Programming and simulating a workpiece

Example task 1338459

Selecting the Editor operating mode

NC programs are always programmed in the Editor operating mode.

Requirement

  • It must be possible to select the icon of the operating mode
  • In order to be able to select the Editor operating mode, the control must have already progressed enough during booting that the operating mode icon is no longer dimmed.

Selecting the Editor operating mode

To select the Editor operating mode:

    1. Select the Editor operating mode
    2. The control displays the Editor operating mode and the most recently opened NC program.

    Creating a new NC program

    The Open File workspace in the Editor operating mode

    To create an NC program in the Editor operating mode:

      1. Select Add
      2. The control shows the Quick selection and Open File workspaces.

      1. Select the desired drive in the Open File workspace

      1. Select a folder

      1. Select New file

      1. Enter a file name (e.g., 1338459.h)

      1. Confirm with the ENT key

      1. Select Open
      2. The control opens a new NC program and the Insert NC function window for definition of the workpiece blank.

      Configuring the control's user interface for programming

      The Editor operating mode gives you several possibilities for writing an NC program.

       
      Tip

      The first steps describe the procedure when you are in the Klartext editor mode with the Form column open.

      Opening the Form column

      You can open the Form column only if an NC program is open.

      To open the Form column:

        1. Select Form
        2. The control opens the Form column

        Defining the workpiece blank

        For the NC program you can define a workpiece blank that the control then uses for the simulation. When you create an NC program, the control automatically opens the Insert NC function window for workpiece blank definition.

         
        Tip

        If you close the window without selecting a workpiece blank, you can use the Insert NC function button to select the workpiece blank definition later.

        The Insert NC function window for workpiece blank definition

        Defining a cuboid workpiece blank

        Cuboid workpiece blank with minimum point and maximum point

        You define a cuboid through a diagonal in space by entering the minimum point and maximum point relative to the active workpiece preset.

         
        Tip

        You can confirm the entries as follows:

        • ENT key
        • Right arrow key
        • Click or tap the next syntax element

        To define a cuboid workpiece blank:

          1. Select BLK FORM QUAD

          1. Select Paste
          2. The control inserts the NC block for definition of the workpiece blank.

          1. Open the Form column

          1. Select the tool axis (e.g., Z)

          1. Confirm your input

          1. Enter the smallest X coordinate (e.g., 0)

          1. Confirm your input

          1. Enter the smallest Y coordinate (e.g., 0)

          1. Confirm your input

          1. Enter the smallest Z coordinate (e.g., –20)

          1. Confirm your input

          1. Enter the largest X coordinate (e.g., 100)

          1. Confirm your input

          1. Enter the largest Y coordinate (e.g., 100)

          1. Confirm your input

          1. Enter the largest Z coordinate (e.g., 0)

          1. Confirm your input

          1. Select Confirm
          2. The control concludes the NC block.
          The Form column with the defined columns

          NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

          Change the following contents as needed:

          • Tools
          • Cutting parameters
          • Feed rates
          • Clearance height or safe position
          • Machine-specific positions (e.g., with M91)
          • Paths of program calls

          Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

          In addition, test the NC programs using the simulation before the actual program run.

           
          Tip

          With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

          0 BEGIN PGM 1338459 MM

          1 BLK FORM 0.1 Z X+0 Y+0 Z-20

          2 BLK FORM 0.2 X+100 Y+100 Z+0

          3 END PGM 1338459 MM

           
          Machine

          The control’s full range of functions is available only if the Z tool axis is used (e.g., PATTERN DEF).

          Restricted use of the tool axes X and Y is possible when prepared and configured by the machine manufacturer.

          Structure of an NC program

          Using a uniform structure for an NC program offers the following advantages:

          • Improved overview
          • Quicker programming
          • Fewer sources of error

          Recommended structure for a contouring program

           
          Tip

          The control automatically inserts the BEGIN PGM and END PGM NC blocks.

          1. BEGIN PGM with selection of the unit of measure
          2. Define the workpiece blank
          3. Call the tool, with the tool axis and the technological data
          4. Move the tool to a safe position, and switch the spindle on
          5. Pre-position the tool in the working plane, near the first contour point
          6. Pre-position the tool in the tool axis, turn coolant on if necessary
          7. Approach the contour, activate tool radius compensation if necessary
          8. Machine the contour
          9. Depart from the contour, turn coolant off
          10. Move the tool to a safe position
          11. Conclude the NC program
          12. END PGM

          Contour approach and departure

          When you program a contour, you need a starting point and end point outside the contour.

