Content      ..     14      15      16      17     ..

SINUMERIK 840D sl. Training. Operate - Turning (2016-2020) - page 16

Operating mode “JOG“

M570

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 sub window indicates that there are more axis values availa-

ble, 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.

Vertical softkey bar

Display area

Description

By pressing the VSK 1 "X=0" the position of the X-axis will be reset to zero.

By pressing the VSK 2 "Y=0" the position of the Y-axis will be reset to zero.

By pressing the VSK 3 "Z=0" the position of the Z-axes 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.

Notes

828D/840Dsl SINUMERIK Operate

Page 13

M570

M570

Operating mode “JOG“

Measure workpiece

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 work-

piece 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%.

Vertical softkey bar

Display area

Description

By pressing the VSK 1 “Calibrate probe“ the input mask for “Calibrate probe“ opens.

Notes

M570

Page 14

828D/840Dsl SINUMERIK Operate

Operating mode “JOG“

M570

Display area

Description

By pressing the VSK 2 “Set edge“ the “Set edge“ window opens.

By pressing the VSK 3 “Align edge” the “Align edge” window opens.

By pressing the VSK 4 “Rectangular corner” the “Rectangular corner” window opens.

By pressing the VSK 5 “1 Hole” the “1 Hole” window opens.

By pressing the VSK 6 “1 Circular spigot” the “1 Circular spigot” window opens.

By pressing the VSK 7 “1 Rectangular spigot” the “1 Rectangular spigot” window opens.

By pressing the VSK 8 "Back" you switch back to the main screen of the Sinumerik Operate.

Selecting the function “Calibrate probe”

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.

Notes

828D/840Dsl SINUMERIK Operate

Page 15

M570

M570

Operating mode “JOG“

Example of two measurment functions “Set edge“ and “Tapinto rectangular“

As already described in section 3, a mechanical probe to be created in the tool list and using “T, S, M“ loaded into the

spindle.

With the VSK 1 "In Manual", the tool is transferred into the input window of T, S, M.

Additional functions of the input mask of "T, S, M" are briefly explained.

The "Spindle M function", a mechanical probe is

oriented for easy reading.

The "Stop position" can be any angle.

In addition, the offset can be activated, in which the measured values are to be entered.

The technology window will display the measuring tool from the tool list, with details of length

and edge number.

Note:

The part to be measured is "Set edge" on the workpiece surface with the meas-

urement function with 1mm oversize and is in the middle of the workpiece, meas-

ured with the measuring function "Rectangular spigot" .

Notes

M570

Page 16

828D/840Dsl SINUMERIK Operate

Operating mode “JOG“

M570

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 loaded in the spindle for scratching when measuring the workpiece zero manually.

 An electronic workpiece probe is loaded 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.

Vertical softkey bar (VSK)

Display area

Description

By pressing the VSK 2 “Select 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 .

Notes

828D/840Dsl SINUMERIK Operate

Page 17

M570

M570

Operating mode “JOG“

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

Measurement

direction:

The selection of the axes directions “X”/”Y”/”Z” is made by the

 X

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

Workpiece zero measure "Rectangular spigot"

The workpiece is parallel to the coordinate system on the work table and is a rectangle. About 4 measuring points of the

center of the rectangle is determined.

The following requirements must be met:

 Any tool can be used for scratching when loaded into the spindle for workpiece zero manual measuring.

 An electronic workpiece probe when loaded into the spindle and activated will measure the workpiece zero automati-

cally.

Pressing the VSK 6 "Rectangular spigot" softkey in the function "Meas. Workp. "

(" Machine "in the" JOG ") appears on the screen the following input mask.

Vertical softkey bar (VSK)

See page 20, Measure workpiece "Set edge".

