Note: All Cutting Condition Parameters
are based from Carbon Steel (e.g. Plain Carbon Steel 1018) and all other
materials are a percentage factor of this. You may develop new materials
specific to your application with this criteria in mind. See the section in
your Mazak User Manual provided with the machine for details on assigning
Cutting Condition Parameters.
MAXIMUM OUTSIDE DIAMETER <MENU>? (
)
•
Input 2.5
inches
MIN INSIDE DIAMETER <MENU>? ( )
•
Input 0
WORKPIECE LENGTH? ( )
•
Input 5.0
inches
This amount allows for 2 inches of the material
to be clamped, in the chuck.
MAX SPINDLE RPM LIMIT (rpm)? ( )
•
Input 3000
FINISH ALLOWANCE X? ( )
•
Input .01
FINISH ALLLOWANCE Z? ( )
•
Input .005
STOCK REMOVAL OF WORKFACE? ( )
•
Input .1
MODE MENU?
From the Menu keys, notice the arrow keys at the
left end (F9). When pressed, a next menu screen is displayed.
•
Choose
M-Code (F5)
•
Input 08
for Flood Coolant (F6)
•
Use cursor
down key to start a new machining process
MODE MENU? ( )
•
Choose EDGE
SECTION TO BE MACHINED ? <MENU>
•
Choose FCE
from the Menu keys
ROUGHING PERIPHERIAL SPEED? ( )
•
Press AUTO
SET (F1)
FINISH PERIPHERIAL SPEED? ( )
•
Press AUTO
SET (F1)
ROUGHING FEEDRATE? ( )
•
Input .016
ROUGHING DEPTH OF CUT PER PASS ( )
•
Input .08
ROUGHING TOOL TYPE? ( )
Choose from tools that are identified in the
tool file and the turret (at the machine). In our case, we will use tool
number 2 for roughing and tool number 4 for finishing, these have been
predefined in the software.
•
Input 2 for
rough turning tool
•
Input tool
4 for the finish turning tool
STARTING POINT X? ( )
•
Input 2.5
STARTING POINT Z? ( )
•
Input .1
FINIAL
POINT X
? ( )
•
Input 0
FINAL POINT Z? ( )
•
Input 0
SURFACE ROUGHNESS or FINISHING FEEDRATE?
<MENU>( )
•
Select Roughness
(F1) and then choose 6 (F6)
Once this data is entered a new process begins.
MODE MENU? ( )
•
Choose BAR
from the Menu keys (F1)
•
Choose BAR
OUT from the Menu keys (F1)
CUTTING PATTERN MENU? ( )
•
Chose #1
for the cut style (F2)
The difference between #0 and #1 is the way the
tool moves at the end of the cut sequence. For BAR OUT 1, the tool feeds up the
back wall, out to the O.D., at the end of the cut on every pass; whereas, on
BAR OUT 2, the tool rapids away from the cut at 45º to a clearance point set by
parameter and then consecutive passes are completed and the back wall is
finished on the last pass only.
CUTTING
POINT X
? ( )
•
Input 2.5
CUTTING POINT Z? ( )
•
Input 0
SURFACE SPEED FOR ROUGH CUT? ( )
•
Select AUTO
SET from the Menu keys (F1)
FINISHING PERIPHERIAL SPEED?
•
Select AUTO
SET from the Menu keys (F1)
ROUGHING FEEDRATE?
•
Input .016
ROUGHING DEPTH OF CUT PER PASS?
• Input .080
ROUGHING TOOL TYPE?
• Input 2, for the rough turning tool
FINISHING TOOL TYPE?
• Input 4, for the finish turning tool
SHAPE PATTERN?
• Choose
LIN
(F1)
CHAMFERING (C) vs. ROUNDING R AT START
POINT
• Input .05 to create the .05 x 45º chamfer (C)
Note: if a Radius is required you must
press the CORNER R Menu key (F1), prior to
entry of the amount.
X END POINT?
• Input 1.0 to create the 1.0 diameter
Z END POINT?
• Input 1.0 to create the length of the 1.0
diameter
CHAMFERING vs. ROUNDING AT END POINT?
• Press Input to omit this setting
RADIUS OF ARC OR TAPER ANGLE?
• Press Input to omit this setting
FINISHING FEEDRATE FOR SURFACE ROUGHNESS?
• Input 6 (F6)
SHAPE PATTERN?
• Choose
LIN
(F1)
CHAMFERING (C) vs. ROUNDING R AT START
POINT?
• Press CORNER R (F1)
• Input .1 to create the .1 radius (R)
X END POINT?
• Input 1.5 to create the 1.5 diameter
Z END POINT?
• Input 2.0 to create the length of the1.5
diameter
CHAMFERING vs. ROUNDING AT END POINT?
