21 X28

N22 X30 Z-50

N23 G00 X36

N24 X80 Z10

N24 M05

N25 M30

3. Interpolation Function

3.3 Circulation Interpolation (G02, G03)

Programming

G02

I_K_



X(U)_Z(W)

_

F_

G03









Explanation of the parameters

G02 a circular path in clockwise direction (CW)

G03 a circular path in counterclockwise direction (CCW)

X, Z

Coordinate values of the circle end point in absolute command

U, W Coordinate values of the circle end point with reference to the circle starting

point in incremental command.

I, K

Coordinate values of the circle center point with reference to the circle

starting point in incremental command.

Circle radius. R is valid when I, K, R are all specified in this command.

Feedrate

u/2

x/2

u/2

x/2

Circle center point

＋Z

Figure 3.5 Description of G02/G03 parameter

3. Interpolation Function

G02 and G03 are defined when the working plane is specified. Figure 3.6 shows the

direction of circular interpolation.

G03

G02

G03

＋Z

G02

G03

G02

Figure 3.6 Direction of Circular Interpolation

Function

The tool is moved along a full circle or arcs.

3. Interpolation Function

Example 2

Use the circular interpolation command to program





R15

Figure 3.8 Circular Interpolation - Example 2

%3310（Absolute programming）

N4 G00 U-90 W-17

N5 G01 W-3 F100

N1 T0101

N6 G03 U30 W-15 R15

N2 M03 S460

N7 G01 W-20

N3 G00 X90Z20

N8 X36

N4 G00 X0 Z3

N9 G00 X90 Z20

N5 G01 Z0 F100

N10 M05

N6 G03 X30 Z-15 R15

N11 M30

N7 G01 Z-35

N8 X36

N9 G00 X90 Z20

N10 M05

N11 M30

%3310（Incremental

programming）

N1 T0101

N2 M03 S460

N3 G00 X90Z20

3. Interpolation Function

Example 3

Use the circular interpolation command to program.

R10

Figure 3.9 Circular Interpolation - Example 3

%3311

N1 T0101

N2 M03 S460

N3 G00 X100 Z40

N4 G00 X0 Z3

N5 G01 Z0 F100

N6 G03 X20 Z-10 R10

N7 G01 Z-20

N8 G02 X24 Z-24 R4

N9 G01 Z-40

N10 G00 X30

N11 X100 Z40

N12 M05

N13 M30

3. Interpolation Function

Example 4

Use the circular interpolation command to program





Figure 3.10 Circular Interpolation - Example 4

%3312

N1 T0101

N2 M03 S460

N3 G00 X80 Z10

N4 G00 X30 Z3

N5 G01 Z-20 F100

N6 G02 X26 Z-22 R2

N7 G01 Z-40

N8 G00 X24

N9 Z3

N10 X80 Z10

N11 M05

N12 M30

3. Interpolation Function

3.4 Chamfering and Rounding (G01, G02, G03)

Note: These commands cannot be used in thread cutting.

3.4.1 Chamfering (G01)

Programming

G01 X(U)_ Z(W)_ C_

Explanation of the parameters

X, Z

Coordinate values of the intersection (point G) in absolute command

U, W Coordinate values of the intersection (point G) in incremental command

Width of chamfer in original direction of movement (c)

u/2

x/2

Figure 3.11 Chamfering (G01)

Function

A chamfer can be inserted between two blocks which intersect at a right angle (point

A→B→C).

Note: The length of GA should be more than the length of GB

3. Interpolation Function

3.4.2 Rounding (G01)

Programming

G01 X(U)_ Z(W)_ R_

Explanation of the parameters

X, Z

Coordinate values of the intersection (point G) in absolute command

U, W Coordinate values of the intersection (pint G) in incremental command

Radius of the rounding (r)

Figure 3.12 Rounding (G01)

Function

A corner can be inserted between two blocks which intersect at a right angle (point

A→B→C).