Parameter Measure workpiece "Rectangular spigot"

The following parameters of Measure workpiece "Set edge" are also at work measure "Rectangular spigot":

[Zero offset G54, X0, Y0]

Notes

M570

Page 18

828D/840Dsl SINUMERIK Operate

Operating mode “JOG“

M570

Measuring a tool

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 refer-

ence 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

828D/840Dsl SINUMERIK Operate

Page 19

M570

M570

Operating mode “JOG“

Vertical softkey bar (VSK)

Display area

Description

By pressing the VSK 1 ”Length manually” the “Length manually” input mask opens.

By pressing the VSK 2 “Radius manual“ or rather “Diameter manual“ the input mask “Radius

manual“ or rather “Diameter manual“ opens.

By pressing the VSK 6 ”Calibrate probe” the “Calibrate probe” input mask opens.

By pressing the VSK 7 ”Calibrate fixed pt.” the “Calibrate: fixed point” input mask opens.

By pressing the VSK 8 “Back“ you jump back to the “Meas. tool” screen of the Sinumerik

Operate.

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.

Vertical softkey bar (VSK)

Display area

Description

By pressing the VSK 1 “Select tool“ the tool list opens.

See module M573 - “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

M570

Page 20

828D/840Dsl SINUMERIK Operate

Operating mode “JOG“

M570

Parameters of measure tool “Length manual“

Parameter

Description

T

Tool name

Alternatively you can select a tool via the VSK 1 “Select tool”.

D

Edge number

(1 to 9)

ST

Replacement tool

(01- 99)

Ref. point

Workpiece or Fixed pt.

Z0

Workpiece edge

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 rotating 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.

Notes

828D/840Dsl SINUMERIK Operate

Page 21

M570

M570

Operating mode “JOG“

Measure tool ”Radius manual“ or “Diameter manual”

By pressing the HSK 4 “Meas. tool” and the VSK 2 “Radius manually“ or “Diameter

manually” (in the operating area “Machine“ and operating mode “JOG”) the following input

mask opens.

Vertical Softkey bar (VSK)

Display area

Description

By pressing the VSK 2 “Select tool” the tool list opens.

By pressing the VSK 7 “Set diamet.“ (or “Set radius.”) all entered values will be accepted.

By pressing the VSK 8 “Back“ you jump back to the “Measure tool” screen of the Sinumerik

Operate“.

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

M570

Page 22

828D/840Dsl SINUMERIK Operate

Operating mode “JOG“

M570

Procedure for measuring the tool “radius manual” (or “diameter manual” )

1.

Load 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.

Selecting the function “Calibrate fixed point”

If you want to measure your tools manually, you must first determine the height of the fixed point on the machine table with

reference to the machine zero.

The fixed point can be either a measuring gauge of a known height or an electronic height gauge of known height. Place

the gauge in the working area of the machine (e.g on the machine table) and align it relative to the machining axes.

You can use any type of tool to measure the fixed point.

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 7 “Calibrate fixed pt.“ (in the operating area

“Machine“ and operating mode “JOG”) the “Fixed point calibration” window opens.

Notes

828D/840Dsl SINUMERIK Operate

Page 23

M570

M570

Operating mode “JOG“

Vertical softkey bar (VSK)

Display area

Description

By pressing the VSK 7 “Calibrate“ the control calculates the fixed point height.

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

Parameters of measure tool “Calibrate: fixed height”

By calibrating the probe the following parameters are displayed:

Parameter

Unit

Description

DZ

[mm]

Is the distance from the table to top of the fixed point gauge.

procedure for tool measure “Calibrating fixed point”

1.

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

fixed point gauge

2.

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

3.

Press the VSK 6 “Calibrate fixed pt.”.

4.

Use the JOG keys in “Incremental mode, or the handwheel to position the tool at the fixed posi-

tion height.

5.

Press the “Calibrate“ softkey to calibrate the fixed point.

Position

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 oper-

ating mode “JOG” the following input mask will be shown on the screen:

Vertical softkey bar (VSK)

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 traverse” 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

M570

Page 24

828D/840Dsl SINUMERIK Operate

Operating mode “JOG“

M570

Parameters of “Position”

Parameter

Unit

Description

F

[mm/min]

Feed

[mm/tooth]

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 specif-

Z

ic.

