EN_ Complete Sinumerik Operate Milling_v26

Operating and Programming Documentation

828D/840Dsl Sinumerik operate

Milling

Edition 2011.1 Training Manual This document was produced for training purposes. Siemens assumes no responsibility for its contents.

SINUMERIK 828D 840D sl SINUMERIK Operate Operating and Programming Manual for Milling machines

Valid for:

Sinumerik 828D Software 4.3 840D sl Sinumerik Operate Software 2.6

Start B551 General Technology basics

Contents B552 Geometry Basics

B553 Simple Contour Elements

B554 Mathematical Principles B555 Zero offset and Reference Points

B556 Program Structure B559 Loops, Jumps, and Repetitions

B558 Program of Subroutines

B557 Cutting Edge Radius Correction

B566 Operating Elements

B567 Switching on the Machine

B568 Basic Operations

B560 Mirror - offset rotate - scale when milling

B565 Basics

B569 Operating Area MACHINE

B570 Operating Mode JOG B573 Operating Area PARAMETER

B572 Operating Mode AUTO

B571 Operating Mode MDA

B574 Operating Area Program

B575 Operating Area Program Manager B576 Operating Area Diagnostics

B577 Operating Area Start-Up

B604 Basics of Programming with programGUIDE

B609 Drilling programGUIDE

B616 Milling programGUIDE

B608 Drilling Shopmill

B600 Basics of Programming with Shopmill

B656 Measure Milling programGUIDE

B624 Contour Milling programGUIDE

B500 Cycles B615 Milling Shopmill

B655 Measure Milling Shopmill B623 Contour Milling Shopmill

B700 Drawings of programming Examples

B639 Straight Circle Shopmill

End

B551

1

General technology basics

Brief description

Objective of the module: Working through this module you become familiar with the most important technological aspects and machine functions. Description of the module: This module explains the general layout of a program, with respect to the technological commands as per DIN 66025 for turning and milling. Content: Layout of a CNC-program Programming of the technology data Switching commands Programmable presettings Summary

828D/840Dsl SINUMERIK Operate 828D/840Dsl SINUMERIK Operate

Page 1

This document was produced for training purposes. Siemens assumes no responsibility for its contents.

B551

B551

B551

Page 2

828D/840Dsl SINUMERIK Operate

B551 General technology basics: Description This module explains the general layout of a program, with respect to the technological commands as per DIN 66025 for turning and milling.

General technological aspect: START

Layout of a CNC-program

Programming of the technology data

Switching commands

Programmable presettings

Summary

General technological aspect: END

Notes :


Page 3

B551

Section 2 Notes:

Layout of a CNC-program A CNC-program, also known as part program, consists of a logical sequence of commands, which are executed step-by-step by the control unit after the program has been started. The manufacturers of control units recognize and apply the guidelines as per DIN 66025. Each program is compiled and stored under a program name in the control unit. The name can contain letters as well as numbers. A block starts with a block number followed by the commands. Each command consists of command words, which in turn consist of an address letter (A-Z) and an associated numerical value (both upper or lower case characters are permissible). Program layout: Departure information Block Nr..

N

Auxiliary command

G

Coordinate axes

X

Y

Switching information

Interpolation parameter

Z

Geometrical data

I

J

K

Feed

Speed

Tool

Misc. function

F

S

T

M

Technological data

The block number is a program-technical assignment, which is not evaluated by the control unit as a command. It is usually programmed to go up in steps of 10 and serves the user only for a better oversight. It has no effect on the program execution. The geometrical data include all instructions that clearly define mathematically the motion of the tool or the axes. The technological data are used for instance to activate the required tool and to pre-select the necessary cutting parameters feed rate and spindle speed. Miscellaneous functions can control for example such things as direction of rotation and auxiliary appliances. Programming example: …. N80 T1; Roughing tool N90 M6 N100 G54 F0.2 S180 M4 N110 G00 X20 Y0 Z2 D1 N120 …. In order to improve the oversight within a program, comments can be optionally added at the end of a block. These must be preceded by a semicolon; Any characters that follow thereafter will not be taken account of by the control unit.

B551

Page 4


Section 3

Programming of the technology data Before every technological working step in a CNC-Program the respective tool must be selected by means of the addresses “T” and “D”.

Notes:

The address “T” is followed by the name of the tool, which may be stated either with numbers or letters (here only the variant using numbers will be dealt with). All applicable tool data (e.g. tool type, length, radius, etc.) are activated in the program with the address “D”. Here a complete set of data “D“ is referred to as “Cutting edge”. Several cutting edge numbers (D1 … D9) may be generated for each tool. Programming example:

Explanation:

N10 T17 ; Drill

Block 10, call-up of tool 17, Commentary to the tool Tool change, The cutting edge D... must be activated in the block with the first axis movement.

N20 M6 N30 … D1

After the call-up of the tool, follows the selection of the optimum cutting values with the addresses “F” and “S”. The feed rate vf with the address “F” can be entered either as feed per min (in mm/min) or as feed per revolution (in mm/rev). The Cutting speed vc with the address “S” can be entered either as spindle speed in revolutions per minute (rev/min) or direct as cutting speed in meters per minute (m/min). Default status of the machines when they are powered up are as follows:  Milling machines with feed rate “F” in mm/min

Code G94

 Turning machines with feed per revolution “F” in mm/rev

Code G95

Selection of cutting speed:  Constant cutting speed “S” in m/min (Relative to workpiece Ø)

Code G96

 Deactivate constant cutting speed “S” spindle speed in rev/min (default)

Code G97

Programming example 1: N10 T20 ; Endmill N20 M6 N30 G94 F200 S1000 M3 D1 N40 ….

Explanation:

vf = 200 mm/min, n = 1000 min-1

Programming example 2:

Explanation:

N10 T2; Turning tool, finishing N20 G96 F0.1 S200 M4 D1 N30 ….

vf = 0,1 mm/rev , vc = 200 m/min


Page 5

B551

Section 4 Notes:

Switching commands There are different commands to control the direction of rotation of the work spindle. Additional auxiliary functions can for example control cooling circuits, clamping devices, auxiliary functions and running of the program. But the presence of these additional functions depends entirely on the technology and the machine design. The following list should be only considered as an example of commands: Instruction

Meaning

M00 M03 M04 M05 M06 M08 M09 M30

Programmed Halt Work spindle ON, clockwise Work spindle ON, anti-clockwise Work spindle Halt (however, the program continues) Tool change Coolant ON Coolant OFF End of program; jump back to the start of the program

Programming example: N10 T1; Face mill N20 M6 N30 G94 G97 F600 S2500 D1 N40 M3 M8 ….. N90 M30

Explanation: Tool change vf = 600 mm/min, n = 2500 min-1 Spindle ON clockwise, coolant ON End of program

(Note: Further functions can be found in the annexure of this manual)

Effect of the switching commands M3 and M4 Example Milling

Example Turning

M3

M4 M3 Viewing direction

M4

B551

Page 6


Section 5

Programmable presettings When starting a part program the basic settings as defined by the manufacturer will be activated. These depend on the individual machine specification and apply thereafter for the whole of the program run (modal) unless they are changed by the operator in the program.

Notes:

This section describes just a few of the possible selections for turning- and milling machines that deserve highlighting. Note: Codes that have already been dealt with are no longer included

Continuous path behaviour: Exact stop

Code G09 block-by-block

Code G60 * modal

In order to reach the final position precisely the path velocity is reduced at the end of the block towards zero. This is useful, for instance, to obtain relatively sharp edges when machining around contour corners. However, it must be borne in mind that, if there are too many positioning sequences, it will result in increased machining time and cannot be neglected.

Continuous control operation

Code G64

In this case the tool moves as much as possible with constant velocity without deceleration at the end of a block. Hence the machining time is less than under the continuous path status “Exact stop“. The corners of contours are machined without any relief and therefore the corners are not so sharply defined. With this function the control works with a speed control taking into account several blocks ahead (Look Ahead). The even speed in this instance results in better cutting conditions and also a better surface quality. The following image compares the frequent braking and accelerating sequences between the individual blocks in case of G60 and the constant speed in case of G64. Feed rate

G64 Continuous path mode with Look Ahead Programmed feed rate

G60 Exact stop

Block path

*

Usual preset starting status


Page 7

B551

Section 5 Notes:

Programmable presettings The continuous path behaviour “Exact stop“ with the Codes G09 or G60 respectively does not entirely ensure dimension-wise as to how precisely a corner point between two positioning blocks is attained. If an exact stop has been activated in a program, the codes described below can be used to specify a very precise braking behaviour at the end of blocks. By this it is possible to determine as to how precisely the programmed corner point will be attained. Change-over when the positioning window “fine” is reached Code G601 The tool motion changes to the next block when the tool has reached the fine positioning window. Sharp contour corners result at the programmed destination points. Change-over when the positioning window “coarse” is reached Code G602 This code can be used to obtain a defined rounding of the programmed contour corners. The block change-over occurs already at the coarse positioning window. Block change-over

G601

Destination point of the programmed path Actual tool paths depending on the positioning window

G60

Tool

A dimensional definition of the positioning windows “coarse” and “fine” is preset by means of machine datum. Please find out the values preset on your machine by the machine manufacturer from his operation manual if you are going to use the described codes.

B551

Page 8


Section 5

Programmable presettings There is yet another means of influencing the continuous path behaviour by changing over to the next positioning block depending on the programmed path velocity of the tool. Change-over when the setpoint position is reached:

Notes:

Code G603

The block change-over is initiated as soon as the control has calculated the setpoint speed for all axes to be equal to zero. Since the physical tool position lags behind the calculated value by a certain amount, the effect in this case is that the axis changes direction before the end of the interpolation is reached. The greater the feed rate, the greater is also the lag of the tool behind the evaluated value and therefore the rounding radius. This permits the contour corners to be formed in dependence on the path velocity.

Destination point of the programmed path (Interpolation ends) Actual tool path with smaller feed rates

Workpiece

Actual tool path with greater feed rates

Hint: The rounding radius depends on the programmed path velocity as swell as the drive dynamics of the machine. The codes G601, G602 and G603 are modal. They only have an effect in conjunction with active exact stop with G09 or G60.


Page 9

B551

Section 6 Notes:

Summary Address

Meaning

T D F S

Tool number Cutting edge (tool data) Feed/Feed rate Speed/Cutting speed

Path information/departure commands Instruction

Meaning

G09 G60 G64 G601 G602 G603

Exact stop, operative block-by-block Exact stop, modal function Continuous path control Change-over when positioning window “fine” is reached Change-over when positioning window “coarse” is reached Change-over when the interpolation end is reached

G70 G71

Input system in inches Input system metrical

G94 G95

Linear feed in mm/min * Feed per revolution in mm **

G96 G97

Constant cutting speed in m/min ** Spindle speed in min-1 * * **

Switching-ON status for milling machines Switching-ON status for turning machines

Switching information Instruction

Meaning

M00

Programmed halt

M03 M04 M05

Work spindle ON, clockwise Work spindle ON, anti-clockwise Work spindle Stop

M06

Tool change

M08 M09

Coolant ON Coolant OFF

M17 M18

End of subprogram End of program, jump back to the beginning of program

All instructions (except G09) mentioned above are modal, until they are programmed to deactivate with different set of instructions. Furthermore there are instructions that are operative only block-by-block, e.g. G09. These are automatically reset by the control unit with the succeeding block.

B551

Page 10


B552

1

General geometry basics

Brief description

Objective of the module: Working through this module you learn to understand the programming planes and also how to specify points in a DIN conforming coordinate system. Description of the module: This module explains the assignment of the axis and plane descriptions to the coordinate system of the machine and also teaches the definition of points in relation to the work space. Content: Right hand rule Explanation of the axis assignments Points and distances in the work space Programming planes


Page 1


B552

B552

B552

Page 2


B552 General geometry basics: Description This module explains the assignment of the axis and plane descriptions to the coordinate system of the machine and also teaches the definition of points in relation to the work space.

General geometry basics: START

Right hand rule

Explanation of the axis assignments

Points and distances in the work space

Programming planes

General geometry basics: END

Notes :


Page 3

B552

Section 2

Right hand rule

Notes: Explanation: According to DIN standard the various axes of motion within work space of CNC machines are addressed by alphabets. The rules for the assignment of the axes are determined in this DIN-standard. The machine coordinate system that is derived from the DIN-standard is the base for the geometrical description of work pieces which allows us to clearly determine the points in a plane or in space. The cartesian (rectangular) spatial coordinate system can be best described with the “Right hand rule”. Here the fingers of the right hand represent the axes: “X” (thumb), “Y” (first finger) and “Z” (middle finger). The finger tips point in the positive direction.

Vertical turning machine

Horizontal milling machine

The position of the machine coordinate system is specified by the machine manufacturer keeping the following in mind:

Definition of axis according to DIN-standard:  Z-Axis: Is aligned parallel to the working spindle or coincides with it. The positive direction points away from the work piece. In case of more than one spindle, one of them will be declared as the main spindle.  X-Axis: Is aligned parallel to the set-up plane or coincides with it. If the Z-axis is vertical, the positive X-axis is directed towards the right. If the Z-axis is horizontal, the positive X-axis is directed towards the left.  Y-Axis: Is perpendicular to the X- and Z-axis, in such a way that a spatial cartesian coordinate system results. The direction “FROM” the work piece “TO” the tool is “PLUS” The tool movement is “ALWAYS” to be programmed!

B552

Page 4


Section 3

Defining of axis within a workspace

Notes:

Explanation as per DIN 66217 or ISO 841: However defining only three axes is not enough on modern machine tools. For instance if the milling head of a milling machine is to be swivelled by a certain angle or the quill of a tailstock is to be moved, a further definition of these axes is required. The DIN standard provides the following variants for such cases.

Here the rotational axes A/B/C are associated with the X/Y/Z axes. Looking in the positive direction of the linear axis, a clockwise rotation equals a positive rotation of the associated rotary axis.

The axes U/V/W are parallel to the axes X/Y/Z. V

The positive direction is that of the associated main axis.

W

U

Y

B

W

X Z


Page 5

B552

Section 4 Notes:

Points and distances within the work space Explanation: For the determination of all points within the work space, the control unit requires a zero point of the coordinate system. This has been determined by the machine manufacturer. All other points have either fixed distances from the machine zero point or else the distance must be defined. The machine zero point (M) is determined by the machine manufacturer and cannot be altered. On milling machines point is usually set on the work table, and on turning machines on the spindle flange. The work piece zero point (W) is the origin of the work piece coordinate system. This can be specified by the programmer and should always be chosen in a way that the least calculation work is required to determine points on the contour given the dimensioning of the drawing. For turning work it lies mostly on the turning axis and the right hand planar face. The reference point (R) is approached for initializing the path measuring system, which means that at this point all axes are set to zero. This is necessary since generally speaking the machine zero point cannot be approached. The tool carrier reference point (F) is of prime importance for the adjustment of preset tools. The lengths “L” (XPF) and offset “O” (ZPF) shown in the image below are used as tool calculation values for instance for the tool radius correction and must be entered into the tool memory of the control unit. ZMR

Example: 2-axis turning machine

B552

Page 6

XMR

ZMW

XMF

XPF

ZMF

ZPF


Points and distances within the work space

Section 4 Notes:

ZMW

ZMR

ZPF

Example: 3-axis milling machine

XMR

YMW

YMR

XMW

XMR = YMR = ZMR =

Distances from the reference point to the machine zero point. These are set by the machine manufacturer during commissioning and are transferred to the control unit when the reference point is reached.

XMW = YMW = ZMW =

These represent distances from the machine zero point to the work piece zero point. The work piece zero point must be determined by the operator by scratching or probing and entered into the tool correction memory.

XPF = ZPF =

Distances from the tool carrier reference point to the tool point on the cutting edge or the front face of the milling cutter.

XMF = ZMF =

Distances from the machine zero point to the tool carrier reference point. The distance is determined by the machine manufacturer and entered into the control unit (only relevant on turning machines).


Page 7

B552

Section 5 Notes:

Programming planes Continuous path control units can control slides and tool carriers simultaneously along 2 or more axes at a programmed feed rate. For this the speed of the individual drives must be matched to one another. This job is taken over by the interpolator of the CNC-control unit. This is a software program for the evaluation of intermediate positions and speed conditions of the individual axes such that the slides can follow the programmed path. Starting with a 2 ½-D Continuous path control unit the interpolation can be switched between the three different planes.

+Z

G18 G19 G17

-Y

+X

A selection of the plane is made with the associated programming instruction:  XY-Plane - programming command G17  XZ-Plane - programming command G18  YZ-Plane - programming command G19 Note: The standard plane being used for working with CNC-Turning machines is G18. With CNC-Milling machines the programming plane G17 is being used. The working plane should either be programmed at the beginning of the NC-program, or before programming an operation in the relevant working plane. The active programming plane is modal and remains active until changed by another programming instruction.

B552

Page 8


B553

1

Simple contour elements

Brief description

Objective of the module: Working through this module you learn to program linear and circular interpolation commands both with absolute and incremental dimensions. Description of the module: This module explains the use of absolute, incremental and mixed coordinate points. It also explains the programming of simple geometrical path conditions. Content: Absolute and incremental dimensioning, mixed programming Rapid traverse motion Straight line interpolation Circular interpolation Summary


Page 1


B553

B553

B553

Page 2


B553 Simple contour elements: Description This module explains the use of absolute, incremental and mixed coordinate points. It also explains the programming of simple geometrical path conditions.

Simple contour elements: START

Absolute and incremental dimensioning, mixed programming

Rapid traverse motion

Straight line interpolation

Circular interpolation

Summary

Simple contour elements: END

Notes :


Page 3

B553

Section 2 Notes:

Absolute and incremental dimensioning, mixed programming 2. 1 Absolute dimensioning When writing CNC-programs a fundamental differentiation must be made between absolute and incremental coordinates. Which of the two options the programmer chooses depends on the usage of the program and the dimensioning on the drawing. Absolute dimensioning, Code G90 All dimensions always refer to the active work piece zero point. About workpiece zero point refer to Module B555 - “reference point, workpiece offset”, Section 3. The absolute coordinates in a departure command describe the position, to which the tool is to traverse. Example: Coordinates for milling:

Workpiece zero point

G90

X

Y

P1

20

35

P2

50

60

P3

70

20

Coordinates An example for turning: (All X values are diameter values, DIAMON)

G90

X

Z

P1

25

-7.5

P2

40

-15

P3

40

-25

P4

60

-35

Code G90 is usually activated as machine status when switching ON. It is modally active for all axes simultaneously and can be reset to incremental dimensioning with G91.

B553

Page 4


Absolute and incremental dimensioning, mixed programming

Section 2 Notes:

2.2 Incremental dimensioning Code G91 (also known as chain dimensioning). All position statements refer to the current starting position of the tool. The programmed value states the coordinate distance, by which the tool is being traversed. Example: Coordinates for milling:

G91

X

Y

P1

20

35

P2

30

20

P3

20

-35

Example: Coordinates for turning: (All X values are radius values, DIAMOF)

G91

X

Z

P1

12.5

-7.5

P2

7.5

-7.5

P3

0

-10

P4

10

-10

Code G91 is modally active for all axes simultaneously and can be reset to absolute dimensioning with G90.


Page 5

B553

Section 2 Notes:

Absolute and incremental dimensioning, mixed programming 2.3 Mixed Programming As already mentioned, the destination point coordinates can be stated in the program for all types of interpolation as absolute or incremental values respectively. Depending on the presently activated status (G90 or G91), all further coordinate values will refer then also this type of dimensioning. In practice, however, it is often sensible to mix the two possibilities within a program block. The control unit provides a comfortable means of instruction to utilize this additional possibility.

Mixed programming:

Codes AC(…) and IC(…)

A dimension value will also be taken as an absolute dimension under G91 if the following syntax is used: AC(numerical value) If a dimension value is to be taken to be an incremental value under G90, it must be written as follows: IC(numerical value) Clarification of mixed programming with an example for milling: G90

X

Y

P1

20

35

P2

IC(30)

IC(25)

P3

70

IC(-40)

G91

X

Y

P1

AC(20)

AC(35)

P2

30

AC(60)

P3

20

-40

A great number of various possibilities are available to the operator in dealing with a mixture of the two types of dimensioning: Note: The above example describes only a small selection of mixed coordinate inputs. A further selection of examples can be found in the description of interpolation types in this manual.

B553

Page 6


Section 3

Rapid traverse motion

Notes:

Code G00 Rapid traverse is used for the quickest possible repositioning of the tool to the contour element or, for instance, for moving the tool to the tool changing position. The highest possible speed along a straight line that the machine is capable of attaining is used, however, no machining is possible here. Hence the control unit does not require a value input under the address “F”. Repositioning with rapid traverse can be programmed to take place in several axes simultaneously.

Programming example: N10 T1 ; End mill N20 M6 N30 G00 X200 Y80 Z2 D1

N90 M30

Explanation:

Motion at rapid traverse to the destination point X200, Y80, Z2 (taking into account the tool length) End of program

The above programming example repositions the tool from point P1 to the point P2.

straight line


Page 7

B553

Section 4 Notes:

Straight line interpolation 4.1 Straight line interpolation Code G01 The straight line interpolation is used to move the tool with an exactly defined speed along a straight line from the current position to the programmed destination point. All axes can be traversed simultaneously, in which case the resulting line of motion can lie anywhere at an angle within the working space. For this the control unit requires a specified feed rate which at the latest must be defined under the address “F” in the block containing the Code G1. The following example describes the milling of a slot with absolute dimensioning as per the drawing shown below. Note: The setup feed rate G94 defines the feed rate in millimetre per minute (mm/min), in comparison to setup feed rate G95 that defines the feed rate in millimetre per revolution (mm/rev). Programming example:

Explanation:

N10 T1 ; End mill Tool call-up T1 N20 M6 N30 G94 F300 S2000 M3 D1 Technology block for the tool T1 with the cutting edge D1, N40 G90 G00 X40 Y48 Z2 M8 With rapid traverse to the starting position P1 on the safety plane (absolute dimensions), N50 G01 Z-12 Plunging with feed rate, N60 X20 Y18 Z-10 Milling the slot in 3 axes (G1 is modally active), N70 Z2 F1000 Retraction with increased feed rate N80 G00 Z200 N90 M30 The following program section shows the milling of the same slot using incremental dimensioning (up to N40 see above):

N50 G91 G1 Z-14 N60 G01 X-20 Y-30 Z2 N70 G90 Z2 F1000 N80 G00 Z200 N90 M30

B553

Page 8

Infeed along Z by –14 mm, Incremental traversing of the axes Retraction with absolute dimensions


Section 4

Straight line interpolation 4.2 Straight line interpolation with mixed programming

Notes:

The example shown below describes the milling of the slot with mixed cordinates input. Program blocks such as the call-up of the tool etc., which have already been dealt with, will not be repeated. Important: If any address letter “X”, “Y”, “Z” is not followed immediately by a numerical value, an equal-sign must be written instead. Syntax:

X=IC(…), Y=AC(…), Z...

Programming example under G90:

Explanation:

…. N40 G90 G00 X40 Y48 Z2 M8 N50 G01 Z=IC(-14) N60 X20 Y=IC(-30) Z-10 N70 Z2 F1000 ….

To starting position absolute Incremental coordinate Z Incremental coordinate Y

Programming example under G91:

Explanation:

N10 G91 …. N40 G00 X=AC(40) Y=AC(48) Z=AC(2) N50 G01 Z-14 N60 X=AC(20) Y-30 Z2 N70 Z=AC(2) F1000 ….

Incremental dimensioning,


To starting position P1 absolute Incremental coordinate Z Absolute coordinate X Absolute coordinate Z

Page 9

B553

Section 5 Notes:

Circular interpolation 5.1 Circular interpolation Code Code

G02 (clockwise) G03 (anti-clockwise)

A circular interpolation permits the traversing of the tool with a defined speed along a circular path from the present start point to the programmed destination point. Apart from the destination point coordinates, the control unit also needs statements about the sense of rotation and the centre of the circle. The centre is entered with “I”, “J” and “K” with incremental dimensions with the centre point as origin. The following assignment applies:  I for the X-axis  J for the Y-axis  K for the Z-axis Programming example with G02: Explanation: ….. N40 G00 X30 Y40 Z2 With rapid traverse to the start point N50 G01 Z-5 Grooving with Z N60 G02 X50 Y40 I10 J-7 Circular interpolation clockwise N70 G01 Z2 F1000 …..

Start point End point

Centre point

The following example describes an anti-clockwise circular interpolation as shown in the sketch above. Note: The endpoint in the sketch is now the starting point for the circular interpolation. Programming example with G03: ….. N40 G00 X50 Y40 Z2 N50 G01 Z-5 N60 G03 X40 Y40 I-10 J-7 N70 G01 Z2 F1000 …..

B553

Page 10

Explanation: With rapid traverse to the start point Circular interpolation anti-clockwise


Section 5

Circular interpolation 5.2 Circular interpolation with mixed programming

Notes:

Particularly the incremental statement of the centre of the circle usually represents some difficulties to the operator in practice, since it must often be evaluated using triangle calculations. This is a prime example of where the mixed coordinate programming of the circle centre point in absolute dimensions comes in useful. Programming example: ….. N40 G00 X30 Y40 Z2 N50 G01 Z-5 N60 G02 X50 Y40 I=AC(40) J=AC(33) N70 G01 Z2 F1000 …..

Explanation:

Circle centre absolute

Start point End point

Centre point


Page 11

B553

Section 5 Notes:

Circular interpolation 5.3 Circular interpolations before and behind the turning axis The sketch below shows once again the principle of direction programming of circular interpolations. Code G02: Circular arc clockwise Code G03: Circular arc anti-clockwise The following sketch shows the circular arc orientation on turning machines with different tool arrangements due to the machine layout.

Tool arrangement behind the turning axis G2 G3

G2 G3

Tool arrangement in front of the turning axis

Note: No matter which tool arrangement is applicable to the particular machine, the program as per DIN ISO always describes the contour of the workpiece behind the turning axis.

B553

Page 12


Section 6

Summary

Notes:

Path information Instruction

Meaning

G90

Coordinate input with absolute dimensions

G91

Coordinate input with incremental dimensions

G00

Linear motion with rapid traverse

G01

Straight line interpolation with defined speed

G02

Circular interpolation clockwise

G03

Circular interpolation anti-clockwise

All the above departure commands are modal.

Interpolation parameter

Meaning

I

Circle centre coordinate in X, incremental from starting point

J

Circle centre coordinate in Y, incremental from starting point

K

Circle centre coordinate in Z, incremental from starting point

The interpolation parameters are operative block-by-block

Mixed programming for coordinate input IC(…) AC(…)

Incremental dimension input Absolute dimension input

The statements IC(…) and AC(…) are valid only for the address preceeding them. Example: Instruction

Meaning

X=IC(10) Y=AC(20)

Traverse by 10 mm in X Traverse to 20 mm in Y


Page 13

B553

Section End Notes:

B553

Page 14


B554

1

Basic mathematical principles

Brief description

Objective of the module: Working through this module you learn the mathematical approach necessary for the programming and for the calculation of missing contour points. Description of the module: In this module contour points will be calculated using the Pythagorean theorem and trigonometrical functions (sine, cosine and tangent). Content: Types of angles The Pythagorean theorem Trigonometrical functions Example calculations


Page 1


B554

B554

B554

Page 2


B554 Basic mathematical principles: Description

Basic mathematical principles: START

In this module contour points will be calculated using the Pythagorean theorem and trigonometrical functions (sine, cosine and tangent).

Types of angles

The Pythagorean theorem

Trigonometrical functions

Example calculations

Basic mathematical principles: END

Notes :


Page 3

B554

Section 2 Notes:

Types of angles 2.1 Basic principles of coordinate evaluation Almost all of the contours encountered during machining can be traced back to a interface of straight lines and circular arcs. For part programming the respective endpoint of the contour element must be known. In most cases these contour points can be taken directly from the drawing provided dimensioning is NC-suitable. In some cases, however, the an evaluation of coordinates may be necessary. For these calculations a basic knowledge of the types of angles, trigonometrical functions and the Pythagorean theorem is required. 2.2 Types of angles In the case of oblique work piece contours angles with a definite relationship to one another result between the contour sections. Depending on their relative position a differentiation is made between complementary angles, step angles and side angles.

Complementary angles add up to 180°



Step angles have always the same value



If a transition is at right angles to the radius centre point it is always a tangential transition, and there is no corner shown on the technical drawing. If a corner line is shown, it is not a tangential transition.

B554

Page 4


Section 3

The Pythagorean theorem The right angled triangle has a special meaning in geometry, since the sides of such a triangle exhibit a definite relationship to one another.

Notes:

The various sides of the right angled triangle are named specifically:  The longest line opposite the right angle is called the hypotenuse.  The two other lines, which form the right angle, are called cathetus.  The side opposite an angle is called the opposite side.  The bounding side of the angle is called the adjacent side.

In case of a right angled triangle the missing length of a side can be calculated if the length of the other two sides is known. For this the Pythagorean theorem is used.

Pythagorean theorem: In a right-angled triangle the square of the hypotenuse (the side opposite the right angle), c, is equal to the sum of the squares of the other two sides, b and a - that is: a² + b² = c².

c²= a² + b²

5x5=25 c 16+9=25

a 3x3=9

b

4x4=16

By suitable rearrangement of the equations the respective sides can be calculated.


c =

a2  b2

b =

c 2  a2

a =

c 2  b2

Page 5

B554

Section 4 Notes:

Trigonometrical functions The trigonometrical ratios describe the relationships between the angles and the sides in a right angled triangle. With the aid of these trigonometrical functions it is possible to calculate both angles and sides in a right angled triangle. For this one side and an angle or two sides must be known. The selection of the suitable trigonometrical function, i. e. the sine, cosine or tangent, depends on which sides and angles are known and which side or angle is to be found.

1. Adjacent side (AS) 2. Hypotenuse (H) 3. Opposite side (OS) β

α Angle

2 3

β Angle

α 1

By the use of the various trigonometrical functions all sides and angles can be calculated.

Sine function

sin α 

OS H

OS sin 

H

OS  sin α * H

Cosine function

cos 

AS H

H 

AS cos 

AS  cos * H

Tangent function

tan  

B554

OS AS

AS 

Page 6

OS tan 

OS  tan * AS


Section 5


Notes:

5.1 Task

P1

M1

X

25

35

Z

-20

-20

P2

P3

P4

M2

40

30

 Evaluate the missing coordinates of the points “P1” to “P4”, as well as “M1” and “M2”  Enter the coordinate values in the table.  The values for the spaces shown with a dark background are dimensions that can be taken directly from the drawing. Note: All X values are diameter values See the next page for the solution of this example. 828D/840Dsl SINUMERIK Operate

Page 7

B554

Section 5 Notes:

Example calculations 5.2 Solution for the example calculation

P1

M1

P2

P3

P4

M2

X

25

35

27,929

37,071

40

30

Z

-20

-20

-23,536

-28,107

-31,642

-31,642

For the solution method see the following page

B554

Page 8


Section 5


Notes:

5.3 Solution method

Since the two sides are equal, all values can be found using the Pythagorean theorem.

xp2  5  5² / 2  3,5355 zp2  xp2  3,5355

zp4  zp2 * (1)   3,5355 xp3  zp4  3,5355

P2x  25  (2 * (5  xp2))  25  (2 * (5  3,5355))  27,929 P2z  P1z  zp2  20  zp2  20  5² / 2  20  3,5355   23,5355

P3x  40  2 * (5  3,5355)  37,071 a  (P3x  p2x) / 2  (37,071  27,929) / 2  4,571

zp3  a  4,571 P3z  P1z  zp 2  zp3  20  3,535  4,571   28,1065

P4z  P3z  zp2  28,1065  3,5355   31,642


Page 9

B554

Section End Notes:

B554

Page 10


B555

1

Zero points, work offset and reference point

Brief description

Objective of the module: In this module you learn to use the various zero points within the working space of a milling machine.

Description of the module: This module describes the call-up of individual work piece zero points on the work piece with reference to various starting conditions. Content: Position of the machine zero point Zero point offset G54 Further zero point offsets Further zero point offsets Summary


Page 1


B555

B555

B555

Page 2


B555 Zero offsets and reference points: Description

Zero offsets and reference points: START

This module describes the call-up of individual work piece zero points on the work piece with reference to various starting conditions.

Position of the machine zero point

Zero point offset G54

Further zero point offsets

Further zero point offsets

Summary

Zero offsets and reference points: END

Notes :


Page 3

B555

Section 2 Notes:

Position of the machine zero point All axis motions on a CNC-machine tool refer to the right-hand Cartesian coordinate system. Note: See also Module B552 - “Geometry basics”. The entire path measuring system is initialized by approaching the reference point with all axes. At the same time the control unit activates the coordinate system at the machine zero point.

M Machine zero point

This fixed coordinate point (origin) is determined by the manufacturer and cannot be altered by the operator. It serves as a reference point for the machine coordinate system (MCS) of the machine tool.

Z X

M

B555

Page 4

Y


Section 3

Zero point offset G54 For machining the workpiece the workpiece coordinate system (WCS) is available on the machine.

Notes:

This can be freely chosen by the operator depending on the manufacturing conditions or according to the usual workshop practice. By this you define a zero point on the workpiece which is offset from the machine zero point by a defined distance, obtaining a work piece zero point that is directly referred to the workpiece to be machined. W Workpiece zero point

Zero point offset:

Code G54 (modally operative)

With this command the workpiece zero point can be defined on the machine. The following image shows how the position of the workpiece zero has been shifted with G54 by the operator to the marked corner point, alternatively any other corner can be defined as workpiece zero

The determined zero point on the machine can be set in JOG mode and can be activated in the program with the same comand (G54). By this the coordinate origin for the program and the machine zero point coordinate are now identical. Programming example:

Explanation:

N10 G17 G54 ...

Plane selection, call-up of the zero point offset G54 Approach tool changing point Call-up tool T1

N20 G00 X200 Z300 N30 T1; Surface cutter ...


Page 5

B555

Section 4 Notes:

Further zero point offsets Nevertheless, for the efficient production of parts the availability of several workpiece zero points often makes sense. The control unit manufacturer provides for up to 99 selectable zero point offsets. Note: Depending on the machine parameters this number can be set differently. Please refer to the machine manual regarding the exact number of available zero points.

Further zero point offsets: Codes G55, G56 and G57 Codes G505 to G599 (all stated codes are modally operative)

The application example shows a requirement for a second workpiece zero offset. In the picture below the work piece zero point has been transferred with G55 exactly to the setting plane of the chuck jaws. In the program this must be activated by means of the code G55. G55 G54

The use of several zero point offsets can substantially reduce the setup times particularly in cases of one-off or small series machining. For example: You could define just once a specific setting point for each one of your clamping fixtures or else a specific work piece zero point for various work pieces. In the program the respective zero point offset depending on the clamping fixture or the work piece can then be selected. If an identical work piece is to be machined at a later time, the respective zero point is immediately available under the same code.

Important: Zero point offset instructions or commands are MODAL COMMANDS .i.e. once executed they remain active until they are newly defined with the same command or a different set of commands is activated.

B555

Page 6


Section 5

Tool changing point Milling machines usually have a fixed tool change position (TCP). This point is typically chosen in a way, that tools can be changed in a collision-proof area in the work space of the machine.

Notes:

For this the tool carrier is generally retracted well back into the positive range of the work space. Note: Take into account the real traverse ranges of your machine; the values used in the example are only exemplary!


Explanation:

N10 G17 G54 ... N20 G00 X300 Z150 N30 T1; Milling cutter ...

Approach of the tool changing point Indexing the turret to position T1

On this basis the tool carrier will traverse to various positions depending on the active tool length (Z) and the position of the work piece zero point. Note: It is always the tool tip that is being positioned.

Pos. Z

Pos. X

Pos. Y

On the next page a suggestion for the programming of an independent tool changing point can be found.


Page 7

B555

Section 5 Notes:

Tool changing point In order to approach a tool changing point that is independent of the length of the tool and the presently active zero point offset, the following conditions must be programmed: Switching OFF of all the active offsets or manipulations of the coordinate system

Code SUPA (operative block-byblock)

Deactivation of the tool lengths in X and Z

Code D0 (modally operative)


Explanation:

N10 G17 G54... N20 G00 X400 Z500 SUPA D0 Approach of tool changing point in the MCS, without tool data, N30 T1; milling cutter Indexing the turret to position T1, N40 D1 Call-up of the tool data for T1 …

Pos. X Pos. Z

Pos. Y Since with the use of the SUPA command any manipulations of the coordinate system have been deactivated for the programmed block only, they do not need to be reactivated. Keep in mind, to call up the required cutting edge again, after each tool change. Note: The extent of programming for the approach of the tool changing point can be reduced if for this purpose a subprogram is written (see page 8 in this module).

B555

Page 8


Section 6

Summary Suggestion of a subprogram for tool changing:

Notes:

Subprogram name: SUBR100.SPF N10 G17 G00 X300 Z500 SUPA G40 D0;

Approach of tool changing point, zero point offsets OFF, all tool corrections OFF

N20 RET;

Return to the main program, without interruption of the feed motion.

Explanation of the symbols

M Machine zero point

W Workpiece zero point

MCS

Machine coordinate system

WCS

Workpiece coordinate system

Instruction

Meaning

G54 to G57

Call-up of a selectable zero point offset *

G505 to G599

Call-up of further zero point offsets * (conditionally available)

D0

Deactivation of the tool offsets *

D1 - D9

Reactivation of the tool offsets after the tool change *

SUPA

Switching-OFF of programmable, selectable and external offsets **

RET

End of subprogram, return jump * **


Modally operative instruction Instruction operative block-by-block

Page 9

B555

Section End Notes:

B555

Page 10


B556

1

Program structure

Brief description

Aim of the module: In this module you learn how to structure a part program clearly and functionally.

Description of the module: This module describes the programming structure of NC-programs. Content: Basic principles of programming Program structure of a part program Program structure of a machining sequence Settings at the start of a program


Page 1


B556

B556

B556

Page 2


B556 Program structure: Description This module describes the programming structure of NC-programs.

Program structure: START

Basic principles of programming

Program structure of a part program

Program structure of a machining sequence

Settings at the start of a program

Program structure: END

Notes :


Page 3

B556

Section 2

Basic principles of programming

Notes: Certain principles should be followed during the creation of part programs:  The program must ensure that an unlimited number of work pieces can be produced with the quality (tolerances, surface quality, form and position deviation, etc.) required on the drawing with a minimum of production time and the least possible material wastage.  It is always the motion of the tool along the drawn ideal contour of the work piece.  If tolerances are shown, the programming is always referred to the middle of the tolerance. Example:  20 + 0,1 - programmed value = 20,05. Precise dimension corrections can be carried out on the machine by means of the wear correction feature for the tool.  The program should exhibit a clear and concise structure and should contain comments wherever possible to ensure that other users can understand the layout easily at later stages.

B556

Page 4


Section 3

Program structure of a part program The following flow chart represents a possible suggestion for a suitable structure of the main program.

Notes:

Program header

Tool call-up 1

Technology block

Approaching the safety level with the tool

Machining sequence 1

Retraction of the tool

no

yes Workpiece finished

Tool call-up 2

End of program

Technology block

Approaching the safety level with the tool

Machining sequence 2


Page 5

B556

Section 4 Notes:

Program structure of a part program The programming of the machining sequence can be achieved by means of description of the individual steps using departure commands (e.g. G00, G01, G02, etc.) or by means of machining cycles. The following representation refers to the flow chart in section 2 of this manual and describes a possible machining sequence. Programming with G-Codes

Activation of radius correction

Programming using cycles

Input of the individual parameters using the input mask and graphical support

Interpolation to the first destination point

Interpolation to the next destination point

Interpolation to the last destination point

Deactivation of the radius correction

The following criteria should be kept in mind when selecting between the two described possibilities:  Availability of the cycles on the respective machine.  Machining time required with cycles or with G-codes.  The relation of the number of work pieces to the required programming extent.

B556

Page 6


Section 5

Settings at the start of a program For the user it may be advantageous to switch on certain settings, that are to be activated in the part program, already in the program heading.

Notes:

If necessary, these modally operative commands can always be reset by other commands at any stage during the program. Suggestion of a program heading for a “milling” application: Programming example:

Explanation:

N10 G17 G54 G64 G71 G90 G94

X/Y-plane, 1st ZP-offset, continuous control, metrical system, absolute dimensions, linear feed rate F in mm/min,

N20…. …. Suggestion of a program heading for a “turning” application: Programming example:

Explanation:

N10 G18 G54 G64 G71 G90 G96

Z/X-plane, 1st ZP-offset, continuous control, metrical system, absolute dimensions, constant cutting speed S in m/ min

N20 DIAMON LIMS=3000

Diameter input*, speed limitation nmax= 3000 min-1

N30…. ….

Note: As the tool progresses towards the centre during facing, the spindle speed evaluated internally in the control unit increases steadily until eventually the maximum possible spindle speed would be attained. Depending on the clamping conditions and the size of the work piece a speed limitation should always be selected for reasons of safety.


Page 7

B556

Section End Notes:

B556

Page 8


B557

1

Cutting edge radius correction

Brief description

Objective of the module: In this module you learn to write a simple milling program, taking into account the radius correction.

Description of the module: This module describes the commands for radius correction, the rounding and the chamfering of edges. These commands can be used for writing a simple CNC-program. A explanations of the commands is provided.

Content: Cutter radius compensation Rounding and chamfering of edges Mixed incremental and absolute programming Summary Solutions of the tasks


Page 1


B557

B557

B557

Page 2


B557 Cutting edge radius correction: Description This module describes the commands for radius correction, the rounding and the chamfering of edges. These commands can be used for writing a simple CNC-program. A explanations of the commands is provided.

Cutting edge radius correction: START

Cutter radius compensation

Rounding and chamfering of edges

Mixed incremental and absolute programming

Summary

Solutions of the tasks

Cutting edge radius correction: END

Notes :


Page 3

B551

Section 2 Notes:

Cutter radius compensation The path programmed with G01, G02 and G03 represents the path taken by the centre of the milling cutter. In this case the radius of the milling cutter must be taken into account. Exercise 1 Open the program editor by pressing the following keys successively:

Write the following program header into the editor. Explain the blocks in the table. While doing this make yourself familiar with the editor. Mark the zero point on the drawing N10 G54 G64 G17 SOFT N20 T1

Select tool Nr. 1 (PF60 with tool tips)

N30 M6 N40 S1000 F200.M3 M8 D1 N50 G00 X115 Y65 Approach of starting point and safety level (P1) Z2 N60 G01 Z0 N70 X-35 N80 G00 Z2 N90 X115 Y15 N100 G01 Z0 N110 X-35 N120 G00 Z150 N130 X150 Y150 M9

Solution see page 13

N70

N50

N110

N90

Motion at feed rate Motion with rapid traverse

B557

Page 4


Section 2

Cutter radius compensation The instructions G41 or G42 are necessary for the programming of contours. With this the contour shown on the drawing can be described directly. The radius value for the milling cutter entered in the tool management is taken into account. The equidistant path for the cutter centre evaluated by the control unit is such that the required contour results on the cutter circumference.

Notes:

To enable the control unit to evaluate the correct equidistant path it must know whether the milling cutter is on the right or the left of the contour. This is determined by relative to the machining direction. Dimensional deviations can then be compensated for by changing the cutter radius.

Before activating the radius compensation a starting point should be chosen that is sufficiently far from the contour. If possible this distance should be greater than the cutter radius. The starting and end point must be chosen such that no damage to the contour occurs.

S=starting point E=end point Px=programmed contour points Equidistant path with feed direction

Solution 1: Approach and exit of the contour


Solution 2: Approach and exit from/into open area. The points „P0“ and „P9“ do not lie on the contour

Page 5

B557

Section 2

Cutter radius compensation

Notes:

The work piece shown on the left is to be machined in the course of this module. First the edge of the contour is to be roughed out. For this the instruction G00, G01, G02, G41 and G40 will be used.

Supplement the program commenced on page 2 in the editor, by the following blocks. Specify the contour in the missing blocks.

N140 T=„SF14“ ;Endmill 14 mm HSS N150 M6 N160 F280 S1400 M3 M8 D1 N170 G00 X-10 Y3 Z2 S N180 G01 Z-5 N190 G... N200 1 N210 2 N220 3 N230 4 N240 5 N250 6 N260 7 N270 8 N280 9 N290 10 N300 11 N310 12 N320 13 N330 14 N340 G... N350 G01 X-10 Y12 E N360 G00 Z150 N370 X150 Y150 M8

Solution see page 14 B557

Page 6


Section 2

Cutter radius compensation The activation of the cutting edge radius correction can be supported by means of the commands G247/G248 and G347/G348. By their use the contour can be approached along a circular arc. This is called a “soft approach” that prevents any contour damage at the point of contact.

Notes:

The function “soft approach and exit” is a tangential approach at the point of contact independently of the starting point. The function is used predominantly in conjunction with the tool radius correction, however, this is not compulsory. G247/G248 (Tangential approach/departure move with a quarter circle)

N40 G00 X=P0 Y=P0 N50 G41 G247 DISR=2 X=P1 Y=P1

N60 G01 X=P2 … N110 G01 X=Pn-1 Y=Pn-1 N120 G40 G248 DISR=2 X=Pn Y=Pn

Positioning for activation of the radius compensation Radius compensation activation. Approach with a quarter circle with radius 2 to position P1. The values for DISCL, FAD F have not been programmed. Machining the contour. Approach of the last contour point Radius compensation deactivation by leaving with a quarter circle of radius 2 to position P0/Pn

G347/G348 (Tangential approach/ departure move with a semi circle)

N40 G00 X=P0 Y=P0 N50 G41 G347 DISR=2 X=P1 Y=P1

N60 G01 X=P2 … N110 G01 X=Pn-1 Y=Pn-1 N120 G40 G348 DISR=2 X=Pn Y=Pn

Positioning for activation of the radius compensation Radius compensation activation. Approach with a half circle with radius 2 to position P1. The values for DISCL, FAD F have not been programmed. Machining the contour.. Approach of the last contour point Radius compensation deactivation by leaving with a quarter circle of radius 2 to position P0/Pn

DISR (Approach/departure radius) progr. contour

is the radius of the tool centre path. If the tool radius correction is activated, an arc is generated with a radius such that also in this case the tool centre path results with the programmed radius.


Page 7

B557

Section 2 Notes:

Cutter radius compensation Possible approach movements: G140

Approach and departure direction depending on the current correction side (basic position value)

G141

Approach from the left and departure to the left

G142

Approach from the right and departure to the right

G143

Approach and departure direction depends on the position of the starting and end point relative to the tangential direction

G147

Approach with a straight motion

P1 P3 at approaching/leaving with straight line (G147)

tool

G148

Departure with a straight motion

tool centre path P4

G247

Approach with a quarter circle

G248

Departure with a quarter circle

contour

DISR P0 P3 at approaching/leaving with quarter circle (G247) DISR

tool centre path tool P4

G347

Approach with a half circle

G348

Departure with a half circle

contour

P0 P3 at approaching/leaving with half circle (G347)

G340

Approach and leaving in space

DISR

tool centre path tool

G341

Approach and departure in a plane

Associated parameter values:

P4

contour

Approaching and leaving shown with interpoint „P4“ (with concurrent activation of the tool radius compensation

DISR

Approach and departure with straights (G147/G148). Distance of the cutter edge from the starting point on the contour. Approach and departure with arcs (G247, G347/G248, G348) Radius of the cutter centre path. Caution: In case of “REPOS” with a semi circle “DISR” states the circle diameter.

DISCL

DISCL=... Distance of the end point of the rapid approach motion from the machining plane. DISCL=AC (...) Statement of the absolute position of the end point of the rapid approach motion.

FAD

Speed of the slow feed motion. FAD=... the programmed value works according to the G-Code of group 15 (feed; G93, G94, etc.). FAD=PM (...) the programmed value is interpreted as a linear feed (like G 94) independent of the active G-Code of the group 15.

The soft approach and departure is very well explained in the module B558 “Program of subroutines”.

B557

Page 8


Section 3

Rounding and chamfering of edges For the machining of the finished contour the instructions RND, CHR, CHF are to be used for the radii and the chamfers.

Notes:

RND: At the programmed intersection between two straights a radius is added. The size of this is defined by RND=7.

CHF: At the programmed intersection between two straights a chamfer is added. The length of the chamfer is defined by CHF=9.

CHR: At the programmed intersection between two straights a chamfer is added. CHR=5 defines the length of the legs of this chamfer.

All not dimensioned radii and chamfers are 2 mm.


Page 9

B557

Section 3 Notes:

Rounding and chamfering of edges Describe the contour using the instructions referred to so far. A milling cutter with a diameter of 8mm is to be used (Name SF8). Start describing the contour at the point X13; Y5.


N380 N390 N400 N410 N420 N430 N440 N450 N460 N470

T=„SF8“ ;End mill 8 mm HSS M6 F280 S1400 M3 M8 D1 G00 X6 Y-7 G01 Z-5 G... G01 X13 y3 Y… G03 X… Y… I … J... G… Y… ...

N480 X… ... N490 Y... N500 G ... X… Y… I… J… N510 G… X… Y… ... N520 X… Y… ... N530 X… Y… ... N540 X… Y… … N550 Y… N560 G… X… Y… I… J… N570 G… X10 N580 G… N590 X… Y… N600 G … Z… M... N610 X150 Y150

Activation of the radius compensation Traverse close to the contour 1st contour point Milling the radius 8 mm Approach of top left contour point and rounding with 2 mm to the subsequent element Milling the contour corner at the chamfer 4 mm Approach of the stating point for the radius 20 mm Milling the radius 20 mm Approach of the starting point of the pocket and chamfer Approach of the top pocket corner and rounding 4 mm Approach of the bottom pocket corner and rounding 4 mm Approach end point of the pocket and chamfer Approach of starting point with radius7 mm Milling the radius 7 mm Leaving the contour Deactivation of the radius compensation Retraction of the cutter Retraction to the tool changing point, coolant OFF Traverse to the tool changing point


B557

Page 10


Section 4

Mixed incremental and absolute programming

Notes:

Angle ANG= If for a straight only one end point coordinate of the plane is known, or in the case of contours the final end point via several blocks, an angular statement can be used to completely define the straight path section. The angle is always referred to the abscissa of the current plane G17 to G19; e.g.: in case of G17 to the X-axis. Positive angles are taken to be anticlockwise.

20 Ordinate

15

23 G01 X15 G01 X20 ANG=-36 G01 X23 ANG=-72

Abscissa

Mixed programming: Absolute and incremental dimensions (G90/G91) you know already for the programming of contours. These two types can be programmed together in one block. For this the instructions “IC” (incremental) and “AC” (absolute) can be used. In this way “IC” can be used to program incremental dimensions within G90. The instruction G90 is modal. X=IC(10)

The cutter moves along the X-axis incrementally by 10 mm in the positive direction. Y=AC(12) The cutter will be positioned absolute along the Y-axis to the Coordinate of Y12 .

20 12

4 G91 G01 X=AC(12) Y=AC(25) G01 X4 Y=AC(22) G01 X=AC(20) Y-3

3

22 25

G90 G01 X12 Y25 G01 X=IC(4) Y22 G01 X20 Y=IC(-3)


Page 11

B557

Section 4 Notes:

Mixed incremental and absolute programming Describe the contour using the instructions referred to so far. A milling cutter with a diameter of 8 mm is to be used (Name SF8).

All radii R4

N620 G00 X17.5 Y60.5 Z2 N630 G... Z… M... N640 G... N650 N660 N670 N680 N690 N700 N710 N720 N730 N740 N750 N760 N770 N780 N790 N800 N810 N820

G01 X12 Y60.5 G01 Y... RND=... G01 X=IC(...) G01 X.. ANG=… G01 X... RND=... G01 X=...(10) RND=... G... G01 Y... RND=... G01 X=AC(...) CHR=... G01 Y=...(...) RND=... G01 X... RND=... G... G01 X... Y... G... G01 X17.5 Y60.5 G00 Z150 M9 G00 X... Y... M...

Positioning above the centre of left upper pocket Plunging into the pocket and coolant ON Activation of cutter radius compensation (climb milling) Approach of contour 1st corner point with rounding to the next element Approach of starting point for 55° chamfer Oblique 55° 2nd corner point with rounding to the next element 3rd corner point with rounding to the next element Switching to incremental dimensions 4th corner point with rounding to the next element 5th corner point with chamfering to the next element 6th corner point with rounding to the next element 7th corner point with rounding to the next element Switching to absolute dimensions Closing of contour Deactivation of cutter radius compensation Retraction of the cutter Leaving the contour and coolant OFF Traverse to tool changing position End of program


B557

Page 12


Section 5

Summary

Notes:

Path information/path commands Instruction

Meaning

G40 G41 G42

Cutter radius compensation deactivated * ** Cutter radius compensation to left of contour Cutter radius compensation to right of contour

CHR

Chamfering the contour corner by statement of leg length Chamfering the contour corner by statement of the length of chamfer Rounding the contour corner (radius statement) Straight with an angle

CHF RND ANG X=IC(…) Y=AC(…)

Statement of the coordinates with incremental dimensions Statement of the coordinates with absolute dimensions * **


Power-ON status of milling machines Power-ON status of turning machines

Page 13

B557

Section 6

Solution of the tasks

Notes: 6.1 Cutter radius compensation The path programmed with G01,G02 and G03 represents the path of the cutter centre. In this case the cutter radius must be taken into account by yourself. Exercise 1 Open the editor by pressing the following keys successively:

Write the following program header into the editor. Explain the blocks in the table. While doing this make yourself familiar with the editor. Mark the zero point on the drawing. N10 G54 G64 G17 SOFT

Zero point offset, continuous control ON, plane selection XY, soft control

N20 T1

Select tool Nr. 1 (PF60 with tool tips)

N30 M6

Load the selected tool

N40 S1000 F200 M3 M8 D1

Speed (rpm), feed (mm/min), rotation clockwise, coolant ON, activation of first cutting edge

N50 G00 X115 Y65 Z2

Approach of starting point and safety level (P1)

N60 G01 Z0

Infeed to command dimension

N70 X-35

Milling (P2)

N80 G00 Z2

Lift-off to safety level

N90 X115 Y15

Approach of starting point for 2nd pass (P3)

N100 G01 Z0

Infeed to command dimension

N110 X-35

Milling (P4)

N120 G00 Z150

Lift-off to tool changing level

N130 X150 Y150 M9 Approach tool changing position, coolant OFF

N70

N50

N110

N90

Motion at feed rate Motion with rapid traverse

B557

Page 14


Section 6

Solution of the tasks The work piece shown on the left is to be machined in the course of this module.

Notes:

First of all the edge of the contour is to be roughed out. For this the instruction G00, G01, G02, G41 and G40 will be used.

In the editor supplement the program commenced on page 2 by the following blocks. Specify the contour In the missing blocks.

N140 T=„SF14“ ;End mill 14 mm HSS N150 M6 N160 F280 S1400 M3 M8 D1 N170 G00 -10 Y3 Z2 N180 G01 Z-4 N190 G41 N200 G01 X4 Y10 N210 Y74 N220 G02 X6 Y76 I2 Y0 N230 G01 X68 N240 Y63.5 N250 X76 Y50 N260 Y42 N270 X64 N280 Y26 N290 X76 N300 Y12 N310 X68 Y4 N320 X12 N330 X0 Y16 N340 G40 N350 G01 X-10 Y12 N360 G00 Z150 N370 X150 Y150 M8


S

1 2 3 4 5 6 7 8 9 10 11 12 13 14 E

Page 15

B557

Section 6 Notes:

Solution of the tasks 6.2 Rounding and chamfering of edges Describe the contour using the instructions referred to so far. A milling cutter with a diameter of 8 mm is to be used (Name SF8). Start describing the contour at the point X13; Y5.


N380 N390 N400 N410 N420 N430 N440 N450 N460 N470

T=„SF8“ ;End mill 8 mm HSS M6 F280 S1400 M3 M8 D1 G00 X6 Y-7 Z2 G01 Z-5 G41 G01 X13 Y3 Y5 G03 X5 Y13 I–8 J0 G01 Y75 RND=2

N480 X67 CHF=4 N490 Y65 N500 G03 X75 Y49 I20 J0 N510 G01 X75 Y43 CHR=1.5 N520 X61 Y43 RND=4 N530 X61 Y25 RND=4 N540 X75 Y25 CHR=1.5 N550 Y12 N560 G03 X68 Y5 I0 J-7 N570 G01 X10 N580 G40 N590 X6 Y-7 N600 G00 Z150 M9 N610 X150 Y150 N620 M30

B557

Page 16

Start point Infeed to depth Activation of radius compensation Approach the contour 1st contour point Milling of radius 8 Approach upper left contour point and rounding 2 mm to the next element Milling of corner of contour at chamfer 4 mm Approach starting point for the radius 20 mm Milling of radius 20 mm Approach of starting point of pocket and chamfering Approach upper corner of pocket and rounding 4 mm Approach lower corner of pocket and rounding 4 mm Approach end point of pocket and chamfering Approach starting point of radius 7mm Milling of radius 7 mm Leaving the contour Deactivation of radius compensation Retraction of cutter Retraction to tool changing level, coolant OFF Traverse to tool changing position


Section 6

Solution of the tasks 6.3 Mixed incremental and absolute programming

Notes:

Describe the contour using the instructions referred to so far. A milling cutter with a diameter of 8mm is to be used (Name SF8). Start describing the contour at the point X13; Y5.

All radii R4

N620 G00 X17.5 Y60.5 Z2 N630 G01 Z-3 M8 N640 G41 N650 N660 N670 N680 N690 N700 N710 N720 N730 N740 N750 N760 N770 N780 N790 N800 N810 N820

G01 X12 Y60.5 G01 Y52 RND=4 G01 X=IC(7.8) G01 X23.8 ang=-55 G01 Y41 RND=4 G01 X=IC(10) RND=4 G91 G01 Y18 RND=4 G01 X=AC(23) CHR=1.5 G01 Y=AC(69) RND=4 G01 X-11 RND=4 G90 G01 X12 Y60.5 G40 G01 X17.5 Y60.5 G00 Z150 M9 G00 X150 Y150 M30


Positioning above the centre of left upper pocket Plunging into the pocket and coolant ON Activation of Cutter radius compensation (climb milling) Approach of the contour 1st corner point with rounding to the next element Approach of starting point for 55° chamfer Oblique 55° 2nd corner point with rounding to the next element 3rd corner point with rounding to the next element Switching to incremental dimensions 4th corner point with rounding to the next element 5th corner point with chamfering to the next element 6th corner point with rounding to the next element 7th corner point with rounding to the next element Switching to absolute dimensions Closing the contour Deactivation of Cutter radius compensation Retraction of the cutter Leaving the contour Traverse to tool changing position End of program

Page 17

B557

Section End Notes:

B557

Page 18


B558

1

Program of subroutines

Brief description

Objective of the module: In this module you will get to know the use of subroutines. You will learn to write subroutines for contours with soft contour approach and departure with cutter radius compensation and how to call them up in a simple milling program. Description of the module: This module explains the programming with subroutines. The soft approach and departure of the contour will be used for contour machining. Content: The use and necessity of sub-routines Call-up of subroutines Programming of subroutines Summary Solution for the programming of subroutines


Page 1


B558

B558

B558

Page 2


B558 Program of subroutines: Description

Program of subroutines: START

This module explains the programming with subroutines. The soft approach and departure of the contour will be used for contour machining.

The use and necessity of sub-routines

Call-up of subroutines

Programming of subroutines

Summary

Solution for the programming of subroutines

Program of subroutines: END

Notes :


Page 3

B558

Section 2 Notes:

The use and necessity of subroutines If contours are programmed that are used repeatedly, it is possible to do this using subroutines. There is a differentiation between local subroutines, which belong to a work piece and global sub-routines, which are generally usable. Subroutines have the file extension *.SPF (Subprogram File).

2.1 Global subroutines These subroutines can be used for all kinds of workpiece programs; they must be written keeping in mind the danger of possible collisions. Both programs using incremental or absolute dimensions can be used. Example: The machine table is to be positioned at a certain location for tool changing after the machining has been completed. The coordinates can therefore be stated with absolute values. In order to avoid collisions, Z must be positioned first followed by X/Y.

2.2 Local subroutines Local subroutines are often used where contours are repeated on the same work piece. If, for instance, a pocket is to be milled several times on one workpiece, it can be programmed just once and then repeated several times. Since the absolute dimension vary, the pocket must be programmed from a defined starting point, which is then approached in the main program. From there the pocket is then described with incremental dimensions. Example: The contour of a pocket must be milled at 2 different locations. Fill in the following program header into the editor. Explain the sentences in the table. By the way make yourself familiar with the editor. Mark the zero point in the drawing.

B558

Page 4


Section 3

Call-up of subroutines The choice of the type of dimensions depends largely on the usage of the subroutine. When programming the following principle must be kept in mind: When exit the subroutine, the status that existed before the call-up must be re-established.

Notes:

The subroutine is called up by its name and the number of times it is to be used. The number of repeats is programmed with the address “P”. At the end there must follow the instruction “M17” (end of subroutine). After this the control jumps back to the calling-up place in the main program and continues with the next block. Main program

Subroutine (contour)

Explanation

N40

G90 G00 X20 Y20 Z2

Approach of the starting point

N50

Contour P1

Call-up of the subroutine Contour for 1 pass

N10 G91

Switching to incremental dimensions

N20 G01 Z-5

Plunging into the contour to Z–3

N30 X10

Motion by 10 mm along X-axis in +direction

N40 Y-10

Motion by 10 mm along Y-axis in -direction

N50 X-10

Motion by 10 mm along x-axis in -direction

N60 Y10

Motion by 10 mm along Y-axis in +direction

N70 G90

Re-establish status of main program

N80 M17

End of subroutine

N60

G01 Z2

Retraction to safety level

N70

G00 X50 Y20 Z2

Approach of next starting point

N80

Contour P2

Call-up of the local subroutine contour for 2 passes Milling of the pocket to –8

N90

Retraction to safety level

G01 Z2

Call-up of the global subroutine Workpiece change

N100 Workpiece change P1

N110 M30


G53 G00 z200

Zero point offset block-by-block OFF and retraction in Z-direction

G53 x200 y200

Zero point offset block-by-block OFF and retraction in X/Y direction

M17

End of subroutine End of main program

Page 5

B558

Section 4 Notes:

Programming of subroutines Below, you are asked to program the pocket as a subroutine (Name:UP_MODUL31). The subroutine is to be called up from the main program (Name: MODUL31).

Task 1: The workpiece has already been programmed in the program “MODUL30.MPF”. This is now to be copied, renamed in “MODUL31.MPF” and then modified. Change to the “Program Manager”. Open the program directory and select the program MODUL30.MPF. By pressing the “PROGRAM MANAGER” button on the keyboard change to the “Program Manager” screen.

In the workpiece directory select the program MODUL30.MPF with the blue cursor keys.

Copy the file by pressing the VSK 5 “COPY”.

The program acknowledges the selection and copying in the status line.

With the now active VSK 6 “PASTE” insert the file into the directory-tree.

The “Paste” window opens. Rename the file in MODUL31.MPF and accept with the VSK 8 “OK”.

B558

Page 6


Section 4

Programming of subroutines Task 2: Commence a new subroutine by the name of “UP_MODUL31.SPF” and programme the following program lines with the respective supplements. The program starts at the centre cross.

N10 G… N20 G… G… DISR=… X5 N30 N40 N50 N60 N70 N80 N90 N100 N110 N120 N130 G… G… DISR=… X-5 N140 G… N150 M…

Notes:

Switching to incremental dimensions Activate cutter radius compensation for climb milling with soft approach in a quarter circle r = 0.5

Contour description using climb milling

Deactivate cutter radius compensation with soft departure the contour in a quarter circle r = 0.5 Switching to absolute dimension programming End of subroutine

Task 3:

For solution see page 10

In the main program “MODUL31.MPF” delete all lines starting with block N620. Open program MODUL31.MPF and set the cursor on N620.


Mark and delete the selected fields.

Page 7

B558

Section 4 Notes:

Programming of subroutines Task 4: Alter the main program “MODUL31.MPF” such that the internal contours are machined using the subroutine. When positioning in the Z-axis care must be taken to consider the infeed amount (Z-4) per subroutine pass.

…. N610 X150 Y150 N620 G… X… Y… Z… M… With rapid traverse to the start-point of the upper left contour and coolant ON N630 …………….. P… Call-up of subroutine for one pass N640 G01 Z1 Retraction from the pocket at feed rate N650 G... X… Y… Z… With rapid traverse to the start-point of the upper right contour N660 …………….. P... Call-up of subroutine for two passes N670 G… Z… Retraction from the pocket at feed rate N680 G… Z… M... Departure in Z to the tool changing point and coolant OFF N690 G… X… Y… Departure in X and Y to the tool changing point N700 M… End of main program

For solution see page 11

B558

Page 8


Section 5

Summary Path information/Approach and Departure commands Instruction

Meaning

UP_... P1

Subroutine call-up with number of repeats

M17

End of subroutine

G147

Approach with a straight

G148

Departure with a straight

G247

Approach with a quarter circle

G248

Departure with a quarter circle

G347

Approach with a semi-circle

G348

Departure with semi-circle

G340

Approach and departure in space

G341

Approach and departure in a plane

Parameter

Explanation

DISR

Radius of the tool centre path for approach and departure

DISCL

DISCL=... Distance of the end point for the rapid infeed motion

FAD

Speed of the slow infeed motion


Page 9

Notes:

B558

Section 6 Notes:

Solution for the programming of subroutines Solution for Task 2:

N10 G91 N20 G41 G247 DISR=0.5 x5

Switching to incremental dimensions Activate cutter radius compensation for climb milling with soft approach in a quarter circle r=0.5

N30 G01 Y9 RND=4 N40 X-10.8 CHF=2.12 N50 Y10 RND=4 N60 X-11 RND=4 N70 Y-17 RND=4 Contour description using climb milling N80 x7.8 N90 Y-5.71 ANG=-55 N100 Y-5.287 RND=4 N110 X10 RND=4 N120 Y9 N130 G40 G248 DISR=0.5 X-5 Deactivate cutter radius compensation and soft departure of the contour in a quarter circle r = 0.5 N140 G90 Switching to absolute dimension programming N150 M17 End of subroutine

Solution for Task 3: Open the program MODUL31.MPF and set cursor on N620 by navigating with the blue cursor keys on the keyboard.

B558

Page 10

Press the VSK 4 “Mark” to select the desired lines. Move the cursor with the “cursor-down” key until all lines are marked. Then press the VSK 7 “Cut” to delete all marked entries.


