NX Open C++ Reference Guide
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Represents a Features::PatternFeature builder
To create a new instance of this class, use Features::FeatureCollection::CreatePatternFeatureBuilder
Default values.
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Public Types | |
enum | ExpressionTransferOptions { ExpressionTransferOptionsCreateNew, ExpressionTransferOptionsLinkToOriginal, ExpressionTransferOptionsOriginalInstance } |
the Expression transfer options. More... | |
enum | OutputOptions { OutputOptionsPatternFeature, OutputOptionsCopiesOfInputFeatures, OutputOptionsCopiesOfInputFeaturesInGroup } |
the Output options. More... | |
enum | PatternMethodOptions { PatternMethodOptionsVariational = 1, PatternMethodOptionsSimple } |
the Pattern method options. More... | |
Public Member Functions | |
void | ClearReferencesToReuse () |
Clears all the existing references to reuse so that new references can be added Created in NX8.0.0. | |
bool | CreateReferencePattern () |
Returns the Create Reference Pattern option Created in NX8.0.0. | |
NXOpen::Features::PatternFeatureBuilder::ExpressionTransferOptions | ExpressionOption () |
Returns the expression transfer option Created in NX7.5.0. | |
NXOpen::Features::SelectFeatureList * | FeatureList () |
Returns the Features Created in NX7.5.0. | |
NXOpen::Features::PatternFeatureBuilder::OutputOptions | OutputOption () |
Returns the output option Created in NX8.0.0. | |
NXOpen::Features::PatternFeatureBuilder::PatternMethodOptions | PatternMethod () |
Returns the Pattern method Created in NX7.5.0. | |
NXOpen::GeometricUtilities::PatternDefinition * | PatternService () |
Returns the Pattern definition service Created in NX7.5.0. | |
NXOpen::Point * | ReferencePoint () |
Returns the reference point Created in NX7.5.0. | |
void | RemoveAllClocking () |
Removes clocking from (unclocks) all instances of the Features::PatternFeature . | |
void | SetCreateReferencePattern (bool createReferencePattern) |
Sets the Create Reference Pattern option Created in NX8.0.0. | |
void | SetExpressionOption (NXOpen::Features::PatternFeatureBuilder::ExpressionTransferOptions expressionOption) |
Sets the expression transfer option Created in NX7.5.0. | |
void | SetOutputOption (NXOpen::Features::PatternFeatureBuilder::OutputOptions outputOption) |
Sets the output option Created in NX8.0.0. | |
void | SetPatternMethod (NXOpen::Features::PatternFeatureBuilder::PatternMethodOptions methodOption) |
Sets the Pattern method Created in NX7.5.0. | |
void | SetReferencePoint (NXOpen::Point *referencePoint) |
Sets the reference point Created in NX7.5.0. | |
void | SetReferencesToReuse (NXOpen::Features::Feature *inputFeature, const std::vector< NXOpen::NXObject * > &referencesFromInputFeatures) |
Sets the references or selections from the input features which are to be reused for all instances. | |
void | SetUseInferredReferencePoint (bool useInferredReferencePoint) |
Sets a flag to indicate whether to use reference point inferred from selected feature(s) or not. | |
bool | UseInferredReferencePoint () |
Returns a flag to indicate whether to use reference point inferred from selected feature(s) or not. |
Represents a Features::PatternFeature builder
To create a new instance of this class, use Features::FeatureCollection::CreatePatternFeatureBuilder
Default values.
