Content      ..      1      2      3      ..

SINUMERIK 840D sl/828D Universal. Operating Manual (2013) - page 2

Machining the workpiece

4.7 Starting execution at a specific point

Cascaded search

You can start another search from the "Search target found" state. The cascading can be

continued any number of times after every search target found.

Note

Another cascaded block search can be started from the stopped program execution only if

the search target has been found.

References

Function Manual Basic Functions; Block Search

Preconditions

1. You have selected the desired program.

2. The controller is in the reset state.

3. The desired search mode is selected.

NOTICE

Risk of collision

Pay attention to a collision-free start position and appropriate active tools and other

technological values.

If necessary, manually approach a collision-free start position. Select the target block

considering the selected block search type.

Toggling between search pointer and search positions

Press the "Search pointer" softkey again to exit the "Search Pointer"

window and return to the "Program" window to define search positions.

- OR -

Press the "Back" softkey.

You have now exited the block search function.

See also

Block search mode (Page 107)

Selecting a program (Page 93)

Universal

102

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

Machining the workpiece

4.7 Starting execution at a specific point

4.7.2

Continuing program from search target

To continue the program at the desired position, press the <CYCLE START> key twice.

● The first CYCLE START outputs the auxiliary functions collected during the search. The

program is then in the Stop state.

● Before the second CYCLE START, you can use the "Overstore" function to create states

that are required, but not yet available, for the further program execution.

By changing to the JOG REPOS mode, you can also manually traverse the tool from the

current position to the setpoint position, if the setpoint position is not to be automatically

approached after the program start

4.7.3

Simple search target definition

Requirement

The program is selected and the controller is in Reset mode.

Procedure

1.

Press the "Block search" softkey.

2.

Place the cursor on a particular program block.

- OR -

Press the "Find text" softkey, select the search direction, enter the

search text and confirm with "OK".

3.

Press the "Start search" softkey.

The search starts. Your specified search mode will be taken into

account.

The current block will be displayed in the "Program" window as soon

as the target is found.

4.

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.

Press the <CYCLE START> key twice.

Processing is continued from the defined position.

Universal

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

103

Machining the workpiece

4.7 Starting execution at a specific point

4.7.4

Defining an interruption point as search target

Requirement

A program was selected in "AUTO" mode and interrupted during execution through CYCLE

STOP or RESET.

Software option

You require the "Extended operator functions" option (only for 828D).

Procedure

1.

Press the "Block search" softkey.

2.

Press the "Interrupt point" softkey.

The interruption point is loaded.

3.

If the "Higher level" and "Lower level" softkeys are available, use these

to change the program level.

4.

Press the "Start search" softkey.

The search starts. Your specified search mode will be taken into

account.

The search screen closes.

The current block will be displayed in the "Program" window as soon as

the target is found.

5.

Press the <CYCLE START> key twice.

The execution will continue from the interruption point.

Universal

104

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

Machining the workpiece

4.7 Starting execution at a specific point

4.7.5

Entering the search target via search pointer

Enter the program point which you would like to proceed to in the "Search Pointer" window.

Software option

You require the "Extended operator functions" option for the "Search pointer"

function (only for 828D).

Requirement

The program is selected and the controller is in the reset state.

Screen form

Each line represents one program level. The actual number of levels in the program depends

on the nesting depth of the program.

Level 1 always corresponds to the main program and all other levels correspond to

subprograms.

You must enter the target in the line of the window corresponding to the program level in

which the target is located.

For example, if the target is located in the subprogram called directly from the main program,

you must enter the target in program level 2.

The specified target must always be unambiguous. This means, for example, that if the

subprogram is called in the main program in two different places, you must also specify a

target in program level 1 (main program).

Procedure

1.

Press the "Block search" softkey.

2.

Press the "Search pointer" softkey.

3.

Enter the full path of the program as well as the subprograms, if

required, in the input fields.

4.

Press the "Start search" softkey.

The search starts. Your specified search mode will be taken into

account.

Universal

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

105

Machining the workpiece

4.7 Starting execution at a specific point

The Search window closes. The current block will be displayed in the

"Program" window as soon as the target is found.

5.

Press the <CYCLE START> key twice.

Processing is continued from the defined location.

Note

Interruption point

You can load the interruption point in search pointer mode.

4.7.6

Parameters for block search in the search pointer

Parameter

Meaning

Number of program level

Program:

The name of the main 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

Type

" " search target is ignored on this level

N no. Block number

Label Jump label

Text string

Subprg. Subprogram call

Line Line number

Search target

Point in the program at which machining is to start

Universal

106

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

Machining the workpiece

4.7 Starting execution at a specific point

Note

Search mode for the ShopMill and ShopTurn programs

The search variant for the ShopMill/ShopTurn machining step programs can be specified via

MD 51024. This applies only to the ShopMill/ShopTurn single-channel view.

Machine manufacturer

Please refer to the machine manufacturer's specifications.

References

For additional information, please refer to the following documentation:

Commissioning Manual SINUMERIK Operate (IM9) / SINUMERIK 840D sl

Procedure

1.

Select the "Machine" operating area.

2.

Press the <AUTO> key.

3.

Press the "Block search" and "Block search mode" softkeys.

The "Search Mode" window appears.

Universal

108

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

Machining the workpiece

4.8 Controlling the program run

Activating program control

You can control the program sequence however you wish by selecting and clearing the

relevant checkboxes.

Display / response of active program controls:

If a program control is activated, the abbreviation of the corresponding function appears in

the status display as response.

Procedure

1.

Select the "Machine" operating area.

2.

Press the <AUTO> or <MDI> key.

3.

Press the "Prog. ctrl.” softkey.

The "Program Control" window appears.

4.8.2

Skip blocks

It is possible to skip program blocks, which are not to be executed every time the program

runs.

The skip blocks are identified by placing a "/" (forward slash) or "/x (x = number of skip level)

character in front of the block number. Several consecutive blocks can also be skipped.

The statements in the skipped blocks are not executed, i.e. the program continues with the

next block, which is not skipped.

The number of skip levels that can be used depends on a machine datum.

Machine manufacturer

Please refer to the machine manufacturer's specifications.

Software option

In order to have more than two skip levels, for 828D you require the

"Extended operator functions" option.

Universal

110

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

Machining the workpiece

4.8 Controlling the program run

Skip levels, activate

Select the corresponding checkbox to activate the desired skip level.

Note

The "Program Control - Skip Blocks" window is only available when more than one skip level

is set up.

Procedure

1.

Select the "Machine" operating area.

2.

Press the <AUTO> or <MDA> key.

3

Press the "Prog. ctrl." and "Skip blocks" softkeys.

The "Program Control" window appears and shows a list of skip levels.

Universal

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

111

Machining the workpiece

4.9 Overstore

4.9

Overstore

With overstore, you have the option of executing technological parameters (for example,

auxiliary functions, axis feed, spindle speed, programmable instructions, etc.) before the

program is actually started. The program instructions act as if they are located in a normal

part program. These program instructions are, however, only valid for one program run. The

part program is not permanently changed. When next started, the program will be executed

as originally programmed.

After a block search, the machine can be brought into another state with overstore (e.g. M

function, tool, feed, speed, axis positions etc.), in which the normal part program can be

successfully continued.

Software option

You require the "Extended operator functions" option for the overstore function

(for 828D).

Precondition

The program to be corrected is in the Stop or Reset mode.

Procedure

1.

Open the program in the "AUTO" mode.

2.

Press the "Overstore" softkey.

The "Overstore" window opens.

3.

Enter the required data and NC block.

4.

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.

You cannot change the operating mode while you are in overstore

mode.

5.

Press the "Back" softkey.

The "Overstore" window closes.

6.

Press the <CYCLE START> key again.

The program selected before overstoring continues to run.

Universal

112

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

Machining the workpiece

4.10 Editing a program

Note

Block-by-block execution

The <SINGLE BLOCK> key is also active in the overstore mode. If several blocks are

entered in the overstore buffer, then these are executed block-by-block after each NC start

Deleting blocks

Press the "Delete blocks" softkey to delete program blocks you have

entered.

4.10

Editing a program

With the editor, you are able to render, supplement, or change part programs.

Note

Maximum block length

The maximum block length is 512 characters.

Calling the editor

● The editor is started via the "Program correction" function in the "Machine" operating area

and with the <INSERT> key.

● The editor is called via the "Open" softkey as well as with the <INPUT> or <Cursor right>

key in the "Program manager" operating area.

● The editor opens in the "Program" operating area with the last executed part program, if

this was not explicitly exited via the "Close" softkey.