Solution for programming of subroutines

Notes:

Solution for Task 4:

…. N610 X150 Y150 N620 G00 X28.8 Y50 Z1 M8 N630 UP_Modul31 P1 N640 G01 Z1 N650 G00 X53.6 Y50 Z3 N660 UP_MODUL31 P2 N670 G01 Z2 N680 G00 Z150 M9 N690 G00 X150 Y150 N700 M30

Section 6

With rapid traverse to the start-point of the upper left contour and coolant ON Call-up of subroutine for one pass Retraction from the pocket at feed rate With rapid traverse to the start-point of the upper right contour Call-up of subroutine for two passes Retraction from the pocket at feed rate Departure in Z to the tool changing point and coolant OFF Departure in X and Y to the tool changing point End of main program


Page 11

B558

Section End Notes:

B558

Page 12


B559

1

Loops, jumps, repetitions

Brief description

Objective of the module: Working through this module you become familiar with the usage of loops, jumps and repetitions in a milling program. Description of the module: In the module you will learn about the commands for looping parts of the program, for jumping to certain blocks in the program and how to repeat certain sections of the program. Content: Label name, Parameter usage Jump instructions, Program section repetitions Example and tasks Summary Solution of the tasks


Page 1


B559

B559

B559

Page 2


B559 Loops, jumps, repetitions: Description

Loops, jumps, repetitions: START

In the module you will learn about the commands for looping parts of the program, for jumping to certain blocks in the program and how to repeat certain sections of the program.

Label name, Parameter usage

Jump instructions, Program section repetitions

Example and tasks

Summary

Solution of the tasks

Loops, jumps, repetitions: END

Notes :


Page 3

B559

Section 2 Notes:

Label name, Parameter usage 2.1 Label name In order to repeat certain sections of a program or the jump to a certain section of the program, we make use of “LABELS” to mark the beginning/ end of certain sections of the program. In most cases a “LABEL” is used to mark the beginning, but when you want to perform repetions of sections of a program, then you require both beginning and end “LABELS” (refer to section 3.2 in this module). The “LABEL” must consist of at least two or a maximum of 8 characters. The first two characters must always be letters or underlines. The “LABEL” must always be followed by a colon. Assigning the name BL123 to a label

N100... N110 BL123: N120 G00 X10..

2.2 Parameter usage In some cases the use of parameters is highly advisable. For instance, the cutting values for the tools to be used can be assigned to parameters in the program header, which can then be used for programming instead of the cutting values themselves. The parameters are programmed with the address letter “R” and a number “R1”. Values can be assigned to these in the section “Parameter” or also in the program itself. ;T1-WSF Dr60 R1=200 ; n for WSF Dr60 Program header R2=30 ; vf for WSF Dr60 ... N100 T1 ; WSF Dr60 N110 M6 N120 S=R1 F=R2 M3 M8 D1 Assignment of speed and feed by means of N130 ... R1 and R2 Parameters can be used within the program for calculation of individual values or for themselves. For reason of the advance calculation by the control unit it is possible that undesirable effects on the active parameters might occur. This can be prevented by using the instruction STOPRE. The next block will only be executed after the previous block has been finished. For this “STOPRE” must be written in a block by itself. N10 R1=0 ... N110 BL123: N120 G00 x10.. … N140 STOPRE N150 R1=R1+1 N160 EL123:STOPRE

B559

Page 4

The control unit waits until block N130 has been completed. Each time the block is run for machining R1 is increased by 1. 828D/840Dsl SINUMERIK Operate

Jump instructions, Program section repetitions

Section 3 Notes:

3.1 Jump instructions Jump instructions can also be used within a program. They permit the omission of certain sections of the program or to jump back for repetitions. The instruction GOTOF is used to jump forward, while the GOTOB is used to jump backward. For this a search is carried out for the included label name or the block number before the jump to this location is carried out. ;T1—WSF Dr60 R1=200 ; n for WSF Dr60 R2=30 ; vf for WSF Dr60 N10 GOTOF N100 N20 LB001: … N90 GOTOF N170 N100 T1 ; WSF Dr60 N110 m6 N120 S=R1 F=R2 M3 M8 D1 N130 … ... N160 GOTOB LB001 N170 T4

Jump to block N100

Jump to block N100

Jump back to label LB001

The jump instruction caused a change in the machining sequence.

3.2 Program section repetitions Program sections between two labels can be repeated any number of times as specified under the address P. For this the program jumps to the first stated label and executes all blocks of the program until the second label is reached. If the number of repetitions is greater than one, this procedure will be repeated as often as stated under address “P”.

1 2

;T1-WSF Dr60 R1=200 ; n for WSF Dr60 R2=30 ; vf for WSF Dr60 N10 T1 ; WSF Dr60 N20 M6 N30 S=R1 F=R2 M3 M8 D1 N40 G00 z2 N50 LB001: N50 G1 Z=IC(-10) … N90 LE001: ... N160 Repeat LB001 LE001 P2 N170 T4


Jump back to Label LB001 and two repetitions between LB001and LE001

Page 5

B559

Section 4 Notes:

Example and tasks 2 Holes are to be drilled into the milled work piece. These holes are to be programmed using jumps and parameters.

Task 1: Copy the program file “MODUL31.MPF” in “Program Manager”. Rename this program to “MODUL32.MPF”. For explanations see Module “B558 Subprogram techniques”. Task 2: Open the program “MODUL32.MPF” and supplement the program by the following lines for the drilling. …. N690 G00 X150 Y150 N700 R1=... R2=...

B559

N710 T=„NC-centre drill“ N720 M6 N730 R1=… R2=... N740 S1000 F=... M3 M8 D1 N750 Repeat ... ... P1 N760 T=„SPB8“ N770 … N775 … N780 ...=8+(8*1/3) ...=50 N790 S800 F=R2 M3 M8 D1 N800 R...=8+(8*1/3) N810 ... LB001 LE001 p1 N820 G00 Z150 N830 X150 Y150 N840 M30

Traverse to the tool changing point in x and y Set the parameter R1 (drilling and counter depth) and R2 (feed rate) to zero Request NC-centre drill Ø larger 12 mm (for simulation SF10) Load NC-centre drill Specify depth for centring and feed rate Specify technology data for centring Execute program between the Labels LB001 and LE001 once Request drill diameter 8 mm (for simulation SF8) Load drill Advance evaluation Stop Specify depth for centring and countering in R1 and feed rate in R2 Specify technology data for the drill Specify depth for drilling (1/3 drill point) Execute the program between the Labels once Retraction in Z-direction Retraction in X- and Y-direction End of program

N850 … N860 G... X... Y... Z... N870 GOTOF ... N880 LB002: N890 G... X... Y... Z... N900 Repeat N... N… N910 …

Give the label the name “LB001“ Traverse to 1st drilling position Jump to block N920 Give the label the name “LB002” Traverse to 2nd drilling position Execute blocks N920 to N940 Give the label the name “LE001”

N920 G01 Z=... F=... N930 G04 S2 N940 G01 Z... F=... N950 ... …

Drill at feed rate Dwell after reaching the drilling depth for smoothing With double the feed rate move to z2 Jump back to Label LB002

Page 6


Section 5

Summary

Notes:

Loops/ jumps/repetitions Instruction

Meaning

GOTOF

Forward jump to destination mark GOTOF LB001 or GOTOF N110

GOTOB

Backward jump to destination mark GOTOB LB002 or GOTOB N10 Note: When using “GOTOB” and “GOTOF” care must be taken against endless loops. They call up each other repeatedly. Hence the program cannot leave this range. The use of block numbers as destination mark is not advisable. If the block number changes, there will be no automatic correction.

REPEAT

Repeats the section between the labels for the programmed number of times. Repeat LB002 LE002 P2 Note: The use of block numbers as destination mark is not advisable. if the block number changes, there will be no automatic correction.

R...

Parameter 1-99 R1

STOPRE

The next block will not be decoded until the previous block has been completed.

….:

Label name LB001: Note: Label names must have at least 2 and a maximum of 8 characters. The first 2 of which must be either letters or underlines.

G04

Dwell G04 S2 Dwell for 2 revolutions G04 F2 Dwell for 2 seconds


Page 7

B559

Section 6 Notes:

Solution of the tasks Solution for task 2:

…. N690 G00 X150 Y150 N700 R1=0 R2=0

Traverse to the tool changing point in X and Y Set the parameter R1 (drilling and counter depth) and R2 (feed rate) to zero N710 T=„NC-centre drill“ Request NC-centre drill Ø larger 12 mm (for simulation SF10) N720 M6 Load NC-centre drill N730 R1=-5 R2=100 Specify depth for centring and feed rate N740 S1000 F=R2 M3 M8 D1 Specify technology data for centring N750 Repeat LB001 LE001 P1 Execute program between the Labels LB001 and LE001 once N760 T=„SPB8“ Request drill diameter 8 mm (for simulation SF8) N770 M6 Load drill N775 STOPRE Advance evaluation Stop N780 R1=8+(8*1/3) R2=50 Specify depth for centring and countering in R1 and feed rate in R2 N790 S800 F=R2 M3 M8 D1 Specify technology data for the drill N800 R1=8+(8*1/3) Specify depth for drilling (1/3 drill point) N810 Repeat LB001 LE001 P1 Execute the program between the labels once N820 G00 Z150 Retraction in Z-direction N830 X150 Y150 Retraction in X- and Y-direction N840 M30 End of program

B559

N850 LB001: N860 G00 X25 Y25 Z2 N870 GOTOF N920 N880 LB002: N890 G00 X50 Y25 Z2 N900 Repeat N920 N940 N910 LE001:

Label name “LB001” Traverse to 1st drilling position Jump to block N920 Label name “LB002” Traverse to 2nd drilling position Execute blocks N920 to N940 Label name LE001

N920 G01 Z=R1 F=R2 N930 G04 S2 N940 G01 Z2 F=R2*2 N950 GOTOB LB002

Drill at feed rate Dwell after reaching the drilling depth for smoothing With double the feed rate move to Z2 Jump back to Label LB002

Page 8


B560

1

Mirror, offset, rotate, scale

Brief description

Objective of the module: With help of this module you will get to know commands for mirroring, shifting, rotating and scaling of contours. Description of the module: This module explains the use of the commands for the machining of identical contour elements in various positions. Content: Shifting Rotating Mirroring Scaling Summary Solutions


Page 1


B560

B560

B560

Page 2


B560 Mirror, offset, rotate, scale: Description This module explains the use of the commands for the machining of identical contour elements in various positions.

Mirror, offset, rotate, scale: START

Shifting

Rotating

Mirroring

Scaling

Summary

Solutions

Mirror, offset, rotate, scale: END

Notes :


Page 3

B560

Section 2 Notes:

Shifting General introduction The commands in this module are known as frames (calculation instructions). They can influence, cancel or condition each other. In our example a known contour, which is described in a subprogram, is to be milled in various positions and sizes. For this the zero point at the starting point of the contour of the subprogram must be rotated. In order to be able to rotate the program about the starting point of the sub-program, this point must be the zero point. Our work piece zero point (G54) lies in the middle of the work piece.

“TRANS”, “ATRANS” The zero point can be shifted in the programmed axes by means of these commands. The command “TRANS” clears all active frames. “ATRANS” (additive shift) works incremental from the active frames.

Workpiece 1

Workpiece 2

ATRANS x30

ATRANS x30 TRANS x60

Workpiece 3

Workpiece 4

ATRANS x30

0 For instance in case of multiple settings of work pieces the zero point can be shifted and the main program repeatedly executed .

B560

Page 4


Section 2

Shifting In the following example the zero point is to be transformed to the starting point of the left hand contour.

Notes:

Task 1: Create a new file with the name MODUL34.MPF!

Task 2: Programme the tool path for face milling the surface. Take into account that the zero point lies in the middle. The Face mill (FACE_MILL_D60) has a diameter of 60 mm, the work piece measures 80 x 80 mm.

N10 G54 G64 G17 SOFT N20 T=…. N30 M…. N40 S1000 F200 M3 M8 D1 N50 G00 X.... Y…. Z…. N60 G01 Z0 N70 X-80 N80 G00 Z2 N90 X80 Y-20 N100 G01 Z0 N110 X-80 N120 G00 Z150 N130 X150 Y150 M9

Task 3: Load a milling cutter “CUTTER_8”, shift the zero point to the starting point of the contour and position the tool at this location. N140 T=.... N150 ... N160 S2000 F100 M3 M8 D1 N170 …. X…. Y…. N180 G00 X... Y... Z...

Call up the tool Tool change Technology data for the tool Shift the zero point additively Position the tool

Solution see page 11 828D/840Dsl SINUMERIK Operate

Page 5

B560

Section 3 Notes:

Rotating “ROT”, “AROT” The coordinate system can be rotated by means of the command “ROT” or “AROT”. The counter-clockwise rotation is taken to be positive. The positive X-axis represents the zero-degree position. There are two ways of programming.

AROT Z=90

X+

+

Y+

Y+

+

Variant 1 Rotation about an axis AROT X.. Y.. Z..

X+

Y+

+

Variant 2 Rotation of the active plane AROT RPL...

X+

The zero point has been rotated by 90° about the Z-axis.

AROT RPL=90

+

Y+ X+ The active plane has been rotated by 90° about the Z-axis. The command “ROT” resets the coordinate system and all other active frames back to the original status.

Task 4: Rotate the coordinate system by the required amount about the now valid zero point. Now plunge into the work piece with the milling cutter at a feed rate of 3 mm. Thereafter start the subprogram. Deactivate all frames. N190… … N200 G… Z... N210……. N220 G00 Z2 N230….

Rotate the coordinate system Plunge into the contour Call up subprogram UP_MODUL31 Retract to 2 mm above the work piece Deactivate all frames

Solution see page 12 B560

Page 6


Section 4

Mirroring

Notes:

“MIRROR”, “AMIRROR” With the command “MIRROR” or “AMIRROR” the coordinate system can be mirrored about the programmed axis or axes. In such a case the programmed coordinates are mirrored about the axis or axes by their sign. Variant 1 Mirroring an axis Y+

Y+

AMIRROR X0 X+

X+

Variant 2 Mirroring several axes

X+ X+

Y+

Y+

MIRROR X0 Y0

The command “MIRROR” resets the coordinate system and all other active frames back to the original status.

Task 5: Mirror the work piece about the X-axis. Shift the zero point to the starting point of the contour and there rotate the coordinate system. Take into account the position of the positive X-axis. N240 ….. X… N250 A…. X... Y... N260 G00 X... Y... Z2 N270 … ...

Mirroring the X-axis Shifting to the starting point of the contour Position the tool Rotate coordinate system additively


Page 7

B560

Section 5

Scaling

Notes:

“SCALE”, “ASCALE” In some cases the scaling of contour elements is quite sensible. The existing contours can be scaled up or down by a given factor. The factor is defined following the command Scale for each individual axis.

SCALE y2

ASCALE y2

SCALE x2

SCALE x2 y2

ASCALE x2

SCALE

When programming with “ASCALE” the calculations are always referred to the presently valid coordinate system. With the command “SCALE” the values of the active zero point offset are taken as a basis. All presently active transformations (frames) like offset, mirror, scale are cancelled. If no value follows the command “SCALE” all frames are cancelled. The same applies to the command “M30”.

The value programmed under “SCALE” represents a factor. If this is >1 an enlargement takes place, in case of values <1 diminished. Care must be taken that radii are also affected. This can possibly lead to errors. Variant 1 ........Scaling of an axis

ASCALE X1.5

All X-values are multiplied by 1.5 Variant 2 .......Scaling of several axes

ASCALE X=1x1.5 Y=1x1.5 The scaling factor can also be calculated in the program by entering the formula.

B560

Page 8


Section 5

Scaling

Notes:

Task 6: Scale the X- and Y-axis. Let the control unit calculate the respective factor. Plunge into the work piece by 3 mm and cal up the subprogram UP_MODUL31. Traverse to the tool changing point. Terminate the main program. The scaling factor (Sf) is calculated from the formula: Sf 

Dimension of command geometry 32.55   1,1625 Dimension of actual geometry 28

N280 ... X=…/21.8 Y=32.55/.. N290 G... Z-3 N300 ….. N310 G... Z200 N320 X150 Y150 M9 N330 M...

Scale additively the X- and Y-axis Plunge into the contour. Call the subprogram Retraction in Z Traverse to tool changing position End of program

Solution see page 13 Task 7: Fill in the missing values for the blank piece and start a simulation.

……... ……...

……... ……...


Page 9

B560

Section 6 Notes:

B560

Summary of the instructions Frame - Concept (Calculation instructions) TRANS X... Y... Z...

Absolute programmable zero point offset as referred to the presently valid, with G54 to G57 and G505 to G599 selected work piece zero point

ATRANS X... Y... Z...

Additive programmable zero point offset as referred to the presently valid, selected or programmed zero point

X..... Y..... Z.....

Shift value in direction of the stated axis

TRANS

Deactivation of programmable zero point offsets, previously programmed frames are cleared

ROT X.. Y.. Z.. RPL=..

Absolute programmable rotation as referred to the presently valid, with G54 to G57 and G505 to G599 selected work piece zero point

AROT X.. Y.. Z.. RPL=..

Additive programmable rotation as referred to the presently valid, selected or programmed zero point

X..... Y..... Z.....

Rotation angle in space: - Geometry axis that is being rotated

RPL= .....

Rotation angle in a plane: - angle by which the coordinate system Is rotated - (plane previously selected with G17 to G19)

ROT

Deactivation of programmable rotation, previously programmed frames are cleared

SCALE X... Y... Z...

Absolute programmable enlarging or diminishing (scaling), as referred to the presently valid, with G54 to G57 and G505 to G599 selected work piece zero point

ASCALE X... Y... Z...

Additive programmable enlarging or diminishing (scaling) as referred to the presently valid, selected or programmed zero point

X..... Y..... Z.....

Scaling factor (smaller / greater 1) in direction of stated axis

SCALE

Deactivation of programmable enlarging or diminishing, previously programmed frames are cleared

MIRROR X... Y... Z...

Absolute programmable mirroring as referred to the presently valid, with G54 to G57 and G505 to G599 selected work piece zero point

AMIRROR X...Y...Z...

Additive programmable mirroring as referred to the presently valid, selected or programmed zero point

X..... Y..... Z.....

Coordinate axis, in which the signs are changed, (the value for X/Y or Z can be freely selected - e. g. X0/Y0/Z0)

MIRROR

Deactivation of programmable mirroring, previously programmed frames are cleared

Page 10


Section 7

Solutions

Notes:

7.1 Solution for “Shifting”

Solution for task 2: N10 G54 G64 G17 Soft N20 T="FACING_TOOL_D60" N30 M6 N40 S1000 F200 M3 M8 D1 N50 G00 X80 Y20 Z2 N60 G01 Z0 N70 X-80 N80 G00 Z2 N90 X80 Y-20 N100 G01 Z0 N110 X-80 N120 G00 Z150 N130 X150 Y150 M9

Solution for task 3: N140 T="CUTTER_8" N150 M6 N160 S2000 F100 M3 M8 D1 N170 ATRANS X-16.02 Y-10.02 N180 G00 X0 Y0 Z2


Call up the tool Tool change Technology data for the tool Shift the zero point additively Position the tool

Page 11

B560

Section 7 Notes:

Solutions 7.2 Solution for “Rotating” Solution for task 4: N190 AROT Z-20 or (AROT RPL-20) N200 G01 Z-3 N210 UP_MODUL31 N220 G00 Z2 N230 TRANS or (ROT)

Rotate the coordinate system Plunge into the contour Call up subprogram UP_MODUL31 Retraction to 2 mm above the work piece Deactivate all frames

7.3 Solution for “Mirroring” Solution for task 5: N240 AMIRROR X0 N250 ATRANS X-16.02 Y-10.02 N260 G00 X0 Y0 Z2 N270 AROT Z-20 or RPL=-20

B560

Page 12

Mirroring the X-axis Shifting to starting point of the contour Position the tool Rotate coordinate system additively


Section 7

Solutions

Notes:

7.4 Solution “Scaling” Solution for task 6: The scaling factor (Sf) is calculated from the formula:

Sf 

Dimension of command geometry 32.55   1,1625 Dimension of actual geometry 28

N280 ASCALE X=26.35/21.8 Y=32.55/28 N290 G01 Z-3 N300 UP_MODUL31 N310 G00 Z200 N320 X150 Y150 M9 N330 M30

Scale additively the X/Y axis Plunge into the contour. Call-up of subprogram Retraction in Z Traverse to tool change pos. End of program

Solution for task 7: “Fill in the missing values and start a simulation”. In the program editor press the HSK 7 „Simulation“. The simulation window opens. Press the VSK 1.8 to extend the vertical softkey bar and press the VSK 2.5 “Blank“. The “Blank input” window with the following input mask opens. Insert the values like shown below.

Accept the values by pressing the VSK 8 “Accept”. Jump back to the VSK 1 by pressing the VSK 2.8. Press the VSK 1.1 and start the simulation run.


Page 13

B560

Section 7 Notes:

B560

Solutions The simulation run starts and ends (see picture below).

Page 14


B565

1

Basics

Brief description

Objective of the module In this module you learn about the functions of the different components of a machine tool and how they work together. Description of the module: In this module you get to know the basic concepts and basic logic functions of the control unit, the possibility of extending the peripherals and common abbreviations. Content: Types of machine tools Advantages of the CNC controlled machine tool Basic concepts - basic logic functions Sample configurations of the Sinumerik Operate Drive system - example Machining centre Shortcuts and abbreviations


Page 1


B565

B565

B565

Page 2


B565 Basics: Description In this module you get to know the basic concepts and basic logic functions of the control unit, the possibility of extending the peripherals and common abbreviations.

Basics: START

Types of machine tools

Advantages of the CNC controlled machine tool

Basic concepts - basic logic functions

Sample configurations of the Sinumerik Operate

Drive system example Machining centre

Shortcuts and abbreviations

Basics: END

Notes :


Page 3

B565

Section 2 Notes:

Types of machine tools 2.1 The conventional machine tool

2.2 The CNC controlled machine tool

B565

Page 4


Advantages of the CNC controlled machine tool

Section 3 Notes:

 Low waste costs  Low control costs  Smaller optimal batch sizes  Shorter cycle times  Multi-shift work  Multi-machine operation  Higher efficiency  Increase of the manufacturing capacity  Rationalisation of the organisation  Shortening of the delivery time  Reduction of the set-up time  Repetition accuracy does not depend on the operator

The CNC technology should not replace the worker or put more load on him, rather it shall:  efficiently use the machine and the cutting tools  shorten the ancillary time and waiting period  produce better quality much faster.  cover the constantly rising demand  make detailed changes faster  insure the competitiveness of the company on the market


Page 5

B565

Section 4 Notes:

Basic concepts - basic logic functions 4.1 Definition of main components: NC

–

CNC – DNC – PLC –

Numerical Control control in numerical form Computerized Numerical Control, numerical control with one or several microcomputer Direct Numerical Control, one or several CNC‘ s receive their part programs from a central computer over a cable or network. Programmable Logic Controller, a programmable logic circuit. is used in the machine tools for adjusting the control.

4.2 CNC basic functions:  A big colour monitor for the display, programming, simulation, operation and diagnosis.  Operation with interactive dialogue with at least two switchable foreign language options.  A bus-linked-, or integrated PLC to control the switching functions.  Software end switches as a substitution of mechanical end-switches.  Operational-/machine data logging, e.g. temperature error compensation, variable space encoding of the tools, tool failure– and service life monitoring  Additional functions:  Axis block  Powered tools  Data interface  Manual input  Correction values  Position set  Program test  Block masking/block search  Re-approaching the contour

B565

Page 6


Section 5

Sample configurations of the Sinumerik Operate The following two graphics show sample configurations of the Sinumerik Operate, their optional components an their communication paths.

Notes:

Sample configuration of the SINUMERIK 840D sl:

Sample configuration of the SINUMERIK 828D: Factory network (Industrial Ethernet)

2 x Handwheels

PLC E/A-Interface based upon PROFINET

Synchronos motor 3

Synchronos motor 2 Asynchronos motor

Synchronos motor 1


Page 7

B565

Section 6 Notes:

Driving mechanisms/positioning actions A typical machining center with feed drives, main spindle drive and auxiliary drive is shown below.

Feed drives

Auxiliary drive

Main spindle drive

According to the drive tasks planed, controlled electrical drives for NCmachines are divided into the following:  Feed drives for all axis, e.g. X, Y, Z.  Main spindle drive, e.g. for the milling spindle of a machining centre, the spindle drive of turning machines or a grinding wheel drive.  Auxiliary drive, e.g. for the tool changer, the circular table or the pallet switcher. Operation diagram of the position-regulated axis:

B565

Page 8


Section 7

Shortcuts and abbreviations ASCII AS AT BA BCD BCS CAD COM COR CNC CPU CRC CUTOM DAC DB DBB DBW DBX DDE DIR DOS DTE DRV EMC ENC EPROM ESD FC FDD FPU FST GIA GUD HD HHU HMI IM IM-Adress INC INI I/O ISA JOG K-Bus LED LF MB MD MCP MCS MCU MDA

American Standard Code for Information Interchange Automation System Advanced Technology Mode of Operation Binary Code Decimals Basic Coordinate System Computer Aided Design Communication Module Coordinate Rotation Computerized Numerical Control Central Processing Unit Cutter Radius Compensation Cutter Radius Compensation (Tool Radius Comp) Digital Analogue Converter Data Block in the PLC Data Block-Byte in the PLC Data Block-Word in the PLC Data Block Bit in the PLC Dynamic Data Exchange Directory Disk Operating System Data Terminal Equipment Driver Module Electromagnetic Compatibility Encoder Erasable Programmable Read Only Memory Electro Static Discharge Function Call Feed Drive Floating Point Unit Feed Stop Gear Interpolation Data Global User Data Hard Disk Handheld Unit Human Machine Interface Interface Module Interface Module-Address Increment Initializing Data Input- / Output Industry Standard Architecture Jogging Communication Bus Light Emitting Diode Line Feed Mega Byte (Million Bytes) Machine Data Machine Control Panel Machine coordinate system Machine Control Unit Manual Data Automatic


Page 9

Notes:

B565

Section 7 Notes:

Shortcuts and abbreviations MM MMC MPI MPF MSD MSTT NC NCK NCU NMI OI OP OPI P-Bus PC PCU

PCMCIA PG PLC PRAL PS PTP P2P RAM REF ROV SBL SK SKP SW SPF SYF T TC TLC TO TRC UFR VGA WCS WPD ZO

B565

Millimetre Man machine communication = HMI Multi Point Interface Main Program File Main Spindle Drive Machine Panel Numerical Control Numerical Control Kernel Numeric Control Unit Non Mask able Interrupt Operator Interface Operator Panel Operator Panel Interface Peripheral-Bus Personal Computer Personal Computer Unit. Component of the NC-control, which allows communication between operator and machine. Personal Computer Memory Card International Association Programming Device Programmable Logic Control Process Alarm Power Supply (SIMATIC S7-300) Point to Point Point to Point Random Access Memory (read write memory) Reference Point Approach Function Rapid Override Single Block Softkey Skip Block Software Sub Programm File System Files Tool Tool Change Tool Length Compensation Tool Offset Tool Radius Compensation User Frame Video Graphics Adapter Workpiece Coordinate System Work Piece Directory Zero Offset

Page 10


B566

1

Operating elements

Brief description

Objective of the module: With help of this module you learn to recognise general operating elements of the Sinumerik Operate, and how to differentiate them from one another.

Description of the module: The general operation of a Sinumerik Operate will be described. Depending on the machine manufacturer the following operating elements can be used:  Operator panels (OP)  CNC-full keyboard  Machine control panel (MCP) Content: Operator panel layouts of the Sinumerik Operate CNC-full keyboard (QWERTY - type) Machine control panel (MCP)


Page 1


B566

B566

B566

Page 2


B566 Operating elements: Description Operating elements: START

The general operation of a Sinumerik Operate will be described. Depending on the machine manufacturer the following operating elements can be used:

Operator panel layouts of the Sinumerik Operate

 Operator panels (OP)  CNC-full keyboard  Machine control panel (MCP)

CNC-full keyboard

Machine control panel

Operating elements: END

Notes :


Page 3

B566

Section 2 Notes:

Operator Panel layouts of the Sinumerik Operate The operator panel (OP) consists of the following operating elements: 

Membrane keyboard with 8 + 4 horizontal and 8 vertical softkeys



Colour display (10.4” Display on 828D, 15” Display on 840D sl)



Front-USB-plug on operator panel front (840D sl),



USB, CF-card, Ethernet on operator panel front (828D)



Fully integrated QWERTY CNC-keyboard (828D)

2.1 Operator panel layout of the Sinumerik 840D sl: 5 2

3

4

1 1

Horizontal softkey strip (HSK) with 4 screen keys (2 each located on the left and right side)

2

Vertical softkey strip (VSK)

3

15“ TFT-colour display

4

Front-USB-plug (Sinumerik 840D sl) , e.g. for connection of external memory media, mouse or keyboard

5

Status-LED: Power Status-LED: Temp

2.2 Operator panel layout of the Sinumerik 828D 2 5

3

4 1 2 6

5 3

6

4 1

B566

Page 4


Operator Panel layouts of the Sinumerik Operate

Section 2 Notes:

1

Horizontal softkey strip with 4 screen keys (2 each located on the left and right side) (HSK)

2

Vertical softkey strip (VSK)

3

10,4“ TFT-colour display

4

USB, CF-card and Ethernet on panel front behind removable cover

5

Ready-LED (Status red/green), NC-LED (Status LED of the NC) and CF-LED (write/read access on CF-card) behind lockable and removable cover

6

Integrated QWERTY CNC-keyboard (for reference see section 3)

2.3. Horizontal and vertical Softkey bar (HSK/VSK) Softkeys are buttons, which are dynamically linked with programmed functions. These functions are presented on the monitor above the softkey bar (HSK) or to the left of the softkey bar (VSK) as a strip of icons.  The 8 horizontal softkeys are used to access the individual operation sectors including further menu layers. There is an associated vertical menu strip/Softkey strip for each of the horizontal menu points.  The 8 vertical Softkeys are functions associated with the presently selected horizontal Softkey. The function will be called up when the vertical softkey is pressed. The content of the vertical softkey bar can therefore change once again if a sub-function to the selected function is chosen. The horizontal softkey bar consists furthermore of:  4 screen keys (see pictures below) “MACHINE”-key: Calls-up the operating area “MACHINE” (in operating mode “JOG”, “MDA” or “AUTO”). “Recall”-key: Jumps to the next highest menu level. “Extend”-key: Extends the horizontal softkey bar. “MENU SELECT”-key: Calls the main menu for operating area selection.


Page 5

B566

Section 2 Notes:

Operator Panel layouts of the Sinumerik Operate 2.4

Screen area

The screen is laid out as follows: 1

4

12

2

9

3

5 8 6

7 10

11

1 2 3

4 5 6 7

B566

Operation sector Program path and name Status, program influence and program name Alarm and message line Channel operation messages Position readout for the axes Display of the active zero point and rotation

Page 6

8

    9 10 11 12

Display of: T = Active tool F = Present feedrate S = Actual spindle revolution Spindle load factor in percent Vertical softkey bar (VSK) Working window Horizontal softkey bar (HSK) Date and Time


Section 3

CNC-full keyboard According to the model of operating panel that is used, a CNC-keyboard can be integrated for operation and programming. The keys that are described here can also be located directly on the operator panel. The layout of the operating panel is described in the documentation of the machine manufacturer. Below follows a description of the basic keys of the CNC-Full keyboard.

Notes:

CNC-Full keyboard “KB 483”:

Alpha-Block

Hotkey-Block

Cursor-Block

Number-Block.

Alpha-Block:

The alpha-block features the letters A, ..., Z, the space key and the special character for the input of text.

Hotkey-Block:

The hotkey-block serves the direct selection of operation areas.

Cursor-Block:

The cursor-block is used for navigation around the screen display.

Number-Block:

The number-block features the numbers 0 ... 9, the decimal point and special characters for the input of numerical characters and operators.

Keys in the Alpha-Block BACKSPACE Clears a value in the input field. If in edit mode, the character in front of the cursor will be cleared. TAB Indent the cursor by several characters. SHIFT If the Shift-key is held depressed, the upper character on keys with double usage will be entered. CTRL With the following key combinations navigation in the work plan and the G-Code-Editor is carried out:  Ctrl + NEXT WINDOW: Jump to the beginning.  Ctrl + END: Jump to the end. ALT ALT-Key


Page 7

B566

Section 3 Notes:

CNC-full keyboard INPUT  Accepts an edited value  Opens / closes a directory  Opens a file Keys in the Hotkey-Block MACHINE Opens up the operating area "Machine" (JOG, MDA, Auto). Corresponds to the yellow HSK 1 “Machine” PROGRAM Opens up the operating area "Program". The key corresponds to the yellow HSK 3 “Program”. OFFSET Opens up the operating area "Parameter” (Tool list, Tool wear, Magazine, Work offset, User variable, Setting data). The key corresponds to the yellow HSK 3 "Parameter". PROGRAM MANAGER Opens up the operating area "Program manager“. The key corresponds to the yellow HSK 4 "Program Manager". ALARM Opens up the actual Alarmlist-window. The key corresponds to the VSK 1"Alarm list" in the operating area “Diagnostics”. CUSTOM This key can be customized by the machine manufacturer. See the machine manufacturer’s documentation . Keys in the Cursor-Block ALARM CANCEL Clears an active alarm shown in the alarm and message line that is identified with this symbol. CHANNEL Selects a channel from 1 - n. HELP Opens the context-sensitive help window in a splitscreen view. In case of the G-Code editor the help documentation with intelligent support for programming instructions is called up. NEXT WINDOW Activates the next subwindow in the actual working window. By pressing “CTRL + NEXT WINDOW“ in the G-Code editor window you can jump to the first line of the program code. PAGE UP or PAGE DOWN Paging up or down in a directory or the work plan.

B566

Page 8


Section 3

CNC-full keyboard

Notes:

Further keys in the Cursor-Block END Locates the cursor in the last input field of a parameter mask. In the G-code editor the cursor will be set to the end of the active line and by pressing STRG + END the cursor jumps to the end of the last line of the program. Cursor-Keys Navigates through the various fields or lines on the screen. While in a program listing, the “cursor-to-the-right”key opens a directory or a program. To change to the next level above the present level press the “cursor-to-the-left”-key. SELECT With this key you can select amongst several given alternatives. Keys in the Number-Block BACKSPACE Clears a value in the active input field. While in the edit mode, just the character in front of the cursor will be cleared. DEL Deletes the value in the parameter field. While in the edit mode, just the character behind the cursor will be deleted. INSERT Activation of the insertion mode or the pocket calculator. Opens a parameter menu in an input field if available. INPUT  Accepts an edited value  Opens/closes a directory  Opens a file


Page 9

B566

Section 4 Notes:

Machine control panel Depending on the type of operating panel the machine manufacturer may be using either a SIEMENS or his own machine control panel for the operation of the machine. This section describes the standard-keys of the Siemens machine control panel. Depending on the machine further keys may be used; such information should be taken from the documentation by the machine manufacturer. Machine control panel “MCP 483”:

Below follows a description of the keys of the machine control panel and their function: EMERGENCY-STOP-key Press this key in the case of an emergency, i.e. if human life is endangered or if the machine or work piece could be damaged. All drives will be braked to a standstill with the greatest possible braking torque. Note: For further reactions that may be caused by pressing the EMERGENCY-OFF key please refer to the documentation by the machine manufacturer. RESET  Stops the machining from executing the presently running program. The NC-control unit remains synchronized with the machine. It is now in the basic condition ready to commence a new program run.  Clears an active alarm. JOG Selection of the operating mode “JOG”. TEACH IN Creation of programs in interactive mode with the machine. MDA Selection of the operating mode “MDA” (Machine Data Automatic). AUTO Selection of the operating mode “Machine Auto”.

B566

Page 10


Section 4

Machine control panel SINGLE BLOCK Runs a program block-by-block (single block).

Notes:

REPOS Repositions and re-approaches a contour. REF. Point Approaches a reference point. VAR (Variable JOG step) Traverse through an incremental dimension with variable step lengths. Inc (Incremental JOG step) Traverse through an incremental dimension with a given step size of 1, ..., 10000 increments. The actual length of an incremental step depends on a machine datum. Note: Read the machine manufacturer’s documentation. CYCLE START Starts a program run. CYCLE STOP Stops a program run. Axis keys Axis (X, Y, Z, 4, 5, 6) selection. to

Direction keys For traversing an axis either in the positive or negative direction. RAPID For traversing an axis at rapid traverse rate (fastest speed). WCS MCS Toggling between the work piece coordinate system (WCS) and the machine coordinate system (MCS).


Page 11

B566

Section 4 Notes:

Machine control panel Feed / Rapid traverse override For increasing or reducing the programmed feedrate. The programmed feedrate is represented by 100% and can be varied within the range of 0% to 120%, in rapid traverse only up to 100%. The new adjusted value appears as an absolute and percentage value in the feed status display on the screen. FEED STOP Stops the machining of the currently running program, in order to stop the axes. FEED START Continuation of the program as from the present block and to increase the feedrate to the programmed value. Spindle override For increasing or reducing the programmed speed. The programmed speed corresponds to 100% and can be varied within the range of 0% to 120%. The new value thus selected appears as an absolute value and as a percentage in the speed status display on the screen. SPINDLE STOP To stop the spindle. SPINDLE START To start the spindle. Key switch Position 0 No key Access stage 7 Position 1 Key 1 black Access stage 6

Lowest access stage

Increasing access rights

Position 2 Key 1 green Access stage 5 Position 3 Key 1 red Access stage 4

Highest access right (Key switch)

Further access rights (Access stage 3 - 0) are possible by means of passwords.

B566

Page 12


B567

1

Switching on the machine / control unit reference point

Brief description

Objectives of the module: In this module you learn how to switch on the machine and / or the control unit and how to approach the reference point of the axes.

Description of the module: Both the machine and the control unit must be switched on before any work can be done on the machine. Following this all axes with incremental measuring systems must be referenced in order to enable the control unit to establish the position of the axes within the machine coordinate system. There is no need to reference any axes equipped with absolute measuring system. In this case the control unit recognizes the position of the axes automatically. Content: Switching on the machine and the control unit Approaching the reference point of the axes


Page 1


B567

B567

B567

Page 2


B567 Switching on the machine: Description Both the machine and the control unit must be switched on before any work can be done on the machine. Following this all axes with incremental measuring systems must be referenced in order to enable the control unit to establish the position of the axes within the machine coordinate system. There is no need to reference any axes equipped with absolute measuring system. In this case the control unit recognizes the position of the axes automatically.

Switching on the machine: START

Switching on the machine and the control unit

Approaching the reference point of the axes

Switching on the machine: END

Notes :


Page 3

B567

Section 2 Notes:

Switching ON the machine and the control unit Switching ON sequence Please note the explicit switching ON rules as stated by the machine manufacturer.

1. Turn on the main switch of the machine. Note: Normally the main switch will be found on the switchgear cabinet.

2. All EMERGENCY-STOP keys of the machine must be released (operating panels, switchgear cabinet, etc.).

Note: The locations of the EMERGENCY-STOP keys are shown in the machine manufacturer’s documentation.

B567

Page 4


Switching on the machine and the control unit 3. Switch on the control unit. Depending on the individual machine this switch can be found on the operating desk or the switchgear cabinet of the machine or else the control unit is switched ON automatically when turning the main switch.

Section 2 Notes:

Note: For more information see the documentation of the machine manufacturer The control unit boots. While booting a welcome image is displayed, followed by the basic screen of the SINUMERIK HMI (displayed below):

4. Any fault messages that might be displayed can be cleared by means of the “RESET“-key on the machine control panel.


Page 5

B567

Section 3 Notes:

Approaching the reference point of the axes 3.1 Referencing sequence

!

Before referencing the axes a check must be carried out to ensure that there is no danger of collisions during the approach.

Machines with incremental measuring systems must be referenced after switching ON in order to synchronize the measuring system with the machine coordinate system. Press the “JOG”-button on the machine control panel. Press the “REF.POINT”-button on the machine control panel. The respective LED’s above the keys are illuminated. The referencing screen 1 opens up with all the axes that need referencing (see image below).

1

3.2 Approaching the reference point Depending on the commissioning of the machine there are various ways of referencing. Note: For further details see the machine manufacturer’s documentation.

3.2.1. Automatic referencing Press the “CYCLE START”-button on the machines control panel. The axes will be referenced one after the other.

B567

Page 6


Approaching the reference point of the axes

Section 3 Notes:

3.2.2 Manual referencing Press the “FEED START“-button on the machine control panel. Select an axis for referencing.

Press

or

.

Note: Refer to the machine manufacturer's documentation. Select all other axes one after the other and start the reference point approach by pressing either “+“ or “-“.

While referencing confirm the feed override setting, since the axes are traversed at the feed rate that has been preset by means of a machine datum.

Axes that have been referenced are shown on the display with a “Reference point symbol“ preceding the axis name. See the screen below.

The axis is referenced as soon as the reference point is reached. The actual value display is set to the reference point value. From now on, path limits, such as software limit switches, are active. End the function via the machine control panel by selecting operating mode “AUTO” or “JOG”. 828D/840Dsl SINUMERIK Operate

Page 7

B567

Section End Notes:

B567

Page 8


B568

1

Basics of operation

Brief Description

Objective of the module: In this module you learn about the screen layout of the display panel of the Sinumerik Operate, as well as the the basic operation of the control using softkeys and buttons. Description of the module: This module describes the relevant parts of the main screen with help of the basic screen layout. In addition to the topic above, this module covers the selection of parameters with respect to units (mm/inch) used and the usage of the calculator within the input masks. Content: Basics of operation Considerations for the input masks


Page 1


B568

B568

B568

Page 2


B568 Basic operations: Description Basic operations: START

This module describes the relevant parts of the main screen with help of the basic screen layout. In addition to the topic above, this module covers the selection of parameters with respect to units (mm/inch) used and the usage of the calculator within the input masks.

Basics of operation

Considerations for the input masks

Basic operations: END

Notes :


Page 3

B568

Section 2 Notes:

Basics of operation 2.1 Main screen of the HMI in the operating mode “JOG” In this section the parts of the main screen will be declared. 1

4

6

2

12 5

3

7 8

9

10

11 1

Active operating area and mode Program path and name Status, program influence and channel name Alarm and message line Channel operation messages Date and time

2 3

4 5 6 7

   

B568

8 9

10 11 12

Position readout for the axes Display of the active zero point, rotation, mirroring and scaling Working window Horizontal softkey bar Vertical softkey bar

Display of: T = Active tool F = Present feedrate S = Spindle Spindle load factor in percent

Page 4


Section 2

Basics of operation 1

Notes: Active operating area and operating mode

(The display mode depends on the selected operating mode on the machine control panel (MCP)). Display area

Description The operating mode “Machine Manual” (setup mode) can be selected by pressing the “JOG”-button on the machine control panel. Functions adjusted under “T,S,M“ like tool selection, work offset and spindle control affect all movements in the manual operating mode. Another function using the “JOG“-Mode is the approaching of the reference point (REF.POINT). Hint: If you use a mouse to operate the HMI Sinumerik Operate, a click in the upper left corner of the display area (here the upper case “M“ with over line and underline) opens the yellow horizontal- and vertical softkey bar, from which you can access comfortably all the main functions of the control unit.

2

Program path and name

NC programs can be created, modified and selected in the three main directories on the NC of the type DIR.

 Folder “Part programs” Part programs have the file extension MPF and are stored in a separate part programs folder. Display in editor

Description The shown program path to the left indicates that the selected program “TEST.MPF” can be found on the NC. The “MPF” in the program path refers to the directory “Part programs“.

 Folder “Subprograms” Subprograms have the file extension SPF and are stored in a separate subprogram folder Display in editor

Description The selected program “TEST.SPF“ is stored on the NC in the SPF subprogram folder as the folder path to the left points out.

 Folder “Workpieces” Workpiece programs have the file extension WPD and are stored in a separate workpiece folder. Display in editor

Description The selected program “TEST.MPF” is stored on the NC in the created workpiece directory “TEST.WPD“ The “WKS” in the program path refers to the directory “Workpieces“.


Page 5

B568

Section 2

Basics of operation

Notes: 3

Status, program influence and channel name

Display area

Description Reset Interrupted Activated

4

Alarm and message line

In case of a syntax error in the program code or a hardware malfunction (e.g. emergency stop) an alarm number with explaining text shows up. MCP

Display area

Description

After correcting the error (correction of the hardware malfunction) you can reset the error message with the “RESET“-button. CNC-keyboard By pressing the “ALARM“-key on the keyboard the “Alarm list”-window shows up, with a list of all active alarm messages.

After correcting the error (correction of the syntax error) you can reset the error message with the “ALARM CANCEL“-key on the keyboard.

B568

Page 6


Section 2


Chanel operation messages Display of operation messages with symbols. Display area Description Attention: In case of conditions with this symbol a manual operation is required.

Notes:

 Operation in case of the message “Stop“: After the fault remedy the machining program will be continued after pressing “NC-Start“.  Operation in case of the message “Wait“: After a successful acknowledgement of the fault the machining program will be continued automatically.  Stop: No NC-Ready  Stop: BAG-Ready (mode-of-operation group)  Stop: EMERGENCY-STOP activated  Stop: Alarm with Stop activated  Stop: M0/M1 activated  Stop: Block completed in single block mode  Stop: Cycle-Stop activated  Wait: Read-in release missing (Part program is not further processed by NC)  Wait: Feed enable missing  Wait: Axis enable missing  Wait: for Feed override  Stop: NC-block erroneous  Wait: for external NC-blocks  Wait: Spindle enable missing  Wait: Axis feed rate is 0  Stop: No channel ready  Stop: SERUPRO has reached the search destination and the NCK has stopped. SERUPRO is the abbreviation for „Search Run by Program test“ and represents a new kind of block search. In case of conditions with this symbol, a manual operation is usually not necessary.  Wait: Remaining dwell time in seconds or in spindle revolutions  Wait: HiFu-acknowledgement missing  Wait: Exact stop not reached  Wait: for positioning axis 828D/840Dsl SINUMERIK Operate

Page 7

B568

Section 2 Notes:

Basics of operation Display area

Description (continuation) Note: In case of conditions with this symbol a manual operation is usually not required.  Wait: for spindle  Wait: for another channel  Wait: due to a SYNACT-instruction  Wait: Block advance activated  Wait: for tool change acknowledgement  Wait: for gear change  Wait: for closed loop  Wait: for tapping start  Wait: for safe operation  Halt: oscillation activated  Wait: during access to a system variable

6

Date/Time

Current date and time are shown in the upper right corner of the screen.

7

Display of T,F,S and spindle-value

Display area

Description T: (Tool) Name of the active tool. The optional display of “TC“ is only available if a swivel head table is present. F: (Feed) Display of the active feed rate for the current machining (top: actual feed rate, large digits during machining), as well as the display of the programmed feed rate (bottom) and the feed override in %. S: (Spindle) Display of the active spindle speed for the current machining (top: actual speed, large digits during machining), as well as the display of the programmed spindle speed (bottom) and the speed override in %.

B568

Page 8


Section 2


Notes:

Position display for the axes

MCP/Display area

Description With the key “WCS MCS” on the MCP or the VSK 7 “Act. vls. MCS” it is possible to switch between the machine coordinate system (MCS) and the workpiece coordinate system (WCS). Display of the available axes with axis assignment and position data in the machine coordinate system (Mach).

Display of the available axes with axis assignment and position data in the work piece coordinate system (WCS). However, programmable zero offsets are not taken into consideration in the display.

9

Display of the active zero point offsets, rotation, mirroring and scaling

The machine coordinate system (MCS) does not consider zero point offsets in comparison to the workpiece coordinate system (WCS). Display area

Description Name of the currently active work offset, rotation, mirroring, rotation and scaling for the present machining sequence.

10

Work window

Depending on the pressed horizontal softkey the associated parameter fields and help pictures are displayed. Here the “T,S,M”-mask is shown.


Page 9

B568

Section 2 Notes:


Horizontal softkey bar (HSK)

The user interface consists of different subsections. At the bottom of the screen is the horizontal softkey bar (HSK) containing 8 softkeys (see Section 2.2.1 in this module). The selection of a new window is made by pressing the buttons just under the softkeys. If the number of functions exceeds the representation capacities of the maximum of 8 softkeys than a partitioning in two different horizontal softkey bars occurs. The change over forth and back takes place with the “Menu extend“-key on the operator panel.

12

Vertical softkey bar (VSK)

The available functions and operating modes can be selected from the keys right beside the vertical softkey bar (VSK) on the right hand side of the screen. If the number of functions exceeds the representation possibility capacity of the maximum of 8 softkeys than a partitioning in two different vertical softkey bars occurs. The changeover takes place with the: “Forward“-key or the “Backward“-key (VSK 8).

2.2

Operating with softkeys and buttons

The Sinumerik Operate separates into 6 different operating areas (“Machine“, “Parameter“, “Program“, “Program Manager“, “Diagnostics“, “Start-up”), 3 operating modes (“JOG”, “MDA”, “AUTO”) and 2 functions (“REPOS”, “REFPOINT”). By pressing the button “MENU SELECT“ on the operator panel the active screen will be overlaid with the display of a yellow horizontal softkey bar at the bottom and a yellow vertical softkey bar on the left side of the screen. They consist of 6 operating area softkeys in the HSK and 3 operating mode-, as well as 2 function softkeys in the vertical softkey bar.

B568

Page 10


Section 2

Basics of operation

Notes:

2.2.1 Horizontal softkey bar (HSK) Display area

Description By pressing HSK 1 “Machine“ the operating are “Machine“ will be called up. See module B569 - “Operating area machine“.

By pressing the HSK 2 “Parameter“ the operating area “Parameter“ will be called up. See module B573 - “Operating area Parameter“.

By pressing the HSK 3 “Program“ the operating area “Programm“ will be called up. See module B574 - “Operating area Programm“.

By pressing the HSK 4 “Program-Manager“ the operating area “Program-Manager“ will be called up. See module B575 - “Operating area ProgramManager“. By pressing the HSK 5 “Diagnose“ the operating area “Diagnose“ will be called up. See module B576 - “Operating area Diagnose“.

By pressing the HSK 6 “Start-up“ the operating area “Start-up“ will be called up. See module B577 - “Operating area Start-up“.

2.2.2 Vertikale Softkey-Leiste (VSK) Display area

Description By pressing the VSK 1 “AUTO“ the operating mode “AUTO“ will be called up See module B572 - “Operating mode AUTO“. By pressing the VSK 2 “MDA“ the operating mode “MDA“ will be called up. See module B571 - “Operating mode MDA“. By pressing the VSK 3 the operating mode “JOG“ will be called up. See module B570 - “Operating mode JOG“.


Page 11

B568

Section 2 Notes:

Basics of operation Display area

Description (continuation) By pressing the VSK 4 „REPOS“ the function „REPOS“ will be called up. See module B569 - “Operating area Machine“. By pressing the VSK 5 „REF POINT“ the function “REF POINT“ will be called up. See module B569 - “Operating area Machine”.

B568

Page 12


Section 3

Notes for the input masks 3.1

Notes:

Measurement units [metric/imperial]

The measurement units of all parameters used in the entire documentation are defined in the metrical system (mm). The following table compares the equivalent imperial measuring units (inch and foot) with the metric system. Note: A description how to change between metric (mm) and imperial system (inch) can be found in the module B570 - “Operating mode JOG“. Metric

Inch/foot

mm

in

mm/tooth

in/tooth

mm/min

in/min

mm/rev

in/rev

m/min

ft/min

3.2

Parameter selection

The following described selection of parameters in an input mask can be called in every entry field where parameter selection is possible and numerical input is not possible. A list of possible parameters is displayed by pressing "INSERT"-key on the keyboard Navigation through the menu occurs with the blue cursor-keys. Hint: Navigation in long lists can be short cutted by pressing the initial letter or number of the parameter directly on the keyboard. Each additional pressed letter continuous to restrict the selection. If the selected entry is orange highlighted (actual cursor position) then with pressing on of the yellow “INPUT“-keys on the keyboard the chosen value is taken over into the input field. Alternatively you can switch through a list of possible choices in the input field by pressing the blue “SELECT“-key repeatedly.


Page 13

B568

Section 3 Notes:

Notes for the input masks 3.3

Pocket calculator

The calculator can be called-up from every part of the operating area. If a numerical entry is necessary in an input field you can open the pocket calculator by pressing the equal sign (=) on the keyboard. If their is already a value existing in the input filed e.g. 100 , then the value will be captured into the calculator window. Softkeys

Description By pressing the softkey “Delete“ every input or outcome value in the calculator will be deleted. For calculating values the four basic arithmetical operators are available, as well as….. square root (R) and…. Square (S). If you enter the letter “R“ with a following number in the calculator and press the “Calculate“ button than the square root of the entry will be calculated. If you place first a “S“ instead of a “R“ in front of the number, the square will be calculated. A mathematical function with values in parenthesis allows the calculation of complex mathematical expressions. The softkey “Accept“ transfers the result to the input field and closes the pocket calculator independently. The button “Cancel“ closes the pocket calculator.

B568

Page 14


B569

1

Operating area "Machine"

Brief Description

Objective of the module: In this module you learn how to work with the different options of the operating area "Machine".

Description of the module: In this module the basic menu is explained, with respect to each operating options. The basic menu consists of a yellow horizontal softkey bar (with 6 operating areas) at the bottom and a yellow vertical softkey bar (with 3 operating modes and 2 functions) at the right hand side of the screen. Depending on the elective operation mode (“JOG”, “MDA”, “AUTO”) a different window option (HSK) and function option (VSK) is displayed in the operating area "Machine".

Content: Operating area "Machine"


Page 1


B569

B569

B569

Page 2


B569 Operating area machine: Description In this module the basic menu is explained, with respect to each operating options. The basic menu consists of a yellow horizontal softkey bar (with 6 operating areas) at the bottom and a yellow vertical softkey bar (with 3 operating modes and 2 functions) at the right hand side of the screen. Depending on the elective operation mode (“JOG”, “MDA”, “AUTO”) a different window option (HSK) and function option (VSK) is displayed in the operating area "Machine".

Operating area machine: START


Operating area machine: END

Notes :


Page 3

B569

Section 2 Notes:

Operating area "Machine". 2.1

Selecting the operating area "Machine"

The operating area "Machine" can be selected as follows: Press the button "MENU SELECT" on the operator panel . The actual operator interface will be overlaid with the display of a basic menu containing the yellow horizontal softkey bar (with the 6 operating areas: “Machine”, “Parameter”, “Program”, “Program manager”, “Diagnostics” and “Start-up”) and the yellow vertical softkey bar (with 3 operating modes: “JOG“, “MDA“, “AUTO“ and 2 functions: “REPOS, “REFPOINT).

By pressing the HSK 1 "Machine" depending on the formerly chosen operation mode:  JOG (see module B520)  MDA (see module B521)  AUTO (see module B522) there will be different window options (HSK) and function options (VSK) available in the operating area "Machine",

After pressing the HSK 1 "Machine" (selecting the operating area "Machine") in the operating mode "JOG" the "Machine" operator interface opens up (see the following image).

B569

Page 4


Section 2


Notes:

You can switch to the operating modes "JOG", "MDA" or "AUTO" in the operating area "Machine" immediately by pressing the respective button on the machine control panel, or by pressing the button “MENU SELECT“ first and then the corresponding VSK. 2.2 Vertical softkey (VSK) bar of the main menu Display section

Description By pressing the VSK 1 "AUTO" in the operating area "Machine", the operation mode "AUTO" will be called up. See module B572 - Operating mode "AUTO". By pressing the VSK 2 “MDA“ in the operating area "Machine" the operation mode “MDA“ will be called up. See module B571 - "Operating mode MDA" By pressing the VSK 3 “JOG“ in the operating area “Machine“ the operating mode "JOG" will be called up. See module B570 - "Operating mode JOG". After a program interruption (“CYCLE STOP“) and after traversing the axis you can reposition the axis to a saved position by pressing the VSK 4 “REPOS“. By pressing the VSK 5 "REF POINT" in the operating mode "JOG" or "MDA" you can approach the reference points.


Page 5

B569

Section End Notes:

B569

Page 6


B570

1

Operating mode “JOG“

Brief description

Objective of the module: In this module you learn the different options of the operating area "Machine" in the operating mode "JOG". Description of the module: In this module the softkeys of the Sinumerik Operate, available in the manual mode (setup- and basic functions), will be described. Content: Operating mode "JOG" Tool-, spindle- and machine commands (T,S,M) Set Work offset (“Set WO”) Measure workpiece Measuring a tool Position Face milling Handwheel Synchronized actions Settings



B570

B570

Page 2


B570 Operating mode jog: Description In this module the softkeys of the Sinumerik Operate, available in the manual mode (setup- and basic functions), will be described.

Operating mode jog: START Synchronized actions Operating mode "JOG" Settings Tool-, spindleand machine commands (T,S,M)

Operating mode jog: END

Set Work offset (“Set WO”)

Measure workpiece

Measuring a tool

Position

Face milling

Handwheel

Notes :


Page 3

B570

Section 2 Notes:

Operating mode “JOG“ Operation mode “JOG” is used, for setting up the machine for program runoff or if you simply want to traverse the axes on the machine:  Reference point approach, i.e. calibration of the position measuring system  Preparing a machine for executing a program in automatic mode, i.e. measuring tools, measuring the workpiece and, if necessary, defining the work offsets used in the program  Traversing axes, e.g. during a program interruption  Positioning axes 2.1

Selecting the operating mode “JOG“

The operating mode "JOG" can be selected as follows: Press the “JOG“ button on the machine control panel (MCP). The operating mode “JOG” opens directly. - OR Press the button “MENU SELECT“ on the machine control panel. Press the VSK 1 “JOG“ in the yellow vertical softtkey bar on the right hand side of the screen to switch directly to the operating mode “JOG“. Then Switch to the operating area “Machine” by pressing the “MACHINE” key on the operator panel or on the keyboard or press the “MENU SELECT“key on the operator panel and the yellow HSK 1 “Machine“. The following screen opens:

B570

Page 4


Operating mode “JOG“ The following functions are offered in the horizontal and vertical softkey bar of the operating area "Machine" ( see section 2.2 and 2.3). 2.2

Vertical softkey bars 1 and 2

Display area

Description The most important G-functions are displayed in a sub-window by pressing the VSK 1.1 "G functions". Available auxiliary functions are displayed in a subwindow by pressing the VSK 1.2 "Auxiliary functions" at the time of the output. By pressing the VSK 1.7 "Act. vls. MCS", the coordinate system will be toggled between the machine coordinate system (MCS) and the workpiece coordinate system (TCS). Note: Refer to the machine manufacturer„s documentation. By pressing the VSK 1.8 "Forward" on the operator panel (OP) the selection of additional softkeys on the vertical softkey bar is possible By pressing the VSK 2.2 "All G functions" all Gfunctions will be shown. By pressing the VSK 2.6 "Zoom act. val." all actual axes positions in the selected coordinate system as well as the currently active feed rate and feed override of each individual axis are displayed full screen. In addition all active zero point offsets, transformations and the T,F,S data is being displayed in the foot line. Note: If the machine is in the sub-mode “REPOS”, then the in manual mode traversed path difference is also being displayed. By pressing the VSK 2.8 "Back" on the operator panel (OP) the vertical softkey bar switches back to the menu of the VSK 1.


Section 2 Notes:

Section 2 Notes:

Operating mode “JOG“ 2.3

Horizontal softkey bar 1 and 2

Display area

Description By pressing the HSK 1 "T,S,M" the input screen "T,S,M" will be activated. By pressing the HSK 2 "Set WO" the input screen for setting the work offset will be activated. By pressing the HSK 3 "Meas. workp.“ the input mask for measuring a workpiece will be activated. By pressing the HSK 4 "Meas. tool" the function "Measure tool" will be activated and the extended options "Length/Radius manual", "Length/Radius auto",and "Calibrate Probe" will be available in the vertical softkey bar. By pressing the HSK 5 "Face mill." the input screen "Face milling" will be activated. By pressing the HSK 7 "Position" the input screen "Position" will be activated. By pressing the "Extend"-button on the operator panel (OP) more softkeys on the HSK are available.

This symbol on the right of the dialogue line indicates that more options on the HSK are available. This symbol indicates that you are in the expanded softkey bar. By pressing the HSK 2.6 "Handwheel" the input mask for traversing the axis in machine coordinate system (MCS) or workpiece coordinate system (WCS) will be available. By pressing the HSK 2.7 "Synchr. Action." the screen which shows the current synchronized actions is displayed. By pressing the HSK 2.8 "Settings" a window opens up where you can adjust the settings for manual operation on the Sinumerik Operate.

B570

Page 6


Tool-, spindle- and machine commands (T,S,M) 3.1

Selecting the function "T,S,M" (Tool, spindle and machine commands) By pressing the HSK 1 "T,S,M" in operation area “Machine” under operation mode “JOG” the following input mask will be displayed on the screen .

3.2


Display area

Description By pressing the VSK 2 "Tool" the tool list opens on the screen. See module B573 - "Operating area Parameter". By pressing the VSK 3 "Work offset" a list with the zero point offsets will be displayed. Refer to Work offset section 4 in this module and module B573 - "Operating area Parameter". By pressing the VSK 8 "Back" switch back to the main screen of the Sinumerik Operate.


Section 3 Notes:

Section 3 Notes:

Tool-, spindle- and machine commands (T,S,M) 3.3

Parameters of "T,S,M" (Tool, spindle and machine commands)

Input mask for tool-, spindle- and machine commands: Values can be entered directly in the orange marked input fields or by selecting predefined parameters with the “SELECT”-key. Alternatively the “INSERT”-button in the marked cursor field opens a select menu of all possible parameters, in which you can navigate with the “Tab”key as well as the blue “cursor-up”- and “cursor-down”-down buttons. The button “INPUT” takes over the selected values. In order to be independently of country specific measuring units [metric/ imperial] not all units are displayed in the input masks. See module B568 - "Basic operations". In this documentation the measuring units are always metric.

Parameter

Unit

Meaning

T

Tool name: e.g.: T12 or Cutter_7 (alphanumerical).

D

Cutting edge number of the tool.

Spindle

[rpm]

Spindle speed (revolutions per minute, numerical). Spindle machine functions: (Make a selection using the "SELECT"-key on the keyboard).

Spindle M funct.:  Empty field

No selection is made.  Right(M 3) Clockwise rotation of the spindle.  Left (M 4) Counter clockwise rotation of the spindle.  Off (M 5) Spindle is stopped.  Positioning (SPOS)

Spindle positioning: Spindle is positioned to the desired position. Manufacturer defined M-functions. By inserting the number of the function, a corresponding M-function is selected.

Other M funct..:

Refer to the machine manufacturer„s table for the correlation between the meaning and the number of the function.

B570

Page 8


Tool-, spindle- and machine commands (T,S,M) Parameter

Unit

Meaning (continuation) Alternative parameter options: The actual value of the work offset refers to the machine zero point, after approaching the reference point. In contrast a machining program refers to the workpiece zero point. This offset is to be entered as zero point offset. You can select work offsets from the tool list of settable work offsets via the "Work offset" softkey.

Work offset:  None  Basic reference  G54  G55  G56  G57

See module B573 - "Operating area Parameter". Alternative parameter options:

Unit of measure.:  none  mm

[mm]

 inch

[inch]

Note: The setting made here has effect on the programming.

Machining plane:  G17

(XY)

 G18

(ZX)

 G19

(YZ)

Gear stage:

Specification of the gear stage (none, auto, I - V).

Stop-Position:

[Degree]

Input of the spindle position in degrees. Note: This parameter shows up by selecting the spindle M-function .

Note: With “CYCLE START“ the inserted values will be executed. The entries in the option fields will be deleted, ready for new inputs.


Section 3 Notes:

Section 4 Notes:

Work offset 4.1

Selecting the function "Work offset" By pressing the HSK 2 "Set WO" in operation area “Machine” under operation mode “JOG” the input field for the programming of a work offset will be opened, like displayed below.

Input value:

By selecting an axis you can insert a value for the zero point offset in the orange marked field (see the picture above). The navigation through the axis-fields can be accomplished by pressing the blue “cursor-up“ and “cursor down“ keys on the keyboard. The slider on the right side of the subwindow indicates that there are more axis values available, that can be reached by using the “cursor-down“ key.

Important:

The horizontal softkey 2 "Set WO" is only selectable if the workpiece coordinate system is selected and a zero point offset (in this example G54) is active. The entered values for a zero point offset of the axis will be accepted and displayed in the workpiece coordinate system (WCS). The difference between the original position to the new entered value will be written to the active zero point offset.

B570

Page 10


Set work offset (“Set WO”) 4.2

Vertical softkey bar

Display area

Description By pressing the VSK 1 "X=0" the position of the Xaxis will be reset to zero. By pressing the VSK 2 "Y=0" the position of the Yaxis will be reset to zero. By pressing the VSK 3 "Z=0" the position of the Zaxes will be reset to zero. By pressing the VSK 4 „X=Y=Z=0“ the position of the X/Y/Z-axis will be reset to zero. By pressing the VSK 5 "Delete active WO" the zero point offset of all axes is set back to zero. By pressing the VSK 8 "Back" you switch back to the main screen of the Sinumerik Operate.

Note: After setting a position or deleting a zero point offset you switch back automatically to the main screen of the Sinumerik Operate.

4.3

Setting the "Work offset" Press the HSK 1 "T,S,M" to activate the “T,S,M“ (Tool-, spindle- and machine) -mode. In the input mask select the input field "Work offset". By pressing the "INSERT"-key on the keyboard, an option menu opens where you can make the desired selection of possible zero point offsets. You can navigate through this menu by means of the blue “cursor-up”- and “cursor-down”-keys on the keyboard. Hint: Navigation in long lists can be easier by pressing the initial letter or number of the parameter directly. Each additionally pressed letter continuous to restrict the selection. When the desired zero point offset is marked orange, you can accept this value by pressing the yellow “INPUT”-key on the keyboard. Alternatively you can toggle through all possible options by pressing the "SELECT"-key repeatedly. By pressing the button "CYCLE START" on the machine control panel the chosen zero point offset is activated.


Section 4 Notes:

Section 4

Set work offset (“Set WO”)

Notes:

4.4 Deactivating the "Work offset" Press the HSK 1 "T,S,M" to select the operation mode “T,S,M”. The “T,S,M” subwindow opens (see picture above). In the "T,S,M" input mask select the input field "Work offset". By using one of the previous described selection methods select the empty input field. Press the button "CYCLE START“ on the machine control panel (MCP) and the "Work offset" will be deactivated.

B570

Page 12


Measure workpiece 5.1

Selecting the function “Measure workpiece“ In the operating area “Machine“ under the operating mode “JOG“ press the HSK 3 "Meas. workp." to open the “Measure workpiece“ window shown below.

