Advanced Finishing Parameters

The information in this section will help you create and edit Advanced Finishing operations in your Manufacturing Program.

Click Advanced Finishing , then select the geometry or the rework area to be machined .

A number of strategy parameters are available:

• in the Machining tab to define:

• the Machining tolerance,
• the Tool path style.

• in the Zone tab to define:

• the Maximum horizontal slope.
• the Distance between pass for vertical and for horizontal zones.

You can also define the feedrates and spindle speeds and transition paths in your machining operations by means of NC macros as needed.
 

Advanced Finishing: Strategy parameters

Advanced Finishing: Machining tab

Machining tolerance: 
Maximum allowed distance between the theoretical and computed tool path.
Consider it to be the acceptable chord error.

Cutting mode:
Specifies the position of the tool regarding the surface to be machined. It can be:

• Climb 
  
• Conventional
  
• Either.
  

Advanced Finishing: Zone parameters

Max. horizontal slope
maximum slope that can be considered to be horizontal (any area that is considered to be horizontal will not be machined).

• Use this parameter to define slope areas if you need a quick tool path computation.
  However, this computation may not be accurate since some parts of the tool movements may be considered as vertical although they are in horizontal areas.

• If you require an accurate tool path computation, we recommend that you define the slope areas with the Machining/Slope Area action before entering the Advanced Finishing action.

Distance between pass:

You can set a different Distance between pass for the vertical and the horizontal zone:

results in


results in

Advanced Finishing: Geometry

• a Part or a Rework Area computed before this operation (mandatory),
• Safety plane.
  The safety plane is the plane that the tool will rise to at the end of the tool path in order to avoid collisions with the part.
  You can also define a new safety plane with the Offset option in the safety plane contextual menu.
  The new plane will be offset from the original by the distance that you enter in the dialog box along
  the normal to the safety plane. If the safety plane normal and the tool axis have opposed directions,
  the direction of the safety plane normal is inverted to ensure that the safety plane is not inside the part to machine.

• Top plane which defines the highest plane that will be machined on the part,
• Bottom plane which defines the lowest plane that will be machined on the part,

  In standard cases, the part will be machined from the upper plane to the lower plane, i.e. from top to bottom. If you want to machine the part from the lower plane to the upper plane, simply enter the lower plane as the top plane and the upper plane as the bottom plane.

• Limiting contour which is the contour that defines the outer machining limit on the part.
  You can also use the Part Autolimit option, with the Side to machine, Stop position, Stop mode and Offset parameters.

  If you have selected a single face to be machined and you are not using Part autolimit, the tool will machine both sides of the face. If you use Part autolimit, the tool will stop when it reaches the edge of the face (as shown below).

Info
When pressed, gives the details on the parameters that were defined with the rework area.

Appears when invalid faces have been detected.
This message disappears when you close the dialog box or when the next computation is successful.

Appears when invalid faces have been detected and when you have decided to ignore them.
This message remains displayed as a warning.

Click the text to switch from one status to the other.

Please refer to the Basic Task - Selecting Geometric Components to learn how to select the geometry.

Macros

General information about macros can be found in NC Macros.
Information about the operating mode can be found in Defining Macros.
Information about Surface Machining macro parameters can be found in Macro Parameters.

Advanced Finishing operations provide the same NC macros as ZLevel operations.