Creating Video Simulations while Using NC Code

This procedure describes how to create a video simulation with NC code.
Before you can run this procedure, take the following steps:
  1. On the Tools > Options > Machining > Output tab, select a Post Processor type for your NC code (e.g., ICAM®).

  2. On the Tools > Options > Machining > Output tab, in the Default File Locations area, specify CATNCCode as the file extension, and select output locations.

  3. Assign an NC machine to the part operation.

  4. In the machine editor dialog box for the NC machine (accessible in NC Machine Tool Simulation by right-clicking the machine on the PPR tree, and selecting machine object > Edit), set the Controller Emulator, Post Processor, and Post Processor words table appropriate for your machine and the Post Processor you selected in Step 1.

    The contents of the lists available on the machine editor dialog box depend on the options selected in Tools > Options > Machining > Output.
Please see Video Mode for Material Removal Simulation, from the NC Manufacturing Infrastructure User's Guide, for information on the video commands.
  1. Double-click on the manufacturing program in the PPR tree.

    The program dialog box appears (the name of the dialog box is the name of the manufacturing program, e.g., 001).
    If your options are set as described above, you can simply right-click on the manufacturing program, and select Start Video Simulation using NC Code.
  2. Select the NC Code Based Simulation check box.

    The options in the Simulation area become available.
    The manufacturing program on the PPR tree has ISO Simulation as part of its name.
    If you alter these selections to return to tool path-based simulation, ISO Simulation ceases to be part of the program's name.
    If you have failed to set up one of the parameters correctly, either in Tools > Options > Machining > Output or in the machine editor dialog box, you receive the following message:
    If you receive this error:
    1. Click OK on the Manufacturing Error message

    2. Select the Tools > Options > Machining > Output and machine editor dialog box as described above

    3. Try again.

  3. (Optional) Click the Edit Program button to select an NC or ISO code file to use as the simulation's source.

    The NC File field becomes blank when you click the Edit Program button. Use the Select ISO File   button to browse among your directories and select the desired file.
    The NC File field is not available unless the NC Code Based Simulation check box is selected.
      By default, the NC File is interactively generated from tool path when the NC Code Based Simulation check box is selected.
    If you want to modify the workpiece origin or cutter compensation data before creating the video replay, see Managing Specific NC Codes.
  4. Click Start Video Simulation .

    Depending on whether you have created any kind of simulation with this process before, you may see the following warning:
    If you receive the above warning, click the Yes button.
    The product geometry data appears in a video window and the video dialog box appears.
    Instead of selecting Start Video Simulation (which creates a video from the machining data in the manufacturing program as it exists at the moment you select the command), you can select Video from last saved result (if you have previously saved a video result).  In that case, you do not see the progress bar.
  5. In the Tool animation area, click the Forward Replay button.

    The geometric data begins showing the replay; the NC Code dialog box appears.
    For more information on the features of the NC Code dialog box, such as collision checking and analysis, see About the NC Code Dialog Box.
  6. Click Associate Video Result with the Entire Machining Operation .

    For more information on video capabilities, see Video Mode for Material Removal Simulation.