The reference point for programming a workpiece is always the workpiece zero. You can determine the workpiece zero on the following workpiece elements:  Edges (Set edge, Align edge)  Corner (Rectangular corner)  Hole (1 Hole, 2 Holes, 3 Holes, 4 Holes))  Spigot (Circular spigot, rectangular spigot) The workpiece zero can be measured either manually or automatically. Measuring manually: For manual measuring their are parameters that depend upon tool type, and therefore are only available for the particular case. The tool must be manually approached to the workpiece. You can use edge probes, sensing probes, or dial gauges with known radii and lengths. You can also use any other tool of which you know the radius and length. The tools used for measuring must not be electronic probes. Measuring automatically: For automatic measurements always use electronic 3-D or mono workpiece probes. You must calibrate the electronic workpiece probes beforehand. First position the workpiece probe manually. As soon as you start the process with the "CYCLE START" key, the workpiece probe automatically approaches the workpiece at measuring feedrate and then returns to the starting position at rapid traverse. The machine manufacturer must first set the appropriate machine parameters (e.g. the measuring feedrate). Note: During all measurements the override of the feedrate should be set to 100%. 828D/840Dsl SINUMERIK Operate

Section 5 Notes:

Section 5 Notes:

Measuring workpiece 5.2


Display area

Description By pressing the VSK 1 “Calibrate probe“ the input mask for “Calibrate probe“ opens. (See section 5.3). By pressing the VSK 2 “Set edge“ the “Set edge“ window opens. (See section 5.4). By pressing the VSK 3 “Align edge” the “Align edge” window opens. (See section 5.5). By pressing the VSK 4 “Rectangular corner” the “Rectangular corner” window opens. (See section 5.6). By pressing the VSK 5 “1 Hole” the “1 Hole” window opens. (See section 5.7). By pressing the VSK 6 “1 Circular spigot” the “1 Circular spigot” window opens. (See section 5.8). By pressing the VSK 8 "Back" you switch back to the main screen of the Sinumerik Operate.

5.3 Selecting the function “Calibrate probe” When the tool probes are attached to the spindle, clamping tolerance usually occurs. This can lead to measurement errors. Furthermore, you need to determine the trigger points of the probe relative to the spindle center. Therefore the tool probe has to be calibrated. The radius is calibrated in a hole, the length is calibrated on a surface. For the hole you can use a bore in the workpiece or a setting ring gauge. The radius of the workpiece probe ball and its length 1 must be stored in the tool list. By pressing the HSK 3 “Meas. workp.” and the VSK 5 “Calibrate probe” (in operating area “Machine” and operating mode “JOG”) the following input screen will be displayed (see the next page).

B570

Page 14


Section 5

Measuring workpiece

Notes:

5.3.1 Vertical softkey bar Display area

Description By pressing the VSK 2 “Length“ the following described parameter fields will be active. (See section 5.3.2) By pressing the VSK 2 “Radius“ the following described parameter fields will be active. (See section 5.3.2). By pressing the VSK 8 "Back" you switch back to the main screen for measuring the workpiece.

5.3.2 Parameters of “Calibrate probe“. Depending on the activated vertical softkey (“Length” or “Radius”) the available parameter input fields are different. Parameter

Unit

Probe number: Z0:

Description Number of Probes

[mm]

Height of reference piece Note: Only with activated vertical softkey „Length“.

Ø:

[mm]

Diameter of the reference piece Note: Only with activated vertical softkey “Radius”.


Section 5 Notes:

Measuring workpiece 5.3.3 Calibration of the probe length: 1.

Change a tool of the type 3-D probe into the spindle.

2.

Position the tool probe approximately over the centre of the measuring surface.

3.

In the operating area “Machine” under the operating mode “JOG“ press the HSK 3 “Meas. workp.“.

4.

Press Softkey "Calibrate probe” and then “Length”. The calibrate probe “Length” window opens.

5.

Enter the reference point “Z0” of the surface, e.g. of the workpiece or the machine table.

6.

Press “CYCLE START” on the machine control panel.

The calibration process starts. The length of the measuring tool will be calculated and entered in the tool list.

5.3.4 Calibration of the probe radius: 1.

Change to a tool of the type 3-D probe.

2.

Move the workpiece probe into the hole and position it into the approximated centre of the hole.

3.


4.

Press the VSK "Calibrate probe” and choose the VSK 3 “Radius”. The calibrate probe window for the “Radius” opens.

5.

Enter the diameter of the hole.

6.

Press “CYCLE START” on the machine control panel.

The calibration starts. First the exact hole centre is determined, then the four trigger points on the inside wall of the hole are being approached.

B570

Page 16



Measure workpiece zero “Set edge”

The workpiece lies parallel to the coordinate system on the work table. One reference point will be measured in one of the axes (“X”, “Y”, “Z”). The following requirements must be fulfilled:  Any tool can be inserted in the spindle for scratching when measuring the workpiece zero manually.  An electronic workpiece probe is inserted in the spindle and activated when measuring the workpiece zero automatically. By pressing the HSK 3 “Meas. workp.” and the VSK 2 “Set edge“, in the operating area “Machine“ and operating mode “JOG“, the following screen will be displayed.

5.4.1 Vertical softkey bar (VSK) Display area

Description By pressing the VSK 2 “Work offset“ a list of the work offsets opens. See module B573 - “Operating area Parameter“. By pressing the VSK 3 “X“ the measured values for the X-axis will be determined. By pressing the VSK 4 “Y“ the measured values for the Y-axis will be determined. By pressing the VSK 5 “Z“ the measured values for the Z-axis will be determined. By pressing the VSK 7 “Set WO“ the values will be accepted for the work offset. By pressing the VSK 8 “Back“ you switch back to the “Measure workpiece“ main screen .


Section 5 Notes:

Section 5 Notes:

Measuring workpiece 5.4.2 Parameters of "Set edge" Parameter

Description

Work offset:

Alternative parameters

 Measure only

The measured values are computed and displayed without changing the coordinate system.

 Work offset  Basic reference  Global base  Channel specific base Measurement direction:  X

The selection of the axes directions “X”/”Y”/”Z” is made by the vertical softkey bar. With the measurement direction (+ or -) it is determined whether the workpiece will be approached from a positive or negative “X”- or “Y”direction. By selection of the axis direction “Z it is only possible to approach the work piece from a negative Z-direction.

 Y

 Z

Reference point

X0, Y0, Z0

5.4.3 Procedure for “Setting edge” manually: 1.

Insert any tool in the spindle for scratching when measuring the workpiece zero manually.

2.


3.

Press the VSK 2 “Set edge.” The "Set edge" window opens.

4.

Select "Meas. only" if you only want to display the measured values. - OR -

4.

Select "Work offset" and the work offset (G54...G57) in which you want to store the zero point in the associated selection box. The selection of the work offsets can differ. Note: Please refer to the machine manufacturer's specifications.

B570

Page 18


Measuring the workpiece zero - OR 4.

Select "Basic ref." if the zero point is to be saved in the active system offset. - OR -

4.

Select "Chan. -spec. base" and the desired basic offset (No.1...No.9) in which the zero point is to be saved. -OR-

4

Select "Global basic" and the desired basic offset (No.1...No.7) in which the zero point is to be saved. -OR-

4.

Press the VSK 2 "Work offset" and select the work offset in which the zero point is to be saved in the "Work offset - G54 … G57" window and press the VSK 1 "In manual". You return to the "Set Edge" window. If it does not, press the VSK 3 “Meas. workp. “.

Note: The selection of work offsets can differ. Please refer to the machine manufacturer's specifications. 5.

Position the cursor to the desired Zero point offset (G54-G57), then press the VSK 1 „In manual“

6.

Use the VSKs 3 - 5 (“X”/ “Y”/ “Z”) to select in which axis direction you want to approach the workpiece first.

7.

Select the measuring direction (+ or -) you want to approach the workpiece in. The measuring direction cannot be selected for “Z0”.

8.

In “X0”, “Y0”, or “Z0”, specify the reference position of the workpiece edge you are approaching. The reference point position corresponds, e.g. to the dimension specifications of the workpiece edge from the workpiece drawing.

9.

Traverse the tool up to the workpiece edge.

10.

Press the VSK 7 "Set WO". The position of the workpiece edge is being calculated and displayed. The reference position of the workpiece edge is being stored as new zero point with “Set WO”. The tool radius is hereby automatically compensated for. Example: Reference point of workpiece edge X1 = -50, measuring direction +, tool radius = 3mm, zero point offset X = 53.

11.

If needed repeat the measuring procedure (step 5 to 10) for the other two axes.


Section 5 Notes:

Section 5 Notes:

B570

Measuring workpiece 5.4.4 Procedure for “setting edge” automatically 1.

Insert a tool of the kind 3-D probe in the spindle.

2.

Prepare the measurement (as described before in section 5.4.3 “Set edge” manually steps 2 to 8, on previous pages).

3.

Approach the tool near to the work piece edge that you want to measure.

4.

Press the "CYCLE START" key. The automatic measuring process is starts. The position of the workpiece edge is being measured. The position of the workpiece edge is being calculated and displayed. The setpoint position of the workpiece edge is being stored as new workpiece zero point if “Set WO” was selected. The tool radius is automatically compensated for.

5.

If desired repeat the measuring process (step 3 to 4) for the other two axes.

Page 20



Measure workpiece zero “Align edge”

The workpiece lies in any direction, i.e. not parallel to the coordinate system on the worktable. By measuring two points on the workpiece reference edge that you have selected, you determine the angle to the coordinate system. The following prerequisites must be fulfilled:  You can insert any tool in the spindle for scratching when measuring the workpiece zero manually.  An electronic workpiece probe is inserted in the spindle and activated when measuring the workpiece zero automatically. By pressing the VSK 3 “Align edge“ under the function “Meas. workp.” (in operating area “Machine“ and operating mode “JOG“) the following screen will be displayed.


Description By pressing the VSK 2 “Work offset“ a list of the work offsets will be displayed. See module B573 - “Operating area Parameter“. By pressing the VSK 3 “Store P1“ the determined position of the measuring point “P1“ is stored. By pressing the VSK 4 “Store P2“ the determined position of the measuring point “P2“ is stored. By pressing the VSK 8 “Back“ you jump back to the previous main screen.


Section 5 Notes:

Section 5 Notes:

Measuring workpiece Optionally two more softkey are available in the VSK, as later on described in this module (see section 5.7): By pressing the VSK 5 “Store P3” the determined position of the measuring point “P3“ is stored. By pressing the VSK 6 “Store P4“ the determined position of the measuring point “P4“ is stored. After completion of measuring a workpiece automatically with the electronic probe, the softkeys “P1 saved” to “P2 saved” are being highlighted and the softkey “Set WO” is being activated. 5.5.2 Parameters measure workpiece “Align edge“ Parameter

Description

Work offset:

Alternative parameters:

 Measure only


 Work offset

G54 ... G57

 Basic reference

G500

 Global Base  Channel-specific base Measurement direction/Measurement axis:  -X

 +X

Alternative parameter selection: With the measuring direction (+ or -) it will be determined whether the workpiece will be approached from positive or negative X- or Y-direction.

 -Y

 +Y

B570

Page 22


Measuring workpiece 5.5.3 Procedure for “Align edge” manually

1.

Insert any tool in the spindle for scratching when measuring the workpiece zero manually.

2.

In operating mode “JOG“ press the HSK 3 “Meas. workp.“.

3.

Press the VSK 2 “Align edge“. The input screen opens.

4.

Select “Measuring only” or "Work offset" , with the desired WO number (G54...G57) in which you want to store the zero point in the associated box (as described in section 5.4.3 “Set edge”, step 4).

5.

In the input fields "Meas. axis", select the axis in which you want to approach the workpiece, and the measuring direction (+ or -).

6.

Select in the input field “Angle. Offs” weather a correction as Coordinate rotation or rotary axis offset is being preformed. Select here “Coord. Rotation” or “C-Axis”. In the last case the rotary axis for which a correction is to be executed can be selected.

7.

Enter the setpoint angle between the workpiece edge and the reference axis.

8.

Traverse the tool to the workpiece edge.

9.

Press the VSK 3 "Store P1".

10.

Reposition the tool and repeat the measuring procedure (steps 5 to 7) to measure the second point, and then press the "Store P2" softkey.

11.

Press the VSK 7 "Set WO" The angle between the workpiece edge and reference axis is calculated and displayed.

With "Set WO", the workpiece edge now corresponds to the setpoint angle. The calculated rotation is stored in the work offset. 5.5.4 Procedure for “Aligning edge” automatically

1.

Insert a tool of the type 3-D probe

2.

Prepare the measurement (as described in section 5.5.3, “Align edge manually”, steps 2-7).

3.

Traverse the workpiece probe close to the workpiece edge on which you wish to measure.

4.

Press the "CYCLE START" key. The automatic measuring process is being started. The position of P1 is being measured and stored. The VSK 3 “P1 saved” becomes active.

4.

Repeat the operation (step 3 to 4) to measure and store P2. The position of P2 is being measured and stored. The VSK 4 “P2 saved” becomes active

6.

Press the VSK 7 "Set WO" or "Calculate".

The angle between the workpiece edge and reference axis is calculated and displayed. With "Set WO", the workpiece edge now corresponds to the setpoint angle. The calculated coordinate rotation is stored in the correction target that you have selected.


Section 5 Notes:

Section 5 Notes:


Measure workpiece zero “Rectangular corner”

The workpiece has a 90° corner and is located anywhere on the work table. By measuring three points you can determine the corner point in the working plane (X/Y plane) and angle α between the reference edge on the workpiece (line through P1 and P2) and the reference axis (always the 1st axis in the working plane). The following prerequisites must be fulfilled:  You can insert any tool in the spindle for scratching when measuring the workpiece zero manually.  An electronic workpiece probe is inserted in the spindle and activated when measuring the workpiece zero automatically. By pressing the VSK 4 “Rectangular corner“ under the function “Meas. workp.” (operating area “Machine“ and operating mode “JOG“) the following screen will be displayed:

5.6.1 Vertical softkey bar (VSK) See page 25/26 measure workpiece “Aligning edge“. 5.6.2 Parameters of measure workpiece “Rectangular corner“ Parameter

Description

Work offset:

Alternative parameters

 Measuring only


 Work offset

G54-G57

 Basic reference

G500

 Global base

B570

Page 24


Measuring workpiece Parameter

Description (continuation)

 Channel-specific The zero point is stored into the active system frame. base Channel -specific base is saved under No. 1 ... No. 7 Outside corner:

Measures the outside corner of the workpiece:

 Pos. 1

 Pos. 2

 Pos. 3

 Pos. 4

Inside corner:

Measures the inside corner of the workpiece:

 Pos. 1

 Pos. 2

 Pos. 3

 Pos. 4

X0

Reference point X

Y0

Reference point Y


Section 5 Notes:

Section 5 Notes:

Measuring workpiece 5.6.3 Procedure for Measuring a “Rectangular corner” manually 1.

Insert any tool in the spindle to scratch on.

2.

In the operating mode “JOG“ press the HSK 3 “Meas. workp.“.

3.

Press the VSK 4 "Rectangular corner" if the workpiece has a right angled corner that is to be measured. The "Rectangular corner" window opens.

4.


5.

Select the “Corner“ (inside corner or outside corner) that you wish to measure and its position (e.g. Pos. 1... Pos. 4).

6.

Specify the setpoint of the workpiece corner (“X0”, “Y0”) you want to measure.

7.

Traverse the tool to the first measuring point “P1”, according to help screen.

8.

Press the VSK 1 "Save P1". The coordinates of the first measuring point are measured and stored.

9.

Reposition the spindle with the tool each time to approach measuring point “P2” and “P3” and press the VSK 4 "Save P2" and VSK 5 "Save P3".

10.


The corner point and angle “α” are calculated and displayed. The corner point now corresponds to the setpoint position. The calculated offset is stored in the work offset. 5.6.4 Procedure for measuring a “Rectangular corner” automatically 1.

Insert a 3-D probe in the spindle

2.

Prepare the measurement (as described in section 5.6.3 Procedure for Measuring a “Rectangular corner” manually, step 2-6).

3.

Approach measuring point “P1” with the workpiece probe.

4.

Press the "CYCLE START" key. This starts the automatic measuring process. The position of “P1” is measured and stored. The VSK 3 "P1 stored" softkey becomes active.

5.

Repeat the operation (step 3 and 4) to measure and store points “P2” and “P3”.

6.

If a corner not equal to 90 degrees is to be measured, repeat the previous step to measure and store P4.

7.

Press the "Set WO" or "Calculate" softkey.

The corner point and angle “α” are calculated and displayed. The corner point now corresponds to the setpoint position. The calculated offset is stored in the correction target that you have selected.

B570

Page 26


Section 5


Measuring workpiece zero “1 Hole”

The workpiece lies anywhere on the work table and has a hole. You can determine the diameter and centre point of the hole with four measuring points (“P1” - “P4”) . The following prerequisites must be fulfilled:  You can insert any tool in the spindle for scratching when measuring the workpiece zero manually.  An electronic workpiece probe is inserted in the spindle and activated when measuring the workpiece zero automatically. By pressing the VSK 5 “1 Hole“ under the function “Meas. workp.” (in operating area “Machine“ and operating mode “JOG“) the following screen will be displayed:

5.7.1 Vertical softkey bar (VSK) See page 25-26 measure workpiece “Aligning edge“. 5.7.2 Parameters of measure workpiece “1 Hole” The following parameters of “Aligning the edge” are used also in “1 Hole” (see page 25-26): [Work offset, G54, X0, Y0] Some additional parameters are available if a 3-D probe is used: Parameter Unit Description Ø Hole

[mm]

Contact ang.

[Degree]Contact angle


Diameter of the hole

Notes:

Section 5 Notes:

Measuring workpiece 5.7.3 Procedure for measuring “1 Hole” manually 1.

Insert any tool in the spindle for scratching on

2.

In operating mode “JOG“ press the HSK 3 “Meas. workp.“.

3.

Press the VSK 5 "1 Hole". The "1 Hole" input screen mask opens.

4.


5.

Specify the setpoint position (“X0”/”Y0”) of pocket centre point “P0”.

6.

Traverse the tool to the first measuring point P1.

7.

Press the VSK 3 "Save P1". The point is measured and stored.

8.

Repeat steps 6 and 7 to measure and store measuring points P2, P3 and P4.

9.


Diameter and centre point position of the hole are calculated and displayed. The set position of the centre point is stored as a new zero point with "Set WO". The tool radius is automatically compensated for in the calculation. 5.7.4 Procedure for measuring “1 Hole” automatically 1.

Insert a tool of the type 3-D probe in the spindle.

2.

Prepare the measurement (as described in section 5.7.3 Procedure for measuring “1 Hole” manually, step 2-5).

3.

Move the workpiece probe until it is positioned approximately at the centre of the hole.

4.

Under "Ø hole" enter the approximate diameter to delimit the area in which the tool can be traversed. If no diameter is entered, travel starts from the starting point at measuring feedrate.

5.

If needed, insert a value in the field “Contact angle“. With the contact angle the direction in which you approach the wall of the hole can be rotated at any angle.

6.

Press "CYCLE START" on the MCP. This starts the automatic measuring process.

The workpiece probe automatically measures four points in succession around the inside wall of the hole. When measurement has been successfully completed, the VSK "P0 stored" becomes active. The diameter and centre point of the hole are calculated and displayed. The set position of the centre point is stored as the new zero point in the correction target that you have selected, if you have selected "Work offset".

B570

Page 28


Section 5


Measuring workpiece zero “1 Circular spigot“

The workpiece is located anywhere on the work table and has a circular spigot. You can determine the diameter and centre point of the spigot with four measuring points. The following prerequisites must be fulfilled:  You can insert any tool in the spindle for scratching when measuring the workpiece zero manually.  An electronic workpiece probe is inserted in the spindle and activated when measuring the workpiece zero automatically. By pressing the VSK 6 “1 Circular spigot” under the function “Meas. workp.” (in operating area “Machine“ and operating mode “JOG“) the following screen will be displayed:

5.8.1 Vertical softkey bar (VSK) See page 25-26 measure workpiece “Aligning edge“. 5.8.2 Parameters of measure workpiece “1 Circular spigot“ The following parameters of “Set edge” (Section 5.4.2) are used also in “1 Circular spigot”: [Work offset, G54...G57, X0, Y0] The following parameters are only shown if a 3-D probe is in the spindle: Parameter

Unit

Description

Ø Spigot

[mm]

Diameter spigot

DZ

[mm]

Infeed measurement depth

Contact ang.

[Degree]Contact angle


Notes:

Section 5 Notes:

Measuring workpiece 5.8.3 Procedure for measuring “1 Circular spigot” manually 1.

Insert any tool in the spindle for scratching on

2.

In the operating mode “JOG” press the HSK 3 “Meas. workp.”

3.

Select the VSK 6 “1 Circular spigot”. The “1 Circular spigot” window opens.

4.


5.

Specify the setpoint position (“X0”/”Y0”) of the spigot centre point “P0”

6.

Traverse the tool to the first measuring point.

7.

Press the "Save P1" softkey. The point is measured and stored.

8.

Repeat steps 6 and 7 to measure and store measuring points P2, P3 and P4.

9.


The diameter and centre point of the spigot are calculated and displayed. The set position of the centre point is stored as a new zero point with "Set WO". The tool radius is automatically compensated for in the calculation.

5.8.4 Procedure for measuring “1 Circular spigot” automatically 1.

Insert a tool of the type 3-D probe in the spindle.

2.

Prepare the measurement like described before (section 5.8.3 Procedure for measuring “1 Circular spigot” manually, steps 2 to 5).

3.

Move the workpiece probe until it is approximately at the centre of the spigot.

4.

In "Ø Spigot", enter the approximate diameter of the spigot. This limits the area for rapid traverse. If no diameter is entered, travel starts from the starting point at measurement feedrate.

5.

Insert a value for “DZ” to set the infeed measurement depth.

6.

Press "CYCLE START" on the machine control panel. This starts the automatic measuring process.

The tool automatically measures four points in succession around the spigot outside wall. When measurement has been successfully completed, the "P0 stored" softkey becomes active. The diameter and centre point of the spigot are calculated and displayed. The set position of the centre point is stored as the new zero point in the correction target that you have selected.

B570

Page 30


Section 6

Measure tool 6.1

Selecting the function “Measure tool“

The geometries of the machining tool must be taken into consideration when executing a part program. These are stored as tool offset data in the tool list. Each time the tool is called, the control considers the tool offset data. When programming the part program, you only need to enter the workpiece dimensions from the production drawing. After this, the controller independently calculates the individual tool path. You can determine the tool offset data, i.e. the length and radius or diameter, either manually or automatically with tool probes. By pressing the HSK 4 “Meas. tool“ in the operating mode “JOG” under the operating area “Machine” the following window opens:

Measuring a tool manually For manual measurement, move the tool manually to a known reference point to determine the tool length and the radius or diameter. The control then calculates the tool offset data from the position of the tool carrier reference point and the reference point. With the measuring of the tool length either the workpiece or a fixed point in the machines coordinate system, e.g. a load cell or a fixed point in conjunction with a distance meter, can be used as a reference point. The position of the workpiece is specified during the measurement. The position of the fixed point however must be announced before the measurement. With the determination of the radius or diameter the workpiece always serves as the reference point. Hint: Depending on the setting in a machine data either the radius or the diameter of the tool can be measured. Note: Refer to the machine manufacturer's specifications.


Notes:

Section 6 Notes:

Measure tool Measuring a tool automatically (Length and radius or rather diameter) For automatic measurement, you determine the length and radius or diameter of the tool with the aid of a tool probe (table contact system). The Sinumerik Operate uses the known positions of the tool holder reference point and tool probe to calculate the tool offset data. Before a toll can be measured automatically, the approximate tool geometry data (length and radius or diameter) must be entered in the tool list and the probe must be calibrated. Depending on the setting in a machine data, the radius or the diameter of the tool can be measured. You can consider a lateral or longitudinal offset “V” when measuring. If the maximum length of the tool is not at the outer edge of the tool or the maximum width is not at the bottom edge of the tool, you can store this difference in the offset. If measuring shows that the length of the tool diameter is greater than the probe diameter, measurement is automatically performed with a turning spindle rotating in the opposite direction. The tool is then not moved over the probe centre-to-centre, but with the outside edge of the tool above the centre of the probe.

6.2


Display area

Description By pressing the VSK 1 ”Length manual” the “Length manual” input mask opens. (See section 6.3). By pressing the VSK 2 “Radius manual“ or rather “Diameter manual“ the input mask “Radius manual“ or rather “Diameter manual“ opens. (See section 6.4). By pressing the VSK 1 ”Length auto” the “Length auto” input mask opens. (See section 6.5). By pressing the VSK 2 “Radius auto“ or rather “Diameter auto“ the input mask “Radius auto“ or rather “Diameter auto“ opens. (See section 6.6). By pressing the VSK 1 ”Calibrate probe” the “Calibrate probe” input mask opens. (See section 6.7). By pressing the VSK 8 “Back“ you jump back to the “Meas. tool” screen of the Sinumerik Operate.

B570

Page 32


Section 6

Measure tool 6.3

Measure tool “Length manual” By pressing the HSK 4 “Meas. tool” and the VSK 1 “Length manual“ (in the operating area “Machine“ under the operating mode “JOG”) the following input mask opens.


Description By pressing the VSK 2 “Tool“ the tool list opens. See module B573 - “Operating area Parameter“. By pressing the VSK 7 “Set length“ the entered values will be accepted. By pressing the VSK 8 “Back“ you jump back to the “Measure tool” screen of the Sinumerik Operate.


Notes:

Section 6 Notes:

Measure tool 6.3.2 Parameters of measure tool “Length manual“ Parameter

Description

T

Tool name Alternatively you can select a tool via the VSK 2 “Tool”.

D

Edge number (1 to 9)

ST

Replacement tool (01- 99)

Z0

Workpiece edge

6.3.3 Procedure for Measuring tool “Length manual” 1.

Load the tool in the spindle you want to measure.

2.

In the operating mode “JOG“ press the HSK 4 “Meas. tool”.

3.

Press the VSK 1 “Length manual”. The “Length manual” input screen opens.

4.

Press the VSK 2 “Tool“. Select a tool from the “Tool list” that opens immediately after pressing the softkey.

5

Press the VSK 1 „In manual“ to switch back with the selected tool to the “Length manual” window.

4.

Select the cutting edge number “D” and the number of the replacement tool “ST”.

5.

Approach the workpiece in the Z direction, scratch it with a turning spindle

6.

Enter the set position “Z0” of the workpiece edge.

7.

Press the VSK "Set length" softkey.

The tool length is calculated automatically and entered in the tool list. Note: If the tool length should be determined not with the help of a work piece but rather with a load cell, no zero offset may be selected, or the basis reference must be zero.

B570

Page 34


Section 6

Measure tool 6.4

Measure tool „Radius manual“ or “Diameter manual” By pressing the HSK 4 “Meas. tool” and the VSK 2 “Radius manual“ or “Diameter manual” (in the operating area “Machine“ and operating mode “JOG”) the following input mask opens.

6.4.1 Vertical Softkey bar (VSK) Display area

Description By pressing the VSK 2 “Tool” the tool list opens. See module B573 - „Operating area Parameter“. By pressing the VSK 7 “Set radius“ (or “Set diameter.”) all entered values will be accepted. By pressing the VSK 8 “Back“ you jump back to the “Measure tool” screen of the Sinumerik Operate“.

6.4.2 Parameters measure tool “Radius manual“ or “Diameter manual” The following parameters of the function “Length manual” are used also with “Radius manual” and “Diameter manual”: [T, D, ST] Beside the before mentioned parameters you find the following additional parameters in the “Radius manual” or “Diameter manual” window: Parameter

Description

X0

Workpiece edge

Y0

Workpiece edge


Notes:

Section 6 Notes:

Measure tool 6.4.3 Procedure for measuring the tool “radius manual” (or “diameter manual” ) 1.

Insert the tool you want to measure in the spindle.

2.

In the operating mode “JOG“ and operating area “Machine” press the HSK 4 “Meas. tool“.

3.

Press the VSK 2 “Radius manual“ ( or “Diameter manual“).

4.

Select the cutting edge number “D” and the number of the replacement tool “ST” of the tool.

5.

Approach the workpiece in the X- or Y-direction and perform scratching with the spindle rotating in the opposite direction.

6.

Specify the setpoint position “X0” or “Y0” of the workpiece edge.

7.

Press the "Set radius" or "Set diameter" softkey.

The tool radius or diameter is calculated automatically and entered in the tool list.

B570

Page 36


Section 6

Measure tool 6.5

Measure tool “Length auto“ By pressing the HSK 4 “Meas. tool” and the VSK 3 “Length auto“ (in the operating area “Machine“ and operating mode “JOG”) the following input mask opens:


Description By pressing the VSK 2 „Tool“ the tool list opens. See module B573 - “Operating area Parameter“. By pressing the VSK 8 “Back“ you switch back to the “Measuring tool” main window.

6.5.2 Parameter for measuring the tool length automatically The following parameters that are available for “Length manual” are available for “Length auto” too: [T, D, ST] With “Length auto” the following additional parameter is available: Parameter

Unit

Description

V

[mm]

Lateral offset


Notes:

Section 6 Notes:

Measuring a tool 6.5.3 Procedure for tool measure “length auto” 1.


2.

Position the tool near the tool probe, so that you can approach the probe collision free.

3.


4.

Press the HSK 3 “Length auto“.

5.


6.

If necessary, enter the lateral offset “V”.

7.

Press “CYCLE START“ on the machine control panel (MCP). This starts the automatic measuring process.

The tool length is calculated automatically and entered in the tool list. Note: How the measuring process works exactly depends on the settings of the machine manufacturer.

B570

Page 38


Section 6

Measure tool 6.6

Measure tool “Radius auto” or “Diameter auto” By pressing the HSK 4 “Meas. tool” and the VSK 2 “Radius auto“ or “Diameter auto” (in the operating area “Machine“ and operating mode “JOG”) the following input mask opens:


Description By pressing the VSK 2 “Tool“ the tool list wil be opened. See module B573 - “Operating area Parameter“. By pressing the VSK 8 “Back“ you switch back to the “Meas. Tool” screen.

6.6.2 Parameters of measure tool “Radius auto” or “Diameter auto” The following parameters that are available for “Length manual” are available for “Radius auto” or “Diameter auto” too: [T, D, ST] With “Radius auto” or “Diameter auto” the following additional parameters are available: Parameter

Unit

Description

V

[mm]

Lateral offset


Notes:

Section 6 Notes:

Measure tool 6.6.3 Procedure for tool measure “radius auto” or “diameter auto” 1.


2.

Position the tool near the tool probe, so that you can approach the probe collision free.

3.


4.

Press the VSK 4 “Radius auto“ or “Diameter auto“.

5.


6.

If necessary, enter the lateral offset “V”.

7.

Press “CYCLE START“ on the machine control panel. This starts the automatic measuring process.

When you measure the tool radius or diameter, measurement is performed with a spindle rotating in the opposite direction. The tool radius and diameter are calculated automatically and entered in the tool list. Note: How the measuring process works exactly depends on the settings of the machine manufacturer.

B570

Page 40


Section 6

Measure tool 6.7

Selecting the function “Calibrate probe”

If you want to measure your tools automatically, you must first determine the position of the tool probe on the machine table with reference to the machine zero. Mechanical tool probes are typically shaped like a cube or a cylindrical disk. Install the tool probe in the working area of the machine (e.g on the machine table) and align it relative to the machining axes. You must use a mill-type calibration tool to calibrate the tool probe. You must enter the length and radius/diameter of the tool in the tool list beforehand. Note: Refer to the machine manufacturer's specifications.

By pressing the HSK 4 “Meas. tool” and the VSK 6 “Calibrate probe“ (in the operating area “Machine“ and operating mode “JOG”) the “Probe calibration” window opens.


Notes:

Section 6 Notes:

Measuring a tool 6.7.1 Vertical softkey bar (VSK) Display area

Description By pressing the VSK 8 “Back“ you switch back to the “Measure tool” window.

6.7.2 Parameters of measure tool “Calibrate probe” By calibrating the probe the following parameters are displayed: Parameter

Unit

Description

Length

[mm]

Automatic determination of the tool length by moving the tool against the probe.

[mm]

Automatic determination of the tool length and diameter by moving the tool against the probe.

or Length and diameter

6.7.3 procedure for tool measure “Calibrating probe” 1.

Move the calibration tool until it is approximately over the centre of the measuring surface of the tool probe.

2.

In the operating mode “JOG“ press the HSK 4 “Meas. tool“.

3.

Press the VSK 6 “Calibrate probe”.

4.

Choose whether you want to calibrate the length or the length and the diameter.

5.

Press the “CYCLE START“ key on the machine control panel.

Calibration is automatically executed at the measuring feedrate. The distance measurements between the machine zero and tool probe are calculated and stored in an internal data area.

B570

Page 42


Section 7

Position 7.1

Selecting the function “Position“

In order to implement simple machining sequences, you can traverse the axes to certain positions in manual mode. Note: The feedrate/rapid traverse override is active during traversing. By pressing the HSK 6 “Position” in the Operating area “Machine” and operating mode “JOG” the following input mask will be shown on the screen:

7.2


Display area

Description By pressing the VSK 5 “Rapid” the value of the set machine data for feed rate velocity in JOG is taken over in the parameter “F” (feed). Hint: The VSK 5 “Rapid” can also be pressed if the input field parameter “F” is not the active input field (highlighted in orange) By pressing the VSK 8 “Back” you switch back to the main screen of the Sinumerik Operate.


Notes:

Section 7 Notes:

Position 7.3

Parameters of “Position”

Parameter

Unit

Description

F

[mm/min] [mm/tooth]

Feed

X

[mm]

Target position of the selected axes [abs/inc]

Y Note: Several target positions can be entered. B-axis and C-axis are manufacturer specific. Follow the documentation of the machine manufacturer.

Z

SP

[Degree]

Target angle [abs, inc]

7.4. Procedure for positioning the axes 1.

Select the “JOG” operating mode.

2.

Press the HSK 6 “Position”.

3.

Specify the desired value for the feedrate “F”. - OR -

3.

Press VSK 5 "Rapid". *Rapid tr.* is displayed in the input field “F”.

4.

Enter the target position or the target angle for the axis or axes to be traversed.

5.

Press the "CYCLE START" button on the machine control panel. The axis is traversed to the specified target position.

Note: If target positions were specified for several axes, the axes are traversed simultaneously.

B570

Page 44


Section 8

Face milling 8.1

Selecting the function “Face milling”

You can use this cycle to face mill any workpiece. A rectangular surface is always machined. By pressing the HSK 7 “Face mill.” in the Operating area “Machine” and operating mode “JOG” the following input mask will be shown on the screen.

8.2


Display area

Description By pressing the VSK 1 „Select tool“ you can insert a tool. Select the desired tool in the tool list (e.g FACING_TOOL_D60) with the orange selection cursor and press VSK 1 “In program” With VSK 2 ”Graphic view” you can switchover between help screen and graphical view. With VSK 3 "lateral limitation left" you can specify the lateral limitation in “X-” direction. With VSK 4 "lateral limitation top" you can specify the lateral limitation in “Y+” direction. With VSK 5 "lateral limitation right" you can specify the lateral limitation in “X+” direction. With VSK 6 "lateral limitation bottom" you can specify the lateral limitation in “Y-” direction.


Notes:

Section 8

Face milling

Notes: Display area

Description (continuation) By pressing the VSK 7 “Cancel” you can escape the screen “face milling”. With pressing of VSK 8 ”Accept” the following program block is generated:

With “CYCLE START“ the cycle “Face milling” will be executed.

8.3

Parameters of “Face milling”

Parameter

Unit

Description

T

Tool name

D

Cutting edge number of the tool.

F

[mm/min] Feed [mm/tooth]

S V

[rpm] [m/min]

Machining

Spindle speed or constant cutting speed The following machining operations can be selected: Roughing Finishing

Direction Same direction of machining Alternating direction of machining

B570

X0 Y0 Z0

mm

Corner point 1 of surface in X direction (abs) Corner point 1 of surface in Y direction (abs) Height of blank (abs)

X1 Y1 Z1

mm

Corner point 2 of surface in X (abs or inc) Corner point 2 of surface in Y (abs or inc) Height of finished part (abs or inc)

DXY

mm %

Max. infeed in the XY plane (dependent on milling cutter diameter) Alternatively you can specify the plane infeed as a %, as a ratio plane infeed (mm) to milling cutter diameter (mm).

DZ

mm

Max. infeed in Z direction (only for roughing)

UZ

mm

Finishing allowance, depth

Page 46


Section 9

Handwheel 9.1

Selecting the function “Handwheel”

You can traverse the axes in the machine coordinate system (MCS) or in the workpiece coordinate system (WCS) via the handwheel. All axes are provided in the following order for handwheel assignment:  Geometry axes (X, Y, Z)  Channel machine axes (X1, Y1, Z1, C1) Note: Refer to the machine manufacturer's instructions. By pressing the HSK 2.6 “Handwheel” in the extended horizontal softkey bar the following input mask will be shown on the screen.

An input field for the assignment of the axes is offered for every handwheel on the machine. The axis-assignment can be made like described in the module B568 - "Basic operations". Besides there is the possibility to assign an axis directly to a handwheel using the corresponding softkey on the VSK. 9.2


The number of softkeys for the axis assignment is limited. For the assignment of all other axes refer to the module B568 - "Basic operations", Section 3.2 "Parameter selection". Generally you can switch through all available axes by repeatedly pressing the blue "SELECT"-key on the keyboard. Display area

Description

Geometry axes: By pressing the VSK 1 "X" the X-axis is assigned to the selected handwheel. By pressing the VSK 2 "Y" the Y-axis is assigned to the selected handwheel. By pressing the VSK 3 "Z" the Z-axis is assigned to the selected handwheel. 828D/840Dsl SINUMERIK Operate

Notes:

Section 9 Notes:

Handwheel Display area


Machine axes By pressing the VSK 4 "X1" the X1-axis is assigned to the selected handwheel. By pressing the VSK 5 "Y1" the Y1-axis is assigned to the selected handwheel. By pressing the VSK 6 "Z1" the Z1-axis is assigned to the selected handwheel. By pressing VSK 7 "C1" the C1-axis is assigned to the selected handwheel. By pressing the VSK 8 "Back" the Handwheel window is being closed. 9.3 Handwheel assignment 1.

In the operating mode “JOG“ (or “MDA” or “AUTO”) select the operating area “Machine”, then press the HSK 2.6 “Handwheel” in the extended horizontal softkey bar.

2.

The “Handwheel” window opens. A field for axis assignment will be offered for every connected handwheel.

3.

Place the cursor in the field next to the handwheel with which you wish to assign the axis (e.g. No. 1).

4.

Press the corresponding VSK to select the desired axis (e.g. "X"). - OR To open the "Axis" selection box using the "INSERT" key on the keyboard, navigate to the desired axis, and press the "INPUT" key. Selecting an axis also activates the handwheel (e.g., "X" is assigned to handwheel no. 1 and is activated immediately).

5.

9.4

Press the HSK 2.6 "Handwheel" again, or press the VSK 8 "Back", to close the "Handwheel" window. Deactivating the handwheel

1.

The cursor must be placed on the handwheel whose axis-assignment should be cancelled (e.g. No.1).

2.

By pressing the corresponding axis-softkey again the assignment is cancelled. - OR -

B570

2.

Open the input field “Axis” with the “INSERT”-key, navigate to the blank field, and press the yellow "INPUT"-key. The empty value will be accepted. Deactivating on of the axes also deactivates the Handwheel (e.g. “X” deactivates Handwheel No. 1)

3.

Press the HSK 2.6 "Handwheel" again, or press the VSK 8 "Back", to close the "Handwheel" window.

Page 48


Synchronized actions 10.1 Selecting the function “Synchronized actions” By pressing the HSK 2.7 “Synchronized actions” in the extended horizontal softkey bar in operation area “Machine” under operation mode “JOG” the following input mask will be shown on the screen.

You can display status information for diagnosing synchronized actions in the “Synchronized actions” window. You get a list with all currently active synchronized actions. In this list the synchronized action programming is displayed in the same form as in the part program. You can see the status of the synchronized action in the “Status” column. 

Waiting



Active



Blocked

Note: Refer to the machine manufacturer„s documentation for further in formation about the programmed synchronized actions.


Section 10 Notes:

Section 11 Notes:

Settings 11.1 Selecting the function “Settings” You can predefine millimetre or inch as the measuring units for the control unit. The change-over of the measurement units is done for the whole control. All necessary entries are thereby converted automatically into the new measurement units, e.g.:  Positional data  Tool corrections  Zero point offsets By pressing the HSK 2.8 “Settings” in the extended horizontal softkey bar in operation area “Machine” under operation mode “JOG” the following input mask will be shown on the screen.

11.2 Vertical softkey bar (VSK) Display area

Description By pressing the VSK 5 "Changeover inch" the measuring units are converted from the metric to the imperial (inch) dimension system. New values have to be entered in inches. By pressing this key the key function switches to "Changeover metric". By pressing the VSK 5 "Changeover metric" the measuring units are converted from the imperial (inch) to the metric dimension system. New values have to be metric. By pressing this key the key function switches to "Changeover inch". Accept the selection by pressing the VSK 8 “OK” or cancel by pressing the VSK 7 “Cancel”. By pressing the VSK 8 "Back" you switch back to the main screen of the Sinumerik Operate with extended HSK.

B570

Page 50


Section 11

Settings

Notes: 11.3 Measurement units [metric/imperial] Country specific settings of the measuring units are not displayed in the input masks. In the following table the measuring units metric and imperial are compared with one another. A switchover can be made in the "T,S,M," input mask or by pressing the HSK 2.8 “Settings” in the extended HSK-bar and VSK 5 “Changeover Inch” or “Changeover Metric” as mentioned before. metric

Inch

mm

in

mm/tooth

in/tooth

mm/min

in/min

mm/U

in/U

m/min

ft/min

11.4 Parameter setting for manual operation In the “Settings for manual mode“ window all configurations for manual operation can be done. Parameter

Unit

Meaning

Type of feedrate:  G94  G95

[mm/min] [mm/rev]

Axis feedrate/linear feedrate Revolutional feedrate

[mm/min] [mm/rev]

Axis feedrate/linear feedrate Revolutional feedrate

Setup feedrate:  G94  G95 Variable increment

Spindle speed

Enter the desired increment for axis traversal by variable increments [rpm]

Spindle speed in revolutions per minute

After inserting the values in the input fields, press the VSK 8 “Back“ to switch back to the main screen of the Sinumerik Operate in the extended view.


Section End

B570

Page 52


B571

1

Operating mode “MDA”

Brief description

Objective of the module: In this module you learn the different options of the operating mode “MDA” in the operating area “Machine“. Description of the module: This module describes how a program can be loaded directly from the program manager into the MDA-buffer and how the processing of the program is started. It will be explained how an edited program, created in the working window, is written from the MDAbuffer to any directory on the control unit. You learn how to create a directory and a workpiece file of the type *.WPD (workpiece directory. Furthermore the functions “Program control” and “Handwheel” will be explained.

Content: Operating mode “MDA“ “Load MDI“ “Save MDI“ Program control Handwheel Synchronized actions


Page 1


B571

B571

B571

Page 2


B551 Operating mode MDA: Description This module describes how a program can be loaded directly from the program manager into the MDA-buffer and how the processing of the program is started. It will be explained how an edited program, created in the working window, is written from the MDA-buffer to any directory on the control unit. You learn how to create a directory and a workpiece file of the type *.WPD (workpiece directory. Furthermore the functions “Program control” and “Handwheel” will be explained.

Operating mode MDA: START

Operating mode “MDA“

“Load MDI“

“Save MDI“

Program control

Handwheel

Synchronized actions

Operating mode MDA: END

Notes :


Page 3

B551

Section 2 Notes:

Operating mode “MDA” In "MDA" mode (Manual Data Automatic), you can enter G-code commands block-by-block and immediately execute them for setting up the machine. You can load an MDA program straight from the Program Manager into the MDA buffer. You may also store programs which were rendered or changed in the MDA operating window into any directory of the program manager. 2.1

Selecting the operating mode “MDA“

The operating mode “MDA“ can be selected as follows: Press the “MDA”-key on the operator panel (OP). The operating mode “MDA“ will be opened immediately. - OR Press the “MENU SELECT”-key on the operator panel. Press the VSK 2 “MDA“ in the yellow vertical softkey bar on the right side of the screen and the operating mode “MDA” will be opened immediately. Now switch to the operating area “Machine” by pressing the “MACHINE” key on the operator panel or on the keyboard or press the “MENU SELECT“key on the operator panel and the yellow HSK 1 “Machine“. The following screen opens:

In the operating mode “MDA“ the following softkeys are shown in the horizontal and vertical softkey bar of the Sinumerik Operate:

B571

Page 4


Operating mode “MDA” 2.2

Section 2 Notes:


Display area

Description By pressing the VSK 1.1 “G functions“ the most important G-functions are displayed in a window. Available auxiliary functions are displayed in a subwindow by pressing the VSK 1.2 "Auxiliary functions" at the time of the output. By pressing the VSK 1.5 “Delete blocks” entered program blocks can be deleted. By pressing the VSK 1.7 "Act. vls. MCS", the coordinate system will be toggled between the machine coordinate system (MCS) and the workpiece coordinate system (MCS). Note the machine manufacturer‘s documentation. By pressing the VSK 1.8 "Forward" on the operator panel (OP) the selection of additional softkeys on the vertical softkey bar 2 is possible By pressing the VSK 2.2 "All G functions" all Gfunctions will be shown. By pressing the VSK 2.6 "Zoom act. val." all actual values are displayed full screen. By pressing the VSK 2.8 "Back" on the operator panel (OP) the vertical softkey bar switches back to the menu of the VSK 1. The VSK-bar 1 is active again.


Page 5

B571

Section 2

Operating mode “MDA”

Notes: 2.3

Horizontal softkey bar 1 and 2

Display area

Description By pressing the HSK 1 “Load MDI” the “Load into MDI” with the program manager window opens. By pressing the HSK 2 “Save MDI” the “Save from MDI : Select storage location” with the program manager window opens. By pressing the HSK 4 “Prog. cntrl.“ the “Program control” subwindow opens on the screen. By pressing the "Extend"-button on the operator panel (OP) more softkeys on the HSK will be available. This symbol on the right of the dialogue line indicates that more options on the HSK are available. Press the “Extend”-button on the OP to open the extended HSK. This symbol indicates that you are in the extended softkey bar. Press the “Extend”-button on the operator panel to switch back to the main HSK. By pressing the HSK 2.6 "Handwheel" the input mask for traversing the axis in machine coordinate system (MCS) or workpiece coordinate system (WCS) will be available. By pressing the HSK 2.7 "Synchr. Action." the screen which shows the current synchronized actions is displayed.

B571

Page 6


“Load MDI” 3.1

Section 3 Notes:

Selecting the function “Load MDI” By pressing the HSK1 “Load MDI” the “Load into MDI” window with the Program Manger is displayed as below:

To navigate in the program manager window use the blue cursor-keys The following operation options are available in the vertical softkey bar to the right: 3.2


Display area

Description Press the VSK 7 “Cancel“ to close the “Load into MDI” window. By pressing the VSK 8 “OK” the marked program will be opened after closing the window “Load into MDI” and taken over in the MDI-window. If a program is already in the MDI-buffer, you will be asked to overwrite. Accept with “OK” or refuse with “Cancel”. A program loaded in the MDI-buffer can be edited or can be executed by pressing the “CYCLE START“-button on the MCP

3. 3

Loading a MDI-program

1.

Switch to operating mode “MDA“ (see section 2.1).

2.

Press the VSK 1 “Load MDA”. The “Load into MDI” Program manger window opens.

3.

Mark the program you want to load with the orange cursor-keys.

4

Press the VSK 8 “OK“.

The window closes and the program is ready for machining. 828D/840Dsl SINUMERIK Operate

Page 7

B571

Section 4 Notes:

“Save MDI“ 4.1

Selecting the function “Save MDI” By pressing the HSK2 “Save MDI” the “Save from MDI : Select storage location” window with the Program Manger is displayed as below:

Navigate through the program manager window by means of the blue cursor-keys. The following softkeys are available in the vertical softkey bar. 4.2


Display area

Description By pressing the VSK 1 “New directory“ a new directory can be created in the “Local drive” folder. An input window opens where a name can be entered for the new directory that is to be created. Create a new directory by pressing the VSK 8 “OK” or abort with pressing the VSK 7 “Cancel”. The “New directory”-softkey is not active if you have placed the cursor on or in the “NC data” directory. By pressing the VSK 3 “Workpiece” a new workpiece of the type WPD (workpiece directory) can be created. The current cursor position determines the location of the folder. An input window opens, where a name can be entered. By pressing “OK” the window “New G-Code program” is being opened. After selecting the file type (Main program: MPF/ Subprogram: SPF) and entering the filename, the program is saved from the MDA-Buffer into the created directory. The “Workpiece”-softkey only becomes active if the cursor is placed on or in the “Workpieces” folder of the “NC data” section.

B571

Page 8


“Save MDI“ Display area

Section 4 Description (continuation)

Notes:

By pressing the VSK 7 “Cancel” the “Save from MDI” window will be closed without saving. By pressing the VSK 8 “OK”, with the cursor on a folder, the “New G code program” window opens. Select the file type (Main program: MPF/ Subprogram: SPF) that you wish to create. After input of the filename the program will be written from the MDI-buffer to the new created file or the file that is marked with the cursor.

4.3 Saving a MDI-program 1.

Select the operating mode “MDA” (see section 2.1) The “MDI” editor opens.

2.

Create the MDI program by entering the G-code commands using the keyboard.

3.

Press the VSK 2 "Save MDI”. The "Save from MDA : Select storage location" window opens. It shows you a view of the program manager.

4.

Select the drive to which you want to save the MDI program you have created, and place the cursor on the directory in which the program is to be stored.

5.

Press the VSK 8 “OK“. Note: When you place the cursor on a folder, a window opens which prompts you to assign a program name. When you place the cursor on a program, you are asked whether the file should be overwritten or not.

7.

Enter a name for the program and press the VSK 8 “OK“.

The program will be saved under the specified name in the selected directory.


Page 9

B571

Section 5 Notes:

Program control 5.1

Selecting the function “Program control“ By pressing the HSK 4 “Prog. cntrl.“ the “Program control” window will be opened, as displayed below.

Navigate with the blue cursor-up and cursor-down through the option fields. To activate or deactivate a “program control” option press the “SELECT”-key on the machine control panel. The following program control options are available: Abbreviation/ Program control PRT no axis motion

Scope The program is started and executed with auxiliary function outputs and dwell times. In this mode, the axes are not traversed. The programmed axis positions and the auxiliary function outputs are controlled this way. Note: Program processing without axis motion can also be activated with the function "Dry run feedrate".

DRY Dry run feedrate

The traversing velocities programmed in conjunction with G1, G2, G3, CIP and CT are replaced by a defined dry run feedrate. The dry run feedrate also applies instead of the programmed revolutional feedrate. Caution: Workpieces should not be machined when "Dry run feedrate" is active, because the altered feedrates might cause the permissible tool cutting rates to be exceeded and the workpiece or machine tool could be damaged.

B571

Page 10


Section 5

Program control

Notes:

Abbreviation/ Program control

Scope (continuation)

RG0 Reduced rapid trav.

In the rapid traverse mode, the traversing speed of the axes is reduced to the percentage value entered in RG0. (Please refer to chapter 9.1 in module B572)

M01 Programmed stop 1

The processing of the program stops at every block in which supplementary function “M01” is programmed. In this way you can check the already obtained result during the processing of a workpiece. Note: In order to continue executing the program, press the "CYCLE START" key again.

Programmed stop 2 (e.g. M101)

The processing of the program stops at every block in which the "Cycle end" is programmed (e.g. with M101). Note: In order to continue executing the program, press the "CYCLE START" key again. This function must be projected via a machine datum. Refer to the machine manufacturer‘s documentation.

DRF Handwheel offset

Enables an additional incremental zero offset while processing in automatic operation mode with an electronic handwheel. This function can be used to compensate for tool wear within a programmed block.

SB

Individual blocks are configured as follows:  SB 1 - Single block, coarse: The machining stops only after blocks that perform a machine function (exept for cycles).  SB 2 - Data block: The machining stops after each block; also for data blocks (except for cycles).  SB 3 - Single block, fine: The machining stops after each machine block (also in cycles). Select the desired setting using the "SELECT" key. The activation of the function “Single block” takes place by pressing “SINGLE BLOCK” on the machine control panel.

SKP

Skip blocks are skipped during machining.


Page 11

B571

Section 5

Program control

Notes: 5.2


Display area

Description By pressing the VSK 8 “Back“ you can switch back to the “Program control” window in “MDA” mode.

5.3 Controlling the program run 1.

In the operating mode “MDA” select the HSK 4 „Progr. cntrl.“. The “Program control” window opens.

B571

2.

Select the desired program control (see Section 5.1 in this module).

3.

Press the VSK 8 “Back” to switch back to the main screen of the Sinumerik Operate in “MDA”-operating mode.

Page 12


Section 6

Handwheel 6.1

Notes:

Selecting the function “Handwheel“

You can traverse the axes in the machine coordinate system (MCS) or in the workpiece coordinate system (WCS) via the handwheel. All axes are provided in the following order for handwheel assignment:  Geometry axes (X, Y, Z)  Channel machine axes (X1, Y1, Z1, C1) By pressing the HSK 2.6 “Handwheel” in the extended horizontal softkey bar the following input mask will be shown on the screen.

An input field for the assignment of the axes is offered for every handwheel parameterised on the machine. The axis-assignment can be made like described in the module B568 - "Basic operations". Besides there is the possibility to assign an axis directly to a handwheel using the corresponding softkey on the VSK. 6.2


The number of softkeys for the axis assignment is limited. For the assignment of all other axes refer to the module B568 - "Basic operations", Section 3.2 "Parameter selection". Generally you can switch through all available axes by repeatedly pressing the blue "SELECT"-key on the keyboard. Display area

Description

Geometry axes By pressing the VSK 1 "X" the X-axis is assigned to the selected handwheel. By pressing the VSK 2 "Y" the Y-axis is assigned to the selected handwheel. By pressing the VSK 3 "Z" the Z-axis is assigned to the selected handwheel. 828D/840Dsl SINUMERIK Operate

Page 13

B571

Section 6

Handwheel

Notes: Display area


Machine axes By pressing the VSK 4 "X1" the X1-axis is assigned to the selected handwheel. By pressing the VSK 5 "Y1" the Y1-axis is assigned to the selected handwheel. By pressing the VSK 6 "Z1" the Z1-axis is assigned to the selected handwheel. By pressing VSK 7 "C1" the C1-axis is assigned to the selected handwheel. By pressing the VSK 8 "Back" you can switch back to the main screen of the Sinumerik Operate with extended HSK-bar. 6.3 Handwheel assignment 1.

In the operating mode “MDA“ (or “JOG” or “AUTO”) select the operating area “Machine”, then press the HSK 2.6 “Handwheel” in the extended horizontal softkey bar.

2.


3.

Place the cursor in the field next to the handwheel with which you wish to assign the axis (e.g. no. 1).

4.

Press the corresponding softkey to select the desired axis (e.g. "X"). - OR To open the "Axis" selection box using the "INSERT" key, navigate to the desired axis, and press the "INPUT" key. Selecting an axis also activates the handwheel (e.g., "X" is assigned to handwheel no. 1 and is activated immediately).

5.

Press the HSK 2.6 "Handwheel" again - OR Press the VSK 8 "Back". The "Handwheel" window closes.

B571

Page 14


Section 6

Handwheel

Notes:

6.4 Deactivating the handwheel 1.

The cursor must be placed on that handwheel whose axis-assignment should be cancelled.

2.

By pressing the corresponding axis-softkey again the assignment is cancelled. -ORAlternatively with pressing the “INSERT”-key, the selection menu with all available axes can be opened.

3.

By using the blue “Cursor-up”- and “Cursor-down”keys on the keyboard, switch to the empty field on top of the menu and press the yellow "INPUT"-keys on the keyboard. The empty value will be accepted. The corresponding handwheel is now deactivated.


Page 15

B571

Section 7 Notes:

Synchronized actions 7.1

Selecting the function “Synchronized actions”

By pressing the HSK 2.7 “Synchronized actions” on the extended horizontal Softkey-bar, in the operation area “Machine” in operation mode “MDA” , the following mask will be shown on the screen.


Waiting



Active



Blocked

Note: Refer to the machine manufacturer‘s documentation for further in formation about the programmed synchronized actions.

B571

Page 16


B572

1

Operating mode “AUTO”

Brief description

Objective of the module: In this module you learn the different options of the operating mode "AUTO" in the operating area "Machine".

Description of the module: This module describes, how to overstore technological parameters (for example, auxiliary functions, axis feed, spindle speed, programmable instructions, etc.) for a program run in the main memory of the NCK. It is described among other things, how the execution of a program can be stopped at a specific part of the program run with the function “Program control“ (programmed stop). The differences between the two block search modes (with or without calculation) will be explained in detail as well as the function “Simultaneous recording”. The handwheel assignment and the functions “Settings” and “Synchronized actions” complete this module.

Content: Operating mode “AUTO“ Overstore Program control Block search Simultaneous recording Program correction Handwheel Synchronized actions Settings


Page 1


B572

B572

B572

Page 2


B572 Operating mode AUTO: Description This module describes, how to overstore technological parameters (for example, auxiliary functions, axis feed, spindle speed, programmable instructions, etc.) for a program run in the main memory of the NCK. It is described among other things, how the execution of a program can be stopped at a specific part of the program run with the function “Program control“ (programmed stop). The differences between the two block search modes (with or without calculation) will be explained in detail as well as the function “Simultaneous recording”. The handwheel assignment and the functions “Settings” and “Synchronized actions” complete this module.

Operating mode AUTO: START Settings

Operating mode “AUTO“ Operating mode AUTO: END Overstore

Program control

Block search

Simultaneous recording

Program correction

Handwheel

Synchronized actions

Notes :


Page 3

B572

Section 2 Notes:

Operating mode “AUTO” 2.1

Selecting the operating mode “AUTO”

The operating mode “AUTO” can be selected as follows: Press the “AUTO“ button on the machine control panel (MCP). The operating mode “AUTO” opens directly. - OR Press the button “MENU SELECT“ on the machine control panel. Press the VSK 1 “AUTO“ in the yellow VSK-bar on the right hand side of the screen to switch directly to the operating mode “AUTO“. Next, switch to the operating area “Machine” by pressing the “MACHINE”-key on the operator panel or the keyboard else press the “MENU SELECT“key on the operator panel and the yellow HSK 1 “Machine“. The following screen opens:

The following softkeys will be shown in the vertical and horizontal softkey bars: 2.2

Vertical softkey bar 1 and 2

Display area

Description By pressing the VSK 1.1 “G functions“ the most important G-functions will be displayed. By pressing the VSK 1.2 “Auxiliary functions“, available auxiliary functions will be displayed at the time of the output. By pressing the VSK 1.3 “Basic blocks“ all G-code commands that trigger a function on the machine will be displayed. The display updates both in the test operation and in the actual machining of the workpiece at the machine.

B572

Page 4


Operating mode “AUTO” Display area

Section 2


Notes:

By pressing the VSK 1.4 “Time counter“ the program run time, the rest of the program run time and the amount of machined workpieces will be displayed. Note: Refer to the machine manufacturer‟s documentation. By pressing the VSK 1.5 “Program levels“ you can display the current program level during the execution of a large program with several subprograms. By pressing the VSK 1.7 “Act vls. MCS” you can switch over from the machine coordinate system (MCS) to the workpiece coordinate system (WCS). Note: Refer to the machine manufacturer‟s documentation. By pressing the VSK 1.8 "Extend" on the operator panel (OP) you switch to the vertical softkey bar 2 with additional softkeys displayed. By pressing the VSK 2.2 “All G functions” all Gfunctions will be displayed. By pressing the VSK 2.6 “Zoom act. val.“ all actual values will be displayed full-screen. By pressing the VSK 2.8 “Back” on the operator panel you can switch back to the vertical softkey bar 1.

2.2 Horizontal softkey bar 1 and 2 Display area Description Pressing the HSK 1.2 “Overstore” allows you to overstore technological parameters (for example, auxiliary functions, axis feed, spindle speed, programmable instructions, etc.) for a program run in the main memory of the NCK. By pressing the HSK 1.4 “Prog. cntrl.” the working window for controlling the program run will be opened. By pressing the HSK 1.5 “Block search” the block search window opens. By pressing the HSK 1.7 “Simultaneous recording“ you can graphically display the execution of the program on the screen before or during machining of the workpiece, to monitor the result of the programming.


Page 5

B572

Section 2 Notes:

Operating mode “AUTO” Display area

Description (continuation) By pressing the HSK 1.8 “Prog. corr.“ (program correction) the program editor opens. By pressing the "Extend"-button on the operator panel you can switch between the normal and the extended horizontal softkey bar. This symbol on the right of the dialogue line indicates that more softkeys are available on the extended horizontal softkey bar. This symbol indicates that the extended horizontal softkey bar is shown on the screen. You can switch back to the HSK 1 again by pressing the “Extend”key. By pressing the HSK 2.6 "Handwheel" the input mask for assigning axes to all parameterized handwheels is displayed. By pressing the HSK 2.7 "Synchr. Action." the screen which shows the current synchronized actions is displayed. By pressing the HSK 2.8 "Settings" a window opens up where you can adjust the settings for manual operation on the Sinumerik Operate.

B572

Page 6


Section 3

Overstore 3.1

Notes:

Selecting the Function “Overstore“ By pressing the HSK 1.2 “Overstore“ the “Overstore” window opens (see picture below).

The program to be corrected has to be in the STOP or RESET mode. In the “Overstore” editor view you can overstore technological parameters (for example, auxiliary functions, axis feed, spindle speed, programmable instructions, etc.) for a program run in the main memory of the NCK. The programs in the part program memory are not changed while using the function “Overstore”. You cannot change the operating mode while you are in overstore mode. 3.2


Display area

Description By pressing the VSK 1.5 “Delete blocks” you can delete the blocks you have entered before.

3.3

By pressing the VSK 1.8 “Back“ the window is being closed. A change of the operation mode is now possible. Press “CYCLE START“ to continue running the previously selected program. Procedure for „Overstore“

1.

Open a program in the operating mode “AUTO” then press the HSK 1.2 “Overstore”. The “Overstore” window opens.

2.

Enter the required data and NC block.

3.

Press the “CYCLE START” key. The blocks you have entered are stored. You can observe execution in the "Overstore" window. After the entered blocks have been executed, you can append blocks again.

4.

Press the VSK 8 "Back". The "Overstore" window closes.

5.

Press the “CYCLE START” key again. The program selected before overstoring continues to run.


Page 7

B572

Section 4 Notes:

Program control 4.1

Selecting the function “Program control” By pressing the HSK 1.4 “Prog. cntrl.“ the “Program control” window opens like displayed below:

Navigation through the option menu takes place by pressing the blue Cursor keys on the keyboard. You can activate or deactivate an option by selecting the entry first and then pressing the blue “SELECT“ key. The following program control options are selectable: Abbreviation/ Program control

Scope

PRT No axis motion

The program is started and executed with auxiliary function outputs and dwell times. In this mode, the axes are not traversed. The programmed axis positions and the auxiliary function outputs are controlled this way. Note: Program processing without axis motion can also be activated with the function "Dry run feedrate".

DRY Dry run feedrate

The traversing velocities programmed in conjunction with G1, G2, G3, CIP and CT are replaced by a defined dry run feedrate. The dry run feedrate also applies instead of the programmed revolutional feedrate. Caution: Workpieces must not be machined when "Dry run feedrate" is active because the altered feedrates might cause the permissible tool cutting rates to be exceeded and the workpiece or machine tool could be damaged.

B572

Page 8


Section 4

Program control

Notes:

Abbreviation/ program control

Scope (Continuation)

RG0 Reduced rapid trav.

In the rapid traverse mode, the traversing speed of the axes is reduced to the percentage value entered in RG0. (Please refer to chapter 9.1 in this module)

M01 Programmed stop 1

The processing of the program stops at every block in which supplementary function “M01” is programmed. In this way you can check the already obtained result during the processing of a workpiece. Note: In order to continue executing the program, press the "CYCLE START" key again.

Programmed stop 2 (e.g. M101)

The processing of the program stops at every block in which the "Cycle end" is programmed (e.g. with “M101”). Note: In order to continue executing the program, press the "CYCLE START" key again. The display can be changed. Please also refer to the machine manufacturer's instructions.

DRF Handwheel offset

Enables an additional incremental zero offset while processing in automatic operation mode with an electronic handwheel. This function can be used to compensate for tool wear within a programmed block.

SB

Individual blocks are configured as follows:  SB 1 - Single block, coarse: The program stops only after blocks which perform a machine function.  SB 2 - Data block: The program stops after each block.  SB 3 - Single block, fine: The program stops also in cycles after blocks, which perform a machine function. Select the desired setting using the "SELECT" key on the keyboard. The selection of the function “Single block” takes place by pressing the “SINGLE BLOCK”-key on the machine control panel (MCP).

SKP

Skipped blocks are skipped during machining.


Page 9

B572

Section 4

Program control

Notes: 4.2


Display area

Description By pressing the VSK 8 “Back” you return to the window “Program control”.

4.3 Controlling the program run 1.

In the operating mode “AUTO“ and the operating area “Machine” press the HSK 4 “Prog. cntrl.“. The “Program control” window opens and shows a list of program control options.

2.

Select the desired program control (see section 4.1 in this module).

3.

Press the VSK 8 “Back” to go back to the main screen of the Sinumerik Operate in the operating mode “AUTO” and operating area “Machine”. Hint: The orange selection cursor disappears, if a skip block is confirmed with the yellow “INPUT”-key. With the blue “cursor to the left” or “cursor to the right” you return again to the selection mode.

B572

Page 10


Section 5

Block search 5.1

Notes:

Selecting the function “Block search” By pressing the HSK 1.5 “Block search” the “block search” window opens as shown below.

If you would only like to perform a certain section of a program on the machine, then you don’t have to start the program from the beginning. You can also start the program from a specified program block. Applications of this function are to stop or interrupt program execution and to specify a target position (e.g. during machining). Determination of search targets per: a. Comfortable search target definitions (search positions)  Direct specification of the search target by positioning the cursor in the selected program (main program).  Search target via text search.  The search target is the interruption point (main program and subprogram). The function is only available if there is an interruption point. After a program interruption (“CYCLE STOP” or “RESET”), the controller saves the coordinates of the interruption point.  The search target is the higher program level of the interruption point (main program and subprogram). The level can only be changed if it was previously possible to select an interruption point in a subprogram. It is then possible to change the program level up to the main program level and back to the level of the interruption point. - OR -


Page 11

B572

Section 5 Notes:

Block search b. Search pointer  Direct entry of the program path in the “Search pointer“ window.

