Isoparametric Machining

This task shows you how to insert a isoparametric machining operation into the program.
Isoparametric machining is an operation which allows you to select strips of faces and machine along their isoparametrics.

To create the operation you define:

  • the geometry of the part to machine ,
  • the parameters of the machining strategy ,
  • the tool to use ;end mill,    face mill , conical mill and T-slotter   tool  can be used for this operation,
  • the feedrates and spindle speeds ,
  • the macros .

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


You can modify the parameters of two or more Isoparametric machining operations in one shot by means of the Selected Objects > Definition... contextual command.
See Editing Parameters of Several Isoparametric machining Operations.

  • 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 Basic2.CATPart then select Machining > Surface Machining in the Start menu.

  1. Click Isoparametric Machining .
    An Isoparametric Machining entity and a default tool are 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 surface is colored red indicating that the geometry is
      equired for defining the area to machine. 
    • The four points on the area to machine are also obligatory.
      They are required in order to define the direction of the isoparameters (from 1 to 2). 
    • All of the other geometry parameters are optional.
    • The tool path will always start on point 1 and finish on point 4.
      This means that, if your parameters are set in such a way that, under normal circumstances,
      the tool path would end on point 3, the tool path will be computed in such a way as to ensure
      that it finishes on point 4.
      In order to do this the last five passes may be closer together than the others (by 20%).
  2. Click the red part surface in the icon and then select these faces in the viewer.

    The faces must be connected to each other.

  3. Click  a red point in the icon and select the four corner points of the part surface.
    The part surface and corner points of the icon are now colored green indicating
    that this geometry is now defined.

  1. Click Tool Path Replay .
    A progress indicator is displayed.
    You can cancel the tool path computation at any moment before 100% completion.