FUSION 640MT

PROGRAMMING

COURSE MANUAL
 640MT PROGRAMMING COURSE CONTENTS

Page
1. General Information………………………………….. 1-1
Machine and Work Co-ordinate System…………. 1-3
Fusion Overview…………………………………… 1-4
Key Layout………………………………………… 1-5
Display Map Screen……………………………….. 1-6

2. Basic Process Information (Turning)……………... 2-1

Edge Process (EDG)……………………………….. 2-3
Bar Process (BAR)………………………………… 2-4
Copy Process (CPY)……………………………….. 2-6
Corner Process (CNR)…………………………….. 2-8
Groove Process (GRV)…………………………….. 2-10
Thread Process (THD)…………………………….. 2-14
Drill Process (DRL)………………………………... 2-16
Tap Process (TAP)………………………………… 2-18

3. Program Examples (1 & 2)………………………….. 3-1

Suggested Set up Procedure………………………. 3-12
Tool Data…………………………………………… 3-13
Program Creation…………………………………. 3-17
Cutting Pattern Process Information…………….. 3-19
Set up Information ………….…………………….. 3-24
Program Layout…………………………………… 3-26
Tool Path…………………………………………… 3-28

4. Crossing Point Calculations………………………… 4-1

Angle Descriptions………………………………… 4-3
Circular and Angular Intersections………………. 4-11

C-1
5. T.P.C. ………………………………………………….. 5-1
T.P.C. Function……………………………………. 5-3
T.P.C. Display……………………………………… 5-4

6. Parameters……………………………………………... 6-1
Parameters (Selected)……………………………... 6-3

7. Program Example (3 & 3a)…………………………. 7-1

Program 3 – ……………….………………………. 7-3
Program 3a – Work-Piece shape………………….. 7-7

8. Tool Suffix Codes……………………………………... 8-1

Application of Tool Suffix…………………………. 8-5

9. Cutting Conditions……………………………………. 9-1

Creation of User Cutting Conditions……………... 9-3

10. Program Example 4…………………………………... 10-1

Manual Programming (MNP)…………………….. 10-8
M Codes……………………………………………. 10-14
Programming of Tailstock………………………… 10-23
End Process………………………………………… 10-24

11. Data I/O…………………………………………………. 11-1

IC Memory Card Operation……………………… 11-4
FDD Operation…………………………………….. 11-8
Hard Disk Operation……………………………… 11-11

C-2
 MAZATROL FUSION 640MT

GENERAL INFORMATION

1-1
MAZATROL FUSION 640MT

1-2
 MAZATROL FUSION 640MT

WORKPIECE COORDINATE SYSTEM

2-AXIS LATHE SPECIFICATION:

1-3
 MAZATROL FUSION 640MT

Q.What is Fusion?

MAZATROL FUSION 640

Control Basic Hardware

Construction

CNC SIDE PC SIDE

64 BIT RISC CHIP

32 BIT - 486DX4
(O/S - VX WORKS)
100MHz
MEMORY (SRAM)
16MB RAM
512KB - FOR TOOL MEMORY
DATA/PARAMETER
ETC.
HARD DRIVE - 2GB
MEMORY (DRAM) WORK PROGRAMS
1MB - WORK SYSTEM FILES ETC.
PROGRAMS

ISA BUS

NUMBER OF REGISTERED PROGRAMS - STANDARD 256

A. The integration of a P.C. and a C.N.C.

P.C. (A personal computer.)

C.N.C. (A computer numerical control)

1-4
 MAZATROL FUSION 640MT

KEY LAYOUT

Function
keys F1-F12

Reset key

Mouse pad

Numeric
Key Pad
Input Key

V.F.C
Page Keys

Alpha
Key Pad
Cursor
Keys

Window Key
Override Tab Key
keys

1-5
 MAZATROL FUSION 640MT

THE DISPLAY MAP SCREEN

This screen is an aid to finding your way around the various displays on the
Mazatrol fusion system.

Using the cursor keys, highlight the display you wish to go to, then press the
INPUT key. The screen will change to the required display.

1-6
 MAZATROL FUSION 640MT

BASIC PROCESS INFORMATION

2-1
MAZATROL FUSION 640MT

2-2
 MAZATROL FUSION 640MT

EDG FCE

X
S

F
Z

POINTS TO NOTE

1. EDG FCE is used to face off the material to the right hand side of Z zero.
2. The control automatically positions the tool(s) clear of the material boundary by
clearance amounts set in parameters
3. The actual equal rough depth of cut per pass is based on the Z axis rough stock
removal and the maximum permissable depth of cut per pass (initially selected from
the Cutting Condition data page)

4. It is the centre of the tool nose radius (and not the setting point of the tool), that
feeds to the Final Point X.
5. The centre of the tool nose radius will optionally feed past the Final Point X by
an amount set in a parameter.

NB. S = Starting Point F = Final Point

2-3
 MAZATROL FUSION 640MT

BAR OUT BAR IN

X X
C

S
S
C
Z Z

F F

POINTS TO NOTE
1. The Cutting Point is the co-ordinate value of the maximum material boundary for
this particular machining process.
2. The control automatically positions the tool(s) clear of the material boundary by
clearance amounts set in parameters.
3. Positions to the right hand side of Z zero are defined as negative (-) Z
co-ordinates.
4. The actual radial roughing depth of cut per pass is as set in the rough depth of cut
column in the program.
5. The order of definition of the SEQuence data, (finish profile shape), should be
the same as the required tool path of the finishing tool.
NB. C = Cutting Point S = Starting position of SEQuence data
F = Main feed direction

2-4
 MAZATROL FUSION 640MT

BAR FCE BAR BAK

X X
C
C

F
F S
S

Z Z

POINTS TO NOTE
1. The Cutting Point is the co-ordinate value of the maximum material boundary for
this particular machining process.
2. The control automatically positions the tool(s) clear of the material boundary by
clearance amounts set in parameters.
3. Positions to the right hand side of Z zero are defined as negative (-) Z
co-ordinates.
4. The actual roughing depth of cut per pass is as set in the rough depth of cut
column in the program.
5. The order of definition of the SEQuence data, (finish profile shape), should be
the same as the required tool path of the finishing tool.
NB. C = Cutting Point S = Starting Position of the SEQuence data
F = Main feed direction

2-5
 MAZATROL FUSION 640MT
CPY OUT CPY IN

X X
C

S S

Z Z

SZ

SX
SX
SZ

F F

POINTS TO NOTE
1. The Cutting Point is the co-ordinate value of the maximum material boundary for
this particular machining process.
2. The control automatically positions the tool(s) clear of the material boundary by
clearance amounts set in parameters.
3. Positions to the right hand side of Z zero are defined as negative (-) Z
co-ordinates.
4. The order of definition of the SEQuence data, (finish profile shape), should be
the same as the required tool path of the finishing tool.
5. The stock removal values for X and Z should be based on the worst conditions in
the X axis
6. The number of passes taken depends on the amount of stock removal X and the
rough depth of cut per pass stated in the program.
7. The cutting feed where the tool moves outside of the stock material shape when
roughing can be increased by parameter setting.
NB. C = Cutting Point S = Starting Position of the SEQuence data
F = Main feed direction SX = Stock Removal X SZ = Stock Removal Z

2-6
 MAZATROL FUSION 640MT
CPY FCE CPY BAK

X X
S
C S
C

F F

Z Z
SX

SX

SZ SZ

POINTS TO NOTE

1. The Cutting Point is the co-ordinate value of the maximum material boundary for
this particular machining process.
2. The control automatically positions the tool(s) clear of the material boundary by
clearance amounts set in parameters.

3. Positions to the right hand side of Z zero are defined as negative (-) Z
co-ordinates.
4. The order of definition of the SEQuence data, (finish profile shape), should be
the same as the required tool path of the finishing tool.

5. The stock removal values for X and Z should be based on the worst conditions in
the Z axis.

6. The number of passes taken depends on the amount of stock removal Z and the
rough depth of cut per pass stated in the program.
7. The cutting feed where the tool moves outside of the stock material shape when
roughing can be increased by parameter setting.
NB. C = Cutting Point S = Start Position of the SEQuence data
F = Main feed direction SX = Stock Removal X SZ = Stock Removal Z

2-7
 MAZATROL FUSION 640MT

CNR OUT CNR IN

E X

X
S
S E

Z Z

F F

POINTS TO NOTE
1. The Starting Point X is the Target Diameter to be finished turned. The Final
Point in Z is the Z co-ordinate being turned to.
2. The control automatically positions the tool clear of the material by clearance
amounts set in parameters.
3. Positions to the right hand side of Z zero are defined as negative (-) Z
co-ordinates.
4. The actual radial roughing depth of cut per pass is as set in the rough depth of cut
column in the program.
NB. S = Starting Point X,Z E = Final Point X,Z F = Main feed direction

2-8
 MAZATROL FUSION 640MT

CNR FCE CNR BAK

E X
E
S
X

F
S

Z F Z

POINTS TO NOTE

1. The Starting Point X is the Target Diameter to be finished turned. The Final
Point Z is the Z co-ordinate to finish face at.
2. The control automatically positions the tool clear of the material by clearance
amounts set in parameters.

3. Positions to the right hand side of Z zero are defined as negative (-) Z
co-ordinates.
4. The actual roughing depth of cut per pass is as set in the rough depth of cut
column in the program.

NB. S = Starting Point X,Z E = Final Point X,Z F = Main feed direction

2-9
 MAZATROL FUSION 640MT

GRV OUT GRV OUT

X X

S
E S E
F F
P -ve P +ve

Z Z

TYPE #0, #3 TYPE #1, #2, #4, #5

POINTS TO NOTE
1. The control automatically positions the tool clear of the material by clearance
amounts set in parameters.
2. A Positive Pitch will move the tool towards the chuck and a Negative pitch will
move the tool away from the chuck to machine subsequent grooves.
3. The width of groove is based on the width at the widest point.

4. For cycles #0 and #3, the reference edge used for programming is the Left Hand
side. For cycles #1, #2, #4 and #5, the reference edge used for programming is the
Right Hand side.
NB. S = Start Point X,Z E = Final Point X,Z P = Pitch
F= Main feed direction

2-10
 MAZATROL FUSION 640MT

GRV IN GRV IN

X X

E
F F
E

S
S

Z Z

P -ve P +ve

TYPE #0, #3 TYPE #1, #2

POINTS TO NOTE

1. The control automatically positions the tool clear of the material by clearance
amounts set in parameter.

2. A Positive Pitch will move the tool towards the chuck and a Negative Pitch will
move the tool away from the chuck to machine subsequent grooves.

3. The width of groove is based on the width at the widest point.

4. For cycles #0 and #3, the reference edge used for programming is the Left Hand
side. For cycles #1 and #2, the reference edge used for programming is the Right
Hand side.

NB. S = Start Point X,Z E = Final Point X,Z P = Pitch

F = Main feed direction

2-11
 MAZATROL FUSION 640MT

GRV FCE GRV FCE

X X

S
P -ve
P +ve
E E S

Z Z

F F

TYP #0, #3 TYP #1, #2

POINTS TO NOTE
1. The control automatically positions the tool clear of the material by clearance
amounts set in parameters.
2. A Positive Pitch will move the tool towards the centreline and a Negative Pitch
will move the tool away from the centreline to machine subsequent grooves.
3. The width of the groove is based on the width at the widest point.

4. For cycles #0 and #3, the reference edge used for programming is the BOTTOM
EDGE. For cycles #1 and #2, the reference edge used for programming is the TOP
EDGE.
NB. S = Start point X,Z E = Final Point X,Z P = Pitch
F = Main feed direction

2-12
 MAZATROL FUSION 640MT

GRV BAK GRV BAK

X X
S

P - ve
P +ve
E F F
E
S

Z Z

TYP #0, #3 TYP #1, #2

POINTS TO NOTE

1. The control automatically positions the tool clear of the material by clearance
amounts set in parameters.
2. A Positive Pitch will move the tool towards the centreline and a Negative Pitch
will move the tool away from the centreline to machine subsequent grooves.

3. The width of the groove is based on the width at the widest point.
4. For cycles #0 and #3, the reference edge used for programming is the BOTTOM
EDGE. For cycles #1 and #2, the reference edge used for programming is the TOP
EDGE.
NB. S = Start Point X,Z E = Final Point X,Z P = Pitch
F = Main feed direction

2-13
 MAZATROL FUSION 640MT

THD OUT THD IN

X X

E S E

Z Z

F F

POINTS TO NOTE

1. The control automatically positions the tool clear of the material by clearance
amounts set in parameters.
2. The amount of stand-off required for acceleration is automatically calculated by
the control but is limited by parameters.
3. The programmed Lead is equal to the Pitch of the thread x the Number of
Entrance.
4. For a thread parallel to the Z axis, the start and final points in the X axis are
equal.
NB. S = Start Point X,Z E = Final Point X,Z F = Main feed direction

2-14
 MAZATROL FUSION 640MT

THD FCE THD BAK

X X

S
F F
S
E
E

Z Z

POINTS TO NOTE

1. The control automatically positions the tool clear of the material by clearance
amounts set in parameters.
2. The amount of stand-off required for acceleration is automatically calculated by
the control but is limited by parameters.
3. The programmed Lead is equal to the Pitch of the thread x the Number of
Entrance.
4. For a thread parallel to the X axis, the start and final points in the Z axis are
equal.
NB. S = Start Point X,Z E = Final Point X,Z F = Main feed direction

2-15
 MAZATROL FUSION 640MT

DRL FCE
BOTTOMED

E S

POINTS TO NOTE

1. The control automatically positions the tool clear of the material by a clearance
amount set in a parameter.
2. Positions to the right of Z zero are defined as negative (-) Z co-ordinates.
3. When using the BOTTOMED drill cycles, the programmed depth is based on the
depth of the drill point in the material.
4. Feedrate at the start can be altered by parameter.
5. Cycle Types: #0 = Peck, Feed Retract. #1 = Peck, Chip Clear.
#2 = Peck, Chipbreak #3 = Ream
#4 = #2 & #1 Combination
NB. S = Starting Point Z E = Final Point Z F = Main feed direction

2-16
 MAZATROL FUSION 640MT

DRL FCE
THROUGH

E S

Z Z

POINTS TO NOTE

1. The control automatically positions the tool clear of the material by a clearance
amount set in a parameter.

2. Positions to the right of Z zero are defined as negative (-) Z co-ordinates.

3. When using the THROUGH drill cycles, the programmed depth is based on the
full diameter drilling depth - (material length). The control automatically allows for
the extra drilling depth by referring to the Tool Data Display page (for the drill
point allowance) and additionally to a parameter for through clearance.
4. Feedrate at the start can be altered by parameter.

5. Cycle Types: #0 = Peck, Feed Retract. #1 = Peck, Chip Clear.

#2 = Peck, Chipbreak #3 = Ream
#4 = #2 & #1 Combination
NB. S = Starting Point Z E = Final Point Z F = Main feed direction

2-17
 MAZATROL FUSION 640MT

TAP FCE

E
S

POINTS TO NOTE

1. The control automatically positions the tool clear of the material by a clearance
amount set in a parameter.

2. Positions to the right of Z zero are defined as negative (-) Z co-ordinates.

3. The Final Point Z co-ordinate is based on the full thread length.
4. The control automatically allows for the taper lead section of the tap by a
parameter setting.
5. The control automatically allows for the tapper elongation when retracting by a
parameter setting.
NB S = Starting Point Z E = Final Point Z F = Main feed direction

2-18
 MAZATROL FUSION 640MT

PROGRAMMING
EXAMPLE NO.1

3-1
 MAZATROL FUSION 640MT

3-2
 TITLE: PROGRAM EXAMPLE 1

100
75
68
48
30 Chamfer 2.5mm x 45°

R20
3

3-3
60

80
45

40
50
70

100
M65 x 2mm

38°
20

30

48
SURFACE FINISH TO BE 3.2um Ra ALL OVER

MATERIAL SIZE: DRAWN BY: CHECKED BY:

100 O/D x 40 I/D x 102mm LONG DRAWING NUMBER:
MATERIAL: ALUMINIUM
MAZATROL FUSION 640MT
 MAZATROL FUSION 640MT

Tooling Sheet - Program 1

GNL OUT GNL OUT

(R.TURN) (F.TURN)
TOOL HOLDER TOOL HOLDER
TYPE 2 TYPE 2

93° 55° (LH TOOL SHOWN) 93° 55° (RH TOOL SHOWN)

GRV OUT THD OUT

(GROOVE) (THREAD)
TOOL HOLDER TOOL HOLDER
TYPE 2 TYPE 2

5 (RH TOOL SHOWN) (RH TOOL SHOWN)

2.1

80°
95°

GNL IN
( ROUGH & FINISH BORE)
TOOL HOLDER
TYPE 1

(LH TOOL SHOWN)

3-4
 MAZATROL FUSION 640MT

EXAMPLE PROGRAM 1

PNo. MAT OD-MAX ID-MIN LENGTH RPM FIN-X FIN-Z WORK FACE
0 S45C 100. 40. 102. 3000 0.4 0.1 2.

PNo. MODE # 1 # 2 # 3 # 4 # 5 # 6 # 7 # 8 # 9 #10 #11 #12

1M 8

PNo. MODE RV FV R-FEED R-DEP. R-TOOL F-TOOL

2EDG FCE 375 400 0.35 3. GNL OUT A GNL OUT B
SEQ SPT-X SPT-Z FPT-X FPT-Z ROUGH
1 100. 2. 40. 0. Rgh 4

PNo. MODE # CPT-X CPT-Z RV FV R-FEED R-DEP. R-TOOL F-TOOL

3BAR OUT 0 100. 0. 150 280 0.4 5.5 GNL OUT A GNL OUT B
SEQ SHP S-CNR SPT-X SPT-Z FPT-X FPT-Z F-CNR/$ RADIUS/ø ROUGH
1LIN C2.5 * * 65. 30. * Rgh 4
2TPR 65. 30. 70. 33.2 38 Rgh 4
3LIN * * 70. 48. * Rgh 4
4CCW 70. 48. 80. 68. 20. Rgh 4
5LIN * * 80. 75. * Rgh 4
6LIN C0.5 * * 100. 75.5 Rgh 4

PNo. MODE # CPT-X CPT-Z RV FV R-FEED R-DEP. R-TOOL F-TOOL

4BAR IN 0 40. 0. 150 280 0.4 5. GNL IN A GNL IN A
SEQ SHP S-CNR SPT-X SPT-Z FPT-X FPT-Z F-CNR/$ RADIUS/ø ROUGH
1LIN R 0.1 * * 50. 20. * Rgh 4
2TPR 50. 20. 45. 30. Rgh 4
3LIN * * 45. 48. * Rgh 4
4LIN C0.5 * * 40. 48.5 Rgh 4

Pno. MODE # No. PITCH WIDTH FINISH RV FV FEED DEP. R-TOOL F-TOOL
5GRV OUT 0 1 3. * * 139 0.1 2. * GRV OUT A
SEQ S-CNR SPT-X SPT-Z FPT-X FPT-Z F-CNR ANGLE ROUGH
1 65. 30. 60. 30.

PNo. MODE # CHAMF LEAD ANG MULTI HGT NUMBER V DEPTH TOOL
6THR OUT 2 0 2. 60 1 1.299 * 105 0.337 THD OUT A
SEQ SPT-X SPT-Z FPT-X FPT-Z
1 65. 0. 65. 29.

PNo. MODE COUNTER RETURN WK.No. CONT. NUM. SHIFT

7END 1 0 0 0 0.