If a search target was found, it is possible to start another search run immediately. This can be done many times after every successful search run. Attention: Pay attention to a collision-free starting position as well as accurate active tools and other technological values. If necessary move the tool to a save starting position. Select the target block considering the selected block search type. Navigation through the program blocks takes place by using the blue cursor-keys on the keyboard. The following functions are available in the vertical softkey bar:

5.2 Vertical softkey bar Display area

Description By pressing the VSK 1 “Start search“ the search run starts depending on the search mode you have selected before. Press the VSK 1 several times, until the found target (z.B. with search text) corresponds to the searched program block. By pressing the VSK 2 “Blk. sear. mode“ the “Block search mode” window opens. Two different block search modes are selectable: With calculation:  Without approach: It is used in order to be able to approach a target position in any circumstance (e.g. tool change position). The end position of the target block or the next programmed position is approached using the type of interpolation valid in the target block. Only the axes programmed in the target block are moved.  With approach: It is used to be able to approach the contour in any circumstance. The end position of the block prior to the target block is found with "CYCLE START". The program runs in the same way as in normal program processing.

B572

Page 12


Section 5

Block search Display area


Notes:

Without calculation:  For a quick search in the main program. Calculations will not be performed during the block search, i.e. the calculation is skipped up to the target block. All settings required for execution have to be programmed from the target block (e.g. feedrate, spindle speed, etc.). Pressing the VSK 3 “Higher level“ changes the program level to one level higher. Pressing the VSK 4 “Lower level“ changes the program level to one level lower. By pressing the VSK 5 “Search for text“ the “Search” window opens. After entering the search direction in the “Direction” field and the search text in the “Text” field and by pressing the VSK 8 “OK” the search run starts. After a successful search you can search for the same search parameter again, by pressing the VSK 8 “Continue search”. The search can be cancelled by pressing the VSK 7 “Cancel”. A new search run with new search parameters can be initiated with the VSK 4 “Search”. By pressing the VSK 6 “Interrupt point” the program that was interrupted before, by pressing the “RESET” key, will be executed again. By pressing the VSK 7 “Search pointer“ you can jump directly to a desired part of the program. The following options are available in a list in the “Search pointer” window:  Program The name of the currently loaded program is automatically entered  Ext. File extension  P Pass counter: If a program section is performed several times, you can enter the number of the pass here at which processing is to be continued  Line Is automatically filled for an interruption point


Page 13

B572

Section 5 Notes:

Block search Display area

Description (continuation)  Type  N no.:  Label:  Text:  Subprg.:  Line:

Block number Jump label Text string Subprogram call Line number

 Search target Search target point in the program at which machining is to start By pressing the VSK 8 “Back” the “Search” window closes. 5.3 Starting a block search 1.

A desired program is selected and the machining was discontinued with pressing “RESET” or “CYCLE STOP“ or the control unit is generally in RESET state.

2.

In the operating mode “AUTO“ and the operating area “Machine” press the HSK 5 “Block search”. For further steps see below:

Simple search target definition: Steps 1 and 2 (see above). 3.

Place the cursor on a particular program block. - OR Press the VSK 5 "Search for text", select the search direction, enter the search text and confirm with the VSK 8 "OK".

4.

Press the VSK 1 “Start search“. The search starts. Your specified search mode will be taken into account (indicated in the upper blue title bar of the search target window). The current block will be displayed and marked in the "Program" window as soon as the target is found.

B572

5.

If the located target (for example, when searching via text) does not correspond to the program block, press the "Start search" softkey again until you find your target.

6.

Press the "CYCLE START"-key twice. Processing is continued from the defined position.

Page 14


Section 5

Block search

Notes:

Interruption point as search target: 1. - 2.

Steps 1 and 2 (see above).

3.

Press the VSK 6 “Interrupt point“ The interruption point is loaded.

4.

If the VSK 3 "Higher level" and the VSK 4 "Lower level" are available, use these to change the program level.

5.

Press the VSK 1 "Start search". The search starts. The specified search mode will be taken into account (indicated in the upper blue title bar of the search target window). The search screen closes. The current block will be displayed and marked in the "Program" window as soon as the target is found.

6.

Press the "CYCLE START"-key on the machine control panel (MCP) twice. The execution will continue from the interruption point.

Search target via search pointer: Steps 1 and 2 (see above). 3.

Press the VSK 7 “Search pointer”. The “Search pointer” window opens.

4.

Enter the full path of the program as well as the subprograms, if required, in the input fields.

5.

Press the VSK 1 “Start search”. The search starts. The specified search mode will be taken into account (indicated in the upper blue title bar of the search target window). The search screen closes. The current block will be displayed and marked in the "Program" window as soon as the target is found.

6

Press the "CYCLE START" key on the machine control panel twice. Processing is continued from the defined location.


Page 15

B572

Section 6 Notes:

Simultaneous recording 6.1

Selecting the function “Simultaneous recording” Pressing the HSK 1.7 “Simult. Record.“ opens the simultaneous recording window.

Before machining the workpiece on the machine, you can graphically display the execution of the program on the screen to monitor the result of the programming. You can replace the programmed feedrate with a dry run feedrate to influence the speed of execution. Simultaneous record can also be turned on, if machining is already running. You can also use simultaneous recording during machining of a workpiece. This helps if the view towards the inside of the cabin is obstructed by coolant. In each different view of the “Simultaneous recording” window you can adjust the view by using the blue cursor keys and zoom in or out by using the plus (“+”) and minus (“-”) keys on the keyboard. The traversing paths of the tool in the “Simultaneous recording” window are displayed in different colours: red for rapid traverse and green for feed motion. The following softkeys, each representing a different view on the simulated workpiece, are available on the vertical softkey bars.

6.2 Vertical softkey bar 1 and 2 Display area

Description By pressing the VSK 1.3 “Top view” the work piece will be shown in a plan view from the top. By pressing the VSK 1.4 “3D view“ the work piece will be shown in a 3-D view. By pressing the VSK 1.5 “Further views“ the vertical softkey bar 3 opens with options to change to different views of the workpiece (see section 6.3).

B572

Page 16


Section 6

Simultaneous recording Display area


Notes:

By pressing the VSK 1.6 “Details“ the vertical softkey bar 4 opens (see section 6.4 in this module). By pressing the VSK 1.7 “Extend” on the operator panel the softkeys of the vertical softkey bar 2 will be shown. By pressing the VSK 1.8 “Back” you switch back to the main screen of the operating area “Machine” in the operating mode “AUTO”. By pressing the VSK 2.1 “Show tool path” the animated path display that follows the programmed tool path of the selected program is shown on the screen. Press this softkey again to turn off the function. The traversing paths are shown in two different colours: red colour for rapid traverse and green colour for feed motion. By pressing the VSK 2.2 “Delete tool path” all tool paths so far generated, including tool paths generated in the background, are deleted. By pressing the VSK 2.3 “Blank“ the “Blank input” window opens. Here, the zero offset, the form and the dimensions of the blank can be entered,. By pressing the VSK 2.8 “Back“ on the operator panel you switch back to the vertical softkey bar 1. 6.3

Vertical softkey bar 3 (from VSK 1.5 “Further views“)

Display area

Description By pressing the VSK “2 windows“ the screen is split into two different views of the workpiece. The 2 -windowed view contains a side view (left-hand window) and a front view (right-hand window) of the workpiece. The viewing direction is always from the front to the cutting surface even if machining is to be performed from behind or from the back side. The active view is shown with a white background. You can switch between both windows by pressing the “NEXT WINDOW” key on the keyboard.

6.4

Vertical softkey bar 4 (from VSK 1.6 “Details“)

Display area

Description By pressing the VSK 4.1 “Autozoom“ the workpiece will be aligned in an optimal way on the screen, so that it fits the whole window. By pressing the VSK 4.2 “Zoom +“ you zoom in to magnify the graphical representation of the workpiece in the window. Alternatively you can press the plus (“+”) key on the number block of the keyboard.


Page 17

B572

Section 6 Notes:

Simultaneous recording Display area

Description (continuation) By pressing the VSK 4.3 “Zoom -“ you zoom out of the window to reduce the graphical representation of the workpiece. Alternatively you can press the minus (“-”) key on the number block of the keyboard. By pressing the VSK 4.4 “Zoom” a zoom window in the shape of a right angled frame is placed on the screen. With the VSK “Zoom +” and the VSK “Zoom -” you can increase or decrease the size of the right angled frame and therefore the zoom-factor. Alternatively you can use the plus (“+”) or minus (“-”) key on the keyboard. The blue cursor keys on the keyboard are used to pan the frame on the screen, adjusting the fragment you wish to magnify. After pressing the VSK 8 “OK” the screen will be zoomed in to the extend of the frame window. You can exit the Zoom function with the Softkey “Cancel” By pressing the VSK 4.5 “Rotate view” the vertical softkey bar 5 opens (see section 6.5). By pressing the VSK 4.8 “Back“ on the operator panel you switch back to the vertical softkey bar 1.

6.5

Vertical softkey bar 5 (from VSK 4.5 “Rotate view“)

Display area

Description By pressing the VSK 5.1 the workpiece will be turned right around its own vertical centre line. By pressing the VSK 5.2 the workpiece will be turned left around its own vertical centre line. By pressing the VSK 5.3 the workpiece will be turned upwards around its own horizontal centre line. By pressing the VSK 5.4 the workpiece will be turned downwards around its own horizontal centre line. By pressing the VSK 5.5 the workpiece will be turned left (counter clockwise) around the centre of the screen. By pressing the VSK 5.6 the workpiece will be turned right (clockwise) around the centre of the screen. By pressing the VSK 5.8 „Back“ on the operator panel you switch back to the vertical softkey bar 4.

B572

Page 18


Section 6

Simultaneous recording 6.6 Simultaneous recording of a program run

Notes:

Simultaneous recording before machining of the workpiece 1.

Load a program in the operating mode “AUTO”.

2.

Press the HSK 1.4 “Prog. cntrl.“ and activate the checkboxes "PRT No axis motion" and "DRY Dry run feedrate". The program is executed without axis movement. The programmed feedrate is replaced by a dry run feedrate. -ORLet the “DRY Dry run feedrate” box unchecked. Simultaneous recording is performed with the programmed feedrate.

3.

Press the HSK 7 “Simultan. record“. The “Simultaneous recording” window opens.

4.

Press the “CYCLE START” key on the machine control panel (MCP). The execution of the program on the machine is started and displayed graphically on the screen.

5.

Press “CYCLE STOP” to stop machining and the HSK 7 "Simultan. record" again to close the “Simultaneous recording” window.

Simultaneous recording during machining of the workpiece 1.

Load a program in the operating mode “AUTO”.

2.

Press the HSK 7 “Simultan. record“. The “Simultaneous recording” window opens.

3.

Press the “CYCLE START”-key on the machine control panel (MCP). The machining of the workpiece is started and graphically displayed on the screen.

4.

Press the “CYCLE STOP”-key and the HSK 7 "Simultan. record" again to stop the recording and to close the “Simultaneous recording” window.


Page 19

B572

Section 7 Notes:

Program correction As soon as a syntax error in the part program is detected by the controller, program execution is interrupted and the syntax error is displayed in the alarm line. Depending on the state of the control, you can make the following corrections using the “Program correction” function:  STOP mode: Only program lines that have not yet been executed can be edited.  RESET state: All program lines can be edited Note: The "Program correction" function is only available for part programs in the NC memory, not for external execution (e.g. on USB media).

7.1

Selecting the function “Program correction” By pressing the HSK 1.8 “Prog. Corr.“ the program editor window opens for correction of the program. See modules B600 and B604 “Basics of programming”.

7.2


A precise description of the vertical softkeys can be found in the modules B600 and B604 “Basics of programming”.

B572

Page 20


Section 7

Program correction

Notes:

7.3 Correcting a program 1.

The program to be corrected is in the STOP or RESET mode.

2.

Press the HSK 8 “Prog. corr.“. The selected program is opened in the editor. The program pre-processing and the current block are displayed. The current block is also updated in the running program, but not the displayed program section, i.e. the current block moves out of the displayed program section. If a subprogram is executed, it is not opened automatically.

3.

Make the necessary corrections.

4.

Press the HSK 8 "NC Execute". The system switches back to the "Machine" operating area and selects operating mode "AUTO".

5.

Press the “CYCLE START“ key on the machine control panel (MCP). The program execution is resumed. Note: Leaving the program editor via the VSK 2.7 “EXIT“, opens the operating area “Program Manager”.


Page 21

B572

Section 8 Notes:

Handwheel 8.1

Selecting the function “Handwheel“

You can traverse the axes in the machine coordinate system (MCS) or in the workpiece coordinate system (WCS) via the handwheel. All axes are provided in the following order for handwheel assignment:  Geometry axes (X, Y, Z)  Channel machine axes (X1, Y1, Z1, C1) By pressing the HSK 2.6 “Handwheel” in the extended horizontal softkey bar the following input mask will be shown on the screen.

An input field for the assignment of the axes is offered for every handwheel on the machine. The axis-assignment can be made like described in the module B568 - "Basic operations". Besides there is the possibility to assign an axis directly to a handwheel using the VSK 1 - 8. 8.2


The number of softkeys for the axis assignment is limited. For the assignment of all other axes refer to the module B568 - "Basic operations", Section 3.2 "Parameter selection. Generally you can switch through all available axes by repeatedly pressing the blue "SELECT"-key on the keyboard. Display area

Description

Geometry axes By pressing the VSK 1 "X" the X-axis is assigned to the selected handwheel. By pressing the VSK 2 "Y" the Y-axis is assigned to the selected handwheel. By pressing the VSK 3 "Z" the Z-axis is assigned to the selected handwheel.

B572

Page 22


Section 8

Handwheel Display area


Notes:

Machine axes: By pressing the VSK 4 "X1" the X1-axis is assigned to the selected handwheel. By pressing the VSK 5 "Y1" the Y1-axis is assigned to the selected handwheel. By pressing the VSK 6 "Z1" the Z1-axis is assigned to the selected handwheel. By pressing VSK 7 "C1" the C1-axis is assigned to the selected handwheel. By pressing the VSK 8 "Back" you can close the window for the “Handwheel” 8.3 Handwheel assignment 1.

In the operating mode “AUTO“ select the operating area “Machine”, then press the HSK 2.6 “Handwheel” in the extended horizontal softkey bar.

2.


3.

Place the cursor in the field next to the handwheel with which you wish to assign the axis (e.g. no. 1).

4.

Press the corresponding softkey to select the desired axis (e.g. "X"). - OR To open the "Axis" selection box using the "INSERT" key, navigate to the desired axis, and press the "INPUT" key. Selecting an axis also activates the handwheel (e.g., "X" is assigned to handwheel no. 1 and is activated immediately).

5.

Press the HSK 2.6 "Handwheel" again. - OR Press the VSK 8 "Back" . The "Handwheel" window closes.

8.4 Deactivating the handwheel The cursor must be placed on that handwheel whose axis-assignment should be cancelled. By pressing the corresponding axis-softkey again the assignment is cancelled. Alternatively with pressing the “INSERT”key, the selection menu with all available axes can be opened. By using the blue “cursor-up”- and “cursor-down”-keys on the keyboard, switch to the empty field on top of the menu and press one of the yellow "INPUT"-keys on the keyboard. The empty value will be accepted. The corresponding handwheel is now deactivated.


Page 23

B572

Section 9 Notes:

Synchronized actions 9.1

Selecting the function “Synchronized actions” By pressing the HSK 2.7 “Synchronized actions” the following mask will be shown on the screen:


Waiting



Active



Blocked

Note: Refer to the machine manufacturer„s documentation for further in formation about the programmed synchronized actions.

B572

Page 24


Section 10

Settings

Notes:

10.1 Selecting the function “Settings” By pressing the HSK 2.8 “Settings” the following input mask with the settings for automatic mode is shown on the screen.

10.2 Vertical softkey bar (VSK) Display area

Description By pressing the VSK 5 "Changeover inch" the measuring units are converted from the metric to the imperial (inch) dimension system. New values have to be entered in inches. By pressing this key the key function switches to "Changeover metric". By pressing the VSK 5 "Changeover metric" the measuring units are converted from the imperial (inch) to the metric dimension system. New values have to be metric. By pressing this key the key function switches to "Changeover inch". Accept the selection by pressing the VSK 8 “OK” or cancel by pressing the VSK 7 “Cancel”. By pressing the VSK 8 "Back" you switch back to the main screen of the Sinumerik Operate.


Page 25

B572

Section 10

Settings

Notes: 10.3 Parameters for "Settings for automatic mode" In the “Settings for automatic mode“ window all configurations for automatic operation can be done. Parameter

Unit

Meaning

Dry run feedrate

[mm/ min]

The feedrate defined here replaces the programmed feedrate during execution if you have selected „DRY dry run feedrate“ under program control.

DRY

Reduced rapid trav- [%] erse RG0

This value entered here reduces the rapid traverse to the entered percentage value if you have selected “RG0 reduced rapid traverse” under program control.

Display result of measurement

Using a MMC command, you can display measurement results in a part program: When the control reaches the command, it automatically jumps into the “Machine” operating area and the window with the measurement results is displayed. The window with the measurement results is opened by pressing the softkey “Measurement result”.

B572

Page 26


B573

1

Operating area “Parameter”

Brief description

Objective of the module: In this module you learn to use the tool management with the Sinumerik Operate. You learn about the programming philosophy of the adjustable and programmable work offset, the function of the user variables and how to modify the “working area limitation”. Description of the module: In the tool management area all tool data relevant for machining (e.g., tool length, radius correction, tool wear and magazine configuration) can be viewed and modified. The tool management contains the following sub-functions:  the tool list  the tool wear  the magazine management In addition to these sub-functions a machine specific list can be configured by the machine manufacturer. Refer to the machine manufacturers documentation. In the "Work offset" menu the linear and rotational offsets can be viewed and modified in the settable work offset (WO). The working range in which a tool can proceed, can be restricted in all axes with the function “Working area limitation”. Hereby safety zones can be installed in the workspace, where tool movement is prohibited. This function limits the traversing area of the axes, in addition to the limit switches. Content: Operating area “Parameter“ Tool list Tool wear Magazine management Zero offset basics Work offset User variable Setting data


Page 1


B573

B573

B573

Page 2


B573 Operating area Parameter: Description In the tool management area all tool data relevant for machining (e.g., tool length, radius correction, tool wear and magazine configuration) can be viewed and modified. The tool management contains the following subfunctions:

Operating area Parameter: START

Operating area “Parameter“

 the tool list  the tool wear Tool list

 the magazine management In addition to these sub-functions a machine specific list can be configured by the machine manufacturer. Refer to the machine manufacturers documentation. In the "Work offset" menu the linear and rotational offsets can be viewed and modified in the settable work offset (WO). The working range in which a tool can proceed, can be restricted in all axes with the function “Working area limitation”. Hereby safety zones can be installed in the workspace, where tool movement is prohibited. This function limits the traversing area of the axes, in addition to the limit switches.

Tool wear

Magazine management

Zero offset basics

Work offset

User variable

Setting data

Operating area Parameter: END

Notes :


Page 3

B573

Section 2 Notes:

Operating area “Parameter“ 2.1

Selecting the operating area “Parameter”

In the Operation area “Parameter” you have a choice of selecting between various lists (e.g. Tool list, tool wear, magazine list, offsets, user variables and setting data). For example in the tool management area, all tools and if configured also the magazine locations are being displayed. Both lists display the same tools in the same order. When switching between lists, the position of the cursor on a particular tool in the current screen is carried over to the same tool in a new screen. The lists differ from each other by the displayed parameters and the Softkey functions. Switching between lists is a specific change from one topic to the next.  Tool list: All parameters and functions required to create and set up tools are displayed.  Tool wear: All parameters and functions that are required during operation, e.g. wear and monitoring functions, are listed here.  Magazine: Magazine and magazine location-related parameters and functions for the tools and magazine locations are listed here. The operating area “Parameter“ can be opened from every operating modes (“JOG”, “MDA”, “AUTO”). Press the “OFFSET”-key on the keyboard. The operating area “Parameter“ respectively the “Tool list” opens directly. - OR Press the “MENU SELECT“-key on the operator panel. The yellow horizontal and vertical softkey bar opens. Then switch to the operating area “Parameter” by pressing the HSK 2 “Parameter” on the operator panel. The operating area “Parameter” opens, with the “Tool list”, “Tool wear”, “Magazine”, “Work offset”, “User variables” and the “Setting data”. These functions are made available in the following described horizontal softkey bar. 2.2

Horizontal softkey bar (HSK)

Display area

Description By pressing the HSK 1 “Tool list” the tool list window opens. See section 3 “Tool list”. By pressing the HSK 2 “Tool wear“ the tool wear list opens. See section 4 “Tool wear”.

B573

Page 4


Section 3

Tool list Display area


Notes:

By pressing the HSK 4 “Magazine“ the Magazine management is opened. See section 5 “Magazine“. By pressing the HSK 5 “Work offset“ a list with all Work offsets is opened. See section 7 “Work offset”. By pressing the HSK 6 “User variable“ a list with all R variables is opened. See section 8 “User variable”. By pressing the HSK 8 “Setting data” a list with all setting data is opened. See section 9 “Setting data”.

3.1

Selecting the “Tool list” By pressing the HSK 1 “Tool list“ the “Tool list“ window opens. (Note the screen below.)

In the tool list all parameters and functions that are required to create and set up the tools are displayed, regardless weather the tools are assigned or not assigned to a magazine location. Each tool is uniquely identified by the location number, the tool name and the replacement tool number. The most common tools and probes for turning, drilling and milling are offered in the tool list. Geometrical and technological tool data can be assigned to each tool type. Depending on the tool type different correction data are necessary.


Page 5

B573

Section 3 Notes:

Tool list 3.2


Display area

Description By pressing the VSK 1.1 “Tool measure” the “Measuring tool” window opens. (See section 3.7 in this module) By pressing the VSK 1.2 “New tool” a new tool can be created. This function is only available, if the cursor is positioned on a filed that does not yet has a tool assigned to it. (See section 3.5 in this module) By pressing the VSK 1.3 “Edges” the vertical softkey bar for assigning new cutting edges and deleting existing cutting edges opens to the right side of the screen. If a tool has several cutting edges each edge gets its own set of correction data. (See section 3.8 in this module) By pressing the VSK 1.4 “Further data” more information about a tool will be displayed. This function is only available for tools which have additional information. (See section 3.5, page 17 in this module) By pressing the VSKs 1.5 ”Unload” or “Load” the actual selected tool wil be unloaded from or loaded to the magazine. Unloaded tools are being displayed on the bottom of the magazine list. (See section 3.10, page 24 in this module) By pressing the VSK 1.6 “Delete tool” the selected tool will be deleted from the tool list. (See section 3.9, page 23 in this module) By pressing the VSK 1.7 “Magazine selection” Softkey multiple times you can jump between buffer location (spindle and gripper), Magazine and NCmemory (unloaded tools) and back to the buffer location. The cursor is always positioned at the beginning of each group. (See section 3.11, page 26 in this module) By pressing the VSK 1.8 “Extend” on the operator panel the extended vertical softkey bar 2 opens on the right hand side of the screen. By pressing the VSK 2.1 “Sort” you can sort the tools in the tool list according to the following criteria:  Magazine  Name  Type  T-Number The suitable softkeys are offered in the vertical softkey bar. (See section 3.12 in this module)

B573

Page 6


Section 3



Notes:

Pressing the VSK 2.2 “Filter” opens the screen to set the filter options. (See section 3.13 in this module) Pressing the VSK 2.4 „Details“ opens a new softkey bar with the functions  Tool Data  Cutting edge data  Monitoring data The details of the tool which is selected by the cursor position are listed in the screen. Pressing the VSK 2.8 “Back“ on the operator panel you switch back to the vertical softkey bar 1. Pressing the VSK 3.3 “Tool data” opens the screen “Tool details - all parameters”.

By pressing the VSK 3.5 “Cutting edge data” the cutting edge data for the selected edge is being displayed. In case of tools with several cutting edges you can switch with VSK 3.1 “Cutting edge +” or VSK 3.2 “Cutting edge - ” between the individual cutting edges.


Page 7

B573

Section 3 Notes:



By pressing the VSK 3.6 “Monitoring data” you can select the monitoring data of the selected tool. In case of tools with several cutting edges you can switch with VSK 3.1 “Cutting edge +” or VSK 3.2 “Cutting edge - ” between the individual cutting edges.

Alternately you can also navigate with the cursor buttons “cursor left” and “cursor right” between the masks “Tool data”, “Cutting edge data” and “Monitoring data”.

B573

Page 8


Section 3

Tool list 3.3

Notes:

Tool parameters

Column header

Meaning

Loc.

Magazine/location number Spindle location as an icon Location for gripper 1 and 2 as icons: (Applies only when a spindle with dual gripper is used.) Magazine number: If more than one magazine is available, first the location number and then the magazine number is displayed separated by a slash. E.g.: Location number 1 in magazine 1 Location number 1 in magazine 2 Tools in the tool list not assigned to a magazine are displayed without a location number at the end of the window. You can manage tools that are not changed automatically, by hands (hand tools). If the orange selection cursor is placed in the type field on a tool icon you can change the tool type by pressing the “SELECT”-key.

Type

Tool type

Tools can be created on a free tool position or by pressing the VSK 1.2 “New tool” in the tool list. The following tool windows can be opened by pressing the corresponding vertical softkeys.

Press the VSK 1 “Favourites” to open the “New tool - favourites” list. In the favourite list the most often used tools are saved as favourites for a fast access.


Page 9

B573

Section 3

Tool list

Notes:

Press the VSK 2 “Cutters 100-199” to open the “New tool milling cutter” list. A list of all available milling cutters opens.

Press the VSK 3 “Drill 200-299” to open the “New tool drill” list. A list with all available Drilling tools opens.

Press the VSK 5 “Spec.tool 700-900” to open the “New tool – special tools” list. A list with special tools opens. Press the VSK 7 “Cancel” to reject the tool selection and to jump back to the “Tool list” window in the operating area “Parameter”. Press the VSK 8 “OK“ to accept the selected tool and to jump back to the “Tool list” window in the operating area “Parameter”. The selected tool will be loaded into the tool list

B573

Page 10


Section 3

Tool list

Notes:

Column header

Meaning (continuation)

Tool name

Name of the tool: To identify a tool you can enter a tool name as text or a T-number. If a new tool is created, tool names are pre-assigned as default.

ST

Replacement tool number: (for replacement tool strategy) As default “1” is being entered here. If a new tool with the same name, as a already existing tool, is being created, then the new tool gets the Index “2”. This way it is possible to define a replacement tool.

D

Cutting edge number: For tools with multiple cutting edges, each tool receives it’s own correction data field. Up to 9 edges per tool can be managed. The max. Number depends upon the control configuration.

Length

Tool length: Geometry length of the tool.

Radius/diameter

Tool radius/diameter For every tool, information about the tool radius or diameter can be entered here. The changeover from diameter to radius or vice versa can be set via a machine datum.

Tip angle or Pitch

 Tip angle for Type 200 - twist drill Type 220 - center drill Type 230 - countersink  Pitch for Type 240 - tap

N

 Number of teeth for: Type 100 - milling tool Type 110 - ball nose cylindrical die sinking cutter Type 111 - ball nose tapered die-sinking cutter Type 120 - end mill Type 121 - end mill with corner rounding Type 130 - angle head cutter Type 140 - facing tool Type 150 - side mill Type 155 - bevelled cutter Type 156 - bevelled cutter with corner rounding Type 157 - tapered die-sinking cutter Type 160 - drill and thread cutter


Page 11

B573

Section 3 Notes:

Tool list 3.4 Icons in the toolbar and their meaning Icons

Meaning

Red X

The tool is disabled

Yellow triangle pointing downward

The pre-warning limit has been reached

Yellow triangle pointing upward

The tool is in a special state Place the cursor on the marked tool. A tool tip will provide a brief description

Green frame

The tool is preselected.

Magazine/location number:

B573

Green double arrow

The magazine location is positioned at the change position

Gray double arrow

The magazine location is positioned at the loading position

Red X

The magazine location is disabled

Page 12


Section 3

Tool list

Notes:

3.5 Additional data The following tool types require geometry data that is not included in the tool list display. Tool type

Additional parameters

111 Conical ball head cutter

Corner radius

121 End mill with Corner radius corner rounding 130 Angle head cutter

Geometry length (length X, length Y, length Z) Wear length (Δlength X, Δlength Y, Δlength Z) Adapter length (length X, length Y, length Z) V (direction vector 1 - 6) Vector X, vector Y, vector Z

131 Angle head Geometry length (length X, length Y, length Z) cutter with Corner radius corner rounding Wear length (Δlength X, Δlength Y, Δlength Z) Adapter length (length X, length Y, length Z) V (direction vector 1 - 6) Vector X, vector Y, vector Z

140 Face milling

External radius Tool angle

155 Bevel cutter

Taper angle

156 Bevel cutter with corner rounding

Corner radius Taper angle

157 Conical die milling cutter

Taper angle

Note: You can use the configuration file to specify the data to be displayed for specific tool types in the "Additional Data" window. The VSK “Further data” is only available for those tool types which will support this function.


Page 13

B573

Section 3 Notes:

Tool list 3.6 New tool In the window “New tool - favourites” you can choose a new tool from a list of favourite tools (VSK 1 “Favourites”). If the desired tool type should not be available in the Favourite list, you can simply select a tool from a group of cutting, drilling, turning or special tools by pressing the corresponding VSKs 2 - 5. 3.6.1 Selecting the function “New tool” By pressing the VSK 1.2 “New tool“ the “New tool - favorits“ window opens.


Description

For the softkeys see section 3.3. 3.6.3 Creating a new tool 1.

In the operating mode “JOG“, “MDA“ or “AUTO“ select the operating area “Parameter” by pressing the “MENU SELECT“-key on the keyboard and the HSK 2 “Parameter”.

1.

-ORAlternatively press the “OFFSET”-key on the keyboard, to get directly to the tool list.

2.

B573

Press the VSK 1 “Tool list” to open the tool management screen. The “Tool list” window opens directly. Page 14


Section 3

Tool list 3.

Place the cursor in the tool list at the position where the new tool should be stored. For this, you can select an empty magazine location or the NC tool memory outside of the magazine. You may also place the cursor on an existing tool in the NC tool memory region. Data from the displayed tool will not be overwritten, but the new tool is created below.

4.

Press the VSK 1.2 “New tool“ The "New tool - favourites" window opens.

Notes:

- OR 5.

If you want to create a tool that is not in the “Favourites” list, press the VSK 2 "Cutters 100-199", VSK 3 "Drill 200-299" or the VSK 5 "Spec. tool 700900" . The corresponding tool window opens.

6.

Select the tool by placing the cursor on the corresponding tool type.

7.

Press the VSK 8 “OK“ to create the new tool. The tool is added to the tool list with a predefined name. If the cursor is located on an empty magazine location in the tool list, then the tool is loaded to this magazine location.

Multiple loading points: If you have configured several loading points for a magazine, then the "Select loading point" window appears when a tool is created directly in an empty magazine location or when the "Load" softkey is pressed. Select the required load point and confirm with the VSK 8 "OK" or abort with pressing the VSK 7 “Cancel”. Additional data: If configured proper, the "New tool" window opens after the required tool has been selected and confirmed with the VSK 8 "OK". You can define the following data in this window:  Names  Tool location type  Size of tool (See section 3.4 in this module) Note: For further information see the commissioning manual of the Sinumerik Operate.


Page 15

B573

Section 3 Notes:

Tool list 3.7 Tool measure You can measure the tool offset data for the individual tools directly from the tool list. Note: Tool measurement is only applicable with an active tool. 3.7.1 Selecting the function “Tool measure” With an active tool selected press the VSK 1.1 “Tool measure” to switch to the “Length manual” window in the operating mode “JOG”.


Description

For the softkeys see module B570 “Operating mode JOG“, section 6.3. 3.7.3 Measuring a tool

B573

1.

Either press the “OFFSET“-key on the keyboard or press “MENU SELECT“ on the operator panel, then the HSK 2 “Parameter” and the HSK 1 “Tool list” to switch to the tool list.

2.

Select the active tool that you want to measure in the tool list and press the VSK 1.1 "Tool measure". You jump to the "JOG" operating mode and the tool to be measured is entered in the "T" field in the "Length manual" screen.

Page 16


Section 3

Tool list 3.

Select the cutting edge number “D” and the replacement tool number “ST”.

4.

Approach the workpiece in Z direction, scratch it with a rotating spindle and enter the set position of the workpiece edge in the “Z0” field.

5.

Press the VSK 7 "Set length".

Notes:

The tool length is calculated automatically and entered in the tool list. 3.8 Managing cutting edges In the case of tools with more than one cutting edge, a separate set of offset data is assigned to each cutting edge. For every tool up to 9 edges can be installed. No gaps in the assignment of edges are allowed. If a tool has 3 cutting edges then edge numbers 1 to 3 have to be assigned. Tool cutting edges that are not required can be deleted. 3.8.1 Selecting the function “Edges” By pressing the VSK 1.3 “Edges“ the following vertical softkey bar opens on the right hand side of the “Tool list”- window.


Page 17

B573

Section 3 Notes:

Tool list 3.8.2 Vertical softkey bar Display area

Description Pressing the VSK 1 “New cutting edge” installs a new cutting edge for a tool in the tool list. Pressing the VSK 2 “Delete cutting edge” deletes a selected cutting edge of a tool.

3.8.3

Installing a new cutting edge

1.


2.

In the tool list, position the cursor on the tool for which you would like to store more cutting edges. Press the VSK 1.3 “Edges”.

3.

Press the VSK1 “New cutting edge”. A new data set is stored in the list. The cutting edge number is incremented by 1 and the offset data is assigned to the values of the cutting edge on which the cursor is positioned.

4.

Enter the offset data for the new cutting edge.

5.

Repeat the steps 3 - 4 if you wish to create more tool edge offset data.

3.8.4 Deleting a cutting edge 1.

Either press the “OFFSET“-key on the keyboard or press “MENU SELECT“ on the operator panel, then the HSK 2 “Parameter”, then press the HSK 1 “Tool list” to switch to the tool list.

3.

In the tool list, position the cursor on the tool for which you would like to delete cutting edges, then press the VSK 1.3 “Edges”.

4.

Press the VSK 2 “Delete cut. edge”. The data set is deleted from the list. The first tool cutting edge cannot be deleted.

B573

Page 18


Section 3

Tool list

Notes:

3.9 Delete tool To keep the tool list short and clear, unused tools can be deleted from the tool list. 3.9.1 Selecting the function “Delete tool” Pressing the VSK 1.6 “Delete tool” the “Delete tool” dialogue window opens.

3.9.2 Deleting a tool 1.


2.

In the tool list window place the cursor on the tool that you would like to delete. Press the VSK 1.6 “Delete tool“. A safety prompt is displayed asking for confirmation.

3.

Press the VSK 8 “OK“ to delete tho tool or press the VSK 7 “Cancel” to abort. The tool is deleted from the tool list. If the tool is in a magazine location, it is unloaded and then deleted.

Several load points If you have configured several loading points for a magazine, then the "Select loading point" window appears after pressing the VSK 6 "Delete tool". Select the required load point and press the VSK 8 "OK" to unload and delete the tool. 828D/840Dsl SINUMERIK Operate

Page 19

B573

Section 3 Notes:

Tool list 3.10 Loading or unloading a tool You can load and unload tools to and from a magazine via the tool list. When a tool is loaded, it is taken to a magazine location. When it is unloaded, it is removed from the magazine and stored in the tool list. When you are loading a tool, the application automatically suggests an empty location. You may also directly specify an empty magazine location. You can unload tools from the magazine that you are not using at present. The Sinumerik Operate then automatically saves the tool data in the tool list in the NC memory outside the magazine. Should you want to use the tool again later, simply load the tool with the tool data into the corresponding magazine location again. Then the same tool data does not have to be entered more than once. 3.10.1 Selecting the function “Load” or “Unload”. By pressing the VSK 1.5 “Load” the following “Load on ...” window opens. The softkey is only active if the cursor is located on a tool that is not assigned to the magazine. By pressing the VSK 1.5 “Unload“ the selected tool will be unloaded from the magazine. The softkey is only active if the cursor is placed on a tool that is assigned to a magazine location.

B573

Page 20


Section 3

Tool list

Notes:


Description Press the VSK 4 “Spindle” to load the selected tool to the spindle location.

3.10.3 Loading a tool 1.


2.

In the tool list press the VSK 1.5 “Load”. The “Load on ...” window opens. The field “... loc." is reallocated with the first empty place in the magazine.

3.

Press the VSK 8 “OK“ to accept the suggested location number. - OR -

3.

Insert another location number and press the VSK 8 “OK”. - OR -

3.

Press the VSK 4 “Spindle“. The tool is loaded into the specified magazine location or spindle.

Several magazines If you have configured several magazines, the "Load on ..." window appears after pressing the VSK 1.5 "Load". If you do not want to use the suggested empty location, then enter your desired magazine and magazine location. Confirm your selection with the VSK 8 "OK".

Several loading points If you have configured several loading points for a magazine, then the "Select loading point" window appears after pressing the VSK 1.5 "Load". Select the required loading point and confirm with the VSK 8 "OK".


Page 21

B573

Section 3 Notes:

Tool list 3.10.4 Unloading a tool 1.


2.

Place the cursor on the tool that you would like to unload from the magazine and press the VSK 1.5 "Unload".

3.

Select the required loading point in the "Select loading point” window.

4.

Confirm the selection with pressing the VSK 8 “OK“ or abort with pressing the VSK 7 “Cancel“.

3.11 Selecting a magazine You can directly select the buffer memory, the magazine, or the NC memory. Press the VSK 1.7 “Magazine selection”. If there is only one magazine, you will move from one area to the next (i.e. from the buffer to the magazine, from the magazine to the NC memory and from the NC memory back to the buffer) each time you press the softkey. The cursor is positioned at the beginning of the magazine each time. If there is more than one magazine, the "Magazine selection" window opens. Position the cursor on the desired magazine in this window and press the "Go to" softkey. The cursor jumps directly to the beginning of the specified magazine. Magazines can be hidden in the magazine list. Uncheck the checkbox alongside the corresponding magazine in the “Magazine selection” window, by pressing the “SELECT”-key on the keyboard. Note: The magazine selection behaviour with multiple magazines can be configured in different ways. Please refer to the machine manufacturer's specifications.

B573

Page 22


Section 3

Tool list

Notes:

3.12 Sort With the help of this function “Sort” you can sort and view the tools in the tool list depending on different sorting criteria.

3.12.1 Selecting the function “Sort” Pressing the VSK 2.1 “Sort“ opens the following softkeys in the vertical softkey bar.


Description The tools in the tool list are sorted numerical by their positions in the magazines. Tools with identical magazine location will be sorted by tool type and tools of the same type are sorted depending on their radius value. The tools are sorted alphabetical by name. The tools are sorted by tool type. Similar types will be sorted by radius. The tools are sorted by tool number.

3.12.3 Sorting tools 1.

Press the “MENU SELECT“-key on the operator panel, then the HSK 2 “Parameter” and the HSK 1 “Tool list” to switch to the tool list. The “Tool list” window opens.

2.

Press the VSK 2.1 “Sort”. A vertical softkey bar with all available sort criteria opens to the right (see section 3.12.2).

3.

I order to sort the tool list depending on the “tool name”, “magazine location”, “tool type” or “T-number” press the corresponding softkey (VSK 1 - 4) (see section 3.12.2). The tool list will be sorted following the chosen search criteria.


Page 23

B573

Section 3 Notes:

Tool list 3.13 Filter The filter function allows you to filter-out tools with specific properties in the tool management lists. 3.13.1 Selecting the function tool “Filter” Pressing the VSK 2.2 “Filter” the “Filter” dialogue window for “the tool list”, “tool wear” and “magazine” list is opened. Following selection window is displayed.

Filter criteria: Only display the first Only tools with the cutting edge number D1 are cutting edge listed. Only tools that are ready to use

Only tools that are ready to use are listed.

Only tools that have Only tools that have reached the pre-warning limit reached the preare displayed. alarm limit

B573

Only locked tools

Only locked tools are displayed.

Note: Multiple selection

You have the option of selecting several criteria. You will receive an appropriate message if conflicting filter options are selected.

Page 24


Section 3

Tool list

Notes: The following shows the filter setting “only tools with pre-warning limit reached”.


Page 25

B573

Section 4 Notes:

Tool wear 4.1

Selecting the function “Tool wear“

All parameters and functions that are required during operation are contained in the tool wear list. Tools that are in use for long periods are subject to wear. You can measure this wear and enter it in the tool wear list. The Sinumerik Operate then takes this information into account when calculating the tool length or radius compensation. This ensures a consistent level of accuracy during workpiece machining. You can automatically monitor the tools' working times via the workpiece count, tool life or wear. In addition, you can disable tools when you no longer wish to use them. Note: Depending on the control configuration, the input of the tool wear can be additive. Please refer to the machine tool manufacturer documentation. By pressing the HSK 2 “Tool wear“ the “Tool wear” screen input mask opens.

4.2


Display area

Description By pressing the VSK 1 “Sort” and “Filter” you can sort and filter the tools in the tool list according to different parameters.( See section 3.12 and 3.13) By pressing the VSK 6 “Reactivate“ locked tools, and tools that have reached their pre-warning limit can be made operational again. (See section 4.7)

B573

Page 26


Section 4

Tool wear 4.3

Notes:

Parameters for “Tool wear”

Parameter

Meaning

Location

Magazine/location number: (Only display, see section 3.3 “Tool list”)

Type

Tool type: (See section 3.3 “Tool list”)

Tool name

Tool name: (See section 3.3 “Tool list”)

ST

Replacement tool number: (Only display, see section 3.3 “Tool list”)

D

Cutting edge number (Only display, see section 3.3 “Tool list”)

ΔLength

Length wear In this field changes for the tool length are entered

ΔRadius

Radius wear The Sinumerik Operate checks the entered values whether they exceed an absolute or incremental threshold or not. The incremental threshold is the maximum difference between present wear and new wear. The absolute threshold is the maximum total wear value that can be entered. Note: Please refer to the machine manufacturer's specifications.

T

 Tool monitoring by tool life: With the tool life T (Time), the service life for tool with machining federate is monitored in minutes.

C

 Tool monitoring by count With the count C, the number of workpieces machined by the tool is counted.

W*

 Tool monitoring by wear With wear W, the greatest value in the wear parameters ΔLength X, ΔLength Z, ΔRadius or ΔØ in the wear list is monitored. * The wear monitoring is configured via a machine data item.


Page 27

B573

Section 4 Notes:

Tool wear Parameter

Meaning (continuation)

Tool life (T)

Tool life

Quantity (C)

Number of workpieces

Wear (W)

Tool wear The wear monitoring is configured via a machine data item. Please refer to the machine manufacturer`s instructions.

Set val

Setpoint value for tool life, workpiece count, or wear.

Prewar limit

Prewarning limit: Specification of the tool life, workpiece count or wear at which a warning is displayed. Note: If the adjusted rest life of the tool, the number of changes or the wear is reached, the tool will be disabled. This tool will not be selected for the next tool change. If present, an adequate sister tool will be used instead. The monitoring refers in each case to the selected cutting edge. It is possible to reactivate a disabled tool.

D

Single tools can also be disabled by hand, if these tools are not in use anymore or if the tools life ran off. (The tool is disabled if the checkbox is activated).

4.4 Icons in the tool wear list and their meaning (See section 3.3, Icons in the tool list, in this module) 4.5 Entering the tool wear or disabling a tool 1.

Press the “MENU SELECT“-key on the operator panel, then the HSK 2 “Parameter” and the HSK 2 “Tool wear” to switch to the tool wear list.

2.

Enter values for length, radius, setpoint, prewarning and tool life. - OR -

2.

B573

Activate the “D”-parameter checkbox for disabling the tool manually.

Page 28


Section 4

Tool wear

Notes:

4.6 Sort and Filter For the functions “Sort” and “Filter” in the tool list refer to the section 3.12 and 3.13 in this module.

4.7 Reactivating a tool You can replace disabled tools or make them ready for reuse. Prerequisite is, that the monitoring function must be active and a setpoint is stored. 1.

Press the “MENU SELECT“-key on the operator panel, then the HSK 2 “Parameter” and the HSK 2 “Tool wear” to switch to the tool wear list.

2.

Position the cursor on the disabled tool which you would like to reuse. Press the VSK 6 "Reactivate". The value entered as the setpoint is entered as the new tool life workpiece count. The disabled tool is active again.

Reactivating and positioning When the "Reactivate with positioning" function is configured, the selected tool's magazine location will also be positioned at a loading point. You can exchange the tool. Reactivation of all monitoring types When the "Reactivation of all monitoring types" function is configured, all the monitoring types set in the NC for a tool are reset during reactivation. Note: Refer to the machine manufacturer„s specifications.


Page 29

B573

Section 5 Notes:

Magazine management 5.1

Selecting the function “Magazine“

Tools are displayed with their magazine-related data in the magazine list. Here, you can take specific actions relating to the magazines and the magazine locations. Individual magazine locations can be location-coded or disabled for existing tools. By pressing the HSK 4 “Magazine“ the following magazine list will be displayed on the screen.

In the magazine list, all magazine locations are shown. It is indicated whether a magazine location is available, disabled or occupied by a tool. If a magazine location is defect, this location can be disabled. If an oversized tool is inserted, which uses more than a half of the neighbouring magazine locations, then the neighbouring magazine locations will be disabled. 5.2


Display area

Description By pressing the VSK 5 “Relocate“ a tool can be transferred from one magazine location to another or, with pressing the VSK 4 “Spindle”, it can be transferred to the spindle. The selected target location must be confirmed with the VSK 8 “OK” or can aborted with VSK 7 “Cancel”. By pressing the VSK 6 “Position magazine“ you can position magazine locations directly on the loading point. (See section 5.6) By pressing the VSK 1.8 “Extend” on the operator panel the extended vertical softkey bar 2 opens with the functions “Sort”, “Filter” and “Details” (see sections 3.12 and 3.13).

B573

Page 30


Section 5

Magazine management

Notes: 5.3

Parameters for “Magazine”

Parameter

Meaning

Loc.

Number of the magazine location: (Only display, see section 3.3 “Tool list“)

Type

Tool type: (Only display, see section 3.3 “Tool list“)

Tool name

Tool name: (See section 3.3 “Tool list“)

ST

Sister tool: (Only display, see section 3.3 “Tool list“)

D

Edge number: (Only display, see section 3.3 “Tool list“)

D

Magazine location disabled

Z

Oversized tool: Marking a tool as oversized. The tool occupies two half locations left, two half locations right, one half location top and one half location bottom in a magazine. Only tools that are not loaded yet can be marked as oversized.

L

Fixed location coding. The tool is fixed to the magazine location.

5.4 Sorting and filtering tools When you are working with many tools, with large magazines or several magazines, it is useful to display the tools sorted according to different criteria. Then you will be able to find a specific tool more easily in the lists. For sorting tools in the magazine see section 3.12 and 3.13 in this module.


Page 31

B573

Section 5 Notes:

Magazine management 5.5 Relocate Tools can be directly relocated within magazines to another magazine location, which means that you do not have to unload tools from the magazine in order to load them into a different location. When you are relocating a tool, the application automatically suggests an empty location. You may also directly specify an empty magazine location. 5.5.1 Selecting the function “Relocate” By pressing the VSK 5 “Relocate” depending on the tool type following window opens.

5.5.2 Relocating a tool 1.

Press the “MENU SELECT“-key on the operator panel, then the HSK 2 “Parameter” to open the operating area “Parameter”. Alternatively press the “OFFSET”-key on the keyboard.

2.

Press the HSK 4 “Magazine“. The magazine window opens.

3.

Position the cursor on the tool that you wish to relocate to a different magazine location.

4.

Press the VSK 5 “Relocate”. The “...move from location...to...” window opens. The "... loc." field is initialized with the number of the first empty magazine location.

5.

B573

Press the VSK 8 "OK" to relocate the tool to the suggested location.

Page 32


Section 5

Magazine management

Notes:

- OR 5.

Enter the location number you require and press the VSK 8 "OK". - OR -

5.

Press the VSK 4 "Spindle" to load a tool into the spindle and press the VSK 8 "OK". The tool is moved to the specified magazine location or the spindle.

Several magazines If you have set up several magazines, then the "...move from magazine... location... to..." window appears after pressing the VSK 5 "Relocate" . Select the desired magazine and location, and confirm your selection with the VSK 8 "OK" to load the tool.

5.6 Positioning a magazine You can position magazine locations directly on the loading point. 1.

Press the “MENU SELECT“-key on the operator panel, then the HSK 2 “Parameter” and the HSK 4 “Magazine”. Alternatively press the “OFFSET”-key on the keyboard.

2.

Place the cursor on the magazine location that you want to position onto the load point.

3.

Press the VSK 6 "Position magazine".

4.

Select a loading point in the input mask. The magazine location is positioned on the loading point.

Several load points If you have configured several loading points for a magazine, then the "Load Point Selection" window appears after pressing the VSK 6 "Position magazine". Select the desired loading point in this window and confirm your selection with the VSK 8 "OK" to position the magazine location at the loading point.


Page 33

B573

Section 6 Notes:

Zero offset basics Following reference point approach, the actual value display for the axis coordinates is based on the machine zero (M) of the machine coordinate system (MCS ). The program for machining the workpiece, however, is based on the workpiece zero (W) of the workpiece coordinate system (WCS ). The machine zero and workpiece zero are not necessarily identical. The distance between the machine zero and workpiece vary in accordance with the type of tool and the way it is clamped. This zero offset is taken into account during execution of the program and can be a combination of different offsets. On the Sinumerik Operate, the position actual value display refers to the SZS-coordinate system (settable zero system). The position of the active tool relative to the workpiece zero is displayed. The offsets are added as follows:

W

WCS

Transformation of coordinates SZS

Tool offset

Work offset fine

Work offset coarse

Base offset

MCS

M

B573

Base offset

The base offset is a zero offset that is always active. If you have not defined a base offset, its value will be zero. You determine the base offset via "Measure workpiece zero” . See Module B570 - ”Operating mode JOG”, in Sinumerik Operate section “Set Work offset” and “Measure workpiece zero”.

Zero offsets

Every zero offset (G54 to G57, G505 to G599) consists of a coarse offset and a fine offset. You can call the work offsets from any sequence program (coarse and fine offsets are added together). You can save the workpiece zero, for example, in the coarse offset, and then store the offset that occurs when a new workpiece is clamped between the old and the new workpiece zero in the fine offset.

Page 34


Section 6

Zero offset basics Fine offsets must be set up by the machine manufacturer.

Notes:

Note: Also refer to the machine manufacturer's instructions. Coordinate transformations:

You always program coordinate transformations for a specific sequence program. They are defined by:  Offset  Rotation  Scaling  Mirroring These transformations can work as “new” or they can work “additive” to the active zero point offset.

Total offset:

The total offset is calculated from the sum of all offsets and coordinate transformations.


Page 35

B573

Section 7 Notes:

Work offset 7.1

Selecting the function “Work offset“ By pressing the HSK 5 “Work offset“. The screen mask of the active work offsets is opened.

The horizontal scroll bar above the horizontal softkey bar indicates that more parameters for the work offset are available. Because of the limited screen area, they are covered by the softkeys of the VSK bar. Move the orange selection cursor, with the help of the blue cursor keys on the keyboard to the left to reach the additional parameters. 7.2


Display area

Description By pressing the VSK 2 “Active“ for all installed axis all current active offsets will be displayed, as well as all active system offsets. Fields in the work offset list with a light blue background can not be altered. (See section 7.4 in this module) By pressing the VSK 3 “Overview” the active offsets and system offsets are displayed for all set-up axes. Only fields with a white background can be edited. (see section 7.4) By pressing the VSK 3 “Base“ for all installed axis the channel specific basic work offsets are displayed in coarse offset and fine offset. The values can be changed directly in the “Work offset - basic” window, (See section 7.5 in this module)

B573

Page 36


Section 7

Work offset Display area


Notes:

By pressing the VSK 4 “G54...G57“ for all installed axis the work offsets G54 to G57 are displayed in coarse offset and fine offset. The values can be changed directly in the “Work offset - G54...G57” window. (See section 7.6 in this module) By placing the cursor in an offset field in the work offset list and pressing the VSK 7 “Details“ more information (fine, coarse, scaling, shifting, mirroring) about all installed axis for the selected offset type will be displayed. Inputs for coarse and fine offset, already entered, are taken over or can be entered. The values can be changed directly in the “Work offset - details:...” window. (See section 7.7 in this module) By pressing the VSK 7 “Details” the following softkeys in the vertical softkey bar open. 7.3

Vertical softkey bar “Details“

Display area

Description By pressing the VSK 1 “WO +“ within the selected offset type (“Active“, “Base“, “G54...57“) you can change to the next work offset in the work offset list without changing back to the “Work offset” window first. By pressing the VSK 2 “WO -“ within the selected offset type (“Active“, “Base“, G54...57“) you can change to the previous work offset in the work offset list without changing back to the “Work offset” window first. By pressing the VSK 7 “Clear offset“ all entered offsets for the installed axis will be deleted from the list. By pressing the VSK 8 “Back“ you switch back to the “Work offset” window.


Page 37

B573

Section 7 Notes:

Work offset 7.4 Active work offset The following work offsets are displayed in the “Work offset - active” window:  Work offsets, for which offsets are included, or for which values are entered  Adjustable work offsets  Total work offset This window is generally used only for monitoring. The availability of the offsets depends on the setting. Please refer to the manufacturer's documentation. 7.4.1 Selecting the function “Active” By pressing the VSK 2 “Active“ the “Work offset active” window opens.

7.5 Work offset overview In the “Work offset - Overview” window, all active offsets and system offsets are displayed for all set-up axes. In addition to the offset, the rotation, scaling and mirroring defined using this are also displayed. This window is generally used for monitoring.

B573

Page 38


Section 7

Work offset 7.5.1 Selection of the function „Work offset - Overview““

Notes:

By pressing the VSK 2 „Overview“ the window “Work offset - overview” opens.

7.5.2 Parameters for “Work offset - active” Parameters

Meaning

DRF

Display of the handwheel axis offset.

Rotary table ref.

Display of additional work offsets programmed with $P_PARTFRAME .

Basic reference

Display of additional work offset programmed with $P_SETFRAME. Access to the system offsets is protected via a keyswitch.

Total base WO

Displays all effective basic offsets as well as rotation, scaling and mirroring. Values can not be changed here.

G500 or G54 - G57

Display of all work offsets activated with G500, G54 G57, as well as rotation, scaling and mirroring. You cannot edit these values here.

Tool reference

Displays the additional work offset programmed with $P_TOOLFRAME..

Workpiece ref.

Displays the additional work offset programmed with $P_WPFRAME.

Programmed WO

Displays the additional work offset programmed with $P_PFRAME.

Cycle reference

Display of all additional work offsets activated via $MC_MM_SYSTEM_FRAME_MASK.

Total WO

Display of the active work offset, representing the sum of all work offsets, as well as rotation, scaling and mirroring.


Page 39

B573

Section 7 Notes:

Work offset 7.6 Base zero offset The defined channel-specific and global base offsets, divided into coarse and fine offsets, are displayed for all set-up axes in the "Work offset - basic" window. 7.6.1 Selecting the function “Work offset - basic” By pressing the VSK 3 “Base“ the “Work offset - basic” window with the channel specific and global basic work offsets opens.

The horizontal scroll bar above the horizontal softkey bar indicates that more parameters for the work offset are available. Because of the limited screen area, they are covered by the softkeys of the vertical softkey bar. Move the orange selection cursor, with the help of the blue cursor keys on the keyboard to the left, to reach the additional parameters.

7.6.2 Displaying and editing base zero offset 1.


2.

Press the HSK 5 “Work offset”

3.

Press the VSK 3 “Base”. The “Work offset - basic” window opens. With the cursor positioned on the fields with the white background you can edit the values directly in the table.

Caution: The entered offset values are active directly.

B573

Page 40


Section 7

Work offset

Notes: 7.7 Settable zero offset All settable offsets, divided into coarse and fine offsets, are displayed in the "Work offset - G54...G57" window. Rotation, scaling and mirroring are displayed. 7.7.1 Selecting the function “Work offset - G54...G57” By pressing VSK 4 “G54...G57“ the following window opens.

7.7.2 Displaying and editing settable zero offset 1.


2.

Press the HSK 5 “Work offset“.

3.

Press the VSK 4 “G54…G57“. The “Work offset - G54...G57” window opens.

4.

Values can be edited directly in the table.

Note: The settable work offsets must first be selected in the program before they have an impact.


Page 41

B573

Section 7 Notes:

Work offset 7.8 Details of the work offset For each work offset, you can display and edit all data for all axes. You can also delete work offsets. For every axis, values for the following data will be displayed:  Coarse and fine offsets  Rotation  Scaling  Mirroring Notes: Settings for rotation, scaling and mirroring are specified here and can only be changed here. 7.8.1 Selecting the function “Work offset - details:“ By pressing the VSK 7 “Details“ a different work offset window opens, depending on the work offset (Active, Base, G54...G57) selected before:  “Work offset - details: Rotary table ref./Basic reference/ Total basic WO/G54 - G55/Tool reference/Workpiece ref./ Programmed WO/Cycle reference/Total WO“  “Work offset - details: 1. chan.-sp. Basic WO“  “Work offset - details: G54 - G57“

7.8.2 Displaying details of the work offset

B573

1.

Press the “MENU SELECT“-key on the operator panel and the HSK 2 “Parameter” to open the operating area “Parameter”. Alternatively press the “OFFSET”-key on the keyboard.

2.

Press the HSK 5 “Work offset”.

Page 42


Section 7

Work offset 3.

Press the VSK "Active", "Base" or "G54…G57". The corresponding window appears.

4.

Place the cursor on the desired work offset to view its details.

5.

Press the VSK 7 “Details”. A window opens, depending on the selected work offset, e.g. "Work offset - details: G54...G57".

6.

Enter changes of values directly into the table.

Notes:

- OR 6.

Press the VSK 1 “WO +“ or the VSK 2 “WO -“ to select the next or previous offset, respectively, within the selected area ("Active", "Base", "G54 to G57") without having first to switch to the overview window. If you have reached the end of the range (e.g. G57), you switch automatically to the beginning of the range (e.g. G54). - OR -

6.

Press the VSK 7 "Clear offset" to reset all entered values.

7.

Press the VSK 8 “Back” to close the window.

Note: The changes become effective immediately in the part program or after pressing the "RESET"-key. 7.9 Measuring the workpiece zero 1.


2.

Press the HSK 5 “Work offset”

3.

Press the VSK 4 ”G54...57”.

4.

Select the work offset in which the zero point ist to be saved by placing the cursor in an axis field right beside the corresponding work offset G54-57.

5.

Press the VSK 1 “Work Measure”. The operating area “Meas. Workp.” in the operating mode “JOG” opens.

6.

Press the VSK 2 “Set edge”, if not already active. The “Set edge” window opens

7.

Use the softkeys “X”, ”Y, “Z” to select in which axis direction you want to approach the workpiece first.

7

Select the measuring direction (+ or -) you want to approach the workpiece in. The measuring direction cannot be selected for Z0.

8.

In X0, Y0, or Z0, specify the setpoint position of the workpiece edge you are approaching. Traverse the tool up to the workpiece edge. Press the VSK 7 "Set WO" to measure the workpiece zero.

For more details see module B570 - “Operating mode JOG”, section 5 “Measuring the workpiece zero”. 828D/840Dsl SINUMERIK Operate

Page 43

B573

Section 8 Notes:

User variables The following variables can be defined:  Arithmetic parameters (“R variables”):  These are channel-specific variables that you can use within a G code program. G code programs can read and write R parameters. These values are retained after the control is switched off.  Global user data (Global GUD) are valid in all programs and can be defined as follows:  Keyword DEF  Range of validity NCK  Data type (INT, REAL,….)  Variable names  Value assignment (optional)  Channel-specific user data (“Channel GUD”) can be defined with a different value for each channel.  Local user data (LUD) are valid in one program.  Program-global user data (“PUD”) are valid in one program and the called subroutines. Local user data (“LUD”) defined in the main program can become program-global user data (“PUD”) by setting a machine datum. With that, they are valid in all subprograms, where they can be read and written. The PUD mode of action is depending on the machine settings. Only local and program-global user data can be displayed. Up to 15 decimal places (including the place after the column) are being evaluated. If a number with more then 15 decimals is being entered, then exponential number format is used (15 places +EXXX). 8.1

Selecting the function “User variable” By pressing the HSK 6 “User variable” the “R variables” window opens like displayed below.

B573

Page 44


Section 8

User variables 8.2

Notes:


Display area

Description By pressing the VSK 1.1 “R variables“ the “R variables” window opens. The entered values (R0 R999, depending on a machine datum) are retained after the control is switched off. By pressing the VSK 1.2 “Global GUD“ a list of ”Global user variables” (UGUD) defined by the user is displayed. Further selection is possible with VSK 1.6 “GUD selection”. By pressing the VSK 1.3 “Channel GUD” all channel-specific user variables will be displayed in a list. Further selection is possible with VSK 1.6 “GUD selection”. By pressing VSK 1.4 “Local LUD“ a list with local user data will be displayed. By pressing the VSK 1.6 “GUD selection”, depending on the softkeys pressed before VSK 1.2 “Global GUD” or VSK 1.3 “Channel GUD” a new vertical softkey will be displayed.  SGUD  MGUD Depending on the control configuration a additional area (UGUD) can be selected. SGUD: Definition of SIEMENS-system applications MGUD: Definitions of machine builder applications. UGUD: Definitions of user applications By pressing the VSK 1.7 “Search” you can search within all available lists for any user variable by entering an arbitrary character string. By pressing the VSK 1.8 “Extend” a new vertical softkey bar (VSK 2) with different functions opens. By pressing the VSK 2.1 “Delete” in the extended vertical softkey bar you can delete R variables in a defined range (from... to...) from the “R variables” list. Deleting must be confirmed with the VSK 1.8 OK” or aborted with the “Cancel” Softkey. Alternatively you can delete all R variable with the VSK “Delete all”. By pressing VSK 2.8 “Back“ you switch back to the vertical softkey bar 1.


Page 45

B573

Section 8 Notes:

User variables 8.3 Arithmetic parameters (R variables) “R variables” (arithmetic parameters) are channel-specific variables that can be used within a G code program. G code programs can read and write “R variables”. 8.3.1 Selecting the function “R variables” By pressing the VSK 1 “R variables” the following window opens.

8.3.2 Displaying and editing R variables

B573

1.

Press the “MENU SELECT“-key on the operator panel and the yellow HSK 2 ”Parameter” to open the operating area “Parameter”. Alternatively press the “OFFSET”-key on the keyboard to switch to the operating area “Parameter” directly.

2.

Press the HSK 6 “User variable”.

3.

Press the VSK 1.1 “R variables“. The “R variables” window opens

4.

Enter the desired “R variable” value in the corresponding “R variable” field.

Page 46


Section 8

User variables 8.3.3 Selecting the function “Delete R variables”

Notes:

After pressing the VSK 2.7 “Delete“ the following “Delete R variables” window opens.

8.3.4 Deleting R variables 1


2.

Press the VSK 8 “Extend”. The vertical softkey bar 2 opens.

3.

Press the VSK 2.7 “Delete“.

4.

Enter the range in which you want to delete “R variables”. Enter even numbers from the range 0 to 99. Accept the selection by pressing the VSK 8 “OK” or abort by pressing the VSK 7 “Cancel”. The selected “R variables” will be deleted. - OR -

5.

Press the VSK 6 “Delete all” to reset all R variables to 0 (zero). Accept your choice by pressing the VSK 8 “OK” or abort by pressing the VSK 7 “Cancel”. All “R variables” will be reset to 0 (zero).


Page 47

B573

Section 8 Notes:

User variables 8.4 Global user data “Global GUD” are NC global user data (Global User Data) which remain available after switching the machine off. GUD apply in all programs. A GUD variable can be defined through:  Keyword DEF  Range of validity NCK  Data type (INT, REAL, ….)  Variable names  Value assignment (optional) Example.: DEF NCK INT COUNTER1 = 10 Note: GUD are defined in files with the extension *.DEF. The following file names are reserved for this purpose: File name

Description

SGUD.DEF

Definitions for system data (reserved)

MGUD.DEF

Definitions for machine manufacturer data

UGUD.DEF

Definitions for user data

GUD4.DEF GUD7.DEF

Definitions for user data

8.4.1 Selecting the function “Global GUD“ By pressing the VSK 1.2 “Global GUD“ the following window opens.

B573

Page 48


Section 8

User variables

Notes:

8.4.1 Displaying and editing global GUD 1.

Press the “MENU SELECT“-key on the operator panel, then the HSK 2 “Parameter” to open the operating area “Parameter”. Alternatively press the “OFFSET”-key on the keyboard, to directly change into the operation area “Parameter”.

2.

Press the HSK 5 “User variable“.

3.

Press the VSK 1.2 “Global GUD“.

4.

The “Global user variables” window opens. A list of the defined “SGUD” variables respectively the data selected by VSK 6 “GUD selection” are displayed. -OR -

4.

By pressing the VSK 6 "GUD selection" further GUD data are available. Please refer to the manufacturer`s manual.


Page 49

B573

Section 8 Notes:

User variables 8.5 Channel specific user data Like the GUD, channel-specific user data are applicable in all programs for each channel. However, unlike GUD, they have specific values. A channel-specific GUD variable is defined with the following:  Keyword DEF  Range of validity CHAN  Data type  Variables names  Value assignment (optional) Example: DEF CHAN REAL X_POS = 100.5 8.5.1 Selecting the function “Channel GUD“ After pressing the VSK 1.3 “Channel GUD“ the following window opens.

8.5.2 Displaying and editing channel GUD 1.


2.

Press the HSK 5 “User variable”.

3.

Press the VSK 3 “Channel GUD“ and the VSK ´6 “GUD selection“ to select the specific GUD area. (See section 7.6 in this module)

B573

Page 50


Section 8

User variables

Notes: 8.6 Local user data LUD are only valid in the program or subroutine in which they were defined. The control displays the LUD after the start of program processing. The display is available until the end of program processing. A local user variable is defined with the following:  Keyword DEF  Data type  Variable names  Value assignment (optional) 8.6.1 Selecting the function “Local LUD“ After pressing the VSK 1.4 “Local LUD“ a window with all present local user variables opens.

8.6.2 Displaying local user data 1.


2.

Press the VSK 6 “User variable“.

