M
ACHINING
U
NIT
Here, the individual machining units are
identified in order to complete the workpiece. In Figure 9 below, note that the
choices are: POINT MACHINING, LINE MACHINING, FACE MACHINING, MANUAL PROGRAM,
OTHER,
WPC,
OFFSET,
END
and
SHAPE CHECK. Additional Machining Units may be entered until the final part
geometry is completed as needed. Some examples are: “POINT MACHINING” used for
Drilling Tapping, Reaming, etc.; “LINE MACHINING” used for Line Center, Line Left, Chamfer Left, etc.; or, “FACE MACH-ING” used for Face Mill, Top End
Mill, Pocket, Step, Slot, etc. The following descriptions will be limited to Point
machining and Line machining.
Figure 9 Machining
Process Menu
POINT MACHINING
Point machining constitutes a large percentage
of Machining Center work. In Figure 10, the different choices for types of
point machining are shown:
Figure 10 Point
Machining Menu
When a selection is made from one of these
choices, unit data are required and automatic tool development is completed,
based on this information. The required information for Drilling is: the
diameter, the depth and whether the hole is to be chamfered. The basic required
tooling is developed based on this information. For example, a center drill or
spot drill, a drill of the size stated and a chamfering cutter will be
developed. This tooling information is taken from a predetermined tool file in
the control. The tool file should be constructed (for all other types of
machining units) by the machinist/programmer prior to programming but can be
done as the program is completed.
S
EQUENCE
D
ATA
Tool Sequence Data
Each individual tool has specific sequence data
that are required as follows:
•
definition of the actual size of the tool
•
the priority in which this tool is to be used
•
the diameter of the hole
•
the hole depth
•
pre-existing hole diameter
•
pre-existing hole depth
•
the desired surface finish
•
the type of drilling cycle (i.e. drilling,
pecking, etc.)
•
the cutting speeds and feeds
•
and, the use of any M-Codes.
Shape Sequence Data
Finally, the shape sequence data is set for the
machining unit. In other words, the actual figure pattern or shape is
identified. In the case of drilling, the choices are: POINT,
LNE,
SQUARE, GRID, CIRCLE,
ARC and CHORD, shown in the Figure 11. As soon as the pattern is completed,
SHAPE END is pressed to end the unit.
Just as with all units, CHECK allows the shape
to be checked graphically for each individual unit. The remainder of the
program is constructed in the same manner until all geometry shapes are
complete.
Figure 11 Point Sequence
Data Menu
LINE MACHINING
Line machining (linear contouring) is another
very common activity performed by Machining Centers. In Figure 12, choices for
types of line machining are shown.
Figure 12 Line Machining
Menu
When a selection is made, unit data are required
and automatic tool development is completed, based on this information. The
required information for line machining is: the depth of cut; the amount of
stock removal in
Z
(
SRV-Z
); the amount of radial
stock removal in
X-Y
(
SRV-R
); the desired finished
surface roughness; chamfer width, if required; the allowance for the finish
Z
depth cut; and, the
allowance for the radial finish width cut. The values input to these items
determine the automatic tool development.
Tool Sequence Data
Each individual tool developed has specific
sequence data that are required, as follows: the nominal diameter of the tool;
the priority in which the tool is to be used; the approach point along the
X
axis, ; the approach
point along the
Y
axis, ;
the cutting direction of either
CW,
or
CCW,
the plunge cutting feedrate along the
Z
axis; the depth of cut,
the cutting speed, and the cutting feedrate; and, any M-Codes as required.
Shape Sequence Data
Finally, the shape sequence data is created in
the machining unit where the actual figure pattern or shape is identified. In
the case of line machining, the choices are: SQUARE, CIRCLE, and
ARBITRY
, shown in Figure 13.
Figure 13 Shape Sequence
Data Menu
The geometric shape is constructed by input of
point data that describe each feature of square, circular or arbitrary shape.
As soon as the pattern is completed, SHAPE END is pressed to end the unit. Just
as with all similar units, the CHECK menu button allows the shape to be
checked graphically for each individual unit.
The remainder of the program is constructed in the same manner until all
geometry shapes are complete.
End Unit
This unit ends the program in the same manner as
M30 does in a G-Code program. The programmer has the option in this unit of
continuing the program for a number of repetitions and to control the Automatic
Tool Change positioning.
Shape Check
When the entire program is written, it is
beneficial to verify its accuracy by performing first a SHAPE CHECK and then
TOOL PATH CHECK. The SHAPE CHECK verifies the geometry and the TOOL PATH CHECK
verifies the actual relationship between the geometry and the tools actual
cutting path. The machinist/programmer has the ability to change from
two-dimensional to three-dimensional views or split the display screen to show
the
X-Y
and
X-Z
, and zoom-in on
features that are hard to see. Once these checks are completed, without errors,
the program is ready for set-up of the tool and work offsets. The machinist may
then begin automatic operation.