          The following positions are necessary for contour approach and departure:

          Help graphic

          Position

          Starting point

          The following preconditions apply for the starting point:

          • No tool radius compensation
          • Approachable without danger of collision
          • Near to the first contour point

          The graphic shows the following information:

          If you define the starting point to be in the dark gray area, the contour will be damaged when the first contour point is approached.

          Approaching the starting point in the tool axis

          Before approaching the first contour point, you must position the tool to the working depth in the tool axis. If there is a danger of collision, approach the starting point in the tool axis separately.

          First contour point

          The control moves the tool from the starting point to the first contour point.

          You need to program tool radius compensation for the tool movement to the first contour point.

          End point

          The following preconditions apply for the end point:

          • Approachable without danger of collision
          • Near to the last contour point
          • In order to make sure that the contour will not be damaged, the optimal ending point should lie on the extended tool path for machining the last contour element

          The graphic shows the following information:

          If you define the end point to be in the dark gray area, the contour will be damaged when the end point is approached.

          Departing from the end point in the tool axis

          Program the tool axis separately when departing from the end point.

          Identical starting and end points

          Do not program any tool radius compensation if the starting point and end point are the same.

          In order to make sure that the contour will not be damaged, the optimal starting point should lie between the extended tool paths for machining the first and last contour elements.

          Programming a simple contour

          Workpiece to be programmed

          The following texts show you how to mill once at a depth of 5 mm around the contour shown here. You have already defined the workpiece blank.

          Defining the workpiece blank

          After you have inserted an NC function, the control shows an explanation about the current syntax element in the dialog bar. You can enter the data directly in the form.

           
          Tip

          Always write an NC program as if the tool were moving. This makes it irrelevant whether a head axis or a table axis performs the motion.

          Calling a tool

          The Form column with the syntax elements of the tool call

          To call a tool:

            1. Select TOOL CALL

            1. Select Number in the form
            2. Enter the tool number (e.g., 16)

            1. Select the tool axis Z

            1. Select the spindle speed S
            2. Enter the spindle speed (e.g., 6500)

            1. Select Confirm
            2. The control concludes the NC block.

            NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

            Change the following contents as needed:

            • Tools
            • Cutting parameters
            • Feed rates
            • Clearance height or safe position
            • Machine-specific positions (e.g., with M91)
            • Paths of program calls

            Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

            In addition, test the NC programs using the simulation before the actual program run.

             
            Tip

            With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

            3 TOOL CALL 16 Z S6500

             
            Machine

            The control’s full range of functions is available only if the Z tool axis is used (e.g., PATTERN DEF).

            Restricted use of the tool axes X and Y is possible when prepared and configured by the machine manufacturer.

            Move the tool to a safe position

            The Form column with the syntax elements of a straight line

            To move the tool to a safe position:

              1. Select the path function L

              1. Select Z
              2. Enter a value (e.g., 250

              1. Select tool radius compensation R0
              2. The control applies R0, which means there is no tool radius compensation.

              1. Select the FMAX feed rate
              2. The control adopts FMAX for rapid traverse.
              3. If needed, enter a miscellaneous function M, such as M3 (turn spindle on)

              1. Select Confirm
              2. The control concludes the NC block.

              NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

              Change the following contents as needed:

              • Tools
              • Cutting parameters
              • Feed rates
              • Clearance height or safe position
              • Machine-specific positions (e.g., with M91)
              • Paths of program calls

              Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

              In addition, test the NC programs using the simulation before the actual program run.

               
              Tip

              With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

              4 L Z+250 R0 FMAX M3

              Pre-positioning in the working plane

              To pre-position in the working plane:

                1. Select the path function L

                1. Select X
                2. Enter a value (e.g., –20

                1. Select Y
                2. Enter a value (e.g., –20

                1. Select the FMAX feed rate

                1. Select Confirm
                2. The control concludes the NC block.

                NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

                Change the following contents as needed:

                • Tools
                • Cutting parameters
                • Feed rates
                • Clearance height or safe position
                • Machine-specific positions (e.g., with M91)
                • Paths of program calls

                Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

                In addition, test the NC programs using the simulation before the actual program run.

                 
                Tip

                With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

                5 L X-20 Y-20 FMAX

                Pre-positioning in the tool axis

                To pre-position in the tool axis:

                  1. Select the path function L

                  1. Select Z
                  2. Enter a value (e.g., –5

                  1. Select the feed rate F
                  2. Enter the value for the positioning feed rate (e.g., 3000)

                  1. If needed, enter a miscellaneous function M, such as M8 (turn coolant on)

                  1. Select Confirm
                  2. The control concludes the NC block.

                  NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

                  Change the following contents as needed:

                  • Tools
                  • Cutting parameters
                  • Feed rates
                  • Clearance height or safe position
                  • Machine-specific positions (e.g., with M91)
                  • Paths of program calls

                  Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

                  In addition, test the NC programs using the simulation before the actual program run.