3.

Press the VSK 1.4 “Local LUD“. The window with the local user data opens. If no local user data are defined the window stays blank.


Page 51

B573

Section 8 Notes:

User variables 8.7 Search You can search for R variables and user data directly. 8.7.1 Selecting the function “Search” Pressing the VSK 1.7 “Search” opens the “Find R variables” window.

8.7.2 Searching for R variables and user data.

B573

1.


2.

Press the VSK1.1 “R variable”, the VSK 1.2 “Global GUD”, the VSK 1.3 “Channel GUD” or the VSK 1.4 “Locale GUD” to select the list in which you would like to search for user data.

3.

Press the VSK 1.7 “Search”. The “Find R variable” or “Find user variable” window opens.

4.

Enter the desired search term in the orange marked input field and press the VSK 8 “OK” to accept or press the VSK 7 “Cancel” to abort the search. The cursor is automatically positioned on the R variable or user data you are searching for, if they exist.

Page 52


Section 9

Setting data With the function “Setting data” you have the option to install safety areas for the tool movement and to alter parameters for the spindle speed. 9.1

Notes:

Selecting the function “Setting data” By pressing the HSK 8 “Setting data” the “Working area limitation” window will be displayed.

9.2


Display area

Description By pressing the VSK 1 “Working area limit.” the working area limitation window opens, where you can install safety zones for the tool movement. By pressing the VSK 3 “Spindle data” the “Spindles” window opens, where you can set limitations for the Spindle speed. By pressing the VSK 6 “Data lists” the window “Setting data list” opens where you can select predefined lists of setting dates. Please refer to the machine manufacturer's documentation.


Page 53

B573

Section 9 Notes:

Setting data 9.3 Working area limitation The "Working area limitation" function can be used to limit the tool traverse range in all channel axes (e.g. X1, Y1, Z1, C1, AWZ1, SP2 and Z2). These commands allow you to set up protection zones in the working area which are out of bounds for tool movements. In this way, you are able to restrict the traversing range of the axes in addition to the limit switches. By marking the checkbox “active” the safety area is activated. 9.3.1 Selecting the function “Working area limitation” Note: You can only make changes in "AUTO" operating mode when in the “RESET” condition. These changes are then immediate. You can make changes in "JOG" operating mode at any time. These changes, however, only become active at the start of a new motion. By pressing the VSK 1 “Working area limit.” the “Working area limitation” window opens.

9.3.2 Specifying working area limitations

B573

1.


2.

Press the HSK 8 “Setting data”. The “Working area limitation” window opens.

3.

Place the cursor in the required field and enter the new values via the numeric keyboard. The upper or lower limit of the protection zone changes according to your inputs.

4.

Click the checkbox "active" to activate the protection zone.

Page 54


Section 9

Setting data

Notes: 9.4 Spindle data The speed limits set for the spindles that must not be exceeded, are displayed in the "Spindles" window. You can limit the spindle speeds in the fields "Minimum" and "Maximum" within the limit values defined in the relevant machine data. In the field "Spindle speed limitation for G96", the programmed spindle speed limitation at constant cutting speed is displayed together with the permanently active limitations. A additional limitation of the Spindle speed with constant cutting speed can be entered. This speed limitation, for example, prevents the spindle from accelerating to the max. spindle speed of the current gear stage (G96) when performing tapping operations or machining very small diameters. 9.4.1 Selecting the function “Spindle data” By pressing the VSK 3 “Spindle data“ the “Spindles” window opens.

9.4.2 Editing spindle data 1.


2.

Press the HSK 8 “Setting data”.

3.

Press the VSK 3 “Spindle data” The “Spindles” window opens.

4.

If you want to change the spindle speed, place the cursor on the "Maximum", "Minimum", or "Spindle speed limitation at G96" and enter a new value.


Page 55

B573

B573

Page 56


B574

1

Operating area “Program”

Brief description

Objective of the module: In this module you learn about the structure of the program editor in the operating area “Program“.

Description of the module: The SINUMERIK Operate provides the opportunity to create NC-programs, and also to integrate comfortably cycles into the program. These programs are created as G-code programs as per DIN 66025, however, elements of the high level language can be included. This module shows the general structure of a G-code programs. The creation of G-code programs is explained in detail in the following modules: B655 “Programming milling”, B656 “Programming contour milling” , B657 “Programming diverse functions” , and B575 “Operating area Program-Manger”.

Content: Structure of the program editor Options in the editor Screen elements and their meaning


Page 1


B574

B574

B574

Page 2


B574 Operating area Program: Description The SINUMERIK Operate provides the opportunity to create NC-programs, and also to integrate comfortably cycles into the program. These programs are created as G-code programs as per DIN 66025, however, elements of the high level language can be included. This module shows the general structure of a Gcode programs. The creation of G-code programs is explained in detail in the following modules: B655 “Programming milling”, B656 “Programming contour milling” , B657 “Programming diverse functions” , and B575 “Operating area ProgramManger”.

Operating area Program: START

Structure of the program editor

Options in the editor

Screen elements and their meaning

Operating area Program: END

Notes :


Page 3

B574

Section 2 Notes:

Structure of the program editor 2.1 Opening a program Press the “MENU SELECT“-key on the operator panel. The following screen of the Sinumerik Operate will be displayed. This example shows the part program NC/WKS/DOKU/DIN_DRILLING_1.

Press the HSK 3 “Program“ or the corresponding key on the keyboard. If a program is already loaded into the program editor, because it was processed or edited before, then it opens immediately. If no program was loaded before, then the program manager opens first, giving you the opportunity to select a program. - ORPress the HSK 4 „Program-Manager“ or the corresponding key on the keyboard. The program manager window opens with a view to the directory structure of the NC-memory. If the desired program is not on the NC-memory, then you can switch over to a local drive by pressing the HSK 2 “Local drive” or to an USB device (such as an USB stick, or USB hard drive) by pressing the HSK 3 “USB”.

See module B575 “Operating area Program manager“.

B574

Page 4


Section 2


Notes:

2.2 The NC main memory The memory structure shown in the picture below, with the 3 main directories  Part programs  Subprograms  Workpieces is always available on the NC, and does not have to be created.

1

1

Here you can see the free available main memory on the NC. The memory can not be fully used. If less then 0,1 MB is available, more memory should be freed by:  deleting unused programs  moving unused programs to another storage (e.g. memory stick). Directories: Directories are displayed with a folder icon in the program manager window and have the extension *.DIR (Directory) or *.WPD (work piece directory). Program/Data: Programs and data are displayed with a document icon.

Used file extensions: *.WPD = Workpiece *.MPF = Main program file *.SPF = Sub program file If the workpiece directory contains a part program with the same name as the directory, this part program is automatically selected for machining when the workpiece directory is selected. For example, with selecting the workpiece POCKET.WPD the main program POCKET.MPF is selected automatically. If an INI-file of the same name exists (e.g. POCKET.INI), it is executed once at the start of the part program selected. 828D/840Dsl SINUMERIK Operate

Page 5

B574

Section 2 Notes:

Structure of the program editor 2.3 Navigation and program selection Shown below is a directory tree of the opened NC-memory:

With the blue “cursor up” and the “cursor down” keys the orange cursor is being positioned and you can navigate through the directory tree in the program manager window. With the blue “cursor to the right” key you can open a folder or subfolder and select and open a file. In case of further subdirectories you can also extend the directory tree with the “cursor to the right”. Alternatively you can use the yellow “INPUT” key or the VSK 1.3 “Open”, to load a selected program directly into the program editor window. A double click with the mouse also opens the program file. The VSK 1.1 “Select” loads a selected program into the main memory of the NC, ready for machining.

With the “cursor to the left” key on the keyboard you can close the selected folders or subfolders and step back one level higher in the directory hierarchy.

B574

Page 6


Section 2


Notes:

2.4 The program editor By pressing the yellow HSK 3 “Program“, or the corresponding key on the keyboard the program editor window opens with the part program selected before, as long as the program was not closed explicitly with the VSK 2.7 “Exit” after editing. Shown below is the opened program editor with a part program loaded:

With the editor you can go through the program more clearly and make necessary changes by editing them. Note: The maximum record length amounts to 512 characters. The navigation in the editor window takes place with the blue cursor keys on the keyboard. NC blocks consist of the following components:  Commands (instructions) as per DIN 66025 (G-code programs)  Elements of the NC high-level language

If the editing of the program is finished, you can take over all changes in the program code with pressing the HSK 8 “NC Select”. The program is taken over and loaded to the machine. The screens switches to the operating area “Machine”. If the part program is already selected for machining the HSK 8 “Execute” appears . The screens switches to the operating area “Machine”. The program editor is described precisely in the module B600 and B604 “Basics of programming“.


Page 7

B574

Section 2 Notes:

Structure of the program editor 3.1 Horizontal softkey bar: In this section the general functions of programming with the SINUMERIK Operate will be described. More information is available in the corresponding modules.

By pressing the HSK 2 “Drill.“ the following cycles for drilling will be called up:  Centering  Drilling and Reaming  Deep hole drilling  Boring  Thread  Positions  Positions repetition See modules B608 and B609 - “Drilling“. By pressing the HSK 3 “Mill.“ the following cycles for milling will be called up:  Face milling  Pocket  Multi-edge spigot  Slot  Thread milling  Engraving See module B615 and B616 - “Milling”. By pressing the HSK 4 “Cont. mill.“ the following cycles for contour milling will be called up:  Contour  Path milling  Rough drill  Pocket  Pocket residual material  Spigot  Spigot residual material See module B623 and B624 - “Contour milling“.

B574

Page 8


Section 3

Options in the editor

Notes: By pressing HSK 6 “Various“ the following functions will be called up:  Blank  High-Speed-Settings  Subprogram See module B600 an B604 “Basics of programming”. By pressing the HSK 7 “Simulation“ the program run and the machining of the workpiece can be simulated. Different views on the simulated workpiece are available:  Top view  3D view  Further views  Details  Program control  Show tool path  Delete tool path  Blank See module B600 an B604 “Basics of programming”. Press the HSK 8 "Select" or “Execute” to change over to the operating area “Machine” and to start the machining of the program. See module B600 an B604 “Basics of programming”.


Page 9

B574

Section 4 Notes:

Screen elements and their meaning 4.1 The “Current block display” screen The following screen shows the actual machined program blocks.

1 2

3

1

Program name/Program path

2

Program code

3

Message bar

4.2 Help menu By pressing the “HELP“-key on the CNC-keyboard, the help window with the vertical softkey bar opens . If there is a specific help item for the current cursor position the corresponding help screen is shown.

B574

Page 10


Section 4

Screen elements and their meaning

Notes: If there is no specific help available the following screen is shown:

A message box with the note „No help available for „…“ appears. You can close this box with VSK 8 „OK“ and afterwards you can call a specific help directly below the line „Overview of Editor“.

4.3 Vertical softkey bar of the help menu Orange marked blocks will be taken over into the editor window. Shows all G-functions.

Opens a search mask for searching for help topics.

Enlarges the help window to full-screen.

Follows a reference to a help topic selected.

Returns to the table of content.

Closes the help window.


Page 11

B574

Notes:

B574

Page 12


B575

1

Operating area “Program manager“

Brief description

Objective of the module: In this module you learn to handle programs and files in the program manager of the Sumerik Operate. Description of the module: All NC-Programs, which are created with the Sinumerik Operate, are stored in the NC-work memory. These programs can be accessed via the program manager for:  execution  alteration  copying  renaming  deletion The SINUMERIK Operate provides the following means of data transmission of NC-programs to other storage media depending on the system components:  NC memory  Local drive memory  Its own hard disk (PCU 50.x)  Network connection  USB-storage (stick or drive) Note: The system components are described in the machine manufacturer documentation.

Content: Selection and function of the program manager Storage medium “NC” Storage medium “Local drive” Storage medium “USB” drive


Page 1


B575

B575

B575

Page 2


B575 Operating area Program Manager: Description All NC-Programs, which are created with the Sinumerik Operate, are stored in the NC-work memory. These programs can be accessed via the program manager for:  execution  alteration  copying  renaming  deletion The SINUMERIK Operate provides the following means of data transmission of NC-programs to other storage media depending on the system components:  Its own hard disk (only with 840D sl and PCU 50.x)  V.24-interface (with PCU 20 and PCU 50.2)  Floppy disk drive (only PCU 20 and PCU 50.2)  PCMCIA Card (only PCU 20)  Network connection  USB-storage (stick or drive)

Operating area Program Manager: START

Selection and function of the program manager

Storage medium “NC”

Storage medium “Local drive”

Storage medium “USB” drive

Operating area Program Manager: END

Note: The system components are described in the machine manufacturer documentation.

Notes :


Page 3

B575

Section 2 Notes:

Selection and functions of the program manager 2.1

Selecting the function „Program manager“

The program manager can be selected as follows: Press the “MENU SELECT”-key on the operator panel. The following horizontal softkey bar of HMI sl will be displayed:

Press the HSK 4 “Program manager“ to open the program manager window. - OR Press the “PROGRAM MANAGER“-key on the CNC -keyboard to open the program manager window directly. The following functions and softkeys will be available in the horizontal softkey bar of the Sinumerik Operate.

2.2

Horizontal softkey bar

Display area

Description By pressing the HSK 1 “NC“ all directories, folders and files of the NC/Hard disc will be displayed in a directory tree view in the program manager window. By pressing the HSK 2 “Local drive” all programs and directories on an allocated network drive or on an allocated user memory on a CF-Card at the NCU will be displayed. Prerequisite for this function is that the "Additional 256 MB HMI user memory on CF card of NCU" option is activated. For larger CFcards also more than 256 MB memory can be enabled. By pressing the HSK 3 “USB“ all programs and directories on an USB drive will be displayed in a directory tree view in the program manager window. Programs created on an external PC can be copied to an USB drive and transferred to the NC via the USB interface where they can be processed further. Direct processing from the USB flash drive is not recommended. The text on the Softkey e.g “USB” can also be replaced by a drive letter e.g. “G”. Note: Refer to the documentation of the machine manufacturer.

B575

Page 4


Storage medium “NC” 3.1

Section 3 Notes:

Selecting the function „NC“ By pressing the HSK 1 “NC“ the program manager opens .

The complete NC-memory is displayed along with all workpieces, the main programs and subroutines. The directories and programs are listed with the following information: (For navigation in the directory structure refer to module B574 “Operating area Program”, Section 2.3)  Name The name can contain up to 28 characters (24 characters for the name + dot + 3-character extension, e.g. MPF). Permissible characters include all upper-case letters (without accents), numbers, and underscores.  Type Directory/ Programs

*.WPD *.MPF *.SPF *.JOB *.TOA *.TMA *.UFR *.RPA *.GUD *.SEA *.PRO *.CEC *.INI

Directory Program Subprogram Job list Tool data Magazine Zero points R-Parameter Definitions Setting data Protection zone Sag Initialization program

(Workpiece Directory) (Main program File) (Subprogram File) (Job list) (Tool Offset Active) (Tool/Magazine data) (User Frame) (R-Parameter Active) (Global User Data) (Setting data) (Protection zones) (Sag/angularity) (Initializing Data)

 Size  The size of files of the selected directory is displayed in byte.  Date/Time  Date and time of file creation or last change 828D/840Dsl SINUMERIK Operate

Page 5

B575

Section 3 Notes:


Vertical softkey bar 1

Display area

Description By pressing the VSK 1.1 “Select“ you can select a program and change over to the operating area “Machine” in order to start machining the selected program. By pressing the VSK 1.2 “New“ you can create a new directory. In the selected directory you can create a new ShopMill- or a programGUIDE-program . (See section 3.4 in this module)

By pressing the VSK 1.3 “Open“ the selected program (marked with an orange cursor) will be opened. Alternatively you can also press the yellow “INPUT”-key on the keyboard or the blue “cursor to the right”-key to open a program. By pressing the VSK 1.4 “Mark“ several programs or directories can be marked for copying or cutting. (See section 3.5 in this module) By pressing the VSK 1.5 “Copy” one or several programs or directories can be copied. (See section 3.6 in this module) By pressing the VSK 1.6 “Paste” the copied program(s) or directorie(s) are inserted into the selected place in the directory tree of the NC, of a local drive or an USB drive. (See section 3.6 in this module) By pressing the VSK 1.7 “Cut“ one to several programs or directories can be cut out and inserted somewhere else on a location in the directory tree of the NC, a local drive or on an external USB drive. (See section 3.7 in this module) By pressing the VSK 8 “Extend” the extended vertical softkey bar 2 with new functions will be displayed.

Note: Files can not be copied under the same name into the same directory. The files are to be renamed.

B575

Page 6



Section 3 Notes:

3.3 Vertical softkey bar 2 Display area

Description (continuation) By pressing the VSK 2.1 “Archive” a new vertical softkey bar is opened (see section 3.10 “Archives”) By pressing the VSK 2.2 “Preview window“ a sub window opens below the file browser window, with a preview of the program code of the selected program (see picture in section 3.5). By pressing the VSK 2.6 “Properties“ the “Properties of ...” input mask opens where you can:  View program path and modify the program name.  View the time and date of creation.  View the time and date of last changing of the program or folder.  User rights for execution, writing, listing and reading of files and folders. (See section 3.11 “Properties“) By pressing the VSK 2.7 “Delete“ the program or folder marked with the cursor will be deleted. (See section 3.8) By pressing the VSK 2.8 “Back“ on the operator panel (OP) you switch back to the vertical softkey bar 1.


Page 7

B575

Section 3 Notes:


Starting a new NC-program Press the VSK 1.2 “New“ to start a new G-code program or workpiece. Depending on the cursor position the following input masks open.

If the cursor is placed on the folder for part programs or subprograms, then a new G-code program of the type “*.MPF” (for part programs) or “*.SPF” (for subprograms) is created by pressing the VSK 1.2 “New”. In the name field of the input mask, a name for the program with a maximum of 28 characters (name + point + extension) has to be entered.  Cursor is positioned on the directory (DIR): With the VSK 2.2 “Workpiece” you can create a new Workpiece directory (WPD).

 Cursor is positioned on or in the workpiece directory (WPD):  Press the VSK 2.3 “ShopMill” to create a new sequential program.

 Press the VSK 2.4 “programGUIDE G-code” to create a new

G code program. In this case you select between a main program (MPF) or a subprogram (SPF).

B575

Page 8


Storage medium “NC” 

Section 3

You can create a program of any type in every directory or subdirectory by pressing the VSK 5 “Any”. However in the area “local drive” and “USB” this does not apply. Only in the area “NC” you can create a program of different types (see the type list below).

Notes:

After pressing the VSK 1.2 “New” the following functions in the vertical softkey bar are available. 3.4.1 Vertical softkey bar Display area

Description By pressing the VSK 2 “Workpiece“ you can create a new workpiece of the type *.WPD (Workpiece directory). The current cursor position determines the folder where the workpiece is created. The “New workpiece” window opens. Note: The softkey is only available if the HSK 1 “NC“ was selected before. By pressing the VSK 2.3 “ShopMill” a new sequential program will be created. By pressing the VSK 2.4 “programGUIDE G code”, a new main program or subprogram will be created, depending on the program type selected in the input mask. By pressing the VSK 2.6 “Any“ an arbitrary program depending on the file type can be created (see the picture above). By pressing the VSK 2.7 “Cancel“ the actual selection will be discarded and the window closed. By pressing the VSK 2.8 “OK“ or pressing the “INPUT”-key on the keyboard the entered values or selection made will be accepted and the window closed.


Page 9

B575

Section 3 Notes:

Storage medium “NC” 3.4.2 Parameters for “New workpiece“ Parameter

Meaning

Type:

Program type:

 WPD

Workpiece directory

Name

Program name: The program name can only consist of a maximum number of 28 characters (Name + dot + 3-character extension, e.g. *.WPD). Permissible characters include all upper-case letters (without accents), numbers, and underscores (_).

3.4.3 Parameters for „New G code program“ Parameter

Meaning

Type:

Program type:

 MPF

Program (Main program file)

 SPF

Subprogram (Subprogram file)

Name

Program name (see section 3.4.2 above)

3.4.4 Parameters for “Any new program“

B575

Parameter

Meaning

Template

If templates are available, they are shown and selectable.

Type:

Program type:

 JOB

Job list

 TOA

Tool data

 TMA

Magazine assignment

 UFR

Zero points

 RPA

R-Variable

 GUD

Definitions

 SEA

Setting data

 PRO

Protection zones

 CEC

Sag compensation

 INI

Initialization program

Name

Program name (see section 3.4.2)

Page 10



Section 3 Notes:

Marking directories / NC-programs

First open the desired directory in the program manager, like described in sections 2.1 and 3.1. 1.

Place the cursor with the blue “cursor down”-key on the first program or folder that you want to mark.

2.

Press the VSK 4 “Mark“. The program or directory selected with the orange cursor is marked.

3.

Mark more NC-programs or directories by pressing the blue “cursor down”-key. All selected files or directories are marked grey.

Thereafter, the marked NC-programs can stored to the clipboard of the PCU by pressing the VSK 5 “Copy” or the VSK 7 “Cut” . The programs stored to the clipboard can then be:  Copied in a different directory or to a different storage device  Deleted from a directory (cut) and pasted into a different directory or storage device. Tip 1: To shortcut the marking process place the cursor on the first program or directory you want to copy. Now press the “SHIFT”-key on the keyboard, hold it pressed and move the cursor with the blue “cursor down” key to the last program or directory you want to copy. Release the “SHIFT”-key. The files are now marked. Tip 2: If you only want to mark a single program or directory place the cursor on the file and press the blue “SELECT”-key on the keyboard. The single file is now selected. Go on with copying, cutting or deleting, like described next. 828D/840Dsl SINUMERIK Operate

Page 11

B575

Section 3 Notes:


Copying and pasting directories / NC- programs

First open the desired directory in the program manager, like described in section 2.1 and 3.1 in this module. 1.

Move the cursor with the blue cursor keys to the directory or file which you want to copy. If you want to copy more then one program or directory, mark them first with the VSK 4 “Mark” (see section 3.5).

2.

Press the VSK 5 “Copy“.

3.

If the program is to be copied into another directory on the NC, move the cursor with the “cursor to the left”-key to the next higher level of the directory tree.

4.

Select the new directory where you want to copy the data with the “cursor up” and “cursor down”-key and open the directory by pressing the “cursor to the right” or the yellow “INPUT”-key on the keyboard.

5.

Alternatively you can select another storage medium e.g. local drive or USB drive on the horizontal softkey bar.

6.

By pressing the VSK 6 “Paste“ the program or directory can be inserted into the selected location. Accept with pressing the VSK 8 “OK” or abort with pressing the VSK 7 “Cancel”. The original file remains.

Tip 3: To shortcut the copying process place the cursor on the program or directory you want to copy and press the CTRL + C keys on the keyboard at the same time. In order to paste the file to another location move the cursor to that location and press CTRL + V at the same time.

3.7

Cutting out directories / NC-programs

First open the desired directory in the program manager, like described in section 2.1 and 3.1 in this module. 1.

2.

Move the cursor with the blue cursor keys to the directory or file which you want to cut out. If you want to cut out more then one program or directory, mark them first with the VSK 4 “Mark” (see section 3.5). Press the VSK 7 “Cut“. In the message line the message “1 element has been cut. It can now be pasted” will be displayed.

3.

If the program or directory is to be moved to another directory on the NC, move the cursor with the “cursor to the left”-key to the next higher level of the directory tree.

4.

Select the new directory with the “cursor up” and “cursor down”-key where you want to insert the data and open the directory by pressing the “cursor to the right” or the yellow “INPUT”key on the keyboard.

5.

Alternatively you can select another storage medium (e.g. USB stick) on the horizontal softkey bar.

Tip 4: To shortcut the cutting out of a program or directory place the cursor on the selected file and press the CTRL + X keys at the same time.

B575

Page 12


Storage medium “NC” 6.

3.8 1.

2.

3.9

Section 3

Press the VSK 6 “Paste“ to insert the clipped data to the directory or storage location of your choice. Accept your selection by pressing the VSK 8 “OK” or abort with pressing the VSK 7 “Cancel”. The source file or directory will be deleted.

Notes:

Deleting directories / NC-programs Move the cursor with the blue cursor keys to the directory or file which you want to copy. If you want to copy more then one program or directory, mark them first with the VSK 4 “Mark” (see section 3.5). Press the VSK 2.7 “Delete“ in the extended vertical softkey bar 2. Accept the deletion process with pressing the VSK 8 “OK” or abort with pressing the VSK 7 “Cancel”. The selected program or directory will be deleted.

Opening a preview window

1.

Press the VSK 2.2 “Preview window” in the extended VSK-bar. The preview sub window opens directly below the program manager window.

2.

Use the blue cursor keys to navigate to the program you want to preview. The program code of the selected program is now displayed in the preview window.

3.

To deselect the function press the VSK 2.2 “Preview window” again. The preview window disappears.

Note: You cannot edit program code in the “preview window”. Tip 5: Press the “NEXT WINDOW“-key on the keyboard to activate the preview window. Now you can navigate freely through the program code by using the blue cursor keys. Tip 6: The preview window stays active, even if you switch back to the vertical softkey bar 1, in order to copy or cut a program or directory.


Page 13

B575

Section 3 Notes:

Storage medium “NC” 3.10 Generating archive files of programs and directories 3.10.1 Vertical softkey bar Pressing the VSK 2.1 “Archive” in the extended VSK-bar, will open the next vertical softkey bar. After pressing the VSK 3.1 “Generate archive” the following input mask appears to select the storage location.

With the VSK 3.7 “Back” you can go back to the previous vertical softkey bar. Afterwards the storage location is selected the next mask appears to enter the name of the archive file.

Pressing the VSK 4.2 “New directory” will open an input mask “New directory”, where you can define a new directory at the selected cursor position. Pressing the VSK 4.7 “Cancel” will abort the generating of archive files and the first vertical softkey bar is selected. Pressing the VSK 4.0 “OK” will start generating the archive file.

B575

Page 14



Section 3

3.11 Properties of programs and directories

Notes:

By pressing the VSK 2.6 “Properties” in the extended vertical softkey bar depending on the cursor position and the selected program (here TEST.MPF) the “properties of ....”-window with security options for the selected program or directory opens.

Note: You can change the program name and the rights. Parameters

Meaning

Path and name:

Program path and Program name; The program with the name “TEST1.MPF” is located in the folder NC/Workpieces/DOKU.

Created:

Date and time of creation: On the right side of the field “Created”: Date and time of creation are displayed here.

Changed:

Date and time change: On the right side of the field “Changed”: Date and time since the last edit of the program are displayed.

Rights:

User rights for executing, writing, listing and reading of a program or directory. 7 protection levels are possible (level 1 highest protection level, level 7 the lowest).

 Protection level 1 Manufacturer

Protected by password

 Protection level 2 Service


 Protection level 3 User


 Protection level 4 Programmer

Key switch 3

 Protection level 5 Qualified worker

Key switch 2

 Protection level 6 Skilled worker

Key switch 1

 Protection level 7 Semi skilled worker

Key switch 0


Page 15

B575

Section 4 Notes:


Selecting the function “Local drive“ By pressing the HSK 2 “Local drive“ the program manager shows the directory structure of the local drive.

A complete listing of all folders and files of the local drive is shown in the program manager window. For a description of the information of name, type, length and date/time displayed in this window, see section 3.1. 4.2


The full functionality available under the NC program manager window is available by pressing the HSK 2 “local drive” or HSK 3 “USB” (see section 3 in this module). Additional, here you can create a new directory by pressing the VSK 1 “Directory”. By pressing the VSK 1 “Directory” the “New directory” input mask opens where you can create a new directory on the local drive. Enter a name for the new directory and accept with pressing the VSK 8 “OK”, or abort with the VSK 7 “Cancel”.

B575

Page 16


Storage medium “USB” drive 5.1

Section 5 Notes:

Selecting the function “USB“ By pressing the HSK 3 “USB“ the following directory tree of the USB drive is displayed.

A complete listing of all folders and files of the USB drive is shown in the program manager window. For a description of the information displayed in this window, see section 3.1. 5.2


The full functionality available under the NC program manager window is available by pressing the HSK 2 “local drive” or HSK 3 “USB” (see section 3 in this module). Additional, here you can create a new directory by pressing the VSK 1 “Directory”. By pressing the VSK 1 “Directory” the “New directory” input mask opens where you can create a new directory on the USB drive. Enter a name for the new directory and accept with pressing the VSK 8 “OK”, or abort with the VSK 7 “Cancel”.


Page 17

B575

B575

Page 18


B576

1

Operating area “Diagnostics”

Brief description

Objectives of the module: With this module you learn to recognize and understand the alarms and messages that can occur during the operation of the machine. Furthermore you learn to correct the problems indicated by alarm messages. Description of the module: Faulty states which can occur during operation are shown in an alarm list on the Sinumerik Operate. If necessary the operation is interrupted, depending on the kind of error. The operator can acknowledge alarms or delete them. Messages give hints to certain behaviour patterns of cycles and to the machining progress. Generally they are displayed during a processing stage or at the end of a cycle. All present alarms and messages are shown in a sequential order of appearance in a alarm protocol.

Content: Selection and function of the operating area “Diagnostics” Displaying and handling alarms Displaying messages Alarm log


Page 1


B576

B576

B576

Page 2


B576 Operating area Diagnostics: Description Faulty states which can occur during operation are shown in an alarm list on the Sinumerik Operate. If necessary the operation is interrupted, depending on the kind of error. The operator can acknowledge alarms or delete them. Messages give hints to certain behaviour patterns of cycles and to the machining progress. Generally they are displayed during a processing stage or at the end of a cycle. All present alarms and messages are shown in a sequential order of appearance in a alarm protocol.

Operating area Diagnostics: START

Selection and function of the operating area “Diagnostics”

Displaying and handling alarms

Displaying messages

Alarm log

Operating area Diagnostics: END

Notes :


Page 3

B576

Section 2 Notes:

Selection and function of the operating area “Diagnostics” 2.1

Selecting the operating area “Diagnostics“

The operating area “Diagnostics” can be selected as follows: Press the “ALARM”-key on the CNC-Keyboard. The operating area “Diagnostics” opens immediately. - OR Press the “MENU SELECT”-key on the CNCkeyboard. The following horizontal softkey bar opens on the Sinumerik Operate.

Press the HSK 5 “Diagnostics“ to open the operating area “Diagnostics”.

The following softkeys and functions are available in the horizontal softkey bar of the operating area “Diagnostics“. 2.2

Horizontal softkey bar 1 (HSK)

Display area

Description By pressing the HSK 1.1 “Alarm list“ the “Alarms”window opens. See section 3 “Alarm list”. By pressing the HSK 1.2 “Messages“ the “Messages” -window opens and PLC or program massages are being displayed. See section 4 “Messages”. By pressing the HSK 1.3 „Alarm log“ a protocol list with all alarms and messages opened so far, are being displayed. See section 5 “Alarm log“. By pressing the HSK 1.4 “NC/PLC variab.“ a window opens where you can observe and modify PLC memory locations and NC system variables. This function is described in the commissioning manual of the Sinumerik Operate. By pressing the HSK 1.6 “Remote diag.“ a window opens where you can make the settings for remote diagnostics (RCS). This function is described in the commissioning manual of the Sinumerik Operate.

B576

Page 4


Selection and function of the operating area “Diagnostics”

Section 2 Notes:

By pressing the HSK 1.8 “Version“ als software components with their version information will be displayed. This function is described in the commissioning manual of the Sinumerik Operate.

2.3

Horizontal softkey bar 2 (HSK)

Display area

Description By pressing the HSK 2.1 “BUS TCP/IP“ in the extended horizontal softkey bar, the profibus status for diagnostic purposes during the configuration or when errors occur will be displayed. This function is described in the commissioning manual of the Sinumerik Operate. By pressing the HSK 2.2 “Axis diag.“ in the extended horizontal softkey bar the “Service overview”-window opens. This function is described in the commissioning manual of the Sinumerik Operate. By pressing the HSK 2.3 “SI diag.” in the extended horizontal softkey bar the “Safety integrated status”window opens. This function is described in the commissioning manual of the Sinumerik Operate. By pressing the HSK 2.7 “System utiliz.” in the extended horizontal softkey bar, the “System utilization”-window opens where the system resources for the NC areas are shown. This function is described in the commissioning manual of the Sinumerik Operate. By pressing the HSK 2.8 “Drive system“ in the extended horizontal softkey bar the “Overview for the drive states”-window opens. This function is described in the commissioning manual of the Sinumerik Operate.


Page 5

B576

Section 3 Notes:

Displaying and handling alarms 3.1

Selecting the function “Alarm list” Press the HSK 1.1 “Alarm list” to open the “Alarms”-window like displayed below. All present alarms are displayed here and can be acknowledged.

If faulty conditions are recognized in the operation of the machine, then an alarm will be generated and, if necessary, the machining will be interrupted. The error text that is displayed together with the alarm number gives you more detailed information on the error cause.  Date and time - If a faulty condition is determined in the control, the system time (hh:mm:ss) and system date (TT.MM.YY) is monitored and displayed in a list. The date is above the clock time.  Clearing criterion - For every alarm an icon shows the key that has to be pressed on the keyboard to clear the alarm (here the “ALARM CANCEL” -Taste auf dem Keyboard).  Alarm number - The alarms are displayed with an alarm number, in sequence of their occurrence.  Alarm text - The alarm text describes the error in short words. Attention: Please check the situation in the plant on the basis of the description of the active alarm(s). Eliminate the cause/s of the alarm/s and acknowledge it/ them as instructed. Failure to observe this warning will place your machine, workpiece, stored settings and eventually even your own safety at risk.

B576

Page 6


Section 3

Displaying and handling alarms 3.2

Notes:


Press the HSK 1.1 „Alarm list“ and select the Alarm with the blue cursor key on the keyboard. Press the following vertical softkeys shown in the VSK-bar to delete or acknowledge the Alarm. Display area

Description Press the VSK 1 “Delete HMI alarm” to delete a marked alarm. -ORPress the VSK 2 “Acknowl. alarm“ to delete a PLC alarm of the SQ type (Alarm numbers starting from 800000).

Note: The softkeys are activated when the cursor is placed on the corresponding alarm. 3.3

Acknowledgement symbols

Symbol

Instruction Turn the unit off and back on (main switch), or press “NCK POWER ON”. Press the “RESET”-key. Press the “ALARM CANCEL"-key. Press the “Acknowl. HMI alarm”-key. Press the key provided by the manufacturer.

3.4

Deleting or acknowledging an alarm

1.

Press the “MENU SELECT”-key on the CNCkeyboard and the yellow HSK 5 “Diagnostics”. Alternatively press the “ALARM”-key on the CNCkeyboard. The operating area “Diagnostics” opens.

2.

Press the VSK 1.1 “Alarm list” to open the “Alarms”window.

3.

Navigate the cursor with the blue cursor keys to the corresponding alarm.

4.

Press the corresponding key on the keyboard that is displayed in the alarm line. - OR -

4.

Press the VSK 1 “Delete HMI alarm” to cancel a HMI alarm. - OR -

4.

Press the VSK 2 “Acknowl. Alarm” to delete a PLC alarm of the SQ type (alarm number as of 800000).

The alarms are now deleted.


Page 7

B576

Section 4 Notes:

Displaying messages 4.1

Selecting the function “Messages By pressing the HSK 1.2 “Messages” the “Messages”-window opens, showing PLC and part program messages during machining.

PLC and part program messages may be issued during machining. Messages provide information with regard to a certain behaviour of the cycles and with regard to the progress of machining and are usually kept beyond a machining step or until the end of the cycle.  Date and time - On the occurrence of the message, the actual system time (hh:mm:ss) and system date (TT.MM.YY) are displayed in this list. The date is above the clock time.  Number - Message number only displayed for PLC messages.  Text - Message text in short words. Note: These message will not interrupt the program execution.

B576

Page 8


Section 5

Alarm log 5.1

Notes:

Selecting the function “Alarm log” By pressing the HSK 1.3 “Alarm log” the following “Alarm log”-screen will be displayed.

A maximum of up to 32000 alarm messages can be displayed in the „Alarm log“ window. They are shown chronological ordered with the following parameters:  Raised - If the alarm message is raised, the actual system time (hh:mm:ss) and system date (TT.MM.YY) is displayed in a list. The date is above the clock time.  Cleared - If the alarm message is cleared, the actual system time (hh:mm:ss) and system date (TT.MM.YY) is displayed in a list. The date is above the clock time.  Number - In this column the alarm number or massage is being output .  Text - In this column a short description of the alarm or massage is being output. Note These message will not interrupt the program execution.


Page 9

B576

Section 5 Notes:

Alarm log 5.2


Display area

Description By pressing the VSK 1 “Display new” the actual alarm log list will be updated. By pressing the VSK 6 “Settings” the “Settings” input mask opens, where you can limit the numbers of entries in the log list and decide to write the log into a file on the control. By pressing the VSK 7 “Store log” the actual alarm log is stored as a text file.

5.3

Showing and saving alarm logs

1.

Press the “MENU SELECT“-key on the operator panel and then the yellow horizontal softkey 5 “Diagnostics“. Alternatively you can press the “Alarm”-key on the keyboard. The operating area “Diagnostics” opens.

2.

Press the VSK 3 “Alarm-log.“. The “Alarm log” window opens with the corresponding vertical softkey bar.

3.

Press the VSK 1 “Display new” to update the log list. - OR -

3.

Press the VSK 2 “Settings” to open the “Settings”input mask. In the “Number of entries”-field enter values for the maximum number of entries (maximum 32000) that shall be displayed in the log window and in the “Write mode file” select:  “off“, if the changes are not to be written to a file.  “At every event“, if every change is to be written to a file.  “Time-controlled” if the file is to be overwritten after a particular time period. A new option field opens where you can insert the write interval in seconds. Accept your inputs by pressing the VSK 8 “OK” or abort with pressing the VSK 7 “Cancel”. - OR -

3.

B576

Press the VSK 7 “Store log” to save the log directly to the file: card/user/sinumerik/hmi/log/alarm_log/alarmlog.txt on the on the control.

Page 10


B577

1

Operating area “Start-up”

Brief description

Objective of the module: In this module you learn to adjust the operating interface of the Sinumerik Operate to your local language and to set the password and the key-switches.

Description of the module: The user interface is adjustable to the most common global languages English, French, German, Italian, simplified Chinese and Spanish, which you can select from a list. Furthermore you can adjust the functionality of the user interface and so the functionality of the control to different levels of user groups, which allows different user groups different operations on the machine, depending on their knowledge and education. This can be done by passwords and key switches. Content: Start-up


Page 1


B577

B577

B577

Page 2


B577 Operating area Start-up: Description The user interface is adjustable to the most common global languages English, French, German, Italian, simplified Chinese and Spanish, which you can select from a list. Furthermore you can adjust the functionality of the user interface and so the functionality of the control to different levels of user groups, which allows different user groups different operations on the machine, depending on their knowledge and education. This can be done by passwords and key switches.

Operating area Start-up: START

Start-up

Operating area Start-up: END

Notes :


Page 3

B577

Section 2 Notes:

Start-up 2.1

Selecting the operating area “Start-up“

The operating area “Start-up” can be selected as follows: Press the “MENU SELECT”-key on the operator panel. The following horizontal softkey bar of the Sinumerik Operate is displayed.

Press the HSK 6 „Start-up“, to open the window for Start-up. The “Machine configuration“ window opens.

2.2 Horizontal softkey bar Display area

Description By pressing the HSK 1 “Mach. data“ the “General MD”-window opens. The display of the machine data or drive mechanism depend on the configuration of the control. The access rights to the machine data are restricted by the position of key switches or passwords. This function is described in the commissioning manual of the Sinumerik Operate. By pressing the HSK 6 “System data” the “System data”-window opens. This function is described in the commissioning manual of the Sinumerik Operate.

B577

Page 4


Section 2

Start-up

Notes:

2.2 Vertical softkey bar Display area

Description By pressing the VSK 3 “Change language” you can adjust the user interface language to the language of your choice. By pressing the VSK 6 “Password“ the VSK 1 “Set password” becomes active. You can switch to different protection levels of the control by using different passwords.

2.3 Selecting the function “Change language” By pressing the VSK 3 “Change language” the “Language selection”-window opens.

2.4 Changing the user language 1.

Press the “MENU SELECT”-key on the operator panel. The yellow horizontal softkey bar opens.

2.

Press the HSK 6 „Start-up“.

3

Press the VSK 3 “Change language” The “Language selection” window opens.

4

Move the orange cursor over the language field of your choice, by using the blue cursor keys. Accept your selection by pressing the VSK 8 “OK” or abort with pressing the VSK 7 “Cancel”. The Sinumerik changes the user interface language to the language of your choice.

Tip: You can change the user language of the interface directly at any time by pressing the “CTRL” + “L” key on the keyboard simultaneously. 828D/840Dsl SINUMERIK Operate

Page 5

B577

Section 2 Notes:

Start-up 2.5 Selecting the function “Password” The access to programs, data and functions is restricted user-oriented by 8 hierarchical protection levels. They are separated into:  4 password levels for system, machine manufacturer, commissioner, and user  4 key-switch positions for the end user There are the protection levels 0 - 7, where 0 is the highest and 7 is the lowest level. By pressing the VSK 6 “Password” and VSK 1 “Set password” an input mask opens where you can set a new protection level by entering a password.

2.6

Changing the protection level via password

1.

Press the “MENU SELECT”-key on the operator panel. The yellow horizontal softkey bar opens.

2.

Press the HSK 6 „Start-up“.

3.

Press the VSK 6 “Password”.

4.

Press the VSK 1 “Set password”. The “Define password” input mask opens.

5.

Enter the password in the orange marked input field and accept with pressing the VSK 8 “OK” or abort with pressing the VSK 7 “Cancel”. Note: The additional softkeys and functions “Set password” and “Change password” are only accessible at a higher protection level.

B577

Page 6


B604

1

Basics of programming with the programGUIDE

Brief description

Objective of the module: Working with this module you will learn the concept of the G code programming with help of the programGUIDE under ShopMill . Description of the module: This module explains the general program structure of a ShopMill G code program, programmed with the programGUIDE. Furthermore the functions of the “Editor“ are described, as well as the functions “Various “, “Simulation“ and “NC-Selection“. Content: Basics Creating G-code programs Editor Various Simulation NC Execute


Page 1


B604

B604

B604

Page 2


B604 Basics of the Programming with the programGUIDE: Description

Basics with programGUIDE: START

This module explains the general program structure of a ShopMill G code program, programmed with the programGUIDE. Furthermore the functions of the “Editor“ are described, as well as the functions “Various “, “Simulation“ and “NCSelection“.

Basics

Creating G-code programs

Editor

Various

Simulation

NC Execute

Basics with programGUIDE: END

Notes :


Page 3

B604

Section 2 Notes:

Basics 2. 1 G code programming with ShopMill ShopMill offers beside the manual operation area, also the possibility, to create a NC-program on the control. These programs can be chained sequential programs, G code programs or a mixture of both. If you do not want to program with the ShopMill functionality, you can generate G code programs with G code commands in the ShopMill user interface. G code commands can be programmed as per DIN 66025. Note: The creation of chained sequential programs is discussed in detail in the module -B600 „Basics of programming with ShopMill”. With the G code programming in ShopMill, with the programGUIDE, parameter masks guide you in the process of measuring, the programming of contours, as well as drilling and milling cycles. From within the parameter masks, G code will be generated, which can also be translated back into the parameter masks. The following functions support the programming of G code programs:  Technology oriented program step selection (cycles) using softkeys  Input masks and -windows for parameters, with animated help graphics  Context sensitive online help for every input mask and window  Comfortable definition of the blank  Support for the contour input (geometric processor) G code programs can be represented in different views:  As a work plan showing the call up of the tool, path commands, revolution settings, spindle data, feed, cycle calls, the program end, etc.

B604

Page 4


Section 2

Basics

Notes:  As a parameter mask, with 3-D help pictures and animation during parameter input, with the VSK 2 “Graphic view” deactivated.

 As a parameter mask with an outline drawing during parameter input, with the VSK 2 “Graphic view” activated.

Note: The animated help pictures are displayed always in the correct position to the adjusted coordinate system. The parameters are dynamically displayed into the graphic and are highlighted in a different colour.


Page 5

B604

Section 2 Notes:

Basics 2.2 General program structure In general, a G code program can be programmed freely. For a good legibility however, the following structure is recommended: 1

Zero point selection, plane selection, absolute dimensioning

2

Blank attribution for the simulation

3

Tool call-up and tool change

4

Technology data, path commands

5

Programming of the technologies (cycles)

5

Program end

1 2 3 4 5 6

B604

Page 6


Section 2

Basics 2.3 Standard commands in the G code Editor

Notes:

Unlike in a program with ShopMill functionality, the following G-code commands are programmed through graphically supported parameter masks, where as in the programGUIDE G-code editor they have to be specifically typed into the editor. Note: Unnamed G commands are freely selectable. The documentation by the machine manufacturer must be observed. Command

Meaning

G 00

Rapid traverse command

G 01

Linear interpolation (Feed motion)

G 02

Circular interpolation clockwise

G 03

Circular interpolation anti-clockwise

G 04

Dwell time: additional parameters F or S are required

G 17

Plane selection XY

G 18

Plane selection ZX

G 19

Plane selection YZ

G 54 - G 57

Selection of the zero points Note: More zero points may be available. The documentation by the machine manufacturer must be observed.

G 90

Absolute dimensions

G 91

Incremental dimensions

The following standard M commands are available in the G code editor. Note: Unnamed M-commands are freely selectable. The documentation by the machine manufacturer must be observed. Command

Meaning

M00

Programmed Halt

M01

Optional Stop, see also M00

M02

End of Program

M03

Spindle Start clockwise

M04

Spindle Start anti-clockwise

M05

Spindle Stop

M06

Tool change

M08

Coolant ON

M09

Coolant OFF

M19

Defined spindle stop

M30

End of Program (see also M02)


Page 7

B604

Section 2 Notes:

Basics The following standard “other“ commands are available in the G code editor. Note: The documentation by the machine manufacturer must be observed. Com- Meaning mand T

Tool call-up (Tool)

S

Speed (Speed)

F

Feed rate (Feed)

2.4 Navigation in the editor window For a fast and comfortable navigation within a G code program and the parameter masks you can use the blue cursor keys. With the blue “cursor-up”-key on the keyboard you can navigate upwards in the program editor and the parameter masks. With the blue “cursor-down”-key on the keyboard you can navigate downwards in the program editor and the parameter masks. The arrow symbol (extend symbol) on the right side of a cycle or workpiece line in the editor window indicates that you can enter the parameter input mask by pressing the “cursor-to-the-right”-key (see picture below).

The “cursor-to-the-right”-key opens the parameter mask of the corresponding program block. The “cursor-to-the-left”-key closes the parameter mask for the cycle or workpiece settings and brings you back to the editor window, displaying the G code program.

B604

Page 8


Section 3

Creating G code programs 3.1 Creating a new G code program or opening an existing one

Notes:

A new G code program can be created from the operating modes “JOG”, “MDA” and “AUTO” as follows: Press the “Program Manager“-key on the keyboard. The program manager for creating and administering programs opens directly. See module B575 - „Operating area Program Manager“. - OR Press the “MENU SELECT“ key on the operator panel (OP). Press the yellow HSK 1.4 “Program Manager“. The program manager for creating new programs and administering existing programs opens. - THEN Select a storage drive (by pressing the horizontal softkey “NC”, “Local drive” or “USB”) where you want to create the program. Move the orange cursor with the blue cursor-keys to the directory of your choice. For the navigation process refer to the modules B566 “Operating elements“ or B575 - “Operating area Program Manager“. Press the VSK 2 “New”. The vertical softkey bar with functions for creating new programs opens. Press the VSK 3 „programGUIDE G code“, to open the input mask for creating a new ShopMill G code program. Here you can create a new main program

or a new subprogram.

Enter a name for the program and confirm your input by pressing the VSK 8 “OK”, or abort with pressing the VSK 7 “Cancel”.


Page 9

B604

Section 3 Notes:

Creating G code programs After creating a new programGUIDE program, the program is loaded into the G code editor in the operating area “Program”, where all the functions for tool selection, entering and editing G code commands and cycles are available (see picture below).

3.2 Programming a tool Within the editor, tools can be selected and inserted in the G code program comfortably by using a softkey. Under the function “Edit” HSK 1 press the VSK 1.1 “Select Tool” to open the tool list in the operating area “Parameter”. Press the VSK 1.2 “New tool” to create a new tool (see module - B573 “Operating area Parameter”). - OR Select an already existing tool from the tool list by placing the orange selection cursor on that tool and pressing the VSK 1.1 “To program”. Afterwards program the tool change (M06), the spindle start (M03/M04), the coolant (M07/M08), the speed (S...), the feed (F) and if needed, some tool specific functions.

B604

Page 10


Section 3

Creating G code programs

Notes:

3.3 Programming the blank The blank is needed for the simulation and the simultaneous recording. Only with a blank, that represents the real blank as precise as possible, a accurate simulation is possible. For the blank you have to define the shape (Block, Pipe, Cylinder, N-corner or Block centric) and dimensions. In the operating area “Program” press the HSK 1.6 “Various” to open the vertical softkey bar with “various” functions. Here, press the VSK 1.1 “Blank” to open the input mask for defining the blank. Fill in the needed parameters and press the VSK 8 “Accept” to take over the blank settings into the program, or abort by pressing the VSK 7 “Cancel” (see section 5.3). 3.4 Programming a cycle Cycles (technologies) can be programmed easily by using softkeys and parameter masks as follow. In the operating area “Program” press the HSK 1.2 “Drill.”, or press the HSK 1.3 “Mill.”, or press the HSK 1.4 “Cont. mill.”, to open the cycles for drilling, milling or contour milling. Select the corresponding technology (cycle) and a position pattern and accept the input. See module B609 - “Drilling“, B616 - “Milling” and B624 - “Contour milling“. 3.5 Inserting G code and programming the program end In the G code editor window several functions for inserting, copying and cutting G code commands are available. In the operating area “Program” press the HSK 1 “Edit” to program a part program with G code commands or to edit an already loaded program. Then program the program end (M02/M30) (see section 4). Press the HSK 1.7 “Simulation“ to simulate the machining (see section 6). - OR Press the HSK 1.8 “NC Execute” to load the program to the NC memory, ready for machining (see section 7).


Page 11

B604

Section 4 Notes:

Edit With the editor you can create, supplement, or change part programs. 4.1 Selecting the function “Edit” The program editor can be opened from the operating modes “JOG”, “MDA” or “AUTO”. By pressing the “PROGRAM“-key on the keyboard the editor window opens directly, with the last opened program. If no program was loaded before, the program manager window opens instead, where you can create or select an existing program. - OR Press the “MENU SELECT“-key on the operator panel. Press the yellow HSK 3 “Program” to open the operating area “Program”. By default the editor window opens with the last opened program (see picture below). Note: If the function is not active, press the HSK 1 “Edit“. If no program had been opened for editing purpose, then the Sinumerik Operate opens the Program Manager window, offering a chance to the user for choosing the desired program for editing. For further details see module - B574 “Operating area Program”, and also module - B576 “Operating area Program Manager”.

The following softkeys are available for editing a program:

B604

Page 12


Section 4

Edit

Notes:


Description The VSK 1.1 “Select tool” opens the tool management area (tool list) in the operating area “Parameter”. Here you can select an existing tool or create a new one. By pressing the VSK 1.1 “To program” you can insert the selected tool data into the G code program. By pressing the VSK 1.3 “Search“ you can search for any text in the current program. A search window opens where you can enter a search string. You can continue searching afterwards (see section 4.3). By pressing the VSK 1.4 “Mark” you can mark one or several program blocks in order to copy or cut (delete) them. By pressing the VSK 1.5 “Copy” you can copy one or several program blocks to the internal memory of the control, to paste them to a different location in the active program or to another program. By pressing the VSK 1.6 “Paste“ copied program code can be inserted anywhere into the active program or into another program on a different location. The pasted program code will be inserted behind the program block marked with the orange selection cursor in the work plan. You can paste the code to the active program as well as to another program on the NC, local drive or USB-drive. By pressing the VSK 1.7 “Cut” you can cut out one or several program blocks, to paste them later somewhere in a program or to delete them. Cut program steps remain in the clipboard and can be inserted again with the VSK 1.6 “Paste” (see VSK 1.6 “Paste“). By pressing the VSK 1.8 “Extend“ the extended vertical softkey bar 2, with the following functions, will be displayed. By pressing the VSK 2.3 “Renumbering” you can assign new numbers for every program step in the editor window. (see section 4.4). By pressing the VSK 2.6 “Settings“ you can change the setting for the program editor (see section 4.5). By pressing the VSK 2.7 “Exit” you close the editor with the active program. By pressing the VSK 2.8 “Back“ you switch back to the vertical softkey bar 1.


Page 13

B604

Section 4 Notes:

Edit 4.3

Search

With the function “Search” you can search for any text in a sequential program and even replace the text with other text. 4.3.1 Selecting the function “Search“ By pressing the VSK1.3 “Search” the search window opens, where you can search for any program code in the current program.


Description By pressing the VSK 1 “Go to start” the cursor will be positioned on the first line of the program. By pressing the VSK 2 “Go to end” the cursor will be positioned on the last line of the program. By pressing the VSK4 “Search” the search mask opens, where you can decide to search for complete words, select the search direction (forward/ backwards) and enter the search text. By pressing the VSK5 “Find + replace” the “Search and replace” mask opens where you can decide to search for complete words, select the search direction (forward/backwards), enter the search text and enter the text you want to use for the replacement. With pressing the VSK 7 “Cancel” you can abort the search process. By pressing the VSK 8 “OK“ you start a search run with the above mentioned search criteria.

B604

Page 14


Section 4

Edit 4.4

Notes:

Renumbering

With the function “Renumbering” you can renumber manually the program steps in the work plan with an increment you can select here. 4.4.1 Selecting the function “Renumbering“ By pressing the VSK 2.3 “Renumbering” the input window opens where you can change the settings for the renumbering of the program blocks in the editor window.

4.4.2 Parameters for “Renumbering” Parameters

Meaning

First block number

The first block number you want to start with. The values shown here by default can be adjusted under the function “Settings” in the input field “First block number” (see section 4.5).

Increment

The Increment between the program blocks. The values shown here by default can be adjusted under the function “Settings” in the input field “Increment” (see section 4.5).


Page 15

B604

Section 4 Notes:

Edit 4.5 Settings With the function “Settings” you can change the settings for the program editor. 4.5.1 Selecting the function „Settings“ By pressing the VSK 2.6 “Settings” the settings window for the program editor opens.

4.5.2 Parameters for “Settings” Parameters

Meaning

Number automatically (Yes/No)

Program blocks will be numbered automatically. Deactivating this parameter, hides the following two parameters too.

First block number

Block number of first block.

Increment

Increment between block numbers.

Show hidden lines (Yes/No)

Show hidden line (with the ID ;*HD).

Display block end as A symbol is displayed at the end of each block. symbol (Yes/No)

B604

Move horizontally (Yes/No)

Blocks are displayed in one line with a scroll bar at the right side.

Save automatically (only local and external drives) (Yes/No)

Changes are saved automatically without a query.

Page 16


Section 5

Various

Notes:

5.1 Selecting the function “Various” The function “Various” can be selected from the operating mode “JOG”, “MDA” or “AUTO” in the operating area “Program” as follows: Press the HSK 6 “Various“ to switch over to the function “Various”. Following functions are displayed in the vertical Softkey-bar in the program editor.


Description By pressing the VSK 1.1 “Blank“ an input mask opens where you can change the settings for the blank (see section 5.3 “Blank”). By pressing the VSK 1.4 “HighSpeed settings“ the input mask for adjusting the settings for the optimal speed in relation to the machining method opens (see section 5.4 “HighSpeed settings”). By pressing the VSK 1.6 “Subprogram” the input mask for calling a subprogram opens in the main program (see section 5.8). By pressing the VSK 1.8 “Extend“ the vertical softkey bar 2 opens By pressing the VSK 2.8 “Back“ you switch back to the vertical softkey bar 1.


Page 17

B604

Section 5 Notes:

Various 5.3 Blank The blank is needed for the simulation and the simultaneous recording during machining. Only with a blank, which corresponds to the real workpiece as exactly as possible, a meaningful simulation is possible. For defining the blank, the form (block, pipe, cylinder, N corner, block centred) and the dimensions are needed.

5.3.1 Selecting the function “Blank“ By pressing the VSK 1.1 “Blank” the blank input window opens.

B604

Page 18


Section 5

Various 5.3.2

Notes:

Parameters for the “Blank”

Parameter

Meaning

Blank

The following blank can be selected:  Block centred  Block  Pipe  Cylinder  N-corner

X0

1 corner point X

Y0

1 corner point Y

X1 (abs/ink)

2 corner point related to X0 (absolute or incremental) (only with block)

Y1 (abs/ink)

2 corner point related to Y0 (absolute or incremental) (only with block)

ZA

Initial dimension

ZI (abs/ink)

Final dimension related to ZA (absolute or incremental)

XA

Outside diameter (only with pipe or cylinder)

XI

Inside diameter (absolute or incremental)

N

Number of edges (only with N corner)

SW

Width across flats (only with N corner)

W

Width of blank (only with Block centred)

L

Length of blank (only with Block centred))


Page 19

B604

Section 5 Notes:

Various 5.3.3 Changing the graphical view on the blank The graphic view on the blank is adjustable in the operation area “Program” under the functions “Edit”, Drilling”, “Milling”, “Contour milling”, “Various” and “Straight Circle” by pressing the VSK 1.2 “Graphic view”. Within the function “Various” you can adjust the graphic settings with the Softkey “Graphic view” for the blank. Help pictures and animations are only displayed if the VSK 2 “Graphic view” is deselected and then only in the side view. You can change the graphic view on the blank as follows: 1.

In the operating area “Program” and operation mode “JOG”, “MDA”, or “AUTO” press the HSK 1.6 “Various”.

2.

Press the VSK 1.1 “Blank” to open the input mask for the blank settings. By activating and deactivating the VSK 2 “Graphic view” you can switch the graphical representation of the blank, the help pictures and animations between 2 different views:  3D view/side view

 A wireframe model

B604

Page 20


Section 5

Various

Notes: 5.3.4 Changing the setting for the blank 1.


2.

Press the VSK 1 “Settings”.

3.

Optionally change the graphic view for the blank between 3D-/side view or wireframe model by pressing the VSK 2 “Graphic view”.

4.

Enter the parameter values for the blank (see parameter list in section 5.3.2).

5.

Confirm your inputs by pressing the VSK 8 “Accept” or abort with pressing the VSK 7 “Cancel”. A new program block “Workpiece” is inserted in the program (see the picture below).

5.4 High Speed Settings With the machining of free form surfaces, there are high demands on machining speed as well as accuracy and surface finish. The optimal speed profile in conjunction with the machining method (roughing, pre-finishing, finishing) can be adjusted easily with the function “HighSpeed settings”. It is advisable to program the cycle in the technology part first, before programming the geometry part. Machining methods: With the function “HighSpeed settings” you can select from 3 different technological machining methods:  "roughing"  "pre-finishing"  "finishing"  "deselect" (default setting) These four machining methods are associated directly with accuracy, velocity and surface quality of the contour path (see the triangle in the Help pictures). The operator/programmer can make an appropriate weighting by adjusting the tolerance value. Different tolerance values and technologies can be assigned to the four machining methods.


Page 21

B604

Section 5 Notes:

Various 5.4.1 Selecting the function “HighSpeed settings“ By pressing the VSK 4 “HighSpeed settings“ the “High-speed Settings” screen opens. The screens roughing, pre-finishing and finishing change in intervals between Help picture and animation.

5.4.2 Parameter for „HighSpeed settings“ Parameter

Help picture

Animation

PL

The parameter for the machining plane is optional and has to be activated by a machine datum.

Tolerance

Tolerance values for the machining

Machining:  Roughing

 Pre-finishing

B604

Page 22


Section 5

Various Parameter

Help picture

Animation (continuation)

Notes:

 Finishing

none

 Deselect

5.4.3 Changing the ”High-speed settings“ 1.

In the operating area “Program“ and operation mode “JOG”, “MDA”, or “AUTO” press the HSK 6 “Various”.

2.

Press the VSK 4 “HighSpeed settings“.

3.

Optionally change the graphic view for the blank by pressing the VSK 2 “Graphic view”.

4.

Enter the parameter values for “Tolerance” and “Machining”. Press the VSK 8 “Accept” to accept your inputs or abort by pressing the VSK 7 “Cancel”. A new program block “CYCLE832” with the “High Speed settings” is inserted into the program (see picture below).


Page 23

B604

Section 5 Notes:

Various 5.5 Subprogram If you require the same machining steps in the programming of different workpieces, you can define these machining steps in a separate routine. You can then call this subroutine in any programs. Identical machining steps therefore only have to be programmed once. ShopMill does not differentiate between main program and subprogram. This means that you can call a "standard" sequential control or G code program as subprogram in another sequential control program. In this subprogram, you can also call another subprogram. The maximum nesting depth is 8 subroutines. You cannot insert subroutines among blocks chained by the control. If you want to call a sequential control program as a subroutine, the program must already have been calculated once (load or simulate program in “Machine Auto” mode). This is not necessary for G code subroutines. The subroutine must always be stored in the NCK main memory (in a separate directory "XYZ" or in the "ShopMill", "Part programs", "Subroutines" directories). If you want to call a subprogram located on another drive, you can use the G code command "EXTCALL". Note: Please note that, when a subprogram is called, ShopMill evaluates the settings in the program header of the subroutine. These settings also remain active even after the subprogram has ended. If you wish to activate the settings from the program header for the main program again, you can make the settings again in the main program after calling the subprogram. 5.5.1 Selecting the function “Subprogram” By pressing the VSK 3 “Subprogram”, the input window for calling up a subprogram opens.

B604

Page 24


Section 5

Various

Notes:

5.5.2 Loading subprograms 1.

In the operating area “Program“ and operating mode „JOG“, „MDA“ or „AUTO“ press the HSK 6 “Various“.

2.

Press the VSK 1.6 ”Subprogram”.

3.

Enter the directory path to the subprogram and the name of the subprogram in the input mask.

4.

Press the VSK 8 “Accept” to confirm your inputs or press the VSK 7 “Cancel” to abort. A new program block “Execute” with the directory path to the subprogram is inserted (see picture below):


Page 25

B604

Section 5 Notes:

Simulation ShopMill provides various extensive and detailed simulation functions for displaying the simulation of the machining. During simulation, the current program is calculated in its complete form and the result is displayed in graphic form. You can select the following modes of representation for simulation:  Top view  3-D view  Side view The simulation uses the correct proportions for the tools and workpiece contours. Cylindrical die-sinking cutters, bevel cutters, bevel cutters with corner rounding and tapered die-sinking cutters are displayed as end milling tools. The traverse paths for the tools are shown in colour: Red line = tool is moving at rapid traverse Green line = tool is moving at machining feedrate In all views, a clock is displayed during graphical processing. The displayed machining time (in hours/minutes/seconds) indicates the approximate time that would actually be required to execute the machining program on the machine (incl. tool change). If a program is interrupted during simultaneous recording, the clock stops. In addition, the current axis coordinates, the override, and the program block currently being executed are also displayed. The active tool with the cutting edge number and feedrate are also displayed in the simulation. Transformations are displayed differently during simulation and simultaneous recording:  Coordinate transformations (translation, scaling, …) are displayed as programmed.  Cylinder surface transformations are displayed as a developed surface.  After swivel transformation, the previous machining operations are deleted from the display and only machining of the swivelled plane is displayed (viewing angle perpendicular to the swivelled plane).  Zero offsets (G54, etc.) do not alter the zero in the graphical display. This means that, in the case of multiple clamping, the machining operations for each of the individual workpieces are plotted on top of one another. Note: If you want to display a different portion of the workpiece from the one defined in ShopMill, you can define a new blank in the program (see section 5.3 “Blank” in this module).

B604

Page 26


Section 6

Simulation

Notes:

6.1 Selecting the function “Simulation“ The function “Simulation” can be selected from the operating mode “JOG“, “MDA“ and “AUTO“ as follows: With a program loaded, press the HSK 1.7 “Simulation“ to start a simulation run. The following screen opens. The simulation starts after a short computing time in the top view by default.

Press the VSK 1.4 “3D view” the simulated workpiece is displayed 3-dimesionally (see picture below).

The following functions will be available in the vertical softkey bar. 828D/840Dsl SINUMERIK Operate

Page 27

B604

Section 6 Notes:

Simulation 6.2 Vertical softkey bar 1 and 2 Display area

Description By pressing the VSK 1.1 “Stop“ the simulation will be halted. The softkey will be replaced with the VSK 1.1 “Start”, in order to continue the simulation again. By pressing the VSK 1.1 “Start” the simulation will be started or continued. The softkey will be replaced with the VSK “Stop”. By pressing the VSK 1.1 “SBL“ the simulation will be processed block by block. This softkey replaces the softkey “Start”, if the VSK 4 “Single block” is activated under the function “Program control”. By pressing the VSK 1.2 “Reset“ the simulation will be aborted, and can be started again by pressing the VSK 1.1 “Start”. The “Top view“ is activated by default and shows the simulation in a plan view from above By pressing the VSK 1.4 “3D view“ the simulation will be shown in a 3-D view By pressing the VSK 1.5 “Further views” the vertical softkey bar opens, with more options to adjust the view on the simulation process (see section 6.3). By pressing the VSK 1.6 “Details“ the vertical softkey bar opens, where you can adjust the level of details that will be shown during the simulation (see section 6.4). By pressing the VSK 1.7 “Program control” the vertical softkey bar opens, with further functions to control the simulation run (see section 6.5). By pressing the VSK 1.8 “Extend” the vertical softkey bar 2 with the following functions will be displayed. By pressing the VSK 2.3 “Show tool path” the display of the simulated tool path can be switched on and off. By pressing the VSK 2.4 “Delete tool path” the animated tool path in the simulation window will be deleted. A new tool path is shown immediately after pressing this softkey or after running a new simulation (if the simulation is in “Stop”- or “Reset”- mode). By pressing the VSK 2.5 “Blank” you can change the dimensions of the simulated blank (see also section 5.3). This softkey is active if the simulation is in “Reset” mode. By pressing the VSK 2.8 “Back” you switch back to the vertical softkey bar 1.

B604

Page 28


Section 6

Simulation

Notes:

6.3 Further views With the function “Further views” you can change the graphical side-views on the blank, to view the simulation process in an optimal way. You can change the sides from which you want to see the simulation. 6.3.1 Selecting the function “Further views” By pressing the VSK 1.5 “Further views” the following window with side views on the blank opens.


