Contour-Driven Between Contour Parameters

 

  The information in this section describes the Between Contour strategy parameters.

In addition to the Guiding Strategy, those parameters are found in the following tabs:

By default, all those tabs are displayed with all their parameters.
However, most operations only require a reduced list of those parameters.

  • Click <<Less button to display only those parameters.

  • Click More>> button to re-display all parameters.

  • You can also use the modal option User Interface Simplified mode in the
    Tools  >  Options  >  Machining  >  Operation     tab.

Between Contour:  Guiding Strategy

4 open contours (i.e. that are not necessarily perfectly connected to each other)

  • With Stepover set to Constant 3D or Maximum 3D.
    Guide 1     and Guide 2 are the two contours between which you are going to machine.
  • With Stepover set to Constant 2D or Via scallop height.
    Stop 1     and Stop 2 delimit the ends of the machining paths.

4 points on a closed contour, with all stepover types.
Select four points on the contour in the order that you see in the sensitive icon.

  • P1, P2, P3 and P4 are the four points that you select on the contour within which you are going to machine.

By default, all tabs and all parameters are displayed:

Click <<Less to display a reduced list of tabs and parameters:

Click here for information about the 3/5-Axis Converter option.

Between Contours:  Machining Parameters 

  • By default, or when the More>> button is pressed:
  • When the <<Less button is pressed:

The parameters to define are:

  • Tool path style:
    • One-way next: the tool path always has the same direction during successive passes and goes diagonally from the end of one tool path to the beginning of the next.
    • One-way same: the tool path always has the same direction during successive passes and returns
      to the first point in each pass before moving on to the first point in the next pass.
    • Zig-zag: the tool path alternates directions during successive passes.
  • Machining tolerance: Maximum allowed distance between the theoretical and computed tool path.
    consider it to be the acceptable chord error.
  • Reverse tool path: Hidden when the <<Less button is pressed.

  • Max Discretization:Hidden when the <<Less button is pressed.
    For some surfaces, such as flat surfaces, the tool path can suffer from a lack of points.
    By setting the maximum discretization distance, the gaps will be filled by the exact surface points resulting in a better distribution of points,  a smoother tool path and then a better machining quality.
In addition, two Distribution Modes are available to improve the quality of the machined surface.
  • With Aligned, the points of the tool path are aligned (as best as possible)
    with those of the tool paths below and above.

    Resulting surface
    (Zoom on details)

  • With Shifted, the points of the tool path do not form a line with those of the  tool paths below and above.

    Resulting surface
    (Zoom on details)
  • This parameter is available with a spherical tool only.
  • This parameter is available with the Constant 3D option only.
  • The number of points of the tool paths will vary with the distribution mode.
 

Between Contours:  Radial parameters

  • By default, or when the More>> button is pressed:
  • When the <<Less button is pressed:

Stepover: the types are available:

  • Constant 2D,
  • Via scallop height,
  • Constant 3D,
  • Maximum 3D.

Use the list to select one of them. The corresponding parameters will be displayed accordingly.
In rework and finishing operations, we recommend that you set the Stepover to Constant 2D or Via scallop height for machining areas that are almost horizontal (i.e. without vertical walls).
The Stepover types Constant 3D and Maximum 3D are more suitable for machining areas with vertical walls.
 

Constant 2D: Has a  maximum stepover distance defined in a plane and projected onto the part. 

The parameters to define are:

  • Scallop height
    defines the maximum allowable height of the crests of material left uncut after machining.  
    If you enter a Scallop height, the Max. distance between paths is computed automatically.

  • Same offset on stops: When an offset is set on guides, you can choose to apply the same offset on stops by selecting the check box.

