Avoiding Collisions

This procedure describes how to avoid collisions by checking the collision list, editing a machining operation (MO).  Using Fault List , you can also choose to modify the tool path; that procedure is described in Modifying NC Tool Paths.

The command works for lathe machines, mill machines, and mill-turn machines.  In the case of simulations that involve mill-turn machines, the collisions are be appended in the collision list in the order of their occurrence. Note that these collisions need not be in the same order as that of the machine operations in which they occurred (as in case of milling machines). Once the user accesses any of the collisions, the mill-turn machine (all the turrets and spindles) is positioned at the place it was when collision occurred. When a collision occurs, the positions of all the mechanisms in the mill-turn (spindles and turrets) are saved. So when the user accesses the collision from Fault List , then the positions of all the mechanisms are retrieved and the mechanisms are positioned accordingly.

The faults listed include:

  • Collisions
  • Violations of travel limits
Open the Process1.CATProcess sample file, and assign a machine to it, and mount the workpiece. Run the simulation as described in Simulating NC Tool Paths, and set at least one collision check.

  1. In the Machine Management toolbar, click Fault List .

    The Fault List dialog box appears.
    • If there are no collisions or other problems (such as violations of travel limits), nothing can be selected in the Fault List dialog box, as shown below:
     
     
    • If there are collisions or other problems (such as violations of travel limits), Fault Selection can be selected, as shown below:
     

  2. Select Collision 1.

    The Tool Name and the Machining Operation that caused the collision are both listed. In the 3D view, the machine and the corresponding tool (attached) move to the point where the collision occurred.

  3. Click the Analyze button.

    A Preview window and the Check Clash dialog box appear.
    For more information on using the Check Clash dialog box, see Viewing Analysis Data.
    At this point, you can select Modify Tool Path or Edit MO (machine operation).  This scenario describes selecting the Edit MO option.  If you choose to modify the tool path, see Modifying NC Tool Paths.

    Edit the Machining Operation (MO)

  4. In the Fault List dialog box, select the Edit MO check box.

    Once the MO is unlocked, the dialog box for that MO appears.

  5. Make the desired modifications to the MO's parameters/definitions and click Tool Path Replay so that the simulation shows the latest changes.

  6. Choose one:

    • Click OK in the MO dialog box to remove the collision that occurred in this particular MO. The Fault List dialog box becomes unavailable until you re-run Machine Simulation.
    • Click Cancel and the MO's parameters and definitions are not modified and this particular collision remains on the collision list.