Description By pressing the VSK 1 “From front” the simulated workpiece will be shown in a front view. By pressing the VSK 2 “From rear” the simulated workpiece will be shown in a rear view. By pressing the VSK 3 “From left” the simulated workpiece will be shown from the left side. By pressing the VSK 4 “From right” the simulated workpiece will be shown from the right side. By pressing the VSK 8 “Back” on the operator panel (OP) you switch back to the vertical softkey bar of the operating area “Details”.


Page 29

B604

Section 6 Notes:

Simulation 6.4 Details With the function “Details” you can zoom in, zoom out, rotate and cut out parts of the workpiece. 6.4.1 Selecting the function “Details” By pressing the VSK 1.6 “Details“ the following functions are available in a vertical softkey bar.


Description By pressing the VSK 1 “Autozoom“ the workpiece fills out the simulation window in an optimal way. By pressing the VSK 2 “Zoom +“ you zoom in into the simulation window. Alternatively you can press the “+“-key on the number block of the keyboard. By pressing the VSK 3 “Zoom -“ you can zoom out of the simulation window. Alternatively you can press the “-“-key on the keyboard. By pressing the VSK 4 “Zoom” a frame opens in the simulation window, that lets you zoom in to the frame size. Press the VSK1 “Zoom +” to increase and the VSK 2 “Zoom -” to decrease the frame size. Alternatively you can change the frame size of the zoom area with the “+”or “-” key on the number pad of the keyboard. Move the frame with the blue cursor keys on the keyboard. Press the VSK 8 “Accept” to zoom to the selected extent or abort with pressing the VSK 7 “Cancel”.

B604

Page 30


Section 6

Simulation Display area


Notes:

By pressing the VSK 5 “Rotate view” a vertical softkey bar opens to the right, with functions to rotate the workpiece in the simulation window (see section 6.4.2.1). By pressing the VSK 6 “Cut” the functions for cutting out parts of the workpiece are available in a vertical softkey bar “(see section 6.4.2.3). By pressing the VSK 8 “Back” on the operator panel you switch back to the vertical softkey-bar 1.

6.4.2.1 Selecting the function “Rotate view” By pressing the VSK 5 “Rotate view” the following functions will be displayed in a vertical softkey bar.

6.4.2.2 Vertical softkey bar Display area

Description By pressing the VSK “Arrow right” the workpiece will be turned right around the centre of the simulation window. By pressing the VSK “Arrow left” the workpiece will be turned left around the centre of the simulation window. By pressing the VSK 3 “Arrow up” the work piece will be turned up around the centre of the simulation window. By pressing the VSK 4 “Arrow down” the work piece will be turned down around the centre of the simulation window. By pressing the 5 “Arrow turns left” the workpiece will be rotated to the left, around the centre of the simulation window (counter clockwise). By pressing the 5 “Arrow turns right” the workpiece will be rotated to the right, around the centre of the simulation window (clockwise). By pressing the VSK 8 “Back” you switch back to the VSK-bar “Details”.


Page 31

B604

Section 6 Notes:

Simulation 6.4.2.3

Selecting the function “Cut” By pressing the VSK 1.7 “Cut“ the functions for cutting out parts of the simulated workpiece will be shown in a vertical softkey bar. The cut surface areas are only displayed during simulation run.


Description By pressing the VSK 1 “Cut active” you can activate the cut surfaces on the workpiece and activate the greyed out axes softkeys in the vertical softkey bar. The function “Cut” stays active until the VSK “Cut active” is deactivated. By pressing the VSK 2 “X+“ the cutting plane is shifted on the X-axis to the positive (“to the right”). By pressing the VSK 3 “X-“ the cutting plane is shifted on the X-axis to the negative (“to the left”). By pressing the VSK 4 „Y+“ the cutting plane is shifted on the y-axis (ordinate) to the positive („to the rear “). By pressing the VSK 5 „Y-“ the cutting plane is shifted on the y-axis (ordinate) to the negative (“forward”). By pressing the VSK 6 “Z+“ the cutting plane will be shifted on the Z-axis (applicate) to the positive (“up”).

B604

Page 32


Section 6

Simulation Anzeigebereich

Beschreibung (Fortsetzung)

Notes:

Durch Drücken des VSK 7 „Z-“ wird die Schnittebene auf der Z-Achse (Ablikate) zum negativen („nach unten“) verschoben. Durch Drücken des VSK 8 „Zurück“ gelangt man wieder in den Bedienbereich „Details“ zurück.

6.5 Programmsteuerung Mit der Funktion „Programmsteuerung“ kann der Override für die Simulation eingestellt werden, das Programm kann Block für Block abgearbeitet werden, und Alarm Meldungen die während der Simulation auftreten, können angezeigt werden. 6.5.1

Anwahl der Funktion „Programmsteuerung“ Durch Drücken des VSK 1.7 „Programmsteuerung“ werden die folgenden Funktionen in der vertikalen Softkey-Leiste zur Verfügung gestellt..

6.5.2

Vertikale Softkey-Leiste

Anzeigebereich

Beschreibung Durch Drücken des VSK 1 „Override 100%“ wird der Vorschub-Override auf die maximale Vorschubgeschwindigkeit von 100% gesetzt. Durch Drücken des VSK 2 „Override +“ wird der Vorschub um jeweils 5%-Schritte bis zur maximalen Vorschubgeschwindigkeit von 100% erhöht. Durch Drücken des VSK 3 „Override -“ wird der Vorschub-Override um jeweils 5%-Schritte reduziert. Bei einem Vorschub-Override von 0% wird die Simulation pausiert. Durch Drücken des VSK 4 „Einzelsatz“ wird die Abarbeitung des Programms Satz für Satz simuliert. Mit jedem Drücken des VSK 1 „SBL“ im Bedienbereich Simulation wird jeder Programm-Block nacheinander abgearbeitet (siehe Abschnitt 6.2, „Vertikale Softkey-Leiste 1 und 2). Durch Drücken des VSK 7 „Alarm“ wird das Fenster mit den Alarmmeldungen geöffnet, die während des Simulationslaufs auftreten, um bspw. eine Fehlerdiagnose durchzuführen. Durch Drücken des VSK 8 „Zurück“ gelangt man wieder in zur Vertikalen Softkey-Leiste 1 zurück.


Page 33

B604

Section 6 Notes:

Simulation 6.6.1

Selecting the function “Alarm” By pressing the VSK 7 “Alarm” the “Simulation alarms” window opens, with a list of all current active alarm messages that occurred during the simulation. For error messages and acknowledgement symbols see module - B576 “Operating area Diagnostics”, section 3.


Description By pressing the VSK 1 “Acknowl. Alarm” all with the “Reset”- or “Cancel”-symbol marked alarm messages can be deleted. This softkey is inactive as long as no appropriate error message is shown. By pressing the VSK 2 “Simulation Power On” you can trigger a warm restart for the active simulation.

Press the VSK 8 “OK” to confirm or the VSK 7 “Cancel” to abort the warm restart. With a warm start the simulation will be ended and started new. By pressing the VSK 8 “Back” you switch back to the operating area “Program control”.

B604

Page 34


Section 7

NC Execute

Notes:

7.1 NC Execute The function “NC Execute” lets you load the active program from the editor to the operating area “Machine” in the operating mode “AUTO”. 7.1.1

Selecting the function “NC Execute” By pressing the HSK 1.8 “NC Execute” the control, switches to the operating area “Machine” under the operating mode “AUTO”. The program is loaded into the internal memory of the NC and is now ready for machining (see picture below). The Softkey “NC Execute” is inactive on a running program.


Page 35

B604

B604

Page 36


B609

1

Drilling

Brief description

Objective of the module: Working through this module you become familiar with the technology “Drilling” by programming two G code programs with the programGUIDE in ShopMill. Description of the module: This module explains the programming of a simple drilling example with the programGUIDE in ShopMill, as well as well as the programming of a more complex workpiece by means of drilling cycles and position patterns. Content: Simple programming example Complex programming example


Page 1


B609

B609

B609

Page 2


B609 Drilling - programGUIDE: Description This module explains the programming of a simple drilling example with the programGUIDE in ShopMill, as well as well as the programming of a more complex workpiece by means of drilling cycles and position patterns.

Drilling programGUIDE: START

Simple programming example

Complex programming example

Drilling programGUIDE: END

Notes :


Page 3

B609

Section 2 Notes:

Simple programming example Description: A simple drilling using the drill cycle is to be programmed with the programGUIDE in ShopMill.

Objective: A new G code program is to be created and opened. The G code lines and the drill cycle must be programmed and the program is to be simulated. For this, the tool and technology data below are to be used: Tool data:

Drill Ø 8,5 mm (DRILL_D8.5)

Technology data:

As a start position for the machining, the first programmed drill hole is to be used. This position is approached in rapid traverse.

2.1 Creating a new programGUIDE program A new G code program can be created from within the operating modes “JOG, “MDA” and “AUTO” as follows: 1.

Press the “Program Manager”-key on the keyboard. The program manager will be opened directly. - OR -

1.

Press the “MENU SELECT”-key on the operator panel. Press the yellow HSK 1.4 “Program Manager”. The program manager opens.

B609

2.

Select a drive by pressing a horizontal softkey where you want to create the program (“NC”, “Local drive”, “USB”).

3.

Press the VSK 2 “New“. The vertical softkey bar with functions for creating new programs opens.

4.

Press the VSK 4 „programGUIDE G code“ to open the input mask for creating a new G code program. Select “Main program MPF”.

5.

Enter a name for the program in the “Name” field, e.g DIN_DRILLING_1.MPF and accept with pressing the VSK 8 “OK”. The editor window for entering G code commands opens. Page 4


Section 2


Notes:

2.2 Example: Drilling The following G code program, with the call up of a simple drilling cycle, is to be programmed.

Create a new G code programGUIDE program, as described before in section 2.1 and give the program the name “DIN_DRILLING_1”. 1.

Program the first line of the program: N10 G54 G17 G90

2.

Insert now a blank for the simulation. Press the HSK 1.6 “Various” to open the operating area “Various”. Press the VSK 1 “Blank” to open the input mask for the blank.

3.

Fill in the following parameters for the blank:

Confirm your inputs by pressing the VSK 8 “Accept”. The following line will be inserted into the program: N20 WORKPIECE(,,,"RECTANGLE",64,0,-20,80,100,100) 4.

Now, insert a drill tool into the program. Press the VSK 1.1 “Select tool“. The tool list window opens. Select the tool “DRILL_D8.5” by using the blue cursor key on the keyboard.


Page 5

B609

Section 2


Notes:

Press the VSK 1.8 “OK”. The following program line is inserted into the program: N30 T="DRILL_D8.5" 5.

Program the following G code commands: N40 M6 N50 S1000 M3 F150 N60 G0 X0 Y0 Z100

6.

Program the drilling-cycle “CYCLE82”. For this, press the HSK 1.2 “Drill.” to open the technology “Drilling”. Press the VSK 2 “Drilling Reaming”. Press the VSK 3 “Drilling“. The input mask for the drilling cycle “CYCLE82” opens.

7.

Insert the values into the parameter mask like displayed below:

The following program line will be inserted into the program: N70 CYCLE82(100,0,1,,25,0,10,1,11) 9.

Program the program end: N80 M30

10.

Simulate the machining. Press the HSK 1.7 “Simulation” to run the simulation of the program.

B609

Page 6


Section 2

Simple programming example Press the VSK 1.4 “3D view” to view the simulation in a 3D view.


Page 7

Notes:

B609

Section 3 Notes:

Complex programming example Description: By using different drilling cycles (Centering, Drilling, Thread drilling) and a position pattern, a more complex programGUIDE-program (drill pattern) is to be created in ShopMill.

Aim: The workpiece shown below is to be programmed. Afterwards, the program is to be simulated.

The following tools and technology data are to be used.

B609

Tool data:

Center drill 12 mm (CENTERDRILL_D12) Drill Ø 8,5 mm (DRILL_D8.5) Tap M10 (TAP_M10)

Technology data:


Page 8


Section 3


Notes:

3.1 Example: Drill pattern The following program, with the call up of a drilling-, center drilling- and thread drilling-cycle, is to be programmed:

Create a new programGUIDE-program in ShopMill, like described in section 2.1 in this module. Give the program a name, for example “DIN_DRILLING_2”. 1.


2.

Now insert a blank for the simulation. For this, press the HSK 1.6 “Various” to open the operating area “Various”. Press the VSK 1 “Blank” to open the parameter mask for the blank.

3.


Confirm your inputs by pressing the VSK 8 “Accept”. The following line will be inserted into the program: N20 WORKPIECE(,,,"BOX",112,0,-20,80,0,0,150,100) 4.

Insert a tool into the program. Press the VSK 1.1 “Select tool”. The tool list window opens. Use the blue cursor keys to select the tool: “CENTERDRILL_D12”.


Page 9

B609

Section 3


Notes: Press the VSK 1.8 “OK”. The program line N30 T="CENTERDRILL_D12" is inserted into the program. 5.

Program the following G code commands: N40 M6 N50 S2000 M3 F100

6.

Program the center drill cycle “CYCLE 81”. Press the HSK 1.2 “Drill.”, to open the technology “Drilling”. Press the VSK 1 “Centering”. The input mask for the centering cycle “CYCLE81” opens. Insert the values into the parameter mask like displayed below:

Accept your inputs by pressing the VSK 8 “Accept”. The following line will be inserted into the program: N60 MCALL CYCLE81(100,0,1,10,,0,10,1,11). 7.

Insert now the position patterns (CYCLE802) for centering. Press the VSK 7 “Positions” for selecting a position pattern. Press the VSK 3 “Positions” to program the “CYCLE802”. Insert DRILLING_1 into the “LAB” field to set a name for the jump marks for the repeat positions. Fill out the rest of the input mask like displayed below.

B609

Page 10


Section 3

Complex programming example Confirm your inputs by pressing the VSK 8 “Accept”.

Notes:

The following line will be inserted into the program: N70 DRILLING_1: CYCLE802(111111111, 111111111,30,25,120,25,120,75,30,75,,,,,,,,,,,0,0,1) 8.

Program the following G code command: N80 MCALL

9.

Insert the tool “DRILL_D8.5” into the program (see step 4) or type into the editor the following line by hand: N90 T="DRILL_D8.5"

10.


11.

Program the cycle for drilling (CYCLE82). Press the VSK 2 “Drilling Reaming”. Press the VSK 3 “Drilling”. The input mask for the drilling cycle “CYCLE82” opens.

12.


Accept your inputs by pressing the VSK 8 “Accept”. The following line will be inserted into the program: N120 MCALL CYCLE82(100,0,1,,25,0,10,1,11). 13.

Program the following G code commands: N130 REPEATB DRILLING_1 N140 MCALL

14.

Insert the tool TAP_M10 into the program (see step 4) or type into the editor the following line by hand: N150 T="TAP_M10"

15.



Page 11

B609

Section 3


Notes: 16.

Finally program the cycle for the thread drilling. Press the VSK 6 “Thread” to open the input mask for the CYCLE84 “Tapping”.

17.


Accept your inputs by pressing the VSK 8 “Accept”. The following line will be inserted into the program: N180 MCALL CYCLE84(100,0,1,25,,0,5,,1.5,0,500,500,0,1,0,0,,1.4,,"ISO_METRIC"," M10",,1001,1001002) 18.

Program the following lines and complete the program: N190 REPEATB DRILLING_1 N200 MCALL N210 M30

19.

Start the simulation of the program. Press the HSK 1.7 “Simulation” to open the simulation window. The control calculates the simulation and shows the simulation in a top view.

B609

Page 12


Section 3


Notes:

Press the VSK 1.4 “3D view“ to run the simulation in a 3-dimensional view.


Page 13

B609

B609


B616

1

Milling

Brief description

Objective of the module: Working through this module you learn about the technology “Milling” by programming two G code programs with the programGUIDE in ShopMill. Description of the module: This module explains the explains the programming of a simple milling example with the programGUIDE in ShopMill, as well as the programming of a more complex workpiece by means of milling cycles and a position pattern. Content: Simple programming example Complex programming example


Page 1


B616

B616

B616

Page 2


B616 Milling - programGUIDE: Description

Milling programGUIDE: START

This module explains the explains the programming of a simple milling example with the programGUIDE in ShopMill, as well as the programming of a more complex workpiece by means of milling cycles and a position pattern.



Milling programGUIDE: END

Notes :


Page 3

B616

Section 2 Notes:

Simple programming example Description: A simple milling operation is to be programmed with the programGUIDE in ShopMill.

Objective: A new G code program is to be created and opened in the editor window. The G code lines and the milling cycle are to be programmed and the program is to be simulated For this the tool and technology data shown below are to be used: Tool data:

Milling cutter Ø 10 mm (CUTTER_D10)

Technology data:

F 0,15 mm/tooth, V120 m/min

2.1 Creating a new programGUIDE program A new programGUIDE program can be created from within the operating modes “JOG, “MDA” and “AUTO” as follows: 1.


1.

Press the “MENU SELECT”-key on the operator panel. Press the yellow HSK 4 “Program Manager”. The program manager opens.

2.

Select a drive, where you want to create the program (“NC”, “Local drive”, “USB”).

3.

Press the VSK 2 “New“. The vertical softkey bar for creating new programs opens.

4.

Press the VSK 4 “programGUIDE G code” to open the input mask for creating a new ShopMill G code program. Select “Main program”. Enter a name for the program in the “Name” field, e.g “DIN_MILLING_1.MPF” and accept with pressing the VSK 8 “OK”. The G code program is loaded to the editor.

B616

Page 4


Section 2


Notes:

2.2 Example: Rectangular pocket The following program, with a simple call up of a milling cycle, is to be programmed with the programGUIDE in ShopMill:

1.


2.

Insert now a blank for the simulation. Press the HSK 1.6 “Various” to open the operating area “Various”. Press the VSK 1 “Blank” to open the parameter mask for the “Blank input”.

3.

Insert the following values into the parameter mask:

Confirm your inputs with pressing the VSK 8 “Accept”: The following line is inserted into the program_ N20 WORKPIECE(,,,"BOX",112,0,-20,80,0,0,150,100) 4.

Insert now a tool into the program. Press the VSK 1.1 “Select tool”. The tool list window opens. Place the orange selection cursor on the tool “CUTTER_D10” by using the blue cursor keys on the keyboard.


Page 5

B616

Section 2


Notes:

Press the VSK 1.8 „OK“. The program line N30 T="CUTTER_D10" is inserted into the program. Alternatively you can also program the line by hand. 5.

Insert the following G code commands into the program: N40 M6 N50 S3820 M3 N60 G95 FZ=0.15

6.

Program now the rectangular pocket. For this, press the HSK 1.2 “Mill.”, to call up the technology “Milling”. Press the VSK 2 “Pocket”. Press the VSK 3 “Rectang. pocket”. The input mask for the rectangular pocket opens.

7.


Confirm your inputs with pressing the VSK 8 “Accept”: The following line will be inserted into the program: N70 POCKET3(100,0,1,-10,60,30,7,75,50,0,10, 0,0,0.15,0.1,0,21,40,8,3,15,2,2,0,1,2,11100,1,111) 9.

Program now the program end with the following G-code command: N80 M30

B616

Page 6


Section 2

Simple programming example 10.

Simulate the machining of the workpiece.

Notes:

Press the HSK 1.7 “Simulation” to start the simulation run. The control calculates the simulation parameters and opens the simulation in the simulation window in “Top view”.

To view the simulation in 3-dimensional press the VSK 1.4 “3D view”.


Page 7

B616

Section 3 Notes:

Complex programming example Description: A more complex program (slanted rectangular pocket) is to be created with the programGUIDE in ShopMill, using milling cycles and a position pattern.

Objective: The workpiece shown below is to be programmed and simulated afterwards. For this the tool and technology data shown below are to be used:

The following tool- and technology data are needed for the programming:

B616

Tool data::

Milling cutter Ø 10 mm (CUTTER_D10) F 0,15 mm/tooth, V 120 m/min (roughing) and F 0,08 mm/tooth, V 150 m/min (finishing)

Technology data:

The pocket is to be roughed first and later on to be finished.

Page 8


Section 3


Notes:

3.1 Example: Slanted rectangular pocket The following program is to be programmed using the milling cycle “Rectang. Pocket”.

For this, create a new programGUIDE G code program, like described in section 2.1 in this module. Give the program for example following name “DIN_MILLING_2”. 1.

Program in the first line following G code command: N10 G54 G17 G90

2.

Insert now a blank for the simulation into the program. Press the HSK 1.6 “Various” to open the operating area “Various”. Press the VSK 1 “Blank” to open the parameter window for the blank input.

3.

Insert the following parameters into the parameter window:

Confirm your inputs by pressing the VSK 8 “Accept”. The following line is inserted into the program: N20 WORKPIECE(,,,"BOX",112,0,-20,80,0,0,150,100) 4.

Insert now a tool into the program.


Page 9

B616

Section 3


Notes:

Press the VSK 1.1 “Select tool”. The tool list in the operating area “Parameter” opens. Use the blue cursor keys on the keyboard to select the tool “CUTTER_D10”. Press the VSK 1.8 “OK”. The program line N30 T="CUTTER_D10" is inserted into the program. Optionally you can program this line by typing it into the editor. 5.

Program the following G code commands: N40 M6 N50 S3820 M3 N60 G95 FZ=0.15

6.

Rough the rectangular pocket. Press the HSK 1.3 “Mill.”, to open the technology “Milling”.. Press the VSK 2 “Pocket”. Press the VSK 3 “Rectang. pocket”. The parameter mask for the rectangular pocket cycle opens.

7.

Here, enter the values displayed below and press the VSK 8 “Accept”.

The following line is inserted into the program: N70 POCKET3(100,0,1,-15,60,40,6,75,50,30,2.5, 0.3,0.3,0.15,0.1,0,21,80,8,3,15,2,2,0,1,2,11100,1,110)

B616

Page 10


Section 3

Complex programming example 8.

Insert now the following G code command:

Notes:

N80 S4775 9.

Finish the rectangular pocket. Press the VSK 2 “Pocket”. Press the VSK 3 “Rectang. pocket”. The parameter mask for the rectangular pocket cycle opens.

10.

Insert the following values into the parameter mask and press the VSK 8 “Accept”.

The following line is inserted into the program: N90 POCKET3(100,0,1,-15,60,40,6,75,50,30,15,0.3, 0.3,0.08,0.1,0,22,80,8,3,15,2,2,0,1,2,11100,1,110) 11.

Program the following G code command and end the program: N100 M30

12.

Start the Simulation of the program. Press the HSK 1.7 “Simulation” to start the simulation run. The control calculates the simulation parameters and opens the simulation in the simulation window in “Top view”.


Page 11

B616

Section 3


Notes:

To view the simulation 3-dimensional press the VSK 1.4 “3D view”.

B616

Page 12


B624

1

Contour milling

Brief description

Objective of the module: Working with this module you learn about the technology “Contour milling”, by programming two G code programs with the programGUIDE in ShopMill. Description of the module: This module explains the programming of a simple contour milling example (straight line) with the programGUIDE in ShopMill, as well as well as the programming of a more complex workpiece (mould plate) by means of contour milling cycles and contour descriptions. Content: Simple programming example Complex programming example


Page 1


B624

B624

B624

Page 2


B624 Contour milling - programGUIDE: Description This module explains the programming of a simple contour milling example (straight line) with the programGUIDE in ShopMill, as well as well as the programming of a more complex workpiece (mould plate) by means of contour milling cycles and contour descriptions.

Contour milling programGUIDE: START



Contour milling programGUIDE: END

Notes :


Page 3

B624

Section 2 Notes:

Simple programming example Description: A simple straight line is to be programmed using the technology “Contour milling” with the programGUIDE in ShopMill. Objective: A new G code program is to be created and opened. The G code lines and the contour milling cycles must be programmed and the program is to be simulated For this the tool and technology data below are to be used: Tool data:


Technology data:

F 0,15 mm/tooth, V 120 m/min As a start position for the machining, the following position is to be used: X0, Y-100 This position is approached in the cycle in rapid traverse.

2.1 Creating a new programGUIDE program A new G code program can be created from within the operating modes “JOG, “MDA” and “AUTO” as follows: 1.


1.

Press the “MENU SELECT”-key on the operator panel. Press the yellow HSK 1.4 “Program Manager”. The program manager opens.

2.

Select a drive by pressing a horizontal softkey where you want to create the program (“NC”, “Local drive”, “USB”).

3.

Press the VSK 2 “New“. The vertical softkey bar with functions for creating new programs opens.

4.

Press the VSK 4 „programGUIDE G code“ to open the input mask for creating a new G code program. Select “Main program MPF”. Enter a name for the program in the “Name” field, e.g. DIN_CONTOURMILLING_1.MPF and accept with pressing the VSK 8 “OK”. The editor window for entering G code commands opens.

B624

Page 4


Section 2


Notes:

2.2 Programming example: Straight line The following G code program “DIN_CONTOURMILLING_1.MPF” is to be programmed:

1.


2.

Insert now a blank for simulation. Press the HSK 1.6 “Various” to open the operating area “Various”. Press the VSK 1 “Blank” to open the input mask for the blank.

3.

Fill in the following parameters for the blank:

Confirm your inputs by pressing the VSK 8 “Accept”. The following line will be inserted into the program: N20 WORKPIECE(,,,"BOX",64,0,-25,-80,-50,100,100,150) 4.

Now, insert a tool into the program. First Press HSK 1 “Edit”. A vertical softkey-bar with additional functions shows on the right of the screen. Press the VSK 1.1 “Select tool“. The tool list window opens. Select the tool “CUTTER_D32” by using the blue cursor key on the keyboard.


Page 5

B624

Section 2


Notes:

Press the VSK 1.8 “OK”. The program line N30 T="CUTTER_D32" is inserted into the program. Alternatively you can type this line by hand into the editor. 5.

Insert the following G code commands into the program: N40 M6 N50 S1194 M3 N60 G95 FZ=0.15

6.

Insert a contour call (CYCLE62) into the program. For this, press the HSK 1.4 “Cont. mill.” to open the technology “Contour milling”. Press the VSK 2 “Contour”. Press the VSK2 “Contour call” to open the input mask for the contour call.

7.

Give the contour a name:

Confirm your inputs by pressing the VSK 8 “Accept”. The following line is inserted into the program: N70 CYCLE62("STRAIGHTLINE",1,,) Press VSK 2.8 to return to the VSK-bar 1. 8.

Insert the cycle “Path milling” (CYCLE72) into the program. Press the VSK 2 “Path milling“ to open the parameter mask for the “Path milling” cycle.

9.

B624

Enter following values into the input mask. Use the “Select” key on the MCP where indicated.

Page 6


Section 2

Simple programming example Confirm your inputs by pressing the VSK 8 “Accept”.

Notes:

The following line will be inserted into the program. N80 CYCLE72("",100,0,1,-15,5,0,0,0.15,0.1, 1,41,1,5,0.1,1,5,0,1,2,101,1001,100) 10

Program the following line: N90 M30

11.

At the end, program the contour for the straight line that you have called up in step 7. Press the VSK 1 “Contour”. The vertical softkey bar with functions for calling up, or creating a new contour description opens. Press the VSK1 “New contour” to insert a new contour description for the contour milling machining into the program.

12.

The input window for a new contour opens. Fill in the following name into the name field:

Confirm your input by pressing the VSK 8 “Accept”. 13.

The contour editor for the input of the start point of the contour description opens.


Page 7

B624

Section 2 Notes:


Insert the following coordinates for the starting point:

Confirm by pressing the VSK 8 “Accept”. 15.

Program the contour with a straight line in Ydirection. Press the VSK 1.3 “Straight line Y“. The input mask for the “Straight line Y” opens.

16.

Enter the coordinates as follows:

Confirm your inputs by pressing the VSK 8 “Accept”. The contour description is now finished. 17.

Now, check the outline of the programmed contour. In order to do this, use the blue cursor keys on the keyboard, to place the orange selection cursor on the symbol, on the left side of the screen. The contour graphic is being displayed.

B624

Page 8


Section 2


Complete the contour description by pressing the VSK 8 “Accept”.

Notes:

The editor window opens and the following program lines are entered into the program: N100 E_LAB_A_STRAIGHTLINE: ;#SM Z:2 ;#7__DlgK contour definition begin - Don't change!;*GP*;*RO*;*HD* G17 G90 DIAMOF;*GP* G0 X0 Y-100 ;*GP* G1 Y150 ;*GP* ;CON,0,0.0000,2,2,MST:0,0,AX:X,Y,I,J;*GP*;*RO*;* HD* ;S,EX:0,EY:-100;*GP*;*RO*;*HD* ;LU,EY:150;*GP*;*RO*;*HD* ;#End contour definition end - Don't change!;*GP*;*RO*;*HD* E_LAB_E_STRAIGHTLINE: Notes: The lines marked as italic are shown optionally (see Settings - Show hidden lines). 19.

Now simulate the machining of the workpiece. Press the HSK 1.7 “Simulation” to start the simulation of the program. The control calculates the simulation and opens the animation of the machining in “top view” by default.


Page 9

B624

Section 2 Notes:

B624

Simple programming example Press the VSK 1.4 “3D view” to view the simulation in a 3-dimensional.

Page 10


Section 3


Notes:

Description: A more complex program (moulding plate) is to be created with the programGUIDE in ShopMill. Objective: The workpiece shown below is to be programmed and simulated.

20

5

A-A

100

20

R30

35

50

40

150

A

90

R36

A R5

60 70

Tool & technology data:

Operations list:

Milling cutter Ø 32 mm (CUTTER_D32) F 0,15 mm/tooth, V 120 m/min (roughing) F 0,08 mm/tooth, V 150 m/min (finishing) Milling cutter Ø 16 mm (CUTTER_D16) F 0,15 mm/tooth, V 120 m/min (roughing) Milling cutter Ø 8.0 mm (CUTTER_D8) F 0,10 mm/tooth, V 120 m/min (roughing) F 0,05 mm/tooth, V 150m/min (finishing) 1. 2. 3. 4. 5.


Outer contour roughing + finishing Spigot contour roughing + finishing Contour pocket roughing Contour pocket rest material roughing Contour pocket wall + base finishing

Page 11

B624

Section 3 Notes:

Complex programming example 3.1 Programming example: Moulding plate The following program is to be programmed with the technology “Contour milling”.

Create a new programGUIDE program in ShopMill, like described in section 2.1 in this module, with the name “DIN_CONTOURMILLING_2.MPF”. 1.

Program the first line of the program with the following G code commands: N10 G54 G17 G90

2.

Insert a blank for the simulation. Press the HSK 1.6 “Various“ to open the operating area “Various”. Press the VSK 1 “Blank” to open the parameter window for the blank.

3.

Insert the following parameters for the blank:

Press the VSK 8 “Accept” to confirm your inputs. The following line is inserted into the program: N20 WORKPIECE(,,,"BOX",64,0,-25,-80,-50,100,100,150)

B624

Page 12


Section 3


Insert now a tool call into the program.

Notes:

First Press HSK 1 “Edit”. A vertical softkey-bar with additional functions shows. Press the VSK 1.1 “Select tool”. The “Tool list” window opens. Use the blue cursor keys on the keyboard to select the tool “CUTTER_D32”. Press the VSK 1.8 “OK”. The line N30 T="CUTTER_D32" will be inserted into the program. Alternatively you can also program this line by hand. 5.

Program now the following G code commands: N40 M6 N50 S1194 M3 N60 G95 FZ=0.15 ; Feedrate per tooth

6.

Insert a contour call into the program (CYCLE62), for the “moulding plate outside”. To do this, press the HSK 1.4 “Cont. Mill” to open the technology “Contour milling”. Press the VSK 1 “Contour”. Press the VSK 2 “Contour call” to open the input mask for calling up a contour in the program. The input mask for naming the contour opens.

7.

Fill out the name field like displayed below:

Confirm the contour name by pressing the VSK 8 “Accept”. The following line will be inserted into the program: N70 CYCLE62("MOULDINGPLATE_OUTSIDE",1,,) Press VSK 2.8 to return to the VSK-bar 1. 8.

Insert now the first “path milling cycle” (CYCLE72) into the program, for “roughing” the outside contour. Press the VSK 2 “Path milling” to open the input mask for the CYCLE72 “Path milling”.


Page 13

B624

Section 3


Notes:


Confirm your inputs by pressing the VSK 8 “Accept”. The following line will be inserted into the program: N80 CYCLE72("",100,0,1,-15,5,0.3,0.3,0.15, 0.1,1,41,1,5,0.1,1,5,0,1,2,101,1001,100) 10.

Program now the following G code command: N90 S1942

11.

Insert now the second path milling cycle (CYCLE72) into the program, for “finishing” the outside contour. Press the VSK 2 “Path milling” to open the parameter mask for the path milling cycle (CYCLE72). Enter following values into the input mask. Use the “Select” key on the MCP where indicated.

B624

Page 14


Section 3


Notes:

The following line will be inserted into the program. N100 CYCLE72("",100,0,1,-15,5,0.3,0.3, 0.08,0.1,2,41,1,5,0.1,1,5,0,1,2,101,1001,100) 12.

Insert another contour call into the program (CYCLE62), for the “spigot boundary”. Press now the VSK 1 “Contour”. Press the VSK 2 ”New contour” to insert a new contour description into the program. The input mask for naming the contour opens.

14.

Give the contour a name as shown below:

Confirm the contour name by pressing the VSK 8 “Accept”. The following line will be inserted into the program: N110 CYCLE62 ("MOULDINGPLATE_BOUNDARY",1,,) Press VSK 2.8 to return to the VSK-bar 1. 15.

Insert another contour call (CYCLE62) into the program for the “moulding plate spigot”. Press the VSK 1 “Contour”. Press the VSK 2 “Contour call” to open the input mask for calling up a contour in the program. The input mask for naming the contour opens.

16.

Give the contour a name as shown below:

Confirm the contour name by pressing the VSK 8 “Accept”. The following line will be inserted into the program: N120 CYCLE62("MOULDINGPLATE_SPIGOT",1,,) Press VSK 2.8 to return to the VSK-bar 1.


Page 15

B624

Section 3 Notes:


Insert now the first spigot milling cycle (CYCLE63), into the program, for “roughing”. Press the VSK 6 “Spigot” to open the input mask for the CYCLE63 “Mill Spigot”.

18.

Enter following values into the input mask. Use the “Select”-key on the MCP where indicated.

Note: With the blue “Select”-key the machining depth “Z1” can be set to “inc” or “abs” and the tool path step over “DXY” can be set to “%” of tool Ø or as value in “mm”. Confirm your inputs by pressing the VSK 8 “Accept”. The following line will be inserted into the program: N130 CYCLE63 ("SPIGOT",1001,100,0,1,5,0.15,,50,2.5,0.3,0,0,0,0,,, ,1,2,,,,0,201,111) 19.

Insert now another spigot milling cycle (CYCLE63) into the program for “wall finishing” Press the VSK 6 “Spigot” to open the input mask for the CYCLE63 “Mill Spigot”. Enter following values into the input mask. Use the “Select”-key on the MCP where indicated.

B624

Page 16


Section 3


Notes:

The following line will be inserted into the program: N140 CYCLE63 ("SPIGOT_FINISH_WALL",1004,100,0,1,5,0.08,,50 ,2.5,0.3,0,0,0,0,,,,1,2,,,,0,201,111) 20.

Insert now a tool call into the program. First Press HSK 1 “Edit”. A Vertical softkey-bar with additional functions opens. Press the VSK 1.1 “Select tool”. The “Tool list” window opens. Use the blue cursor keys on the keyboard to select the tool “CUTTER_D16”. Press the VSK 1.8 “OK”. The line N150 T="CUTTER_D16" will be inserted into the program. Alternatively you can also program this line by hand.

21.

Program now the following G code commands: N160 M6 N170 S2388 M3 N180 G95 FZ=0.15; Feedrate per tooth

22.

Insert another contour call (CYCLE62) into the program for the “Moulding plate pocket”. To do this, press the HSK 1.4 “Cont. Mill” to open the technology “Contour milling”. Press the VSK 1 “Contour”. Press the VSK 2 “Contour call” to open the input mask for calling up a contour in the program. The input mask for naming the contour opens.

23.

Fill out the name field like displayed below:

Confirm the contour name by pressing the VSK 8 “Accept”. The following line will be inserted into the program: N190 CYCLE62 ("MOULDINGPLATE_POCKET",1,,) Press VSK 2.8 to return to the VSK-bar 1.


Page 17

B624

Section 3 Notes:


Insert now a “pocket milling cycle” (CYCLE63) into the program for “roughing” the pocket. Press the VSK 4 “Pocket” to open the input mask for the CYCLE63 “Mill pocket”. Enter following values into the input mask. Use the “Select” key on the MCP where indicated.

Note: With the blue “Select”-key the machining depth “Z1” can be set to “inc” or “abs” and the tool path step over “DXY” can be set to % of tool Ø or a value in mm of the tool Ø. Confirm your inputs by pressing the VSK 8 “Accept”. The following line will be inserted into the program: N200 CYCLE63("CONTOUR_POCKET",1011,100,5,1,15,0.15,0.1,50,5,0.3,0.3,0,0,0,6,1.25,15,1,2,,,,0,1 01,111) 26.

Insert now a tool call into the program. First Press HSK 1 “Edit”. Vertical softkey-bar with additional functions opens. Press the VSK 1.1 “Select tool”. The “Tool list” window opens. Use the blue cursor keys on the keyboard to select the tool “CUTTER_D8”. Press the VSK 1.1 “To program”. The line N210 T="CUTTER_D8" will be inserted into the program. Alternatively you can enter this line by hand.

B624

Page 18


Section 3


Program now the following G code commands:

Notes:

N220 M6 N230 S4774 M3 N240 G95 FZ=0.1; Feed rate per tooth 28.

Insert now a “Pocket residual material” cycle (CYCLE63) for residual material “roughing” of the pocket into the program. To do this, press the HSK 1.4 “Cont. Mill” to open the technology “Contour milling”. Press the VSK 5 “Pocket res.mat.” to open the input mask for the CYCLE63 “Pocket residual material”. Enter following values into the input mask. Use the “Select” key on the MCP where indicated.

Note: With the blue “Select”-key the machining depth “Z1” can be set to “inc” or “abs” and the tool path step over “DXY” can be set to % of tool Ø or a value in mm of the tool Ø. Confirm your inputs by pressing the VSK 8 “Accept”. The following line will be inserted into the program: N250 CYCLE63 ("POCKET_RESID_MAT",1001,100,0,1,20,0.1,,50, 2.5,0.3,0.3,0,0,0,,,,,,"CUTTER_D16",1,,0,1101,11) 29.

Insert another pocket milling cycle (CYCLE63) into the program for “base finishing”. Press the VSK 4 “Pocket” to open the input mask for the CYCLE63 “Mill pocket”.

30.

Program now the following G code commands: N260 S5968


Page 19

B624

Section 3


Notes:


Confirm your inputs by pressing the VSK 8 “Accept”. The following line will be inserted into the program: N270 CYCLE63 ("POCKET_FINISH_BASE",1003,100,0,1,20,0.05,0 .1,50,5,0.3,0.3,0,0,0,6,1.25,15,1,2,,,,0,101,111) 31.

Insert another “pocket milling cycle” (CYCLE63) into the program for “Wall finishing”. Press the VSK 4 “Pocket” to open the input mask for the CYCLE63 “Mill pocket”. Enter following values into the input mask. Use the “Select” key on the MCP where indicated.

B624

Page 20


Section 3


Notes:

The following line will be inserted into the program: N280 CYCLE63 ("POCKET_FINISH_WALL",1004,100,0,1,20,0.05,0 .1,50,5,0.3,0.3,0,0,0,6,1.25,15,1,2,,,,0,101,111) 32.

Program the following G code command to end the program: N290 M30

33.

Now program the contour description for the “Moulding plate outside”, that you have called up in step 7 and in the program line N70 before. Press now the VSK 1 “Contour”. Press the VSK ”New contour” to insert a new contour description for the machining operation. The window for the contour name input opens. Assign the following name for the new contour.

Confirm your input by pressing VSK 8 “Accept”. 34.

The contour description window opens, where you can enter a starting point for the new contour.


Page 21

B624

Section 3


Notes:

Enter the starting point coordinates as follows:

Confirm your inputs by pressing the VSK 8 “Accept”. The contour description is being started and new functions to define the contour are available on the vertical softkey-bar on the right of the screen. 35.

Start now the contour description with the first contour element “Straight line Y”. Press the VSK 1.3 “Straight line Y”. The input mask for the straight line in Y-direction opens. Enter the following coordinates:

Confirm your inputs by pressing the VSK 8 “Accept”. The first contour element is to be created. 36.

Extend the contour now, by adding a straight line in X-direction. Press the VSK 1.2 “Straight line X“. The input mask for the straight line in X-direction opens. Enter the following coordinates:

Confirm your inputs by pressing the VSK 8 “Accept”. The contour description is extended by a new element. 37.

B624

Finish the contour description by adding a straight line in Y-direction. Page 22


Section 3

Complex programming example Press the VSK 1.3 “Straight line Y” The input mask for the “Straight line Y” opens.

Notes:

Enter the following coordinates:

Confirm your inputs by pressing the VSK 8 “Accept”. The contour description will be finished. 38.

Check now the outline of the programmed contour. For this, use the blue cursor keys on the keyboard to place the orange selection cursor on the symbol on the left side of the screen. The following screen will be shown.


Page 23

B624

Section 3


Notes:

Finish now the contour description by pressing the VSK 8 “Accept” . The editor window opens and the following lines will be inserted into the program: N300 E_LAB_A_MOULDINGPLATE_OUTSIDE: ;#SM Z:2 ;#7__DlgK contour definition begin - Don't change!;*GP*;*RO*;*HD* G17 G90 DIAMOF;*GP* G0 X-35 Y-100 ;*GP* G1 Y35 RND=15 ;*GP* X35 RND=15 ;*GP* Y-100 ;*GP* ;CON,0,0.0000,3,3,MST:0,0,AX:X,Y,I,J;*GP*;*RO*;* HD* ;S,EX:-35,EY:-100;*GP*;*RO*;*HD* ;LU,EY:35;*GP*;*RO*;*HD* ;R,RROUND:15;*GP*;*RO*;*HD* ;LR,EX:35;*GP*;*RO*;*HD* ;R,RROUND:15;*GP*;*RO*;*HD* ;LD,EY:-100;*GP*;*RO*;*HD* ;#End contour definition end - Don't change!;*GP*;*RO*;*HD* E_LAB_E_MOULDINGPLATE_OUTSIDE:

39.

Now program the contour description for the “Moulding plate pocket”, that you have called up in step 22 and in the program line N180. Press now the VSK 1 “Contour”. Press the VSK ”New contour” to insert a new contour description for the machining operation.

40.

The window for the contour name input opens. Assign the following name for the new contour.


B624

The contour description window opens, where you can enter a starting point for the new contour,

Page 24


Section 3


Notes:

42.



Start now the contour description with the first contour element “Straight line X”. Press the VSK 1.2 “Straight line X”. The input mask for the straight line in X-direction opens. Enter the following coordinates:

Confirm your inputs by pressing the VSK 8 “Accept”. The first contour element is being created. 44.

Extend the contour now, by adding a straight line in Y-direction. Press the VSK 1.3 “Straight line Y“. The input mask for the straight line in Y-direction opens.


Page 25

B624

Section 3 Notes:

Complex programming example .

Enter the following coordinates:


Extend the contour now, by adding a circle in clockwise direction. Press the VSK 1.5 “Circle“. The input mask for the circle opens. Enter the following coordinates:

Confirm your inputs by pressing the VSK 8 “Accept” . The contour description is extended by a new element. 46.

Extend the contour now, by adding a straight line in Y-direction. Press the VSK 1.3 “Straight line Y“. The input mask for the straight line in Y-direction opens.

B624

Page 26


Section 3

Complex programming example Enter the following coordinates:

Notes:


Finish the contour description by adding a straight line in X-direction. Press the VSK 1.2 “Straight line X” The input mask for the “Straight line X” opens. Enter the following coordinates:

Confirm your inputs by pressing the VSK 8 “Accept”. The contour description of the pocket will be finished. 48.

Check now the outline of the programmed contour.


Page 27

B624

Section 3 Notes:

Complex programming example For this, use the blue cursor keys on the keyboard to place the orange selection cursor on the symbol on the left side of the screen. The following screen will be shown.

Finish now the contour description by pressing the VSK 8 “Accept” . The editor window opens and the following lines will be inserted into the program: N310 E_LAB_A_MOULDINGPLATE_POCKET: ;#SM Z:5 ;#7__DlgK contour definition begin - Don't change!;*GP*;*RO*;*HD* G17 G90 DIAMOF;*GP* G0 X0 Y-90 ;*GP* G1 X30 RND=5 ;*GP* Y-20 RND=5 ;*GP* G2 X-30 I=AC(0) J=AC(-.1) RND=5 ;*GP* G1 Y-90 RND=5 ;*GP* X0 ;*GP* ;CON,0,0.0000,6,6,MST:0,0,AX:X,Y,I,J;*GP*;*RO*;* HD* ;S,EX:0,EY:-90;*GP*;*RO*;*HD* ;LR,EX:30;*GP*;*RO*;*HD* ;R,RROUND:5;*GP*;*RO*;*HD* ;LU,EY:-20;*GP*;*RO*;*HD* ;R,RROUND:5;*GP*;*RO*;*HD* ;ACW,DIA:0/235,EX:-30,EY:20,RAD:36;*GP*;*RO*;*HD* ;R,RROUND:5;*GP*;*RO*;*HD* ;LD,EY:-90;*GP*;*RO*;*HD* ;R,RROUND:5;*GP*;*RO*;*HD* ;LR,EX:0;*GP*;*RO*;*HD* ;#End contour definition end - Don't change!;*GP*;*RO*;*HD* E_LAB_E_MOULDINGPLATE_POCKET:

B624

Page 28


Section 3


Now program the contour description for the “Boundary”, that you have called up in step 13 and in the program line N110.

Notes:

Press now the VSK 1 “Contour”. Press the VSK ”New contour” to insert a new contour description for the machining operation. The window for the contour name input opens. Assign the following name for the new contour.





Start now the contour description with the first contour element “Straight line Y”.


Page 29

B624

Section 3


Notes:

Press the VSK 1.3 “Straight line Y”. The input mask for the straight line in Y-direction opens. Enter the following coordinates:

Confirm your inputs by pressing the VSK 8 “Accept”. The first contour element is being created. 52.

Extend the contour now, by adding a Straight line in X-direction. Press the VSK 1.2 “Straight line X“. The input mask for the “straight line X” opens. Enter the following coordinates:


Extend the contour now, by adding a Straight line in Y-direction. Press the VSK 1.3 “Straight line Y”. The input mask for the “straight line Y” opens. Enter the following coordinates:

Confirm your inputs by pressing the VSK 8 “Accept”. The contour description is extended by a new element.

B624

Page 30


Section 3


Finish the contour description by adding a straight line in X-direction.

Notes:

Press the VSK 1.2 “Straight line X” The input mask for the “Straight line X” opens. Enter the following coordinates:

Confirm your inputs by pressing the VSK 8 “Accept”. The contour description of the “Boundary” will be finished. 55.

Check now the outline of the programmed contour. For this, use the blue cursor keys on the keyboard to place the orange selection cursor on the symbol on the left side of the screen. The following screen will be shown.


Page 31

B624

Section 3


Notes:

Finish now the contour description by pressing the VSK 8 “Accept” . The editor window opens and the following lines will be inserted into the program: N320 E_LAB_A_BOUNDARY: ;#SM Z:2 ;#7__DlgK contour definition begin - Don't change!;*GP*;*RO*;*HD* G17 G90 DIAMOF;*GP* G0 X-30 Y-100 ;*GP* G1 Y40 ;*GP* X30 ;*GP* Y-100 ;*GP* X-30 ;*GP* ;CON,0,0.0000,5,5,MST:0,0,AX:X,Y,I,J;*GP*;*RO*;* HD* ;S,EX:-30,EY:-100;*GP*;*RO*;*HD* ;LU,EY:40;*GP*;*RO*;*HD* ;LR,EX:30;*GP*;*RO*;*HD* ;LD,EY:-100;*GP*;*RO*;*HD* ;LL,EX:-30;*GP*;*RO*;*HD* ;#End contour definition end - Don't change!;*GP*;*RO*;*HD* E_LAB_E_BOUNDARY: 56.

Now program the contour description for the “Moulding plate spigot”, that you have called up in step 7 and in the program line N120. Press now the VSK 1 “Contour”. Press the VSK ”New contour” to insert a new contour description for the machining operation.

.

The window for the contour name input opens. Assign the following name for the new contour:


B624


Page 32


Section 3


Notes:



Start now the contour description with the first contour element a “Circle” in clockwise direction. Press the VSK 1.5 “Circle“. The input mask for the circle opens. Enter the following coordinates:

Confirm your inputs by pressing the VSK 8 “Accept”. The contour description is extended by a new element. 828D/840Dsl SINUMERIK Operate

Page 33

B624

Section 3 Notes:


Extend the contour now, by adding a Straight line in Y-direction. Press the VSK 1.3 “Straight line Y”. The input mask for the straight line in Y-direction opens. Enter the following coordinates:


Extend the contour now, by adding a circle in clockwise direction. Press the VSK 1.5 “Circle“. The input mask for the “circle” opens. Enter the following coordinates:

Confirm your inputs by pressing the VSK 8 “Accept”. The contour description is extended by a new element.

B624

Page 34


Section 3


Extend the contour now, by adding a Straight line in Y-direction.

Notes:

Press the VSK 1.3 “Straight line Y”. The input mask for the straight line in Y-direction opens. Enter the following coordinates:


Finish the contour description by adding a circle in clockwise direction. Press the VSK 1.3 “Circle” The input mask for the “Straight line X” opens. Enter the following coordinates:

Confirm your inputs by pressing the VSK 8 “Accept”. The contour description of the “Spigot” is now finished. 63.

Check now the outline of the programmed contour.


Page 35

B624

Section 3 Notes:

Complex programming example For this, use the blue cursor keys on the keyboard to place the orange selection cursor on the symbol on the left side of the screen. The following screen will be shown.

Finish now the contour description by pressing the VSK 8 “Accept” . The editor window opens and the following lines will be inserted into the program: N330 E_LAB_A_MOLDINGPLATE_SPIGOT: ;#SM Z:5 ;#7__DlgK contour definition begin - Don't change!;*GP*;*RO*;*HD* G17 G90 DIAMOF;*GP* G0 X0 Y-30 ;*GP* G2 X-20 Y-22.361 I=AC(0) J=AC(0) ;*GP* G1 Y22.361 ;*GP* G2 X20 I=AC(0) J=AC(0) ;*GP* G1 Y-22.361 ;*GP* G2 X0 Y-30 I=AC(0) J=AC(-0) ;*GP* ;CON,0,0.0000,6,6,MST:0,0,AX:X,Y,I,J;*GP*;*RO*;* HD* ;S,EX:0,EY:-30;*GP*;*RO*;*HD* ;ACW,DIA:207/15,EX:20,CX:0,RAD:30;*GP*;*RO*;*HD* ;LU,EY:22.361;*GP*;*RO*;*HD* ;ACW,DIA:7/215,EX:20,CX:0,RAD:30;*GP*;*RO*;*H D* ;LD,EY:-22.361;*GP*;*RO*;*HD* ;ACW,DIA:0/35,EX:0,EY:30,RAD:30;*GP*;*RO*;*HD* ;#End contour definition end - Don't change!;*GP*;*RO*;*HD* E_LAB_E_MOLDINGPLATE_SPIGOT:

B624

Page 36


Section 3

Complex programming example Program overview “DIN_COUNTOURMILLING_2.MPF” after completion of all inputs.

Notes:

N10 G54 G17 G90 N20 WORKPIECE(,,,"BOX",64,0,-25,-80,-50,-100,100,150) N30 T="CUTTER_D32" N40 M6 N50 S1194 M3 N60 G95 FZ=0.15 N70 CYCLE62("MOULDINGPLATE_OUTSIDE",1,,) N80 CYCLE72("",100,0,1,15,5,0.3,0.3,0.15,0.1,1,41,1,5,0.1,11,5,0,1,2,101,1011,100) N90 S1942 N100 CYCLE72("",100,0,1,15,5,0.3,0.3,0.08,0.1,2,41,1,5,0.1,1,5,0,1,2,101,1011,100) N110 CYCLE62("BOUNDRY",1,,) N120 CYCLE62("MOLDINGPLATE_SPIGOT",1,,) N130 CYCLE63 ("SPIGOT_ROUGHING",1001,100,0,1,5,0.15,,50,2.5,0.3,0,0,0,0,,,,1,2,,,,0,201,111) N140 CYCLE63 ("SPIGOT_FINISH_WALL",1004,100,0,1,5,0.08,,50,2.5,0.3,0,0,0,0,,,,1,2,,,,0,201,111) N150 T="CUTTER_D16" N160 M6 N170 S2388 M3 N180 G95 FZ=0.15 N190 CYCLE62("MOULDINGPLATE_POCKET",1,,) N200 CYCLE63("POCKET_ROUGHING",1011,100,5,1,15,0.15,0.1,50,5,0.3,0.3,0,0,0,6,1.25,15,1,2,,,,0,101,111) N210 T="CUTTER_D8" N220 M6 N230 S4766 M3 N240 G95 FZ=0.1 N250 CYCLE63 ("POCKET_RESID_MAT",1001,100,0,1,20,0.1,,50,2.5,0.3,0.3,0,0,0,,,,,,"CUTTER_ D16",1,,0,1101,11) N260 S5968 N270 CYCLE63 ("POCKET_FINISH_BASE",1003,100,0,1,20,0.05,0.1,50,5,0.3,0.3,0,0,0,6,1.25,15, 1,2,,,,0,101,111) N280 CYCLE63 ("POCKET_FINISH_WALL",1004,100,0,1,20,0.05,0.1,50,5,0.3,0.3,0,0,0,6,1.25,15, 1,2,,,,0,101,111) N290 M30 N300 E_LAB_A_MOULDINGPLATE_OUTSIDE: ;#SM Z:2 ;#7__DlgK contour definition begin - Don't change!;*GP*;*RO*;*HD* G17 G90 DIAMOF;*GP* G0 X-35 Y-100 ;*GP* G1 Y35 RND=15 ;*GP* X35 RND=15 ;*GP* Y-100 ;*GP* ;CON,0,0.0000,4,4,MST:0,0,AX:X,Y,I,J;*GP*;*RO*;*HD ;S,EX:-35,EY:-100;*GP*;*RO*;*HD* ;LU,EY:35;*GP*;*RO*;*HD* ;R,RROUND:15;*GP*;*RO*;*HD* ;LR,EX:35;*GP*;*RO*;*HD* ;R,RROUND:15;*GP*;*RO*;*HD* ;LD,EY:-100;*GP*;*RO*;*HD* ;#End contour definition end - Don't change!;*GP*;*RO*;*HD* E_LAB_E_MOULDINGPLATE_OUTSIDE: 828D/840Dsl SINUMERIK Operate

Page 37

B624

Section 3


Notes: N310 E_LAB_A_MOULDINGPLATE_POCKET: ;#SM Z:5 ;#7__DlgK contour definition begin - Don't change!;*GP*;*RO*;*HD* G17 G90 DIAMOF;*GP* G0 X0 Y-90 ;*GP* G1 X30 RND=5 ;*GP* Y-20 RND=5 ;*GP* G2 X-30 I=AC(0) J=AC(-.1) RND=5 ;*GP* G1 Y-90 RND=5 ;*GP* X0 ;*GP* ;CON,0,0.0000,6,6,MST:0,0,AX:X,Y,I,J;*GP*;*RO*;*HD* ;S,EX:0,EY:-90;*GP*;*RO*;*HD* ;LR,EX:30;*GP*;*RO*;*HD* ;R,RROUND:5;*GP*;*RO*;*HD* ;LU,EY:-20;*GP*;*RO*;*HD* ;R,RROUND:5;*GP*;*RO*;*HD* ;ACW,DIA:0/235,EX:-30,EY:-20,RAD:36;*GP*;*RO*;*HD* ;R,RROUND:5;*GP*;*RO*;*HD* ;LD,EY:-90;*GP*;*RO*;*HD* ;R,RROUND:5;*GP*;*RO*;*HD* ;LR,EX:0;*GP*;*RO*;*HD* ;#End contour definition end - Don't change!;*GP*;*RO*;*HD* E_LAB_E_MOULDINGPLATE_POCKET: N320 E_LAB_A_BOUNDARY: ;#SM Z:2 ;#7__DlgK contour definition begin - Don't change!;*GP*;*RO*;*HD* G17 G90 DIAMOF;*GP* G0 X-30 Y-100 ;*GP* G1 Y40 ;*GP* X30 ;*GP* Y-100 ;*GP* X-30 ;*GP* ;CON,0,0.0000,5,5,MST:0,0,AX:X,Y,I,J;*GP*;*RO*;*HD* ;S,EX:-30,EY:-100;*GP*;*RO*;*HD* ;LU,EY:40;*GP*;*RO*;*HD* ;LR,EX:30;*GP*;*RO*;*HD* ;LD,EY:-100;*GP*;*RO*;*HD* ;LL,EX:-30;*GP*;*RO*;*HD* ;#End contour definition end - Don't change!;*GP*;*RO*;*HD* E_LAB_E_BOUNDARY: N330 E_LAB_A_MOLDINGPLATE_SPIGOT: ;#SM Z:5 ;#7__DlgK contour definition begin - Don't change!;*GP*;*RO*;*HD* G17 G90 DIAMOF;*GP* G0 X0 Y-30 ;*GP* G2 X-20 Y-22.361 I=AC(0) J=AC(0) ;*GP* G1 Y22.361 ;*GP* G2 X20 I=AC(0) J=AC(0) ;*GP* G1 Y-22.361 ;*GP* G2 X0 Y-30 I=AC(0) J=AC(-0) ;*GP* ;CON,0,0.0000,6,6,MST:0,0,AX:X,Y,I,J;*GP*;*RO*;*HD* ;S,EX:0,EY:-30;*GP*;*RO*;*HD* ;ACW,DIA:207/15,EX:-20,CX:0,RAD:30;*GP*;*RO*;*HD* ;LU,EY:22.361;*GP*;*RO*;*HD* ;ACW,DIA:7/215,EX:20,CX:0,RAD:30;*GP*;*RO*;*HD* ;LD,EY:-22.361;*GP*;*RO*;*HD* ;ACW,DIA:0/35,EX:0,EY:-30,RAD:30;*GP*;*RO*;*HD* ;#End contour definition end - Don't change!;*GP*;*RO*;*HD* E_LAB_E_MOLDINGPLATE_SPIGOT:

B624

Page 38


Section 3


Start the simulation of the program.

Notes:

Press the HSK 1.7 “Simulation” to open the simulation window. The control calculates the simulation and shows the simulation by default in the “top view”.

Press the VSK 1.4 “3D view“ to run the simulation in a 3D view.


Page 39

B624

Section End Notes:

B624

Page 40


B656

1

Measurement milling

Brief description

Objective of the module: Working through this module you become familiar with the technology “Measurement milling” by programming two G-code programs with the programGUIDE in ShopMill. Description of the module: This module shows the efficient measuring of the top side of a workpiece, as well as the measuring of the 4 edges of a rectangular workpiece

Content: Simple programming example Complex programming example


Page 1


B656

B656

B656

Page 2


B656 Measure milling - programGUIDE: Description

Measure milling programGUIDE: START

This module shows the efficient measuring of the top side of a workpiece, as well as the measuring of the 4 edges of a rectangular workpiece



Measure milling programGUIDE: END

Notes :


Page 3

B656

Section 2 Notes:

Simple programming example Description: A simple measuring movement on the top side of the work piece is to be programmed with the programGUIDE in ShopMill.

Aim: A new G code program is to be created and opened in the editor window. The G code lines and the measuring cycle are to be programmed and the program is to be simulated For this, the data shown below is to be used: Tool data:

3D-Probe (3D_PROBE)

2.1 Creating a new programGUIDE program A new programGUIDE program can be created from within all operating modes as follows: 1.

Press the “Program Manager”-key on the keyboard. The program manager is opened directly. - OR -

1.


2.


3.


4.

Press the VSK 4 “programGUIDE G code” to open the input mask for creating a new G code program. Enter a name for the program in the “Name” field, e.g. “DIN_MEASURING_1.MPF” and accept with pressing the VSK 8 “OK”. The program is loaded to the editor.

B656

Page 4


Section 2

Simple programming example 2.2 Programming example: Measuring a surface

Notes:

The following program, with a simple call up of a measuring cycle (CYCLE978), is to be programmed with the programGUIDE in ShopMill:

1.


2.

Insert a blank for the simulation into the program. Press the HSK 1.6 “Various” to open the operating area “Various”. Press the VSK 1 “Blank” to open the parameter mask for the “Blank input”.

3.


Confirm your inputs with pressing the VSK 8 “Accept”. The following line is inserted into the program: N110 WORKPIECE(,,"","RECTANGLE",0,0,-50,80,70,70) 4.

Insert now a measuring probe into the program. Press the HSK 1 “Edit” to open the operating area Edit. Press the VSK 1.1 “Select tool”. The tool list window opens.


Page 5

B656

Section 2


Notes:

Place the orange selection cursor on the tool “3D_PROBE” by using the blue cursor keys on the keyboard an press the VSK 1.8 „OK“. The program line N120 T="3D_PROBE" is inserted into the program. 5.

Insert the following G code commands into the program: N130 M6 N140 G0 Z100 N150 G0 X0 Y0 N160 G0 Z10

6.

Program now the measuring cycle (CYCLE978): Press the “Extend”-key on the operator panel in order to switch to the horizontal softkey bar 2. The horizontal softkey bar 2 opens. Press the HSK 2.6 “Measurem. milling”. The work area “Measurement milling” with extended measuring functions opens. Press the VSK 4 “Workpiece measure”. A vertical softkey bar with functions for measuring workpieces opens. Press the VSK 4 “Plane”. The input window for the cycle “1-pt. Meas./ CYCLE978” opens.

7.


Accept your inputs by pressing the VSK 8 “OK”.

B656

Page 6


Section 2

Simple programming example The following lines are inserted into the program:

Notes:

_MVAR=100 _SETVAL=0 _PRNUM=1 _MA=3 _KNUM=1 _FA=5 _TSA=1 _VMS=0 _NMSP=1 _EVNUM=0 CYCLE978

11.

Program the program end with the following G code command: N170 M30

12.

At the end, simulate the machining of the workpiece. Switch back to the vertical softkey bar 1, by pressing the “Extend”-key on the operator panel.

Press the HSK 1.7 “Simulation” to start the simulation of the program. The control calculates the simulation parameters and opens the simulation in the simulation window in “Top view”.

To view the simulation in 3-D press the VSK 1.4 “3D view”.


Page 7

B656

Section 2


Notes:

B656

Page 8


Section 3


Notes:

Description: A more complex measurement movement on the top side and the 4 edges of the work piece is to be programmed with the programGUIDE in ShopMill. A new G code program is to be created and opened in the editor window. The G code lines and the milling cycle are to be programmed and the program is to be simulated For this, the data shown below are to be used: Tool data:

3D-Probe (3D_PROBE)

3.1 Programming example: Measuring edges The following program with the call up of two measuring cycles is to be programmed.

For this, create a new programGUIDE G code program, like described in section 2.1. Give the program the following name: “DIN_MEASURING_2.MPF“. 1.


2.

Insert now a blank for the simulation into the program. Press the HSK 1.6 “Various” to open the operating area “Various”. Press the VSK 1 “Blank” to open the parameter window for the blank input.


Page 9

B656

Section 3 Notes:



Confirm your inputs by pressing the VSK 8 “Accept”. The following line is inserted into the program: N110 WORKPIECE(,,"","RECTANGLE",0,0,-50,80,70,70) 4.

Insert now a measuring probe into the program. Press the HSK 1 “Edit” to open the operating area Edit. Press the VSK 1.1 “To program”. The tool list window in the operating area “Parameter” opens. Use the blue cursor keys on the keyboard to select the tool “3D_PROBE“. Press the VSK 1.8 “OK”. The program line N120 T="3D_PROBE" Is inserted into the program. Optionally you can program the tool by hand.

5.

Program now the following G code commands: N130 M6 N140 G0 Z10 N150 G0 X0 Y0

6.

Program now the measurement cycle (CYCLE978): Press the “Extend”-key on the operator panel in order to switch to the horizontal softkey bar 2. The horizontal softkey bar 2 opens. Press the VSK 2.6 “Measurem. milling”. The work area “Measurement milling” with extended measuring functions opens . Press the VSK 4 “Workpiece measure”. A vertical softkey bar with functions for measuring workpieces opens. Press the VSK 4 “Plane”. The input window for the cycle “1-pt. Meas./ CYCLE978” opens.

B656

Page 10


Section 3



Notes:

Confirm your inputs by pressing the VSK 8 “OK“. The following lines are inserted into the program: _MVAR=100 _SETVAL=0 _PRNUM=1 _MA=3 _KNUM=1 _FA=5 _TSA=1 _VMS=0 _NMSP=1 _EVNUM=0 CYCLE978 8.

Program now the CYCLE977 to measure the edges of the workpiece. Press the VSK 4 “Workpiece measure”. The vertical softkey bar with different functions for measuring workpieces opens. Press the VSK 1.7 “Extend” to open the vertical softkey bar 2, with more functions for measuring workpieces Here, press the VSK 2.2 “Rectangle” The input window for the cycle „Meas.rectang/ CYCLE977” opens.


Page 11

B656

Section 3 Notes:



Confirm your inputs by pressing the VSK 8 “OK“. The following line is inserted into the program: _MVAR=106 _SETV[0]=100 _SETV[1]=100 _PRNUM=1 _KNUM=1 _FA=10 _TSA=1 _VMS=0 _NMSP=1 _ID=-20 CYCLE977 10.

At last, program the end of the program with the following G code command: N160 M30

11.

Simulate now the measuring of the workpiece. Switch back to the horizontal softkey bar 1, by pressing the “Extend”-key on the operator panel. Press the HSK 1.6 „Simulation“ to start the simulation of the program. The control calculates the simulation parameters and opens the simulation in the simulation window in “Top view”. First, the top side of the workpiece is measured, then successively the edges.

B656

Page 12


Section 3


Notes:

To view the simulation in 3-D press the VSK 1.4 “3D view”.


Page 13

B656

Notes:

B656

Page 14


B600

1

Basics of programming with ShopMill

Brief description

Objective of the module: Working with this module you will learn the basics of creating ShopMill sequential programs. Description of the module: This module explains the general structure of a ShopMill program which includes the program header, the program block and the program ending. In addition to this, the programming of chained programming blocks (sequential programs), the functions of the “Editor”, as well as the functions “Various”, Simulation” and “NC Execute” will be described. Content: Basics Creating ShopMill programs Editor Various Simulation NC Execute


Page 1


B600

B600

B600

Page 2


B600 Basics of programming with Shopmill: Description

Basics of programming with Shopmill: START

This module explains the general structure of a ShopMill program which includes the program header, the program block and the program ending. In addition to this, the programming of chained programming blocks (sequential programs), the functions of the “Editor”, as well as the functions “Various”, Simulation” and “NC Execute” will be described.