Property | Value |
---|---|
CreateReferencePattern |
True |
ExpressionOption |
CreateNew |
OutputOption | |
PatternMethod |
Variational |
PatternService.AlongPathDefinition.XOnPathSpacing.NCopies.Value |
2 |
PatternService.AlongPathDefinition.XOnPathSpacing.SpaceType | |
PatternService.AlongPathDefinition.XPathOption | |
PatternService.AlongPathDefinition.YDirectionOption | |
PatternService.AlongPathDefinition.YOnPathSpacing.NCopies.Value |
1 |
PatternService.AlongPathDefinition.YPathOption | |
PatternService.AlongPathDefinition.YSpacing.NCopies.Value |
1 |
PatternService.AlongPathDefinition.YSpacing.PitchDistance.Value |
10 (millimeters part), 1 (inches part) |
PatternService.AlongPathDefinition.YSpacing.SpaceType | |
PatternService.AlongPathDefinition.YSpacing.SpanDistance.Value |
100 (millimeters part), 10 (inches part) |
PatternService.CircularDefinition.AngularSpacing.NCopies.Value |
12 |
PatternService.CircularDefinition.AngularSpacing.PitchAngle.Value |
30 |
PatternService.CircularDefinition.AngularSpacing.PitchDistance.Value |
10 (millimeters part), 1 (inches part) |
PatternService.CircularDefinition.AngularSpacing.SpaceType | |
PatternService.CircularDefinition.AngularSpacing.SpanAngle.Value |
360 (millimeters part), 360 (inches part) |
PatternService.CircularDefinition.AngularSpacing.UsePitchOption |
Angle |
PatternService.CircularDefinition.CreateLastStaggered |
true |
PatternService.CircularDefinition.HorizontalRef.RotationAngle.Value |
0 (millimeters part), 0 (inches part) |
PatternService.CircularDefinition.IncludeSeedToggle |
true |
PatternService.CircularDefinition.RadialSpacing.NCopies.Value |
1 |
PatternService.CircularDefinition.StaggerType |
None |
PatternService.PatternFill.FillMargin.Value |
0 (millimeters part), 0 (inches part) |
PatternService.PatternFill.FillOptions |
None |
PatternService.PatternFill.SimplifiedBoundaryToggle |
False |
PatternService.PatternOrientation.AlongOrientationOption |
NormalToPath |
PatternService.PatternOrientation.CircularOrientationOption |
FollowPattern |
PatternService.PatternOrientation.FollowFaceProjDirOption |
PatternPlaneNormal |
PatternService.PatternOrientation.GeneralOrientationOption | |
PatternService.PatternOrientation.LinearOrientationOption | |
PatternService.PatternOrientation.MirrorOrientationOption |
FollowPattern |
PatternService.PatternOrientation.OrientationOption (deprecated) | |
PatternService.PatternOrientation.PolygonOrientationOption |
FollowPattern |
PatternService.PatternOrientation.SpiralOrientationOption |
FollowPattern |
PatternService.PatternType |
Linear |
PatternService.PolygonDefinition.NumberOfSides.Value |
6 |
PatternService.PolygonDefinition.PolygonSizeOption |
Inscribed |
PatternService.PolygonDefinition.PolygonSpacing.NCopies.Value |
4 |
PatternService.PolygonDefinition.PolygonSpacing.PitchDistance.Value |
25 (millimeters part), 1 (inches part) |
PatternService.PolygonDefinition.PolygonSpacing.SpaceType | |
PatternService.PolygonDefinition.PolygonSpacing.SpanAngle.Value |
360 |
PatternService.PolygonDefinition.RadialSpacing.NCopies.Value |
1 |
PatternService.PolygonDefinition.RadialSpacing.PitchDistance.Value |
25 (millimeters part), 1 (inches part) |
PatternService.PolygonDefinition.RadialSpacing.SpanDistance.Value |
100 (millimeters part), 4 (inches part) |
PatternService.RectangularDefinition.CreateLastStaggered |
true |
PatternService.RectangularDefinition.SimplifiedLayoutType |
Square |
PatternService.RectangularDefinition.StaggerType |
None |
PatternService.RectangularDefinition.XSpacing.NCopies.Value |
2 |
PatternService.RectangularDefinition.YSpacing.NCopies.Value |
1 |
PatternService.SpiralDefinition.DirectionType |
Lefthand |
PatternService.SpiralDefinition.NumberOfTurns.Value |
1 (millimeters part), 1 (inches part) |
PatternService.SpiralDefinition.RadialPitch.Value |
50 (millimeters part), 2 (inches part) |
PatternService.SpiralDefinition.SizeSpiralType |
NumberOfTurns |
PatternService.SpiralDefinition.TotalAngle.Value |
360 (millimeters part), 360 (inches part) |
UseInferredReferencePoint |
True |
Created in NX7.5.0.
the Expression transfer options.
Clears all the existing references to reuse so that new references can be added
Created in NX8.0.0.
License requirements : solid_modeling ("SOLIDS MODELING")
Returns the Create Reference Pattern option
Created in NX8.0.0.
