Facing Feature

The Face Feature Parameters

Rapid Movements

1. • Clearance Plane - The height at which the tool can rapid safely from operation to operation.

   • Rapid Plane - The height at which the tool can rapid safely within the current machining feature.

   • Top of Part - The top of the material for the feature. This value is incremental from the Machine Setup or machining origin.

Posting Page

Posting Parameters

1. • Work Offset # - This box allows you to choose which work offset code to use for this feature in the posted NC program. The post processor must be configured to support the work offset selected.

   • Output Rotary Angle - When selected, the angle entered into the Rotation Angle box is output in the posted NC program.

   • • Rotation Angle - When performing 4th axis indexing, the rotary angle is entered here. This box is unavailable until the Output Rotary Angle check box is selected.

Operations Pages

Rough Tool Page

• To learn about creating tools for milling features, please view the Milling Tool Pages.

Patterns Page

Patterns

1. • Zig Zag - A pattern of parallel cuts where the tool feeds in both directions of the pattern.

   • Zig - A pattern of parallel cuts where the tool feeds in one direction and retracts then moves form the end of the last cut to the beginning of the next cut.
      

   • Off Workpiece - When selected, BobCAM begins the facing toolpath by the Distance value.

   • On Workpiece - When selected, BobCAM begins the facing toolpath directly on the edge of the material.
      

   • Distance - When Off Workpiece is selected, enter the distance from the material here.  This distance is added to half of the diameter of the tool, plus the offset.

   • Percent of Tool - When On Workpiece is selected, the percentage of the tool used can be defined.
      

Cut Direction

1. • X Direction - When selected, the tool feeds in the X direction.  This option can be selected for both Zig Zag and Zig.

   • Y Direction - When selected, the tool feeds in the Y direction.  This option can be selected for both Zig Zag and Zig.
      

Parameters

1. • Cut Width % - This box indicates the distance between passes based on a percentage of the cutter width.

   • Length X - This box determines the distance of the facing operation in the X-axis.

   • Length Y - This box determines the distance of the facing operation in the Y-axis.

Parameters Page

Finish

1. • Bottom Allowance - This sets the amount of material that remains on the floor for finishing.  The material is removed on the finish pass. 

Depth

1. • Single Step - The depth entered in the Total Depth box is processed in one pass.

   • Multiple Steps - When selected, the values in the Total Depth and Depth of Cut are used to generate the number of equal cuts used to process the facing operation.

1. • Even Depths - When this option is selected the distance that the tool plunges for each step, at any given point, is equal.

   • Defined Depths - When this option is selected the distance that the tool plunges for each step, at any given point is less than or equal to the Depth of Cut value.

1. 1. • Total Depth - The depth of the material removed by the facing operation.

      • Depth of Cut - When the Multiple Steps option is selected, this box becomes active. The Depth of Cut is the depth at which each equal pass is processed. This value may be different than entered because the value of Number of Cuts must be a whole number and the depth of each pass is the Total Depth divided by the Number of Cuts.

      • Number of Cuts - When the Even Depth option is selected this value is automatically calculated by the system when the Depth of Cut is entered.

Leads Page

Lead In

1. • Length - The distance traveled leading into the surface to tool contact area.
      

Lead Out

• Same As Lead In - When this check box is selected, the Lead Out matches the Lead-In settings.

• 1. • Length - The distance traveled leading away from the surface to tool contact area.

Finish Tool Page

1. • Please see the Milling Tool Pages.