DimpleBuilder Class — NXOpen Python API Reference 12.0.0 documentation

# DimpleBuilder Class

class `NXOpen.Features.SheetMetal.``DimpleBuilder`

  Bases: `NXOpen.Features.FeatureBuilder`

  Represents a Dimple feature builder.

  To create a new instance of this class, use `NXOpen.Features.SheetMetal.SheetmetalManager.CreateDimpleFeatureBuilder()`

  New in version NX4.0.0.

# Properties

Property | Description
--- | ---
DepthType | Returns or sets the Direction in which the Dimple is punched.
DimensionType | Returns or sets the Offset Dimension
FilletSectionCorners | Returns or sets the Rounding Option for section Corners which contain Non Fillet Radii
IncludeRounding | Returns or sets the Rounding type of the Sharp edges of bottom face and top face.
MinimumToolClearance | Returns the minimum tool clearance expression.
ParentFeatureInternal | Returns or sets whether or not the latest timestamped parent feature of this feature should be made internal
PatchSolutionFlag | Returns or sets the patch solution flag
PatchSurfaceFilename | Returns or sets the patch surface filename
Section | Returns or sets the Section used by the Dimple.
SectionSide | Returns or sets the section Side for the Dimple section.
SidewallType | Returns or sets the side where the material must be added to the dimple.
Sketch | Returns or sets the Slave Sketch used by the Dimple, If one exists.
SurroundingPatchSurfaceFilename | Returns or sets the surrounding patch surface filename
Tag | Returns the Tag for this object.

# Methods

Method | Description
--- | ---
Commit | Commits any edits that have been applied to the builder.
CommitFeature | Commits the feature parameters and creates the feature
Destroy | Deletes the builder, and cleans up any objects created by the builder.
GetCommittedObjects | For builders that create more than one object, this method returns the objects that are created by commit.
GetDepth | Depth of the Dimple
GetDieRadius | Radius value of the sharp edges of the bottom face
GetFeature | Returns the feature currently being edited by this builder.
GetFilletRadius | Fillet Radius to be applied for rounding the Sharp section Corners
GetObject | Returns the object currently being edited by this builder.
GetPunchRadius | Radius value of the sharp edges on the top face
GetTaperAngle | Taper Angle of the Dimple.
HideInternalParentFeatureAfterEdit | Re-suppress an internal parent feature (a slave feature) after it has been edited.
SetDepth |
SetDieRadius |
SetFilletRadius |
SetParentFeatureInternal | Set the parent features which would be internal or slaves to the feature being created or commited
SetPunchRadius |
SetTaperAngle |
ShowInternalParentFeatureForEdit | Unsuppress an internal parent feature (a slave feature) so it can be edited.
ShowResults | Updates the model to reflect the result of an edit to the model for all builders that support showing results.
UnsetParentFeatureInternal | Set the internal parent feature of the feature being edited to external
Validate | Validate whether the inputs to the component are sufficient for commit to be called.
ValidateBuilderData | Verify whether the builder data is valid for creating a dimple or not.

# Enumerations

DimpleBuilderDepthTypeOptions Enumeration | This enum represents the depth direction for the dimple.
DimpleBuilderDimensionTypeOptions Enumeration | the Dimension options for dimple.
DimpleBuilderSectionSideOptions Enumeration | This enum represents the side of the section that the dimple punches material.
DimpleBuilderSidewallTypeOptions Enumeration | the side walls material option.

# Property Detail

## DepthType

`DimpleBuilder.``DepthType`

  Returns or sets the Direction in which the Dimple is punched.

  This is used to specify the direction in which the punching should happen. If Punching must happen in the direction of the Section Normal (specified using the `NXOpen.Features.SheetMetal.DimpleBuilder.Section`()`) then pass the value of `NXOpen.Features.SheetMetal.DimpleBuilderDepthTypeOptions.SectionNormalSide` If punching must happen in the opposite direction to that of Section Normal, set the value to be `NXOpen.Features.SheetMetal.DimpleBuilderDepthTypeOptions.SectionReverseNormalSide`

  `-------------------------------------`

  Getter Method

  Signature `DepthType`

  Returns: |
  Return type: | `NXOpen.Features.SheetMetal.DimpleBuilderDepthTypeOptions`

  New in version NX4.0.0.