Note

Please note that the changes to programs stored in the NC memory take immediate

effect. You can exit the editor only after you have saved the changes.

If you are editing on a local drive or external drives, you can also exit the editor without

saving, depending on the setting.

Exit the program correction mode using the "Close" softkey to return to the "Program

manager" operating area.

Universal

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

113

Machining the workpiece

4.10 Editing a program

- OR -

Activate the "Exact expression" checkbox if, for example, you want to

search for place holders ("*", "?") in program lines.

4.

Position the cursor in the "Direction" field and choose the search

direction (forward, backward) with the <SELECT> key.

5.

Press the "OK" softkey to start the search.

If the text you are searching for is found, the corresponding line is

highlighted.

6.

Press the "Continue search" softkey if the text located during the search

does not correspond to the point you are looking for.

- OR -

Press the "Cancel" softkey when you want to cancel the search.

Further search options

Softkey

Function

The cursor is set to the first character in the program.

The cursor is set to the last character in the program.

4.10.2

Replacing program text

You can find and replace text in one step.

Requirement

The desired program is opened in the editor.

Procedure

1.

Press the "Search" softkey.

A new vertical softkey bar appears.

2.

Press the "Find and replace" softkey.

The "Find and Replace" window appears.

Universal

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

115

Machining the workpiece

4.10 Editing a program

3.

In the "Text" field, enter the term you are looking for and in the "Replace

with" field, enter the text you would like to insert automatically during the

search.

4.

Position the cursor in the "Direction" field and choose the search

direction (forward, backward) with the <SELECT> key.

5.

Press the "OK" softkey to start the search.

If the text you are searching for is found, the corresponding line is

highlighted.

6.

Press the "Replace" softkey to replace the text.

- OR -

Press the "Replace all" softkey to replace all text in the file that

corresponds to the search term.

- OR -

Press the "Continue search" softkey if the text located during the search

should not be replaced.

- OR -

Press the "Cancel" softkey when you want to cancel the search.

Note

Replacing texts

• Read-only lines (;*RO*)

If hits are found, the texts are not replaced.

• Contour lines (;*GP*)

If hits are found, the texts are replaced as long as the lines are not read-only.

• Hidden lines (;*HD*)

If hidden lines are displayed in the editor and hits are found, the texts are replaced as

long as the lines are not read-only. Hidden lines that are not displayed, are not replaced.

See also

Editor settings (Page 121)

Universal

116

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

Machining the workpiece

4.10 Editing a program

4.10.3

Copying/pasting/deleting program blocks

Requirement

The program is opened in the editor.

Procedure

1.

Press the "Mark" softkey.

- OR -

Press the <SELECT> key.

2.

Select the desired program blocks with the cursor or mouse.

3.

Press the "Copy" softkey in order to copy the selection to the buffer

memory.

4.

Place the cursor on the desired insertion point in the program and press

the "Paste" softkey.

The content of the buffer memory is pasted.

- OR -

Press the "Cut" softkey to delete the selected program blocks.

Note: When editing a program, you cannot copy or cut more than 1024

lines. While a program that is not on the NC is opened (progress display

less than 100%), you cannot copy or cut more than 10 lines or insert

more than 1024 characters.

Note

The buffer memory contents are retained even after the editor is closed, enabling you to

paste the contents in another program, as well.

Note

Copy/cut current line

To copy and cut the current line where the cursor is positioned, it is not necessary to mark or

select it. You have the option of making the "Cut" softkey only operable for marked program

sections via editor settings.

Universal

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

117

Machining the workpiece

4.10 Editing a program

See also

Opening additional programs (Page 120)

4.10.4

Renumbering a program

You can modify the block numbering of programs opened in the editor at a later point in time.

Requirement

The program is opened in the editor.

Procedure

1.

Press the ">>" softkey.

A new vertical softkey bar appears.

2.

Press the "Renumber" softkey.

The "Renumbering" window appears.

3.

Enter the values for the first block number and the increment to be used

for numbering.

4.

Press the "OK" softkey.

The program is renumbered.

Note

If you only want to renumber a section, select the program blocks whose block numbering

you want to edit.

Universal

118

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

Machining the workpiece

4.10 Editing a program

4.10.5

Creating a program block

In order to structure programs in order to achieve a higher degree of transparency, you have

the option of combining several G-code blocks to form program blocks.

You then have the option of opening and closing these blocks depending on your

requirement.

Settings for a program block

Display

Meaning

Text

Block designation

Spindle

• S1

• S2

Spindle assignment. Defines at which spindle a program block is to be

executed.

Addit. run-in code

• Yes

For the case that the block is not executed, as the specified spindle should

not be processed, then it is possible to temporarily activate a so-called

"Addit. run-in code".

• No

Automat. Retraction

• Yes

Block start and block end are moved to the tool change point, i.e. the tool

is brought into a safe range.

• No

Procedure

1.

Select the "Program Manager" operating area.

2.

Select the storage location and create a program or open a program.

The program editor is opened.

3.

Select the required program blocks that you wish to combine to form a

block.

4.

Press the "Build group" softkey.

The "Build group" window is opened.

Universal

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

119

Machining the workpiece

4.10 Editing a program

5.

Enter a designation for the block, assign the spindle, if required, select

the Addit. run-in code and the automatic retraction and then press the

"OK" softkey.

Opening and closing blocks

6.

Press the ">>" and "View" softkeys.

7.

Press the "Open blocks" softkey if you wish to display the program with

all blocks.

8.

Press the "Close blocks" softkey, if you wish to display the program

again in a structured form.

4.10.6

Opening additional programs

You have the option of viewing and editing two programs simultaneously in the editor.

For instance, you can copy program blocks or machining steps of a program and paste them

into another program.

Opening several programs

You have the option of opening up to ten program blocks.

1.

In the program manager, select the programs that you wish to open and

view in the multiple editor and then press on the "Open" softkey.

The editor is opened and the first two programs are displayed.

2.

Press the <NEXT WINDOW> key to change to the next opened

program.

3.

Press the "Close" softkey to close the actual program.

Note

Pasting program blocks

JobShop machining steps cannot be copied into a G code program.

Requirement

You have opened a program in the editor.

Universal

120

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

Machining the workpiece

4.10 Editing a program

Procedure

1.

Press the ">>" and "Open additional program" softkeys.

The "Select Additional Program" window is opened.

2.

Select the program or programs that you wish to display in addition to

the already opened program.

3.

Press the "OK" softkey.

The editor opens and displays both programs next to each another.

See also

Copying/pasting/deleting program blocks (Page 117)

4.10.7

Editor settings

Enter the default settings in the "Settings" window that are to take effect automatically when

the editor is opened.

Defaults

Setting

Meaning

Number

• Yes: A new block number will automatically be assigned after every line

automatically

change. In this case, the specifications provided under "First block

number" and "Increment" are applicable.

• No: No automatic numbering.

First block number

Specifies the starting block number of a newly created program.

The field is only editable when "Yes" is displayed under "Number

automatically".

Increment

Defines the increment used for the block numbers.

The field is only editable when "Yes" is displayed under "Number

automatically".

Display hidden lines

• Yes: Hidden lines marked with "*HD" (hidden) will be displayed.

• No: Lines marked with ";*HD*" will not be displayed.

Note:

Only visible program lines are taken into account with the "Search" and

"Search and Replace" functions.

Display block end a

The "CFLF" (line feed) symbol ¶ is displayed at the block end.

symbol

Universal

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

121

Machining the workpiece

4.10 Editing a program

Setting

Meaning

Scroll horizontally

Yes: A horizontal scrollbar is displayed. In this way, you can scroll horizontally

to the end of long lines that would otherwise wrap.

Automatic save (only

• Yes: The changes are saved automatically when you change to another

local and external

operating area.

drives)

• No: You are prompted to save when changing to another operating area.

Save or reject the changes with the "Yes" and "No" softkeys.

Visible programs

•

1 - 10

Select how many programs can be displayed next to one another in the

editor.

• Auto

Specifies that the number of programs entered in a job list or up to 10

selected programs will be displayed next to each other.

Width of the program

Here, you enter the width of the program that has the input focus in the editor

with focus

as a percentage of the window width.

Cut only after

• Yes: The cutting of program sections is possible only when program lines

selecting

have been selected, i.e. the "Cut" softkey only then is active.

• No: The "Cut" softkey is available by default.

Note

All entries that you make here are effective immediately.

Procedure

1.

Select the "Program" operating area.

You have activated the editor.

2.

Press the ">>" and "Settings" softkeys.

The "Settings" window opens.

3.

Make the desired changes here and press the "OK" softkey to confirm

your settings.

