Contour-driven Parameters

If you are working on a process created in a R9 release or higher, the slope parameters are managed by the slope area.

Contour-Driven: Strategy parameters

Contour-Driven: Guiding strategy

Between Contours

There are two ways to define those contours:

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

• Guide 1 and Guide 2 are the two contours between which you are going to machine.
  
• Stop 1 and Stop 2 delimit the ends of the machining paths.

  Stop1 and Stop2 are not taken into account when step over mode is equal to Constant 3D or Maximum 3D. In these cases, it is not possible to select Stop1 and Stop2.

• 4 points on a closed contour

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.
  

• The Contour-driven Between Contours strategy parameters are distributed into 5 tabs.
  By default, all 5 tabs are displayed with all their parameters.
  However, current operations only require a reduced list of those parameters.

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

  • The Axial, Strategy and Island tabs are hidden,

  • as well as Reverse tool path and Max Discretization in the Machining tab

  • and View direction in the Radial tab.

• 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.

• By default, all tabs and all parameters are displayed:
  

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

Parallel contour

Select a contour on the part to be the reference for your operation.

• The Contour-driven Parallel Contour strategy parameters are distributed into 5 tabs.
  By default, all 5 tabs are displayed with all their parameters.
  However, current operations only require a reduced list of those parameters.

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

  • The Axial and Island tabs are hidden,

  • as well as Reverse tool path and Max Discretization in the Machining tab,

  • View direction in the Radial tab

  • and Pencil rework in the Strategy tab.

• 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.

• By default, all tabs and all parameters are displayed:
  

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

Spine Contour

Select a contour on the part to be the reference for your operation.

• The Contour-driven Spine contour  strategy parameters are distributed into 5 tabs
  (but the Strategy tab is not available).
  By default, all 5 tabs are displayed with all their parameters.
  However, current operations only require a reduced list of those parameters.

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

  • The Axial, Strategy and Island tabs are hidden,

  • as well as Reverse tool path and Max Discretization in the Machining tab

  • and View direction in the Radial tab.

• 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.

• 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.

Contour-Driven: Machining parameters 

For Between contours

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

For Parallel contour

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

For Spine contour

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

Tool path style 

• One-way next: the tool path always has the same direction during successive passes and goes diagonally
  rom 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. 

• 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.

Contour-Driven: Radial parameters

For Between contours

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

For Parallel contour

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

Spine contour

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

Stepover type:

The stepover type depends on the Guiding strategy:

• for Between contours, those types are available:
  • Constant 2D,
  • Via scallop height,
  • Constant 3D,
  • Maximum 3D.

• for Parallel contour, those types are available:
  • Constant 2D,
  • Via scallop height,
  • Constant 3D.
• for Spine contour, those types are available:
• Constant 2D,
• Via scallop height.

Use the list to select one of them. The corresponding parameters will be displayed accordingly.

• Constant2D: Has a  maximum stepover distance defined in a plane and projected onto the part. 

  

  The parameters to define are:
  

  • Max. distance between paths
    

  • 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.

• 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:
  
  • Max. distance between paths and Minimum distance between paths
    
  • Scallop height i.e.  the maximum thickness remaining between two paths.

• 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:
  • Distance between paths: the constant distance between two successive paths
    (measured relatively to tool tips)
    
  • Sweeping strategy, i.e. where you want to start machining and where you want to end, the possibilities are:

  • From guide 1 to guide 2 (starts at guide 1 and ends at guide 2)
    

  • From guide 2 to guide 1 (starts at guide 2 and ends at guide 1),
    

  • From guide to zone center
    (starts at guide 1 and works towards the center of the zone
    then goes to guide 2 and works towards the center of the zone),
    

  • From zone center to guide
    (starts at the center of the zone and works towards guide 1
    then comes back to the center and works towards guide 2),

  • From guide to zone center (spiral)
    (starts at guide 1 and spirals towards the center),
    

  • From zone center to guide (spiral)
    (starts at the center and spirals towards the guide contours),
    

  • Reference 
    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

Tool initial Position with respect to the guide contour (inside, outside, on),

• On:
  
• Inside:
  
• Outside:
  

Offset on guide 1, Offset on guide 2

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.

When Other axis is active, select this check box to search for toolholder-part collisions.

Contour-Driven: Axial parameters  

For Between contours

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

For Parallel contour

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

For Spine contour

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

Multi-pass

Use the list to select the mode of input:

• Maximum cut depth and total depth: Enter the Total depth and the Maximum cut depth
  
• Number of levels and total depth: Enter the Number of levels and the Total depth
  .
• Number of levels and Maximum cut depth: Enter the Number of levels and the Maximum cut depth.
  

Only two can be selected at time, you select which two via the input mode choice.
The example below was obtained with 3 levels at a cut depth of 5mm, but could just as easily have  been obtained by:

• A cut depth of 5mm and a total depth of 15 mm,
• or a total depth of 15 mm and 3 levels. 
  

Contour-Driven: Strategy parameters

For Between contours

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

For Parallel contour

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

For Spine contour

Not available

Those parameters depend on the Guiding strategy as listed above.

Pencil rework  

Lets you start an automatic pencil operation (defined with a set of default parameters)
at the end of the contour driven operation.

Offset on contour 

Distance the tool will be from the guide contour at the beginning of the operation

Maximum width to machine 

Defines the width of the area to machine starting from the guide contour,

Stepover side

Defines the side of the contour where machining will be performed (left or right), i.e. if you choose Left,
the tool will machine on the left side of the guide contour for the Maximum width distance,

Direction 

• To contour: the tool path  starts parallel to the guide at the width to machine and
  the stepover is done towards the guide 
• From contour: the tool path  starts parallel to the guide contour  and the stepover follows 
  the offset side up to the width to machine 

Initial tool position

Position where the tool will start with respect to the guide contour (in red); it can be:

to	on	past

Contour-Driven: Island parameters

For Between contours

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

For Parallel contour

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

For Spine contour

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

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 below, 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.

Contour-Driven: Geometry

• Part with possible offset on part (double-click  the label).
• Check element with possible offset on check element (double-click  the label).
  The check is often a clamp that holds the part and therefore is not an area to be machined.

  The tool path quality is improved along "between paths" if check surfaces are selected.

• Area to avoid if you do not wish to machine it (light brown area in the left hand corner near the part selection area).

• 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. The safety plane contextual menu allows you to define:

• an offset safety plane at a distance that you give in a dialog box that is displayed.
  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

• and the tool retract mode which may be either normal to the safety plane or normal to the tool axis.

• 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,
• Limiting contour which defines the machining limit on the part.
  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.

• Guide contours and Stop contours (only used for machining with parallel contours) are defined
  within the Guiding strategy.
• The picture is slightly different if you are using a rework area and will have fewer parameters.

When using a rework area, please remember to use a smaller tool than the one defined the rework area as
this is necessary to ensure the generation of a tool path inside it. 

If you are editing a rework, an additional information is displayed, indicating which type of subset you are working on.
This field is not editable (you can not go from one subset to another).

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

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

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.