  License requirements: nx_sheet_metal (“NX Sheet Metal”)

  `-------------------------------------`

  Setter Method

  Signature `DepthType`

  Parameters: | depthType (`NXOpen.Features.SheetMetal.DimpleBuilderDepthTypeOptions`) –

  New in version NX4.0.0.

  License requirements: nx_sheet_metal (“NX Sheet Metal”)

## DimensionType

`DimpleBuilder.``DimensionType`

  Returns or sets the Offset Dimension

  The actual extent distance of the Dimple will be determined by the active dimension option. In case of `NXOpen.Features.SheetMetal.DimpleBuilderDimensionTypeOptions.Offset` the actual extent distance will be offset dimension distance plus the thickness of sheet. In case of `NXOpen.Features.SheetMetal.DimpleBuilderDimensionTypeOptions.Full` the actual extent distance will be the Full dimension distance.

  `-------------------------------------`

  Getter Method

  Signature `DimensionType`

  Returns: |
  Return type: | `NXOpen.Features.SheetMetal.DimpleBuilderDimensionTypeOptions`

  New in version NX4.0.0.

  License requirements: nx_sheet_metal (“NX Sheet Metal”)

  `-------------------------------------`

  Setter Method

  Signature `DimensionType`

  Parameters: | dimensionType (`NXOpen.Features.SheetMetal.DimpleBuilderDimensionTypeOptions`) –

  New in version NX4.0.0.

  License requirements: nx_sheet_metal (“NX Sheet Metal”)

## FilletSectionCorners

`DimpleBuilder.``FilletSectionCorners`

  Returns or sets the Rounding Option for section Corners which contain Non Fillet Radii

  `-------------------------------------`

  Getter Method

  Signature `FilletSectionCorners`

  Returns: |
  Return type: | bool

  New in version NX4.0.0.

  License requirements: nx_sheet_metal (“NX Sheet Metal”)

  `-------------------------------------`

  Setter Method

  Signature `FilletSectionCorners`

  Parameters: | filletSectionCorners (bool) –

  New in version NX4.0.0.

  License requirements: nx_sheet_metal (“NX Sheet Metal”)

## IncludeRounding

`DimpleBuilder.``IncludeRounding`

  Returns or sets the Rounding type of the Sharp edges of bottom face and top face.

  `-------------------------------------`

  Getter Method

  Signature `IncludeRounding`

  Returns: |
  Return type: | bool

  New in version NX4.0.0.

  License requirements: nx_sheet_metal (“NX Sheet Metal”)

  `-------------------------------------`

  Setter Method

  Signature `IncludeRounding`

  Parameters: | includeRounding (bool) –

  New in version NX4.0.0.

  License requirements: nx_sheet_metal (“NX Sheet Metal”)

## MinimumToolClearance

`DimpleBuilder.``MinimumToolClearance`

  Returns the minimum tool clearance expression.

  `-------------------------------------`

  Getter Method

  Signature `MinimumToolClearance`

  Returns: |
  Return type: | `NXOpen.Expression`

  New in version NX6.0.0.

  License requirements: nx_sheet_metal (“NX Sheet Metal”)

## Section

`DimpleBuilder.``Section`

  Returns or sets the Section used by the Dimple.

  Section can be Open/Closed.

  The section is protruded on the reference face at finite distance of extent and in the direction of extent side. The actual extent distance will be determined by the active dimension option i.e. Offset Dimension or Full Dimension. In case of Offset Dimension the actual extent distance will be offset dimension distance plus the thickness of sheet. In case of Full Dimension the actual extent distance will be the Full dimension distance. In case of open section, the end segments are extended to the nearest flat face edges. If the end segments are already crossing the flat face edges, those segments will be trimmed to the edges.

  `-------------------------------------`

  Getter Method

  Signature `Section`

  Returns: |
  Return type: | `NXOpen.Section`

  New in version NX4.0.0.

  License requirements: nx_sheet_metal (“NX Sheet Metal”)

  `-------------------------------------`

  Setter Method

  Signature `Section`

  Parameters: | section (`NXOpen.Section`) –

  New in version NX4.0.0.

  License requirements: nx_sheet_metal (“NX Sheet Metal”)

## SectionSide

`DimpleBuilder.``SectionSide`

  Returns or sets the section Side for the Dimple section.

