NX Open C++ Reference Guide
Public Member Functions
NXOpen::Features::ThickenBuilder Class Reference

Represents a builder for a Features::Thicken feature. More...

Inheritance diagram for NXOpen::Features::ThickenBuilder:
NXOpen::Features::FeatureBuilder NXOpen::Builder NXOpen::TaggedObject NXOpen::GeometricUtilities::IComponentBuilder

List of all members.

Public Member Functions

bool ApproximateOffset ()
 Returns the "approximate offset surface" or "resolve self-intersections using patches" option.
NXOpen::GeometricUtilities::BooleanOperationBooleanOperation ()
 Returns the boolean operation.
NXOpen::ScCollectorFaceCollector ()
 Returns the faces to thicken.
NXOpen::ExpressionFirstOffset ()
 Returns the first offset.
bool RemoveGashes ()
 Returns the remove gashes option.
bool ReverseDirection ()
 Returns the reverse direction.
NXOpen::ExpressionSecondOffset ()
 Returns the second offset.
void SetApproximateOffset (bool approximateOffset)
 Sets the "approximate offset surface" or "resolve self-intersections using patches" option.
void SetRemoveGashes (bool removeGashes)
 Sets the remove gashes option.
void SetReverseDirection (bool reverseDirection)
 Sets the reverse direction.
void SetTolerance (double tolerance)
 Sets the tolerance.
double Tolerance ()
 Returns the tolerance.

Detailed Description

Represents a builder for a Features::Thicken feature.

This allows creation and editing of a Thicken feature which takes a set of faces and offsets them along their normals to create a solid body which has constant thickness. Since this can not be done precisely for the supported geometry types there is a tolerance to specify the accuracy of the result.
To create a new instance of this class, use Features::FeatureCollection::CreateThickenBuilder
Default values.

Property Value

ApproximateOffset

True

BooleanOperation.Type

Create

FirstOffset.Value

2.5 (millimeters part), 0.1 (inches part)

RemoveGashes

False

ReverseDirection

False

SecondOffset.Value

0.0 (millimeters part), 0.0 (inches part)


Created in NX5.0.0.


Member Function Documentation

Returns the "approximate offset surface" or "resolve self-intersections using patches" option.

The option to approximate offset surfaces for thickening operation is renamed to "resolve self-intersections using patches". This option is available for editing pre-NX8 thicken features only. The value set by the user for this option is ignored for thicken features created from NX8 onwards and its value will always be set to true internally for thicken features created in NX8 and later.
Created in NX5.0.0.

License requirements : None

Returns the boolean operation.

The boolean operation associated with the Thicken feature
Created in NX5.0.0.

License requirements : None

Returns the faces to thicken.

A list of one or more faces to thicken.
Created in NX5.0.0.

License requirements : None

Returns the first offset.

The first offset for the Thicken feature. A positive value is applied along the normal of the face to be thickened. Negative values are applied in the opposite direction. The difference between the first and second offset must be non-zero.
Created in NX5.0.0.

License requirements : None

Returns the remove gashes option.

If the option is selected, Thicken will heal the input and attempt the operation on the healed input. If after healing the input, the Thicken operation succeeds, the Part Navigator will indicate as such with an information symbol and an entry in the Alert column.
Created in NX8.0.0.

License requirements : None

Returns the reverse direction.

A flag to indicate whether the offset direction is reversed with respect to the normal of the face to be thickened.
Created in NX5.0.0.

License requirements : None

Returns the second offset.

the second offset for the Thicken feature.
Created in NX5.0.0.

License requirements : None

Sets the "approximate offset surface" or "resolve self-intersections using patches" option.

The option to approximate offset surfaces for thickening operation is renamed to "resolve self-intersections using patches". This option is available for editing pre-NX8 thicken features only. The value set by the user for this option is ignored for thicken features created from NX8 onwards and its value will always be set to true internally for thicken features created in NX8 and later.
Created in NX5.0.0.

License requirements : solid_modeling ("SOLIDS MODELING")

Parameters:
approximateOffsetapproximateoffset

Sets the remove gashes option.

If the option is selected, Thicken will heal the input and attempt the operation on the healed input. If after healing the input, the Thicken operation succeeds, the Part Navigator will indicate as such with an information symbol and an entry in the Alert column.
Created in NX8.0.0.

License requirements : solid_modeling ("SOLIDS MODELING")

Parameters:
removeGashesremovegashes

Sets the reverse direction.

A flag to indicate whether the offset direction is reversed with respect to the normal of the face to be thickened.
Created in NX5.0.0.

License requirements : solid_modeling ("SOLIDS MODELING")

Parameters:
reverseDirectionreversedirection

Sets the tolerance.

The maximum allowable distance between the true theoretical sheet and the body created to approximate it.
Created in NX5.0.0.

License requirements : solid_modeling ("SOLIDS MODELING")

Parameters:
tolerancetolerance

Returns the tolerance.

The maximum allowable distance between the true theoretical sheet and the body created to approximate it.
Created in NX5.0.0.

License requirements : None


The documentation for this class was generated from the following file:
Copyright 2011 Siemens Product Lifecycle Management Software Inc. All Rights Reserved.