3-5
 MAZATROL FUSION 640MT

3-6
 MAZATROL FUSION 640MT

PROGRAMMING
EXAMPLE No 2

3-7
 MAZATROL FUSION 640MT

3-8
 TITLE: PROGRAM EXAMPLE 2

0
R2
R2
3

40°
21
25

3-9
75

90
50
55
90
95

120
60.15

110.41
40 M62 x 1.5mm

20 Chamfer 1mm x 45°

25

55

65

90
MATERIAL SIZE: DRAWN BY: DATE:
120 O/D x 50 I/D x 95mm LONG DRAWING NUMBER:
MATERIAL: ALUMINIUM
MAZATROL FUSION 640MT
 MAZATROL FUSION 640MT
Tooling Sheet - Program 2

GNL OUT GNL OUT

(R.TURN) (F.TURN)
TOOL HOLDER TOOL HOLDER
TYPE 2 TYPE 2

95° 80° (LH TOOL SHOWN) 93° 55° (RH TOOL SHOWN)

GRV OUT
(GROOVE)
TOOL HOLDER
TYPE 2

6 (RH TOOL SHOWN)

2.

80°
95°

GNL IN
( ROUGH & FINISH BORE)
TOOL HOLDER
TYPE 1

(LH TOOL SHOWN)

THD IN
( THREAD)
TOOL HOLDER
TYPE 1

(RH TOOL SHOWN)

3-10
 MAZATROL FUSION 640MT

EXAMPLE PROGRAM 2

PNO. MAT OD-MAX ID-MIN LENGTH RPM FIN-X FIN-Z WORK FACE
0 AL 120. 50. 95. 3000 0.4 0.1 5.

PNo. MODE # 1 # 2 # 3 # 4 # 5 # 6 # 7 # 8 # 9 #10 #11 #12

1M 8

PNo. MODE RV FV R-FEED R-DEP. R-TOOL F-TOOL

2EDG FCE 375 400 0.35 3. GNL OUT A GNL OUT B
SEQ SPT-X SPT-Z FPT-X FPT-Z ROUGH
1 120. 5. 50. 0. Rgh 4

PNo. MODE # CPT-X CPT-Z RV FV R-FEED R-DEP. R-TOOL F-TOOL

3BAR OUT 0 120. 0. 375 468 0.4 5.5 GNL OUT A GNL OUT B
SEQ SHP S-CNR SPT-X SPT-Z FPT-X FPT-Z F-CNR/$ RADIUS/ø ROUGH
1TPR 75. 0. 90. 20. R 2. Rgh 4
2LIN * * 95. 55. * Rgh 4
3CCW 110.41 55. 120. 65. 20. Rgh 4

PNo. MODE # CPT-X CPT-Z RV FV R-FEED R-DEP. R-TOOL F-TOOL

4BAR IN 0 50. 0. 150 280 0.4 5. GNL IN A GNL IN A
SEQ SHP S-CNR SPT-X SPT-Z FPT-X FPT-Z F-CNR/$ RADIUS/ø ROUGH
1TPR 63.15 0. 60.15 1.5 Rgh 4
2LIN * * 60.15 25. * Rgh 4
3LIN * * 55. 40. * Rgh 4
4TPR 55. 40. 50. 42.979 40. Rgh 4

Pno. MODE # No. PITCH WIDTH FINISH RV FV FEED DEP. R-TOOL F-TOOL
5GRV OUT 0 2 5. 3. * * 348 0.1 2. * GRV OUT A
SEQ S-CNR SPT-X SPT-Z FPT-X FPT-Z F-CNR ANGLE ROUGH
1 95. 25. 90. 25. Rgh 4

PNo. MODE # CHAMF LEAD ANG MULTI HGT NUMBER V DEPTH TOOL
6THR IN 0 2 1.5 60 1 0.974 9 121 * THD IN A
SEQ SPT-X SPT-Z FPT-X FPT-Z
1 62. 0. 62. 21.

PNo. MODE COUNTER RETURN WK.No. CONT. NUM. SHIFT

7END 1 0 0 0 0.

3-11
 MAZATROL FUSION 640MT

SUGGESTED PROGRAM & SET-UP PROCEDURE

1. DECIDE MACHINING METHOD & TOOLING REQUIREMENTS.

2. ENTER (TOOL DATA) INFORMATION & (TOOL SET)

3.CREATE (PROGRAM) & (SHAPE CHECK)

4.CREATE (SET-UP INFO.) DESCRIBE (CHUCK JAW DATA) Z-OFFSET ETC.

5. (TOOL PATH) CHECK, AND/OR (SOLID MODE)

6. EDIT (PROGRAM) OR (LAYOUT) AS NECESSARY.

7.RE - (TOOL PATH) CHECK.

NB: ACCESS TO ALL THE ABOVE (----) SCREENS CAN BE MADE VIA
(DISPLAY- MAP).

3-12
 MAZATROL FUSION 640MT

TOOL DATA DISPLAY

To enter a tool in to the TOOL DATA DISPLAY, move the cursor to the required
magazine position, either horizontal or vertical depending upon the attitude the tool will be
working, then push the EDIT TOOL menu. (If the tool position has data in it, use the
ERASE key to clear the existing information.)

The display will change to look like this. Select the appropriate tool shape from the Menu
options, for example:

3-13
 MAZATROL FUSION 640MT

MACHINING PART OF TOOL. Describe which part of the work-piece the tool is
going to cut on. The options are. OUT = outside Dia, IN = inside Dia, EDG = the face of
the component. (Machines having 2nd spindle capability will also have the BAK options to
consider.)

ID CODE: can be used to give a tool a unique identity, distinguishing it from other tools
of the same type, for which a description already exist in Tool Data.

Setting the CUTTING DIRECTION tells the machine which way the cutting tool face’s,
and is used to fix the direction the spindle will rotate when the tool is in use.

Next, input the TOOL NOSE RADIUS of the cutting tool.

3-14
 MAZATROL FUSION 640MT

Now enter the angles for the tool, firstly the CUTTING ANGLE, this is taken
from the horizontal plane to the leading edge of the tool (e.g. 93 degrees.).Then
the CUTTING EDGE ANGLE, the angle of the insert in the cutting tool.(e.g. 80
degrees).

HOLDER TYPE, enter a value from 1 to 4 at this point, from this the machine
is told the type and size of tool holder to be used, the information is set in
parameters, and will vary depending on the machine model type. Entering a
0 at this stage would indicate no tool holder to be used.

TOOL USAGE; Describes the type of cutting operation the tool is to be used for.
The options are ROUGH, stating the tool to be used for only rough machining.
FINISH for Finish machining only. COMMON and the tool can be used for both
rough and finish machining operations. This information is used for AUTO tool selection.

3-15
 MAZATROL FUSION 640MT
WIDTH OF TOOL SHANK; Enter the shank size of the cutting tool (e.g. 25mm).

MATERIAL; Enter the material that the cutting tool tip is made of, from the menu choices
(e.g. HSS L, CARBIDE L etc.)

COMMENT; Various information could be entered at this position. (e.g. Tool tip grade, or,
tool tip code for reordering. ) Entry is optional in this area.

GROUP No.; you may enter here the tool group number you want this tool to become a part
of when using Sister Tooling and considering spare tool selection.

OFS No.; This is the offset used for this tool, only when using EIA/ISO programming
format.
TURRET DIRECTION; This will default to the attitude of the tool as it is set
in the magazine of the machine, but if required a tool can be rotated through 180 degrees
from forward facing to reverse facing by selecting the highlighted options
at this point.

3-16
 MAZATROL FUSION 640MT

PROGRAM CREATION

To create new a program, first push the “F1” key (far left-hand menu key).

The menus will change to appear like this.

Now push the menu key, corresponding to the PROGRAM menu.

3-17
 MAZATROL FUSION 640MT

A window will appear within the screen display. This window shows you the programs
that are currently stored in the machine memory (Program File). To start a new program
then, enter an identifying Work Number (between 1~99999999) checking from the
window that the number to be selected doesn’t already exist in the machine and a new
program record will be started.

3-18
 MAZATROL FUSION 640MT

3-19
 MAZATROL FUSION 640MT

3-20
 MAZATROL FUSION 640MT

3-21
 MAZATROL FUSION 640MT

3-22
 MAZATROL FUSION 640MT

3-23
 MAZATROL FUSION 640MT

3-24
 MAZATROL FUSION 640MT

3-25
 MAZATROL FUSION 640MT

PROGRAM LAYOUT DISPLAY

To access the Program Layout Display select the PROGRAM option from the main menu,
then press the LAYOUT key.

The PROGRAM LAYOUT display allows you to change the order in which the program
will run. This is achieved by assigning a priority order to the units in the program. The
information shown in the LAYOUT display is; The unit number from within the program,
the Unit name and tool description along with the roughing and finishing prefix.

The layout shown in the view shown above is in Program Priority, that is the order in which
it was originally written, this is the order in which the units would be processed in cycle. To
make the machine cut all the roughing operations, and then all the finishing operations,
push the ROUGHING PRIORITY menu key and then INPUT.

3-26
 MAZATROL FUSION 640MT

The view above shows the Program Layout in ROUGH priority order. The new running
order of the program can be viewed, now all rough turning operations are performed 1 st,
followed by all finish turning operation, if there are milling units in the program then they
will be performed after the turning in rough and then finishing order.
NOTE.
Care should be taken when ROUGH priority is selected, and M code or Manual Program
units are used within the program. The control see’s all M code and Manual program units as
being Roughing operations.

To change the position of an individual unit within the layout, highlight the unit to be
moved then select the MOVE key, using the cursor control keys re-position the unit
in the desired position, press input to complete the move.

3-27
 MAZATROL FUSION 640T
TOOL PATH DISPLAY
The TOOL PATH display can be used to simulate your program, once it’s complete.
To access the TOOL PATH display, from the PROGRAM display, select the menu
marked TOOL PATH.

The screen will show the outline of your material. Push the PART SHAPE menu, and the
part profile will be drawn.

The menu, DISPLAY MODE, allows you to change the screen view from a sectional
view only, to a sectional, and end on view. (3 Axis spec machines only). SCALE
CHANGE allows you to zoom in or out on a particular section of the screen.

3-28
 MAZATROL FUSION 640T
CHECK CONTINUE will run the tool path check permitting you to see the path taken by
the tool. Rapid movements are shown as dotted lines, feed movements as solid lines. The
position of the tool nose radius centre is represented by an inverted red triangle.
The CHECK STEP menu allows you to step the tool path through each movement the
machine will make. The menu, TOOL PATH ERASE, allows you to remove the tool path’s
that have already taken place, allowing you a clearer view of the tool path’s to come.
Necessary

SOLID MODE

Solid mode allows you to see a 3 dimensional view of your component. It will also show the
cutting tools in 3D.
The ZOOM +/- menu allows you to increase or decrease the size of the 3D image. Use the
UP cursor key to increase. The DOWN cursor key to reduce.
The menu, ROTATION, allows you to rotate the 3D image; again the cursor keys are
used. LEFT CURSOR to rotate to the left, RIGHT CURSOR to rotate to the right, UP
CURSOR to rotate the front of the image up and DOWN CURSOR, to rotate the front of
the image down.

The SECTION menu allows you to remove a quarter or a half section of the image. This
can be particularly useful when internal operations have been programmed.

3-29
 MAZATROL FUSION 640T

Push the menu CHECK CONTINUE, and the tool path graphics will be performed in 3D
mode. The CHECK STEP menu allows you to run the tool path one step at a time.

The menu PROGRAM MONITOR when pushed opens a window within the Tool Path
screen. This window will show you a Program listing. This list will consist of: the unit
numbers with the roughing and finishing prefix, the unit names i.e. BAR OUT, BAR IN
etc, and the tool numbers used in each unit.
The PROGRAM MONITOR will highlight each line being shown, as it is being performed
in the tool path graphics.

If the PROGRAM MONITOR window obscures your view of the tool path graphics, push
the MOVE menu, then, using the cursor keys, move the graphics to a more convenient
location. (The MONITOR window must be closed when you do this).

3-30
 MAZATROL FUSION 640MT

CROSSING POINT CALCULATIONS

4-1
 MAZATROL FUSION 640MT

4-2
 MAZATROL FUSION 640MT

AUTOMATIC CROSSING-POINT CALCULATION

FUNCTION
Automatic crossing-point calculation function for the NC system is to compute
unknown coordinates of a point of intersection on an arbitrary form and to
automatically enter the result in a program.

AUTOMATIC CROSSING-POINT CALCULATION IN THE LINEAR AND FACE

MACHINING UNITS
A crossing-point of arbitrary form is automatically calculated in the linear and
face machining units.

COORDINATES OF THE CROSSING-POINT

Even if coordinates of a crossing-point are unknown as illustrated below, the
NC system will automatically obtain it from the coordinates of the start and
end points and from angles involved.

FIG SHP SHIFT-R Z Y RADIUS/θ I J P CNR RGH

1 LIN 10. 50. 20.
2 LIN u ? ? 30.
3 LIN u 150. 20. 100.

FIG SHP SHIFT-R Z Y RADIUS/θ I J P CNR RGH

1 LIN 10. 50. 20.
Displayed in yellow

2 LIN u 140.76 72.4 30.

3 LIN u 150. 20. 100.

150
50 Program origin

Z
20

30° Y
100° Start point

After checking the plane, return to the PROGRAM display again and the
coordinates so automatically obtained as a crossing-point will be displayed in
yellow.
Note 1: When unknown coordinates of a crossing-point are automatically
obtained in a combination of a line with an arc or of two arcs, do not
fail to enter P. (Select the position of crossing-point.)

4-3
 MAZATROL FUSION 640MT
FIG SHP SHIFT-R Z Y RADIUS/θ I J P CNR RGH
1 LIN 10. 50. 20.
2 LIN u ? ? 30.
3 CW u 165. 20. 40. 125. 20.

125

(125, 20) 50
Program origin
(165, 20)
Z
20
30°

R:40 Y
(?,?)

Select RIGHT or UP
in the item P.

Select LEFT or DOWN

in the item P.

Note 2: To obtain the coordinates of the crossing-point of the right side,

press the RIGHT or UP menu key

Examples of automatic crossing-point calculation

A crossing-point is automatically calculated for combinations of line with
line, line with arc and arc with arc as shown in the examples below.

Pattern Shape Shape sequence

150
50
FIG SHP SHIFT-R Z Y RADIUS/θ I J P CNR
LIN
1 LIN 50. 20.
20
| 2 LIN ? ? 30.
30°
LIN 120° 3 CW 150 20. 120. 120. 20.
.
( ?, ? )

LIN 150
50 FIG SHP SHIFT-R Z Y RADIUS/θ I J P CNR
|
1 LIN 50. 20.
ARC
(120, 20) 20
2 LIN ? ?
(Contacting)
3 CW 150 20. 30. 120. 20.
R30
( ?, ? ) .

4-4
 MAZATROL FUSION 640MT

Pattern Shape Shape sequence

50
LIN
(200, 0)
FIG SHP SHIFT-R Z Y RADIUS/θ I J P CNR
| 20
1 LIN 50. 20.
ARC (200, 80) 30°
Z 2 LIN ? ? 30. R
(Intersecting) R80 3 CW 200 0. 80. 200 80.
Select RIGHT or UP.
Y

Closed

R4
FIG SHP SHIFT-R Z Y RADIUS/θ I J P CNR

(40, 5) R10 1 CW ? ? 10. 20. 5. D R4

ARC (20, 5) 2 CW ? ? 15. 40. 5. U R4

R15

R4

Open

ARC (55, ?) R10

(?, ?) 10
FIG SHP SHIFT-R Z Y RADIUS/θ I J P CNR
(45, ?)
1 LIN 10. 5.
(25, 5) 5
2 CW ? ? 15. 25. 5. U

3 CCW 55. ? 10. 45. ?

R15

Closed g4
(?, ?)
ARC g5
FIG SHP SHIFT-R Z Y RADIUS/θ I J P CNR
(?, ?)
|
1 LIN ? ?
(55, 5) R10
LIN 2 CW ? ? 10. 20. 5.
(20, 5)
| R15 3 LIN ? ?
(?, ?) 4 CW ? ? 15. 55. 5.
ARC g2
(?, ?)
g3

ARC g2 10
g3 FIG SHP SHIFT-R Z Y RADIUS/θ I J P CNR
(75, 5) (?, ?)
|
1 LIN 10. 5.
(60, 5) (20, 5) 5
ARC 2 CW ? ? 10. 20. 5.
R15
| R10 3 CCW ? ? 45.

4 CCW 75. 5. 15. 60. 5.

ARC
R45

l: Both Z and Y coordinates are known (i, j in the case of the center of an arc).
†: Both Z and Y coordinates are not known (i, j in the case of the center of an arc

4-5
 MAZATROL FUSION 640MT
AUTOMATIC CROSSING-POINT CALCULATION FUNCTION IN THE
TURNING UNIT
When a TPR, or shape is to be defined on the sequence line of the bar-materials
machining unit (BAR) or the copy-machining unit (CPY), or when an oblique groove,
isopodic trapezoidal groove, or tapered groove shape is to be defined on the sequence line
of the groove-machining unit (GRV), you can make the NC unit automatically calculate
any unknown coordinates of the start point or end point of that shape.
Automatic calculation may be performed within one sequence or it may span over two
sequences.
Conditions for automatic calculation are as follows.
- Automatic calculation within one sequence
Unit Shape pattern Conditions
BAR 1. TPR One of the items SPT-X, SPT-Z, FPT-X and FPT-Z is unknown; tapering angle known.
or 2. Arc One item of the data pair (SPT-X, SPT-Z) or (FPT-X, FPT-Z) is unknown;
CPY center coordinates and radius of arc known.

GRV 3. - One of the items SPT-X, SPT-Z, FPT-X and FPT-Z is unknown; tapering angle known.

- Automatic calculation over two sequences

Unit Shape pattern Conditions
4. Intersection of X- and Z-coordinates of the intersecting point of two taperings are unknown;
two TPRs two angels of tapering known.
5. Intersection of X- and Z-coordinates of the intersecting point of tapering and arc are unknown;
TPR and arc tapering angle and center coordinates and radius of arc known.
BAR
6. Osculation of X- and Z-coordinates of the osculation point of tapering and arc are unknown;
or
TPR and arc center coordinates and radius of arc, or tapering angle and radius of arc, are known.
CPY
7. Intersection of X- and Z-coordinates of the intersecting point of two arcs are unknown;
two arcs center coordinates and radii of both arcs known.
8. Osculation of X- and Z-coordinates of the osculation point of two arcs are unknown;
two arcs center coordinates and radius of one arc, and radius of the other arc are known.

- “Intersecting point” refers to a non-smoothly crossing point. Press the I. POINT? menu key
for an unknown intersecting point.
- “Osculation point” refers to a smoothly crossing point. Press the C. POINT? menu key
for an unknown osculation point.

TPR and TPR Arc and TPR Arc and Arc

Intersecting
point

Arc and TPR Arc and Arc

Osculation
point

4-6
 MAZATROL FUSION 640MT

- Automatic calculation can also be performed in grafically checking the

programmed data on the TOOL PATH or SHAPE CHECK display and the
result is entered in a program.
Given below is the procedure of data setting for automatic calculation in cases 1
to 8 shown in the table above.

1. IF START OR END POINT OF A TAPER IS UNKNOWN.

Example: FPT-Z of tapering is unknown.

20
End point to of tapering

30°

φ50 Start point of tapering

φ30

T4P288

Set data as follows:

UNo. UNIT # CPT-X CPT-Z RV FV R-FEED R-DEP.
BAR OUT

SEQ SHP S-CNR SPT-X SPT-Z FPT-X FPT-Z F-CNR/$ RADIUS/θ

1 LIN u u 30. 20. u
2 TPR 30. 20. 50. ? 30.

Press the I. POINT? menu key for the unknown FPT-Z.

Enter the tapering angle, 30°, for RADIUS/θ.
Note: Enter positive angle value to designate upward tapering, or negative
value for downward tapering.

OUT OUT IN IN FCE FCE BAK BAK

θ: Positive θ
value θ

θ θ

θ
θ: Negative
value
θ
θ θ

4-7
 MAZATROL FUSION 640MT

2. IF START OR END POINT OF ARC IS UNKNOWN.

SPT-Z and FPT-X of convex arc is unknown.

60

Start point of arc

End point of arc

R30

40 φ30
φ10

UNo. UNIT # CPT-X CPT-Z RV FV R-FEED R-DEP.