See also

Replacing program text (Page 115)

Universal

122

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

Machining the workpiece

4.11 Display and edit user variables

4.11

Display and edit user variables

4.11.1

Overview

The defined user data may be displayed in lists.

The following variables can be defined:

● Data parameters (R parameters)

● Global user data (GUD) is valid in all programs

● Local user data (LUD) is valid in one program

● Program-global user data (PUD) is valid in one program and the called subroutines.

Channel-specific user data can be defined with a different value for each channel.

Entering and displaying parameter values

Up to 15 positions (including decimal places) are evaluated. If you enter a number with more

than 15 places, it will be written in exponential notation (15 places + EXXX).

LUD or PUD

Only local or program-global user data can be displayed at one time.

Whether the user data are available as LUD or PUD depends on the current control

configuration.

Machine manufacturer

Please also refer to the machine manufacturer's instructions.

Note

Reading and writing variables protected

Reading and writing of user data are protected via a keyswitch and protection levels.

Searching for user data

You may search for user data within the lists using any character string.

Refer to the "Defining and activating user data" section to learn how to edit displayed user

data.

Universal

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

123

Machining the workpiece

4.11 Display and edit user variables

4.11.2

R parameters

R parameters (arithmetic parameters) 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 controller is switched off.

Number of channel-specific R parameters

The number of channel-specific R parameters is defined in a machine data element.

Range: R0-R999 (dependent on machine data).

There are no gaps in the numbering within the range.

Machine manufacturer

Please refer to the machine manufacturer's specifications.

Procedure

1.

Select the "Parameter" operating area.

2.

Press the "User variable" softkey.

3.

Press the "R variables" softkey.

The "R Parameters" window appears.

Delete R variables

1.

Press the ">>" and "Delete" softkeys.

The "Delete R parameters" window appears.

2.

Enter the R parameter(s) whose channel-specific values you would like

to delete and press the "OK" softkey.

A value of 0 is assigned to the selected R parameters or to all R

parameters.

Universal

124

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

Machining the workpiece

4.11 Display and edit user variables

4.11.3

Displaying global user data (GUD)

Global user variables

Global GUDs are NC global user data (Global User Data) that remains available after

switching the machine off.

GUDs apply in all programs.

Definition

A GUD variable is defined with the following:

● Keyword DEF

● Range of validity NCK

● Data type (INT, REAL, ….)

● Variable names

● Value assignment (optional)

Example

DEF NCK INT ZAEHLER1 = 10

GUDs are defined in files with the ending DEF. The following file names are reserved for this

purpose:

File name

Meaning

MGUD.DEF

Definitions for global machine manufacturer data

UGUD.DEF

Definitions for global user data

GUD4.DEF

User-definable data

GUD8.DEF, GUD9.DEF

User-definable data

Procedure

1.

Select the "Parameter" operating area.

2.

Press the "User variable" softkey.

3.

Press the "Global GUD" softkeys.

Universal

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

125

Machining the workpiece

4.11 Display and edit user variables

The "Global User Variables" window is displayed. A list of the defined

UGUD variables will be displayed.

- OR -

Press the "GUD selection" softkey and the "SGUD" to "GUD6" softkeys

if you wish to display SGUD, MGUD, UGUD as well as GUD4 to GUD 6

of the global user variables.

- OR -

Press the "GUD selection" and ">>" softkeys as well as the "GUD7" to

"GUD9" softkeys if you want to display GUD 7 to GUD 9 of the global

user variables.

Note

After each start-up, a list with the defined UGUD variables is displayed in the "Global User

Variables" window.

4.11.4

Displaying channel GUDs

Channel-specific user variables

Like the GUDs, channel-specific user variables are applicable in all programs for each

channel. However, unlike GUDs, they have specific values.

Definition

A channel-specific GUD variable is defined with the following:

● Keyword DEF

● Range of validity CHAN

● Data type

● Variable names

● Value assignment (optional)

Example

DEF CHAN REAL X_POS = 100.5

Universal

126

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

Machining the workpiece

4.11 Display and edit user variables

Procedure

1.

Select the "Parameter" operating area.

2.

Press the "User variable" softkey.

3.

Press the "Channel GUD" and "GUD selection" softkeys.

A new vertical softkey bar appears.

4.

Press the "SGUD" ... "GUD6" softkeys if you want to display the SGUD,

MGUD, UGUD as well as GUD4 to GUD 6 of the channel-specific user

variables.

- OR -

Press the "Continue" softkey and the "GUD7" to "GUD9" softkeys if you

want to display GUD 7 to GUD 9 of the channel-specific user variables.

4.11.5

Displaying local user data (LUD)

Local user variables

LUDs are only valid in the program or subprogram in which they were defined.

The controller displays the LUDs after the start of program processing. The display is

available until the end of program processing.

Definition

A local user variable is defined with the following:

● Keyword DEF

● Data type

● Variable names

● Value assignment (optional)

Universal

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

127

Machining the workpiece

4.11 Display and edit user variables

Procedure

1.

Select the "Parameter" operating area.

2.

Press the "User variable" softkey.

3.

Press the "Local LUD" softkey.

4.11.6

Displaying program user data (PUD)

Program-global user variables

PUDs are global part program variables (Program User Data). PUDs are valid in all main

programs and subprograms, where they can also be written and read.

Machine manufacturer

Please refer to the machine manufacturer's specifications.

Procedure

1.

Select the "Parameter" operating area.

2.

Press the "User variable" softkey.

3.

Press the "Program PUD" softkey.

Universal

128

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

Machining the workpiece

4.11 Display and edit user variables

4.11.7

Searching for user variables

You can search for R parameters and user variables.

Procedure

1.

Select the "Parameter" operating area.

2.

Press the "R parameters", "Global GUD", "Channel GUD", "Local GUD"

or "Program PUD" softkeys to select the list in which you would like to

search for user variables.

3.

Press the "Search" softkey.

The "Search for R Parameters" or "Search for User Variables" window

opens.

4.

Enter the desired search term and press "OK".

The cursor is automatically positioned on the R parameter or user

variables you are searching for, if they exist.

By editing a DEF/MAC file, you can alter or delete existing definition/macro files or add new

ones.

Procedure

1.

Select the "Start-up" operating area.

2.

Press the "System data" softkey.

3.

In the data tree, select the "NC data" folder and then open the

"Definitions" folder.

4.

Select the file you want to edit.

5.

Double-click the file.

- OR -

Press the "Open" softkey.

- OR -

Universal

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

129

Machining the workpiece

4.11 Display and edit user variables

Press the <INPUT> key.

- OR -

Press the <Cursor right> key.

The selected file is opened in the editor and can be edited there.

6.

Define the desired user variable.

7.

Press the "Exit" softkey to close the editor.

Activating user variables

1.

Press the "Activate" softkey.

A prompt is displayed.

2.

Select whether the current values in the definition files should be

retained

- OR -

Select whether the current values in the definition files should be

deleted.

This will overwrite the definition files with the initial values.

3.

Press the "OK" softkey to continue the process.

Universal

130

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

Machining the workpiece

4.12 Display G and auxiliary functions

4.12

Display G and auxiliary functions

4.12.1

Selected G functions

16 selected G groups are displayed in the "G Function" window.

Within a G group, the G function currently active in the controller is displayed.

Some G codes (e.g. G17, G18, G19) are immediately active after switching the machine

control on.

Which G codes are always active depends on the settings.

Machine manufacturer

Please refer to the machine manufacturer's specifications.

G groups displayed by default

Group

Meaning

G group 1

Modally active motion commands (e.g. G0, G1, G2, G3)

G group 2

Non-modally active motion commands, dwell time (e.g. G4, G74, G75)

G group 3

Programmable offsets, working area limitations and pole programming (e.g.

TRANS, ROT, G25, G110)

G group 6

Plane selection (e.g. G17, G18)

G group 7

Tool radius compensation (e.g. G40, G42)

G group 8

Settable work offset (e.g. G54, G57, G500)

G group 9

Offset suppression (e.g. SUPA, G53)

G group 10

Exact stop - continuous-path mode (e.g. G60, G641)

G group 13

Workpiece dimensioning inches/metric (e.g. G70, G700)

G group 14

Workpiece dimensioning absolute/incremental (G90)

G group 15

Feedrate type (e.g. G93, G961, G972)

G group 16

Feedrate override on inside and outside curvature (e.g. CFC)

G group 21

Acceleration profile (e.g. SOFT, DRIVE)

G group 22

Tool offset types (e.g. CUT2D, CUT2DF)

G group 29

Radius/diameter programming (e.g. DIAMOF, DIAMCYCOF)

G group 30

Compressor ON/OFF (e.g. COMPOF)

Universal

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

131

Machining the workpiece

4.12 Display G and auxiliary functions

G groups displayed by default (ISO code)

Group

Meaning

G group 1

Modally active motion commands (e.g. G0, G1, G2, G3)

G group 2

Non-modally active motion commands, dwell time (e.g. G4, G74, G75)

G group 3

Programmable offsets, working area limitations and pole programming (e.g.