Via scallop height

The stepover is computed from the scallop height you have set, within the range defined by
Max. distance between paths and Min. distance between paths.
The stepover depends on the scallop height that you choose. 
All selected geometries are taken into account in the stepover computation even if these geometries are not milled.
For example, filled holes or vertical walls outside the limiting contour influence the stepover computation and may generate useless paths. The by-pass consists in not selecting these useless geometries to compute the toolpath.
The parameters to define are:

Constant 3D:  Stepover with a constant distance measured relatively to the tool tips in 3D space.

and Maximum 3D:  stepover limited to a maximum distance measured relatively to the tool tips in 3D space.

The parameters to define are:

  • Reference 
    Available for Between contours and Parallel contour.
    Defines whether the tool end or the tool contact point is used for the computation:
    • If stepover mode is Constant 3D or Maximum 3D, it is possible to choose a Tool end or a Contact point reference.
    • If stepover mode is Constant 2D or Scallop height, the reference is always Tool end.
      Contact point:
      Tool end:
  • Position on guide 1, Position on guide 2 (for all stepover types):
    Tool initial Position with respect to the guide contour (inside, outside, on),

    • On:
    • Inside:
    • Outside:
  • Offset on guide 1, Offset on guide 2  (for all stepover types):
    Tool Offset with respect to the guide contour. 
    With a negative value the tool path will start outside the guide contour,
    with a positive value it will start inside the guide contour.
  • You can define a different offset and a different position on each guide for
    the four types of Stepover (Maximum 3D, Constant 3D, Constant 2D, Via scallop height).
  • The default values of guide 2 are those of guide 1.
  • If you open a process created with a previous version of V5, the Offset on guide and Position values
    defined in this process are propagated automatically to guide 1 and guide 2.
  • If 2 negative offsets are defined and if the offset guide contours intersect each other,
    the replay is stopped and an error message is displayed.
  • If 2 positive offsets are defined and if stop contours are selected, stop contours are extended
    (linear extension) so as to define a closed domain.
  • If at least 1 negative offset is defined, stop contours are ignored.
 
  • View Direction
    (Hidden when the <<Less button is pressed, active with a Constant 2D or a stepover Via scallop height)

    • Along tool axis is used to compute the stepover distance, as if you were looking along the tool axis. 
    • Other axis is used to compute the stepover distance, as if you ware looking along an axis other than the tool axis.
      The icon at the top of the tab for axis selection has changed and you can now select an axis
      (the oblique axis in the icon) other than the tool axis for the view direction.
      Other axis can only be used with a ball-nose tool. 
  • Collision check
    When Other axis is active, select this check box to search for toolholder-part collisions.

Between Contours:  Axial Parameters  

The tab is hidden when the <<Less button is pressed.

The parameters to define are:

Between Contours:  Strategy Parameters

The tab is hidden when the <<Less button is pressed.

The parameters to define are:

  • Pencil rework:  Lets you start an automatic pencil operation (defined with a set of default parameters) at the end of the contour driven operation.
  • Follow check border: Available with Between Contours, and when the stepover is set to Constant 3D or Maximum 3D.
    When this check box is selected, if there is some check in the area to sweep, the pattern follows the border of the check.

    When this check box is cleared, the pattern fully respects the guideline and does not take the check into account.

Between Contours:  Island Parameters

The tab is hidden when the <<Less button is pressed.

The parameters to define are:

  • Island skip: Select this check box if you want to use intermediate approaches and retracts
    (i.e. those that link two different areas to machine and that are not at the beginning nor  the end of the tool path).
    • With Island skip selected:

    • With Island skip cleared:

     
  • Direct: When this check box is selected, the tool is not allowed to rise on intermediate approaches and retracts.
    When Direct is not checked, the tool will rise to 10 mm on intermediate approaches and retracts.
  • Feedrate length: Defines the distance beyond which tool path straight lines will be replaced by intermediate approaches and retracts.
    In the picture above, the Feedrate length was set to 45 mm.
    Note that the gaps that were less than 45 mm are crossed by a straight line tool path and those that are greater than 45 mm are crossed with a standard intermediate tool path with an approach and a retract.
Feedrate length is only active if the Direct check box is selected.