BAR OUT

SEQ SHP S-CNR SPT-X SPT-Z FPT-X FPT-Z F-CNR/$ RADIUS/θ

1 30. ? ? 60. 30.
2 CTR u 10. 40. u u u u

Press the I. POINT? menu key for the unknown SPT-Z and FPT-X.
Enter the radius of the convex arc, 30, for RADIUS/θ.
For the sequence data line next to that of convex arc, first press the CENTER
menu key and then enter the X- and Z-coordinates of the arc center in SPT-X and
SPT-Z, respectively.
<Supplement>
1. Enter the X-coordinate with minus sign for a center below the workpiece
center
line; likewise the Z-coordinate for a center on the right of program origin.
Example:

R40 10

φ40

φ20

4-8
 MAZATROL FUSION 640MT
SEQ SHP S-CNR SPT-X SPT-Z FPT-X FPT-Z F-CNR/$ RADIUS/θ RGH
1 ? 0. 40. ? 40.
2 CTR u -20. -10. u u u ←

2. / item for unknown SPT or at ROUGH In general, an arc and a line cross
each other at two points. To specify which one is to be set, use the menu keys
UP , DOWN , LEFT or RIGHT on the CTR sequence line at the
RADIUS for FPT.
Example:

47.321

b a

R20 SPT
FPT
φ50
φ40 30
φ20

SEQ SHP S-CNR SPT-X SPT-Z FPT-X FPT-Z F-CNR/$ RADIUS/θ RGH
1 50. ? 40. 47.321 20.
2 CTR u 20. 30. u u u →

To specify (a) for calculation of SPT-Z, press the RIGHT menu key at
RADIUS/ since the one point (a) lies on the right of the other possible
point (b).

3. IF START OR END POINT OF TAPERED SHAPE IS UNKNOWN

(FOR GRV UNIT).
As for the case 1, one of the items SPT-X to FPT-Z can be auto-set if the tapering
angle is clearly known.
Example: FPT-Z of tapering is unknown.

50

SPT

60°

φ80 FPT

φ40

4-9
 MAZATROL FUSION 640MT
Set data as follows:
UNo. UNIT # No. PITCH WIDTH FINISH RV FV
GRV OUT 0 1 0. 30. u u 120
SEQ S-CNR SPT-X SPT-Z FPT-X FPT-Z F-CNR ANGLE
1 80. 50. 40. ? 60.

For the grooving pattern #0, the ANGLE data must be entered as a positive or
negative value according to the direction of the respective tapering.
Enter positive values for θ Enter negative values for θ

OUT OUT

θ θ

θ θ
BAK BAK FCE
FCE
θ
θ θ θ
IN IN

For the patterns #1 to #3, the sign of the ANGLE data is insignificant.

4. IF INTERSECTING POINT OF TWO TAPERINGS IS UNKNOWN.

40
SHP SPT-X SPT-Z FPT-X FPT-Z RADIUS/θ

TPR 20. 0. ? ? 45.

*1 *2
TPR ? ? 80. 40. 30.
30° *1 *3
(?, ?)

φ80
*1. Press the I. POINT? menu key for unknown
45°
coordinates of the intersecting point of two taperings.
*2. Enter the tapering angle.
φ20 *3. Enter the tapering angle.

4-10
 MAZATROL FUSION 640MT

5. IF INTERSECTING POINT OF TAPERING AND ARC IS

UNKNOWN.
(?, ?)

(b)
(60, 55)
R25 (a)

30°

40
φ20 φ20

SHP S-CNR SPT-X SPT-Z FPT-X FPT-Z F-CNR RADIUS/θ RGH

TPR 20. 0. ? ? 30. *2
*1
? ? 60. 55. 25.
u u u u
*1 *3
CTR 20. 40. ←
*4 *5

*1. Press the I. POINT? menu key for unknown coordinates of the intersecting point of tapering and arc ( ).
*2. Enter the tapering angle.
*3. Enter the radius of arc.
*4. Enter the coordinates of arc center.
*5. To specify (b) from among the two intersecting points of tapering and arc, press the LEFT ← (or UP ↑)
menu key.

6. IF OSCULATION POINT OF TAPERING AND ARC IS UNKNOWN.

(?, ?)

(60, 65)
R25

50
φ20 φ20

SHP S-CNR SPT-X SPT-Z FPT-X FPT-Z F-CNR RADIUS/θ RGH

TPR 20. 0. ? ? *1† †
?† ? *1 60. †65. 25. *2
CTR u 20. 50. *3 u u u
*1. Press the C. POINT † ? menu key for unknown coordinates of the osculation point of tapering
and arc ( ).
*2. Enter the radius of arc.
*3. Enter the coordinates of arc center.

4-11
 MAZATROL FUSION 640MT

6. IF INTERSECTING POINT OF TWO ARCS IS UNKNOWN.

(80, 50)

R30
(?, ?)
(40, 0)
R25

φ20 20
φ10

50

SHP S-CNR SPT-X SPT-Z FPT-X FPT-Z F-CNR RADIUS/θ RGH

40. 0. ? ? *1 25. *2
TPR u 10. 20.
*3
u u u ↑
*6
? ? *1 80. 50. 30.
CTR u 20. 50. *5 u u u *4

*1. Press the I. POINT? menu key for unknown coordinates of the intersecting point of two convex arcs.
*2. Enter the radius of arc.
*3. Enter the coordinates of arc center.
*4. Enter the radius of arc.
*5. Enter the coordinates of arc center.
*6. To specify the upper one of the two possible intersecting points, press the UP ↑ menu key in response to
the message “INTERSEC POS OF FINAL POINT?”.

7. IF OSCULATION POINT OF TWO ARCS IS UNKNOWN.

95

R50

(?, ?)
φ140
R25
φ70
φ20

SHP S-CNR SPT-X SPT-Z FPT-X FPT-Z F-CNR RADIUS/θ RGH

70. 0. ? † ? † *1 25.
u u u
*2
CTR 20. 0. *3
u ? † ? † *1 140. 95. 50. *4

*1. Press the C. POINT † ? menu key for unknown coordinates of the osculation point of convex and
concave arcs.
*2. Enter the radius of convex arc.
*3. Enter the center coordinates of convex arc.
*4. Enter the radius of concave arc.

4-12
 MAZATROL FUSION 640MT

Supplement
IN CASES 5 TO 8, THE FOLLOWING UNKNOWN INTEMS CAN ALSO BE AUTO-
SET.
Example: For intersecting point of tapering and arc, SPT-X or -Z of tapering
and FPT-X or -Z of arc are unknown.

60

(b)
(d) (c)

R20
(a)
30°
φ50

30
φ20 φ20

SHP S-CNR SPT-X SPT-Z FPT-X FPT-Z F-CNR RADIUS/θ RGH

TPR 20. 0. ? ? 30.
*1 *2
? ? 50. ? 20.
u u u u
*1 *3 *4
CTR 20. 30. → ←
u u
*5 *6 *7
LIN 50. 60.

*1. Press the I. POINT? menu key for unknown coordinates of the intersecting point of tapering and
convex arc.
*2. Enter the tapering angle.
*3. Press the I. POINT? menu key for unknown FPT-Z of the convex arc.
In general, even an unknown coordinate of arc end point can be calculated with the intersecting point
of tapering and arc remaining unknown.
*4. Enter the radius of convex arc.
*5. Enter the center coordinates of convex arc.
*6, 7 Press the menu key UP ↑, DOWN , LEFT ← or RIGHT → at the items RADIUS/θ and ROUGH to
specify one of the two possible intersecting points of arc and tapering.
Press at RADIUS/θ the RIGHT → (or DOWN ↓) menu key to specify (a) from among the two
intersecting points of tapering and convex arc.
Press at ROUGH the LEFT ← menu key to specify (d) from among the two intersecting points of arc
and straight line.

4-13
 MAZATROL FUSION 640MT

4-14
 MAZATROL FUSION 640MT

4-15
 MAZATROL FUSION 640MT

4-16
 MAZATROL FUSION 640MT

T.P.C

(TOOL PATH CONTROL)

5-1
 MAZATROL FUSION 640MT

5-2
 MAZATROL FUSION 640MT

5-3
 MAZATROL FUSION 640MT

T.P.C. DISPLAY

The TOOL PATH CONTROL screen allows you to make changes to a specific
unit in a program. These changes will only effect the unit to which the T.P.C.
data is connected, and no other.
To access T.P.C. Push the PROGRAM menu at the program display.

Move the cursor to the unit heading you wish to change T.P.C. data for. Then
push the “F12” (menu select) key.

Now push the T.P.C. menu key.

5-4
 MAZATROL FUSION 640MT

T.P.C. DISPLAY cont.

The screen will change to look like this.

The T.P.C. display comprises of two basic areas.

These are: Parameters and Relay Points.

Parameters: Here you will see a list of selected parameters, and their settings.
Any changes made here will only effect this unit, and will make no changes to
the main parameter set.

Relay Points: These are broken down into two sections, one for APPROACH
relay points, which allow you to control the path of the tool when it is travelling
towards the cutting point of the unit. The second, ESCAPE relay points, allows
you to control the path of the tool when the tool is travelling away from the
component i.e. returning to the tool change position.
Relay points are also set separately for ROUGHING and FINISHING
operations, this allows you to control the paths taken by the roughing and
finishing tools independently of each other.

To input data in to the relay point positions, cursor to the position “[AUTO]”.
This position must be changed to “[MANUAL]”, as the machine will not allow
you to cursor into the areas below until this change has been made.

5-5
 MAZATROL FUSION 640MT

T.P.C. DISPLAY cont.

The cursor will automatically move to the position “1” for the APPROACH relay
point. Figures can now be input for the points you want the tool to pass through
when approaching the work piece. The “Z OFFSET” position is the reference for
these figures. For the “Z AXIS”, figures to the right of the “Z OFFSET” are
negative values. This is true for all units with the exception of EDG FCE, where
the figures to the right of the “Z OFFSET” are positive.

To close the TPC screen, push the “TPC END” menu key.

5-6
 MAZATROL FUSION 640MT

T.P.C. DISPLAY cont.

Once the TPC screen has been closed. You will notice a symbol has appeared next
to the unit number. This symbol (a white cross in a blue square) indicates that the
TPC data has been edited.

5-7
 MAZATROL FUSION 640MT

5-8
 MAZATROL FUSION 640MT

PARAMETERS (TURNING)

6-1
 MAZATROL FUSION 640MT

6-2
 MAZATROL FUSION 640MT

PARAMETERS (SELECTED)

6-3
 MAZATROL FUSION 640MT

6-4
 MAZATROL FUSION 640MT
PARAMETER
Parameters are constants and various data required for setting machine and NC
equipment operation modes required for machining.
When machines are delivered, parameters are set at factory. Some of them can be
changed by the user.
If wrong values are set as parameter, operation of machines and NC equipment may be
hampered. For changing parameters, their meaning and functions must be well
understood.
This parameter list shows important parameters for the user. Those which the user
hardly need change settings and those not used are omitted from the list. The meaning
and functions of parameters are described only important points. If functions of
parameters to be changed are not clearly understood, contact our service centers.

How to Use Parameter List

The parameters are listed in a form as shown below.
Title of display (1)

Address Meaning Description

(3)

(2)
(7)

Unit (4)
Effective
condition
(5)
Applicable
program
(6)

(1): Title of display showing required parameter

(2): Address (nomenclature) of required parameter
- Bit input type parameters have the bit No. shown in the parentheses below
address.
Example:
Setting value for parameter
P1 (bit 0) is indicated here
Address

P1 P1
(bit 0) Bit 0
Bit 1
Bit 2
Bit 3
Bit 4
Bit 5
Bit 6
Bit 7

6-5
 MAZATROL FUSION 640MT

(3): Meaning of required parameter

(4): Setting unit for parameter
(5): Conditions on which set value is effective
Example 1: “Instant” designates that new parameter value becomes effective
upon parameter change.
Example 2: “Power OFF/ON” designates that new parameter value will become
effective after procedure below.
[1] Change parameter setting value.
× (By procedure similar to changing of ordinary data)
[2] Press power off button on the operation panel.
×
[3] Press power on button on the operation panel.

Example 3: In the parameter list, “I/O start” means that the system operates at the
parameter data entered before the start of I/O. If the parameter data
is modified during I/O operation, the new data will not become valid
until the I/O operation has been completed.
(6): Applicable program
M....................Effective only for MAZATROL programs
E ....................Effective for EIA/ISO programs
M, E ...............Effective for MAZATROL programs and EIA/ISO programs
(7): Description of required parameter
Relevant parameters are indicated in the parentheses at bottom.

Precautions
1. The type and setting value for required parameters may vary according to machine
types, use/disuse of optional equipment and manufacturing time.
Values set for specific machines and NC equipment must not be used for other
machines and NC equipment.
2. The factory set parameters are recorded on separate paper and stored inside the
control cabinet. This paper must not be lost.
3. If parameter-setting values are changed, values before and after the change must
be recorded for storage.
4. If machines are not operated for a long time, battery backup may be lost and data
will be destroyed (battery alarm indicated). In this case, confirm parameter-setting
values by referring to the parameter record paper. If machines are operated with
data lost, error will be caused.

6-6
 MAZATROL FUSION 640MT

Title of display PARAMETER (USER, CUTTING)

P2 (bit 2) = 0
The tool change position is not reached.
Selection of whether the return to the tool
change position is to be executed upon P2 (bit 2) = 1
issuance of T-command with the same The tool change position is reached.
P2
TNo. but followed different suffix.
(bit 2) This parameter is effective only for tools with suffix H or V of the V/H
turret specifications.

Unit 
Effective
Instant
condition
Applicable
M
program
P2 (bit 4) = 0
A13 is not added

Selection of whether the position of fixed P2 (bit 4) = 1

point is to be shifted by an amount of A13 is added.
P2 A13
(bit 4)

Unit 
Effective
Instant
condition
Applicable
M
program
Select whether the position of fixed point is to be shifted in the direction
of the B-axis by an amount of machine parameter A13 (Amount of
Selection of whether the position of the shifting of the B-axis movement origin from machine home position
fixed point is to be shifted in the direction reference).
of the B-axis by an amount of parameter
P2 P2 (bit 5) = 0
A13
(bit 5) Then the position of the fixed point is shifted without machine parameter
A13 being added.

P2 (bit 5) = 1
Unit 
Then the position of the fixed point is shifted by an amount of machine
Effective
Instant parameter A13
condition
Applicable
M
program
An angle margin for nose shape compensation can be selected by
setting data in bits 6 and 7.

Selecting an angle margin for nose Setting Angle margin for nose
P2 shape compensation Bit 7 Bit 6 shape compensation
(bit 6) 0 0 3.0

(bit 7) 0 1 2.0
1 0 1.0
Unit  1 1 0.5
Effective
Instant
condition
Applicable
M
program

6-7
 MAZATROL FUSION 640MT
Title of display PARAMETER (USER, CUTTING)
Selection of tool change position Specify tool change position from 1 through 8 below.
specification code
A5 Z-axis
A5
6 1 3 X-axis

Machine
origin point 4

0
5 2
Lx

βx
Lz

Zc : Stock material edge projection length

Dmax : Stock material maximum outside diameter
7
βx : Tool turning clearance (X-axis) U1/2
D max Workpiece
βz : Tool turning clearance (Z-axis) U2
8 Lx : Length of the longest tool in X direction
Lz : Length of the longest tool in Z direction
Program
origin point

Setting X-axis Z-axis

NM211-00215 Zc βz
0 Clearance position Clearance position
1 Machine origin point Clearance position
2 Clearance position Machine origin point
3 Machine origin point Machine origin point
4 Fixed point Fixed point
P17
5 Clearance position End point of previous machining
6 Machine origin point End point of previous machining
7 End point of previous machining Clearance position
8 End point of previous machining Machine origin point

Note:
P17=5 or 6, Z-axis tool change position is identical with the end point of
previous machining. In the case below, however, this may not be
applied.
As shown here, if the longest tool comes into the hatched portion, the
position will escape in Z-axis direction by the distance determined by U2.

U2

Stock material
edge protrusion length
Stock material length NM211-00216

Unit 
Effective
Instant (ÕU1, U2, A5)
condition
Applicable
M
program

6-8
 MAZATROL FUSION 640MT
Title of display PARAMETER (USER, CUTTING)
Select spare tool indexing conditions below.

Setting Description
Indexing of spare tool when number of machined
1
workpieces has reached limit
Indexing of spare tool when tool use time has reached
2
limit
Indexing of spare tool when tool wear amount X has
4
exceeded limit
Indexing of spare tool when tool wear amount Z has
8
exceeded limit
Selection of spare tool indexing condition Indexing of spare tool when tool wear amount Y has
16
exceed limit
P18
To combine the several conditions listed above, set the sum total of
setting numbers corresponding the conditions to be selected.

Example:
To combine the workpiece machining quantity and tool wear amount X,
set 5 (1 + 4).

Unit 
Effective
Instant
condition
Applicable
M, E
program
Specify input data unit system.
P19 = 0
Data input in mm
Minimum command unit 0.001 mm

P19 = 1
Data input in inch
Minimum command unit 0.0001 inches

Note:
Selection of unit system between When this parameter is changed, data below must also be changed.
mm/inch - In parameter, unit must be recorded for mm and inch.
- Cutting condition data
P19
Mere change of P19 will not convert automatically above data.

Unit 
Effective Power
condition OFF → ON
Applicable
M, E
program

6-9
 MAZATROL FUSION 640MT
Title of display PARAMETER (USER, CUTTING)
Tool will stop at groove bottom while spindle rotates N times when P24 is
set to N (N=0  

Dwell (specification of spindle rotation

number) at groove bottom in groove
cutting unit (GRV)
P24

Unit Revolutions
Effective Remaining at groove bottom until
Instant NM211-00218
condition the spindle rotates N times.
Applicable
M
program
This parameter will be used to select escape pattern (0, 1 or 2) when
wall is vertical in G71/G72 mode.
P26 = 0 ......... Identical with ordinary path
Selection of escape pattern from wall P26 = 1 ......... Escape at 45° from wall
(90°) in rough cutting cycle
P26 = 2 ......... Feedrate accelerated at wall
P26 Accelerated feedrate F is expressed as follows.
K3
F = Fo × 100
Unit 
(where F0=Feedrate specified in program)
Effective
Instant
condition
Applicable
E
program (ÕK3)
This parameter automatically determines milling axis gear. Output M
code will be as shown below if P27 is set to n.

Specification of first M code for milling Gear 1st step 2nd step 3rd step 4th step
axis gear selection M code n n+1 n+2 n+3
P27

Unit 
Effective
Instant
condition
Applicable
M
program
This parameter automatically determines spindle gear.
Output M code will be as shown below if P28 is set to n.