Note: The length of GA should be more than the length of GB

3. Interpolation Function

3.4.3 Chamfering (G02, G03)

Programming

G02



X(U)_ Z(W)_ R _ RL



G03





Explanation of the parameters

X, Z

Coordinate values of the intersection (point G) in absolute command

U, W Coordinate values of the intersection (point G) with reference to the circle

starting point (point A) in incremental command

Circle Radius (r)

RL= Width of chamfer in original direction of movement (RL)

D C

RL=

Figure 3.14 Chamfering (G02/G03)

Function

A chamfer can be inserted between two blocks which intersect at a right angle (point

A→B→C).

Note: RL must be capitalized letters.

3. Interpolation Function

3.4.4 Rounding (G02, G03)

Programming

G02



X(U)_ Z(W)_ R _ RC



G03





Explanation of the parameters

X, Z

Coordinate values of the intersection (point G) in absolute command

U, W Coordinate values of the intersection (point G) with reference to the circle

starting point (point A) in incremental command

Circle radius (r)

RC Radius of rounding (rc)

rc=

x/2

Figure 3.15 Rounding (G02/G03)

Function

A corner can be inserted between two blocks which intersect at a right angle (point

A→B→C).

Note: RC must be capitalized letters.

3. Interpolation Function

Example

Use the chamfering and rounding command (G02/G03):

R15

Figure 3.16 Chamfering and Rounding (G02/G03) - Example

%3315

N1 T0101

N2 G00 X70 Z10 M03 S460

N3 G00 X0 Z4

N4 G01 W-4 F100

N5 X26 C3

N6 Z-21

N7 G02 U30 W-15 R15 RL=4

N8 G01 Z-70

N9 G00 U10

N10 X70 Z10

N11 M30

3. Interpolation Function

3.5 Thread Cutting with Constant Lead (G32)

Programming

G32 X(U)__Z(W)__R__E__P__F/I__Q__

Explanation of the parameters

X, Z

Coordinate values of end point in absolute command

U, W Coordinate values of end point with reference to the starting point in

incremental command

Thread lead i.e. the feed of tool with reference to the tool at one spindle

revolution

Thread lead at inch measurement. Unit: threads/inch

R, E Retraction amount of thread cutting. R is the retraction amount on axis Z. E is

the retraction amount on axis X. They all use the incremental command in absolute or

incremental programming. The positive R or E means the positive retraction on axis Z

or X. The negative R or E means the negative retraction on axis Z of X. The retraction

slot can be ignored when using R or E. When there is no R or E, it means that the

retraction function is not validated. In general, R is set as two times value of thread

lead, and E is set as the thread height.

Spindle angle of thread cutting start point at the spindle reference pulses

1) Acceleration constant of thread cutting retraction. When it is set to zero, the

acceleartion is maximum. The more this value is, the acceleration time is longer,

and the retraction is longer. Q must be set to zero or more than zero.

2) When there is no Q, the set acceleration constant on each axis is used in the

retraction.

3) R and E must be set when the retraction function is required.

4) The retraction ratio of minor axis:major axis should not be more than “20“.

5) Q is one-shot G code.

3. Interpolation Function

u/2

x/2

Figure 3.17 Thread Cutting with Constant Lead (G32)

Function

Cylindrical thread, taper thread and face thread can be machined with G32.

Thread cutting is form turning and the feed is much. If the tool intensity is low, it is

required to feed cutting at serveral times. The following table is the general feed times

and amount of thread cutting.

3. Interpolation Function

Table 3-1 feed times and amount of thread cutting

Thread in metric measurement

Lead

1.0

1.5

2.5

3.5

Threads (radius)

0.649

0.974

1.299

1.624

1.949

2.273

2.598

Once

0.7

0.8

0.9

1.0

1.2

1.5

Twice

0.4

0.6

0.7

0.8

Three

0.2

0.4

0.6

feed times

Four

0.16

0.4

0.6

and

Five

0.1

0.4

amount

Six

0.15

0.4

(diameter)

Seven

0.2

0.4

Eight

0.15

0.3

Nine

0.2

Thread in inch measurement

Threads/in

Threads (radius)

0.678

0.904

1.016

1.162

1.355

1.626

2.033

Once

0.8

0.9

1.0

1.2

Twice

0.4

0.6

0.7

feed times

Three

0.16

0.3

0.5

0.6

and

Four

0.11

0.14

0.3

0.4

0.5

amount

Five

0.13

0.21

0.4

0.5

(diameter)

Six

0.16

0.4

Seven

0.17

Note:

1) The spindle speed should remain constant during rough cutting and finish

cutting.