TRANS, ROT, G25, G110)

G group 6

Plane selection (e.g. G17, G18)

G group 7

Tool radius compensation (e.g. G40, G42)

G group 8

Settable work offset (e.g. G54, G57, G500)

G group 9

Offset suppression (e.g. SUPA, G53)

G group 10

Exact stop - continuous-path mode (e.g. G60, G641)

G group 13

Workpiece dimensioning inches/metric (e.g. G70, G700)

G group 14

Workpiece dimensioning absolute/incremental (G90)

G group 15

Feedrate type (e.g. G93, G961, G972)

G group 16

Feedrate override on inside and outside curvature (e.g. CFC)

G group 21

Acceleration profile (e.g. SOFT, DRIVE)

G group 22

Tool offset types (e.g. CUT2D, CUT2DF)

G group 29

Radius/diameter programming (e.g. DIAMOF, DIAMCYCOF)

G group 30

Compressor ON/OFF (e.g. COMPOF)

Procedure

1.

Select the "Machine" operating area.

2.

Press the <JOG>, <MDA> or <AUTO> key.

3.

Press the "G functions" softkey.

The "G Functions" window is opened.

4.

Press the "G functions" softkey again to hide the window.

Universal

132

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

Machining the workpiece

4.12 Display G and auxiliary functions

The G groups selection displayed in the "G Functions" window may differ.

Machine manufacturer

Please refer to the machine manufacturer's specifications.

References

For more information about configuring the displayed G groups, refer to the following

document:

SINUMERIK Operate (IM9) / SINUMERIK 840D sl Commissioning Manual

4.12.2

All G functions

All G groups and their group numbers are listed in the "G Functions" window.

Within a G group, only the G function currently active in the controller is displayed.

Additional information in the footer

The following additional information is displayed in the footer:

● Current transformations

Display

Meaning

TRANSMIT

Polar transformation active

TRACYL

Cylinder surface transformation active

TRAORI

Orientation transformation active

TRAANG

Inclined axis transformation active

TRACON

Cascaded transformation active

For TRACON, two transformations (TRAANG and TRACYL or TRAANG and

TRANSMIT) are activated in succession.

● Current zero offsets

● Spindle speed

● Path feedrate

● Active tool

Universal

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

133

Machining the workpiece

4.12 Display G and auxiliary functions

Procedure

1.

Select the "Machine" operating area.

2.

Press the <JOG>, <MDA> or <AUTO> key.

3.

Press the ">>" and "All G functions" softkeys.

The "G Functions" window is opened.

4.12.3

G functions for mold making

In the window "G functions", important information for machining free-form surfaces can be

displayed using the "High Speed Settings" function (CYCLE832).

Software option

You require the "Advanced Surface" software option in order to use this function.

High-speed cutting information

In addition to the information that is provided in the "All G functions" window, the following

programmed values of the following specific information is also displayed:

● CTOL

● OTOL

● STOLF

The tolerances for G0 are only displayed if they are active.

Particularly important G groups are highlighted.

You have the option to configure which G functions are highlighted.

Universal

134

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

Machining the workpiece

4.12 Display G and auxiliary functions

References

● Additional information is available in the following references:

Function Manual, Basic Functions; Chapter, "Contour/orientation tolerance"

● For information about configuring the displayed G groups, refer to the following

document:

Commissioning Manual SINUMERIK Operate (IM9) / SINUMERIK 840D sl

Procedure

1.

Select the "Machine" operating area

2.

Press the <JOG>, <MDI> or <AUTO> key.

3.

Press the ">>" and "All G functions" softkeys.

The "G Functions" window is opened.

Universal

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

135

Machining the workpiece

4.12 Display G and auxiliary functions

4.12.4

Auxiliary functions

Auxiliary functions include M and H functions preprogrammed by the machine manufacturer,

which transfer parameters to the PLC to trigger reactions defined by the manufacturer.

Displayed auxiliary functions

Up to five current M functions and three H functions are displayed in the "Auxiliary

Functions" window.

Procedure

1.

Select the "Machine" operating area.

2.

Press the <JOG>, <MDA> or <AUTO> key.

3.

Press the "H functions" softkey.

The "Auxiliary Functions" window opens.

4.

Press the "H functions" softkey again to hide the window again.

Universal

136

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

Machining the workpiece

4.13 Displaying status of synchronized actions

Display of synchronized actions

Using softkeys, you have the option of restricting the display to activated synchronized

actions.

Procedure

1.

Select the "Machine" operating area.

2.

Press the <AUTO>, <MDA> or <JOG> key.

3.

Press the menu forward key and the "Synchron." softkey.

The "Synchronized Actions" window appears.

You obtain a display of all activated synchronized actions.

4.

Press the "ID" softkey if you wish to hide the modal synchronized

actions in the automatic mode.

- AND / OR -

Press the "IDS" softkey if you wish to hide static synchronized actions.

- AND / OR -

Press the "Blockwise" softkey if you wish to hide the non-modal

synchronized actions in the automatic mode.

5.

Press the "ID", "IDS" or "Blockwise" softkeys to re-display the

corresponding synchronized actions.

Universal

138

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

Machining the workpiece

4.15 Setting for automatic mode

Procedure

1.

Select the "Machine" operating area.

2.

Press the <AUTO> key.

3.

Press the "Times, Counter" softkey.

The "Times, Counter" window opens.

4.

Select "Yes" under "Count workpieces" if you want to count completed

workpieces.

5.

Enter the number of workpieces needed in the "Desired workpieces"

field.

The number of workpieces already finished is displayed in "Actual

workpieces". This value can be corrected if necessary.

After the defined number of workpieces is reached, the current

workpieces display is automatically reset to zero.

4.15

Setting for automatic mode

Before machining a workpiece, you can test the program in order to identify programming

errors early on. Use the dry run feedrate for this purpose.

In addition, you have the option of additionally limiting the traversing speed for rapid traverse

so that when running-in a new program with rapid traverse, no undesirable high traversing

speeds occur.

Dry run feedrate

The feedrate defined here replaces the programmed feedrate during execution if you have

selected "DRY run feedrate" under program control.

Reduced rapid traverse

This value entered here reduces the rapid traverse to the entered percentage value if you

selected "RG0 reduced rapid traverse" under program control.

Universal

140

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

Machining the workpiece

4.15 Setting for automatic mode

Displaying measurement results

Using an MMC command, you can display measurement results in a part program:

You can define the following settings:

● When it reaches the command, the control automatically jumps to the "Machine"

operating area and the window with the measurement results is displayed

● The window with the measurement results is opened by pressing the "Measurement

result" softkey.

Procedure

1.

Select the "Machine" operating area.

2.

Press the <AUTO> key.

3.

Press the menu forward key and the "Settings" softkey.

The "Settings for Automatic Operation" window is opened.

4.

In "DRY run feedrate," enter the desired dry run speed.

5.

Enter the desired percentage in the "Reduced rapid traverse RG0" field.

RG0 has not effect if you do not change the specified amount of 100%.

6.

Enter "Automatic" in the "Display measurement result" box if the

measurement result window should be automatically opened, or

"Manual", if the measurement result window should be opened by

pressing the "Measurement result" softkey.

References

Programming Manual Measuring Cycles / 840D sl/828D

Note

The feedrate can be changed while the operation is running.

Universal

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

141

Machining the workpiece

4.16 Mold making view

4.16

Mold making view

4.16.1

Mold making view

For large mold making programs, as provided by CAD systems, you have the option, using a

fast view, to display the machining paths. This allows you to obtain a fast overview of the

program and possibly correct it.

Checking the program

For instance, you can check whether

● The programmed workpiece has the correct form (shape)

● Whether there are large traversing errors

● If yes, which block must be corrected

● How the approach and retraction are performed

Simultaneous view of the program and mold making view

In the editor, next to the program block display, switch-in the graphic view.

At the left in the editor, if you set the cursor to an NC block with position data, then this NC

block is selected in the graphic view.

If you select a point to the right in the graphic view - then the NC block is selected in the left-

hand part of the editor - i.e. in the other direction. This is how you jump directly to a position

in the program in order to edit a program block for example.