  This is used to specify which side of the section should remain stationary during the Dimple operation. Dimple’s section is a set of connected curves. The material exists on both sides of the section curves. section Side specifies - the material on which side of the curve must be punched.The other side shall be bent to the specified angle with respect to this fixed side. This is how you calculate Left/Right. Get the Section Normal (N)Get the Tangent of the section.(T) Result = CrossProduct(N, T). The resultant vector is called RIGHT. This vector shall be in the direction of one if the two sides of the material.If you want the material on the side of Result to be punched, then you have to pass the value of `NXOpen.Features.SheetMetal.DimpleBuilderSectionSideOptions.Right` If you want the other side to be punched, then you have to send `NXOpen.Features.SheetMetal.DimpleBuilderSectionSideOptions.Left`.

  `-------------------------------------`

  Getter Method

  Signature `SectionSide`

  Returns: |
  Return type: | `NXOpen.Features.SheetMetal.DimpleBuilderSectionSideOptions`

  New in version NX4.0.0.

  License requirements: nx_sheet_metal (“NX Sheet Metal”)

  `-------------------------------------`

  Setter Method

  Signature `SectionSide`

  Parameters: | sectionSide (`NXOpen.Features.SheetMetal.DimpleBuilderSectionSideOptions`) –

  New in version NX4.0.0.

  License requirements: nx_sheet_metal (“NX Sheet Metal”)

## SidewallType

`DimpleBuilder.``SidewallType`

  Returns or sets the side where the material must be added to the dimple.

  Done with Respect to the section

  If `NXOpen.Features.SheetMetal.DimpleBuilderSidewallTypeOptions.Inside` is specified, the material of the dimple sidewalls will be added to the interior of the section. If `NXOpen.Features.SheetMetal.DimpleBuilderSidewallTypeOptions.Outside` is specified,the material will be added from the lifted section such that the volume of the dimple cavity is increased.

  `-------------------------------------`

  Getter Method

  Signature `SidewallType`

  Returns: |
  Return type: | `NXOpen.Features.SheetMetal.DimpleBuilderSidewallTypeOptions`

  New in version NX4.0.0.

  License requirements: nx_sheet_metal (“NX Sheet Metal”)

  `-------------------------------------`

  Setter Method

  Signature `SidewallType`

  Parameters: | sidewallType (`NXOpen.Features.SheetMetal.DimpleBuilderSidewallTypeOptions`) –

  New in version NX4.0.0.

  License requirements: nx_sheet_metal (“NX Sheet Metal”)

## Sketch

`DimpleBuilder.``Sketch`

  Returns or sets the Slave Sketch used by the Dimple, If one exists.

  If the Sketch is created internally as part of the Dimple command in the UI, then it shall be consumed by the Dimple and shall not show up as a separate feature in the Part Navigator. If such a behaviour is desired, then specify the Sketch here.

  `-------------------------------------`

  Getter Method

  Signature `Sketch`

  Returns: |
  Return type: | `NXOpen.Features.SketchFeature`

  New in version NX4.0.0.

  License requirements: nx_sheet_metal (“NX Sheet Metal”)

  `-------------------------------------`

  Setter Method

  Signature `Sketch`

  Parameters: | sketch (`NXOpen.Features.SketchFeature`) –

  New in version NX4.0.0.

  License requirements: nx_sheet_metal (“NX Sheet Metal”)

# Method Detail

## GetDepth

`DimpleBuilder.``GetDepth`

  Depth of the Dimple

  Signature `GetDepth()`

  Returns: |
  Return type: | `NXOpen.Expression`

  New in version NX4.0.0.

  License requirements: nx_sheet_metal (“NX Sheet Metal”)

## GetDieRadius

`DimpleBuilder.``GetDieRadius`

  Radius value of the sharp edges of the bottom face

  Signature `GetDieRadius()`

  Returns: |
  Return type: | `NXOpen.Expression`

  New in version NX4.0.0.

  License requirements: nx_sheet_metal (“NX Sheet Metal”)

## GetFilletRadius

`DimpleBuilder.``GetFilletRadius`

  Fillet Radius to be applied for rounding the Sharp section Corners

  Signature `GetFilletRadius()`

  Returns: |
  Return type: | `NXOpen.Expression`

  New in version NX4.0.0.