License requirements : None
NXOpen::Features::PatternFeatureBuilder::ExpressionTransferOptions NXOpen::Features::PatternFeatureBuilder::ExpressionOption | ( | ) |
Returns the expression transfer option
Created in NX7.5.0.
License requirements : None
Returns the Features
Created in NX7.5.0.
License requirements : solid_modeling ("SOLIDS MODELING")
NXOpen::Features::PatternFeatureBuilder::OutputOptions NXOpen::Features::PatternFeatureBuilder::OutputOption | ( | ) |
Returns the output option
Created in NX8.0.0.
License requirements : None
NXOpen::Features::PatternFeatureBuilder::PatternMethodOptions NXOpen::Features::PatternFeatureBuilder::PatternMethod | ( | ) |
Returns the Pattern method
Created in NX7.5.0.
License requirements : None
NXOpen::GeometricUtilities::PatternDefinition* NXOpen::Features::PatternFeatureBuilder::PatternService | ( | ) |
Returns the Pattern definition service
Created in NX7.5.0.
License requirements : None
Returns the reference point
Created in NX7.5.0.
License requirements : None
Removes clocking from (unclocks) all instances of the Features::PatternFeature .
Created in NX8.0.0.
License requirements : solid_modeling ("SOLIDS MODELING")
void NXOpen::Features::PatternFeatureBuilder::SetCreateReferencePattern | ( | bool | createReferencePattern | ) |
Sets the Create Reference Pattern option
Created in NX8.0.0.
License requirements : solid_modeling ("SOLIDS MODELING")
createReferencePattern | createreferencepattern |
void NXOpen::Features::PatternFeatureBuilder::SetExpressionOption | ( | NXOpen::Features::PatternFeatureBuilder::ExpressionTransferOptions | expressionOption | ) |
Sets the expression transfer option
Created in NX7.5.0.
License requirements : solid_modeling ("SOLIDS MODELING")
expressionOption | expressionoption |
void NXOpen::Features::PatternFeatureBuilder::SetOutputOption | ( | NXOpen::Features::PatternFeatureBuilder::OutputOptions | outputOption | ) |
Sets the output option
Created in NX8.0.0.
License requirements : solid_modeling ("SOLIDS MODELING")
outputOption | outputoption |
void NXOpen::Features::PatternFeatureBuilder::SetPatternMethod | ( | NXOpen::Features::PatternFeatureBuilder::PatternMethodOptions | methodOption | ) |
Sets the Pattern method
Created in NX7.5.0.
License requirements : solid_modeling ("SOLIDS MODELING")
methodOption | methodoption |
void NXOpen::Features::PatternFeatureBuilder::SetReferencePoint | ( | NXOpen::Point * | referencePoint | ) |
Sets the reference point
Created in NX7.5.0.
License requirements : solid_modeling ("SOLIDS MODELING")
referencePoint | referencepoint |
void NXOpen::Features::PatternFeatureBuilder::SetReferencesToReuse | ( | NXOpen::Features::Feature * | inputFeature, |
const std::vector< NXOpen::NXObject * > & | referencesFromInputFeatures | ||
) |
Sets the references or selections from the input features which are to be reused for all instances.
The references for reuse should belong to some input feature which needs to be specified while calling this API.
Created in NX8.0.0.
License requirements : solid_modeling ("SOLIDS MODELING")
inputFeature | inputfeature |
referencesFromInputFeatures | referencesfrominputfeatures |
void NXOpen::Features::PatternFeatureBuilder::SetUseInferredReferencePoint | ( | bool | useInferredReferencePoint | ) |
Sets a flag to indicate whether to use reference point inferred from selected feature(s) or not.
If 'true', the reference point will be inferred every time the selected feature(s) get modified or updates. If 'false, the reference point provided will be independent of the selected feature(s) but will be associative to the rule by which it was created (e.g. End of Line, Center of Arc).
Created in NX8.0.0.
License requirements : solid_modeling ("SOLIDS MODELING")
useInferredReferencePoint | useinferredreferencepoint |
Returns a flag to indicate whether to use reference point inferred from selected feature(s) or not.
If 'true', the reference point will be inferred every time the selected feature(s) get modified or updates. If 'false, the reference point provided will be independent of the selected feature(s) but will be associative to the rule by which it was created (e.g. End of Line, Center of Arc).
Created in NX8.0.0.
License requirements : None