Specification of first M code for spindle Gear 1st step 2nd step 3rd step 4th step
gear selection
M code n n+1 n+2 n+3
P28

Unit 
Effective
Instant
condition
Applicable
M
program

6-10
 MAZATROL FUSION 640MT
Title of display PARAMETER (USER, CUTTING)
It is a parameter to automatically control the parts catcher.
If the set value of P29 is set to n, M code of No. n (parts catcher forward)
is outputted at the start of cutting off (GRV #4, #5), and M code of No.
n+1 (Parts catcher backward) is outputted at the end.
Specification of first M code for parts
catcher control
P29

Unit 
Effective
Instant
condition
Applicable
M
program
Set chamfering angle at thread portion in thread cutting cycle (G76/G92)

P30
Threading chamfering angle

P30

Chamfering data NM211-00219

Unit Degree
Note:
Effective
Instant Set 45 or 60.
condition
Applicable
E
program
Simultaneous operation pattern for transfer of workpieces between two
unit jobsites

P31 = 1
Simultaneous operation pattern for Rotation of the spindle and movement of the Z-axis
transfer P31 = 2
P31 Orientation of the spindle and movement of the Z-axis

P31 = 4
Positioning of the C-axis and movement of the Z-axis simultaneously
Unit  occur.
Effective Note:
Instant
condition To combine patterns, set the sum total of setting numbers corresponding
Applicable the conditions.
M
program

6-11
 MAZATROL FUSION 640MT

Title of display PARAMETER (USER, CUTTING)

Address Meaning Description

Tool turning clearance is required to prevent interference between the

tool and stock material during tool change in automatic operation.
U2

Chuck
U1/2

Stock material shape

Dmax l0
Tool turning clearance (diametral value)
in X-axis

U1

Dmax: Stock material maximum outside diameter

l 0: Stock material edge projection length

0.001 mm or
Unit
0.0001 inches
Effective
Instant
condition
Applicable
M
program

Tool turning clearance (diametral value)

in Z-axis

U2

0.001 mm or
Unit
0.0001 inches
Effective
Instant
condition
Applicable
M
program

6-12
 MAZATROL FUSION 640MT
Title of display PARAMETER (USER, CUTTING)
Safety contour clearance is provided for outside of the stock material
shape specified by common data in program.
Safety contour clearance Tool approach and escape paths for each unit will be automatically
determined according to set data (outside diameter, inside diameter,
- Outside diameter clearance
front clearance, back clearance) for parameters from U3 to U6.
(diametral value)
U3 U6 l U5

Safety contour
0.001 mm or U3/2
Unit
0.0001 inches
Dmin
Effective Stock material shape
Instant
condition
U4/2
Applicable
M
program
Dmax
l0
Safety contour clearance
- Inside diameter clearance (diametral
value)
U4 Dmax: Stock material maximum outside diameter
Dmin: Stock material minimum inside diameter
l 0: Stock material edge projection length
0.001 mm or
Unit l: Stock material length
0.0001 inches
Effective
Instant
condition
Applicable
M
program

Safety contour clearance

- Front clearance

U5

0.001 mm or
Unit
0.0001 inches
Effective
Instant
condition
Applicable
M
program

Safety contour clearance

- Back clearance

U6

0.001 mm or
Unit
0.0001 inches
Effective
Instant
condition
Applicable
M
program

6-13
 MAZATROL FUSION 640MT
Title of display PARAMETER (USER, CUTTING)
Thread cutting clearance is provided to specify tool return distance for
each cycle in thread cutting unit (THR).
Thread cutting clearance will be added to the highest portion of thread
and repeating path will be determined automatically.

<OUT>

U7

Programmed shape

Thread cutting
acceleration distance
NM211-00222

<IN>

Programmed shape Thread cutting

acceleration distance

U7
Thread cutting clearance (radial value)
NM211-00223
U7
<FCE>

Programmed U7
shape

Thread cutting
acceleration
distance NM211-00224

<BAK>
Thread cutting
acceleration distance

U7

0.001 mm or
Unit
0.0001 inches Programmed shape
Effective
Instant NM211-00225
condition
Applicable
M
program

6-14
 MAZATROL FUSION 640MT
Title of display PARAMETER (USER, CUTTING)
Groove cutting clearance is provided at machining start portion in groove
cutting unit (GRV).
<OUT>
Tool path Outside diameter
clearance U3/2

U8/2
Groove cutting clearance (diametral
value) in X-axis

U8 NM211-00226

<IN>

Front
clearance U5
Tool path

U8/2
0.001 mm or
Unit
0.0001 inches
Effective NM211-00227
Instant
condition
Applicable <FCE>
M
program Tool path Outside diameter
clearance U3/2

Front
Groove cutting clearance (diametral clearance U5 NM211-00228
U9
value) in Z-axis
<BAK>
U9
Outside diameter
Tool path clearance U3/2

0.001 mm or
Unit
0.0001 inches Back clearance
U6 U9
Effective NM211-00229
Instant
condition
Applicable
M
program

6-15
 MAZATROL FUSION 640MT
Title of display PARAMETER (USER, CUTTING)
Milling line right/left cutting clearance is provided to specify tool approach
point and escape point in milling line right and left cutting unit (LFT,
RGT).

Mill line
right cutting
End point Start point

Mill line
left cutting
Milling line right/left cutting clearance
U10 U10
U10

NM211-00230

0.001 mm or
Unit
0.0001 inches
Effective
Instant
condition
Applicable
M
program
Workpiece transfer clearance is provided to specify workpiece transfer
position in workpiece transfer unit (TRS).
Example:
Workpiece transferred from No. 1 spindle head to No. 2 spindle head.

No. 1 No. 2
Workpiece
spindle head spindle head

Workpiece transfer clearance

U11 U11

Workpiece transfer position specified

in TRANSFER display
NM211-00231

No. 2 spindle head traverse by rapid feedrate from transfer position to

position distant by clearance distance U11, and then transfer operation
initiated.

0.001 mm or
Unit
0.0001 inches
Effective
Instant
condition
Applicable
program
M Õ
( U26, U27, U50)

6-16
 MAZATROL FUSION 640MT
Title of display PARAMETER (USER, CUTTING)
After EDG unit roughing, this parameter works instead of safety contour
clearance FCE parameter U5. If, however, U12 is zero, then U5 is used.

Amount of edge clearance after EDG

roughing

U12

0.001 mm or
Unit
0.0001 inches
Effective
Instant
condition
Applicable
M
program
Inside diameter enlarging cycle
U35 U35

NM211-00241

Cutting is promoted gradually from the edge,

and machining chip removal efficient.

Cut depth per cycle for machining inside

diameter in bar machining unit (BAR) cf. Standard inside diameter cutting

U35
Cutting to specified depth once
through, and machining chip
removal not efficient

NM211-00242

0.001 mm or
Unit
0.0001 inches
Effective
Instant
condition
Applicable
M
program

6-17
 MAZATROL FUSION 640MT
Title of display PARAMETER (USER, CUTTING)
Example:
Outside diameter machining in normal (– Z-axis direction)

Reverse feed tolerance for contour dr Reverse feed contour

machining data
Contour
U36

0.001 mm or
Unit dr
0.0001 inches NM211-00243
Effective
Instant dr ≤ U36 No alarm
condition
dr > U36 Alarm
Applicable
M
program

PS PE U37

PE PS
U37
Overtravelling in X-axis direction in edge PS: Start point
machining unit (EDG) PE: End point
NM211-00244
U37

Note:
By setting an adequate value for U37, uncut residue will not be produced
in edge machining.
Uncut residue because of
Tool nose R. etc.

0.001 mm or
Unit
0.0001 inches
Effective NM211-00245
Instant
condition
Applicable
M
program

6-18
 MAZATROL FUSION 640MT

Title of display PARAMETER (USER, CUTTING)

U38
L L0

Program start Thread cutting

point start point
Acceleration distance clamp value for
thread cutting unit (THR) NM211-00246
U38
L : Effective thread length
Lo: Acceleration distance

If L0>U38, alarm will be caused.

If, however, P1 (bit 3)=0, alarm will not be caused.

Unit Lead/10
Effective
Instant
condition
Applicable Õ
( P1 (Bit 3))
M
program

Cut depth (diametral value) for final cut in

thread cutting unit (THR)
Cut depth (diametral value) for final cut in 1st cut
composite type thread cutting cycle G76
U39
(n/2-1)th cut
0.001 mm or (n/2)th cut
Unit
0.0001 inches
U39/2 nth cut
Effective
Instant
condition NM211-00247
Applicable
M, E
program

Tool

Pecking return distance in groove cutting

unit (GRV)

U41

0.001 mm or
Unit
0.0001 inches U41
Effective
Instant
condition
Applicable NM211-00248
M, E
program

6-19
 MAZATROL FUSION 640MT
Title of display PARAMETER (USER, CUTTING)

d
d: Tool diameter
Overlap distance for machining wide l: Groove width
groove in groove cutting unit (GRV) Tool

U42

0.001 mm or
Unit
0.0001 inches U42
Effective
Instant
condition
Applicable NM211-00249
M l
program
<Rough cutting> <Finish cutting>

U43 U43
Escape value after machining in edge
machining unit (EDG)

U43

0.001 mm or
Unit
0.0001 inches
Effective
Instant
condition
U43 U43
Applicable NM211-00250
M
program
Maximum spindle speed during cutting off cycle (GRV #4, #5) is set.

Spindle revolution clamp value in cutting

off cycle (GRV)
U54

Unit min  (rpm)

Effective
Instant
condition
Applicable
M
program

6-20
 MAZATROL FUSION 640MT

Title of display PARAMETER (USER, CUTTING)

During finishing that uses #0 (standard pattern) of a threading unit,
finishing is executed the number of times that has been set in parameter
U55 with the depth of U39/U55.

U55 = 0 or 1
Then the finishing is executed one time with the depth of U39.

U55 ≥ 2
The finishing is repeated the number of times determined by U55 with
the depth of U39/U55.
Number of times of finishing when #0
(standard pattern) is selected in Notes:
threading unit 1. Parameter U55 is valid only for #0 or [#0]. It is not valid for #1,[#1],
U55 #2 or[#2].
2. Parameter U55 is not valid if U39 = 0.
3. The refinishing of threading is executed once as before.

Unit Times
Effective
Instant
condition
Applicable
M
program
The staring feed value for cutting-off is a feed value that has been
designated in unit data, and the ending feed value for cutting-off is a feed
value that has been designated in sequence data. The feedrate from the
start of machining to the end is reduced in steps according to the number
of times that has been designated here.
Example:
Feedrate set at “R-FEED” item in unit data = 0.5
Feedrate set at “ROUGH” item in sequence data = 0.1
U56: 3
Number of times that the feedrate is to be Feedrate : 0.5
U56 reduced during the #4 and #5 cutting-off
cycles of a grooving unit

Feedrate : 0.3

Workpiece Workpiece

Feedrate : 0.1

6-21
 MAZATROL FUSION 640MT

Title of display PARAMETER (USER, CUTTING)

Set the height of the second referential
point during the Torando cycle. Cutting feed
Rapid feed
With chamfering (i0 ≠ 0)

Initial point
Referential point Approach point
Second referential point
U3 Approach from a
position distant through
Surface to be U83
cut
(Face
machining:
U5) Amount of Pitch 1
chamfering

Height of the second referential point Pitch 2

during the Tornado cycle

U83

Without chamfering (i0 = 0)

Initial point
Referential point
Approach point
Second referential point
U3 Approach from a
position distant through
Surface to be cut U83
(Face machining: U5)

DEPTH DEPTH

0.001 mm or Pitch 2
Unit
0.0001 inches
Effective
Instant MEP322
condition
Applicable
M
program

6-22
 MAZATROL FUSION 640MT

Title of display PARAMETER (USER, CUTTING)

F1 : Feedrate for rough cutting

F3
F3 : Reduced feedrate
F1
Deceleration rate in down-going wall
slope (90°) for rough cutting in bar
machining unit (BAR) NM211-00265
K5
F3 = F1 × K5
100

Unit % Notes:
Effective 1. This is effective only when P1 (bit 1)=1.
Instant 2. Up to 500 % can be set.
condition
Applicable
M
program

Stock material shape

F2
Acceleration rate on outside stock
contour for rough cutting in copy F1 F1 : Feedrate inside stock
contour
machining unit (CPY)
K6 F2 : Feedrate outside stock
contour
K6
F 2 = F1 ×
100
NM211-00266
Unit %
Effective Note:
Instant
condition Up to 500 % can be set.
Applicable
M
program
Used to calculate acceleration distance in thread cutting unit
K7 K7
L = L0 – ln ( 1000 ) – 1 + 1000
Acceleration pitch error ratio in thread L : Acceleration distance
cutting unit (THR) L0 : Distance over which feedrate become constant
K7
Note:
Up to 2 % can be set.
Unit 0.1%
Effective
Instant
condition
Applicable
M
program
PS
PS : Programmed start point
PE : Programmed end point
l l : Groove machining depth
Rough cutting residue ratio in cutting off
d
l = PS PE
cycle (#4, #5) in groove cutting unit
d : Rough cutting residue
(GRV) K8
K8 PE
d = l × 100

NM211-00267

➀ Cutting at rough cutting feedrate to a point short of end PE by

Unit % distanced d
Effective ➁ Cutting off at finish cutting feedrate to end point PE
Instant
condition
Note:
Applicable Up to 100 % can be set.
M
program

6-23
 MAZATROL FUSION 640MT
Title of display PARAMETER (USER, CUTTING)
F1

P2 P1
Reamer return speed calculation
coefficient
K18
F2 NM211-00271

K18 F1 : Specified feedrate

F2 = F1 × 100 F2 : Return speed
Unit %
P1 : Start point
Effective P2 : End point
Instant
condition Note:
Applicable Up to 999 % can be set.
M
program

L2 L1 L

End
point
Start
point

NM211-00272

Chamfering data calculation coefficient in L : Effective thread length

thread cutting unit (THR) L1 : Same pitch incomplete thread length (copy delay)
K19 L2 : Chamfering data
ψ : Chamfering angle

K19
L2 = L0 × 10
L0 : Thread lead

Note:
Up to 40 can be set.
Unit Lead/10
Effective
Instant
condition
Applicable
M, E
program
K20
l=P× Programmed Programmed
10 end point start point
P : Tapping pitch
Incomplete threading portion length l : Incomplete thread
Tap
portion length
calculation coefficient for tap tip
K20 l

Cutting end point specified

Unit Pitch/10 farther by this length l NM211-00273

Effective Note:
Instant
condition
Up to 99 can be set.
Applicable
M
program

6-24
 MAZATROL FUSION 640MT
Title of display PARAMETER (USER, CUTTING)
K21
l=P× Normal state
10 Tap
P : Tapping pitch
l : Tapper elongation Pressed state
Tapper elongation calculation coefficient Tap during cutting, etc.

K21
l
NM211-00274

Unit Pitch/10 Note:

Effective Up to 99 can be set.
Instant
condition
Applicable
M
program
Ratio of axial feedrate to diametral feedrate is set.
K22 or K23
(Axial feedrate) = (Diametral feedrate) × 100
Calculation coefficient for axial feedrate Tool
of rough cutting in milling line machining
unit (MGV, LCT, RGT, LFT)
K22

Axial feedrate
Unit %
Workpiece
Effective Diametral feedrate
Instant
condition
Applicable
M NM211-00275
program
K22 for rough cutting
K23 for finish cutting

Calculation coefficient for axial feedrate

of finish cutting in milling line machining Note:
unit (MGV, LCT, RGT, LFT) Up to 999 % can be set.
K23

Unit %
Effective
Instant
condition
Applicable
M
program
K24
h = P × 10000
h : Thread height
Thread height calculation coefficient for
P : Thread pitch
outside diameter, face/rear thread cutting
(metric)
K24

Unit 0.01%
Effective
Instant
condition
Applicable
M
program

6-25
 MAZATROL FUSION 640MT
Title of display PARAMETER (USER, CUTTING)
Refer to K24.

Thread height calculation coefficient for

inside diameter thread cutting (metric)
K25

Unit 0.01%
Effective
Instant
condition
Applicable
M
program
Refer to K24.

Thread height calculation coefficient for

outside diameter, face/rear thread cutting
(inch)
K26

Unit 0.01%
Effective
Instant
condition
Applicable
M
program
Refer to K24.

Thread height calculation coefficient for

inside diameter thread cutting (inch)
K27

Unit 0.01%
Effective
Instant
condition
Applicable
M
program

6-26
 MAZATROL FUSION 640MT

Title of display PARAMETER (USER, CUTTING)

P
Polishing margin width for #1 to #3
K34

K33 K33 NM211-00277

<#1>

0.001 mm or
Unit K34
0.0001 inches
Effective
Instant
condition
Applicable
M K33
program
P
NM211-00278
<#2>

Polishing margin depth #1 to #3

K34
K33 P
0.001 mm or K34
Unit
0.0001 inches
Effective K34 K33
Instant NM211-00279
condition
P: Program end point
Applicable <#3>
M
program
<#4>

Polishing margin width for #4

P

K35 K36

0.001 mm or
Unit K35
0.0001 inches NM211-00280
Effective
Instant
condition P: Program end point
Applicable
M
program

Polishing margin depth for #4

K36

0.001 mm or
Unit
0.0001 inches
Effective
Instant
condition
Applicable
M
program

6-27
 MAZATROL FUSION 640MT
Title of display PARAMETER (USER, CUTTING)
<#5>

Polishing margin width for #5 K38

K37

0.001 mm or
Unit
0.0001 inches
Effective K37
Instant P
condition
Applicable
M
program NM211-00278

P: Program end point

Polishing margin depth for #5

K38

0.001 mm or
Unit
0.0001 inches
Effective
Instant
condition
Applicable
M
program
<#6>

Polishing margin width for #6

K39 K39 P
K40
0.001 mm or
Unit
0.0001 inches
NM211-00279
Effective K40 K39
Instant
condition
Applicable P: Program end point
M
program

Polishing margin depth for #6

K40

0.001 mm or
Unit
0.0001 inches
Effective
Instant
condition
Applicable
M
program

6-28
 MAZATROL FUSION 640MT
Title of display PARAMETER (USER, CUTTING)
Address Meaning Description

(1) X-axis (diametral value), Z-axis

Specifying fixed point position.
Coordinates are determined on the machine coordinate system
based on the origin points as reference.

A5 (Z-axis)

Machine
origin point
A5 (X-axis)/2

Fixed
point

NM211-00302

(2) C-axis
Specifying fixed point position
Fixed point return position or second Coordinates are based on the deviation angle from the C-axis
reference point return position machine origin point.
A5

Fixed point

(+) direction

A5 (C-axis) C-axis machine

origin point
(–) direction

NM211-00303

0.001 mm (0.0001 inches)

Unit
or 0.001 deg
Effective
Instant
condition
Applicable
M, E
program

6-29
 MAZATROL FUSION 640MT
Title of display PARAMETER (USER, CUTTING)
Setting tool tip measurement tool change position on the machine
coordinate system

Tool tip measurement tool change

position or third reference point return
position in X-axis (diametral value), Z-
A6 (X-axis)/2 Machine
axis Setting tool tip measurement tool origin point
change position on the machine
A6 coordinate system A6 (Z-axis)

Tool change
position
0.001 mm or
Unit
0.0001 inches NM211-00304
Effective
Instant
condition
Applicable
M, E
program
Setting workpiece origin point position with respect to machine origin
point on the machine coordinate system

Workpiece origin
point
A7 (Z-axis) (Fi d i t)
Workpiece origin (fixed point) coordinate
or fourth reference point return position

A7 A7 (X-axis)

Machine
origin point
NM211-00305

0.001 mm or
Unit (This parameter determines workpiece origin point upon power on. This
0.0001 inches
Effective can be changed by G50 command.)
Instant
condition
Applicable
E
program
Setting reference workpiece origin point position with respect to machine
origin point

Machine
A8 (Z-axis) origin point

Machine reference position

A8

A8 (X-axis)/2

0.001 mm or
Unit
0.0001 inches Reference workpiece
Effective origin point NM211-00306
Instant
condition
Applicable
M, E
program

6-30
 MAZATROL FUSION 640MT
Title of display PARAMETER (USER, CUTTING)
Setting of chuck outside diameter of No. 1 spindle head

Chuck outside diameter of No. 1 spindle

head (for chuck barrier)
B33
B33
0.001 mm or
Unit
0.0001 inches
Effective Power
NM211-00312
condition OFF → ON
Applicable
M, E
program
Setting of chuck width of No. 1 spindle head

B34
Chuck width of No. 1 spindle head (for
chuck barrier)
B34

0.001 mm or
Unit
0.0001 inches
Effective Power
condition OFF → ON
NM211-00313
Applicable
M, E
program
Setting of chuck inside diameter of No. 1 spindle head

Chuck inside diameter of No. 1 spindle

head (for chuck barrier)

B35
B35

0.001 mm or
Unit
0.0001 inches
Effective Power NM211-00314
condition OFF → ON
Applicable
M, E
program

6-31
 MAZATROL FUSION 640MT

Title of display PARAMETER (USER, CUTTING)

Setting of tail body outside diameter

Tail body outside diameter (for tail

barrier)
B37
B37

0.001 mm or
Unit
0.0001 inches NM211-00315
Effective Power
condition OFF → ON
Applicable
M, E
program
Setting of tail body length
B38

Tail body length (for tail barrier)

B38

0.001 mm or
Unit
0.0001 inches
NM211-00316
Effective Power
condition OFF → ON
Applicable
M, E
program
Setting of tail spindle outside diameter

Tail spindle outside diameter

(for tail barrier)
B39
B39

0.001 mm or
Unit
0.0001 inches NM211-00317
Effective Power
condition OFF → ON
Applicable
M, E
program
Setting of length with tail spindle at back end

B40
Length with tail spindle at back end
(for tail barrier)

B40

0.001 mm or
Unit
0.0001 inches NM211-00318
Effective Power
condition OFF → ON
Applicable
M, E
program

6-32
 MAZATROL FUSION 640MT
Title of display PARAMETER (USER, CUTTING)
Setting of tail head outside diameter

Tail head outside diameter

(for tail barrier)
B41
B41

0.001 mm or
Unit
0.0001 inches NM211-00319
Effective Power
condition OFF → ON
Applicable
M, E
program
Setting of tail head length

B42
Tail head length
(for tail barrier)

B42

0.001 mm or
Unit
0.0001 inches NM211-00320
Effective Power
condition OFF → ON
Applicable
M, E
program
Setting of tail head taper angle

Tail head taper angle B43

(for tail barrier)
B43

NM211-00321
Unit 0.001 deg
Effective Power
condition OFF → ON
Applicable
M, E
program
Setting of biting diameter when tail head is used

Tail head biting diameter

(for tail barrier)
B44
B44

Workpiece origin point

0.001 mm or
Unit
0.0001 inches NM211-00322
Effective Power
condition OFF → ON
Applicable
M, E
program

6-33
 MAZATROL FUSION 640MT
Title of display PARAMETER (USER, CUTTING)
Setting of tool holder mounting position. When plus data is used, the tool
Tool holder mounting position holder is mounted horizontally, and minus data downward.