Follow the documentation of the machine manufacturer.

SP

[Degree]

Target angle [abs, inc]

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.

Notes

828D/840Dsl SINUMERIK Operate

Page 25

M570

M570

Operating mode “JOG“

Face milling

Selecting the function “Face milling”

You can use this cycle to face mill any workpiece. A rectangular surface is always machined.

“Measuring the workpiece" is already mentioned in section 5. The input mask “Face milling” is described in relation to a

workpiece with dimensions 25x100x100 mm, with 1mm to be removed leaving a thickness of 24mm.

The zero point in the X and Y axis has been determined in the workpiece

center with measuring function "Rectangular spigot" and the Z axis was "set

edge" with Z value +1 mm determined and stored at zero 1 (G54).

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.

Vertical softkey bar (VSK)

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 FACEMILL_50 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.

Notes

M570

Page 26

828D/840Dsl SINUMERIK Operate

Operating mode “JOG“

M570

Vertical softkey bar (VSK)

Display area

Description

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.

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.

Parameters of “Face milling”

Parameter

Unit

Description

T

Tool name

D

Cutting edge number of the tool.

F

[mm/min]

Feed

[mm/tooth]

S

[rpm]

Spindle speed

V

[m/min]

or constant cutting speed

Machining

The following machining operations can be selected:

Roughing

Finishing

Direction

Same direction of machining

Alternating direction of machining

X0

Corner point 1 of surface in X direction (abs)

Y0

mm

Corner point 1 of surface in Y direction (abs)

Z0

Height of blank (abs)

X1

Corner point 2 of surface in X (abs or inc)

Y1

mm

Corner point 2 of surface in Y (abs or inc)

Z1

Height of finished part (abs or inc)

Notes

828D/840Dsl SINUMERIK Operate

Page 27

M570

M570

Operating mode “JOG“

Parameters of “Face milling”

Parameter

Unit

Description

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

Setting

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.

Vertical softkey bar (VSK)

Display area

Description

By pressing the VSK 4 "Measure. report" the settings for the measuring report can be

configured.

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 imperi-

al (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.

Notes

M570

Page 28

828D/840Dsl SINUMERIK Operate

Operating mode “JOG“

M570

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 press-

ing 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

Notes

828D/840Dsl SINUMERIK Operate

Page 29

M570

M570

Operating mode “JOG“

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

[mm/min]

Axis feedrate/linear feedrate

[mm/rev]

Revolutional feedrate

 G95

Setup feedrate:

 G94

[mm/min]

Axis feedrate/linear feedrate

[mm/rev]

Revolutional feedrate

 G95

Variable increment

Enter the desired increment for axis traversal by variable increments

Spindle speed

[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 Op-

erate in the extended view.

M570: END

Notes

M570

Page 30

828D/840Dsl SINUMERIK Operate

Operating mode “MDA”

M571

Operating mode

"MDA":

START

Operating

mode “MDA“

“Load MDI“

“Save MDI“

Operating mode

"MDA":

END

Notes

828D/840Dsl SINUMERIK Operate

Page 3

M571

M571

Operating mode “MDA”

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.

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:

Vertical softkey bar

Display area

Description

By pressing the VSK 1.5 “Delete blocks” entered program blocks can be deleted.

Notes

M571

Page 4

828D/840Dsl SINUMERIK Operate

Operating mode “MDA”

M571

Horizontal softkey bar 1

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.

“Load MDI“

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:

Notes

828D/840Dsl SINUMERIK Operate

Page 5

M571

M571

Operating mode “MDA”

Vertical softkey bar

Display area

Description

Press the VSK 3 “Search“ to open the “Find file” window.

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

Loading a MDI-program

1.

Switch to operating mode “MDA“.

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.

“Save MDI“

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.