Universal

142

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

Machining the workpiece

4.16 Mold making view

Changing and adapting the mold making view

Just the same as for simulation and simultaneous recording, you have the option of changing

and adapting the simulation graphical representation in order to achieve the optimum view.

● Increasing or reducing the size of the graphic

● Moving the graphic

● Rotating the graphic

● Changing the section

4.16.2

Starting the mold making view

Procedure

1.

Select the "Program manager" operating area.

2.

Select the desired storage location and position the cursor on the

program that you would like to display in the mold making view.

3.

Press the "Open" softkey.

The program is opened in the editor.

4.

Press the ">>" and "Mold making view" softkeys.

The editor splits up into two areas.

The G code blocks are displayed in the left half of the editor.

The workpiece graphic is displayed in the right half of the editor.

All of the points and paths programmed in the part program are shown

in the graphical representation.

5.

Press the "Graphic" softkey in order to hide the graphic and to view the

program as usual in the editor

- OR -

Press the "NC blocks" softkey in order to hide the G code blocks and

therefore only to display the graphic.

Universal

144

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

Machining the workpiece

4.16 Mold making view

4.16.3

Specifically jump to the program block

If you notice anything peculiar in the graphic or identify an error, then from this location, you

can directly jump to the program block involved to possibly edit the program.

Preconditions

● The required program is opened in the mold making view.

● The "Graphic" softkey is active.

Procedure

1.

Press the ">>" and "Select point" softkeys.

Cross-hairs for selecting a point is shown in the diagram.

2.

Using the cursor keys, move the cross-hairs to the appropriate position

in the graphic.

3.

Press the "Select NC block" softkey.

The cursor jumps to the associated program block in the editor.

4.16.4

Searching for program blocks

Using the "Search" function, you can search for specific program blocks as well as edit

programs; you can do this in one step by replacing the text that you are searching for by a

new text.

Precondition

● The required program is opened in the mold making view.

● The "NC blocks" softkey is active.

Procedure

1.

Press the "Search" softkey.

A new vertical softkey bar appears.

Universal

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

145

Machining the workpiece

4.16 Mold making view

See also

Searching in programs (Page 114)

Replacing program text (Page 115)

4.16.5

Changing the view

4.16.5.1

Enlarging or reducing the graphical representation

Precondition

● The mold making view has been started.

● The "Graphic" softkey is active.

Procedure

1.

Press the <+> and <-> keys if you wish to enlarge or reduce the graphic

display.

The graphic display enlarged or reduced from the center.

- OR -

Press the "Details" and "Zoom +" softkeys if you wish to increase the

size of the segment.

- OR -

Press the "Details" and "Zoom -" softkeys if you wish to decrease the

size of the segment.

- OR -

Press the "Details" and "Auto zoom" softkeys if you wish to

automatically adapt the segment to the size of the window.

The automatic scaling function "Fit to size" takes account of the largest

expansion of the workpiece in the individual axes.

Universal

146

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

Machining the workpiece

4.16 Mold making view

Note

Selected section

The selected sections and size changes are kept as long as the program is selected.

4.16.5.2

Modifying the viewport

Use the magnifying glass if you would like to move, increase or reduce the size of the

section of the mold making view, e.g. to view details or display the complete workpiece.

Using the magnifying glass, you can define your own segment and then increase or

decrease its size.

Precondition

● The mold making view has been started.

● The "Graphic" softkey is active.

Procedure

1.

Press the "Details" softkey.

2.

Press the "Zoom" softkey.

A magnifying glass in the shape of a rectangular frame appears.

3.

Press the "Magnify +" or <+> softkey to enlarge the frame.

- OR -

Press the "Magnify -" or <-> softkey to reduce the frame.

- OR -

Press one of the cursor keys to move the frame up, down, left or right.

4.

Press the "Accept" softkey to accept the section.

Universal

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

147

Simulating machining

5.1 Overview

Examples

Several examples for machine types that are supported:

Swivel head 90°/90°

Swivel head 90°/45°

Universal

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

153

Simulating machining

5.1 Overview

Swivel table 90°/90°

Swivel table 90°/45°

Universal

154

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

Simulating machining

5.1 Overview

Swivel combination 90°/90°

Swivel combination 45°/90°

Universal

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

155

Simulating machining

5.2 Simulation prior to machining of the workpiece

5.2

Simulation prior to machining of the workpiece

Before machining the workpiece on the machine, you have the option of performing a quick

run-through in order to graphically display how the program will be executed. This provides a

simple way of checking the result of the programming.

Feedrate override

Feedrate override is also active during simulation.

You can change the feedrate during the simulation via the user interface.

0 %: The simulation stops.

100 %: The program is executed as quickly as possible.

See also

Changing the feedrate (Page 162)

Simulating the program block by block (Page 163)

Procedure

1.

Select the "Program Manager" operating area.

2.

Select the storage location and position the cursor on the program to be

simulated.

3.

Press the <INPUT> or <Cursor right> key.

- OR -

Double-click the program.

The selected program is opened in the "Program" operating area.

4.

Press the "Simulation" softkey.

The program execution is displayed graphically on the screen. The

machine axes do not move.

5.

Press the "Stop" softkey if you wish to stop the simulation.

- OR -

Universal

156

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

Simulating machining

5.3 Simultaneous recording prior to machining of the workpiece

Press the "Reset" softkey to cancel the simulation.

6.

Press the "Start" softkey to restart or continue the simulation.

Note

Operating area switchover

The simulation is exited if you switch into another operating area. If you restart the

simulation, then this starts again at the beginning of the program.

5.3

Simultaneous recording prior to machining of the workpiece

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.

Software option

You require the option "Simultaneous recording (real-time simulation)" for the

simultaneous recording.

You can replace the programmed feedrate with a dry run feedrate to influence the speed of

execution and select the program test to disable axis motion.

If you would like to view the current program blocks again instead of the graphical display,

you can switch to the program view.

Procedure

1.

Load a program in the "AUTO" mode.

2.

Press the "Prog. ctrl." softkey and activate the checkboxes "PRT no axis

movement" and "DRY run feedrate".

The program is executed without axis movement. The programmed

feedrate is replaced by a dry run feedrate.

3.

Press the "Sim. rec." softkey.

Universal

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

157

Simulating machining

5.4 Simultaneous recording during machining of the workpiece

4.

Press the <CYCLE START> key.

The program execution is displayed graphically on the screen.

5.

Press the "Sim. rec." softkey again to stop the recording.

5.4

Simultaneous recording during machining of the workpiece

If the view of the work space is blocked by coolant, for example, while the workpiece is being

machined, you can also track the program execution on the screen.

Software option

You require the option "Simultaneous recording (real-time simulation)" for the

simultaneous recording.

Procedure

1.

Load a program in the "AUTO" mode.

2.

Press the "Sim. rec." softkey.

3.

Press the <CYCLE START> key.

The machining of the workpiece is started and graphically displayed on

the screen.

4.

Press the "Sim. rec." softkey again to stop the recording.

Note

• If you switch-on simultaneous recording after the unmachined part information has

already been processed in the program, only traversing paths and tool are displayed.

• If you switch-off simultaneous recording during machining and then switch-on the function

again at a later time, then the traversing paths generated in the intermediate time will not

be displayed.

Universal

158

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

Simulating machining

5.5 Different views of the workpiece

5.5

Different views of the workpiece

In the graphical display, you can choose between different views so that you constantly have

the best view of the current workpiece machining, or in order to display details or the overall

view of the finished workpiece.

The following views are available:

● Top view

● 3D view

● Side views

5.5.1

Plan view

1.

Start the simulation.

2.

Press the "Top view" softkey.

The workpiece is shown from above in the top view.

Changing the display

You can increase or decrease the size of the simulation graphic and move it, as well as

change the segment.

See also

Enlarging or reducing the graphical representation (Page 164)

Panning a graphical representation (Page 165)

Modifying the viewport (Page 166)

5.5.2

3D view

1.

Start the simulation.

2.

Press the "Other views" and "3D view" softkeys.

Software option

You require the option "3D simulation (finished part)" for the simulation.

Universal

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

159

Simulating machining

5.5 Different views of the workpiece

Changing the display

You can increase or decrease the size of the simulation graphic, move it, turn it, or change

the segment.

Displaying and moving cutting planes

You can display and move cutting planes X, Y, and Z.

See also

Enlarging or reducing the graphical representation (Page 164)

Panning a graphical representation (Page 165)

Rotating the graphical representation (Page 165)

Modifying the viewport (Page 166)

Defining cutting planes (Page 167)

5.5.3

Side view

1.

Starting the simulation.

2.

Press the "Other views" softkey.

3.