B49 - Type 1 Example: Type 1

B49 B52 - Type 2
B52 B55 - Type 3
B58 - Type 4
B55
B49 ( > 0)
B58
0.001 mm or
Unit
0.0001 inches
Effective
Instant
condition B49 ( < 0) NM211-00327
Applicable
M Same for types 2, 3, 4
program
Setting tool holder width in X-axis direction
Tool holder width in X-axis direction Example: Type 1
B50 - Type 1
B50 B53 - Type 2
B53 B56 - Type 3
B59 - Type 4
B56 B50 (where B49 > 0)
B50 (where B49 < 0)
B59
0.001 mm or
Unit
0.0001 inches
Effective
Instant NM211-00328
condition
Applicable Same for types 2, 3, 4
M
program
Setting of tool holder width in Z-axis direction

Tool holder width in Z-axis direction Example: Type 1

B51 - Type 1
B51 B54 - Type 2
B54 B57 - Type 3
B60 - Type 4
B57
B60
0.001 mm or
Unit
0.0001 inches
Effective B51 (where B49 > 0) B51 (where B49 < 0)
Instant
condition
NM211-00329
Applicable
M Same for types 2, 3, 4
program

6-34
 MAZATROL FUSION 640MT

PARAMETERS (MILLING)

6-35
 MAZATROL FUSION 640MT

6-36
 MAZATROL FUSION 640MT
Title of display PARAMETER (USER, POINT)

Address Meaning Description

Height of the second R-point

Initial point

D1
Second R-point

MPL001

Height of the second referential point The heigt of the referential point during point machining is basically U3 to
during point machining U6, however, it is changed to D1 under the following conditions.
D1
Tool sequence Conditions
- Bit 6 of parameter D91 is set to 1 (D1 valid).
Drill - There is a spot drill in the pre-machining tool
sequence of the same unit.
- Bit 2 of parameter D92 is set to 1 (D1 valid).
Reamer - There is a chamfering cutter in the pre-
machining tool sequence of the same unit.

However, when a drills is included in the pre-machining tool sequence in

0.001 mm or
Unit case of a drilling tool sequence, the height is changed to D42. (Refer to
0.0001 inches
D42.)
Effective
Instant
condition
Applicable
M
program
The nominal diameter of a spot-machining tool that is automatically set
during automatic tool development.
Example:

Nominal diameter of spot-machining tool SNo. TOOL NOM HOLE-φ HOLE-DEP

1 CTR-DR 20. 10.
D2
D2

Unit 1 mm or 0.1 inches

Effective
Instant
condition
Applicable
M
program
Axis feed dwell time at the hole bottom in a spot-machining cycle. Set
this time in spindle revolutions.
When the spot-machining tool reaches
Spot-machining hole bottom dwell time the hole bottom, the Z-axis will firstly
element stop moving until the spindle makes D3
D3 revolutions, and then refurn to the
original position at the rapid feedrate.

Unit Revolution
Effective
Instant
condition (Stops at hole bottom.)
Applicable
M MPL002
program

6-37
 MAZATROL FUSION 640MT
Title of display PARAMETER (USER, POINT)

Address Meaning Description

Element used to set the maximum spot-chamfering hole diameter (d)
during automatic tool development
Spot-chamfering occurs if
D2 d ≤ D2 – D4.
Maximum allowable spot-chamfering hole
diameter element d If d > D2 – D4, the chamfering
D4 cutter is developed automatically.

Unit 0.1 mm or 0.01 inches Chamfering

Effective
Instant
condition
Applicable
M MPL003
program
The feedrate of a tool as it is being passed through the prehole during an
inversed spot-facing cycle
Note: 0.5 mm/rev if this parameter setting is 0.
Prehole through speed during inversed
spot-facing
D5

At the feedrate of D5
Unit 1 mm or 0.1 inches
Effective
Instant
condition MPL004
Applicable
M
program
Element used to automatically set drill-machining cycles during
automatic tool development

Machining cycle Conditions

Drill-machining cycle setting element
DEPTH
D6 Drilling cycle
DIA ≤ D6

High-speed deep-hole DEPTH

Unit — drilling cycle D6 < DIA ≤ D7
Effective DEPTH
Instant Deep-hole drilling cycle
condition DIA
D7 <
Applicable
M
program

Drill-machining cycle setting element

D7

Unit —
Effective
Instant
condition
Applicable
M
program

6-38
 MAZATROL FUSION 640MT
Title of display PARAMETER (USER, POINT)

Address Meaning Description

Element used to automatically set the number of drills which are
automatically developed according to the hole diameter of the drill unit

Maximum diameter of holes machinable Number of drills

Conditions
developed
on one drill
D8 1 DIA ≤ D8
2 D8 < DIA ≤ D9
3 D9 < DIA ≤ D10
Unit 1 mm or 0.1 inches Alarm D10 < DIA
Effective
Instant
condition
Applicable
M
program

Maximum diameter of holes machinable

on two drills
D9

Unit 1 mm or 0.1 inches

Effective
Instant
condition
Applicable
M
program

Maximum diameter of holes machinable

on three drills
D10

Unit 1 mm or 0.1 inches

Effective
Instant
condition
Applicable
M
program
Element used to automatically set the hole-drilling, endmilling, and
boring depths during automatic tool development of inversed spot-facing,
tapping, back-boring, through-hole drilling, through-hole counter-boring,
and spot-faced tapping units
Through-hole/tap-prehole machining
overshoot
D11 DEPTH DEPTH
D11
D11 MPL005

Unit 0.1 mm or 0.01 inches Example:

Effective SNo. TOOL NOM No. HOLE-φ HOLE-DEP
Instant 21. ← (DEPTH + D11)
condition 1 DRILL 10. 10.
Applicable Note: See also parameter K20 for tapping units.
M
program

6-39
 MAZATROL FUSION 640MT
Title of display PARAMETER (USER, POINT)

Address Meaning Description

Element used to automatically set the hole-drilling depth during
automatic tool development of stop-hole counter-boring and stop-hole
boring units

Stop-hole machining hole-bottom DEPTH

clearance
D12 MPL006
D12
Example:
SNo. TOOL NOM No. HOLE-φ HOLE-DEP
1 DRILL 10. 10. 19.
Unit 0.1 mm or 0.01 inches
Effective (DEPTH – tool tip compensation – D12)
Instant
condition
Note:
Applicable This parameter is invalid when the residual hole diameter is not 0.
M
program
Hole diameter is automatically set during automatic tool development
when spot-chamfering is not to be performed.
D13
Spot-machining hole diameter
(fixed value)
D13
MPL007

Unit 1 mm or 0.1 inches Example:

Effective SNo. TOOL NOM No. HOLE-φ HOLE-DEP
Instant
condition 10.
1 CTR-DR 20.
Applicable D13
M
program
Element used to automatically set the depth-of-cut per drilling operation
during automatic tool development
HOLE-φ × D14 : when the material of the stock workpiece is AL
Depth-of-cut setting element for drilling (aluminum) in article MAT. 6
(ALMINUM)
HOLE-φ × D15 : when the material of the stock workpiece is other than
D14 AL in article MAT. 6

Unit 0.1
Effective
Instant
condition
Applicable
M
program

Depth-of-cut setting element for drilling

(except AL)
D15

Unit 0.1
Effective
Instant
condition
Applicable
M
program

6-40
 MAZATROL FUSION 640MT
Title of display PARAMETER (USER, POINT)

Address Meaning Description

Z-axis feed dwell time at the hole bottom in a chamfering cutter
machining cycle. Set this time in spindle revolutions.
When the chamfering cutter reaches the
Hole-bottom dwell time for chamfering hole bottom, the axis will firstly stop
cutter moving until the spindle makes D16
D16 revolutions, and then return to the
original position at the rapid feedrate.
Note:
This parameter is invalid for chamfering
Unit Revolution
with true-circle processing.
Effective
Instant
condition (Stops at hole bottom.)
Applicable MPL008
M
program
The clearance in order to prevent tool interference with a wall of the
workpiece or with the hole bottom during a chamfering cycle
D17
Interference clearance of chamfering
cutter

D17
Interferes.
0.01 mm or
Unit
0.0001 inches
Effective
Instant
condition
D17
Applicable MPL009
M Interferes.
program
The feedrate at which the tool is returned from the hole bottom during
reaming or boring.

Return feedrate for reaming or boring D18

(cycle 3)
D18
MPL010
Notes:
1. Valid only when the setting of ZFD for the reamer (tool sequence) is
Unit 1 mm/min or 0.1 inch/min G01.
Effective 2. Valid only when the setting of PRE-DIA for the boring tool (tool
Instant sequence) is CYCLE 3.
condition
3. If this parameter is 0, the tool is returned at the same feedrate as
Applicable
M that of cutting.
program
Axis feed dwell time at the hole bottom in an end milling cycle. Set this
time in spindle revolutions.

When the end mill reaches the hole

Hole-bottom dwell time for end milling bottom, the axis will firstly stop
moving until the spindle makes D19
D19 revolutions, and then return to the
original position at the rapid feedrate.

Unit Revolution Note:

Effective This parameter is invalid for true-circle
Instant
condition processing.
Applicable (Stops at hole bottom.)
M MPL011
program

6-41
 MAZATROL FUSION 640MT
Title of display PARAMETER (USER, POINT)

Address Meaning Description

Element used to automatically set the radial depth-of-cut per end milling
operation
Depth-of-cut = nominal diameter × D20
Radial depth-of-cut setting element for Depth-of-cut is automatically set according to the value of this parameter
end milling when nominal diameter of the end mill is input.
D20 Example:
SNo. TOOL NOM HOLE-φ HOLE-DEP PRE-DIA PRE-DEP RGH DEPTH
1 E-MILL 20. 40. 10. 30. 0. 12.
Unit % (NOM × D20)
Effective
Instant
condition
Applicable
M
program
The reference value for calculation of a bottom-finishing allowance which
corresponds to the roughness level of the end milling (tool sequence).
The finishing allowance in the case of roughness level 4 becomes the
Reference bottom-finishing allowance for value of this parameter, and the values for all other roughness levels are
end milling set using the expressions listed in the table below.

D21 Roughness Bottom-finishing allowance

0 to 3 0.0
4 D21
0.001 mm or 5 D21×0.7
Unit
0.0001 inches 6 D21×0.7×0.7
Effective 7 D21×0.7×0.7×0.7
Instant
condition 8 D21×0.7×0.7×0.7×0.7
Applicable 9 D21×0.7×0.7×0.7×0.7×0.7
M
program
Dwell time at the hole bottom or at the referential point. This value is
valid when 1 is set for bit 0, 1 or 2 of parameter D91.

Tapping-cycle dwell time

D22

Unit 0.01 sec

Effective Note:
Instant This parameter is valid only when the setting for roughness of tapping
condition
Applicable (tool sequence) is FIX.
M
program
Axis feed dwell time at the hole bottom in a boring cycle. Set this time in
spindle revolutions.
When the boring bar reaches the hole
bottom, the axis will firstly stop moving
Hole-bottom dwell time for boring
until the spindle makes D24 revolutions,
D24 and then the spindle orientation will be
performed.
Note:
Unit Revolution This parameter is invalid if the roughness
Effective of the boring (tool sequence) is 0.
Instant
condition
Applicable (Stops at hole bottom.) MPL013
M
program

6-42
 MAZATROL FUSION 640MT
Title of display PARAMETER (USER, POINT)

Address Meaning Description

The distance which the boring or back-boring tool is returned at the
same feedrate as for cutting after the tool has reached the hole bottom

Boring or back-boring hole-bottom return

D26
D26
MPL015
0.001 mm or Has reached the Returned at the Returned at a
Unit
0.0001 inches hole bottom. same feedrate. rapid feedrate.
Effective
Instant
condition Note:
Applicable Not valid if the setting for the roughness of the boring (tool sequence) is 1.
M
program
The distance which the boring bar is fed in at 70% of the original
feedrate to finish the hole bottom

Bottom-finishing amount of boring

D28
D28
MPL016
0.001 mm or
Unit The feedrate is reduced to 70% of the original value before the hole
0.0001 inches
bottom is reached.
Effective
Instant Note:
condition
Applicable Not valid if the setting for the roughness of the boring (tool sequence) is 1.
M
program
The number of inertial turns in tapping cycle that the spindle has rotated
clockwise during the time from output of a spindle CCW rotation
command to the start of spindle CCW rotation
Number of spindle revolutions until
spindle CCW rotation begins in tapping
cycle
D32

Unit Revolution
Effective
Instant
condition
Applicable
M
program
The amount of relief provided for a back-boring tool tip to be kept clear of
the prehole walls as it is being passed through the prehole in the
oriented state of the spindle
Back-boring tool tip relief D33

D33

0.001 mm or
Unit MPL019
0.0001 inches During back-boring During passage
Effective
Instant
condition
Applicable
M
program

6-43
 MAZATROL FUSION 640MT
Title of display PARAMETER (USER, POINT)

Address Meaning Description

Element used to automatically set the prehole-drilling diameter during
automatic tool development of the reamer unit (When the pre-machining
unit is drilling.)
DIA

Prehole-drilling diameter setting element

for reamer (drilling) DIA – D35

D35
MPL020

Example:

0.01 mm or SNo. TOOL NOM HOLE-

Unit 10. ← D35
0.001 inches 1 DRILL 10.
Effective
Instant
condition
Applicable
M
program
used to automatically set the prehole-drilling diameter during automatic
tool development of the reamer unit (When the pre-machining unit is
boring.)
DIA

Prehole-drilling diameter setting element

for reamer (boring) DIA – D36

D36
MPL020

Example:

0.01 mm or SNo. TOOL NOM HOLE-φ

Unit 10. ← D36
0.001 inches 1 DRILL 10.
Effective
Instant
condition
Applicable
M
program
Element used to automatically set the prehole-drilling diameter during
automatic tool development of the reamer unit (When the pre-machining
unit is end milling.)
DIA

Prehole-drilling diameter setting element

for reamer (end milling) DIA – D37

D37
MPL020

Example:

0.01 mm or SNo. TOOL NOM HOLE-φ

Unit 10. ← D37
0.001 inches 1 DRILL 10.
Effective
Instant
condition
Applicable
M
program

6-44
 MAZATROL FUSION 640MT
Title of display PARAMETER (USER, POINT)

Address Meaning Description

1) In automatic tool development of the reamer unit, if the pre-
machining unit is boring:
DIA
Reamer-prehole diameter setting
element for boring or end milling

D38 Boring-hole diameter

= DIA – D38

0.01 mm or
Unit MPL021
0.001 inches
Effective Example:
Instant
condition SNo. TOOL NOM HOLE-φ
1 BOR BAR 10. 10. ← (DIA – D38)
Applicable
M
program
2) In automatic tool development of the reamer unit, if the pre-
machining unit is end milling:
DIA

Reamer-prehole diameter setting

First end milling hole diameter
element for end milling
= DIA – D39
D39 Second end milling hole diameter
= DIA – D38
MPL022
0.01 mm or
Unit
0.001 inches Example:
Effective SNo. TOOL NOM HOLE-φ
Instant
condition 20. ← (DIA – D39)
1 E-MILL 15.
Applicable 21. ← (DIA – D38)
M 1 E-MILL 10.
program
Axis feed dwell time at the spot-faced hole bottom in an inversed spot
facing cycle. Set this time in spindle revolutions.
When the inversed spot-facing tool
Spot-faced hole bottom dwell time for reaches the hole bottom, firstly the
inversed spot-facing axis will stop moving until the
D40 spindle makes D40 revolutions, and
then the rotational direction of the
spindle will reverse.
(Feeding stops at
Unit Revolution hole bottom.)
MPL023
Effective
Instant
condition
Applicable
M
program

6-45
 MAZATROL FUSION 640MT
Title of display PARAMETER (USER, POINT)

Address Meaning Description

Height of the third referential point

Initial point

D42
Third referential point

MPL001

Height of the third referential point during

point machining The height of the referential point during point machining is basically U3
to U6, however, it is changed to D42 under the following conditions.
D42
Tool sequence Conditions
- Bit 6 of parameter D91 is set to 1 (D42 valid).
Drill - There is a spot drill in the pre-machining tool
sequence of the same unit.
Chamfering - Bit 7 of parameter D91 is set to 1 (D42 valid).
cutter - CYCLE 2 is selected for the machining cycle.

0.001 mm or
Unit
0.0001 inches
Effective
Instant
condition
Applicable
M
program
To set number of incomplete threads in tapping cycle for piped screws
(PT, PF, PS). In tapping, internal thread is tapped extra for the depth of
(D43 pitch/10).
This is also used as an element for automatically determining hole-
drilling depth in the automatic tool development of the tapping unit.

DEPTH

Number of incomplete threads in tapping

D43 × Pitch/10
cycle
D43 D11
MPL07

Example:
SNo. TOOL NOM HOLE-φ HOLE-DEP
1 DRILL 10. 10. 19.

DEPTH + D11 + (D43 × pitch/10)

Unit Pitch/10
Effective
Instant
condition
Applicable
M
program

6-46
 MAZATROL FUSION 640MT
Title of display PARAMETER (USER, POINT)

Address Meaning Description

This parameter specifies a method of automatic calculation of the
amount of chamfering using the tapping unit.
Amount of (MAJOR-φ + 2 PITCH) – PRE-DIA
Automatic calculation method for the chamfering 2
amount of chamfering using the tapping 0: =
unit Amount of MAJOR-φ – PRE-DIA
D44 chamfering 2
1: =

Note:
Unit —
Select 1 if the loss of the threaded section by chamfering is likely.
Effective
Instant
condition
Applicable
M
program
Set the amount of mill-drilling depth attenuation.
D
dn di d1
Cut
depth

End Start
d1 point
point

d2 n-th cycle i-th cycle 1st cycle

di
Amount of mill-drilling depth attenuation

D45 b
dn

1 2 i n Number of cutting in
NM211-00251

D : Drilling depth
d1 : Cut depth in 1st cycle
di : Cut depth in i-th cycle
0.001 mm or di : d1 – D45 × (i – 1) (di E
Unit
0.0001 inches di : b (di < b)
Effective b :Drilling depth clamping value (D46)
Instant
condition
Applicable
program
M Õ
( D46)

Set the minimum drilling depth.