                   
                  Tip

                  With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

                  6 L Z-5 F3000 M8

                  Approaching the contour

                  Workpiece to be programmed
                  The Form column with the syntax elements of an approach function

                  To approach the contour:

                    1. Select the APPR DEP path function
                    2. The control opens the Insert NC function window.

                    1. Select APPR

                    1. Select an approach function (e.g., APPR CT)

                    1. Select Paste
                    2. Enter the coordinates of the starting point 1 (e.g., X 5 Y 5)

                    1. For the center angle CCA, enter the approach angle (e.g., 90)

                    1. Enter the radius of the circular arc (e.g., 8

                    1. Select RL
                    2. The control applies tool radius compensation to the left.

                    1. Select the feed rate F
                    2. Enter the value for the machining feed rate (e.g., 700)

                    1. Select Confirm
                    2. The control concludes the NC block.

                    NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

                    Change the following contents as needed:

                    • Tools
                    • Cutting parameters
                    • Feed rates
                    • Clearance height or safe position
                    • Machine-specific positions (e.g., with M91)
                    • Paths of program calls

                    Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

                    In addition, test the NC programs using the simulation before the actual program run.

                     
                    Tip

                    With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

                    7 APPR CT X+5 Y+5 CCA90 R+8 RL F700

                    Machining a contour

                    Workpiece to be programmed

                    To machine the contour:

                      1. Select the path function L
                      2. Enter the coordinates of contour point 2 that differ (e.g., Y 95)

                      1. Conclude the NC block with Confirm
                      2. The control applies the changed value and retains all of the other information from the previous NC block.

                      1. Select the path function L
                      2. Enter the coordinates of contour point 3 that differ (e.g., X 95)

                      1. Conclude the NC block with Confirm

                      1. Select the path function CHF
                      2. Enter the chamfer width (e.g., 10

                      1. Conclude the NC block with Confirm

                      1. Select the path function L
                      2. Enter the coordinates of contour point 4 that differ (e.g., Y 5)

                      1. Conclude the NC block with Confirm

                      1. Select the path function CHF
                      2. Enter the chamfer width (e.g., 20

                      1. Conclude the NC block with Confirm

                      1. Select the path function L
                      2. Enter the coordinates of contour point 1 that differ (e.g., X 5)

                      1. Conclude the NC block with Confirm

                      NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

                      Change the following contents as needed:

                      • Tools
                      • Cutting parameters
                      • Feed rates
                      • Clearance height or safe position
                      • Machine-specific positions (e.g., with M91)
                      • Paths of program calls

                      Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

                      In addition, test the NC programs using the simulation before the actual program run.

                       
                      Tip

                      With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

                      8 L Y+95

                      9 L X+95

                      10 CHF 10

                      11 L Y+5

                      12 CHF 20

                      13 L X+5

                      Departing from the contour

                      The Form column with the syntax elements of a departure function

                      To depart from the contour:

                        1. Select the APPR DEP path function
                        2. The control opens the Insert NC function window.

                        1. Select DEP

                        1. Select a departure function (e.g., DEP CT)

                        1. Select Paste

                        1. For the center angle CCA, enter the departure angle (e.g., 90)

                        1. Enter the departure radius (e.g., 8

                        1. Select the feed rate F
                        2. Enter the value for the positioning feed rate (e.g., 3000)

                        1. If needed, enter a miscellaneous function M, such as M9 (turn coolant off)

                        1. Select Confirm
                        2. The control concludes the NC block.

                        NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

                        Change the following contents as needed:

                        • Tools
                        • Cutting parameters
                        • Feed rates
                        • Clearance height or safe position
                        • Machine-specific positions (e.g., with M91)
                        • Paths of program calls

                        Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

                        In addition, test the NC programs using the simulation before the actual program run.

                         
                        Tip

                        With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

                        14 DEP CT CCA90 R+8 F3000 M9

                        Moving the tool to a safe position

                        To move the tool to a safe position:

                          1. Select the path function L

                          1. Select Z
                          2. Enter a value (e.g., 250

                          1. Select tool radius compensation R0

                          1. Select the FMAX feed rate
                          2. Enter a miscellaneous function M if required

                          1. Select Confirm
                          2. The control concludes the NC block.

                          NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

                          Change the following contents as needed:

                          • Tools
                          • Cutting parameters
                          • Feed rates
                          • Clearance height or safe position
                          • Machine-specific positions (e.g., with M91)
                          • Paths of program calls

                          Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

                          In addition, test the NC programs using the simulation before the actual program run.