Notes

M571

Page 6

828D/840Dsl SINUMERIK Operate

Operating mode “MDA”

M571

Vertical softkey bar

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.

Press the VSK 3 “Search“ to open the “Find file” window.

Display area

Description

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.

Saving a MDI-program

1.

Select the operating mode “MDA”.

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.

M571: END

Notes

828D/840Dsl SINUMERIK Operate

Page 7

M571

M571

Operating mode “MDA”

Notes

M571

Page 8

828D/840Dsl SINUMERIK Operate

Operating area “Parameter”

M573

Operating area

"Parameter":

START

Operating

area

“Parameter“

Tool list

Tool wear

Magazine

management

Zero offset

basics

Work offset

Operating area

"Parameter":

END

Notes

828D/840Dsl SINUMERIK Operate

Page 3

M573

M573

Operating area “Parameter”

Operating area “Parameter“

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 soft-

key bar opens.

Then switch to the operating area “Parameter” by pressing the HSK 2 “Parameter” on the oper-

ator 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.

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”.

Notes

M573

Page 4

828D/840Dsl SINUMERIK Operate

Operating area “Parameter”

M573

Display area

Description (continuation)

By pressing the HSK 4 “Magazine“ the Magazine management is opened.

By pressing the HSK 5 “Work offset“ a list with all Work offsets is opened.

By pressing the HSK 6 “User variable“ a list with all R variables is opened.

By pressing the HSK 8 “Setting data” a list with all setting data is opened.

By pressing the "Extend"-button on the operator panel (OP) more softkeys on the HSK are

available.

By pressing the HSK 2.6 “CTRL Energy“ the SINUMERIK Ctrl-Energy analysis screen is

opened.

Tool List

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.

Notes

828D/840Dsl SINUMERIK Operate

Page 5

M573

M573

Operating area “Parameter”

Vertical softkey bar

Display area

Description

By pressing the VSK 1.1 “Tool measure” the “Measuring tool” window opens.

By pressing the VSK 1.2 “New tool” a new tool can be created. This function is only availa-

ble, if the cursor is positioned on a filed that does not yet has a tool assigned to it.

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 cut-

ting edges each edge gets its own set of correction data.

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.

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.

By pressing the VSK 1.6 “Delete tool” the selected tool will be deleted from the tool list.

By pressing the VSK 1.7 “Magazine selection” Softkey multiple times you can jump between

buffer location (spindle and gripper), Magazine and NC-memory (unloaded tools) and back to

the buffer location. The cursor is always positioned at the beginning of each group.

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.

Pressing the VSK 2.2 “Filter” opens the screen to set the filter options.

Pressing the VSK 2.3 “Search“ opens a new softkey bar with the functions



Tool



Magazine location



Empty location

The type of search is selected by the sotfkey selection.

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.

Notes

M573

Page 6

828D/840Dsl SINUMERIK Operate

Operating area “Parameter”

M573

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 num-

ber 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 win-

dows can be opened by pressing the corresponding vertical softkeys.

Press the VSK 1 “Favourites” to open the “New tool - favour-

ites” list. In the favourite list

the most often used tools are saved as favourites for a fast

access.

Notes

828D/840Dsl SINUMERIK Operate

Page 7

M573

M573

Operating area “Parameter”

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

Notes

M573

Page 8

828D/840Dsl SINUMERIK Operate

Operating area “Parameter”

M573

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

Notes

828D/840Dsl SINUMERIK Operate

Page 9

M573

M573

Operating area “Parameter”

Icons in the toolbar and their meaning

Icons

Meaning

Red X

The tool is disabled

Yellow triangle pointing

The pre-warning limit has been reached

downward

Yellow triangle pointing

The tool is in a special state

upward

Place the cursor on the marked tool. A tool tip will provide a brief description

Green frame

The tool is preselected.

Magazine/location number:

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

Tool wear

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.