Mill-drilling depth clamping value

D46

0.001 mm or
Unit
0.0001 inches
Effective
Instant
condition
Applicable
M
Õ
( D45)
program

6-47
 MAZATROL FUSION 640MT
Title of display PARAMETER (USER, POINT)

Address Meaning Description

Element used to automatically set the hole depth of drilling, end milling
and boring during automatic tool development of the reamer unit

Reamer-prehole machining overshoot

DEPTH DEPTH

D47
D47 D47

0.01 mm or For drilling For end milling or boring MPL025

Unit
0.001 inches
Example:
Effective
Instant SNo. TOOL NOM HOLE-φ HOLE-DEP
condition
1 DRILL 10. 10. 21. ← (DEPTH + D47)
Applicable
M
program
Specify DEP-A range for the end mill and the face mill from the learning
data of cutting conditions.
When learning data on the condition that DEP-A is in the following range
has been stored in the memory, learning is not effectuated again.
For a DEP-A range of the end mill, set a value of DEPTH/NOM (at a
unit of 0.1%) .
0 to D73 ..................DEP-A range (for end mill) 1
D73 to D74 .............DEP-A range (for end mill) 2
D74 to D75 .............DEP-A range (for end mill) 3
For a DEP-A range of the face mill, set a value of DEPTH (at a unit of
Learning of cutting conditions 0.1 mm or 0.01 inch) .
D73 (DEP-A range)
0 to D76 DEP-A range (for face mill) 1
to D76 to D77 DEP-A range (for face mill) 2
D77

Unit —
Effective
Instant
condition
Applicable
M
program

6-48
 MAZATROL FUSION 640MT
Title of display PARAMETER (USER, POINT)

Address Meaning Description

Specify WID-R range for the boring bar, back boring bar and end mill
from the learning data of cutting conditions.
When learning data on the condition that WID-R is in the following range
has been stored in the memory, learning is not effectuated again.
For a WID-R range of the boring bar and back boring bar, set a value of
DEPTH (at a unit of 0.1 mm/0.01 inch) .
0 to D78 .................. WID-R range (for boring bar and back boring bar) 1
D78 to D79 ............. WID-R range (for boring bar and back boring bar) 2
For a WID-R range of the end mill, set a value of DEPTH/NOM (at a
unit of 0.1%) .
Learning of cutting conditions
D78 0 to D80 .................. WID-R range (for end mill) 1
(WID-R range)
D80 to D81 ............. WID-R range (for end mill) 2
to
D81 to D82 ............. WID-R range (for end mill) 3
D82

Unit —
Effective
Instant
condition
Applicable
M
program

76543210 (1: Execution, 0: No execution)

M04 is output after the tool has dwelled at the

hole bottom during a tapping cycle.
The tool dwells after M04 has been output at the
hole bottom during a tapping cycle.
The tool dwells after it has been returned to the
referential point during a tapping cycle.
The finishing tool path is shortened during a
true-circle processing cycle (end milling).
— The tool path is shortened during a true-circle
processing cycle (chamfering).
D91
If a spot drill/drill is included in the pre-machining
tool sequence of the same unit, the referential
point height of the drill is set as D1 or D42.
The referential point height of the chamfering
cutter during the cycle 2 is set as D42.

Unit —
Effective
Instant
condition
Applicable
M
program

6-49
 MAZATROL FUSION 640MT
Title of display PARAMETER (USER, POINT)

Address Meaning Description

76543210 (1: Execution, 0: No execution)

During a true-circle processing (end milling)

cycle, K41 is used for axial feed.
The referential point 1 height of the back spot
facing is set as D1.
If a chamfering cutter is included in the pre-
machining tool sequence of the same unit, the
referential point height of the reamer is set as
D1.
— If a chamfering cutter is included in the pre-
machining tool sequence of the same unit, the
D92 referential point height of the tapping is set as
D1.
Minimum point machining at the C-axis position
Invalid (0), valid (1)

Unit —
Effective
Instant
condition
Applicable
M
program

6-50
 MAZATROL FUSION 640MT
Title of display PARAMETER (USER, LINE)

Address Meaning Description

Element used to set cutting start point and escape point for closed-
pattern line- or face-machining
Example:
Closed-pattern cutting start point and Defined closed
Defined closed pattern
escape point setting element pattern
E1 SRV-R

E2 E2
0.001 mm or
Unit
0.0001 inches E1 Cutting Escape E1
Effective start point point MPL026
Instant
condition [Applicable units]
Applicable - LINE OUT, LINE IN, CHMF OUT and CHMF IN
M
program - Wall finishing of POCKET
The reference value of each finishing allowance R (FIN-R) which is
automatically set when the roughness levels of the line- or face-
machining units have been set
The finishing allowance R in the case of roughness level 4 becomes the
Reference allowance of finishing in radial value of this parameter, and the values for all other roughness levels are
direction calculated using the expressions listed in the table below.
E4 Roughness FIN-R
0 to 3 0.0
4 E4
0.001 mm or 5 E4×0.7
Unit
0.0001 inches 6 E4×0.7×0.7
Effective 7 E4×0.7×0.7×0.7
Instant 8 E4×0.7×0.7×0.7×0.7
condition
Applicable 9 E4×0.7×0.7×0.7×0.7×0.7
M
program
Element used to set the cutting start point and escape point (the second
clearance)
U10 is used generally as a clearance on the plane, however, E5 is used
when the condition meets both of 1) and 2) mentioned below.
1) There is pre-machining in the same unit.
2) The parameter (E92, E95) that makes E5 effective is set to ON (1).
[Applicable units]
LINE OUT, LINE IN, POCKET
[Related parameters]
Element used to set the cutting start point
and escape point (the second clearance) E92 bit 3
Parameter that effectuates E5 in the applicable unit.
E95 bit 7
E5

0.001 mm or
Unit
0.0001 inches
Effective
Instant
condition
Applicable
M
program

6-51
 MAZATROL FUSION 640MT
Title of display PARAMETER (USER, LINE)

Address Meaning Description

The reference value of each finishing allowance which is automatically
set when the roughness levels of the line- or face-machining units have
been set
The finishing allowance in the case of roughness level 4 becomes the
Reference allowance of finishing in axial value of this parameter, and the values for all other roughness levels are
direction calculated using the expressions listed in the table below.
E6 Roughness FIN-A
0 to 3 0.0
4 E6
5 E6×0.7
0.001 mm or
Unit 6 E6×0.7×0.7
0.0001 inches
7 E6×0.7×0.7×0.7
Effective
Instant 8 E6×0.7×0.7×0.7×0.7
condition
9 E6×0.7×0.7×0.7×0.7×0.7
Applicable
M
program
Allowance of cutting start point in axial direction
For the line- or face-machining, U3 to U6 is used as an axial clearance
for rapid access to the machining point from the initial point, however, E7
is used when the condition meets both of 1) and 2) mentioned below.
1) There is pre-machining in the same unit.
2) The parameter (E92, E95, E96 and E97) that makes E7 effective is set
to ON (1).
[Applicable units]
All line-/face-machining units except the face milling face unit.
Allowance of cutting start point in axial
[Related parameters]
direction (the second clearance)
E92 bit 2
E7 E95 bit 6 Parameter that effectuates E7 in the applicable unit.
E96 bit 1
E97 bit 2

0.001 mm or
Unit
0.0001 inches
Effective
Instant
condition
Applicable
M
program
The amount of clearance that prevents interference of the chamfering
cutter with the hole walls during face-machining
E8
Radial interference clearance of
chamfering cutter

E8
Interferes.
0.001 mm or
Unit
0.0001 inches
Effective
Instant Interference distance MPL028
condition
Applicable
M
program

6-52
 MAZATROL FUSION 640MT
Title of display PARAMETER (USER, LINE)

Address Meaning Description

Element used to automatically set the radial depth-of-cut of the tool
sequence in FACE MIL or TOP EMIL unit
NOM × E10
Depth-of-cut-R automatic setting element WID-R = 10
(Face milling, End milling-top)
Example:
E10
SNo. TOOL NOM APRCH-1 APRCH-2 TYPE AFD DEP-A WID-R
R1 F-MILL 100A ? ? XBI 1. 19.

Unit 10% NOM × E10

Effective 10
Instant
condition
Applicable
M
program
The amount of clearance that prevents interference of the chamfering
cutter with the hole bottom during chamfering

Axial interference clearance of

chamfering cutter

E11
E11

0.001 mm or
Unit Interference depth
0.0001 inches Interferes. MPL030
Effective
Instant
condition
Applicable
M
program
The amount of clearance that prevents interference between the tool and
the figure during face milling
Example:
Radial interference clearance of face
Escape point Defined figure
milling unit

E12

0.001 mm or
Unit
0.0001 inches
Cutting
Effective start point
Instant E12 E12
condition MPL031
Applicable
M
program
Element used to set the tool path internal to the figure for end milling-top
unit
Example:
Tool path setting element for end milling-
top unit
E13 Tool diameter × E13
10

Tool diameter × E13

Unit 10% 10
Effective Defined figure MPL032
Instant
condition
Applicable
M
program

6-53
 MAZATROL FUSION 640MT
Title of display PARAMETER (USER, LINE)

Address Meaning Description

Element used to automatically set the radial depth-of-cut of the tool
sequence in POCKET unit
NOM E14
Depth-of-cut-R automatic setting element WID-R = 10
(Pocket milling)
Example:
E14
SNo. TOOL NOM APRCH-1 APRCH-2 TYPE AFD DEP-A WID-R
R1 E-MILL 20. ? ? CW G01 10. 12.

Unit 10% NOM× E14

Effective 10
Instant
condition
Applicable
M
program
Element used to set the tool path external to the defined figure for
reciprocating-short machining with face milling unit
Example:
Tool path setting element for face milling-
top unit (reciprocating short) Tool diameter × E15
10
E15

Unit 10%
Tool diameter × E15
Effective 10
Instant
condition Defined figure MPL033
Applicable
M
program
Denote the feed override value for axial movement to the intended plane
during the use of a line- or plane-machining unit, except for face-milling.
Notes:
1. This parameter is valid only when tool sequence AFD is G01.
2. Feed override is invalid if this parameter is “0”.

Example:

Feed in the E17

tool sequence ×
Axial cutting feed override 10
E9 SRV-Z
E17 Face to be
machined
MPL035

Unit 10%
Effective
Instant
condition
Applicable
M
program

6-54
 MAZATROL FUSION 640MT
Title of display PARAMETER (USER, LINE)

Address Meaning Description

Override value of feedrate when the pocket-machining radial depth-of-
cut becomes equal to the tool diameter
Example:
Override in case of the overall width FR × E18
cutting for pocket-machining 10
E18

MPL036
Unit 10% Note:
Effective Overriding for overall width cutting is not valid when this parameter is 0.
Instant
condition
[Applicable units]
Applicable
M Rough-machining of POCKET
program
Denote the depth of overlapping between the starting and ending
positions of wall cutting in a closed line- or plane-machining pattern.
Example:
Defined closed pattern

Escape point Cutting start

E21 point MPL037
Overlapping depth during wall cutting in a
closed pattern [Applicable units]
E21 - LINE OUT, LINE INE, CHMF OUT and CHMF IN
- Wall finishing of E-MIL and SLOT.

0.001 mm or
Unit
0.0001 inch
Effective
Instant
condition
Applicable
M
program

6-55
 MAZATROL FUSION 640MT
Title of display PARAMETER (USER, LINE)

Address Meaning Description

76543210
0: Machining from inside to outside
1: Machining from outside to inside
0: The referential point height is set always as
U3 to U6.
1: The referential point height is set as E7 or U3
to U6 when there is or isn’t pre-machining in
the same unit, respectively.
0: The clearance in plane direction is set always
as U10.
1: The clearance in plane direction is set as E5
Tool-path pattern selection for pocket
or U10 when there is or isn’t pre-machining in
milling unit
the same unit, respectively.
E92
1: Rapid feed up to the intended surface + U3 to
U6

Unit —
Effective
Instant
condition
Applicable
M
program

6-56
 MAZATROL FUSION 640MT
Title of display PARAMETER (USER, LINE)

Address Meaning Description

76543210
For the 2nd and subsequent rounds of cutting:
0: Not via the approach point
1: Via the approach point
For the 2nd and subsequent rounds of cutting:
0: Escape to the axis initial point
1: No escape on the axis
1: Rapid feed up to the intended surface + U3 to
U6
1: Escape is set to a point where the tool comes
out of the removal allowance.
The referential point height for central, right hand,
left hand, outside and inside linear machining is:
0: Set always as U3 to U6
1: Set as E7 or U3 to U6 when there is or isn’t pre-
machining in the same unit, respectively.
The plane direction clearance for outside and inside
linear machining is:
0: Set always as U10
1: Set as E5 or U10 when there is or isn’t pre-
machining in the same unit, respectively.
- Bit 2
Bit 2 = 1 Bit 2 = 0

Initial point
Tool-path pattern selection for line-
machining unit
E95
1st removal allowance
2nd removal allowance

Approach point Cutting start point MPL501

- Bit 3
Approach point Escape point

Bit 3 = 0
Initial point

1st removal allowance

Bit 3 = 1 2nd removal allowance

MPL502

- Bit 5
Bit 5 = 0 Bit 5 = 1
U10

Unit —
Escape point U10
Effective WID-R
Instant MPL503
condition
Applicable Note:
M
program Bit 3 valid only for inside/outside linear machining unit.

6-57
 MAZATROL FUSION 640MT
Title of display PARAMETER (USER, LINE)

Address Meaning Description

76543210
0: The referential point height is set always as
U3 to U6.
Tool-path pattern selection for end 1: The referential point height is set as E7 or U3
milling-slot unit to U6 when there is or isn’t pre-machining in
the same unit, respectively.
E96
For the 2nd and subsequent rounds of cutting:
0: Not via the approach point
1: Via the approach point
Unit — 1: Rapid feed up to the intended surface + U3 to
Effective U6
Instant
condition
Applicable
M
program

6543210
0: The referential point height is set always as
U3 to U6
Tool-path pattern selection for end 1: The referential point height is set as E7 or U3
milling-top unit to U6 when there is or isn’t pre-machining in
E97 the same unit, respectively.
1: Rapid feed up to the intended surface + U3 to
U6

Unit —
Effective
Instant
condition
Applicable
M
program

76543210

This bit specifies the returning position for each

cutting operation during face-machining.
Tool path selection
0: Clearance point
E104 1: Initial point

Unit —
Effective
Instant
condition
Applicable
M
program

6-58
 MAZATROL FUSION 640MT

PROGRAMMING
EXAMPLE NO.3

7-1
MAZATROL FUSION 640MT

7-2
 TITLE: PROGRAM EXAMPLE 3

60 Chamfer 1mm x 45° unless otherwise stated

Face Thread 0.5mm Pitch

10
35°

10
6
42
50

7-3
160
120
°
16
R5

6
Drill 13.5 dia x 25 deep
Tap 5/8-11 UNC x 20 deep

40 SURFACE FINISH TO BE 1.6um ALL OVER

MATERIAL SIZE: DRAWN BY: CHECKED BY:

160 O/D x 65mm LONG DRAWING NUMBER:
MATERIAL: ALUMINIUM
MAZATROL FUSION 640MT
 MAZATROL FUSION 640MT

Tooling Sheet - Program 3

GNL OUT GNL OUT

(R.TURN) (F.TURN)
TOOL HOLDER TOOL HOLDER
TYPE 2 TYPE 2

95° 80° (LH TOOL SHOWN) 93° 55° (RH TOOL SHOWN)

10 GRV EDG
THD EDG
(FACE GROOVE)
(FACE SCROLL)
TOOL HOLDER
TOOL HOLDER
3.5 TYPE 1
TYPE 1
(RH TOOL SHOWN)
(RH TOOL SHOWN)

TOOL DIA TOOL DIA

CUT ANGLE

DRL
TAP
(DRILL)
(TAP)
TOOL HOLDER
TOOL HOLDER
TYPE 1
TYPE 1

7-4
 MAZATROL FUSION 640MT

EXAMPLE 3 –Program1 (BAR FCE)

PNo. MAT OD-MAX ID-MIN LENGTH RPM FIN-X FIN-Z WORK FACE
0 AL 160. 0. 65. 3000 0.4 0.1 5.

PNo. MODE # CPT-X CPT-Z RV FV R-FEED R-DEP. R-TOOL F-TOOL

1BAR FCE 0 160. -5. 375 630 0.4 5. GNL OUT A GNL OUT B
SEQ SHP S-CNR SPT-X SPT-Z FPT-X FPT-Z F-CNR/$ RADIUS/ø ROUGH
1LIN * * 120. 20. * Rgh 5
2TPR 120. 20. 91.437 10. 35. Rgh 5
3LIN * * 50. 10. R 5. * Rgh 5
4LIN C 1. * * 0. 0. * Rgh 5

PNo. MODE # CHAMF LEAD ANG MULTI HGT NUMBER V DEPTH TOOL
2THR FCE 2 2 1. 60 1 0.649 * 262 0.234 THD EDG A
SEQ SPT-X SPT-Z FPT-X FPT-Z
1 92. 10. 72. 10.

Pno. MODE # No. PITCH WIDTH FINISH RV FV FEED DEP. R-TOOL F-TOOL
3GRV FCE 1 1 6. 0.1 262 280 0.08 2. GRV EDG A GRV EDG A
SEQ S-CNR SPT-X SPT-Z FPT-X FPT-Z F-CNR ANGLE ROUGH
1 R 0. 42. 0. 40.314 6. Rgh 5

PNo. MODE # DRL-DIA DEP-1 DEP-2 DEP-3 V FEED TOOL

4DRL FCE 1 13.5 13.5 3. 3. 62 0.25 DRL A
SEQ SPT-Z FPT-Z
1 0. 25.

PNo. MODE NOM-DIA PITCH V TOOL

5TAP FCE 5E-11UN 2.3091 10 TAP A
SEQ SPT-Z FPT-Z
1 0. 20.

PNo. MODE COUNTER RETURN WK.No. CONT. NUM. SHIFT

6END 1 0 0 0 0.

7-5
MAZATROL FUSION 640MT

7-6
 MAZATROL FUSION 640MT

PROGRAMMING
EXAMPLE No.3A

7-7
MAZATROL FUSION 640MT

7-8
 TITLE: PROGRAM EXAMPLE 3a - COPY

68.284
CUTTING POINT
40

0
30

R3
15

C2

40
55
60
90

80

120

7-9
20

45
SURFACE FINISH TO BE 1.6um ALL OVER
65
100 DRAWN BY: CHECKED BY:
DRAWING NUMBER:
MATERIAL: CAST IRON
MAZATROL FUSION 640MT
 MAZATROL FUSION 640MT

TOOLING SHEET PROG.3A

GNL OUT GNL OUT

(R.TURN) (F.TURN)
TOOL HOLDER TOOL HOLDER
TYPE 2 TYPE 2

95° 80° (LH TOOL SHOWN) 93° 55° (RH TOOL SHOWN)

7-10
 MAZATROL FUSION 640MT

PROGRAM EXAMPLE No.3A

UNo. MAT OD-MAX ID-MIN LENGTH RPM FIN-X FIN-Z WORK FACE
0ALUMINUM 120. 0. 100. 4000 0.4 0.1 0.

UNo. UNIT
1MTR OUT
SEQ SHP SPT-X SPT-Z FPT-X FPT-Z RADIUS
1TPR 60. 0. 90. 20. *
2LIN * * 90. 45. *
3TPR 90. 45. 120. 65. *

UNo. UNIT # 1 # 2 # 3 # 4 # 5 # 6 # 7 # 8 # 9 #10 #11 #12

2M 8

UNo. UNIT CPT-X CPT-Z SRV-X SRV-Z RV FV R-FEED R-DEP. R-TOOL F-TOOL
3CPY OUT 120. 0. 8. 6. 375 700 0.45 4. GNL OUT B GNL OUT D
SEQ SHP S-CNR SPT-X SPT-Z FPT-X FPT-Z F-CNR/$ RADIUS/ø ROUGH
1TPR 40. 0. 55. 15. Rgh 5
2TPR 55. 15. 80. 30. C 2. Rgh 5
3LIN * * 80. 40. * Rgh 5
4CCV 80. 40. 120. 68.284 30. Rgh 5

PNo. MODE COUNTER RETURN WK.No. CONT. NUM. SHIFT

4END 1 0 0 0 0.