Press the "From front" softkey if you wish to view the workpiece from

the front.

- OR -

Press the "From rear" softkey if you wish to view the workpiece from the

rear.

- OR -

Press the "From left" softkey if you wish to view the workpiece from the

left.

- OR -

Press the "From right" softkey if you wish to view the workpiece from

the right.

Changing the display

You can increase or decrease the size of the simulation graphic and move it, as well as

change the segment.

Universal

160

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

Simulating machining

5.6 Editing the simulation display

5.6

Editing the simulation display

5.6.1

Blank display

You have the option of replacing the blank defined in the program or to define a blank for

programs in which a blank definition cannot be inserted.

Note

The unmachined part can only be entered if simulation or simultaneous recording is in the

reset state.

Procedure

1.

The simulation or the simultaneous recording is started.

2.

Press the ">>" and "Blank" softkeys.

The "Blank Input" windows opens and displays the pre-assigned values.

3.

Enter the desired values for the dimensions.

4.

Press the "Accept" softkey to confirm your entries. The newly defined

workpiece is displayed.

5.6.2

Showing and hiding the tool path

The path display follows the programmed tool path of the selected program. The path is

continuously updated as a function of the tool movement. The tool paths can be shown or

hidden as required.

Procedure

1.

The simulation or the simultaneous recording is started.

2.

Press the ">>" softkey.

The tool paths are displayed in the active view.

3.

Press the softkey to hide the tool paths.

The tool paths are still generated in the backg0round and can be shown

again by pressing the softkey again.

4.

Press the "'Delete tool path" softkey.

All of the tool paths recorded up until now are deleted.

Universal

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

161

Simulating machining

5.7 Program control during simulation

5.7

Program control during simulation

5.7.1

Changing the feedrate

You can change the feedrate at any time during the simulation.

You can track the changes in the status line.

Note

If you are working with the "Simultaneous recording" function, the rotary switch (override) on

the control panel is used.

Procedure

1.

Simulation is started.

2.

Press the "Program control" softkey.

3.

Press the "Override +" or "Override -" softkey to increase or decrease

the feedrate by 5%.

- OR -

Press the "Override 100%" softkey to set the feedrate to the maximum

value.

- OR -

Press the "<<" softkey to return to the main screen and perform the

simulation with changed feedrate.

Note

Toggling between "Override +" and "Override -"

Press the <CTRL> and <Cursor down> or <Cursor up> keys to toggle

between the "Override +" and "Override -" softkeys.

Universal

162

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

Simulating machining

5.7 Program control during simulation

5.7.2

Simulating the program block by block

You can control the program execution during simulation, i.e. execute a program block by

block, as when executing a program.

Procedure

1.

Simulation is started.

2.

Press the "Program control" and "Single block" softkeys.

3.

Press the "Back" and "Start SBL" softkeys.

The pending block of the program is simulated and then stops.

4.

Press "Start SBL" as many times as you want to simulate a single

program block.

5.

Press the "Program control" and the "Single block" softkeys to exist the

single block mode.

Note

Enabling/disabling single block

Press the <CTRL> and <S> keys simultaneously to enable and disable

the single block mode.

+

6

Universal

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

163

Simulating machining

5.8 Modifying and adapting the simulation graphics

5.8

Modifying and adapting the simulation graphics

5.8.1

Enlarging or reducing the graphical representation

Precondition

The simulation or the simultaneous recording is started.

Procedure

1.

Press the <+> and <-> keys if you wish to enlarge or reduce the graphic

display.

The graphic display enlarged or reduced from the center.

- OR -

Press the "Details" and "Zoom +" softkeys if you wish to increase the

size of the segment.

- OR -

Press the "Details" and "Zoom -" softkeys if you wish to decrease the

size of the segment.

- OR -

Press the "Details" and "Auto zoom" softkeys if you wish to

automatically adapt the segment to the size of the window.

The automatic scaling function "Fit to size" takes account of the largest

expansion of the workpiece in the individual axes.

Note

Selected section

The selected sections and size changes are kept as long as the program is selected.

Universal

164

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

Simulating machining

5.8 Modifying and adapting the simulation graphics

5.8.2

Panning a graphical representation

Precondition

The simulation or the simultaneous recording is started.

Procedure

1.

Press a cursor key if you wish to move the graphic up, down, left, or

right.

5.8.3

Rotating the graphical representation

In the 3D view you can rotate the position of the workpiece to view it from all sides.

Precondition

Simulation has been started and the 3D view is selected.

Procedure

1.

Press the "Details" softkey.

2.

Press the "Rotate view" softkey.

2.

Press the "Arrow right", "Arrow left", "Arrow up", "Arrow down", "Arrow

clockwise" and "Arrow counterclockwise" softkeys to change the

position of the workpiece.

- OR -

Universal

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

165

Simulating machining

5.8 Modifying and adapting the simulation graphics

Keep the <Shift> key pressed and then turn the workpiece in the desired

direction using the appropriate cursor keys.

5.8.4

Modifying the viewport

If you would like to move, enlarge or decrease the size of the segment of the graphical

display, e.g. to view details or display the complete workpiece, use the magnifying glass.

Using the magnifying glass, you can define your own segment and then increase or

decrease its size.

Precondition

The simulation or the simultaneous recording is started.

Procedure

1.

Press the "Details" softkey.

2.

Press the "Magnifying glass" softkey.

A magnifying glass in the shape of a rectangular frame appears.

3.

Press the "Magnify +" or <+> softkey to enlarge the frame.

- OR -

Press the "Magnify -" or <-> softkey to reduce the frame.

- OR -

Press one of the cursor keys to move the frame up, down, left or right.

4.

Press the "Accept" softkey to accept the section.

Universal

166

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

Simulating machining

5.8 Modifying and adapting the simulation graphics

5.8.5

Defining cutting planes

In the 3D view, you have the option of "cutting" the workpiece and therefore displaying

certain views in order to show hidden contours.

Precondition

The simulation or the simultaneous recording is started.

Procedure

1.

Press the "Details" softkey.

2.

Press the "Cut" softkey.

The workpiece is displayed in the cut state.

3.

Press the corresponding softkey to shift the cutting plane in the required

direction.

…

Universal

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

167

Simulating machining

5.9 Displaying simulation alarms

5.9

Displaying simulation alarms

Alarms might occur during simulation. If an alarm occurs during a simulation run, a window

opens in the operating window to display it.

The alarm overview contains the following information:

● Date and time

● Deletion criterion

Specifies with which softkey the alarm is acknowledged

● Alarm number

● Alarm text

Precondition

Simulation is running and an alarm is active.

Procedure

1.

Press the "Program control" and "Alarm" softkeys.

The "Simulation Alarms" window is opened and a list of all pending

alarms is displayed.

Press the "Acknowledge alarm" softkey to reset the simulation alarms

indicated by the Reset or Cancel symbol.

The simulation can be continued.

- OR -

Press the "Simulation Power On" softkey to reset a simulation alarm

indicated by the Power On symbol.

Universal

168

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

Multi-channel view (only 840D sl)

6.2 Multi-channel view in the "Machine" operating area

Single-channel view

If, for your multi-channel machine, you always only wish to monitor one channel, then you

can set a permanent single-channel view.

Horizontal softkeys

● Block search

When selecting the block search, the multi-channel view is kept. The block display is

displayed as search window.

● Program control

The "Program Control" window is displayed for the channels configured in the multi-

channel view. The data entered here applies for these channels together.

● If you press an additional horizontal softkey in the "Machine" operating area (e.g.

"Overstore", "Synchronized actions"), then you change into a temporary single-channel

view. If you close the window again, then you return to the multi-channel view.

Switching between single- and multi-channel view

Press the <MACHINE> key in order to briefly switch between the single-

and multi-channel view in the machine area.

Press the <NEXT WINDOW> key in order to switch between the upper

and lower window within a channel column.

Editing a program in the block display

You can perform simple editing operations as usual with the <INSERT>

key in the actual block display.

If there is not sufficient space, you switch over into the single-channel view.

Running-in a program

You select individual channels to run-in the program at the machine.

Requirement

● Several channels have been set-up.

● The setting "2 channels", "3 channels" or "4 channels" is selected.

Universal

170

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

Multi-channel view (only 840D sl)

6.2 Multi-channel view in the "Machine" operating area

Displaying/hiding a multi-channel view

1.

Select the "Machine" operating area

2.

Select the "JOG", "MDA" or "AUTO" mode.

3.

Press the menu forward key and the "Settings" softkey.

4.

Press the "Multi-channel view" softkey.

5.

