ZLevel Machining




This task shows you how to insert a ZLevel operation into the program. 

ZLevel operations are finishing or semi-finishing operations that machine the whole part by parallel horizontal 
planes that are perpendicular to the tool axis.

To create the operation you define:

  • the tool to use ; you have the choice of end mill , conical or TSlotter tools for this operation,

Only the geometry is obligatory, all of the other requirements have a default value.

  • make the Manufacturing Program current in the specification tree if you want to define an operation and
    the part/area to machine at the same time,
  • or select a machining feature from the list if you have already defined the area to machine and
    now you want to define the operation to apply to it.

Below we are going to see how to do the first of these.

Open file Basic1.CATPart then select Machining > Surface Machining in the Start menu.

  1. Click ZLevel .The ZLevel dialog box is displayed. 
    A ZLevel entity and a default tool area added to the program.
    The dialog box opens at the geometry tab page .
    This page includes a sensitive icon to help you specify the geometry to be machined.
    The area that represents the part geometry is colored red indicating that the geometry is required
    or defining the area to machine. All the other geometry parameters are optional.

  2. Right-click the red area that represents the part geometry.
    Choose Select faces... in the contextual menu and select the belt of faces around the outside of the part.
    The edges surrounding the selected faces are highlighted. Click OK to confirm your selection.

  3. Click Tool Path Replay . A progress indicator is displayed.
    You can cancel the tool path computation at any moment before 100% completion.
    You will see that the outside of the part has been machined.


Invalid Face

  1. If a tool path cannot be computed because of invalid faces,
    an explicit warning message like this one will appear:

    Each invalid face is highlighted in red, with an arrow pointing on it.

    This visualization is removed when you close the main dialog box or
    when you select Remove in the contextual menu.

  2. Click OK in the Warning box to revert to the main dialog box.
    In the Geometry tab, a message Ignore invalid faces: No is displayed:

  3. You can either:

    • close the dialog box.
      When you reopen it, the Ignore invalid faces: No will not be displayed.
    • heal the defective geometry and restart the computation.
      If it is successful the message Ignore invalid faces: No will disappear.
    • ignore the invalid faces. Click the text Ignore invalid faces: No.
      It will turn to Ignore invalid faces: Yes and the computation will continue.
      The message remains displayed as a warning.
Be very careful when you choose to ignore invalid faces.
We recommend that you ignore only faces that will not affect the tool path. Otherwise this may lead to defective tool paths.