2) The feed hold function is ineffective during the thread cutting. Even though

the “feed hold” button is pressed, it is effective until the thread cutting is done.

3) It is not recommended to use the constant surface speed control during the

thread cutting.

4) Allowant amount must be specified to avoid the error.

3. Interpolation Function

Example

Given that F=1.5mm, _ =1.5mm,   =1mm, cutting for four times and each cutting

depth is separately: 0.8mm, 0.6 mm, 0.4mm, 0.16mm. It is diameter programming.

100

Figure 3.18 Thread Cutting - Example

%3316

N1 T0101

N2 G00 X50 Z120

N3 M03 S300

N4 G00 X29.2 Z101.5

N5 G32 Z19 F1.5

N6 G00 X40

N7 Z101.5

N8 X28.6

N9 G32 Z19 F1.5

N10 G00 X40

N11 Z101.5

N12 X28.2

N13 G32 Z19 F1.5

N14 G00 X40

N15 Z101.5

N16 U-11.96

N17 G32 W-82.5 F1.5

N18 G00 X40

N19 X50 Z120

N20 M05

N21 M30

3. Interpolation Function

3.6 Tapping (G34)

Programming

G34 K_ F_ P_

Explanation of the parameters

K The distance from the starting point to the bottom of the hole

F Thread lead

P Dwell time at the bottom of a hole

Figure 3.19 Rigid Tapping

Function

With this command, the operator can rigid tap a thread.

In general, there is overshoot of the tap at the bottom of the thread during the

spindle-braking portion of the tapping cycle. It can be set by PMC parameters (Table

3-1) to eliminate the overshoot errors.

3. Interpolation Function

Table 3-2 PMC parameters

CNC system

PMC parameters

Maximum spindle speed during

#0062

tapping

Minimum spindle speed during

#0063

HNC 18/19i

tapping

#0064

Dwelled unit for tapping

#0065

Optional dwelled unit for tapping

Maximum spindle speed during

#0017

tapping

Minimum spindle speed during

#0018

HNC 21/22

tapping

#0019

Dwelled unit for tapping

#0030

Optional dwelled unit for tapping

Optional dwelled unit for tapping is only effective when “dwelled unit for tapping” is

assigned to “0”. Moreover, it is not necessary to restart the system.

The following formular is to calculate the dwelled unit (X):

D =

(S * S / C) * X / 10000 = L * 360 / F

D dwelled amount

S spindle speed

C Transmission gear ratio

X dwelled unit

L overshoot error

F thread lead

Since the workpiece is chucked on the spindle, the spindle decceleration time of

turning machine is more than a milling machine’s. The quicker the spindle rotates, the

quicker the feedrate on Z axis is, and then the more time the decceleration time takes.

Thus, the spindle speed should be set accoording to the thread length.

3. Interpolation

Function

Example

The following is a tested data for tapping when the thread lead is 1.25mm.

%0034

T0101

S100

G90G1X0Z0F500

G34K-10F1.25P2

S200

G90G1X0Z0F500

G34K-10F1.25P2

S300

G90G1X0Z0F500

G34K-10F1.25P2

S400

G90G1X0Z0F500

G34K-20F1.25P2

S500

G90G1X0Z0F500

G34K-30F1.25P3

S600

G90G1X0Z0F500

G34K-40F1.25P3

S700

G90G1X0Z0F500

G34K-50F1.25P3

S800

G90G1X0Z0F500

G34K-50F1.25P2

S1000

G90G1X0Z0F500

G34K-60F1.25P3

M30

3. Interpolation Function

3.7 Direct Drawing Dimension Programming (G01)

Angles of straight lines, chamfering value, corner rounding values, and other

dimensional values on machining drawings can be programmed by directly inputting

these values. In addition, the chamfering and corner rounding can be inserted

between straight lines having an optional angle. It is called direct drawing dimension

programming.