In the window "Settings for Multi-Channel View" in the selection

box "View", select the required entry (e.g. "2 channels") and

define the channels as well as the sequence in which they are to

be displayed.

In the basic screen for the "AUTO", "MDA" and JOG" operating

modes, the upper window of the left-hand and right-hand channel

columns are occupied by the actual value window.

6.

Press the "T,F,S" softkey if you wish to view the "T,F,S" window.

The "T,F,S" window is displayed in the lower window of the left-

hand and right-hand channel column.

Note:

The "T,F,S" softkey is present only for smaller operator panels,

i.e. up to OP012.

Universal

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

171

Multi-channel view (only 840D sl)

6.3 Multi-channel view for large operator panels

Toggling between the channels

Press the <CHANNEL> key to toggle between the channels.

Press the <NEXT WINDOW> key to toggle within a channel column

between the three or four windows arranged one above the other.

Note

2-channel display

Unlike the smaller operator panels, the T,F,S window is visible for a 2-channel view in the

"Machine" operating area.

Program operating area

You can display as many as ten programs next to each other in the editor.

Displaying a program

You can define the width of the program in the Editor window using the settings in the editor.

This means that you can distribute programs evenly - or you can widen the column with the

active program .

Channel status

When required, channel messages are displayed in the status display.

Machine manufacturer

Please refer to the machine manufacturer's specifications.

Universal

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

173

Multi-channel view (only 840D sl)

6.4 Setting the multi-channel view

6.4

Setting the multi-channel view

Setting

Meaning

View

Here, you specify how many channels are displayed.

•

1 channel

•

2 channels

•

3 channels

•

4 channels

Channel selection and

You specify which channels in which sequence are displayed in the multi-

sequence

channel view.

(for "2 - 4 channels"

view)

Visible

Here, you specify which channels are displayed in the multi-channel view.

You can quickly hide channels from the view.

(for "2 - 4 channels"

view)

Example

Your machine has 6 channels.

You configure channels 1 - 4 for the multi-channel view and define the display sequence

(e.g. 1,3,4,2).

In the multi-channel view, for a channel switchover, you can only switch between the

channels configured for the multi-channel view; all others are not taken into consideration.

Using the <CHANNEL> key, advance the channel in the "Machine" operating area - you

obtain the following views: Channels "1" and "3", channels "3" and "4", channels "4" and "2".

Channels "5" and "6" are not displayed in the multi-channel view.

In the single-channel view, toggle between all of the channels (1...6) without taking into

account the configured sequence for the multi-channel view.

Using the channel menu, you can always select all channels, also those not configured for

multi-channel view. If you switch to another channel, which is not configured for the multi-

channel view, then the system automatically switches into the single-channel view. There is

no automatic switchback into the multi-channel view, even if a channel is again selected,

which has been configured for multi-channel view.

Universal

174

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

Multi-channel view (only 840D sl)

6.4 Setting the multi-channel view

Procedure

1.

Select the "Machine" operating area.

2.

Select the "JOG", "MDA" or "AUTO" mode.

3.

Press the menu forward key and the "Settings" softkey.

4.

Press the "Multi-channel view" softkey.

The "Settings for Multi-Channel View" window is opened.

5.

Set the multi-channel or single-channel view and define which channels

are to be seen in the "Machine" operating area - and in the editor - in

which sequence.

Universal

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

175

Collision avoidance (only 840D sl)

7.2 Switching the collision avoidance on and off

Precondition

● Collision avoidance is setup and an active machine model is available.

● In the "Collision avoidance" setting, for the AUTO mode, collision avoidance is selected.

Procedure

1.

Select the "Machine" operating area

2.

Press the <AUTO> key.

3.

Press the "Sim. rec." softkey.

4.

Press the "Other views" and "Machine area" softkeys.

An active machine model is displayed for simultaneous recording.

7.2

Switching the collision avoidance on and off

Using "Settings", you have the option of separately activating or deactivating the collision

monitoring for the Machine operating area (operating modes, AUTO, JOG and MDI)

separately for the machine and tools.

Using machine data, you define from which protection level the collision monitoring for the

machine or the tool can be activated or deactivated in the operating modes JOG/MDI or

AUTO.

Machine manufacturer

Please refer to the machine manufacturer's specifications.

Setting

Effect

JOG/MDI operating mode

They switch the collision monitoring for the operating modes JOG/MDI

completely on or off.

Collision avoidance

AUTO mode

They switch the collision monitoring for the operating mode AUTO

completely on or off.

Collision avoidance

Universal

178

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

Collision avoidance (only 840D sl)

7.2 Switching the collision avoidance on and off

Setting

Effect

JOG/MDI

If the collision monitoring for the JOG/MDI operating modes is

activated, then as a minimum, the

Machine

machine protection areas are monitored.

The parameter cannot be changed.

AUTO

If the collision monitoring for the AUTO operating mode is activated,

then as a minimum, the

Machine

machine protection areas are monitored.

The parameter cannot be changed.

JOG/MDI

They switch the collision monitoring of the tool protection areas for the

operating modes JOG/MDI on or off.

Tools

AUTO

They switch the collision monitoring of the tool protection areas for the

operating mode AUTO on or off.

Tools

Procedure

1.

Select the "Machine" operating area.

2.

Select the "JOG", "MDI" or "AUTO" mode.

3.

Press the menu forward key and the "Settings" softkey.

4.

Press the "Collision avoidance" softkey.

The "Collision Avoidance" window opens.

5.

In the "Collision avoidance" line for the required operating modes (e.g.

for JOG/MDI), select the entry "On" to activate the collision avoidance

or "Off" to deactivate collision avoidance.

6.

Deactivate the "Tools" checkbox if you only want to monitor the

machine protection areas.

Universal

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

179

Tool management

8.3 Tool types

8.3

Tool types

A number of tool types are available when you create a new tool. The tool type determines

which geometry data is required and how it will be computed.

Tool types

Figure 8-1

Example of Favorites list

Figure 8-2

Available tools in the "New Tool - Milling Cutter" window

Universal

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

183

Tool management

8.3 Tool types

Figure 8-3

Available tools in the "New Tool - Drill" window

Figure 8-4

Tools listed in the "New Tool - Grinding Tools" window

Figure 8-5

Available tools in the "New Tool - Special Tools" window

Universal

184

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

Tool management

8.4 Tool dimensioning

8.4

Tool dimensioning

This section provides an overview of the dimensioning of tools.

Tool types

'LDPHWHU

Figure 8-6

End mill (Type 120)

'LDPHWHU

2XWHU GLDPHWHU

Figure 8-7

Face mill (Type 140)

Universal

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

185

Tool management

8.4 Tool dimensioning

/HQJWK ;

<

;

Figure 8-8

Angle head cutter (Type 130)

'LDPHWHU

7LS DQJOH

Figure 8-9

Drill (Type 200)

Universal

186

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

Tool management

8.4 Tool dimensioning

'LDPHWHU

Figure 8-10 Tap (Type 240)

'LDPHWHU

Figure 8-11 3D tool with an example of a cylindrical die-sinking cutter (Type 110)

Universal

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

187

Tool management

8.4 Tool dimensioning

&RUQHU UDGLXV

'LDPHWHU

Figure 8-12 3D tool type with an example of a ballhead cutter (Type 111)

'LDPHWHU

&RUQHU UDGLXV

Figure 8-13 3D tool with an example of an end mill with corner rounding (Type 121)

Universal

188

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

Tool management

8.4 Tool dimensioning

$QJOH IRU FRQLFDO

WRROV

'LDPHWHU

Figure 8-14 3D tool type with an example of a bevel cutter (Type 155)

$QJOH IRU FRQLFDO WRROV

'LDPHWHU

&RUQHU UDGLXV

Figure 8-15 3D tool with an example of a bevel cutter with corner rounding (Type 156)

Universal

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

189

Tool management

8.4 Tool dimensioning

$QJOH IRU FRQLFDO WRROV

'LDPHWHU

Figure 8-16 3D tool with an example of a tapered die-sinking cutter (Type 157)

'LDPHWHU

Figure 8-17 Electronic workpiece probe

Universal

190

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

Tool management

8.5 Tool list

Machine manufacturer

The tool length of the workpiece probe is measured to the center of the ball

(length m) or to the ball circumference (length u).

Please refer to the machine manufacturer's specifications.

Note

An electronic workpiece probe must be calibrated before use.

8.5

Tool list

8.5.1

Tool list

All parameters and functions that are required to create and set up the tools are displayed in

the tool list.

Each tool is uniquely identified by the tool identifier and the replacement tool number.

Tool parameters

Column heading

Meaning

Location

Magazine/location number

• The magazine location numbers

The magazine number is specified first, followed by the location

number in the magazine.