                           
                          Tip

                          With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

                          15 L Z+250 R0 FMAX M30

                          Programming a machining cycle

                          The following texts show you how to mill the circular slot of the example task at a depth of 5 mm. You have already defined the workpiece blank and created the outside contour.

                          Example task 1338459

                          After you have inserted a cycle, you can define the associated values in the cycle parameters. You can program the cycle directly in the Form column.

                          Calling a tool

                          To call a tool:

                            1. Select TOOL CALL

                            1. Select Number in the form
                            2. Enter the tool number (e.g., 6)

                            1. Select the tool axis Z

                            1. Select the spindle speed S
                            2. Enter the spindle speed (e.g., 6500)

                            1. Select Confirm
                            2. The control concludes the NC block.

                            NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

                            Change the following contents as needed:

                            • Tools
                            • Cutting parameters
                            • Feed rates
                            • Clearance height or safe position
                            • Machine-specific positions (e.g., with M91)
                            • Paths of program calls

                            Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

                            In addition, test the NC programs using the simulation before the actual program run.

                             
                            Tip

                            With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

                            16 TOOL CALL 6 Z S6500

                            Moving the tool to a safe position

                            The Form column with the syntax elements of a straight line

                            To move the tool to a safe position:

                              1. Select the path function L

                              1. Select Z
                              2. Enter a value (e.g., 250

                              1. Select tool radius compensation R0
                              2. The control applies R0, which means there is no tool radius compensation.

                              1. Select the FMAX feed rate
                              2. The control adopts FMAX for rapid traverse.
                              3. If needed, enter a miscellaneous function M, such as M3 (turn spindle on)

                              1. Select Confirm
                              2. The control concludes the NC block.

                              NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

                              Change the following contents as needed:

                              • Tools
                              • Cutting parameters
                              • Feed rates
                              • Clearance height or safe position
                              • Machine-specific positions (e.g., with M91)
                              • Paths of program calls

                              Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

                              In addition, test the NC programs using the simulation before the actual program run.

                               
                              Tip

                              With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

                              17 L Z+250 R0 FMAX M3

                              Pre-positioning in the working plane

                              To pre-position in the working plane:

                                1. Select the path function L

                                1. Select X
                                2. Enter a value (e.g., +50

                                1. Select Y
                                2. Enter a value (e.g., +50

                                1. Select the FMAX feed rate

                                1. Select Confirm
                                2. The control concludes the NC block.

                                NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

                                Change the following contents as needed:

                                • Tools
                                • Cutting parameters
                                • Feed rates
                                • Clearance height or safe position
                                • Machine-specific positions (e.g., with M91)
                                • Paths of program calls

                                Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

                                In addition, test the NC programs using the simulation before the actual program run.

                                 
                                Tip

                                With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

                                18 L X+50 Y+50 FMAX

                                Defining a cycle

                                The Form column with possibilities for entering cycle information

                                To define the circular slot:

                                  1. Select the CYCL DEF key
                                  2. The control opens the Insert NC function window.

                                  1. Select Cycle 254 CIRCULAR SLOT

                                  1. Select Paste
                                  2. The control inserts the cycle.

                                  1. Open the Form column
                                  2. Enter all input values in the form

                                  1. Select Confirm
                                  2. The control saves the cycle.

                                  NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

                                  Change the following contents as needed:

                                  • Tools
                                  • Cutting parameters
                                  • Feed rates
                                  • Clearance height or safe position
                                  • Machine-specific positions (e.g., with M91)
                                  • Paths of program calls

                                  Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

                                  In addition, test the NC programs using the simulation before the actual program run.