Basics

Creating ShopMill programs

Editor

Various

Simulation

NC Execute

Basics of programming with Shopmill: END

Notes :


Page 3

B600

Section 2 Notes:

Basics 2. 1 Programming with ShopMill ShopMill offers the option to create NC programs directly on the control in the manner of chained sequential block programs. It also offers the option to program G-code programs directly, with additional ShopMill functionality. Note: The creation of G code programs under ShopMill is described in detail in module - B604 „Basics of programming programGUIDE“. The advantage of programming a ShopMill program lies in the graphical guiding of the programming process in the editor. The following functions are available for this task:  Technology oriented program step selection (technology/cycles) using softkeys  Input masks and windows for parameters, with animated help graphics  Context sensitive online help for every input mask and window  Support for the contour input (geometric processor) ShopMill programs can be represented in different views:  As a work plan, showing the program header, the programming steps with their linkages (chains) and the end of the program.

B600

Page 4


Section 2

Basics

Notes:  As a programming graphic in the graphic view (with activated VSK 3 “Graphic view”): The workpiece or machining step are shown as an outline graphic in side view or top view. The marked program block in the work plan is shown with a different colour.

 As a parameter mask with a help graphic in 3-D, or a simulation of the machining step in side view or top view. If available, the view changes continuously from Help picture to animation.

The animated help graphics are displayed always in the correct position to the adjusted coordinate system. The parameters are dynamically overlayed into the graphic and are highlighted in a different colour.


Page 5

B600

Section 2 Notes:

Basics 2.2 The work plan Main aspect of programming with ShopMill is the “Work plan” in the editor window. The structure of the “Work plan” is as below:  Program header (with the base settings of the program like measuring units, work offset, blank dimensions, retraction plane, safety distance etc.)  Program blocks (the program steps with the cycles)  End of program (see also picture below)

2.2.1 Program header The program header (also see section 2.2) contains the dimensions of the blank for the simulation, as well as the parameters that influence the whole program, as for example:  Work offset  Dimension units (mm/inch)  Tool axis X, Y or Z  Retraction plane, safety distance and machining sense In the work plan, the program header is at the beginning of the program and is labelled with the icon , and the signature “Program header” and the corresponding parameters (see picture below).

2.2.2 Program blocks Program blocks are programmed working steps, which are shown in the editor in single rows marked with an icon and text representing the corresponding technology and the entered parameters (alike the picture below).

2.2.3 Sequential program blocks For the functions “Drill”, “Mill”, and “Contour milling”, technology blocks and contours are programmed separately. These programming blocks are automatically linked by the control and connected in the work plan with square brackets. Technology blocks are blocks that describe in which manner the machining is to be processed, such as for instance centring and drilling. Position blocks or geometry blocks respectively, describe the positions where machining takes place, e.g. holes on a bolt hole pattern. A sequential program block (chain) is only considered closed, if one ore more Technology blocks, end with a Position block. A error massage will be output if one of these elements is missing.

B600

Page 6


Section 2

Basics The icons of these blocks are marked by a square bracket, right beside the Technology block icon, from the beginning of the program chain to the end of the program chain. Every technology is represented by a unique icon. This icon and its chaining are also displayed on the left edge of the screen in the programming graphics and parameter input masks. (here centering, drilling and position circle).

Notes:

2.2.4 End of program The program end indicates to the control the end of the processing of the workpiece. Besides, you can define to repeat the program for multiple workpieces. The program end is marked with the icon and the text “End of program” and if selected with the text “Repetition = Yes” (see picture below).

2.2.5 G code programming steps In the work plan, G code program blocks can also be inserted. For this, you must place the cursor on the desired position in the editor window, where you want to insert the G code block. Pressing the yellow “INSERT”-key on the keyboard, opens a new orange command line, marked with the letter G and a blinking cursor where you can enter G code commands. With the blue “cursor up” or “cursor down” the block can be closed. The input value is now accepted. From a G code line you can not switch to a parameter mask window.

2.3 Navigation in the editor window For a fast and comfortable navigation within a sequential program and the parameter masks you can use the blue cursor keys. With the blue “cursor-up” key on the keyboard you can navigate upwards in the program editor and the parameter masks. With the blue “cursor-down”-key on the keyboard you can navigate downwards in the program editor and the parameter masks. The arrow symbol (extend-symbol) on the right side of program block line in the editor window indicates that you can enter the parameter input mask by pressing the “cursor-to-the-right” key. The “cursor-to-the-right” key opens the parameter mask of the corresponding program block. The “cursor-to-the-left” key closes the parameter mask of the corresponding program block and brings you back to the editor window, displaying the ShopMill program steps.


Page 7

B600

Section 3 Notes:

Creating ShopMill programs 3.1 Creating a new ShopMill program A new ShopMill program can be created from the operating modes “JOG”, “MDA” and “AUTO” as follows: Press the “Program Manager“ key on the keyboard. The window for creating and manage programs opens directly. See module B575 - „Operating area Program Manager“. - OR Press the “MENU SELECT“ key on the operator panel (OP). Press the yellow HSK 4 “Program Manager“. The window for creating and managing programs opens.

- THEN Select a storage drive by pressing the horizontal softkey “NC”, “Local drive” or “USB” where you want to create the program. Move the orange cursor with the blue cursor-keys to the directory of your choice. For the navigation process refer to the modules B566 “Operating elements“ or B575 - “Operating area Program Manager“. Press the VSK 2 “New”. The vertical softkey bar with functions for creating new programs opens. Press the VSK 3 “ShopMill”, to open the input mask for creating a new sequential ShopMill program, like displayed below.

B600

Page 8


Section 3


Notes:

3.2 Defining the program header After entering a name for the program and pressing the VSK 8 “OK” the mask for entering the parameters for the program header opens automatically. Here you can enter parameters for the measuring units, the work offset, blank shape, blank dimensions, retraction plane, safety distance, machining sense and the retract position patterns (see picture below).

Enter the appropriate parameter values and confirm with pressing the VSK 8 “Accept” or abort with pressing the VSK 7 “Cancel”, to switch back to the editor window. The view changes to the work plan view in the editor window. Program header and program end are automatically programmed.


Page 9

B600

Section 3 Notes:

Creating ShopMill programs 3.3 Creating program blocks Place the orange cursor on the program header block, or any other program block after which you want to insert a new program block. Select a technology you want to apply like “Drilling”, “Milling”, “Contour milling”, “Straight Circle”. For example select “Milling” -> “Pocket” -> “Rectangular pocket” to open the corresponding parameter window and help screen by means animation for this technology.

Enter the appropriate parameter values and confirm with pressing the VSK 8 “Accept” or abort with pressing the VSK 7 “Cancel”, to switch back to the editor window. The new program block is inserted automatically into the editor window. The “cursor-to-the-right” key opens the parameter window anytime, to change the input parameters you have done before.

If necessary enter more program steps like described above.

B600

Page 10


Section 3


Notes:

3.4 End of program The program block “End of program” is already created automatically upon creation of a new program. if you want to make changes to the program end, you have to place the orange selection cursor with the blue arrow keys on the “End of program” block and extend the display by pressing the “cursor-to-the-right” key. The parameter input mask for “END of program” opens as displayed below. You can set here , if the program is to be repeated for multiple workpieces.

Select “Yes” if you want to repeat the workpiece and confirm with pressing the VSK 8 “Accept” or abort with pressing the VSK 7 “Cancel” to switch back to the editor window. The new values entered are updated automatically .


Page 11

B600

Section 4 Notes:

Edit With the editor you can create, supplement and change part programs. 4.1 Selecting the function “Edit“ The function “Editor” can be opened from the operating mode “JOG”, “MDA“ and “AUTO“. By pressing the “PROGRAM“-key on the keyboard the operating area “Program” opens, showing the last program you have worked on. - OR Press the “MENU SELECT“-key on the operator panel (OP). Press the yellow HSK 3 “Program“ to switch to the operating area “Program“. The operating area “Program” opens, showing the last program you have worked on (see picture below). If not selected, press the HSK 1 “Edit”. If no program was loaded after starting the control, the “program manager” window opens first, after pressing the HSK 3 “Program”. Here you can select either a existing ShopMillprogram or create a new one. See module - B574 “Operating area Program” und module - B576 “Operating area Program Manager“. The following softkeys with their corresponding functions are now available in the vertical softkey bar:

B600

Page 12


Section 4

Edit

Notes:


Description In a ShopMill program the tool call is inside the cycle mask. The function “Select tool” is available for ShopMill programs under the technologies “Drilling”, Milling, “Contour milling”, “Straight Circle” or in a corresponding program block with tool utilization. This is the reason for VSK 1.1 “Select tool” being grayed out (inactive) as long their is no G code line inserted. (see section 2.2.5) By pressing the VSK 1.2 “Graphic view” you can see the simulated workpiece from a top view as an outline drawing (see section 2.1, picture programming graphic). By pressing the VSK 1.3 “Search“ you can search for any text in the program blocks. A search window opens where you can enter a search string. You can continue searching afterwards (see section 4.3). By pressing the VSK 1.4 “Mark” you can mark one or several program blocks in order to copy or cut (delete) them. By pressing the VSK 1.5 “Copy” you can copy one or several program blocks to the internal memory of the control, to paste them to a different location in the active program or to another program. By pressing the VSK 1.6 “Paste“ copied or cut program blocks can be inserted behind the selected program block (actual cursor position). You can paste the block to the active program as well as to another ShopMill program. By pressing the VSK 1.7 “Cut” you can cut out one or several program blocks, to paste them later somewhere in a program or to delete them. Cut out program blocks remain in the clip board and can be inserted again with the VSK 1.6 “Paste” (see VSK 1.6 “Paste“). By pressing the VSK 1.8 “Extend“ the extended vertical softkey bar 2 will be displayed. By pressing the VSK 2.3 “Renumbering” you can assign new numbers for every program step in the Work plan window. (see section 4.4) By pressing the VSK 2.6 “Settings“ you can change the settings for the editor (see section 5.3) By pressing the VSK 2.7 “Exit” you close the editor with the active program. By pressing the VSK 2.8 “Back“ you switch back to the vertical softkey bar 1.


Page 13

B600

Section 4 Notes:

Edit 4.3

Search

With the function “Search” you can search for any text in a sequential program and even replace the text with other text. 4.3.1 Selecting the function “Search” By pressing the VSK1.3 “Search” the search window opens like displayed below, with the following functions available in the vertical softkey bar.


Description By pressing the VSK 1 “Go to start” the cursor will be positioned on the first line of the program. By pressing the VSK 2 “Go to end” the cursor will be positioned on the last line of the program. By pressing the VSK4 “Search” the search mask opens, where you can decide to search for complete words, select the search direction (forward/ backwards) and enter the search text. By pressing the VSK5 “Find + replace” the “Search and replace” mask opens where you can decide to search for complete words, select the search direction (forward/backwards), enter the search text and enter the text you want to use for the replacement. With pressing the VSK 7 “Cancel” you can abort the search process. By pressing the VSK 8 “OK“ you start a search run with the above mentioned search criteria.

B600

Page 14


Section 4

Edit 4.4

Notes:

Renumbering

With the function “Renumbering” you can renumber the program steps in the editor window with an increment you can select here. 4.4.1 Selecting the function “Renumbering” By pressing the VSK 2.3 “Renumbering” the input mask for the renumbering settings of blocks opens.

4.4.2 Parameters for “Renumbering” Parameters

Meaning

First block number

The first block number you want to start with. The values shown here by default can be adjusted under the function “Settings” in the input field “First block number” (see section 4.5).

Increment

The Increment between the program blocks. The values shown here by default can be adjusted under the function “Settings” in the input field “Increment” (see section 4.5).


Page 15

B600

Section 4 Notes:

Edit 4.5

Settings

With the function “Settings” you can change the settings for the editor. 4.5.1 Selecting the function “Settings” By pressing the VSK2.6 “Settings” the input mask for the editor settings opens.

4.5.2 Parameters for “Settings” Parameters

Meaning

Number automatically (Yes/No)

Program blocks will be numbered automatically. Deactivating this parameter, hides the following two parameters too.

First block number

Block number of first block.

Increment

Increment between block numbers.

Show hidden lines (Yes/No)

Show hidden line (with the ID ;*HD).

Display block end as A symbol is displayed at the end of each block. symbol (Yes/No)

B600

Move horizontally (Yes/No)

Blocks are displayed in one line with a scroll bar at the right side.

Save automatically (only local and external drives) (Yes/No)

Changes are saved automatically without a query.

Page 16


Section 5

Various

Notes:

5.1 Selecting the function “Various“ The function “Various” can be selected from the operating mode “JOG”, “MDA” or “AUTO” in the operating area “Program” as follows: Press the HSK 1.6 “Various“ to switch over to the function “Various”. A screen similar to the screen shown below opens.

The following functions with their corresponding softkeys are displayed in a vertical softkey bar: 5.2 Vertical softkey bar 1 and 2 Display area

Description By pressing the VSK 1.1 “Settings“ an input mask opens where you can change the settings for the blank (see section 5.3 “Settings”). By pressing the VSK 1.4 “HighSpeed settings“ the input mask for adjusting the settings for the optimal speed in relation to the machining method opens (see section 5.4). By pressing the VSK 1.5 “Transformations” the vertical softkey bar with the functions for the coordinate transformations is displayed (see section 5.5). By pressing the VSK 1.6 “Subprogram” the input mask for loading a subprogram to the main program opens (see section 5.8). By pressing the VSK 1.8 “Extend“ the vertical softkey bar 2 opens.


Page 17

B600

Section 5 Notes:

Various Display area

Description (Continuation) By pressing the VSK 2.3 “Repeat program” the vertical softkey bar with the function for repeating parts of programs opens (see section 5.7). By pressing the VSK 2.8 “Back“ you switch back to the vertical softkey bar 1.

5.3 Settings Each parameter defined in the program header, except the measuring units, can be changed everywhere in the program. The settings in the program header are constant, as long as they are not altered later in the program. For example you can define a new blank in a sequential program later on, if during a simulation run there is the need to change the visible view on the workpiece. This can be reasonable within the functions “Work offset” “Coordinate transformation” “Cylinder barrel transformation” and “Swivelling”. With that you can program the above mentioned functions first, and then define the blank afterwards. The function “Settings” can be opened as follows: 5.3.1 Selecting the function “Settings” By pressing the VSK 1.1 “Settings” the following window for entering the parameters for the blank opens.

B600

Page 18


Section 5

Various 5.3.2

Notes:

Parameters for setting the blank

Parameter

Meaning

X0

1 corner point X

Y0

1 corner point Y

X1 (abs/ink)

2 corner point related to X0 (absolut or incremental)

Y1 (abs/ink)

2 corner point related to Y0 (absolut or incremental)

ZA

Initial dimension

ZI (abs/ink)

Finishing dimension related to ZA (absolut or incremental)

PL

Machining plane:

Help picture/animation

 G17  G18  G19

RP

Retraction plane

SC

Safety distance


Page 19

B600

Section 5 Notes:

Various Parameter

Meaning

Machining sense

Down-cut

Help picture/animation (continuation)

Up-cut

Retraction position RP: pattern Liftmode before new infeed related to parameter RP

Optimized: Lift mode before anew infeed, optimized

B600

Page 20


Section 5

Various 5.3.3 Changing the graphical view on the blank

Notes:

The graphic view on the blank is adjustable under the functions “Edit”, Drilling”, “Milling”, “Contour milling”, “Various” and “Straight Circle” by pressing the softkey “Graphic view”. Within the function “Various” you can adjust the graphic settings with the Softkey “Graphic view” for the blank. Help pictures and animations are only displayed if the VSK 2 “Graphic view” is deselected and only in the side view. You can change the graphic view on the blank as follows: 1.


2.

By activating and deactivating the VSK 2 “Graphic view” you can switch the graphical representation of the blank, the help pictures and animations between 2 different views:  3D-/side view

 A wireframe model


Page 21

B600

Section 5 Notes:

Various 5.3.4 Changing the setting for the blank 1.


2.

Press the VSK 1 “Settings”.

3.

Optionally change the graphic view for the blank between 3D-/side view or wireframe model by pressing the VSK 2 “Graphic view”.

4.

Enter the parameter values for the blank (see parameter list in section 5.3.2).

5.

Confirm your inputs by pressing the VSK 8 “Accept” or abort with pressing the VSK 7 “Cancel”. A new program block “Settings” is inserted in the program (see the picture below).

5.4 High Speed Settings With the machining of free form surfaces, there are high demands on machining speed as well as accuracy and surface finish. The optimal speed profile in conjunction with the machining method (roughing, pre-finishing, finishing) can be adjusted easily with the function “HighSpeed settings”. It is advisable to program the cycle in the technology part first, before programming the geometry part. Machining methods: With the function “HighSpeed settings” you can select from 3 different technological machining methods:  "roughing"  "pre-finishing"  "finishing"  "deselect" (default setting) These four machining methods are associated directly with accuracy, velocity and surface quality of the contour path (see the triangle in the Help pictures). The operator/programmer can make an appropriate weighting by adjusting the tolerance value. Different tolerance values and technologies can be assigned to the four machining methods.

B600

Page 22


Section 5

Various 5.4.1 Selecting the function “HighSpeed settings“

Notes:

By pressing the VSK 4 “HighSpeed settings“ the “High-speed Settings” screen opens. The screen changes in intervals between Help picture and animation.

5.4.2 Parameter for „HighSpeed settings“ Parameter

Help picture

Animation

PL

The parameter for the machining plane is optional and has to be activated by a machine datum.

Tolerance

Tolerance values for the machining

Machining:  Roughing

 Pre-finishing


Page 23

B600

Section 5 Notes:

Various Parameter

Help picture

Animation (continuation)

 Finishing

none

 Deselect

5.4.3 Changing the ”High-speed settings“ 1.

In the operating area “Program“ and operation mode “JOG”, “MDA”, or “AUTO” press the HSK 6 “Various”.

2.

Press the VSK 4 “HighSpeed settings“.

3.

Optionally change the graphic view for the blank between sectional drawing/3-D model or wireframe model by pressing the VSK 2 “Graphic view”.

4.

Enter the parameter values for “Tolerance” and “Machining”. Press the VSK 8 “Accept” to accept your inputs or abort by pressing the VSK 7 “Cancel”. A new program block “High-speed settings” is inserted into the program (see picture below).

B600

Page 24


Section 5

Various

Notes:

5.5 Transformations To make programming easier, you can transform the coordinate system. Use this function, for example, to rotate the coordinate system. Coordinate transformations only apply in the current program. You can define displacement, rotation, scaling or mirroring. You can select between a new or an additive coordinate transformation. In the case of a new coordinate transformation, all previously defined coordinate transformations are deselected. An additive coordinate transformation acts in addition to the currently selected coordinate transformations. Supported are:  Offset: For each axis, you can program an offset of the zero point.  Rotation: You can rotate every axis through a specific angle. A positive angle corresponds to a counter-clockwise rotation.  Scaling: You can specify a scale factor for the active machining plane as well as for the tool axis. The programmed coordinates are then multiplied by this factor. Note that the scaling always refers to the zero point of the workpiece. For example, if you increase the size of a pocket whose centre point does not coincide with the zero point, scaling will shift the centre of the pocket.  Mirroring: Furthermore, you can mirror all axes. Enter the axis to be mirrored in each case. Note that with mirroring, the travel direction of the cutting tool (conventional/climb) is also mirrored.


Page 25

B600

Section 5 Notes:

Various 5.5.1 Selecting the function „Transformations“ By pressing the VSK 5 “Transformations“ the following vertical softkey bar in the editor window opens.


Description By pressing the VSK 1 “Work offset” the parameter window for the work offset opens (see section 5.5.3). By pressing the VSK 2 “Offset” the parameter window for the offset opens (see section 5.5.4). By pressing the VSK 3 “Rotation” the parameter window for the rotations opens (see section 5.5.5). By pressing the VSK 4 “Scaling” the parameter window for the scaling opens (see section 5.5.6). By pressing the VSK 5 “Mirroring” the parameter window for the mirroring opens (see section 5.5.7). The VSK 8 “Back” brings you back to the start screen of the function “Various”.

B600

Page 26


Section 5

Various

Notes:

5.5.3 Work offset You can call work offsets (G54, etc.) from any program. You can use these offsets, for example, when you want to machine workpieces with various blank dimensions using the same program. The offset will, in this case, adapt the workpiece zero to the new blank. 5.5.3.1 Selecting the function “Work offset” By pressing the VSK 1 “Work offset” the input mask “work offset” opens.

5.5.3.2 Parameters for the work offset Parameter

Meaning

Work offset.

Alternative work offsets

 Basic ref.

Basic

 G54

Storable Zero offset

 G55


 G56


 G57



Reference G500

Page 27

B600

Section 5 Notes:

Various 5.5.3.3 Setting the work offset 1.

In the operating area “Program“ and operation mode “JOG”, “MDA”, or “AUTO” press the HSK 6 “Various“ and the VSK5 “Transformations”.

2.

Press the VSK 1 “Work offset”.

3.


4.

Select the work offset (Basic reference, G54, G55, G56 or G57). Press the VSK 8 “Accept” to confirm your selection or press the VSK 7 “Cancel” to abort. A new program block “Work offset” is inserted into the program in the editor window (see picture below).

5.5.4 Offset Offsets apply only to the current program. Besides, you can select between a new and an additive offset. With a new offset, all offsets defined before are deselected. An additive offset works additional to the current selected offset. For every axis an offset can be programmed.

5.5.4.1 Selecting the function “Offset” By pressing the VSK 2 “Offset” the input screen mask ”Offset” opens.

B600

Page 28


Section 5

Various

Notes:

5.5.4.2 Parameters for the “Offset” Parameters

Description

Help picture/Animation

Offset:  New

Adds a new offset

 Additive

Adds an additive offset

Axes:

Unit

 X

Offset X-axis

mm

 Y

Offset Y-axis

mm

 Z

Offset Z-axis

mm

5.5.4.3 Setting the “Offset” 1.


2.

Press the VSK 2 “Offset”.

3.


4.

Select the kind of offset “new” or “additive”. Enter the offset values for the different axes (X,Y,Z) in millimetre. Press the VSK 8 “Accept” to confirm your inputs or press the VSK 7 “Cancel” to abort. A new program block “Offset” is inserted into the program in the editor window (see picture below).


Page 29

B600

Section 5 Notes:

Various 5.5.5 Rotation Rotations apply only to the current program. Besides, you can select between a new and an additive rotation. With a new rotation, all rotations defined before are deselected. An additive rotation works additional to the current selected rotation. For every axis an rotational angle in degrees can be programmed. A positive angle means a rotation counter clockwise. 5.5.5.1 Selecting the function “Rotation“ By pressing the VSK 3 “Rotation“ the input screen mask “Rotation” opens.

5.5.5.2 Parameters for “Rotation” Parameters

Description


Rotation:  New

B600

Adds a new rotation

Page 30


Section 5

Various Parameter

Description

Help picture/Animation (continuation)

Notes:

Rotation:  Additive

Incremental rotation

Axes:  X

Units Rotation around the

mm

X-axis  Y

Rotation around the

mm

Y- axis  Z

Rotation around the

mm

Z-axis 5.5.5.3

Setting the rotations

1.


2.

Press the VSK 3 “Rotation“.

3.


4.

Select if you want to add a “new” or a “additive” rotation. Enter the values for the rotation about the axes X, Y, und Z in degrees. Press the VSK 8 “Accept” to confirm your inputs or press the VSK 7 “Cancel” to abort. A new program block “Rotation” is inserted into the program in the editor window (see picture below).


Page 31

B600

Section 5 Notes:

Various 5.5.6 Scaling Scaling applies only to the current program. Besides, you can select between a new and an additive scaling. With a new scaling, every scaling defined so far is deselected. An additive scaling works incremental to the current selected scaling. You can specify a scale factor for the active machining plane as well as for the tool axis. The programme coordinates are then multiplied by this factor. Note: Note that the scaling always refer to the zero point of the workpiece. For example, if you increase the size of a pocket whose centre point does not coincide with the zero point, scaling will shift the centre of the pocket. 5.5.6.1 Selecting the function “Scaling” By pressing the VSK 4 “Scaling” the input screen mask “Scaling” opens.

5.9.2 Parameters for “Scaling” Parameter

Description


Scaling:  New

B600

Adds a new scaling

Page 32


Section 5

Various Parameter

Description

Help picture/Animation (continuation)

Notes:

Scaling:  Additive

Adds an additive scaling

Axes:  XY

Scaling factor XY

 Z

Scaling factor Z

5.5.6.3 Setting the scaling 1.


2.

Press the VSK 4 „Scaling“.

3.


4.

Select whether the scaling “new” or “additive”. Insert the values for the scaling factor XY and Z. Press the VSK 8 “Accept” to confirm your inputs or press the VSK 7 “Cancel” to abort. A new program block “Rotation” is inserted into the program in the editor window (see picture below).


Page 33

B600

Section 5 Notes:

Various 5.5.7 Mirroring Mirroring applies only to the current program. Besides, you can select between a new and an additive mirroring. With a new mirroring, all mirror images defined so far are deselected. An additive mirroring works additional to the current selected mirroring. Furthermore it is possible to mirror all axes. Activate the axis to be mirrored in each case. Note: Note that with mirroring, the travel direction of the cutting tool (down-cut/up -cut) is also mirrored. 5.5.7.1 Selecting the function “Mirroring” By pressing the VSK 5 “Mirroring” the input screen mask “Mirroring” opens.

5.5.7.2 Parameters for “Mirroring” Parameter

Description


Mirroring:  New

B600

Adds a new mirroring

Page 34


Section 5

Various Parameters

Description

Help picture/animation (continuation)

Notes:

Mirroring:  Additive

Adds an additive mirroring

Axes:  X

Mirroring for the Xaxis (on/off)

 Y

Mirroring for the Yaxis (on/off)

 Z

Mirroring for the Zaxis (on/off)

5.5.7.3 Mirroring the axes 1.


2.

Press the VSK 5 “Mirroring”.

3.


4.

Select whether the Mirroring is “new” or “additive”. Switch on or off the axis that you want to have mirrored. Press the VSK 8 “Accept” to confirm your inputs or press the VSK 7 “Cancel” to abort. A new program block “Mirroring” is inserted into the program in the editor window (see picture below).


Page 35

B600

Section 5 Notes:

Various 5.6 Subprogram If you require the same machining steps in the programming of different workpieces, you can define these machining steps in a separate subroutine. You can then call this subroutine in any program. Identical machining steps therefore only have to be programmed once. ShopMill does not differentiate between main program and subprogram. This means that you can call a "standard" sequential program or G code program as subprograms in another sequential program. In this subprogram, you can also call another subprogram. The maximum nesting depth is 8 subroutines. You cannot insert subroutines among blocks chained by the control. If you want to call a sequential control program as a subroutine, the program must already have been calculated once (load or simulate program in “AUTO” operating mode). This is not necessary for G code subroutines. The subroutine must always be stored in the NCK main memory (in a separate directory "XYZ" or in the "ShopMill", "Part programs", "Subprograms" directories). If you want to call a subprogram located on another drive, you can use G code command "EXTCALL". Note: Please note that, when a subprogram is called, ShopMill evaluates the settings in the program header of the subroutine. These settings also remain active even after the subprogram has ended. If you wish to activate the settings from the program header for the main program again, you can make the settings again in the main program after calling the subprogram. 5.6.1 Selecting the function “Subprogram“ By pressing the VSK 3 “Subprogram” the input screen mask “Subprogram” opens.

B600

Page 36


Section 5

Various

Notes:

5.6.2 Inserting a subprogram 1.

In the operating area “Program“ and operation mode “JOG”, “MDA”, or “AUTO” press the HSK 6 “Various“

2.

Press the VSK 1.6 ”Subprogram”.

3.

Optionally change the graphic view on the blank by pressing the VSK 2 “Graphic view”.

4.

Enter the path to the subprogram folder and the name of the subprogram in the input mask. Press the VSK 8 “Accept” to confirm your inputs or press the VSK 7 “Cancel” to abort. A new program block “Execute” is inserted into the program in the editor window (see picture below).

5.7 Repeating program blocks If certain steps in the machining of a workpiece have to be executed more than once, it is only necessary to program these steps once. ShopMill offers a function for repeating program blocks. You must mark the program blocks that you want to repeat with a start and end marker. You can then call these program blocks up to 9999 times again within a program. The markers must be unique, i.e. they must have different names. No names used in the NCK can be used for this. You can also set markers and repeats after creating the program, but not within chained program blocks. Note: It is also possible to use the same marker as the end marker of the preceding program blocks and as the start marker for the following program blocks. 5.7.1

Selecting the function “Repeat program” By pressing the VSK 3 “Repeat Program” the following vertical softkey bar with the functions for repeating program parts opens.


Description By pressing the VSK 1 “Set Mark” the window for setting a start or end mark opens. By pressing the VSK 2 “Repeat program” an input mask opens where you can specify the start and end marker which enclose the program parts you want to repeat.


Page 37

B600

Section 5 Notes:

Various 5.7.3

Repeating a program block

1.

In the operating area “Program“ and operation mode “JOG”, “MDA”, or “AUTO” press the HSK 6 “Various“

2.

Press the VSK 1.8 “Extend” to open the extended vertical softkey bar 2.

3.

Press the VSK 2.3 “Repeat program”.

4.

Place the orange selection cursor on the program block before the program block that you want to repeat.

5.

Press the VSK 1 “Set Mark” to open the input screen mask for input of the start mark. In the “Set mark” input window, enter a unique name for the start mark (see the following picture).

With pressing the VSK 8 “Accept” a new program block “MARK1” is inserted into the work plan (see picture below).

6.

Place the orange selection cursor on that program block in the editor window that shall be the last block in the repetition sequence.

7.

Press the VSK 1 “Set mark” to open the input screen mask for input of the end mark. In the “Set mark” input window, enter a unique name for the end mark (see the following picture).

With pressing the VSK 8 “Accept” A new program block “MARK2” is inserted into the work plan (see picture below)..

B600

Page 38


Section 5

Various 8.

Place the orange selection cursor on that block, after that you want to repeat the program sequence.

9.

Press the VSK 2.3 “Repeat program”. In the input mask enter the name for the start mark and the end mark as well as the number of repetitions.

Notes:

Confirm your selection by pressing the VSK 8 “Accept”. A new program block “Repetition MARK1 MARK2” is inserted into the work plan (see picture below).

10.

The program blocks between the marks will be repeated during machining of the program.


Page 39

B600

Section 6 Notes:

Simulation ShopMill provides various extensive and detailed simulation functions for displaying the simulation of the machining. During simulation, the current program is calculated in its complete form and the result is displayed in graphic form. You can select the following modes of representation for simulation:  Top view  3-D view  Side view The simulation uses the correct proportions for the tools and workpiece contours. Cylindrical die-sinking cutters, bevel cutters, bevel cutters with corner rounding and tapered die-sinking cutters are displayed as end milling tools. The traverse paths for the tools are shown in colour: Red line = tool is moving at rapid traverse Green line = tool is moving at machining feedrate In all views, a clock is displayed during graphical processing. The displayed machining time (in hours/minutes/seconds) indicates the approximate time that would actually be required to execute the machining program on the machine (incl. tool change). If a program is interrupted during simultaneous recording, the clock stops. In addition, the current axis coordinates, the override, and the program block currently being executed are also displayed. The active tool with the cutting edge number and feedrate are also displayed in the simulation. Transformations are displayed differently during simulation and simultaneous recording:  Coordinate transformations (translation, scaling, …) are displayed as programmed.  Cylinder surface transformations are displayed as a developed surface.  After swivel transformation, the previous machining operations are deleted from the display and only machining of the swivelled plane is displayed (viewing angle perpendicular to the swivelled plane).  Zero offsets (G54, etc.) do not alter the zero in the graphical display. This means that, in the case of multiple clamping, the machining operations for each of the individual workpieces are plotted on top of one another. Note: If you want to display a different portion of the workpiece from the one defined in ShopMill, you can define a new blank in the program (see section 5.3 in this module).

B600

Page 40


Section 6

Simulation

Notes:

6.1 Selecting the function “Simulation“ The function “Simulation” can be selected from the operating mode “JOG“, “MDA“ and “AUTO“ as follows: With a program loaded, press the HSK 1.7 “Simulation“ to start a simulation run. The following screen opens. The simulation starts after a short computing time in the top view by default.

Press the VSK 1.4 “3D view” the simulated workpiece is displayed 3-dimesionally (see picture below).

The following functions will be available in the vertical softkey bar. 828D/840Dsl SINUMERIK Operate

Page 41

B600

Section 6 Notes:

Simulation 6.2 Vertical softkey bar 1 and 2 Display area

Description By pressing the VSK 1.1 “Stop“ the simulation will be halted. The softkey will be replaced with the VSK 1.1 “Start”, in order to continue the simulation again. By pressing the VSK 1.1 “Start” the simulation will be started or continued. The softkey will be replaced with the VSK “Stop”. By pressing the VSK 1.1 “SBL“ the simulation will be processed block by block. This softkey replaces the softkey “Start”, if the VSK 4 “Single block” is activated under the function “Program control”. By pressing the VSK 1.2 “Reset“ the simulation will be aborted, and can be started again by pressing the VSK 1.1 “Start”. The “Top view“ is activated by default and shows the simulation in a plan view from above By pressing the VSK 1.4 “3D view“ the simulation will be shown in a 3-D view By pressing the VSK 1.5 “Further views” the vertical softkey bar opens, with more options to adjust the view on the simulation process (see section 6.3). By pressing the VSK 1.6 “Details“ the vertical softkey bar opens, where you can adjust the level of details that will be shown during the simulation (see section 6.4). By pressing the VSK 1.7 “Program control” the vertical softkey bar opens, with further functions to control the simulation run (see section 6.5). By pressing the VSK 1.8 “Extend” the vertical softkey bar 2 with the following functions will be displayed. By pressing the VSK 2.3 “Show tool path” the display of the simulated tool path can be switched on and off. By pressing the VSK 2.4 “Delete tool path” the animated tool path in the simulation window will be deleted. A new tool path is shown immediately after pressing this softkey or after running a new simulation (if the simulation is in “Stop”- or “Reset”- mode). By pressing the VSK 2.5 “Blank” you can change the dimensions of the simulated blank (see also section 5.3). This softkey is active if the simulation is in “Reset” mode. By pressing the VSK 2.8 “Back” you switch back to the vertical softkey bar 1.

B600

Page 42


Section 6

Simulation

Notes:

6.3 Further views With the function “Further views” you can change the graphical side-views on the blank, to view the simulation process in an optimal way. You can change the sides from which you want to see the simulation. 6.3.1 Selecting the function “Further views” By pressing the VSK 1.5 “Further views” the following window with side views on the blank opens.


Description By pressing the VSK 1 “From front” the simulated workpiece will be shown in a front view. By pressing the VSK 2 “From rear” the simulated workpiece will be shown in a rear view. By pressing the VSK 3 “From left” the simulated workpiece will be shown from the left side. By pressing the VSK 4 “From right” the simulated workpiece will be shown from the right side. By pressing the VSK 8 “Back” on the operator panel (OP) you switch back to the vertical softkey bar of the operating area “Details”.


Page 43

B600

Section 6 Notes:

Simulation 6.4 Details With the function “Details” you can zoom in, zoom out, rotate and cut out parts of the workpiece. 6.4.1 Selecting the function “Details” By pressing the VSK 1.6 “Details“ the following functions are available in a vertical softkey bar.


Description By pressing the VSK 1 “Autozoom“ the workpiece fills out the simulation window in an optimal way. By pressing the VSK 2 “Zoom +“ you zoom in into the simulation window. Alternatively you can press the “+“-key on the number block of the keyboard. By pressing the VSK 3 “Zoom -“ you can zoom out of the simulation window. Alternatively you can press the “-“-key on the keyboard. By pressing the VSK 4 “Zoom” a frame opens in the simulation window, that lets you zoom in to the frame size. Press the VSK1 “Zoom +” to increase and the VSK 2 “Zoom -” to decrease the frame size. Alternatively you can change the frame size of the zoom area with the “+”or “-” key on the number pad of the keyboard. Move the frame with the blue cursor keys on the keyboard. Press the VSK 8 “Accept” to zoom to the selected extent or abort with pressing the VSK 7 “Cancel”.

B600

Page 44


Section 6



Notes:

By pressing the VSK 5 “Rotate view” a vertical softkey bar opens to the right, with functions to rotate the workpiece in the simulation window (see section 6.4.2.1). By pressing the VSK 6 “Cut” the functions for cutting out parts of the workpiece are available in a vertical softkey bar “(see section 6.4.2.3). By pressing the VSK 8 “Back” on the operator panel you switch back to the vertical softkey-bar 1.

6.4.2.1 Selecting the function “Rotate view” By pressing the VSK 5 “Rotate view” the following functions will be displayed in a vertical softkey bar.


Description By pressing the VSK “Arrow right” the workpiece will be turned right around the centre of the simulation window. By pressing the VSK “Arrow left” the workpiece will be turned left around the centre of the simulation window. By pressing the VSK 3 “Arrow up” the work piece will be turned up around the centre of the simulation window. By pressing the VSK 4 “Arrow down” the work piece will be turned down around the centre of the simulation window. By pressing the 5 “Arrow turns left” the workpiece will be rotated to the left, around the centre of the simulation window (counter clockwise). By pressing the 5 “Arrow turns right” the workpiece will be rotated to the right, around the centre of the simulation window (clockwise). By pressing the VSK 8 “Back” you switch back to the VSK-bar “Details”.


Page 45

B600

Section 6 Notes:

Simulation 6.4.2.3

Selecting the function “Cut” By pressing the VSK 1.7 “Cut“ the functions for cutting out parts of the simulated workpiece will be shown in a vertical softkey bar. The cut surface areas are only displayed during simulation run.


Description By pressing the VSK 1 “Cut active” you can activate the cut surfaces on the workpiece and activate the greyed out axes softkeys in the vertical softkey bar. The function “Cut” stays active until the VSK “Cut active” is deactivated. By pressing the VSK 2 “X+“ the cutting plane is shifted on the X-axis to the positive (“to the right”). By pressing the VSK 3 “X-“ the cutting plane is shifted on the X-axis to the negative (“to the left”). By pressing the VSK 4 „Y+“ the cutting plane is shifted on the y-axis (ordinate) to the positive („to the rear “). By pressing the VSK 5 „Y-“ the cutting plane is shifted on the y-axis (ordinate) to the negative (“forward”). By pressing the VSK 6 “Z+“ the cutting plane will be shifted on the Z-axis (applicate) to the positive (“up”).

B600

Page 46


Section 6



Notes:

By pressing the VSK 7 “Z-“ the cutting plane will be shifted on the Z-axis (Ablikate) to the negative (“downward”). By pressing the VSK 8 “Back” you switch back to the operating area “Details”. 6.5 Program control With the function “Program control” the override can be adjusted for the simulation, the program can be executed in single blocks and alarm messages, that occurred during simulation, can be displayed. 6.5.1 Selecting the function “Program control” By pressing the VSK 1.7 “Program control” the following functions will be shown in a vertical softkey bar on the right side of the screen. 6.5.2


Display area

Description By pressing the VSK 1 “100% override” the feedrate override is set to the maximum override of 100%. By pressing the VSK 2 “Override +” the override will be increased in 5% steps each time you press the softkey, until a maximum of 100% is reached. By pressing the VSK 3 “Override -” the override will be decreased in 5% steps each time you press the softkey until a minimum of 0% is reached. With a feedrate override of 0% the simulation is paused. By pressing the VSK 4 “Single block” the simulation will be executed block by block. With pressing this softkey the VSK 1.1 “Start” in the operating area “Simulation” will be exchanged with the “VSK 1.1 “SBL” (see section 6.2). By pressing the VSK 7 “Alarm” the “Simulation alarms” window opens, with alarm messages that have occurred during a simulation run. This can be used for error detection. By pressing the VSK 8 “Back” you switch back to the vertical softkey bar 1.


Page 47

B600

Section 6 Notes:

Simulation 6.6

Selecting the function “Alarm” By pressing the VSK 7 “Alarm” the “Simulation alarms” window opens, with a list of all current active alarm messages that occurred during the simulation. For error messages and acknowledgement symbols see module - B576 “Operating area Diagnostics”, section 3.


Description By pressing the VSK 1 “Acknowl. Alarm” all with the “Reset”- or “Cancel”-symbol marked alarm messages can be deleted. This softkey is inactive as long as no appropriate error message is shown. By pressing the VSK 2 “Simulation Power On” you can trigger a warm restart for the active simulation.

Press the VSK 8 “OK” to confirm or the VSK 7 “Cancel” to abort the warm restart. With a warm start the simulation will be ended and started new. By pressing the VSK 8 “Back” you switch back to the operating area “Program control”.

B600

Page 48


Section 7

NC Execute

Notes:

7.1 NC Execute The function “NC Execute” lets you load the active program from the editor to the operating area “Machine” in the operating mode “AUTO”. 7.1.1

Selecting the function “NC Execute” By pressing the HSK 1.8 “NC Execute” the control, switches to the operating area “Machine” under the operating mode “AUTO”. The program modified in the editor is now ready for machining (see picture below). The Softkey is deactivated if the program is running.


Page 49

B600

Notes:

B600

Page 50


B608

1

Drilling

Brief description

Objective of the module: Working through this module you become familiar with the technology “Drilling” by programming two chained sequential ShopMill programs. Description of the module: This module explains the programming of a simple drilling example with ShopMill functionality, as well as well as the programming of a more complex workpiece by means of chained drilling cycles and position patterns. Content: Simple programming example Complex programming example


Page 1


B608

B608

B608

Page 2


B608 Drilling - Shopmill: Description This module explains the programming of a simple drilling example with ShopMill functionality, as well as well as the programming of a more complex workpiece by means of chained drilling cycles and position patterns.

Drilling Shopmill: START



Drilling Shopmill: END

Notes :


Page 3

B608

Section 2 Notes:

Simple programming example Description: A simple drilling machining, using a drill cycle is to be programmed as a sequential program with ShopMill functionality. Aim: A new sequential ShopMill program is to be created and opened in the editor. The program header, as well as drilling cycle and position cycle (sequential chain program) are programmed. After this the program is to be simulated. For this, the below listed tool and technology data are to be used: Tool data:

Drill Ø 8,5 mm (DRILL_D8.5)

Approach strategy:


2.1 Creating a new sequential program A new ShopMill program can be created from within the operating modes “JOG, “MDA” and “AUTO” as follows: 1.


1.

Press the “MENU SELECT”-key on the operator panel and then the yellow HSK 4 “Program Manager”. The program manager opens.

2.


3.


4.

Press the VSK 3 “ShopMill” to open the input mask for creating a new ShopMill sequential program. Enter a name for the program in the “Name” field and accept with pressing the VSK 8 “OK”. The program is loaded to the “editor” and the parameter window for the program header is opened by default.

B608

Page 4


Section 2


Notes:

2.2 Example: Drilling The following sequential program, with the call up of a simple drilling cycle, chained with a position pattern, is to be programmed.

1.

Create a new ShopMill program like described in the previous section 2.1 and give the program a name, for example “SM_DRILL_1.MPF”. The input window for the program header opens.

2.

Enter following values in the program header like displayed below, and confirm your inputs with by pressing the VSK 8 “Accept”.

The following program block “Program header” will be inserted into the program.


Page 5

B608

Section 2 Notes:


Program the drilling cycle. For this, press the HSK 1.2 Drill.”, to open the technology “Drilling”. Press the VSK 2 “Drilling Reaming”. Press the VSK 3 “Drilling”. The input mask for the drilling cycle opens.

4.

Enter the following parameters like displayed below:

To insert a tool into the parameter window, press the VSK 1 “Select tool”, mark the desired tool (here DRILL_D8.5) in the tool list with the orange selection cursor and press the VSK 8 “OK”. The following program block “Drilling” will be inserted into the program.

5.

Insert now the position pattern for the drilling. Press the VSK 7 “Positions”. Select the VSK 4 “Positions” as a position pattern for the drilling. The input window for the position settings opens.

6.

Enter the following position values into the mask and confirm by pressing the VSK 8 “Accept”.

The program block “Positions” will be inserted into the program:

7.

B608

Program the end of the program and simulate the machining. Place the orange selection cursor on the program block “End of program” and extend the program block by pressing the blue “cursor-to-the-right”-key on the keyboard.

Page 6


Section 2


The settings window for the program end opens, where you can define to repeat the workpiece.

Notes:

Accept the default value by pressing the VSK 8 “Accept”. For starting the simulation, press the VSK 1.7 “Simulation”. The control calculates the simulation parameters and opens the simulation in the simulation window in “Top view”.

To view the simulation in 3-dimensional press the VSK 1.4 “3D view”.


Page 7

B608

Section 3 Notes:

Complex programming example Description: A more complex program (hole pattern) with chained program blocks is to be created in ShopMill. For this, different drilling cycles and a position pattern cycle will be called up and chained to a sequential program. Objective: The following workpiece is to be programmed and simulated. For this, the tool data and technology data shown below shall be used.

The following tool- and technology data are needed for the programming:

B608

Tool data:

Center drill 12 mm (CENTERDRILL_D12) Drill Ø 8,5 mm (DRILL_D8.5) Tap M10 (TAP_M10)

Approach strategy:


Page 8


Section 3


Notes:

3.1 Example: Hole pattern The following program with call of the drilling cycles “Centering”, “Drilling”, “Taping” and a hole pattern is to be programmed.

Create a new ShopMill program, like described in section 2.1 in this module. Give the program a name, for example “SM_DRILL_2.MPF”. The program with the parameter mask for the program header opens automaticlly. 1.

Program the “Program header”, by taking over the following values:

Confirm your inputs by pressing the VSK 8 “Accept”. The following program block “Program header” will be inserted into the program:


Page 9

B608

Section 3 Notes:


Program the center drilling cycle. Press the HSK 1.2 “Drill.”. Press the VSK 1 “Centering”. The parameter mask for the “Centering” opens.

3.

Insert the following values for centering in the parameter input mask, like displayed below.

To insert a tool into the parameter window, press the VSK 1 “Select tool”. Mark the desired tool (CENTERDRILL_D12) in the tool list with the orange selection cursor and press the VSK 8 “OK”. Confirm the input with the VSK 8 “Accept”. The following program block “Centering” will be inserted into the program. The program chain starts (see bracket symbol). 4.

Program the drill cycle. Press the VSK 2 “Drilling Reaming”. Select the VSK 3 “Drilling” to open the input mask for the drilling.

5.

Fill out the input mask like displayed below:

To insert a tool into the parameter window, press the VSK 1 “Select tool”. Mark the desired tool (DRILL_D8.5) in the tool list with the orange selection cursor and press the VSK 8 “OK”. Confirm the input with the VSK 8 “Accept”. The following program block “Drilling” will be inserted into the program. The program chain will be extended.

B608

Page 10


Section 3


Now program the tapping cycle.

Notes:

Press the VSK 5 “Thread”. The “Tapping” window opens. 7.

Insert the following values into the input mask:

To insert a tool into the parameter window, press the VSK 1 “Select tool”. Mark the desired tool (here TAP_M10) in the tool list with the orange selection cursor and press the VSK 8 “OK”. Confirm the input with the VSK 8 “Accept”. The following program block “Tapping” will be inserted into the program. The chaining of the program blocks will be extended. 8.

Program now the position pattern for the drilling, in order to close the program block chain. Press the VSK 7 „Positions“. The positions window opens. To set the positions for the drillings press the VSK 4 “Positions”. The drill position window opens.

9.

Insert following values:

Confirm your inputs by pressing the VSK 8 “Accept”. The following program block “Positions” will be inserted: The program block chain will be closed.


Page 11

B608

Section 3 Notes:


Program the program end and simulate the machining. Place the orange selection cursor on the “End of Program” program block. Extend the program block by pressing the blue “cursor-to-the-right”-key on the keyboard. The input mask for the “End of program” opens.

11.


Accept the default value by pressing the VSK 8 “Accept”. Press the HSK 1.7 “Simulation” to start the simulation of the program. The control calculates the simulation parameters and opens the simulation in the simulation window in “Top view”.

B608

Page 12


Section 3

Complex programming example To view the simulation 3-dimesional press the VSK 1.4 “3D View”.


Page 13

Notes:

B608

Notes:

B608

Page 14


B615

1

Milling

Brief description

Objective of the module: Working through this module you become familiar with the technology “Milling” by programming two chained sequential ShopMill programs. Description of the module: This module explains the programming of a simple milling machining with ShopMill functionality, as well as the programming of a more complex workpiece by means of milling cycles and a position pattern. Content: Simple programming example Complex programming example


Page 1


B615

B615

B615

Page 2


B615 Milling - Shopmill: Description This module explains the programming of a simple milling machining with ShopMill functionality, as well as the programming of a more complex workpiece by means of milling cycles and a position pattern.

Milling Shopmill: START



Milling Shopmill: START END

Notes :


Page 3

B615

Section 2 Notes:

Simple programming example Description: A simple milling machining is to be programmed as a chained sequential program in ShopMill.

Objective: A new ShopMill program is to be created and opened in the editor. The program header, a milling cycle and a position pattern (program chain) are programmed. After this the program is to be simulated. For this, the tool and technology data below are to be used: Tool data:

Milling cutter Ø 10mm (CUTTER_D10)

Technology data:

F 0,15 mm/tooth, V120 m/min

2.1 Creating a new ShopMill program A new ShopMill program can be created from within the operating modes “JOG, “MDA” and “AUTO” as follows: 1.


1.


2.


3.


4.


B615

Page 4


Section 2


Notes:

2.2 Example: Rectangular pocket The following program with a chained milling cycle and position pattern is to be programmed.

1.

Create a new ShopMill program like described in the previous section 2.1 and give the program a name, for example “SM_MILLING_1.MPF”. The input window for the program header opens automatically.

2.

In the parameter mask for the program header enter the following values.

Accept your inputs by pressing the VSK 8 “Accept”. The following program block is inserted into the program:


Page 5

B615

Section 2 Notes:


Program now the rectangular pocket. For this, press the HSK 1.3 “Milling” to open the technology “Milling”. Press the VSK 2 “Pocket”. Press the VSK 3 “Rectang. pocket”. The parameter mask for the rectangular pocket cycle opens.

3.

In the parameter mask for the rectangular pocket enter the following values:

To insert a tool into the parameter window, press the VSK 1 “Select tool”, mark the desired tool (here CUTTER_D10) in the tool list, with the orange selection cursor and press the VSK 8 “OK” Accept your inputs by pressing the VSK 8 “Accept”. The program block “Rectangular pocket” will be inserted into the program. The program chain opens. 4.

Insert now a position pattern for the milling cycle. Press the HSK 1.2 “Drill.”. Press the VSK 7 “Positions”. Select the VSK 4 “Positions” as a position pattern for the milling. The input window for the position settings opens.

B615

Page 6


Section 2


In the parameter mask for the “Position pattern”, enter the following values and confirm your inputs by pressing the VSK 8 “Accept”.

Notes:

The program block “Row of positions” is inserted into the work plan. The program chain closes. 6.

Program now the end of the program and simulate the machining. For this, place the orange selection cursor on the program block “End of program” using the blue cursor keys and switch over to the parameter window by pressing the blue “cursor-to-the-right” key on the keyboard.

7.


Accept the default value and press the VSK 8 “Accept”. In order to start the simulation, press the HSK 1.7 “Simulation”. The control calculates the simulation parameters and opens the simulation in the simulation window in “Top view”.


Page 7

B615

Section 2


Notes:


B615

Page 8


Section 3


Notes:

Description: A more complex program (a slanted rectangular pocket) with chained program blocks is to be created in ShopMill.

Objective: The workpiece shown below is to be programmed and simulated. For this, the tool and technology data below are to be used:

The following tool- and technology data are needed for the programming: Tool data:

Milling tool Ø 10 mm (CUTTER_D10)

Technology data:

F 0,15 mm/tooth, V 120 m/min (roughing) and F 0,08 mm/tooth, V 150 m/min (finishing) The pocket is to be roughed first and finished afterwards.


Page 9

B615

Section 3 Notes:

Complex programming example 3.1 Example: Slanted rectangular pocket The following program, with the call up of rectangular pocket cycles and a position pattern, is to be programmed.

Create a new ShopMill program first, like described in Section 2.1 in this module. Name the program, e. g. “SM_MILLING_2.MPF”. The new ShopMill program, with the parameter window for the program header opens. 1.

Program the program header like displayed below:

Confirm your inputs by pressing the VSK 8 “Accept”. The following program block will be inserted into the program.

B615

Page 10


Section 3


Rough the rectangular pocket.

Notes:

Press the HSK 1.3 “Mill.” to open the technology “Milling”. Press the VSK 2 “Pocket”. Press the VSK 3 “Recttang. pocket”. The input mask for the rectangular pocket cycle opens. 3.

Insert the following values and confirm your inputs by pressing the VSK 8 “Accept”.

: To insert a tool into the program, press the VSK 1 “Select tool”, in the opening tool list, select the tool “CUTTER_D10” with the orange selection cursor and press the VSK 8 “OK”. Confirm your inputs by pressing the VSK 8 “Accept”. The program block “Rectang. Pocket” is inserted into the program: The program chain starts (see chain symbol). 4.

After this finish the rectangular pocket. Press the VSK 2 “Pocket”. Press the VSK 3 “Rectang. pocket”. The parameter mask for the rectangular pocket cycle opens.


Page 11

B615

Section 3 Notes:


Insert the following values into the parameter mask and confirm your inputs by pressing the VSK 8 “Accept”:

To insert a tool into the program, press the VSK 1 “Select tool”, in the opening tool list, select the tool “CUTTER_D10” with the orange selection cursor and press the VSK 8 “OK”. Confirm your inputs by pressing the VSK 8 “Accept”. The program block “Rectang. Pocket” is inserted into the program: The program chain is extended (see chain symbol). 6.

Insert now a position pattern for the rectangular pocket. Press the HSK 1.2 “Drill.”. Press the VSK 7 “Positions“. The window for setting a position patterns for the rectangular pocket opens. Press the VSK 4 “Position pattern” to open the position pattern input mask for the pocket positions.

B615

Page 12


Section 3


Enter the following values into the parameter window:

Notes:

Confirm your inputs by pressing the VSK 8 “Accept”. The program block “Row of positions” is inserted into the program: The program chain closes. 8.

Program now the program end and simulate the machining. Place the orange selection cursor on the program block “Program end” and open the parameter list by pressing the blue “cursor-to-the-right”-key on the keyboard. The input mask for the “End of program” settings opens.

9.

Here you can define to repeat the program for multiple workpieces.

Take over the default value and press the VSK 8 “Accept”. Press the HSK 1.7 “Simulation” to start the simulation of the program run. The control calculates the simulation parameters and opens the simulation in the simulation window in “Top view”.


Page 13

B615

Section 3


Notes:

To view the simulation 3-dimensional, press the VSK 1.4 “3D view”.

B615

Page 14


B623

1

Contour milling

Brief description

Objective of the module: Working with this module you become familiar with the technology “Contour milling” by programming two chained sequential ShopMill programs Description of the module: This module explains the programming of a simple and a more complex contour in ShopMill, with the technology contour milling and with help of the contour editor. Content: Simple programming example Complex programming example


Page 1


B623

B623

B623

Page 2


B623 Contour milling - Shopmill: Description This module explains the programming of a simple and a more complex contour in ShopMill, with the technology contour milling and with help of the contour editor.

Contour milling Shopmill: START



Contour milling Shopmill: END

Notes :


Page 3

B623

Section 2 Notes:

Simple programming example Description: A simple contour milling operation is to be programmed as a chained sequential program in ShopMill. Objective: A new ShopMill program is to be created and opened in the editor. The program header, a contour description and a contour milling cycle (as chain program) are to be programmed. Afterwards, the program is to be simulated. For this, the tool and technology data below are to be used: Tool data:


Technology data:

F 0,3 mm/tooth, V120m/min

2.1 Creating a new ShopMill program A new ShopMill program can be created from within the operating modes “JOG, “MDA” and “AUTO” as follows: 1.


1.


2.


3.


4.


B623

Page 4


Section 2


Notes:

2.2 Programming example: Straight line The following ShopMill program with a contour description and a contour milling cycle, chained together, is to be programmed.

1.

Create a new ShopMill sequential program like described in the previous section 2.1 and give the program for example the name “SM_CONTOURMILLING_1.MPF”. The input window for the program header opens automatically.

2.

Insert the following parameter values. Use the blue “Select”-key on the MCP where indicated.

Accept your inputs by pressing the VSK 8 “Accept”. 828D/840Dsl SINUMERIK Operate

Page 5

B623

Section 2


Notes:

The following program block is inserted into the program:

3.

Start with the programming of a contour path for the contour milling machining. For this, press the HSK 1.4 “Cont. mill.” to open the technology “Contour milling”. Press the VSK 1 “New contour”. A parameter mask where you can insert a new name for the new contour opens.

4.

Enter a name for the new contour, e.g. “PATH”,

Confirm your input by pressing the VSK 8 “Accept”. The contour editor opens automatically and the parameter mask for entering a start point for the contour is active by default. 5.

Insert the following coordinates for the starting point:

Confirm your inputs by pressing the VSK 8 “Accept”. The contour description begins and new functions for defining a contour are available as yellow vertical softkeys on the right side of the screen. 6.

Extend the contour path by adding a straight line in Y-direction. Press the VSK 3 “Straight line Y”. The parameter mask where you can define a straight line in Y direction opens. Enter following coordinates into the parameter mask:

B623

Page 6


Section 2

Simple programming example Confirm your inputs by pressing the VSK 8 “Accept”.

Notes:

The contour path will be extended with a straight line in Y-direction. Note: In the input field “Y” you can switch between “inc” and “abs” by pressing the blue “SELECT”-key on the keyboard. 7.

Now, check the programmed contour. For this, place the orange selection cursor on the -symbol in the yellow column on the left side of the screen, by using the blue cursor keys on the keyboard. The contour path is displayed graphically.

Note: In the white column on the left side of the screen you see all the program blocks programmed so far as symbols (representing the technology) and in the yellow column you see the symbols of all the programmed contour elements. 8.

Finish now the contour description by pressing the VSK 8 “Accept”. The program editor opens and the following program block is inserted into the program: The program chain opens.


Page 7

B623

Section 2 Notes:


Program now the contour milling cycle. Press the HSK 1.4 “Cont. Mill.” to open the technology “Contour milling”. Press the VSK 1.2 “Path milling” to select the function “Path milling”. The parameter mask for the path milling cycle opens.

10.

Insert the following parameter values. Use the blue “Select” key on the MCP where indicated.

Note: In the input field “F” you can switch between “mm/tooth” or “mm/min” . The input field for Speed can either be “V” in “m/min” or “S” in “rev/min” by pressing the blue “SELECT”-key on the keyboard. To insert a tool into the cycle input mask, press the VSK 1 “Select tool”. The “Tool list” window opens. Use the blue cursor keys on the keyboard, to mark the tool “CUTTER_D32”, with the orange selection cursor. Press the VSK 1.8 “OK”. The tool “CUTTER_D32" will be inserted into the cycle input mask. Confirm your inputs by pressing the VSK 8 “Accept”. The following program block will be inserted into the program. The program chain closes. 11.

End the programming by placing the orange selection cursor on the program block “End of program” and switch to the parameter mask by pressing the blue “cursor-to-the-right”-key on the keyboard.

B623

Page 8


Section 2

Simple programming example The setting window for the program end opens, where you can define to repeat the program for multiple workpieces.

Notes:

Accept the default value “No” and press the VSK 8 “Accept”. 12.

Simulate now the program to verify tool path. Press the HSK 1.7 “Simulation” to start the simulation. The control calculates the simulation and opens the simulation window in a “Top view” on the workpiece.

To view the simulation 3-dimensional, press the VSK 1.4 “3D view”.


Page 9

B623

Section 3 Notes:

Complex programming example Description: A more complex program (moulding plate) with chained program blocks is to be created in ShopMill with the technology “Contour milling”. Objectives: Following workpiece is to be programmed and simulated.

20

5

A-A

100

40

20

R30

35

50

R15

150

A

90

R36

A R5

60 70

The following Tool & technology data are needed in the program: Tool & technology data:

Operations list:

B623

Milling cutter Ø 32 mm (CUTTER_D32) F 0,30 mm/tooth, V 120 m/min (roughing) F 0,15 mm/tooth, V 150 m/min (finishing) Milling cutter Ø 16 mm (CUTTER_D16) F 0,15 mm/tooth, V 120 m/min (roughing) Milling cutter Ø 8.0 mm (CUTTER_D8) F 0,10 mm/tooth, V 120 m/min (roughing) F 0,05 mm/tooth, V 150m/min (finishing) 1. 2. 3. 4. 5. Page 10

Outer contour roughing + finishing Spigot contour roughing + finishing Contour pocket roughing Contour pocket rest material roughing Contour pocket wall + base finishing 828D/840Dsl SINUMERIK Operate

Section 3

Complex programming example 3.1 Programming example: Moulding plate

Notes:

The following program is to be programmed with the technology “Contour milling”.

1.

Create a new ShopMill program like described in section 2.1 in this module with the name “SM_CONTOURMILLING_2.MPF”. The program with the parameter mask for the program header opens automatically.

2.

Insert following values for the program header. Use the “Select” key on the MCP where indicated.

Confirm your inputs by pressing the VSK 8 “Accept”. The following program block is inserted into the program:


Page 11

B623

Section 3 Notes:


Start programming the contour description for the “Moulding plate outside” with help of the contour editor. Press the HSK 1.4 “Cont. mill.”, to open the technology “Contour milling”. Press the VSK 1 “New contour”. A parameter mask where you can enter a name for the new contour opens.

4.

Enter a name for the new contour, e.g. “MOULDINGPLATE_OUTSIDE”,

Confirm your input by pressing the VSK 8 “Accept”. The contour editor opens automatically and the parameter mask for entering a start point for the contour is active by default.

5.

Enter the following coordinates for the starting point:

Confirm your input by pressing the VSK 8 “Accept”. The contour description starts and new functions for defining a contour are available as yellow vertical softkeys on the right side of the screen. 6.

Extend the contour description by adding a straight line in Y-direction. Press the VSK 3 “Straight line Y”. The input window for the “Straight line Y” opens.

B623

Page 12


Section 3

Complex programming example Enter following values into the parameter mask:

Notes:

Confirm your input by pressing the VSK 8 “Accept”. A straight line in Y-direction is added to your contour description. 7.

Extend the contour description by adding a straight line in X-direction. Press the VSK 2 “Straight line X”. The input window for the “Straight line X” opens. Enter the following values into the parameter mask:

Confirm your input by pressing the VSK 8 “Accept”. A straight line in X-direction is added to your contour description. 8.

Now finish the programming of the contour path by adding a straight line in Y-direction. Press the VSK 3 “Straight line Y”. The input window for the straight line in Y-direction opens. Enter the following values into the parameter mask:

Confirm your inputs by pressing the VSK 8 “Accept”. The contour description is finished. 828D/840Dsl SINUMERIK Operate

Page 13

B623

Section 3


Notes: 9.

Now, check the outline of the contour path. For this, place the orange selection cursor on the -symbol in the yellow column on the left side of the screen, by using the blue cursor keys on the keyboard. The contour is displayed graphically.

Note: The white column on the left side of the help screen shows all the program blocks programmed as symbols (representing the technology). The yellow column next to it shows all the programmed contour elements as symbols. 10. Finish now the programming of the contour by pressing the VSK 8 “Accept”. The program editor opens and the following program block is inserted into the program: The program chain opens.

B623

Page 14


Section 3


Insert now a “path milling” cycle into the program for “roughing” the moulding plate.

Notes:

Press the HSK 1.4 “Cont. mill.” to open the technology “Contour milling”. Press the VSK 1.2 “Path milling”. The input window for the path milling cycle opens. 12.


Note: In the input field “F” you can switch between “mm/tooth” or “mm/min” . The input field for Speed can either be set to cutting speed “V” in “m/min” or Spindle speed “S” in “rpm”. The machining depth “Z1” can be “inc” or “abs”. To insert a tool into the cycle input mask, press the VSK 1 “Select tool”. The “Tool list” window opens. Use the blue cursor keys on the keyboard, to mark the tool “CUTTER_D32”, with the orange selection cursor. Press the VSK 1.8 “OK”. The tool “CUTTER_D32" will be inserted into the cycle input mask. Confirm your inputs by pressing the VSK 8 “Accept”. The following program block will be added to the program chain. The program chain closes.


Page 15

B623

Section 3 Notes:


Extend now the program chain by inserting another “path milling” cycle for “finishing” the outside. Press the VSK 1.2 “Path milling”. The input window for the path milling cycle opens.

14.


Note: In the input field “F” you can switch between “mm/tooth” or “mm/min” . The input field for Speed can either be set to cutting speed “V” in “m/min” or Spindle speed “S” in “rpm”. The machining depth “Z1” can be “inc” or “abs”. To insert a tool into the cycle input mask, press the VSK 1 “Select tool”. The “Tool list” window opens. Use the blue cursor keys on the keyboard, to mark the tool “CUTTER_D32”, with the orange selection cursor. Press the VSK 1.8 “OK”. The tool “CUTTER_D32" will be inserted into the cycle input mask. Confirm your inputs by pressing the VSK 8 “Accept”. The following program block will be added to the program chain. The program chain is now complete and closed.

B623

Page 16


Section 3


Start programming the contour description for the “Spigot boundary” with help of the contour editor.

Notes:

Press the VSK 1 “New contour”. A parameter mask where you can enter a name for the new contour opens. 16.

Enter a name for the new contour, e.g. “SPIGOT_BOUNDARY”.


17.


Confirm your inputs by pressing the VSK 8 “Accept”. The contour description starts and new functions for defining a contour are available as yellow vertical softkeys on the right side of the screen. 18.

Enter the first contour element by adding a straight line in Y-direction. Press the VSK 3 “Straight line Y”. The input window for the “Straight line Y” opens.


Page 17

B623

Section 3


Notes:

Enter following coordinates into the parameter mask:

Confirm your inputs by pressing the VSK 8 “Accept”. A straight line in Y-direction is added to your contour description. 19.

Extend the contour description by adding a straight line in X-direction. Press the VSK 2 “Straight line X”. The input window for the “Straight line X” opens. Enter following coordinates into the parameter mask:

Confirm your inputs by pressing the VSK 8 “Accept”. A straight line in X-direction is added to your contour description. 20.