If there is only one magazine, only the location number is displayed.

BS

• Load position in the load magazine

The following icons can also be displayed for other magazine types (e.g.

for a chain):

• Spindle location as an icon

* If activated in magazine

• Locations for gripper 1 and gripper 2 (applies only when a spindle with

selection

dual gripper is used) as icons.

Type

Tool type

Specific tool offset data is displayed depending on the tool type

(represented as an icon).

Universal

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

191

Tool management

8.5 Tool list

Column heading

Meaning

You have the option of changing the tool type using the <SELECT> key.

Tool name

The tool is identified by the name and the replacement tool number. You

may enter the names as text or numbers.

Note: The maximum length of tool names is 31 ASCII characters. The

number of characters is reduced for Asian characters or Unicode

characters. The following special characters are not permitted: | # ".

ST

Replacement tool number (for replacement tool strategy)

D

Cutting edge number

Length

Tool length

Geometry data, length

Radius

Tool radius

Tip angle or

Tip angle for Type 200 - twist drill and Type 220 - centering tool and Type

230 countersink

Pitch

Pitch for Type 240 - tap

N

Number of teeth for Type 100 - milling tool, Type 110 - ball end mill for

cylindrical die-sinking cutter, Type 111 - ball end mill or tapered die-

sinking cutter, Type 120 - end mill, Type 121 - end mill with corner

rounding, Type 130 - angle head cutter, Type 131 - angle head cutter with

corner rounding, Type 140 - facing tool, Type 150 - side mill, Type 155 -

bevel cutter, Type 156 - bevel cutter with corner rounding and Type 157 -

tapered die-sinking cutter.

Direction of spindle rotation

Spindle is not switched on

CW spindle rotation

CCW spindle rotation

Coolant 1 and 2 (e.g. internal and external cooling) can be switched on

and switched off.

The coolant infeed at the machine does not necessarily have to be set-up.

M1 - M4

Other tool-specific functions such as additional coolant infeed, monitoring

functions for speed, tool breakage, etc.

Further parameters

If you have created unique cutting edge numbers, they will be displayed in the first column.

Column heading

Meaning

D no.

Unique cutting edge number

SN

Cutting edge number

EC

Setting-up offsets

Display of the available setup offsets

Universal

192

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

Tool management

8.5 Tool list

You use the configuration file to specify the selection of parameters in the list.

Machine manufacturer

Please refer to the machine manufacturer's specifications.

References

Information about the configuration and setup of the tool list can be found in the following

references:

SINUMERIK Operate (IM9) / SINUMERIK 840D sl Commissioning Manual

Icons in the tool list

Icon/

Meaning

Marking

Tool type

Red "X"

The tool is disabled.

Yellow triangle pointing

The prewarning limit has been reached.

downward

Yellow triangle pointing

The tool is in a special state.

upward

Place the cursor on the marked tool. A tooltip provides a

short description.

Green border

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.

(configurable)

Red "X"

The magazine location is disabled.

Procedure

1.

Select the "Parameter" operating area.

2.

Press the "Tool list" softkey.

The "Tool List" window opens.

Universal

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

193

Tool management

8.5 Tool list

8.5.2

Creating a new tool

When creating a new tool, the "New tool - favorites" window offers you a number of selected

tool types, known as "favorites".

If you do not find the desired tool type in the favorites list, then select the milling, drilling,

grinding or special tool via the corresponding softkeys.

Note

Grinding tools

Only grinding tools are available depending on the particular machine configuration.

Procedure

1..

The tool list is opened.

2.

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 position the cursor on an existing tool in the area of the

NC tool memory. Data from the displayed tool will not be overwritten.

3.

Press the "New tool" softkey.

The "New tool - favorites" window opens.

- OR -

If you want to create a tool that is not in the "Favorites" list, press the

softkey "Cutters 100-199", "Drill 200-299", Grinders 400-499" or "

Spec.tool 700-900".

The "New tool - milling cutter", "New tool - drill", "New tool - grinding

tool" or "New tool - special tools" window opens.

4.

Select the tool by placing the cursor on the corresponding icon.

5.

Press the "OK" softkey.

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.

The tool creation sequence can be defined differently.

Universal

194

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

Tool management

8.5 Tool list

Tool type

Additional parameters

140 Face milling

External radius

Tool angle

155 Bevel cutter

Taper angle

156 Bevel cutter with corner

Corner radius

rounding

Taper angle

157 Conical die-milling cutter

Taper angle

585 Calibration tool

Geometry length (length X, length Y, length Z)

Wear length (Δ length X, Δ length Y, Δ length Z)

710 3D-probe milling

Geometry length (length X, length Y, length Z)

Wear length (Δ length X, Δ length Y, Δ length Z)

712 Mono-probe

Geometry length (length X, length Y, length Z)

Wear length (Δ length X, Δ length Y, Δ length Z)

713 L-probe

Geometry length (length X, length Y, length Z)

Wear length (Δ length X, Δ length Y, Δ length Z)

Boom length (length)

714 Star-type probe

Geometry length (length X, length Y, length Z)

Wear length (Δ length X, Δ length Y, Δ length Z)

Outer diameter (∅)

You can use the configuration file to specify the data to be displayed for specific tool types in

the "Additional Data" window.

Machine manufacturer

Please refer to the machine manufacturer's specifications.

Procedure

1.

The tool list is opened.

2.

In the list, select an appropriate tool, e.g. an angle head cutter.

3.

Press the "Additional data" softkey.

The "Additional Data - ..." window opens.

The "Additional data" softkey is only active if a tool for which the

"Additional Data" window is configured is selected.

Universal

196

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

Tool management

8.5 Tool list

8.5.4

Managing several 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. The number of possible cutting edges depends on the

controller configuration.

Tool cutting edges that are not required can be deleted.

Procedure

1.

The tool list is opened.

2.

Position the cursor on the tool for which you would like to store more

cutting edges.

3.

Press the "Edges" softkey in the "Tool list".

4.

Press the "New cutting edge" softkey.

A new data set is stored in the list.

The cutting edge number is incremented by one and the offset data is

assigned the values of the cutting edge on which the cursor is

positioned.

5.

Enter the offset data for the 2nd cutting edge.

6.

Repeat this process if you wish to create more tool edge offset data.

7.

Position the cursor on the cutting edge that you want to delete and

press the "Delete cutting edge" softkey.

The data set is deleted from the list. The first tool cutting edge cannot

be deleted.

Universal

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

197

Tool management

8.5 Tool list

8.5.5

Deleting a tool

Tools that are no longer in use can be deleted from the tool list for a clearer overview.

Procedure

1.

The tool list is opened.

2.

Place the cursor on the tool that you would like to delete.

3.

Press the "Delete tool" softkey.

A safety prompt is displayed.

4.

Press the "OK" softkey if you really want to delete the tool.

Use this softkey to delete the tool.

If the tool is in a magazine location, it is unloaded and then deleted.

Multiple load points - tool in magazine location

If you have configured several loading points for a magazine, then the "Loading Point

Selection" window appears after pressing the "Delete tool" softkey.

Select the required load point and press the "OK" softkey to unload and delete the tool.

8.5.6

Loading and unloading tools

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 NC memory.

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. HMI then

automatically saves the tool data in the NC memory.

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.

Universal

198

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

Tool management

8.5 Tool list

Procedure

1.

The tool list is opened.

2.

Place the cursor on the tool that you want to load into the magazine (if

the tools are sorted according to magazine location number you will find

it at the end of the tool list).

3.

Press the "Load" softkey.

The "Load to… " window opens.

The "... location" field is initialized with the number of the first empty

magazine location.

4.

Press the "OK" softkey to load the tool into the suggested location.

- OR -

Enter the location number you require and press the "OK" softkey.

- OR -

Press the "Spindle" softkey.

The tool is loaded into the specified magazine location or spindle.

Loading empty magazine location directly with tool

1.

Position the cursor at an empty magazine location where you want to

load a tool and press the "Load" softkey.

The "Load with ..." window opens.

Select the desired tool in the " ... Tool" field and press the "OK" softkey.

Several magazines

If you have configured several magazines, the "Load to ..." window appears after pressing

the "Load" softkey.

If you do not want to use the suggested empty location, then enter your desired magazine

and magazine location. Confirm your selection with "OK".

Multiple load points

If you have configured several loading points for a magazine, then the "Loading Point

Selection" window appears after pressing the "Load" softkey.

Select the required loading point and confirm with "OK".

Universal

Operating Manual, 03/2013, 6FC5398-6AP40-3BA1

199

Content      ..      1      2      3      ..