  License requirements: nx_sheet_metal (“NX Sheet Metal”)

## GetPunchRadius

`DimpleBuilder.``GetPunchRadius`

  Radius value of the sharp edges on the top face

  Signature `GetPunchRadius()`

  Returns: |
  Return type: | `NXOpen.Expression`

  New in version NX4.0.0.

  License requirements: nx_sheet_metal (“NX Sheet Metal”)

## GetTaperAngle

`DimpleBuilder.``GetTaperAngle`

  Taper Angle of the Dimple.

  In case of a tapered dimple, the taper angle is applied on the side faces of the above-protruded section. The affects of taper angle will always increases the cavity volume of the dimple.

  Signature `GetTaperAngle()`

  Returns: |
  Return type: | `NXOpen.Expression`

  New in version NX4.0.0.

  License requirements: nx_sheet_metal (“NX Sheet Metal”)

## SetDepth

`DimpleBuilder.``SetDepth`

  Signature `SetDepth(extent)`

  Parameters: | extent (str) –

  New in version NX4.0.0.

  Deprecated since version NX10.0.0: Use `NXOpen.Expression.RightHandSide()` on the `NXOpen.Expression` object returned from `NXOpen.Features.SheetMetal.DimpleBuilder.GetDepth()` instead.

  License requirements: nx_sheet_metal (“NX Sheet Metal”)

## SetDieRadius

`DimpleBuilder.``SetDieRadius`

  Signature `SetDieRadius(dieRadius)`

  Parameters: | dieRadius (str) –

  New in version NX4.0.0.

  Deprecated since version NX10.0.0: Use `NXOpen.Expression.RightHandSide()` on the `NXOpen.Expression` object returned from `NXOpen.Features.SheetMetal.DimpleBuilder.GetDieRadius()` instead.

  License requirements: nx_sheet_metal (“NX Sheet Metal”)

## SetFilletRadius

`DimpleBuilder.``SetFilletRadius`

  Signature `SetFilletRadius(filletRadius)`

  Parameters: | filletRadius (str) –

  New in version NX4.0.0.

  Deprecated since version NX10.0.0: Use `NXOpen.Expression.RightHandSide()` on the `NXOpen.Expression` object returned from `NXOpen.Features.SheetMetal.DimpleBuilder.GetFilletRadius()` instead.

  License requirements: nx_sheet_metal (“NX Sheet Metal”)

## SetPunchRadius

`DimpleBuilder.``SetPunchRadius`

  Signature `SetPunchRadius(punchRadius)`

  Parameters: | punchRadius (str) –

  New in version NX4.0.0.

  Deprecated since version NX10.0.0: Use `NXOpen.Expression.RightHandSide()` on the `NXOpen.Expression` object returned from `NXOpen.Features.SheetMetal.DimpleBuilder.GetPunchRadius()` instead.

  License requirements: nx_sheet_metal (“NX Sheet Metal”)

## SetTaperAngle

`DimpleBuilder.``SetTaperAngle`

  Signature `SetTaperAngle(taperAngle)`

  Parameters: | taperAngle (str) –

  New in version NX4.0.0.

  Deprecated since version NX10.0.0: Use `NXOpen.Expression.RightHandSide()` on the `NXOpen.Expression` object returned from `NXOpen.Features.SheetMetal.DimpleBuilder.GetTaperAngle()` instead.

  License requirements: nx_sheet_metal (“NX Sheet Metal”)

## Validate

`DimpleBuilder.``Validate`

  Validate whether the inputs to the component are sufficient for commit to be called.

  If the component is not in a state to commit then an exception is thrown. For example, if the component requires you to set some property, this method will throw an exception if you haven’t set it. This method throws a not-yet-implemented NXException for some components.

  Signature `Validate()`

  Returns: | Was self validation successful
  Return type: | bool

  New in version NX3.0.1.

  License requirements: None.

## ValidateBuilderData

`DimpleBuilder.``ValidateBuilderData`

  Verify whether the builder data is valid for creating a dimple or not.

  If the Builder data is valid, returned value shall be 0

  Signature `ValidateBuilderData()`

  Returns: | Data Validity Flag.
  Return type: | int

  New in version NX4.0.0.

  License requirements: nx_sheet_metal (“NX Sheet Metal”)