Extend the contour description by adding a straight line in Y-direction. Press the VSK 3 “Straight line Y”. The input window for the straight line in Y-direction opens. Enter following coordinates into the parameter mask:

Confirm your inputs by pressing the VSK 8 “Accept”. A straight line in Y-direction is added to your contour description. 21.

Now finish the contour description by adding a straight line in X-direction. Press the VSK 2 “Straight line X”. The input window for the straight line in Y-direction opens.

B623

Page 18


Section 3

Complex programming example Enter following coordinates into the parameter mask:

Notes:

Confirm your inputs by pressing the VSK 8 “Accept”. The contour description of the “Spigot Boundary” is finished. 22.


Note: The white column on the left side of the help screen shows all the program blocks programmed as symbols (representing the technology). The yellow column next to it shows all the programmed contour elements as symbols. 23. Finish now the contour description by pressing the VSK 8 “Accept”. The program editor opens again and the following program block is inserted into the program:

The program chain opens. 828D/840Dsl SINUMERIK Operate

Page 19

B623

Section 3 Notes:


Start programming the contour description for the “Spigot” with help of the contour editor. Press the VSK 1 “New contour”. A parameter mask where you can enter a name for the new contour opens.

25.

Enter a name for the new contour, e.g. “SPIGOT”,


26.


Press the VSK 8 “Accept” to confirm your updates. The contour description starts and new functions for defining a contour are available as yellow vertical softkeys on the right side of the screen. 27.

Start the contour description with a circle in clockwise direction. Press the VSK 1.5 “Circle”. The input window for the “Circle” opens.

B623

Page 20


Section 3


Notes:

Confirm your input by pressing the VSK 8 “Accept”. A circle in clockwise direction is added to your contour description. 28.

Extend the contour description by adding a straight line in Y-direction. Press the VSK 3 “Straight line Y”. The input window for the “Straight line Y” opens. Enter following coordinates into the parameter mask:

Confirm your input by pressing the VSK 8 “Accept”. A straight line in Y-direction is added to your contour description. 29.

Extend the contour description by adding a circle in clockwise direction. Press the VSK 5 “Circle”. The input window for the “Circle” opens.


Page 21

B623

Section 3


Notes:

Enter following coordinates into the parameter mask:

Confirm the VSK 8 “Accept”. A circle in clockwise direction is added to your contour description. 30.

Extend the contour description by adding a straight line in Y-direction. Press the VSK 1.3 “Straight line Y”. The input window for the “Straight line Y” opens. Enter following coordinates into the parameter mask:

Confirm the VSK 8 “Accept”. A straight line in Y-direction is added to your contour description. 31.

Now finish the contour description by adding a circle in clockwise direction. Press the VSK 5 “Circle”. The input window for the circle opens.

B623

Page 22


Section 3


Notes:

Confirm your inputs by pressing the VSK 8 “Accept”. The contour description of the “Spigot” is finished. 32.


33.

Finish now the programming of the contour by pressing the VSK 8 “Accept”. The program editor opens and the following program block is inserted into the program:

The program chain remains open. 828D/840Dsl SINUMERIK Operate

Page 23

B623

Section 3 Notes:


Insert now a “spigot milling” cycle into the program for “roughing” the spigot contour within the defined boundary area. Press the VSK 1.6 “Spigot”. The input window for the spigot milling cycle opens.

35.

Insert the following parameter values. Use the blue “Select” key on the MCP where indicated. .

Note: In the input field “F” you can switch between “mm/tooth” or “mm/min” . The input field for Speed can either be set to cutting speed “V” in “m/min” or Spindle speed “S” in “rpm”. The machining depth “Z1” can be “inc” or “abs”. The tool path step over “DXY” can be set to % of tool Ø or a value in mm of the tool Ø. To insert a tool into the cycle input mask, press the VSK 1 “Select tool”. The “Tool list” window opens. Use the blue cursor keys on the keyboard, to mark the tool “CUTTER_D32”, with the orange selection cursor. Press the VSK 1.8 “OK”. The tool “CUTTER_D32" will be inserted into the cycle input mask. Confirm your inputs by pressing the VSK 8 “Accept”. The following program block will be added to the program chain. The program chain closes.

B623

Page 24


Section 3


Extend the program chain by inserting another “spigot milling” cycle into the program for “finishing” the spigot “Wall”.

Notes:

Press the VSK 1.6 “Spigot”. The input window for the spigot milling cycle opens. 37.


Note: In the input field “F” you can switch between “mm/tooth” or “mm/min” . The input field for Speed can either be set to cutting speed “V” in “m/min” or Spindle speed “S” in “rpm”. The machining depth “Z1” can be “inc” or “abs”. To insert a tool into the cycle input mask, press the VSK 1 “Select tool”. The “Tool list” window opens. Use the blue cursor keys on the keyboard, to mark the tool “CUTTER_D32”, with the orange selection cursor. Press the VSK 1.8 “OK”. The tool “CUTTER_D32" will be inserted into the cycle input mask. Confirm your inputs by pressing the VSK 8 “Accept”. The following program block will be added to the program chain.

The program chain is now complete and closed.


Page 25

B623

Section 3 Notes:


Start programming the contour description for the “Moulding plate pocket” with help of the contour editor. Press the VSK 1 “New contour”. A parameter mask where you can enter a name for the new contour opens. Enter a name for the new contour, e.g. “MOULDINGPLATE_POCKET”.


39.


Press the VSK 8 “Accept” to confirm your inputs. The contour description starts and new functions for defining a contour are available as yellow vertical softkeys on the right side of the screen.

B623

Page 26


Section 3


Begin the contour description by adding a straight line in X-direction.

Notes:

Press the VSK 1.2 “Straight line X”. The input window for the “Straight line X” opens. Insert the following values into the parameter mask.

Press the VSK 8 “Accept” to confirm your inputs. The first Kontur element is generated and a straight line in X-direction is added to your contour description. 41.

Extend the contour description by adding a straight line in Y-direction. Press the VSK 3 “Straight line Y”. The input window for the “Straight line X” opens. Insert the following values into the parameter mask.

Press the VSK 8 “Accept” to confirm your inputs. A straight line in Y-direction is added to your contour description. 42.

Extend the contour description by adding a circle in clockwise direction. Press the VSK 5 “Circle”. The input window for the “Circle” opens.


Page 27

B623

Section 3


Notes: Enter following coordinates into the parameter mask:

Confirm the VSK 8 “Accept”. A circle in clockwise direction is added to your contour description. 43.

Extend the contour description by adding a straight line in Y-direction. Press the VSK 3 “Straight line Y”. The input window for the “Straight line Y” opens. Insert the following values into the parameter mask.

Confirm the VSK 8 “Accept”. A straight line in Y-direction is added to your contour description. 44.

Now finish the programming of the contour path by adding a straight line in X-direction. Press the VSK 2 “Straight line X”. The input window for the “straight line Y” opens. Enter following coordinates into the parameter mask:

Confirm your inputs by pressing the VSK 8 “Accept”. The contour description is now closed by a straight line in Y-direction and therefore finished.

B623

Page 28


Section 3


Now, check the outline of the contour path.

Notes:

For this, place the orange selection cursor on the -symbol in the yellow column on the left side of the screen, by using the blue cursor keys on the keyboard. The contour is displayed graphically.

Note: The white column on the left side of the help screen shows all the program blocks programmed as symbols (representing the technology). The yellow column next to it shows all the programmed contour elements as symbols. 46. Finish now the programming of the contour by pressing the VSK 8 “Accept”. The program editor opens and the following program block is inserted into the program:

The program chain opens.


Page 29

B623

Section 3 Notes:


Insert now a “pocket milling” cycle into the program for “roughing” the moulding plate pocket. Press the VSK 1.4 “Pocket”. The input window for the pocket milling cycle opens.

48.


Note: In the input field “F” you can switch between “mm/tooth” or “mm/min” . The input field for Speed can either be set to cutting speed “V” in “m/min” or Spindle speed “S” in “rpm”. The machining depth “Z1” can be “inc” or “abs”. The tool path step over “DXY” can be set to “%” of tool Ø or a value in “mm” . To insert a tool into the cycle input mask, press the VSK 1 “Select tool”. The “Tool list” window opens. Use the blue cursor keys on the keyboard, to mark the tool “CUTTER_D16”, with the orange selection cursor. Press the VSK 1.8 “OK”. The tool “CUTTER_D16" will be inserted into the cycle input mask. Confirm your inputs by pressing the VSK 8 “Accept”. The following program block will be added to the program chain. The program chain closes.

B623

Page 30


Section 3


Extend the program chain by inserting a “Pocket residual material” cycle for “roughing” of the residual material of the moulding plate pocket.

Notes:

Press the VSK 1.5 “Pocket resid. mat.”. The input window for the pocket residual material cycle opens. 50.


Note: In the input field “F” you can switch between “mm/tooth” or “mm/min” . The input field for Speed can either be set to cutting speed “V” in “m/min” or Spindle speed “S” in “rpm”. The tool path step over “DXY” can be set to “%” of tool Ø or a value in “mm” . To insert a tool into the cycle input mask, press the VSK 1 “Select tool”. The “Tool list” window opens. Use the blue cursor keys on the keyboard, to mark the tool “CUTTER_D8”, with the orange selection cursor. Press the VSK 1.8 “OK”. The tool “CUTTER_D8" will be inserted into the cycle input mask. Confirm your inputs by pressing the VSK 8 “Accept”. The following program block will be added to the program chain. The program chain is closed.


Page 31

B623

Section 3 Notes:


Extend the program chain by inserting another “Pocket milling” cycle for “finishing” the “base” of the moulding plate pocket. Press the VSK 1.4 “Pocket”. The input window for the pocket milling cycle opens.

50.


Note: In the input field “F” you can switch between “mm/tooth” or “mm/min” . The input field for Speed can either be set to cutting speed “V” in “m/min” or Spindle speed “S” in “rpm”. The machining depth “Z1” can be “inc” or “abs”. The tool path step over “DXY” can be set to “%” of tool Ø or a value in “mm” of the tool Ø. To insert a tool into the cycle input mask, press the VSK 1 “Select tool”. The “Tool list” window opens. Use the blue cursor keys on the keyboard, to mark the tool “CUTTER_D8”, with the orange selection cursor. Press the VSK 1.8 “OK”. The tool “CUTTER_D8" will be inserted into the cycle input mask. Confirm your inputs by pressing the VSK 8 “Accept”. The following program block will be added to the program chain. The program chain is closed.

B623

Page 32


Section 3


Insert another “Pocket milling” cycle into the program for “finishing” the “base” of the moulding plate pocket.

Notes:

Press the VSK 1.4 “Pocket”. The input window for the pocket milling cycle opens. 52.


Note: In the input field “F” you can switch between “mm/tooth” or “mm/min” . The input field for Speed can either be set to cutting speed “V” in “m/min” or Spindle speed “S” in “rpm”. The machining depth “Z1” can be “inc” or “abs”. To insert a tool into the cycle input mask, press the VSK 1 “Select tool”. The “Tool list” window opens. Use the blue cursor keys on the keyboard, to mark the tool “CUTTER_D8”, with the orange selection cursor. Press the VSK 1.8 “OK”. The tool “CUTTER_D8" will be inserted into the cycle input mask. Confirm your inputs by pressing the VSK 8 “Accept”. The following program block will be inserted into the program. The program chain is now finished and closed.


Page 33

B623

Section 3 Notes:


End the programming by placing the orange selection cursor on the program block “End of program” and switch to the parameter mask by pressing the blue “cursor-to-the-right”-key on the keyboard. The parameter mask for the program end opens, where you can define to repeat the program for multiple workpieces.

Accept the default value “No” and press the VSK 8 “Accept”. The program is now completed and ready for simulation.

B623

Page 34


Section 3


Simulate now the program to verify tool path.

Notes:

Press the HSK 1.7 “Simulation” to start the simulation. The control calculates the simulation and opens the simulation window in a “Top view” on the workpiece.

Press the VSK 1.4 “3D view“ to run the simulation in a 3-dimensional view.


Page 35

B623

Section 3 Notes:

Complex programming example Press the blue highlighted HSK 1.7 “Simulation" to return to the ShopMill chain program. After completion of the workpiece Simulation, the Total machining time is being displayed behind the „End of program“ program block

Note: The total time represents approximately the real time of machining. Tool change time and rapid traverse movements are being taken into consideration based on the values in the machine data.

B623

Page 36


B639

1

Straight Circle

Brief description

Objective of the module: Working with this module you become familiar with the technology “Straight Circle” in ShopMill with the programming of two sequential ShopMill programs. Description of the module: This module explains the programming of a simple program using the straight circle technology in ShopTurn, as well as well as the programming of a more complex workpiece by means of chained straight circle cycles.


840D/828D SINUMERIK Operate 840D/828D SINUMERIK Operate

Page 1


B639

B639

B639

Page 2


B639 Straight - Circle: Description

Straight Circle: START

This module explains the programming of a simple program using the straight circle technology in ShopTurn, as well as well as the programming of a more complex workpiece by means of chained straight circle cycles.



Straight Circle: END

Notes :


Page 3

B639

Section 2 Notes:

Simple programming example Description: A simple straight circle machining is to be programmed with ShopMill functionality.

Objective: A new sequential program is to be created and opened in the editor. The program header, a Straight line and circle and the program end are to be programmed. Afterwards the program is to be simulated. For this the following tool- and technology data are to be used: Tool data:

Cutter Ø 20 mm (CUTTER_D20)

Technology data:

Constant cutting speed V 80 m/min

2.1 Creating a new sequential program A new ShopMill program can be created from within the operating modes “JOG, “MDA” and “AUTO” as follows: 1.


1.

Press the “MENU SELECT”-key on the operator panel. Press the yellow HSK 1.4 “Program manager”. The program manager window opens.

2.


3.


4.

Press the VSK 3 “ShopMill” to open the input mask for creating a new ShopMill sequential program. Enter a name for the program and accept with pressing the VSK 8 “OK”. The program is loaded to the editor and the parameter window for the program header is opened by default.

B639

Page 4

840D/828D SINUMERIK Operate

Section 2


Notes:

2.2 Example: Straight The following ShopMill program is to be programmed:

1.

Create a new ShopMill program, as described in section 2.1 and enter a new program name e.g. “SM_STRAIGHT_CIRCLE_1.MPF” The input mask for the program header is opened by default.

2.

Enter following values for the program header and confirm with the VSK 8 “Accept”:

The following program block is inserted into the work plan:


Page 5

B639

Section 2 Notes:


Program now the tool. For this, extend the horizontal softkey bar by pressing the “Extend”-key on the operator panel. The horizontal softkey bar 2 opens Press the HSK 2.2 “Strght Circle” to open the function “Straight Circle” with the corresponding vertical softkeys . Press now the VSK 1 “Tool”. The input mask for the tool parameters opens.

4.

Enter following values into the input mask:

To insert a tool into the parameter window, press the VSK 1 “Select tool”, mark the desired tool (here CUTTER_D20) in the tool list with the orange selection cursor and press the VSK 1.8 “OK”. The following program block will be inserted into the work plan.

5.

Insert a straight line for positioning to the starting point of the milling operation. Press the VSK 2 “Straight”. The input mask for the straight parameters opens.

6.

Enter the following values for approaching the workpiece in a straight line into the input mask:

Press the VSK 5 “Rapid traverse” in order to position to the starting point in rapid traverse. 7.

Press the VSK 8 “Accept” to confirm your input. The following program block is inserted into the work plan:

B639

Page 6


Section 2


Insert a work step to approach the target position Z in a straight line.

Notes:

Press the VSK 2 “Straight” The window for the straight parameters opens. 9.

Enter the following values into the input mask:

Press the VSK 5 “Rapid traverse” in order to approach the target position Z in rapid traverse. 10.


11.

As next work step insert a straight line in Y-direction Press the VSK 2 “Straight”. The input mask for the straight line opens.

12.


13.


14.

As next work step insert a straight line in Z-direction, to retract the tool. Press the VSK 2 “Straight”. The input mask for the parameter values for the straight opens.


Page 7

B639

Section 2 Notes:



Press the VSK 5 “Rapid traverse” to execute the movement in rapid traverse.

16.


17.

Program the end of the program and simulate the machining. Place the orange selection cursor on the program block “End of program” and extend the program block by pressing the blue “cursor-to-the-right”-key on the keyboard. The input mask for the end of program opens. Leave the parameter “Repetition” on “No”, as shown below.

Accept the default value by pressing the VSK 8 “Accept”. In order to start the simulation, extend the horizontal softkey bar by pressing the “Extend”-key on the operator panel. The horizontal softkey bar 1 opens Press the HSK 1.7 “Simulation” to start the simulation of the program. The control calculates the simulation parameters and opens the simulation in the simulation window in “Top view”.

B639

Page 8


Section 2


Notes:



Page 9

B639

Section 3 Notes:

Complex programming example Description: A more complex program (die plate) is to be programmed, by using the technology “Straight Circle”.

Aim: The workpiece shown in the graphic below is to be programmed. Afterwards the program is to be simulated.

The following tool and technology data are used for the programming. Tool data: :

Cutter Ø 20 mm (CUTTER_D20)

Technology data: :

Constant cutting speed V 80 m/min As starting point for the machining the following position is specified: X - 12 Y

- 12

Z

-5

This point is approached in rapid traverse. The contour starting point (X5 and Y5) is approached in a straight line (F 100 mm/min, cutter radius compensation left).

B639

Page 10


Section 3


Notes:

3.1 Programming example: die plate The following ShopMill program is to be created.

1.

Create a new ShopMill program like described in section 2.1 in this module. Give the program the following name: “SM_STRAIGHT_CIRCLE_2.MPF“. The program, with the input mask for the program header opens by default.

2.

Enter the following values into the program header:


Page 11

B639

Section 3 Notes:


Confirm your inputs by pressing the VSK 8 „Accept“. The following program block is inserted into the work plan:

4.

Inset now a tool (CUTTER_D20) into the program. In order to do this, switch to the horizontal softkey bar 2, by pressing the “Extend”-key on the operator panel. The horizontal softkey bar 2 opens. Press the HSK 2.2 “Strght Circle” to select the function “Straight Circle”. The operating area of the function “Straight Circle” opens. Now press the VSK 1 “Tool” to open the input mask for the tool (see picture below).

To insert a tool into the parameter mask, press the VSK 1 “Select tool”. Select the The tool list window opens. Here, place the orange selection cursor on the tool “CUTTER_D20”, by using the blue cursor keys on the keyboard and press the VSK 1.8 “OK”. The selected tool is inserted into the tool input mask like displayed below 5.

Fill out the rest of the input mask, as follows:

Confirm your inputs by pressing the VSK 8 “Accept”. The following program block is inserted into the work plan:

B639

Page 12


Section 3


Position now the tool to the starting position of the machining operation in a straight line.

Notes:

Press the VSK 2 “Straight” to open the input mask for the function “Straight”. 7.

Insert the following values into input mask:

Press the VSK 5 “Rapid traverse” in order to position to the starting point in rapid traverse. Confirm your inputs by pressing the VSK 8 “Accept”. The following program block is inserted into the program:

8.

Insert now another straight move into the program. Press the VSK 2 “Straight” to open the input mask for the function “Straight”.

9.


Press the VSK 5 “Rapid traverse”, in order to move to the Z depth in rapid traverse. Confirm your inputs by pressing the VSK 8 “Accept”. The following program block is inserted into the program:

10.

Insert now another Straight move into the program. Press the VSK 2 “Straight” to open the input mask for the function “Straight”.


Page 13

B639

Section 3 Notes:


Insert the following values into the parameter window:


12.

Define now the reference point of the polar coordinate system (pole) for the technology “Straight circle”. Press the VSK 6 „Polar“ to open the input window for the function “Polar”. Press the VSK 2 „Pole“ to open the input mask for the function “Pole”.

13.

Define the pole as follows:


14.

Insert now a “Straight polar” move into the program. Press the VSK 6 „Polar“ to open the input window for the function “Polar”. Press the VSK 3 “Straight polar“ to open the input mask for the function “Straight polar”.

15.

Enter the values as follows:


B639

Page 14


Section 3


Insert another “Circle polar” move into the program.

Notes:

Press the VSK 6 „Polar“ to open the operating area for the function „Polar“. Press the VSK 4 „Circle polar“, the input mask for the circle polar opens. 17.

Enter the values into the input window like displayed below:


18.

Insert now a straight machining movement. Press the VSK 2 „Straight“ to open the input window.

19.

Enter the values into the input window like displayed below:


20.

Define now a second reference point of the polar coordinate system (pole) for the technology “Straight circle”. Press the VSK 6 „Polar“ to open the input mask for the function „Polar“. Press the VSK 2 „Pole” to open the input mask for the function „Pole“.


Page 15

B639

Section 3 Notes:


Enter the values into the input mask as displayed below:


22.

Insert another „Circle polar“ move into the program. Press the VSK 6 „Polar“ to open the operating area for the function „Polar“. Press the VSK 4 „Circle polar“, to open the input mask for “Circle polar”.

23.



24.

Insert now a straight machining movement. Press the VSK 2 „Straight“ to open the input window.

25.



B639

Page 16


Section 3


Insert another “Straight” machining movement into the program.

Notes:

Press the VSK 2 „Straight“ to open the input mask for the function “Straight”. 27.



28.

Insert the final straight machining movement into the program. Press the VSK 2 „Straight“ to open the input window.

29.



30.

Program the end of the program and simulate the machining. Place the orange selection cursor on the program block “End of program” and extend the program block by pressing the blue “cursor-to-the-right”-key on the keyboard.


Page 17

B639

Section 3


Notes:

The input mask for the program end opens. Leave the parameter “Repetition” on “No” as shown below.

Accept the default value by pressing the VSK 8 “Accept”. 31.

To run the simulation go back to the horizontal softkey bar 1. Extend the horizontal softkey bar by pressing the “Extend”-key on the operator panel. The horizontal softkey bar 1 opens. Press the HSK 1.7 “Simulation” to start the simulation of the program. The control calculates the simulation parameters and opens the simulation in the simulation window in “Top view”.

B639

Page 18


Section 3

Complex programming example To view the simulation 3-dimensional press the VSK 1.4 “3D view”.


Page 19

Notes:

B639

Section End Notes:

B639

Page 20


B655

1

Measurement Milling ShopMill

Brief description

Objective of the module: Working with this module you become familiar with the technology “Measurement milling” by programming two sequential ShopMill programs. Description of the module: This module explains the programming of a simple and a complex measuring process of the workpiece with the function “Measurement milling” in ShopMill.



Page 1


B655

B655

B655

Page 2


B655 Measure milling - Shopmill: Description This module explains the programming of a simple and a complex measuring process of the workpiece with the function “Measurement milling” in ShopMill.

Measure milling Shopmill: START



Measure milling Shopmill: END

Notes :


Page 3

B655

Section 2 Notes:

Simple programming example Description: A simple measuring movement with a 3d-probe to the top side of a workpiece is to be programmed under ShopMill. Objective: A new ShopMill program is to be created and opened in the editor. The program header, a measuring cycle and the program end are to be programmed. Later, the program is to be simulated. For this, the data below are to be used: Tool data:

3D Probe (3D_PROBE))

2.1 Creating a new ShopMill program A new ShopMill program can be created from within all operating modes as follows: 1.


1.


2.


3.


4.


B655

Page 4


Section 2

Simple programming example 2.2 Programming example: Measuring a surface

Notes:

The following ShopMill program with a measuring cycle is to be programmed:

1.

Create a new ShopMill program like described in the previous section 2.1 and give the program a name, for example “SM_MEASURING_MILLING_1.MPF”. The input mask for the program header opens automatically.

2.

Insert the following values into the input mask of the program header and confirm the input with the VSK 8 “Accept”:


Page 5

B655

Section 2


Notes:


3.

Insert a probe tool (3D_PROBE) into the program. In order to do this, you have to access the tool list window from the work area “Straight Circle”! Note: This is necessary, since the tool list is not directly accessible over the technology “Measurem. Milling”. Press the “Extend”-key on the operator panel to reach to the “Straight Circle” function The vertical softkey bar 2 opens. Press the HSK 2.2 “Strght Circle”, to get access to the function “Tool”. Press the VSK 1 “Tool”, to open the input mask for the tool. Press the VSK 1 “Select tool”. The tool list window opens. Mark the desired tool (here 3D_PROBE) by using the blue cursor key on the keyboard and press the VSK 8 “OK”. The selected tool is loaded into the “tool“ input mask.

4.

Leave the value as follows:

Confirm your tool selection by pressing the VSK 8 “Accept”. The following program block is inserted into the work plan: 5.

Program the approach of the tool probe in a straight line with rapid traverse. Press the VSK 2 “Straight”. The input mask for the technology “Straight” opens. Insert the following position values into the parameter mask:

B655

Page 6


Section 2

Simple programming example Press the VSK 5 “Rapid traverse”, to set the federate to rapid traverse.

Notes:


6.

Program the approach of the tool probe in a straight line in XY with rapid traverse. Press the VSK 2 “Straight”. The input mask for the technology “Straight” opens.

7

Insert the following position values into the parameter mask:

Press the VSK 5 “Rapid traverse”, to set the federate to rapid traverse. Confirm your inputs by pressing the VSK 8 “Accept”. The following program block is inserted into the work plan: 8.

Program the approach of the probe tool in a straight line in Z direction with rapid traverse. Press the VSK 2 “Straight”. The input mask for the technology “Straight” opens.

9.


Press the VSK 5 “Rapid traverse”, to set the federate to rapid traverse. Confirm your inputs by pressing the VSK 8 “Accept”. The following program block is inserted into the work plan:


Page 7

B655

Section 2 Notes:


Program now a measuring cycle (CYCLE978). Press the HSK 2.6 “Measurem. milling”. The work area “Measurement milling” with extended measuring functions opens. Press the VSK 4 “Workpiece measure”. The vertical softkey bar with functions for the measurement of workpieces opens. Press the VSK 4 “Plane”. The Input window for the cycle “1-pt.meas./ CYCLE978” opens.

11.


Confirm your inputs by pressing the VSK 8 “OK”. The following two program blocks are inserted into the work plan.

12.

Program the program end and simulate the measurement of the work piece. Place the orange selection on the program block “End of program” and extend the line by pressing the blue “cursor-to-the-right” key on the keyboard.

13.

The input mask for the program end opens. Here, you can decide to repeat the program run.

Accept the default value and press the VSK 8 “Accept”.

B655

Page 8


Section 2

Simple programming example Switch back to the vertical softkey bar 1 by pressing the “Extend”-key on the control panel.

Notes:

The horizontal softkey bar 1 opens. Press the HSK 1.6 “Simulation” to start the simulation of the program. The control calculates the simulation and opens the simulation window in “Top view” by default.

To view the simulation 3-dimensional press the VSK 1.4 “3D-view”.


Page 9

B655

Section 3 Notes:

Complex programming example Description: Another program to measure a square work piece is to be programmed in ShopMill. Objective: The program header, two measuring cycles and the program end are to be programmed. Afterwards the program is to be simulated. For this, the data below is to be used: Tool data:

3d probe (3D_PROBE)

3.1 Programming example: Measuring edges

The following program with two measuring cycles is to be programmed:

1.

Create a new ShopMill program like described in the previous section 2.1 and give the program a name, for example “SM_MEASURE_MILLING_2.MPF”. The input mask for the program header opens automatically.

B655

Page 10


Section 3


Insert the following values for the program header into the input mask and confirm your inputs by pressing the VSK 8 “Accept”:

Notes:


3.

Insert a probe tool (3D_PROBE) into the program. In order to do this, you have to access the tool list window from the work area “Straight Circle”! Note: This is necessary, since the tool list is not directly accessible over the technology “Measurement Milling”. Press the “Extend”-key on the operator panel to switch to the vertical softkey bar 2. The vertical softkey bar 2 opens. Press the HSK 2.2 “Strght Circle”, to get access to the function “Tool”. Press the VSK 1 “Tool”, to open the input mask for the tool. Press the VSK 1 “Select tool”. The tool list window opens. Mark the desired tool (here 3D_PROBE) by using the blue cursor key on the keyboard and press the VSK 8 “OK”. The selected tool is loaded into the tool parameter window.


Page 11

B655

Section 3 Notes:


Leave the value as follows:

Confirm your tool selection by pressing the VSK 8 “Accept”. The following program block is inserted into the work plan:

5.

Program the approach of the probe tool in a straight line with rapid traverse. Press the VSK 2 “Straight”. The input mask for the technology “Straight” opens. Insert the following position values into the parameter mask:

Press the VSK 5 “Rapid traverse”, to set the federate to rapid traverse. Confirm your tool selection by pressing the VSK 8 “Accept”. The following program block is inserted into the work plan: 6.

Program the approach of the probe tool in a straight line in XY with rapid traverse. Press the VSK 2 “Straight”. The input mask for the technology “Straight” opens. Insert the following position values into the parameter mask:

Press the VSK 5 “Rapid traverse”, to set the feedrate to rapid traverse. Confirm your tool selection by pressing the VSK 8 “Accept”. The following program block is inserted into work plan.

B655

Page 12


Section 3


Program the approach of the probe tool in a straight line in Z with rapid traverse.

Notes:

Press the VSK 2 “Straight”. The input mask for the technology “Straight” opens. 9.


Press the VSK 5 “Rapid traverse”, to set the feedrate to rapid traverse. Confirm your tool selection by pressing the VSK 8 “Accept”. The following program block is inserted into the work plan. 10.

Program now a measuring cycle (CYCLE978). Press the HSK 2.6 “Measurem. milling”. The work area “Measurement milling” with extended measuring functions opens. Press the VSK 4 “Workpiece measure”. The vertical softkey bar with functions for the measurement of workpieces opens. Press the VSK 4 “Plane”. The Input window for the cycle “1-pt.meas./ CYCLE978” opens.

11.



Page 13

B655

Section 3

Complex programming example Confirm your inputs by pressing the VSK 8 “OK”.

Notes:

The following two program blocks are inserted into the work plan window.

12.

Program now a measuring cycle to measure the 4 edges of the workpiece. Press the VSK 4 “Workpiece measure”. The vertical softkey bar with functions for the measurement of workpieces opens. Press the VSK 1.7 “Extend”, to open the vertical softkey bar 2, where are more functions for measuring workpieces available. Press the VSK 2.2 “Rectangle”. The input window for the cycle “Meas.rectang./ CYCLE977” opens.

13.


Confirm your inputs by pressing the VSK 8 “OK”. The following two program blocks are inserted into the work plan window.

B655

Page 14


Section 3


Program the program end and simulate the measurement of the work piece.

Notes:

Place the orange selection on the program block “End of program” and extend the line by pressing the blue “cursor-to-the-right” key on the keyboard. 15.

The input mask for the program end opens. Here, you can decide to repeat the program run.

Accept the default value and press the VSK 8 “Accept”. Switch back to the horizontal softkey bar 1 by pressing the „Extend“-key on the operator panel. The horizontal softkey bar 1 opens. Press the HSK 1.6 “Simulation” to start the simulation of the measurement. The control calculates the simulation and opens the simulation window in “Top view” by default.

To view the simulation 3-dimensional, press the VSK 1.4 “3D view” (see following page).


Page 15

B655

Section 3


Notes:

B655

Page 16


B500

1

Cycles

Brief Description

Objective of the module: With the help of this module you will get to know the various cycle parameters in ShopMill and ShopTurn.

Description of the module: This module explains the various parameters that are called up in the cycle masks in tabular form . In the course of this the relationship and the differences of the parameters to the individual cycles and techniques are pointed out. Content: Fundamentals Turning Drilling Milling


Page 1

This documentation was produced for training purposes. SIEMENS does not accept resposibility for the contents.

B500

B500

B500

Page 2


B500 Cycles: Description This module explains the various parameters that are called up in the cycle masks in tabular form . In the course of this the relationship and the differences of the parameters to the individual cycles and techniques are pointed out.

Cycles: START

Fundamentals

Turning

Drilling

Milling

Cycles: END

Notes :


Page 3

B500

Section 2

Fundamentals

Notes.

2. 1 Cycles Cycles are sub-programs (technology-orientated functions) for the execution of a repeatedly occurring operation on a work piece. Cycles can be selected comfortably via Softkeys and can simply be parameterised by means of input masks. Programmed cycles are inserted in G-Code or step-chain-programs as a program step and can be re-selected and newly parameterised at any time. The following functionality is available both in ShopMill and ShopTurn  Technology-orientated cycle selection with help of Softkeys  Input masks for cycle parameters (cycle masks) with help pictures and animations  Context-sensitive online-help for every input window  Support for the contour input (geometry processor)


Page 5

B500

Section 3

Turning

Notes:

Unit α Plunge angle (Thread relief)

Degrees

α0

Starting angle offset

Degrees

α1

Angle of the tapers

Degrees

α1 (Stock removal)

Angle of the first edge

Degrees

α1 (Groove)

Flange angle 1

Degrees

α2 (Stock removal)

Angle of the second edge

Degrees

α2 (Groove)

Flange angle 2

Degrees

αP

Infeed taper (angle)

Degrees

Allowance (Stock removal)

Finishing allowance (only with finishing)

mm



Yes U1 contour allowance



No

Selection (Thread)

Table value, e.g. M10, M12, M14,…

B1

Width of groove, bottom

mm

B2

Width of groove, top

mm

Machining

  

Roughing Finishing Roughing + Finishing

Machining Machining directions direction  Planar Turning  Longitudinal (Stock removal parting)

Machining  direction  (Thread relief)

B500

Longitudinal Parallel to contour

Page 6


Turning

Section 3 Unit

Machining direction



Contourturning (Stock removal)

Notes.

Planar Longitudinal Parallel to contour From inside outward From outside inward From front to rear end From rear end to front

BL

Blank description (contour, cylinder, allowance)

D

Cutting edge number

D

Maximum infeed depth (inc)

mm

D1 (Thread)

First infeed depth

mm

DA

Start-changing depth (inc)

DI

At 0 continuous cut

DIR (parting)

Spindle rotation direction  counter-clockwise (CCW)  clockwise (CW)

DP (Longitudinal thread)

Infeed taper as a flank (inc)

DP (Groove)

Distance of back-cut (inc) DP is not displayed when N = 1

DX

Maximum infeed depth (only parallel to contour mm alternatively to D)

DZ

Maximum infeed depth (only for parallel to con- mm tour and UX)

Limit

Machining range limitation  Yes

mm

XA: 1st limit XA Ø XB: 2nd limit XB Ø (abs) or 2nd limit referred to XA (inc) ZA: 1st limit ZA ZB: 2nd limit ZB (abs) or 2nd limit referred to ZA 

No


Page 7

B500

Section 3

Turning

Notes:

Unit F

Feed

Form  (Thread relief) 

B500

mm/min mm/rev

Normal (Form A) Short (Form B)

FR (Parting)

Reduced feedrate

FR (Stock removal)

Plunging feedrate for relief cuts

FS (Stock removal)

Chamfer (n = 1...3) alternative to R

mm

FS

Chamfer width

mm

FS1

Chamfer width 1

mm

FS2

Chamfer width 2

mm

FS3

Chamfer width 3

mm

FS4

Chamfer width 4

mm

FX

Feed in X-direction

mm/rev

FZ

Feed in Z-direction

mm/rev

G

Change of thread pitch per rev.

Thread (Longitudinal thread )

 

H1 (Taper thread)

Calculated from thread pitch

mm

H1 (Longitudinal thread )

Depth of thread obtained from thread table

mm

Relief cuts (Stock removal)

Machining of relief cuts  Yes  No

Location turning (Stock removal)

Location of stock removal  right top  right bottom  left top  left bottom

mm/rev

Internal thread External thread

Page 8


Turning

Section 3 Unit

Location contourturning (Stock removal, parting)

   

LR

Thread run-out (inc)

mm

LW

Thread lead (inc)

mm

Multi-start



No α0 Starting angle offset



Yes Nr. of thread starts are spread evenly around the circumference of work piece

Notes.

front back internal external

N (Groove)

Number of grooves (N = 1...65535)

N (Thread)

Nr of thread starts

NN (Thread)

Number of dummy passes

P (Thread relief DIN)

Thread pitch (to be selected from DIN-table) or mm/rev entered manually

P (Longitudinal thread )

Selection of the thread pitch/-starts  Thread pitch in mm/rev  Thread pitch in inch/rev  Threads per inch  Thread pitch in modulus

mm/rev in/rev threads/" modulus

R1

Rounding radius 1

mm

R2

Rounding radius 2

mm

R3

Rounding radius 3

mm

R4

Rounding radius 4

mm

R

Radius (n = 1...3) alternative to FS

mm

S

Spindle speed

rev/min

SR

Reduced speed

rev/min

SV

Maximum rotary speed for constant cutting speed

rev/min


Page 9

B500

Section 3

Turning

Notes:

Unit Table

Selection of the thread table  without  ISO metric  Whitworth BSW  Whitworth BSP  UNC

T

Tool name

T1 (Groove)

Groove depth Ø (abs) or groove depth referred to X0 (inc)

mm

U1

Contour allowance

mm

U

Finishing allowance

mm

UX

Finishing allowance in X

mm

UZ

Finishing allowance in Z

mm

V

Constant cutting speed

m/min

VR

Retraction distance (inc)

mm

VX (Relief cut)

Planar pass Ø (abs) or planar pass (inc)

mm

X0 (Groove)

Reference point Ø (abs)

mm

X1 (Relief cut)

Allowance in X Ø (abs) or allowance in X (inc) mm

X1 End point of the thread Ø (abs) or thread (Stock removal length (inc) Thread)

mm

X1 End point X Ø (abs) or end point referred to X0 mm (Taper thread) (inc)

X1α Thread taper (Taper thread)

B500

Degrees

X1 (Parting cut)

Depth for speed reduction Ø (abs) or depth for mm speed reduction referred to X0 (inc)

X2 (Parting cut)

Final depth Ø (abs) or final depth referred to X1 (inc)

Page 10

mm


Turning

Section 3 Unit

XA

Notes.

1st limit XA Ø (abs) (limiting)

XB 2nd limit XB Ø (abs) (limiting) (Stock removal) XD (Parting)

Allowance or cylinder dimension (inc)

mm

XDA (Parting)

1st parting-limit tool Ø (abs)

mm

XDB (Parting)

2nd parting-limit tool Ø (abs)

mm

XF2 Relief cut (alternative to FS2 or R2) (Stock removal)

mm

XM

Intermediate point referred to X0

mm

Z0 (Groove)

Reference point Z (abs)

mm

Z1 End point Z Ø (abs) referred to Z0 (Stock removal)

mm

Z1 (Relief cut)

Allowance in Z

mm

Z1 (Thread)

End point of the thread

mm

ZA 1st limit ZA (abs) (limiting) (Stock removal) ZB 2nd limit ZB (abs) (limiting) (Stock removal) ZD (Parting)

Allowance or cylinder dimension (inc)

mm

ZM

Intermediate point Z

mm

Infeed



Linear: Infeed with constant cutting depth



Degressive: Infeed with constant chip cross-section


Page 11

B500

Section 4

Drilling

Notes:

Unit α

Lifting angle (tool orientation angle) (only for lifting the tool), spindle position for orientated spindle stop in the cycle.

Degrees

α0

Rotation angle for the straight line, referred to the X-axis

Degrees

α1 (Pitch circle)

Advancing angle (only for circular pattern pitch Degrees circle)

Lifting mode



Degrees

No lifting The cutting edge is not retracted, but returns to the safety clearance with rapid traverse.



Lifting The cutting edge is moved clear of the edge of the hole and is then lifted to the retraction level.

αS

Starting angle offset (only for tapping without a Degrees compensating chuck)

αX

Shearing angle X (only for the location patterns grid or frame)

Degrees

αY

Shearing angle Y (only for the location patterns grid or frame)

Degrees

Centre drilling

Centre drilling with reduced feedrate 

Yes



No The reduced feedrate is executed as follows: Drilling feedrate F1 < 0,15mm/rev: Centre drilling feedrate = 30% of F1 Path feedrate F1=> 0,15mm/rev: Centre drilling feedrate = 0,1 mm/rev

Selection (tapping)

B500

Selection of table value: 

M1 - M68 (ISO metric)



W3/4"; etc. (Whitworth BSW)



G3/4"; etc. (Whitworth BSP)



1" - 8 UNC; etc. (UNC)

Page 12


Drilling

Section 4 Unit

Selection

Machining (Drilling)

Notes.

Coordinate system  

Right-angled (Cartesian) Polar



Chip breaking



Chip clearing

Machining The following machining methods are avail(without comp. able: chuck)  One cut only: (Tapping) The tapping takes place in one pass without interruption.

Machining (with comp. chuck)



Chip breaking: The drill is retracted by an amount V2 for chip breaking.



Chip clearing: The drill is retracted from the work piece for chip clearing.

The following machining methods are available: 

With encoder: Tapping with spindle encoder



Without encoder: Tapping without spindle encoder selection with specification of the "pitch" parameter



Single location: Drilling at the programmed location



Location pattern: Location with MCALL

(Tapping)

Machining location

Drilling depth Referred to 

Shaft: Drilling until the drill-shaft has reached the programmed value X1. The angle in the tool list is taken into account.



Point: Drilling until the drill point has reached the programmed value X1.


Page 13

B500

Section 4

Drilling

Notes:

Unit C0 (Locations)

Polar coordinates of the 1st location, with the selection "polar" longitudinal (abs) angle (abs)

C1...C7 (Locations)

mm Degrees

Polar coordinates of further locations, with the selection "polar" longitudinal (abs) angle (abs)

Ø

Drilling continues until the diameter has been reached (only with centring)

Ø (internal thread milling)

Nominal diameter

D

Cutting edge number

D

maximum depth infeed (only with chip clearing or chip breaking)

mm

D (Boring)

Lift-off amount (inc) (only for lifting, SN)

mm

DF



Percentage for all further infeeds or

%



amount for every further infeed

mm

DIR

DT

DTB

DTS

B500

mm Degrees

mm

Direction of rotation 

counter-clockwise (CCW)



clockwise (CW)



Dwell at final drilling depth in seconds

s



Dwell at final drilling depth in revs

rev



Dwell at drilling depth in seconds

s



Dwell at drilling depth in revs

rev



Dwell at the start point for chip clearing in seconds (only for chip clearing)

s



Dwell at the starting point for chip clearing in revs (only for chip clearing)

rev

Page 14


Drilling

Section 4 Unit

Through drilling

Notes.

Remaining drilling depth at path feedrate  

Yes No

DX

Lift-off amount in X-direction (inc) (only for lifting, standard)

DY

Lift-off amount in Y-direction (inc) (only for lifting, standard)

DZ

Lift-off amount in Z-direction (inc) (only for lifting, standard)

Chip clearing Chip clearing before thread milling (Drill + thread milling)  Yes  No Retract to work piece surface for chip clearance before thread milling. F

Feedrate

mm/min mm/rev

F1

Path feedrate

mm/min mm/rev

FD1

Percentage feedrate for the first infeed

%

FR Drilling feedrate for remaining depth (Drill + thread milling)

mm/min mm/rev

FR

Feedrate for retraction

mm/min

FS

Finishing feedrate (only for down cut / up cut )

mm/min mm/tooth

Milling  direction  (Drill + thread  milling) Thread

Down-cut (climb milling) Up-cut (conventional milling) Down cut / up cut (climb/conventional milling)

Thread sense  

Right-hand-thread Left-hand-thread


Page 15

B500

Section 4

Drilling

Notes:

Unit L0

Distance of the first location from the reference point (only for location pattern straight line)

L0 (Locations)

Polar coordinates of the first location with selection "polar" longitudinal (abs) angle (abs)

mm

mm Degrees

L

Distance between the locations (only for location mm pattern straight line)

L1

Distance between the columns (only for location mm pattern grid or frame)

L1...L7 (Locations)

Polar coordinates of further locations, with selection "polar" longitudinal (abs) angle (abs)

mm Degrees

L2

Distance between the lines (only for location pattern grid or frame)

mm

LAB

Repeat of jump mark for location

Compensa-  ting chuck  mode

with compensating chuck without compensating chuck

N

Number of locations (only for location pattern straight line)

N1

Number of columns (only for location pattern grid or frame)

N2

Number of lines (only for location pattern grid or frame)

P

Thread pitch…    

in modulus: modulus = pitch/π in mm/rev in inch/rev in threads per inch

modulus mm/rev in/rev Threads/"

Positioning Positioning motions between the locations (Pitch circle)  Straight  Circle PL

B500

Machining plane G17 (XY)

Page 16


Drilling

Section 4 Unit

R

Radius

mm

RP

Retraction plane (abs)

mm

Retraction

(only for machining with "Chip breaking") retraction amount  

manually automatically

SC

Safety distance (inc)

SDE

Direction of rotation after end of cycle

S/V

Spindle speed or constant cutting speed

rev/min m/min

SPOS

Spindle stop position

Degrees

SR

Spindle speed for retraction

rev/min

Pitch  (only for ma-  chining without encoder)

User entry of the input active feed, pitch is derived from the feed rate

T

Tool name

Table

Selection of the thread table:     

Notes.

without ISO metric Whitworth BSW Whitworth BSP UNC

V1

Minimum infeed depth

mm

V2 (Tapping)

Retraction amount (only for retraction "manually")

mm

Amount, by which the tap is retracted for chip breaking. V2 = automatically: The tool retracts by one revolution. V2 (drilling)

Retraction amount after each machining operation (only for machining "chip breaking")

mm

V3

Pre-stopping distance (only for pre-stopping distance "manually")

mm


Page 17

B500

Section 4

Drilling

Notes:

Unit Pre-stopping (only for machining "chip clearing") distance  manually  automatically

B500

VR

Constant cutting speed for retraction

XD

Centre offset

X0

X-coordinate of the reference point X (abs)

mm

X1...X7 (Locations)

X-coordinate of further reference points (abs or inc)

mm

Y0

Y-coordinate of the Reference point Y (abs)

mm

Y1...Y7 (Locations)

Y-coordinate of further reference points (abs or inc)

mm

Z0

Reference point Z

mm

Z1 (Drilling)

Final drilling depth X (abs) or final drilling depth referred to Z0 (inc)

mm

Z1 (Thread)

End point of the thread (abs) or thread length (inc)

mm

Z1 (Drilling)

Final drilling depth X (abs) or final drilling depth referred to Z0 (inc)

mm

Z1 (Thread)


mm

Z2

Retraction amount before thread milling

mm

ZR

Remaining depth for through drilling ("Yes" only for through-holes)

mm

Page 18

m/min


Drilling

Section 4 Notes.


Page 19

B500

Section 5

Milling

Notes:

Unit α0

Rotation angle

Degrees

α0 (circular slot)

Start angle

Degrees

α1 (circular slot)

Opening angle of the slot

Degrees

α1 (Engraving)

Text direction (only for linear alignment)

Degrees

α1 (contour)

Starting direction relative to X-axis

Degrees

α1 (circular slot)

Opening angle of the slot

Degrees

α2 (circular slot)

Advancing angle (only for pitch circle)

Degrees

α2 (contour)

angle to previous element

Degrees

αS (ThreadMilling)

Starting angle

Degrees

Retract mode Retract mode in plane (Path milling)  Quarter circle: Part of a spiral (only for path milling to the left and the right of contour)

Retract strategy (Path milling)

B500



Semi circle: Part of a spiral (only for path milling to the left and the right of the contour)



Straight: Oblique in space

 

Axis-by-axis spatial

Page 20


Milling

Section 5 Unit

Lift mode (Centring)

Lifting mode before a renewed infeed

Notes.

mm

If for the machining several plunging points are required, the retraction height can be programmed:

Lift mode (Path milling)



to RP (retraction plane)



Z0 + safety distance

If several depth infeeds are required, the retraction height to which the tool is retracted to between the individual infeeds, can be specified here. (at the transition at the end of the contour to the beginning).

mm

Lifting mode before a renewed infeed

Lift mode (Pre-drilling centring) (Pocket milling)



No retraction



to RP (retraction plane)






by safety distance

Lifting mode before renewed infeed

mm

If for the machining several plunging points are required, the retraction height can be programmed as following: 

to RP






X0 + safety distance


Page 21

B500

Section 5

Milling

Notes:

Unit Approach (Path milling)

Approach strategy (Path milling)

Approach mode in plane 

Quarter circle: Part of a spiral (only for path milling left and right of the contour)



Semi circle: Part of a spiral (only for path milling left and right of the contour)



Straight: Oblique in space



Vertical: Perpendicular to the path (only for path milling on the centre line path)



Axis-by-axis (only for approach "quarter circle or semi circle")



Spatial (only for approach "quarter circle, semi circle or straight")

Removing  (Rectangular pocket, only for roughing) 

Alignment (Engraving)

B500

mm

Complete machining: The rectangular pocket is milled out of the solid material. Re-machining: An already existing small rectangular pocket or a bore is enlarged in one or more axes. In this case the parameters AZ, W1, and L1 must be programmed.



Linear alignment



Curved alignment, arch at the top



Curved alignment, arch at the bottom

Page 22


Milling

Section 5 Unit

Selection (Threadmilling)

Selection of table values: 

M3, M10, etc. (ISO metric)



W3/4"; etc. (Whitworth BSW)



G3/4"; etc. (Whitworth BSP)



1" - 8 UNC; etc. (UNC)

AZ

Depth of roughing (only for re-machining)

mm

β1

End-angle to X-axis

Degrees

β2

Opening angle of the circle

Degrees

Machining  (Planar-/ thread-milling) 

Machining  (Rectangular/ round spigot)  (path milling) 

Machining (Rectangular/ circ. pocket) (Longitudinal/ circ. slot) (multi edge spigot) (Rectangular/ circ. spigot)

Notes.

Roughing Finishing

Roughing Finishing Chamfering



Roughing



Finishing



Finishing edge



Chamfering


Page 23

B500

Section 5

Milling

Notes:

Unit Machining plane

Machining type (Circular pocket)

Selection of the machining plane   

G17 (X/Y) G18 (Z/X) G19 (Y/Z)



Centric: Clearing a circular pocket plane-by-plane



Helical: Clearing a circular pocket helically

Machining  face (Planar milling) 

Machining  face (Rectangular/ circ. spigot)  Thread milling)

Machining face (Rectangular pocket) (Longitudinal/ circular slot) (Open slot) (Circ. spigot) (Engraving) (Path milling)

Machining direction (Thread milling)

B500

Front Y: Machining on a front face with Y-axis Mantle Y: Machining on a cylindrical surface with Y-axis Front C: Machining on a front face with C-axis Front Y: Machining on a front face with Y-axis



Mantle Y: Machining on a cylindrical surface with Y-axis



Front C: Machining on a front face with C-axis



Front Y: Machining on a front face with Y-axis



Mantle C Machining on a cylindrical surface with C-axis



Mantle Y Machining on a cylindrical surface with Y-axis



Z0 → Z1 Machining from top to bottom



Z1 → Z0 Machining from bottom to top Page 24


Milling

Section 5 Unit

Machining direction (Path milling)

Notes.

Machining in the programmed contour direction 

Forward: The machining takes place in the programmed contour direction



Backward: The machining takes place against the programmed contour direction

Machining location (Rectangular pocket) (Longitudinal slot)



Single location: Milling a rectangular pocket at the programmed location (X0, Y0, Z0) .



Location pattern: Location MCALL

Machining location (circular pocket)



Single location: Milling a circular pocket at the programmed location (X0, Y0, Z0).



Location pattern: Several circular pockets are milled on a location pattern (e.g. full circle, pitch circle, grid etc.).

Machining  location (Rectangular/ circular spigot) 

Single location: Milling a rectangular/circular spigot at a programmed location (X0, Y0, Z0). Location pattern: Location with MCALL.


Page 25

B500

Section 5

Milling

Notes:

Unit Machining location (multi-edge spigot)

Machining location (Open slot)

Single location: A multi-edge spigot is milled at the programmed location (X0, Y0, Z0).



Location pattern: Several multi-edge spigots are milled on the programmed location pattern (e.g. pitch circle, grid, straight line).



Single location: Milling a slot at the programmed location (X0, Y0, Z0).



Location pattern: Milling of several slots on a programmed location pattern (e.g. full circle or grid).

Reference point (Open slot)

Location of the reference point:

Reference point (Engraving)

Location of the reference point:

Reference point (Slot)

B500



  

Left edge Centre Right edge

  

Bottom left Bottom centre Bottom right

  

Top left Top centre Top right

  

Centre left Centre Centre right

Location of the reference point:     

Left edge Inside left Centre Inside right Right edge

Page 26


Milling

Section 5 Unit

Reference point (Rectangular pocket)

The following various locations of the reference point can be selected:     

Centre Bottom left Bottom right Top left Top right

CP

Positioning angle for machining range (only for front Y)

Degrees

C0

Positioning angle for machining face (only for mantle Y)

Degrees

Ø (Circular pocket)

Diameter of the pocket

mm

Ø (Circular spigot)

Diameter of the spigot

mm

Ø (Threadmilling)

Nominal diameter, Example: Nominal diameter of M12 = 12 mm

mm

Ø1 (Circularspigot, multi-edge spigot)

Diameter of the blank spigot

mm

Ø1 (Circular pocket)

Diameter of pre-machining (only for re-machining)

mm

D

Cutting edge number of the tool (1 - 9)

Direction of rotation (Threadmilling)

Direction of the thread rotation:

Rotation (Milling)

Notes.



Right hand thread A right-hand thread is milled



Left hand thread A left-hand thread is milled

 

Rotation clockwise Rotation counter-clockwise


Page 27

B500

Section 5

Milling

Notes:

Unit DX1 (Engraving)

Character spacing or total width (only for linear alignment) for front face machining

mm

DX

Maximum depth infeed

mm

DXY

Maximum plane infeed

mm

Alternatively the plane infeed can also be stated as a percentage ratio of plane infeed (mm) to the milling cutter diameter (mm)

%

DY1 (Engraving)

Character spacing or total width (only for linear alignment) for mantle machining

mm

DYZ

Maximum plane infeed

mm

Alternatively the plane infeed can also be de- % fined as a percentage ratio of the plane infeed (mm) to the milling cutter diameter (mm) DZ

Maximum depth infeed (only for roughing)

Plunging (Rectangular pocket) (Longitudinal slot) (Pocket milling)



Vertical: Vertical plunging to the pocket centre



Helical: Plunging along a spiral path



Oscillating: Plunging with an oscillating motion along the central axis of the rectangular pocket.



Vertical: Vertical plunging at the centre of pocket.



Helical: Plunging along a spiral path

Plunging (Circular pocket)

EP Maximum pitch of the helix (Rectangular/ (only for helical plunging) circular pocket)

B500

Page 28

mm

mm/rev


Milling

Section 5 Unit

ER Radius of the helix (Rectangular/ (only for helical plunging) circular pocket)

mm

EW (Rectangular pocket) (Longitudinal slot)

Maximum plunge angle (only for oscillatory plunging)

Degrees

F

Feed

mm/min mm/rev

FR (Path milling)

Retraction feed for intermediate positioning

Milling direction (Open slot)

Milling direction (other than plunge milling)  

Notes.

Climb milling Conventional milling

FS Chamfer width for chamfering (Rectangular/ (only for chamfering) circular pocket) (Rectangular/ circular spigot) (Path milling)

mm

FX Infeed feed depth (Rectangular/ (only for vertical and pre-drilled plunging) circular for mantle C/Y pocket) (Longitudinal slot)

mm/min mm/tooth

FZ Infeed feed depth (Rectangular/ (only for vertical and pre-drilled plunging) circular for front C/Y machining pocket) (Longitudinal slot)

mm/min mm/tooth

Engraving text (Engraving)

Maximum 100 characters

H1 (Threadmilling)

Thread depth


mm

Page 29

B500

Section 5

Milling

Notes:

Unit I

Circle centre point in X-direction (abs or inc)

mm

J

Circle centre point in Y-direction (abs or inc)

mm

Circular pattern (Circular slot)



Full circle: The circular slots are positioned on a full circle. The distance of one circular slot to the next circular slot is always the same and is determined by the control unit.



Pitch circle: The circular slots are positioned on a pitch circle. The distance of one circular slot to the next circular slot can be determined by means of angle α2.

L1 (Rectangular pocket)

Pre-machined pocket length (only for further machining)

mm

L1 (Rectangular spigot)

Blank material length of spigot (only for further machining)

mm

L1 (Path milling)

Approach length (only for approach "Straight")

mm

L2 (Path milling)

Exit length (only for exiting "Straight")

mm

L2 (Circle)

(abs) Distance between pole and circle centre mm point mm (inc) Distance between the last point and circle centre point

B500

L

Length of pocket, spigot, slot, straight

Position of the thread (Threadmilling)

Position of the thread: 

Internal thread: An internal thread is milled



External thread: An external thread is milled

Page 30

mm


Milling

Section 5 Unit

N (multi-edge spigot)

Number of edges

N (Circular slot)

Number of slots

NT (Thread milling)

Number of teeth per cutter

P

Thread pitch…

(Thread milling)

   

in modulus: modulus = pitch/π in mm/rev in inch/rev in threads per inch

Notes.

modulus mm/rev in/rev Threads/"

The thread pitch depends on the tool used PL

Machining plane   

Positioning (Circular slot)

G17 (XY) G18 (ZX) G19 (YZ)

Positioning between the slots: 

Straight: The next location is approached along a straight line at rapid traverse.



Circle: The next location is approached along a circular path at the programmed feedrate

R1 (multi-edge spigot)

Rounding radius

mm

R2 (Path milling)

Exit radius (only when exiting contour with "quarter circle or semi circle")

mm


Page 31

B500

Section 5

Milling

Notes:

Unit R (Rectangular pocket/spigot)

Corner radius

mm

R (circular slot)

Radius of the circular slot

mm

R (Milling)

Radius of the circle

mm

RP (Centring)

Retraction plane

mm

Radius correction



Left (machining to the left of the contour)

(Path milling)



Right (machining to the right of the contour)



OFF (machining tool centre path)

Direction



Same machining direction  to the right  to the top



Changing machining direction  meandering left/right  meandering up/down

S

Spindle speed

rev/min

Stop-Position Input of the spindle position in degrees Starting point  (Pocket  milling)

B500

Manually preset starting point Automatic starting point calculation

SW (multi-edge spigot)

Spanner size A/F

T

Input of the tool (Name or number)

Page 32


Milling

Section 5 Unit

Table (Threadmilling)

Techno-logy (Open slot)

Notes.

Selection the thread table:     

without ISO Metric Whitworth BSW Whitworth BSP UNC



Whirling: Circular motion of the cutter through the slot and back again



Plunge milling: Sequential boring motions along the tool axis.

TR Reference tool for rest material machining (Pocket Restmaterial) U (ThreadMilling)

Finishing allowance in Y and X

mm

UX (Longitudinal slot)

Finishing allowance depth

mm

UXY

Finishing allowance plane

mm

UYZ

Finishing allowance plane

mm

UZ

Finishing allowance depth

mm

V

Feed constant cutting speed

m/min


Page 33

B500

Section 5

Milling

Notes:

B500

Unit W (Rectangular pocket)

Width of the pocket

mm

W (Rectangular spigot)

Width of the spigot

mm

W (Longitudinal/ circular slot)

Width of the slot

mm

W (Engraving)

Character height

mm

W1 (Rectangular pocket)

Width of the pre-machining (only for further machining)

mm

W1 (Rectangular spigot)

Width of the raw material spigot (Important for mm the determination of the approach location)

X0 (Rectangular /circular pocket) (Rectangular spigot)

Reference point X (only for single location)

mm

X0 (Planar milling)

Reference point 1 X

mm

X1 (Planar milling)

Reference point 2 X (abs) or reference point 2X referred to X0 )inc)

mm

X1 (Rectangular/ circular spigot)

Spigot depth (abs) or depth referred to Z0 or X0 (inc)

mm

X1 (Longitudinal slot)

Slot depth (abs) or depth referred to Z0 or X0 (inc)

mm

XFS

Plunging depth of tool tip (abs or inc) (only for chamfering) Machining mantle C/Y

mm

XM (Engraving)

Centre point X (abs) or centre point polar length (only for curved alignment)

mm or Degrees

XS (Pocket milling)

Starting point X (only if starting point is preset manually)

Page 34


Milling

Section 5 Unit

Y0 Reference point Y (Rectangular/ (only for a single location) circular pocket) (Rectangular spigot)

mm or Degrees

Y0 (Planar milling)

Reference point 1 in Y

mm

Y1 (Planar milling)

Reference point 2 in Y referred to Y0

mm

YM (Engraving)

Centre point Y (abs) or C (abs) (only for curved alignment) (only for machining mantle C/Y)

mm or Degrees

YS (Pocket Milling)

Starting point Y (only if starting point is preset manually)

Z0 Reference point Z (Rectangular/ (only for single location) circular pocket) (Rectangular spigot)

mm

Z0 (Planar milling)

Height of blank material

mm

Z1 (Planar milling)

Height of the finished item referred to Z0

mm

Z1

Final depth (abs) or final depth referred to Z0 or X0 (inc)

mm

Z1 (Engraving)

Engraving depth (abs) or depth referred to Z0 or X0 (inc)

mm

Z1 (Threadmilling)


mm

ZFS

Plunging depth tool point (abs or inc) (only for chamfering) (only for machining front C/Y)

mm

ZM (Engraving)

Centre point Z (abs) (only for curved alignment) (only for machining mantle C/Y)

mm


Page 35

Notes.

B500

B500

Page 36


Drawings of programming examples

B700

1

Brief description

Objective of the module: This module provides the means to carry out further exercises regarding the programming with ShopMill and to consolidate the programming knowledge so far attained. Description of the module: This module contains all the drawings that were used in the individual modules so far and additional work piece drawings as exercises for the consolidation of the acquired knowledge.

Content: 

Shop drawings - Mould - Mould plate - Guide plate_1 - Mounting plate - Perforated plate - Housing cover - Longitudinal guide - Example_1 - Mould_2 - Exhibition example - Mould plate_2 - Excercise_12 - Flange - Pressure plate - Guide plate_2 - Kidney-shaped plate - Con-rod - Wing - Connecting piece


Page 1


B700

B700

B700

Page 2


B700 Drawings of programming examples: Description This module contains all the drawings that were used in the individual modules so far and additional work piece drawings as exercises for the consolidation of the acquired knowledge.

Drawings of programming examples: START Mould_2

Con-rod

Exhibition example

Wing

Mould

Mould Plate Mould plate_2 Guide Plate_1 Exercise-12

Connecting piece

Drawings of programming examples: END

Mounting Plate Flange Perforated Plate Pressure plate Housing Cover Guide plate_2 Longitudinal guide Kidneyshaped plate Example_1

Notes :


Page 3

B700

Section 2

2.1

Mould

20

15

5

Notes:

Shop drawings

150 95

R2 0

M10

75

60 4°

25

A

30°

100

40

50

R6

A 145

120

75

30

5

- 12

5 0

- 12

Y X

B700

Page 4


Section 2

Shop drawings

Notes:

Mould plate

10

15

25

5

2.2

A-A 40 80°

R3

0

150

20

22

A

22

5

R2

3

35

R15

90

100

R36

A R5

60

Y

70

X


100

Page 5

B700

Section 2 Notes:

Shop drawings 2.3

Guide plate_1

30

15

10

A-A

70

30

0 R2 0 R1

240

140

A

Scaling factor: 1,5

A

120 240

Y X

B700

Page 6


Section 2

Shop drawings 2.4

Notes:

Mounting plate

25

10

75

100

100

Ø50

Y X


Page 7

B700

Section 2 Notes:

Shop drawings 2.5

Perforated plate

25

10

90

100

20

5 Ø2

100

20

R5

25

Y 30

X Alle nicht bemaßten Radien 5 mm

B700

Page 8


Section 2

Shop drawings 2.6

Notes:

Housing cover

40

35 30

25

Section A-A

10

150

0

M1

0

100

R2 Ø8

A

A

15

Y X


Page 9

B700

Section 2 Notes:

Shop drawings 2.7

Longitudinal guide

M10

20

10

Ø11

Ø10

A

100 130

100

80

61

0 Ø4

A

150

Y X

B700

Page 10


Section 2

Shop drawings

Notes:

Example_1

10

5

2.8

84 27

9

24

27

36

60

51

R14

12 53

Y

108

X


Page 11

B700

2.9

Mould_2

15

10 5

Notes:

Shop drawings

20

Section 2

150 95

R2

0

Ø30

75

60

25

A

30°

100

40

50

R6

A 145

120

75

30

5

0

Y X

B700

Page 12


Section 2

Shop drawings

Notes:

2.10 Exhibition example

100 90 70

15

R5

R5

5 R2

R4 5

70

30 Ø

60

°

30

8

15

30

A

30

5

Y

15

10

10

M6

X


Page 13

B700

2.11 Mould plate_2

10

A-A

20

Notes:

Shop drawings

15

Section 2

Ø10

Ø10

R1

5

45

35

R2

2 ,5

Ø30 R3 0

45 R36

90

92.5

100

A

A

45

(42.5)

100

R5

60

Y

70 85

X

B700

Page 14


Section 2

Shop drawings

Notes:

2.12 Excercise_12

Section A-A

20

10

4

8

Ø50

8,5

R1 0

100 90

10

100

80

60

R1 8

70

15°

A

R15

120

A

150

Y X


Page 15

B700

2.13 Flange

20

10

Notes:

Shop drawings

5

Section 2

18

110°

R10

R4

2

18

R5

R2 5

100

40°

50

8

82

R5 2

8

132 150

Y X

B700

Page 16


Section 2

Shop drawings

Notes:

15

5

2.14 Pressure plate

140 115 83

60

40

10

5

20

R5

10

R5

40

90

15

R5

15

0 R1

15

R6

15

15

Y X


Page 17

B700

Section 2 Notes:

Shop drawings 2.15 Guide plate_2

Section A-A

60

35

40

10

M12

140

160

R20

160

A

5 R1

20

40

40

A 90

Y X

B700

Page 18


Section 2

Shop drawings

Notes:

15

5

2.16 Kidney-shaped plate

60

R2 0

R80

R75

200

30

50

R10

15

200

Y X


Page 19

B700

Section 2 Notes:

Shop drawings 2.17 Con-rod

Section A-A 18 8

28

20

22

R 18

A

R20 6

R5

75

115±0,1

12

20

Y

A X

B700

Page 20


Section 2

Shop drawings

Notes:

2.18 Wing

15

5

10

Ø110

25°

R4 5

50

R2

R1

5

0

10

R

Y X


Page 21

B700

Section 2 Notes:

Shop drawings 2.19 Connecting piece

Section A-A Ø38 Ø14H7

1 Ø26 5

15

42,5

4

Ø16

4

12

Ø10H7

Ø26 Ø40 R3

A

A 116,8

Y X

B700

Page 22


Notes:


Page 23

B700

B700


EN_ Complete Sinumerik Operate Milling_v26

Recommend Documents