• Press CORNER R (F1)
• Input .1 to create the .1 radius (R)
RADIUS OF ARC OR TAPER ANGLE?
• Press Input to omit this setting
FINISHING FEEDRATE FOR SURFACE ROUGHNESS?
• Input 6 (F6)
SHAPE PATTERN?
• Choose
LIN
(F1)
CHAMFERING (C) vs. ROUNDING R AT START
POINT
• Input .25 to create the .25 x 45º chamfer (C)
X END POINT?
• Input 2.5 to create the 2.5 diameter
Z END POINT?
• Input 3.0 to create the length of the 2.5
diameter
CHAMFERING vs. ROUNDING AT END POINT?
• Press Input to omit this setting
RADIUS OF ARC OR TAPER ANGLE?
• Press Input to omit this setting
FINISHING FEEDRATE FOR SURFACE ROUGHNESS?
• Input 6 (F6)
Select SHAPE END from the Menu keys (F9)
A new Process Number is started. Select the
Machining Unit type next.
• Select
GRV
for Groove from the Menu keys (F6)
SECTION TO BE MACHINED?
• Choose OUT (F1)
MACHINING PATTERN?
• Choose type #1 (F2)
NUMBER OF GROOVES?
• Input 1
SPACING AMOUNT OF MULTIPLE GROOVES?
• Press Input to omit this setting
GROOVE WIDTH?
• Input .156 for the groove width
FINISH REMOVAL ALLOWANCE?
• Input .01 for the groove finish allowance
ROUGHING PERIPHERIAL SPEED?
• Press the AUTO SET Menu key (F1)
FINISHING PERIPHERIAL SPEED?
• Press the AUTO SET Menu key (F1)
ROUGHING FEEDRATE?
• Input .010
ROUGHING DEPTH OF CUT PER PASS?
• Input .04
ROUGHING TOOL TYPE?
• Input 8 for the rough grooving tool
FINISHING TOOL TYPE?
• Input 8 for the finish grooving tool
CHAMFERING (C) vs. ROUNDING R AT START
POINT?
• Input .04 for chamfering at the start of the
groove
X START POINT?
• Input 1.0
Z START POINT?
• Input .75
X END POINT?
• Input .9
Z END POINT?
• Input .75
CHAMFERING vs. ROUNDING AT END POINT?
• Press Input to omit this setting
FINISHING FEEDRATE FOR SURFACE ROUGHNESS?
• Input 6 (F6)
A new Process Number is started. Select the next
Machining Unit type.
• Select
THR
for Threading from the Menu keys (F6)
SECTION TO BE MACHINED?
• Choose OUT (F1)
MACHINING PATTERN?
• Choose #0 STANDARD (F1)
CHAMFER ANGLE <0: NO CHAMFER, 1:45
DEGREES, 2:60 DEGREES>?
• Choose #0 for no chamfer
THREADING LEAD?
• Input .125 for the thread lead
This amount is determined by dividing one by the
number of threads per inch. In
this case, 1/8 = .125.
THREADING ANGLE?
• Input 59 for the threading angle
NUMBER OF THREADS?
• Input 1 for the number of thread starts
THREADING HEIGHT?
• Input .0801 for the thread height
NUMBER OF TIMES THREADING?
• Input AUTO SET (F1)
SPINDLE PERIPHERIAL SPEED?
• Input AUTO SET (F1)
FIRST THREADING AMOUNT?
• Input .010
TOOL TYPE?
• Input 6 for the threading tool number.
X START POINT?
• Input 1.0
Z START POINT?
• Input 0
X END POINT?
• Input 1.0
Z END POINT?
• Input .85
• Select SHAPE END from the Menu keys
A new Process Number is started. Select the next
Machining Unit type.
Select END from the Menu keys (F8)
COUNT NUMBER OF MACHINED WORKPIECES
<YES = 1, NO = 0>?
• Input 0
TOOL RETURN POSITION <0 = CHANGE
POSITION, 1 = HOME,
2 = FIXED POINT>?
• Input 1
Inputting this value will send the turret to the
Home position at the end of the
program.
WORK NUMBER OF FOLLOWING PROGRAM?
• Press Input to omit this setting
EXECUTE PERPETUALLY = 1; EXECUTE NUMBER
OF TIMES IN NUM = (0)
• Press Input to omit this setting
NUMBER OF TIMES TO REPEAT PROGRAM?
• Press Input to omit this setting.
Z SHIFT AMOUNT OF PROGRAM ORIGIN?
• Press Input to omit this setting.
This concludes programming of the part. A sample
of the program shape plot is displayed
in Figure 16 and the program output is displayed
in Figure 17.
Figure 16 Program Shape
Plot
Courtesy Solution Ware
Corp.
Figure 17 Finished
Turning Program
Courtesy SolutionWare
Corp