7-11
 MAZATROL FUSION 640MT

7-12
 MAZATROL FUSION 640MT

TOOL SUFFIX CODES

8-1
MAZATROL FUSION 640MT

8-2
 MAZATROL FUSION 640MT

Setting Tool Suffix Codes

1. Press F1 function Key
2. Select TOOL DATA
3. Cursor down to selected tool on TOOL LIST
4. Press Menu (',7722/

5. Select INSERT: The control will display a new tool data line into which a
secondary tool description can be entered. (This can be repeated if required).

8-3
 MAZATROL FUSION 640MT

6. Select the attitude for the new tool description, from the menu options as shown
below.

7. Drop the cursor into the Tool Shape window and enter the new tool description.

8-4
 MAZATROL FUSION 640MT

TOOL SUFFIX CODES-EXAMPLE

DRL A

GNL IN A

GNL OUT A

PNo. MAT OD-MAX ID-MIN LENGTH RPM FIN-X FIN-Z WORK FACE
0 SCM 70. 0. 30. 3000 0.4 0.1 0.

PNo. MODE # DRL-DIA DEP-1 DEP-2 DEP-3 V FEED TOOL

1DRL FCE 1 30. 40. 3. 3. 47 0.1 DRL A
SEQ SPT-Z FPT-Z
1 0. 35.

PNo. MODE # CPT-X CPT-Z RV FV R-FEED R-DEP. R-TOOL F-TOOL

2BAR IN 0 30. 0. 375 468 0.4 5.5 GNL IN A GNL IN A
SEQ SHP S-CNR SPT-X SPT-Z FPT-X FPT-Z F-CNR/$ RADIUS/ø ROUGH
1LIN * * 35. 30. * Rgh 4

PNo. MODE # CPT-X CPT-Z RV FV R-FEED R-DEP. R-TOOL F-TOOL

3BAR OUT 0 70. 0. 135 252 0.4 5.5 GNL OUT A GNL OUT A
SEQ SHP S-CNR SPT-X SPT-Z FPT-X FPT-Z F-CNR/$ RADIUS/ø ROUGH
1LIN * * 50. 14. * Rgh 4

PNo. MODE COUNTER RETURN WK.No. CONT. NUM. SHIFT

4END 0 0 0 0 0.

8-5
MAZATROL FUSION 640MT

8-6
 MAZATROL FUSION 640MT

CUTTING CONDITIONS

9-1
 MAZATROL FUSION 640MT

9-2
 MAZATROL FUSION 640MT
CUTTING CONDITIONS (TURNING)
To enter a material into Cutting Conditions:
Press F1 key, select CUTTING COND. from the function key menu.

The screen will now change to display MATERIAL REGIST. To enter a material
description, position the cursor in the window for either WORK MAT or TOOL MAT.
The naming of work or tool materials must not exceed 8 characters.

Once this has been done select C-COND TURNING. You will now enter an area
where values are listed appropriate to a Mazatrol process in respect of velocity,
feedrate and depth of cut. These are the BASE PROCESS FIGURES, which are
affected by Workpiece Material and Tool Material.

9-3
 MAZATROL FUSION 640MT

The values are factory set but can be changed to suit your average material type.

By selecting WORKMAT. PERCENT from the function keys you will access
an area where the base figure is affected by workpiece and tool material. In
this table, percentages are set against materials to reflect the characteristics of
that material, increasing or decreasing dependant on the value set.

9-4
 MAZATROL FUSION 640MT
CUTTING CONDITIONS (MILLING)
To display the cutting conditions data for milling operations, select the C-SP menu as
displayed below.

This table represents a matrix containing relevant surface speed values for each type
of tool.

9-5
 MAZATROL FUSION 640MT
By pressing the Page keys ↑↑ or ↓↓ , the different types of tool can be selected.
To read the matrix, for the DRILL displayed in the picture above, select for example
SUS440 located under the W. -MAT. row, select CARBIDE under the T.-MAT.
column and the surface speed would be 48 (m/min).

A similar display is available for FEEDRATE.

Select the menu FR.

To read the matrix, for the DRILL displayed in the picture above, select for example
SUS440 located under the W. -MAT. row, select CARBIDE under the T.-MAT.
column and the cutting feedrate would be 0.182 (mm/rev).

9-6
 MAZATROL FUSION 640MT

CUTTING CONDITIONS LEARN

Select CUT. COND. LEARN from the Function keys.

There are 2 displays available, TURNING L. (Learn) DATA and MILLING L.
(Learn) DATA.

During machining with the Mazatrol program, when the machining conditions are
modified using VFC, the system will learn and store the modifications in this display.
When creating a new program for automatic setting of cutting conditions, if the data
matches information stored within the CUT COND LEARN library, the control will
return these values in preference to using the conventional cutting condition
calculation method.
A maximum of 112 types of patterns can be registered. If more than 112 types of
patterns are entered, the excess will be erased with the oldest pattern first.

9-7
 MAZATROL FUSION 640MT
Select MILLING L.DATA

It is not possible to edit the data in the specified register. However, it is possible to
erase an entry. Cursor down to the register number no longer required, select the
ERASE menu, then <INPUT>.

9-8
 MAZATROL FUSION 640MT
It is possible without the need to erase the register, to prevent the control from
temporarily using a particular register containing learned data.

Cursor down against the selected register, press the menu → LEARN OFF then
<INPUT>. A key will then be shown against the register number as shown below.
To remove the Lock, cursor down against the selected register, press the menu →
LEARN then <INPUT>.

9-9
 MAZATROL FUSION 640MT

9-10
 MAZATROL FUSION 640MT

PROGRAMMING
EXAMPLE 4

10-1
 MAZATROL FUSION 640MT

10-2
 TITLE: PROGRAM EXAMPLE 4

GROOVE DETAIL

Radius 0.5

40°
5

Chamfer 0.5mm x 45°

10-3
6
40
48

30
50

50.8
M35 x 2mm Pitch

3 30 Chamfer 2.5mm x 45°

35

60

87 SURFACE FINISH TO
BE 3.2um ALL OVER
MATERIAL SIZE:
50.8 O/D x 1.5 METRE LONG DRAWN BY: CHECKED BY:
DRAWING NUMBER:
MATERIAL: ALUMINIUM
MAZATROL FUSION 640MT
 MAZATROL FUSION 640MT

Tooling Sheet - Program 4

DRL
(BAR STOP)
GNL OUT
TOOL HOLDER
(R.TURN)
TYPE 1
TOOL HOLDER
TYPE 2

93° 55° (LH TOOL SHOWN)

GNL OUT
(BACK TURN)
TOOL HOLDER
TYPE 2

55° 93° (RH TOOL SHOWN) DRL (C'DRILL)

TOOL HOLDER
TYPE 1

GRV OUT
(PART OFF)
GNL OUT THD OUT TOOL HOLDER
(R.TURN) (THREAD) TYPE 2
TOOL HOLDER TOOL HOLDER
TYPE 2 TYPE 2
(RH TOOL SHOWN)
30
93° 55° (RH TOOL SHOWN) (RH TOOL SHOWN)
3.0

10-4
 MAZATROL FUSION 640MT

EXAMPLE 4 Program 1

PNo. MAT OD-MAX ID-MIN LENGTH RPM FIN-X FIN-Z WORK FACE
0 AL 50.8 0. 200. 3000 0.4 0.1 1.

MODE CHANGE-PT GEAR TOOL

1MNP 1 1 DRL EDG A
SEQ G DATA-1 DATA-2 DATA-3 RADIUS/VARIABLE RPM FEEDRATE M OFS
1 00X 0. Z 5. * 5
2 01 Z -89. * MIN 3000. 6
3 04X 1.5 *
4 01 Z 1. * MIN 5000. 7
5 04X 1.5 *
6 00 Z 20. < * 8
7 *

PNo. MODE RV FV R-FEED R-DEP. R-TOOL F-TOOL

2EDG FCE 375 400 0.35 3. GNL OUT A GNL OUT B
SEQ SPT-X SPT-Z FPT-X FPT-Z RGH
1 50.8 1. 0. 0. Rgh 4

PNo. MODE # DRL-DIA DEP-1 DEP-2 DEP-3 V FEED TOOL

3DRL FCE 1 5. 2. 1.5 1. 62 0.05 DRL EDG B
SEQ SPT-Z FPT-Z
1 0. 8.

PNo. MODE CHANGE-PT GEAR TOOL

4MNP 1 1 GNL OUT A
SEQ G DATA-1 DATA-2 DATA-3 RADIUS/VARIABLE RPM FEEDRATE M OFS
1 00 Z 360. * 5
2 * 9
3 * 11
4 04X 2. *
5 01 Z 100. * MIN 2000.
6 * 10
7 04X 2. *
8 * 31

PNo. MODE COUNTER RETURN WK.No. CONT. NUM. SHIFT

5END 1 0 2 1 0 0.

10-5
 MAZATROL FUSION 640MT
EXAMPLE 4 Program 2

PNo. MAT OD-MAX ID-MIN LENGTH RPM FIN-X FIN-Z WORK FACE
0 AL 50.8 0. 100. 3000 0.4 0.1 0.

PNo. MODE # 1 # 2 # 3 # 4 # 5 # 6 # 7 # 8 # 9 #10 #11 #12

1M 8

PNo. MODE # CPT-X CPT-Z RV FV R-FEED R-DEP. R-TOOL F-TOOL

2BAR OUT 0 50.8 0. 375 468 0.4 5.5 GNL OUT A
SEQ SHP S-CNR SPT-X SPT-Z FPT-X FPT-Z F-CNR/$ RADIUS/ø RGH
1LIN C2.5 * * 35. 30. *
2LIN * * 48. 35. *
3LIN * * 40. 60. *

PNo. MODE # CPT-X CPT-Z RV FV R-FEED R-DEP. R-TOOL F-TOOL

3BAR OUT 0 35. 22. 150 252 0.4 1. GNL OUT B
SEQ SHP S-CNR SPT-X SPT-Z FPT-X FPT-Z F-CNR/$ RADIUS/ø RGH
1TPR 35. 22.021 30. 25. R 0.5 -40.
2LIN * * 30. 30. R 0.5 *

PNo. MODE # CPT-X CPT-Z RV FV R-FEED R-DEP. R-TOOL F-TOOL

4BAR OUT 0 50.8 0. 375 468 0.4 5.5 GNL OUT B
SEQ SHP S-CNR SPT-X SPT-Z FPT-X FPT-Z F-CNR/$ RADIUS/ø RGH
1LIN C2.5 * * 35. 22.021 * Rgh 4
2TPR 35. 22.021 30. 25. R 0.5 Rgh 4
3LIN * * 30. 30. R 0.5 * Rgh 4
4LIN * * 48. 35. * Rgh 4
5LIN * * 40. 60. * Rgh 4
6LIN * * 50. 91. * Rgh 4

PNo. MODE # RV FV R-FEED R-DEP. R-TOOL F-TOOL

5CNR OUT 0 260 400 0.3 2.5 GNL OUT C GNL OUT C
SEQ SPT-X SPT-Z FPT-X FPT-Z F-CNR/$ RGH
1 40. 39. 48. 35. Rgh 4

PNo. MODE # CHAMF LEAD ANG MULTI HGT NUMBER V DEPTH TOOL
6THR OUT 0 0 2. 60 1 1.299 8 103 * THR OUT A
SEQ SPT-X SPT-Z FPT-X FPT-Z
1 35. 0. 35. 29.

PNo. MODE CHANGE-PT GEAR TOOL

4MNP 1 1 GNL OUT A
SEQ G DATA-1 DATA-2 DATA-3 RADIUS/VARIABLE RPM FEEDRATE M OFS
1 00 Z 100. * 5
2 * 32
3 * 11
4 04X 2. *
5 01 Z 360. * MIN 2000.
6 * 10
7 04X 2. *

PNo. MODE COUNTER RETURN WK.No. CONT. NUM. SHIFT

7END 1 0 3 1 0 0.

10-6
 MAZATROL FUSION 640MT
EXAMPLE 4 Program 3

PNo. MAT OD-MAX ID-MIN LENGTH RPM FIN-X FIN-Z WORK FACE
0 AL 50. 0. 100. 1500 0.4 0.1 0.

Pno. MODE # No. PITCH WIDTH FINISH RV FV FEED DEP. R-TOOL F-TOOL
1GRV OUT 4 1 * 0. * 348 0.1 2. * GRV OUT A
SEQ S-CNR SPT-X SPT-Z FPT-X FPT-Z F-CNR ANGLE RGH
1 C 0.5 50. 87. 0. 87. *

PNo. MODE COUNTER RETURN WK.No. CONT. NUM. SHIFT

2END 1 0 1 1 0 0.

10-7
 MAZATROL FUSION 640MT

Manual Program Machining Unit (MNP)

The manual program machining unit complements the turning units described so
far (BAR, CPY, CNR, EDG, THR, GRV, DRL and TAP).
These turning units have respective tool paths automatically generated according
to the unit data and sequence data you have set, whereas the manual program
machining unit requires user setting of its tool path.
Select this unit if a machining type or machine action that cannot be programmed in
usual machining units is required, or if it is likely to be more convenient to directly
set a tool path.
Press the MANUAL PROGRAM menu key to select this unit.
Setting unit data

UNo. UNIT CHANGE-PT GEAR TOOL

MNP ① ② ③

① CHANGE-PT
Specify whether you want to return the tool to a predetermined tool change position before executing
the manual program machining unit.
- Set 1 if tool return is required.
- Set 0 if tool return is not required.
Setting 1 in this item returns a turret to predetermined tool change position, that is, the position
previously specified using parameter P17, after the previous unit ends, and then the tool to be used for
the manual program machining unit is indexed at that position.
Setting 0 in this item causes tool change to occur at the end position of the previous machining unit.
Before setting 0, therefore, you must make sure that the tool does not contact the workpiece during
tool change.
Note: The figure below illustrates the tool motion in the transition from an outside or inside turning
unit to the MNP unit.
To avoid the interference on path “A” from the ending position of an inside turning, select
path “B” (return to tool change position) by setting “CHANGE-PT=1” or set an escape route in
the TPC display for the inside turning.

First position of MNP unit

(specified in its sequence data)

B
A Tool change position
Ending A
position
B
CL

B
CL
CL : Safety profile clearance
A : Path after outside/inside turning for MNP
with CHANGE-PT = 0
CL B : Path after outside/inside turning for MNP
with CHANGE-PT = 1
Ending position

10-8
 MAZATROL FUSION 640MT

<In case of setting 1>

Tool change position

Turret swing

U3 End position of the previous

2 machining unit

T4P136

<In case of setting 0>

Tool change position

Turret swing

U3 End position of the previous

2 machining unit

T4P137

Note: See P17 of the Parameter List for tool change position.

② GEAR
Set the number of the spindle gear to be used. Gear shifting will not occur if no data is set in this data
field.
Note 1: A gear is not automatically selected for the manual program machining unit (MNP). Gear
shifting will not occur if no data is set in this data field.
Note 2: Set 1 in this item if the spindle has stepless, automatic transmission capabilities.

10-9
 MAZATROL FUSION 640MT
③TOOL
Select a tool to be used. See the relevant items in “Bar-Materials Machining Unit (BAR)” for tool
selection method. For manual program machining unit, R-TOOL/F-TOOL distinction is not drawn. The
NC regards the tool as R-tool.
If a tool is not designated here, the currently valid tool will be used as it is.

Setting sequence data

UNo. UNIT CHANGE-PT GEAR TOOL

MNP
RADIUS/VARIABL
SEQ G DATA-1 DATA-2 DATA-3 E RPM FEED M OFS
1 ① ② ③ ④ ⑤ ⑥ ⑦ ⑧ ⑨

①G
The following menu will be displayed when the cursor is placed at this item.

G00 G01 G02 G03 G04 G32 G34 SHAPE

END
(a) (b) (c) (d) (e) (f) (g)

From (a) through (g) above, select G-code to be used. The data of the displayed menu denote the
following function.
G00 : Rapid feed positioning
G01 : Linear interpolation
G02 : Clockwise arc interpolation
G03 : Counterclockwise arc interpolation
G04 : Dwell
G32 : Fixed-pitch threading
G34 : Variable-pitch threading

Note: The codes G00, G01, G02, G03, G32 and G34 are modal information information that
remains valid until you have set any other G-code. The code G04 is unmodal information
information that becomes valid only for the sequence data you set.

② DATA-1, ③ DATA-2, ④ DATA-3

The following menu will be displayed when the cursor is placed at either one of these three items:

X Z

- If the G-code you have selected for item ① above is other than G04:
Select an axis from the menu shown above, and then specify the position to which the movement is
to be performed on the axis.
- If the G-code you have selected for item ① above is G04:
After pressing the X menu key, set the desired dwell time in seconds.
For the manual program machining unit, use the following coordinate system to specify the position to
which the cutting edge of the tool is to be moved.

10-10
 MAZATROL FUSION 640MT
<X- and Z-axis>

+X

+Z

Program origin

Either absolute programming or incremental programming must be used to specify the moving
position.
(a) Absolute programming
Directly set the coordinates of the intended moving position in the coordinate system shown in the
diagram above.
(b) Incremental programming
Set an increment or decrement in distance from one moving position to another.
Selection of an axis displays the following menu:

INCRMENT
INPUT

To use this programming method, first press the INCRMENT INPUT menu key to reverse its display
and then set data.
Example: To move the cutting edge of the tool in the following order (P1 → P2 → P3 → …
→ P9 → P1):

Rapid feed
Cutting feed

P1

P9

P7 P6 P5
P8
P4 P3
P2

P1 (300, 50) : Tool change position P6 (80, –105) : End point of a line
P2 (70, 5) : Approach point P7 (80, –135) : End point of a counterclockwise arc
P3 (70, –35) : End point of a line P8 (80, –145) : End point of a line
P4 (70, –70) : End point of a clockwise arc P9 (130, –145) : End point of a line (Return point)
P5 (80, –95) : End point of a taper line

T4P140

10-11
 MAZATROL FUSION 640MT
For absolute programming, set the following data: For incremental programming, set the following data:

UNo. UNIT CHANGE-PT UNo. UNIT CHANGE-PT

MNP 1 MNP 1
SEQ G DATA-1 DATA-2 DATA-3 SEQ G DATA-1 DATA-2 DATA-3
1 00 X 70. Z 5. 1 00 X 70. Z 5.
2 01 X 70. Z -35. 2 01 X 0. < Z -40. <
3 02 X 70. Z -70. 3 02 X 0. < Z -35. <
4 01 X 80. Z -95. 4 01 X 10. < Z -25. < Incremental
5 01 X 80. Z -105. 5 01 X 0. < Z -10. < programming
(*1) (*1) (*2)
6 03 X 80. Z -135. 6 03 X 0. < Z -30. <
7 01 X 80. Z -145. 7 01 X 0. < Z -10. <
8 01 X 130. Z -145. 8 01 X 50. < Z -0. <
(*1) (*1)

*1: Since G01 is modal information, corresponding data can be omitted.

*2: Setting data using the incremental programming method displays the data with a < marking on the
right side.
⑤ RADIUS/VARIABLE
- If you have selected whether G02 or G03 for item ① above:
Set a radius for the desired arc.

G03
End point
RADIUS
Start point End point
RADIUS
Start point
G02

T4P141

- If you have selected G34 for item ① above:

Set the desired increment or decrement in thread pitch per revolution.
- If you have selected other G-code: No data can be set. (A ◆ mark will be displayed.)

