Contour-driven Parameters

The information in this section will help you create and edit Contour-driven operations in your Manufacturing Program.

For all strategy types, click:

to define the geometry of the part to machine,
to specify the tool to use (you have the choice of end mill or conical tools for this operation),
to define the feedrates and spindle speeds,
to define transition paths in your machining operations by means of NC macros as needed,
to define strategy parameters: those parameters depend on the cycle type you choose, as listed below.

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. Whole tabs or only some parameters in a given tab will be hidden. They are marked hidden in the table below.
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.
Complete information on parameters common to all three strategies is given in the Between Contours section.
In the other two sections (Parallel contour and Spine contour), you will find:
- a list of the relevant parameters with a link to the complete information,
- information specific to that contour strategy.
Below is a summary of those parameters:

Between Contours:

In the machining strategy tab, use

the sensitive icon:

to define the tool axis,

to visualize the tool path style that you chose.

the 3/5-Axis Converter option.

Parallel contour:

In the machining strategy tab, use

the sensitive icon:

to define the tool axis,

to visualize the tool path style that you chose.

the 3/5-Axis Converter option.

Spine contour:

In the machining strategy tab, use

the sensitive icon:

to define the tool axis,

to visualize the tool path style that you chose.

the 3/5-Axis Converter option.

the Machining tab to define:

the Tool path style,

the Machining tolerance,

activate the Reverse tool path (hidden) and Max Discretization (hidden) with its Step and Distribution mode options.

the Machining tab to define:

the Tool path style,

the Machining tolerance,

activate the Reverse tool path (hidden) and Max Discretization (hidden) with its Step and Distribution mode) options.

the Machining tab to define:

the Tool path style,

the Machining tolerance,

activate the Reverse tool path (hidden) and Max Discretization (hidden) with its Step and Distribution mode options.

the Radial tab to define the stepover type:

Constant 2D (though Max. distance between paths, Scallop height),

Constant 3D or Maximum 3D (through Distance between paths, Sweeping strategy, Reference, Position, Offset),

Via scallop height (Max. distance between paths, Min. distance between paths, Scallop height),

the Reference (for Constant 3D or Maximum 3D),
the Position on guide,
the Offset on guide and on stops,
or activate the Along tool axis (hidden) or Other axis (hidden) options.

the Radial tab to define:

Constant 2D (though Max. distance between paths, Scallop height),

Constant 3D (through Distance between paths),

Via scallop height (through Maximum and Minimum distances between paths, Scallop height),

the Reference (for Constant 3D or Maximum 3D),
or activate the Along tool axis (hidden) or Other axis (hidden) options.

the Radial tab to define:

Constant 2D (though Max. distance between paths, Scallop height),

Via scallop height (through Maximum and Minimum distances between paths, Scallop height),

or activate the Along tool axis (hidden) or Other axis (hidden) options.

the Axial tab (hidden) to define:

the Multi-pass,

the Number of levels,

the Maximum cut depth,

the Total depth.

the Axial tab (hidden) to define:

the Multi-pass,

the Number of levels,

the Maximum cut depth,

the Total depth.

the Axial tab (hidden) to define:

the Multi-pass,

the Number of levels,

the Maximum cut depth,

the Total depth.

the Strategy tab (hidden) to activate:

the Pencil rework option,

the Follow check border option.

the Strategy tab:

to activate the Pencil rework option (hidden),

to define the Offset on contour,

the Maximum width to machine,

the Stepover side,

the Strategy side,

the Direction,

the Initial tool position.

the Strategy tab is not available.

the Island tab (hidden):

to activate the Island skip or the Direct option,

to define the Feedrate length.

the Island tab (hidden):

to activate the Island skip or the Direct option,

to define the Feedrate length.

the Island tab (hidden):

to activate the Island skip or the Direct option,

to define the Feedrate length.

The Machined Zone tab has been removed from the machining strategy.
However, if you are working on a process created in a R8 release, with values other than the default values,
the Machined Zone tab is displayed with the maximum slope that can be considered to be horizontal
(any area that is considered to be horizontal will not be machined),

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: Geometry

You can specify the following 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 (small light brown corner near the part selection area).
This is in fact a list of faces removed from from the list of faces built from the Part.
Those removed faces are not taken into account to compute the tool path.
Use Area to avoid for a quick definition of a sub-element of the Part you want to machine.
For example, you want to machine the Part below, but not its pocket.

To do so:

select the whole part as the Part,

then define the Area to avoid by selecting the faces of the pocket.

A longer alternative would be to define the Part face by face.

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. See also Defining the Guide in Parallel Contour Mode.
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.

Subset
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).

Info
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.