Notes

M573

Page 10

828D/840Dsl SINUMERIK Operate

Operating area “Parameter”

M573

Vertical softkey bar

Display area

Description

By pressing the VSK 1 “Sort” and “Filter” you can sort and filter the tools in the tool list ac-

cording to different parameters.

By pressing the VSK 1 “Search” and “Details” you can search and view the tool details in the

tool list according to different parameters.

By pressing the VSK 6 “Reactivate“ locked tools, and tools that have reached their pre-

warning limit can be made operational again.

Notes

828D/840Dsl SINUMERIK Operate

Page 11

M573

M573

Operating area “Parameter”

Parameters for “Tool wear”

Parameter

Meaning

Location

Magazine/location number:

Type

Tool type:

Tool name

Tool name:

ST

Replacement tool number:

D

Cutting edge number

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.

 Tool monitoring by wear

With wear W, the greatest value in the wear parameters ΔLength X, ΔLength Z, ΔRadius or

W*

ΔØ in the wear list is monitored.

* The wear monitoring is configured via a machine data item.

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 manu-

facturer`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).

Notes

M573

Page 12

828D/840Dsl SINUMERIK Operate

Operating area “Parameter”

M573

Icons in the tool wear list and their meaning

(See section Tool List, Icons in the tool list, in this module)

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.

Activate the “D”-parameter checkbox for disabling the tool manually.

Sort and Filter

For the functions “Sort” and “Filter” in the tool list refer to the section 3 in this module.

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.

Notes

828D/840Dsl SINUMERIK Operate

Page 13

M573

M573

Operating area “Parameter”

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.

Magazine management

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 disa-

bled.

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.

Vertical softkey bar

Display area

Description

By pressing the VSK 5 “Unload all“ all tools can be transferred from the magazine location to

the tool libuary, “Unload all“ must be confirmed with the VSK 8 “OK”.

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 select-

ed target location must be confirmed with the VSK 8 “OK” or can aborted with VSK 7

“Cancel”.

Notes

M573

Page 14

828D/840Dsl SINUMERIK Operate

Operating area “Parameter”

M573

Vertical softkey bar continued

Display area

Description

By pressing the VSK 6 “Position magazine“ you can position magazine locations directly on

the loading point.

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 "Tool Wear").

Parameters for “Magazine”

Parameter

Meaning

Loc.

Number of the magazine location:

(Only display, see section “Tool list“)

Type

Tool type:

(Only display, see section “Tool list“)

Tool name

Tool name:

(See section “Tool list“)

ST

Sister tool:

(Only display, see section “Tool list“)

D

Edge number:

(Only display, see section “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.

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.

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:

Notes

828D/840Dsl SINUMERIK Operate

Page 15

M573

M573

Operating area “Parameter”

W

WCS

Transformation of coordi-

Tool offset

SZS

Work offset fine

Work offset coarse

Base offset

MCS

M

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”.

Every zero offset (G54 to G57, G505 to G599) consists of a coarse offset and a fine offset. You

Zero offsets

can call the work offsets from any sequence program (coarse and fine offsets are added to-

gether).

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.

Fine offsets must be set up by the machine manufacturer.

Note:

Also refer to the machine manufacturer's instructions.

You always program coordinate transformations for a specific sequence program.

Coordinate

They are defined by:

transformations:

 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.

Notes

M573

Page 16

828D/840Dsl SINUMERIK Operate

Operating area “Parameter”

M573

Work offset

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.

Selecting the function “Active”

By pressing the VSK 2 “Active“ the “Work offset - active” window opens.

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.

Notes

828D/840Dsl SINUMERIK Operate

Page 17

M573

M573

Operating area “Parameter”

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.

Selecting the function “Work offset - G54...G57”

By pressing VSK 4 “G54...G57“ the following window opens.

Displaying and editing settable zero offset

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 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.

M573: END

Notes

M573

Page 18

828D/840Dsl SINUMERIK Operate

M575

Operating area “Program manager“

Selection and function of the program manager

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.

