Download Fanuc Macro PDF

TitleFanuc Macro
File Size297.2 KB
Total Pages3
Document Text Contents
Page 1

S. K. Sinha / International Journal of Engineering Science and Technology
Vol. 2(12), 2010, 7616-7618



AUTOMATING FACING OPERATION
ON A CNC MACHINING CENTRE



S. K. SINHA

Department of Mechanical Engg.
Institute of Technology, Banaras Hindu University

Varanasi-221005, India
E-mail : [email protected]

Abstract
Facing is usually the first and an essential process on a CNC machining centre, using a face-milling cutter, on
any workpiece, because many a time, the workpiece is obtained through a “rough” casting process. The
advantage of a cast part is that a workpiece with slightly oversize dimensions is made available, usually
requiring very little machining. This saves machining costs. However, the inherent limitation of common casting
processes is inaccuracy in dimensions as well as surface roughness. Because of this reason, facing becomes the
first machining operation. On a CNC milling machine, this requires a facing program written in terms of G-
codes. Since dimensions of different workpieces are likely to be different, offering different areas to be faced,
the same program would not work on all workpieces. The present paper uses the latest macro-programming
technique, available on modern CNC machines, to develop a single program for workpieces of all dimensions.

Keywords

CNC; G-codes; Macro programming; Custom Macro B

1. Introduction
Machining, casting and forging are the most common manufacturing processes. Each technique has its own
advantages and limitations. For example, casting produces the weakest part whereas the strongest part is
produced by forging. However, an advantage with casting is that it is less expensive than a forging process,
Moreover, machinability of a cast part is extremely good. Therefore, in applications where too much strength is
not a criterion, casting becomes the first choice. However, inaccuracy in dimensions, along with surface
roughness, is the inherent limitation of a cast part. Hence, usually a cast part invariably requires some
machining, often facing being the first one.

When it comes to a facing operation, a G-code program can be written, mostly involving rapid traverse
(G00) and linear interpolation (G01). Though the actual program does depend on the control being used on the
machine, in a simple case such as this, the program would be essentially same for all the controls, because all
control manufactures use the same basic program codes, such as G00 for rapid traverse, G01 for linear
interpolation, G02 for clockwise circular interpolation, G03 for counterclockwise circular interpolation, and so
on [1, 2]. Therefore, while program portability is not really a problem, one does have to write a new program for
every new workpiece, because of difference in facing area/geometry. Moreover, since a CNC machine is pretty
expensive, one has to first prove a program before actually executing on the machine. Writing a program,
followed by proving it meticulously, is a time taking process. And if the services of an expert programmer are
not readily available, the company has to look for a suitable person, many a time from outside the company.
This not only increases the production cost, but also affects productivity adversely. Therefore, it is desirable to
have a ready-made program which could be used for workpieces of all dimensions. The aim of the present paper
is to develop such a general-purpose program.

2. Existing Solution
As discussed, separate programs for workpieces of different sizes need to be written. For example, consider
facing operation on a workpiece of 100 mm x 90 mm size, with a facing tool of 30 mm diameter. With the lower
left corner of the top surface selected as the program zero point, and using an overlap/clearance of 2 mm in
cutting passes, the following program can be written, which initially places the tool at position A and follows
the shown toolpath to reach position B in the end (see Fig. 1):

O0001; Program number
G21 G94; Millimeter mode and feed in mm/min selected
G91 G28 Z0; Z-homing
G28 X0 Y0; XY-homing
M06 T01; Tool change

ISSN: 0975-5462

Page 2

S. K. Sinha / International Journal of Engineering Science and Technology
Vol. 2(12), 2010, 7616-7618



100

X

Y

A

B

Facing tool

9
0




Fig. 1: Facing operation on a rectangular plate

G90 G00 G43 H01 Z200; Tool placed 200 mm above the workpiece
X-17 Y13; Tool placed at A (using 2 mm clearance)
Z2; Tool placed 2 mm above the workpiece, at position A
M03 S500; Spindle starts with 500 clockwise rpm
G01 Z-0.5 F60; Facing depth assumed to be 0.5 mm
G91 X134; First facing pass
Y28; Positioning for second facing pass
X-134; Second facing pass
Y28; Positioning for third facing pass
X134; Third facing pass
Y28; Positioning for fourth facing pass
X-134; Fourth facing pass, to reach position B
G00 Z200; Tool retracts, after facing is complete
M05; Spindle stops
M30; Execution ends and control resets

While there is nothing wrong with this program which will do the required facing without any problem,
the fact remains that this is a specific program for a specific job. If there is any change in the workpiece
dimension, a new program would need to be written. This would be a time-consuming process, since the
programmer will have to do all the calculations again, and verify the new program by meticulously analyzing its
simulation. Moreover, services of an expert programmer may not be available all the time.

4. Proposed Solution
The author presents a general-purpose program, using the latest macro-programming technique available on
modern CNC machines [3, 4], which can face workpieces of any dimension, without making any change in the
program. This program would need to be stored as a macro in the CNC memory, which may be called by any
program needing facing. Instead of fixed values, the macro has been developed in terms of variables, the initial
values of which are passed on to the macro, from the calling program, using the macro-call code G65. The tool
number and the offset number of the facing tool, and spindle rpm would need to be specified in the main
program (the macro-calling program), though it is possible to make the macro even more general by using
variables for these also, inside the macro. The specific language for writing the program is Fanuc Custom Macro
B. For other controls, minor changes in the program might be needed; the basic structure of the program would
remain unchanged. For using this program, the machine-table should be made datum for Z-axis. X/Y datum can
be placed at any convenient location. After clamping the workpiece onto the table, one would need to measure
the coordinates of the lower left corner, as well as the thickness (Z-coordinate) of the workpiece.

List of variables used in the macro:
Length (X-dimension) of workpiece, A #1
Width (Y-dimension) of workpiece, B #2
Overlap in facing passes, C #3
Facing tool diameter, D #7
Depth of cut, E #8
Facing feedrate in mm/min, F #9
Lower left corner X-coordinate #24
Lower left corner Y-coordinate #25

ISSN: 0975-5462

Similer Documents