Simulating a Machine Using NC Code

You can simulate a machine using NC Code, define a set of NC Code lines to simulate and define conditions in the NC Code where you want the simulation to stop.

This task shows you how to:

See Also
Guidelines for Simulating Machines

Simulate a Machine Using NC Code

You can simulate Milling Machine, Milling Machine with Head, and Mill-Turn Machine (Mill-Turn Machine with Single Spindle and Single Turret; Mill-Turn Machine with Single Spindle and Multiple Turrets; and Mill-Turn Machine with Multiple Spindle and Multiple Turrets) using NC Code. This also validates the given NC Code.

Note: The simulation does not currently support indexing turrets that have the axis of rotation of the rotary joint for Indexing, that is at an angle neither parallel nor perpendicular to the axis of rotation of the spindle.

  1. Go to Me > Preferences > App Preferences > Simulation > Machining > NC Machining Apps Common Services > Output.
    1. Select a Post Processor.
    2. Select NC Code File location and extension in NC Code output and NC Guide Location.
  2. Go to Me > Preferences > App Preferences > Simulation > Machining > NC Machining Apps Common Services > Resources.
    Select a PP table location in Catalogs and Files for Tools and PP tables.
  3. Assign an NC Machine to the manufacturing cell.
    1. Set Controller Emulator, Post Processor, and Post Processor words table, and NC Data Format appropriate for the assigned machine in the Generic Machine dialog box.
    2. Select ISO (that is, NC code) as NC data type and click OK.
      An error message appears if the NC Code Simulation command is launched without setting the above options.

      See Creating a Generic Machine and Managing Its Parameters.

  4. Optional: Generate NC Code Files by doing one of the following:
    1. Right-click the manufacturing program in the tree and select Generate NC Code Interactively to generate NC Code files.
    2. Click Generate NC Code Interactively from the Analysis and Output section of the action bar.

      If not already generated, the NC Code get generated during the NC Code Simulation

  5. Double-click the manufacturing program and assign NC Code files if they are generated by other means.
  6. Launch the NC Code Simulation command.

    Activity selection during NC Code Simulation depends on the NC Machine to be simulated:

    • Part Operation: Mill-Turn Machine is simulated by right-clicking Part Operation > Simulate Machine using NC Code. You cannot select a manufacturing program or a part operation to simulate a Mill-Turn machine. The instructions in NC Code files associated with the manufacturing programs of the selected part operation are simulated. You have to enable manufacturing programs for NC Code Simulation.
    • Manufacturing Program: Milling Machine and Milling Machine with Head is simulated by right-clicking Manufacturing Program > Simulate Machine using NC Code. You cannot select a part operation to simulate a Milling machine or Milling machines with Head. The instructions in NC Code files associated with the selected manufacturing program are simulated.
    • Manufacturing Operation: Not Supported
    Note: An error message is displayed if you select an invalid activity for a given NC Machine.

    The NC Code Simulation Player and Simulation Analysis context toolbars appear after launching the NC Code Simulation command.

    The NC Code files are generated if they are not available or not up to date. You can run or pause the simulation using the Simulation Player tab.

    When you run NC Code Simulation, the material removal simulation result corresponding to the last line of the NC code file associated with the manufacturing program is persisted in transient mode. You can use this persisted result in the following commands:

    • Design Part Comparison : To analyze material remaining or gouges between the simulation result and the design part.
    • Save Material Removal Simulation Result : To store the simulation result in the database to reuse later.
      Note: You can also use this command to export the simulation result to a 3D Part using the Export material removal simulation result function in the Stock Creation Wizard.

  7. Click in Simulation Analysis tool bar.
    The ISO dialog box appears, displaying the currently executed NC Code, of one or several programs.

    Note:
    • Support for partial simulation and Video NC Code Simulation is not provided.
    • Tool Path traces are not provided in NC Code Simulation.

    Make sure your post processor and controller emulator are set in Me > Preferences > App Preferences > Simulation > Machining > NC Machining Apps Common Services > Output and set the post processor in the Generating NC Code.

Stop the Simulation

In the NC Code, you can define a condition where you want the simulation to stop such as at a program line, tool change or character string you define. This applies to milling machines only. If you choose a program line that cannot be simulated, such as a comment line, the condition is automatically moved to the next line that can be simulated.

Before you begin: Open the NC Code panel by pressing Shift+F5 and select the NC Code check box. At the right edge of the work area, click Simulation Options and select the NC code simulation check box in the NC Simulation tab.
  1. In the NC Code panel, expand the NC Code Options area.
  2. From the Stop At Definition list, select an item such as Program line number.
  3. Enter the line number where you want the simulation to stop and click .
    A list appears, displaying the created condition. If you select Program line number or User Defined String, an icon also appears in the NC Code, next to the defined line number or character string.
  4. Optional: Continue to add conditions to the NC Code.
  5. Click the Play button of the Compass to launch the simulation.

Tips:
  • To find a specific line, enter a string in the search bar of the NC Code panel.
  • To add or delete a condition, or to simulate a line, use the various context menu items that appear when you right-click a condition or an ISO line.

Simulating from a Line

You can simulate the NC code from a selected line or simulate only a line of the NC code.

  1. In the NC Code panel, expand the NC Code Options area.
  2. Right-click an ISO line and do one of the following:
    • Select Simulate from this line to simulate the NC code starting from the selected line.
    • Select Simulate this line to simulate only the selected ISO line.

    Note: These commands appear only if you have run the simulation at least once before and if the selected ISO line can be simulated.

  3. Click the Play button of the Compass to launch the simulation.

Simulate a Set of ISO Lines

Once you have simulated the NC Code, you can define a set of ISO lines to be simulated by defining start and end points. This applies to milling machines only.

Before you begin: Close the simulation player to activate the commands to define start and end points.
  1. In the NC Code panel, right-click the line where you want the simulation to start and select Set the Simulation Start Point.
    An icon appears next to the selected line.
  2. Right-click the line where you want the simulation to stop and select Set the Simulation End Point.
    An icon appears next to the selected line, and the experience player appears in the work area.
  3. From the experience player, click Play Forward to launch the simulation.