Horizontal softkey bar

Display area

Description

By pressing the HSK 1 “NC“ all directories, folders and files of the NC/Hard disc will be dis-

played 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. Prerequi-

site for this function is that the "Additional 256 MB HMI user memory on CF card of NCU"

option is activated. For larger CF-cards 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.

Storage medium “NC

Selecting the function „NC“

By pressing the HSK 1 “NC“ the program manager opens .

Notes

M575

Page 4

828D/840Dsl SINUMERIK Operate

Operating area “Program manager“

M575

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:

 Name

The name can contain up to 28 characters (24 characters for the name + dot + 3-character extension, e.g. MPF). Per-

missible characters include all upper-case letters (without accents), numbers, and underscores.

 Type

*.WPD

Directory

(Workpiece Directory)

Directory/

*.MPF

Program

(Main program File)

Programs

*.SPF

Subprogram

(Subprogram File)

 Size

 The size of files of the selected directory is displayed in byte.

 Date/Time

 Date and time of file creation or last change

Notes

828D/840Dsl SINUMERIK Operate

Page 5

M575

M575

Operating area “Program manager“

Vertical softkey bar 1

Display area

Description

By pressing the VSK 1.1 “Execute“ you can select a program and change over to the operat-

ing 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 .

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.

By pressing the VSK 1.5 “Copy” one or several programs or directories can be copied.

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.

By pressing the VSK 1.7 “Cut“ one to several programs or directories can be cut out and in-

serted somewhere else on a location in the directory tree of the NC, a local drive or on an

external USB drive.

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.

Vertical softkey bar 2

Display area

Description (continuation)

By pressing the VSK 2.1 “Archive” a new vertical softkey bar is opened.

By pressing the VSK 2.2 “Preview window“ a sub window opens below the file browser win-

dow, with a preview of the program code of the selected program.

By pressing the VSK 2.3 “Search“ you can search for “File name”, using the Vertical softkeys.

Notes

M575

Page 6

828D/840Dsl SINUMERIK Operate

Operating area “Program manager“

M575

Vertical softkey bar 2

Display area

Description (continuation)

By pressing the VSK 2.5 “Multiple clamping“ you can optimize tool changes over several

workpiece clamping.

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.

By pressing the VSK 2.7 “Delete“ the program or folder marked with the cursor will be deleted.

By pressing the VSK 2.8 “Back“ on the operator panel (OP) you switch back to the vertical soft-

key bar 1.

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 2.1 “Directory” 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.

Notes

828D/840Dsl SINUMERIK Operate

Page 7

M575

M575

Operating area “Program manager“

Starting a new NC-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).



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).

After pressing the VSK 1.2 “New” the following functions in the vertical softkey bar are available.

Notes

M575

Page 8

828D/840Dsl SINUMERIK Operate

Operating area “Program manager“

M575

Vertical softkey bar

Display area

Description

By pressing the VSK 2 “Directory“ 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.

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 under-

scores (_).

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 above)

Notes

828D/840Dsl SINUMERIK Operate

Page 9

M575

M575

Operating area “Program manager“

Parameters for “Any new program“

Parameter

Meaning

Template

If templates are available, they are shown and selectable.

Type:

Program type:

 MPF

Program (Main program file)

Name

Program name (see section above)

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.

Notes

M575

Page 10

828D/840Dsl SINUMERIK Operate

Operating area “Program manager“

M575

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.

Copying and pasting directories / NC- programs

First open the desired directory in the program manager, like described 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”.

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.

Cutting out directories / NC-programs

First open the desired directory in the program manager, like described in this module.

1.

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”.

2.

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.

6.

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

828D/840Dsl SINUMERIK Operate

Page 11

M575

M575

Operating area “Program manager“

Deleting directories / NC-programs

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”.

Press the VSK 2.7 “Delete“ in the extended vertical softkey bar 2. Accept the deletion process with pressing

2.

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 pro-

gram or directory.

Generating archive files of programs and directories

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.

