Programming on CNC Machines for Machining Operations

Before starting any machining operation, it is mandatory to plan the sequence of operation. Once the sequence is planned the same has to b... thumbnail 1 summary
Before starting any machining operation, it is mandatory to plan the sequence of operation. Once the sequence is planned the same has to be fed to the computer. This activity is known as Programming. Any operation cannot be possible on CNC machines unless it has been programmed. The accuracy and the shape of the work piece depend on the quality of the programme written in the computer.

Writing Program to Suit Sinumeric 810/ E

It is already seen how various G and M codes are used. All the examples were designed with a view to explain specific G codes. In general, a job may require several of such machining operations which need to be performed in a proper sequence. The most efficient machining technique is to first give an overall final shape to the job (as far as possible) by G71, the multiple turning cycles or by G72, the multiple facing cycles. These cycles are invariably used for bulk material removal and often referred to as roughing cycles. However, it is not always possible to obtain the exact final shape with the help of these cycles only. For example, a part may have threads on it for which a threading cycle has to be used. Similarly, the grooving cycle will have to be used for grooving/parting operations. Moreover, both G71 and G72 suffer from the inherent limitation that they cannot produce any undercut on the job. G 73, the pattern repeating cycle, is the only cycle which can produce virtually any type of undercut, provided suitable tools are available which avoid undesirable interference. The thumb rule is to use G71 or G72 first, and thereafter, other cycles also may be used, if required.

Sample Program. This program produces the job shown in figure below. This job involves the following machining operations:
  • Step-I: Straight/Taper turning       
  • Step-2: Grooving
  • Step-3: Threading   
  • Step-4: Chamfering

jobs produced during maching operations
As already discussed, first G71 is used to give an approximate overall shape to the work piece (step-I). Thereafter, G75 is used to make the groove (step-2). Then, threading is done (step-3), and finally, chamfering is performed (step-4), completing the job. Step -2 and step-3 may be interchanged. Also, step-4 may be included in step-1 (recommended).

It may be noted that G70 also has to be used to machine the extra material left as machining allowances by G71. Sample lathe program is given in the following lines for the machining of the component shown in above figure.
G21 G97 G98

G28 U0 W0

M06 T3
Roughing tool
M03 S2000 G00

X30 Z1

G71 U0.5 R0.2
Depth of cut = 0.5 mm and radial tool retraction = 0.2 mm
G71 P10 Q20 U0.l W0.1 F60
X/Z finishing allowances = 0.1 mm and feed = 60 mm/min
N10 G00 X16
Start of the profile
G01 Z-25 F30
Feed specified here is ignored by G71. It is used by G70
X22 Z-40

N20 X30 Z-50
End of the profile
G28 U0 W0

M06 T7                                                  
Finishing tool
M03 S3000
RPM increased for finishing operation
G70 P10 Q20

G28 U0 W0
Step-1 complete
M06 T1
Grooving tool
M03 S2000

G00 X18 Z 22
Thickness of the grooving tool assumed to be 2 mm and its leftcomer taken as the reference point.
G75 R1
Radial retraction = 1 mm
G75 X12 Z-25 P200 Q1500 F10
The lower left comer of the groove is at (12,-25), peck length = 0.2 mm, lateral shift = 1.5 mm, and feed = 10 mm/min
G28 U0 W0
Step-2 complete
M06 T5
Threading tool
M03 S500
RPM reduced for threading
G00 X18 22 X16

G92 X 15.75 Z-20 F2
for M16, pitch=2mm and minor diameter = 13.5462 mm

X15.50

X15.25

X15

X14.75

X14.50

X14.25 X14

X13.9 X13.8

X13.7 X13.6

X13.5462

G28 U0 W0
Step-3 complete
M06 T3

M03 S2000 G00

X18 Z0

G90 X16 Z-1 R-1 F60

X16 Z-1.23 R-l.23

G28 U0 W0
Step-4 complete
M05

M38 M30

No comments

Post a Comment