Machining Center
Abbreviations and Acronyms
CST IRN
= Cast Iron
DUCT IRN
= Ductile Iron
CBN STEEL
= Carbon Steel
ALY STEEL
= Alloy Steel
STNLESS
= Stainless Steel
AL
= Aluminum
COPPER
= Copper
WPC
= Workpiece Coordinate
ATC
= Automatic Tool Change
UNo.
= Unit Number
ARBITRY
= Arbitrary
FACE MIL
= Face Mill
TOP EMIL
= Top End Mill
PCKT MT
= Pocket Mountain
PCKT VLY
= Pocket Valley
SRV-Z
= the amount of stock removal in Z
SRV-R
= the amount of radial stock removal in
X-Y
BTM
= Bottom
RGH
= Surface roughness
WAL
= Wall roughness (Same number system applies)
WID-R
= Width of Cut (radial)
CHMF
= Chamfer amount
FIN-Z
= Finish allowance for the Z axis
FIN-R
= Finish allowance for the X-Y axis
NOM Ø
= Nominal diameter of the tool
PRI–NO.
= Priority number for the tool
APPRCH-X
= Approach point for the tool in the X
axis
APPRCH-Y
= Approach point for the tool in the Y
axis
CW CUT
= Clockwise cutting direction
CCW CUT
= Counterclockwise cutting direction
ZFD
= Z Feed, Move to depth of cut at linear
feedrate in the Z axis. Rapid may
be selected here but the default setting is G01.
Caution should be used here because a rapid
movement into solid material
will break the tool and possibly damage the
machine.
DEP-Z
= Depth of Cut
C-SP
= Cutting Speed
FR
= Feedrate
SNo. 1
= Sequence Number
X BI-DIR
= BI-Directional cutting both directions
along the X axis
Y UNI-DIR
= UNI-Directional
(Single) cutting along the Y axis
CN1
= Corner 1
LNE
= Line
CHMF
= Chamfer
CTR-DR
= Center Drill
PT
= Point
INIT
= Initial
R
= Reference or Radius
Following are brief descriptions of the
programming process for Machining Centers: The control must be in the
program-editing mode and a work number (program number) must be identified.
Note: There is no
need for the letter address O to precede the program number with Mazatrol
programs.
Before
any programming can take place, the type of program to create either EIA/ISO or
Mazatrol must be determined. All MAZAK machines use Mazatrol as their standard
with EIA/ISO (G-Code) on some older generation machines as an optional feature.
The construction of a MazatrolMachining Center program contains these basic
parts: a Common Data Unit, identification of a Coordinate System, the Machining
Units and their Sequence Data and, an End unit.
C
OMMON
D
ATA
U
NIT
The information at the head of the program
applies to the entire program. The programmer is prompted to answer the
following questions for this common data.
MATERIAL <Menu>?
The controller is preset with standard materials
of Cast Iron, Ductile Cast Iron, Carbon Steel, Alloy Steel, Stainless Steel,
Aluminum and Copper Alloy to choose from. This choice, combined with tool
material, affects the automatic calculation of cutting feeds and speeds
throughout the program. It is possible to add other materials to the cutting
condition parameters, if the material needed is not available.
INITIAL POINT Z (CLEARANCE)?
This value identifies where all of the tools
will move to, at rapid traverse, before machining begins. In G-Code
programming, this is the same as the Initial Reference Plane. A common reason
for setting this at a particular height is to provide for clearance of work
holding clamps.
ATC MODE ZERO RETURN <Z.X+Y:0,
X+Y+Z:1>?
The choice of Zero Return method establishes how
the tool is returned to the Automatic Tool Change (ATC) position for a tool
change. For example, a selection of 0 returns the
Z
axis to the tool change
position and then, the
X
and
Y
, simultaneously. This is the safest choice, in
most cases; however, if no clearance issues are evident, then simultaneous
movement of
X,
Y
and
Z
may be chosen by
selection of 1 here.
Note:
that this movement is always at rapid traverse.
MULTI MODE <Menu>?
There are three choices for establishing a work
coordinate systems: MULTI OFF, MULTI 5 x 2 and OFFSET TYPE. When MULTI OFF is
selected, the next unit is started and this unit is commonly used for the Workpiece
Coordinate system or WPC. Values are set for the location of the origin of the
workpiece coordinate system, just as with G-Code programs, additionally,
offsets G54–59 may be used.
MULTI 5 X 2
By selecting MULTI 5 x 2, the machining of
multiple repetitions of the same program for several workpieces can be used. A
MULTI FLAG is required, in conjunction with this call, in order to identify how
many repetitions and where. This technique is limited to each of the
repetitions having corresponding distances from part to part. For example, the
distance between all repetitions in the
X
axis must be equal and the
Y
axis distances must be
the same. Up to ten duplications can be set.
OFFSET TYPE
Using this type of coordinate system arrangement
allows the arbitrary location of the Workpiece Zero or origin for multiple
workpieces within the working envelope of the machine. The locations may be
random and polar rotation of the coordinate system is allowed. Up to 10
individual offsets are allowed.
C
OORDINATE
S
YSTEM
In this unit, the actual physical locations for
the coordinate system axis zero points are entered. As mentioned earlier, this
can be in the form of a WPC or work offset using G54-G59 as is common in G-Code
programs. The operator measures the distances in
X
,
Y
and
Z
in relation to the
Machine Zero and enters these values into the program in this unit by using the
WPC MEASURE function.