                                   
                                  Tip

                                  With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

                                  19 CYCL DEF 254 CIRCULAR SLOT ~

                                  Q215=+0

                                  ;MACHINING OPERATION ~

                                  Q219=+15

                                  ;SLOT WIDTH ~

                                  Q368=+0.1

                                  ;ALLOWANCE FOR SIDE ~

                                  Q375=+60

                                  ;PITCH CIRCLE DIAMETR ~

                                  Q367=+0

                                  ;REF. SLOT POSITION ~

                                  Q216=+50

                                  ;CENTER IN 1ST AXIS ~

                                  Q217=+50

                                  ;CENTER IN 2ND AXIS ~

                                  Q376=+45

                                  ;STARTING ANGLE ~

                                  Q248=+225

                                  ;ANGULAR LENGTH ~

                                  Q378=+0

                                  ;STEPPING ANGLE ~

                                  Q377=+1

                                  ;NR OF REPETITIONS ~

                                  Q207=+500

                                  ;FEED RATE MILLING ~

                                  Q351=+1

                                  ;CLIMB OR UP-CUT ~

                                  Q201=-5

                                  ;DEPTH ~

                                  Q202=+5

                                  ;PLUNGING DEPTH ~

                                  Q369=+0.1

                                  ;ALLOWANCE FOR FLOOR ~

                                  Q206=+150

                                  ;FEED RATE FOR PLNGNG ~

                                  Q338=+5

                                  ;INFEED FOR FINISHING ~

                                  Q200=+2

                                  ;SET-UP CLEARANCE ~

                                  Q203=+0

                                  ;SURFACE COORDINATE ~

                                  Q204=+50

                                  ;2ND SET-UP CLEARANCE ~

                                  Q366=+2

                                  ;PLUNGE ~

                                  Q385=+500

                                  ;FINISHING FEED RATE ~

                                  Q439=+0

                                  ;FEED RATE REFERENCE

                                  Calling a cycle

                                  To call the cycle:

                                  1. Select CYCL CALL

                                  NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

                                  Change the following contents as needed:

                                  • Tools
                                  • Cutting parameters
                                  • Feed rates
                                  • Clearance height or safe position
                                  • Machine-specific positions (e.g., with M91)
                                  • Paths of program calls

                                  Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

                                  In addition, test the NC programs using the simulation before the actual program run.

                                   
                                  Tip

                                  With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

                                  20 CYCL CALL

                                  Moving the tool to a safe position and concluding the NC program

                                  To move the tool to a safe position:

                                    1. Select the path function L

                                    1. Select Z
                                    2. Enter a value (e.g., 250

                                    1. Select tool radius compensation R0

                                    1. Select the FMAX feed rate
                                    2. Enter miscellaneous function M (e.g., M30, end of program run)

                                    1. Select Confirm
                                    2. The control concludes the NC block and the NC program.

                                    NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

                                    Change the following contents as needed:

                                    • Tools
                                    • Cutting parameters
                                    • Feed rates
                                    • Clearance height or safe position
                                    • Machine-specific positions (e.g., with M91)
                                    • Paths of program calls

                                    Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

                                    In addition, test the NC programs using the simulation before the actual program run.

                                     
                                    Tip

                                    With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

                                    21 L Z+250 R0 FMAX M30

                                    Configuring the control's user interface for simulation

                                    In the Editor operating mode you can test NC programs graphically. The control simulates the active NC program in the Program workspace.

                                    In order to simulate the NC program you must open the Simulation workspace.

                                     
                                    Tip

                                    For the simulation you can close the Form column to get a better view of the NC program and the Simulation workspace.

                                    Opening the Simulation workspace

                                    You can open additional workspaces in the Editor operating mode only if an NC program is open.

                                    To open the Simulation workspace:

                                    1. In the application bar, select Workspaces
                                    2. Select Simulation
                                    3. The control then additionally displays the Simulation workspace.
                                     
                                    Tip

                                    You can also open the Simulation workspace with the Test Run operating mode key.

                                    Configuring the Simulation workspace

                                    You can simulate the NC program without needing to enter any special settings. However, an adjustment to the simulation speed is recommended for best viewing of the simulation.

                                    To adjust the speed of the simulation:

                                    1. Use the slider to select the factor (e.g., 5.0 * T)
                                    2. The control then performs the subsequent simulation at five times the speed of the programmed feed rate.

                                    If you use different tables, such as tool tables, for program run and the simulation, then you can define the tables in the Simulation workspace.

                                    Simulating an NC program

                                    You can test the NC program in the Simulation workspace.

                                    Starting the simulation

                                    The Simulation workspace in the Editor operating mode

                                    To start the simulation:

                                      1. Select Start
                                      2. The control might ask whether the file should be saved.

                                      1. Select Save
                                      2. The control starts the simulation.
                                      3. The control uses the Control-in-operation symbol to show the simulation status.

                                      Definition

                                      Control-in-operation:
                                      The control uses the Control-in-operation symbol to show the current simulation status in the action bar and on the tab of the NC program:

                                      • White: no movement command
                                      • Green: active machining, axes are moving
                                      • Orange: NC program interrupted
                                      • Red: NC program stopped