This programming is only valid in turning system G01.

3.7.1 Instruct a line

Programming

G01 X_Z_A_

Explanation of the parameters

X_Z_: Line location address;

A_: Angle between linear motion direction and the positive Z-axis direction. Counter

clockwise is positive, while clockwise is negative. Unit: degree.

(X2, Z2)

X1_Z1_

X2_( Z2_)A_;

(X1, Z1)

Note: the target position only needs to specify a movement value in one direction.

E.g.:Z50a45 or X100a45

3. Interpolation Function

Example

135゜

Φ 80

Φ 50

Φ 40

%3324

N1 T0101

N2 M03S400

N3 G00 X100Z40

N4 G00 X0Z0

N5 G01X40A135

N6 G00 X100Z40

N7 M30

3.7.2 Rounding

Programming

G01 X_Z_R_

G01 X_Z_

Explanation of the parameters

X_/Z_: Line location address;

R_: Rounding radius;

Function

An arc is inserted between two linear interpolations. This arc is tangent to the two

lines.

3. Interpolation Function

Explanation of the parameters

X_Z_: Line location address;

C_: Chamfer edge length;

Function

Chamfering is inserted between two linear interpolations.

X2_Z2_C1_;

(X3, Z3)

X3_Z3

(X2, Z2)

(X1, Z1)

Example

Φ 50

C10

Φ 10

Φ 20

%3326

N1 T0101

N2 M03 S400

N3 G00 X100 Z40

N4 X0 Z0

N5 G01 X0 Z-20 C10

N6 G01X60Z-50

N7 G00X100 Z40

N8 M30

3. Interpolation Function

3.7.4 Continuous Rounding

Programming

G01 X_Z_R_

G01 X_Z_

Explanation of the parameters

X_/Z_: Line location address;

R_: Rounding radius;

Function

Circular Interpolation is continuously inserted between two linear interpolations.

X2_Z2_R1_;

X3_Z3_R2_;

(X4, Z4)

(X3, Z3)

X4_Z4_

A2 R1

(X2, Z2)

Example

Φ 30

Φ 15

Φ 80

Φ 70

Φ 80

%3327

N1 T0101

3. Interpolation

Function

N2 M03 S400

N3 G00 X100 Z40

N4 X0 Z0

N5 G01 X0 Z-15 R15

;the first rounding

N6 G01 X60 Z-15 R15

;the second rounding

N7 G01 X60 Z-30

N8 G00X100 Z40

N9 M30

3.7.5 Continuous Chamfering

Programming

G01 X_Z_C_

G01 X_Z_

Explanation of the parameters

X_/Z_: Line location address;

C_: Chamfer edge length;

Function

Chamfering is continuous inserted between two linear interpolation.

X2_Z2_C1_;

X3_Z3_C2_;

(X3, Z3)

X4_Z4_

(X4, Z4)

(X2, Z2)

3. Interpolation Function

Example

Φ 70

Φ 50

Φ 80

C10

Φ 10

Φ 20

Φ 70

Φ 80

%3328

N1 T0101

N2 M03 S400

N3 G00 X100 Z40

N4 X0 Z0

N5 G01 X0 Z-20C10

;the first chamfering

N6 G01 X60 Z-50C10

;the second chamfering

N7 G01 X60 Z-70

N8 G00X100 Z40

N9 M30

3.7.6 Rounding then Chamfering

Programming

G01 X_Z_R_

G01 X_Z_C_

G01 X_Z_

Explanation of the parameters

X_/Z_: Line location address;

R_: Rounding radius;

C_: Chamfer edge length;

Function

Round and Chamfering are inserted between two linear interpolation.

Century Star Turning CNC System. Programming Guide (V3.5 April, 2015) - page 2