Simulating while Using NC Code

This procedure describes how to run a simulation based on an ISO-based program.  Otherwise, simulation is based on the tool path.
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.

  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 Simulate Machine using NC Code.
    Click the Add button on Additional NC Files to add controller-specific sub-programs or continuation file to this list. Normally, these are not generated by the Post Processor.
    If you want to modify the workpiece origin or cutter compensation data before running the simulation, see Managing Specific NC Codes.

  2. Click Start Machine Simulation .

    For more general information on running simulations, please see Viewing a 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 processing of the simulation may take some time.  Depending on the post processor you selected, you may see a progress bar window in your task bar.
    The Process Simulation toolbar appears.

  3. Click Run .

    The NC Code dialog box appears.
    While the simulation is running, the dialog box shows the line and Machining Operation affected.  Once the simulation is complete, select the X (close) button on the Process Simulation toolbar.  The Process Simulation toolbar disappears, and the NC Code dialog box can be used for collision checking and analysis.  You can also select a subset of sequential lines of code to run a partial simulation. Tool path display is not applicable for NC Code simulation.
      If you are running a subprogram it has its own ISO (NC Code) dialog box which gets updated with the simulation. When simulation is happening for the Isubprogram, both the main and sub-program dialog box are visible. Once the control returns to the main program, the NC Code dialog box for the subprogram disappears. In case of multiple subprogram calls, only the main NC Code dialog boxand the active subprogram’s NC Code dialog box are visible. i.e., all the transient NC Code dialog box are hidden.
    For more information on the features of the NC Code dialog box, see About the NC Code Dialog Box.