⑥ RPM
Set a rotational speed (rpm) or peripheral speed for the spindle.
1) To set a rotational speed: RADIUS/VARIABLE RPM FEED
Set the desired rpm value directly. An S marking S2000
will then be displayed to the left of that value.
Setting data

2) To set a peripheral speed:

RADIUS/VARIABLE RPM FEED
After reversing SURF SPD V display by pressing
V130
its menu key, set the desired value in m/min or
ft/min units. Setting data
A V marking will then be displayed to the left of
that value.

10-12
 MAZATROL FUSION 640MT
Note: The rotational speed or peripheral speed that you have set remains valid until new such value
is set.

⑦ FEED
If G01, G02, G03, G32 or G34 is selected for item above, set the desired feedrates for the X-axis
and Z-axis in either feedrate per revolution (synchronous feed) or feedrate per minute (asynchronous
feed).
1) Setting in feedrate per revolution: RADIUS/VARIABLE RPM FEED
Directly set the feedrate per spindle revolution V130
(mm/rev or inch/rev). REV 0.35
A REV marking will then be displayed to the left
of that value. Setting data

2) Setting in feedrate per minute: RADIUS/VARIABLE RPM FEED

After reversing FEEDRATE/min display by V130 MIN 100
pressing its menu key, set the desired value in
mm/min or inch/min units.
A MIN marking will then be displayed to the left Setting data

of that value.
Note 1: During sequence of G00, the axis movement will be carried out at the rapid feedrate preset in
the specifications. The feedrate you set in this item is valid only for sequences corresponding
to your selection of either G01, G02, G03, G32 or G34.
Note 2: Feedrate preset remains valid until new data is set.
Note 3: If you have selected either G32 or G34 for item ① above, set a lead for the threads.
(Lead) = (Pitch) × (Number of threads)

⑧M
When an M-code (auxiliary function code) is to be used, set the number of that M-code.
The M-code you set in this item becomes valid only for the next and subsequent sequences.
Note: If a feedrate is to be set in mm/rev or inch/rev units for the next sequence, you must first
select either M03 (forward rotation of the spindle) or M04 (reverse rotation of the spindle),
unless the rotational direction of the spindle with respect to the tool to be used has been
specified on the TOOL DATA display.

⑨ OFS
If tool offsetting is to be done using either one of the offset amounts registered on the TOOL OFFSET
display, set the offset number corresponding to the desired offset amount.
During tool offsetting, the offset data specified in this item ⑨ will be added to the WEAR COMP. data
on the TOOL DATA display.
Note: Nose R offsetting cannot be performed for manual program machining.

10-13
 MAZATROL FUSION 640MT

M-Code Unit (M)

Select the M-code unit when M-codes (auxiliary function codes) are to be set.
Up to a maximum of 12 M-codes can be set for one M-code unit.
Press M CODE menu key for this unit.

Setting unit data (M-code)

UNo. UNIT #1 #2 #3 #4 #5 #6 #7 #8 #9 #10 #11 #12

* M ① ① ① ① ① ① ① ① ① ① ① ①

① #1 to #12
Set the desired M-code number in each of the 12 items.
The M-codes you have set are executed in the following order:
#1 #2 #3 #4 #5 #6 #7 #8 #9 #10 #11 #12

1. (Synchronous) 2. (Synchronous) 3. (Synchronous)

If not all of the intended M-codes are to be executed at the same time, therefore, divide them into
three groups (#1 through #4, #5 through #8, and #9 through #12) and then set those M-codes
separately.
Note: For the list of M-codes provided in the NC system, see the M-code list given below.
Of all listed M-codes, those which can be actually selected differ according to the particular
specifications of your machine.
The M-codes M02 (Program End), M98 (Subprogram Call), or other dedicated M-codes for
EIA/ISO program cannot be selected.
All M-codes, including those for software options, are listed in the M-code list.

10-14
 MAZATROL FUSION 640MT
M-code-list
: Option
M-code Function Remarks
M00 Program stop
M01 Optional stop
M02 Program end (Only for EIA/ISO specifications)
M03 Spindle forward rotation
M04 Spindle reverse rotation
M05 Spindle stop
M06 Chuck open
M07 Chuck close
M08 Cutting oil feed
M09 Cutting oil stop (M45 off)
M10 Tailbody connection release/Independent movement of tailstock spindle
M11 Tailbody connection/Simultaneous movement of tailstock spindle
M12 Milling spindle mode cancel (Turning mode selection)
M13 Milling tool normal rotation
M14 Milling tool reverse rotation
M15 Milling tool stop
M16 Orient position 0° (for AJC)
M17 Orient position 120° (for AJC)
M18 Orient position 240° (for AJC)
M19 Spindle orientation position (robot work insertion)
M20 Robot command 1
M21 Robot command 2
M22 Robot command 3
M23 Robot command 4
M24 Robot command 5
M25 Robot command 6
M26 Robot command 7
M27 Robot command 8
M28 Robot command 9
M29 Robot command 10
M30 Reset and rewind (Only for EIA/ISO specifications)
M31 Tailstock spindle and tailbody advance
M32 Tailstock spindle and tailbody retract
M33 Chuck pressure low
M34 Chuck pressure high
M35
M36
M37 Spindle gear change low speed
M38
M39
M40
M41 Spindle gear change low speed
M42

10-15
 MAZATROL FUSION 640MT
: Option
M-code Function Remarks
M43
M44
M45 Air coolant blow ON (coolant stop: M09)
M46
M47
M48 Parts catcher forward
M49 Parts catcher backward
M50
M51 Error detection off
M52 Error detection on
M53 Chamfering off
M54 Chamfering on
M55 Piece count
M56 Front door open
M57 Front door close
M58 Chuck Air blast
M59 Program end preparation announce
M60 C-axis unclamp
M61
M62
M63
M64
M65
M66 C-axis clamp
M67 C-axis brake (G01 machining)
M68 Cycle Bar feeder command 1
M69 Cycle Bar feeder command 2
M70 Ejector drill coolant ON
M71 Ejector drill coolant OFF
M72 Chuck internal clamping
M73 Chuck external clamping
M74 Steady rest – Turret connection mode release
M75 Steady rest – Turret connection mode start
M76 Spindle jaw return to AJC unit (AJC)
M77 Mounting AJC unit jaw to spindle
M78 Steady rest auto unclamp limit switch, valid
M79 Steady rest auto unclamp limit switch, invalid
M80
M81 Workpiece measurement ON
M82 Workpiece measurement OFF
M83 Tool tip measurement ON
M84 Tool tip measurement OFF
M85 Mist Coolant ON (OFF: M09)
M86 Workpiece rest-1 unclamp
M87 Workpiece rest-1 clamp

10-16
 MAZATROL FUSION 640MT
: Option
M-code Function Remarks
M88 Workpiece rest-2 unclamp
M89 Workpiece rest-2 clamp
M90
M91
M92
M93
M94
M95
M96 User macro interruption, valid
M97 User macro interruption, invalid
M98 Subprogram call (Only for EIA/ISO specifications)
M99 Return from subprogram (Only for EIA/ISO specifications)
M100 MES DIA start
M101 MES DIA end
M102 MES STP start
M103 MES STP end
M104 MES GRV start
M105 MES GRV end
M106 MES WID start
M107 MES WID end
M108 MES DIS start
M109 MES DIS end
M110 MES TOL start
M111 MES TOL end
M112 MES EXT start
M113 MES EXT end
M114 MES ZOF start
M115 MES ZOF end
M116 MES COF start
M117 MES COF end
M118
M119
M120 Measurement print out demand
M121
M122
M123
M124
M125
M126
M127
M128
M129
M130

10-17
 MAZATROL FUSION 640MT

: Option
M-code Function Remarks
M131 Chuck pressure selection 1 (minimum pressure)
M132 Chuck pressure selection 2
M133 Chuck pressure selection 3/Steady rest clamp high pressure
M134 Chuck pressure selection 4/Steady rest clamp low pressure
M135 Chuck pressure selection 5
M136 Chuck pressure selection 6
M137 Chuck pressure selection 7
M138 Chuck pressure selection 8
M139 Chuck pressure selection 9
M140 Chuck pressure selection 10
M141
M142
M143
M144
M145
M146
M147
M148
M149
M150 Workpiece unload demand to robot
M151 Milling spindle through air blow ON
M152 Milling spindle through air blow OFF
M153 Milling spindle through coolant ON
M154 Milling spindle through coolant OFF
M155 Chuck coolant ON (composed movement)
M156 Chuck air blow ON (composed movement)
M157 Spindle through coolant blow ON (OFF: M159)
M158 Spindle through air blow ON (OFF: M159)
M159 M157, M158 OFF
M160 Shower coolant ON/chuck stopper extend
M161 Shower coolant OFF/chuck stopper retract
M162 Workpiece rechucking (after delivering robot work)
M163 Tailstock spindle thrust low pressure
M164 Tailstock spindle thrust high pressure
M165
M166
M167 Turret coolant ON
M168 Turret coolant OFF
M169 Magnum coolant ON
M170 Magnum coolant ON
M171 Magnum coolant ON
M172 Index 0° (KOUYOU)
M173 Index 90° (KOUYOU)
M174 Index 180° (KOUYOU)
M175 Index 270° (KOUYOU)

10-18
 MAZATROL FUSION 640MT
: Option
M-code Function Remarks
M176 Index 270° (KOUYOU)
M177 Index 270° (KOUYOU)
M178 Index 270° (KOUYOU)
M179 Index 270° (KOUYOU)
M180
M181 Chuck jaw #1 select
M182 Chuck jaw #2 select
M183 Chuck jaw #3 select
M184 Chuck jaw #4 select
M185 Chuck jaw #5 select
M186 Chuck jaw #6 select
M187 Chuck jaw #7 select
M188 Chuck jaw #8 select
M189 Chuck jaw #9 select
M190 Chuck jaw #10 select
M191 Chuck jaw #11 select
M192 Chuck jaw #12 select
M193 Chuck jaw #13 select
M194 Chuck jaw #14 select
M195 Chuck jaw #15 select
M196
M197
M198 MAZATROL program called from EIA/ISO program and executed (Only for
EIA/ISO specifications)
M199 MAZATROL program called from EIA/ISO program and stop (Only for
EIA/ISO specifications)
M200 Milling point machining start
M201 Milling line machining start
M202 Turning mode
M203 Milling tool normal rotation
M204 Milling tool reverse rotation
M205 Milling tool stop
M206
M207 M208, M209 mode cancel
M208 ATC prohibition mode during finishing, coolant ON
M209 ATC prohibition mode during finishing, coolant OFF
M210 C axis clamp (for milling)
M211 C axis brake (for milling)
M212 C axis unclamp (for milling)
M213 C axis brake only (brake by M211)
M214 C axis unclamp only (unclamp by M211)
M215 M213, M214 and M216 mode cancel
M216 C axis unclamp neglect mode (cancel: M215)
M217
M218
M219 Milling tool orient

10-19
 MAZATROL FUSION 640MT
: Option
M-code Function Remarks
M220

M221
M222
M223
M224
M225
M226
M227
M228
M229
M230 Grinding mode ON
M231 Grinding speed setting
M232
M233 Steady rest 2 clamp low pressure selection
M234 Steady rest 2 clamp high pressure selection
M235
M236 C-axis servo gain normal
M237 C-axis servo gain low
M238 C-axis servo gain middle
M239 C-axis servo gain highl
M240
M241
M242
M243
M244
M245
M246
M247
M248 Spindle speed check (cutting start interlock)
M249 Turret selection preparation
M250 Turret/B-axis clamp
M251 B-axis clamp
M252 Milling spindle unclamp
M253 Milling spindle clamp
M254 Turret/B-axis unclamp
M255
M256
M257
M258 Tool air blow
M259
M260 Polygon mode ON
M261 Polygon mode OFF
M262

10-20
 MAZATROL FUSION 640MT
: Option
M-code Function Remarks
M263
M264
M265

M266
M267
M268
M269
M270
M271
M272
M273
M274 Steady rest coolant ON
M275 Steady rest coolant OFF
M276 Steady rest 1 up
M277 Steady rest 1 down
M278
↓
M329
M330 Stopper 1 in the spidle
M331 Stopper 2 in the spindle
M332 Chip conveyor start
M333 Chip conveyor stop
M334
↓
M347
M348 Yt-axis selection
M349 Y-axis selection
M350
M351 M352 Cancel
M352 Spindle speed arrival signal check cancel
M353
↓
M369
M370 Axis load detection, invalid
M371 Axis load detection, valid
M372 Axis load detection, temporarrily invalid
M373 Axis load detection, restart
M374 NC feed holding on overload detection
M375 NC feed holding & spindle stop on overload detection
M376 Overload detection level % setting
M377 Overload detection time setting (unit: 0.1 sec)
M378 Overload detection peak % / detection frequency setting
M379 Overload detection table No. registration
M380

10-21
 MAZATROL FUSION 640MT
: Option
M-code Function Remarks
↓
M389
M390 M391 Cancel
M391 Spindle mis-chucking cancel (M3/M4 completed with chuck open)
M392
M393 Spindle face driver valid
M394
M395
M396
M397
M398 Turret coolant ON
M399
↓
M589
M590 T code execution during axis movement
M591
M592
M593
M594
M595
M596 M code execution during axis movement
M597
M598
M599
M600 Tool setting for turret
M601 Magazine tool rotation
M602 Stand-by tool setting
M603
↓
M999

10-22
 MAZATROL FUSION 640MT

10-23
 MAZATROL FUSION 640MT
End Unit (END)
Select the end unit after the entire program data required for machining has been set.
For this unit, set data about the machine action to occur at the end of machining and about the
program execution mode. Such data is referred to as end data.
You must set this unit on the last line of a program.
Press END menu key for this unit.

Setting unit data

UNo. UNIT COUNTER RETURN WK. No. CONT. NUM. SHIFT

END

COUNTER
Specify whether you want the NC unit to count the number of machined workpieces (number of
program loops).
- Set 1 if counting is desired.
- Set 0 if counting is not desired.
If you set 1, the number of machined workpieces will be displayed at COUNTER of the POSITION
display.
Note: Counting does not occur if no data has been set in this item.

RETURN
Specify the position to which the tool is to be returned after machining.
- Set 0 to return the tool to the required tool change position.
- Set 1 to return the tool to the machine home position.
- Set 2 to return the tool to the required fixed point.
Note 1: The required tool change position refers to the position preset in parameter P17. The
required fixed point refers to the position preset in parameter A5. (See separate Parameter
List for further details.)
Note 2: For program loops, the tool return position at the end of machining cycles other than the last
one differs according to the particular data setting in bit 7 of parameter P1. (See separate
Parameter List for further details.)
Note 3: If no data has been set in this item, the NC will interpret that 0 has been set.

WK. No.
If the starting part of a different program is to be called up after machining, set the work number of that
program.
Note: If no data has been set in this item, the starting part of the current program will be called up
automatically after machining.
CONT.
Specify whether you want to carry out the machining operation repeatedly in succession.
- Set 1 to execute the current program perpetually or to execute a different program following
completion of the current program.
- Set 0 to execute the current program once or to repeatedly execute the current program the number
of times that is to be specified in item below.

10-24
 MAZATROL FUSION 640MT
Note: If no data has been set in this item, the NC will interpret that 0 has been set.

NUM.
If the current program is to be executed repeatedly, set the desired number of times of execution.

SHIFT
Shifting the origin of the current program and repeatedly executing it enable multiple parts of the same
shape, or a single part of identical recurring shape patterns as shown in diagram below, to be made
from one workpiece.
For such machining, set the desired shift amount of the program origin in this item.

SHIFT

T4P280

Note 1: Data set in this item becomes valid only if the number of times of program execution has
been set in item above.
Note 2: If no data has been set in this item, the shift amount will be regarded as 0.
Note 3: Data must not be set in this item if a measurement unit (MES) is to be executed. Setting data
other than 0 may cause contact between the touch sensor and the workpiece.
Note 4: As for repetitive machining on a single workpiece, the following condition must be satisfied:
LENGTH > NUM. × SHIFT + WORK FACE
(Common data) (END unit) (Common data)

10-25
 MAZATROL FUSION 640MT

10-26
 MAZATROL FUSION 640MT

DATA I/O (Input/Output)

11-1
 MAZATROL FUSION 640MT

11-2
 MAZATROL FUSION 640MT
DATA I/O - (INPUT/OUTPUT)

1. Press F1 key, select DATA IN/OUT from the menu shown below.

2. Select the method of data transfer.

CMT I/O- Enables transfer via RS232C interface.(using Mazak Micro Disk)
TAPE I/O-Enables transfer via RS232c interface (using paper tape punch/reader
or personal computer).
DNC I/O- Enables transfer via RS232C interface with an external CPU.
HARD DISK-Enables transfer from NC memory to PC hard disk of the Mazatrol
Fusion 640 control.
FLOPPY-Enables transfer(I/O) to a standard Dos format 3.5 inch floppy disk.
CARD- Enables transfer (I/O) to a standard PCMCIA Flash disk.

11-3
 MAZATROL FUSION 640MT

CARD OPERATION

The location of the I/C Memory card

interface can be found to the right hand
side of the NC monitor as shown on the
picture to the left.

To transfer data onto the card, insert the

card into the slot and follow the procedure
as explained below.

3. Select CARD from the menu shown below.

11-4
 MAZATROL FUSION 640MT
4. Press the menu DIR. SELECT

5. Select a directory by positioning the cursor onto the directory name or type in a
new directory name (Max. 8 characters), and then press OK to confirm.

11-5
 MAZATROL FUSION 640MT

6. The directory name selected will then be set. Select either LOAD or SAVE
option from the menu keys shown below.

11-6
 MAZATROL FUSION 640MT

7. Select data to be transferred, and then press START. ( If using the SAVE
command, by selecting PROGRAM FILE, a list of the program numbers
within memory can be viewed for ease of selection)

NOTE: When using the SAVE command to the selected directory, it is not
possible to add further data to this directory at a later stage. This will result
in the previous data being overwritten !!

11-7
 MAZATROL FUSION 640MT
FDD OPERATION

1. Select FLOPPY from the menu on the DATA I/O display.

2. Press the menu DIR. SELECT

11-8
 MAZATROL FUSION 640MT

3. Select a directory by positioning the cursor onto the directory name or type in a
new directory name (Max. 8 characters), and then press OK to confirm.

4. The directory name selected will then be set. Select either LOAD or SAVE
option from the menu keys shown below.

11-9
 MAZATROL FUSION 640MT

5. Select data to be transferred, and then press START. (If using SAVE
command, by selecting PROGRAM FILE, a list of the program numbers
within memory can be viewed for ease of selection)

NOTE: When using the SAVE command to the selected directory, it is not
possible to add further data to this directory at a later stage. This will result
in the previous data being overwritten!!

11-10
 MAZATROL FUSION 640MT
HARD DISK OPERATION

1. Select HARD DISK from the menu on the DATA I/O display.

2. Press the menu DIR. SELECT

11-11
 MAZATROL FUSION 640MT
3. A window will appear within the screen.

4. Select a directory by positioning the cursor onto the directory name within the
window, or, type in a new directory name (Max. 8 characters), and then press OK
to confirm.

11-12
 MAZATROL FUSION 640MT
4. The directory name selected will then be set. Select either the LOAD or SAVE
option from the menu keys shown below.

5. Select data to be transferred and then press START. (If using the SAVE
command, by selecting PROGRAM FILE, a list of program numbers stored
within the memory can be viewed for ease of selection.

11-13
 MAZATROL FUSION 640MT

NOTE: When using the SAVE command to the selected directory, it is not
possible to add further data to this directory at a later stage. This will result
in the previous data being overwritten !!

The picture below shows the Microsoft Windows ’95 Explorer TM taken from the
FUSION 640T display.
The Directories you create are stored in a directory named “OTHER”. This
directory is stored in a directory called “T_BACKUP” on the hard drive (C:
Drive) of the FUSION 640MT’s P.C. side.

WARNING: No attempt should be made to alter or delete this structure.

11-14