Notes

M575

Page 12

828D/840Dsl SINUMERIK Operate

Operating area “Program manager“

M575

Generating archive files of programs and directories

Vertical softkey bar

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.

Generating archive files of programs and directories

Vertical softkey bar

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.

3.11

Multiple clamping

By pressing the VSK 2.5 “Multiple clamping“ you can optimize tool changes over several work-

piece clamping

Notes

828D/840Dsl SINUMERIK Operate

Page 13

M575

M575

Operating area “Program manager“

Multiple clamping

Parameters

Meaning

Number of clampings:

Total number of workpieces being machined..

First work offset:

Choose the first work offset to be used for “multiple clamping..

Name:

Name of the new program with optimized tool clamping over several workpiece clamping.

By pressing the VSK 8 “OK” all parameters and names will be accepted.

Multiple clamping continued

By pressing the VSK 2.1 “Select program“ you can choose the programs for optimizing tool

changes over several workpiece clamping.

Notes

M575

Page 14

828D/840Dsl SINUMERIK Operate

Operating area “Program manager“

M575

Multiple clamping continued

By pressing the VSK 2.3 “Search“ you can search for “File name”, using the Vertical softkeys.

By pressing the VSK 2.6 “On all clampings“ you can apply the same file name to all clamping.

By pressing the VSK 2.5 “Delete entry“ you can delete the file name that the curser has high-

lighted .

By pressing the VSK 2.6 “Delete all“ you can delete all file names for each clamping name.

Multiple clamping continued

By pressing the VSK 8 “OK” all parameters and names will be accepted.

The multiple clamping program is then calculated.

Notes

828D/840Dsl SINUMERIK Operate

Page 15

M575

M575

Operating area “Program manager“

Multiple clamping continued

Properties of programs and directories

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.

Notes

M575

Page 16

828D/840Dsl SINUMERIK Operate

Operating area “Program manager“

M575

Properties of programs and directories

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

Protected by password

 Protection level 3

User

Protected by password

 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

Storage medium “Local drive”

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.

Notes

828D/840Dsl SINUMERIK Operate

Page 17

M575

M575

Operating area “Program manager“

Vertical softkey bar

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”.

Storage medium “USB” drive

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.

Vertical softkey bar

The full functionality available under the NC program manager window is available by pressing the HSK 2 “local drive” or

HSK 3 “USB”.

M575: END

Notes

M575

Page 18

828D/840Dsl SINUMERIK Operate

Basics of programming with ShopMill

M600

Basics of

programming with

Shopmill:

START

Basics

Creating

ShopMill

programs

Editor

Various

Simulation

NC Execute

Basics of

programming with

Shopmill:

END

Notes

828D/840Dsl SINUMERIK Operate

Page 3

M600

M600

Basics of programming with ShopMill

Basics

Programming with ShopMill

ShopMill offers the option to create NC programs directly on the control in the manner of chained sequential block pro-

grams. 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 - M604 “Basics of programming program-

GUIDE“.

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.

Notes

M600

Page 4

828D/840Dsl SINUMERIK Operate

Basics of programming with ShopMill

M600

 As a programming graphic in the graphic view (with activated VSK 2.2 “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.

Notes

828D/840Dsl SINUMERIK Operate

Page 5

M600

M600

Basics of programming with ShopMill

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)

Program header

The program header 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).

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).

Sequential program blocks

For the functions “Drill”, “Mill”, and “Contour milling”, technology blocks and contours are programmed sepa-

rately. 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 pro-

cessed, such as for instance centring and drilling. Position blocks or geometry blocks respectively, de-

scribe 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.

Notes

M600

Page 6

828D/840Dsl SINUMERIK Operate

Basics of programming with ShopMill

M600

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).

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 work pieces. The program end is marked with the icon

and the text “End of program” and if se-

lected with the text “Repetition = Yes” (see picture below).

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.

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.

Notes

828D/840Dsl SINUMERIK Operate

Page 7

M600

Content      ..     14      15      16      17     ..