Issue
How can I split a part using the API? Is there any difference from part context and assembly context?
Solution
Before Inventor 2010, you can call the SplitFeatures.SplitPart method to split a part. This method takes two parameters and returns the newly created SplitFeature. Input Object SplitTool that specifies the entity that will be used to define the split. The input can be a WorkPlane, WorkSurface, or 2D Path. A Path object is obtained using the CreatePath method of the SplitFeatures object. Optional input Boolean value RemovePositiveSide that indicates which portion of the split part is to be removed. The default value is True, which indicates that the positive side will be removed.
From Inventor 2010 , Inventor supports multiple surface bodies. SplitFeatures.SplitPart is hidden. It will split all surface bodies. A new method is provided: SplitFeatures.TrimSolid which can split the specific surface body.
The following code demonstrate how to use the methods, based on the attached sample model.
The first sample passes a WorkSurface as the input to create a SplitFeature:
Sub splitByWorkSurface()
' assume we have had Inventor application
Try
Dim oDoc As PartDocument =
_InvApplication.Documents.Add(
DocumentTypeEnum.kPartDocumentObject,
_InvApplication.FileManager.GetTemplateFile(
DocumentTypeEnum.kPartDocumentObject))
Dim oDef As PartComponentDefinition =
oDoc.ComponentDefinition
Dim oSketch As PlanarSketch =
oDef.Sketches.Add(oDef.WorkPlanes.Item(3))
Dim oTG As TransientGeometry =
_InvApplication.TransientGeometry
oSketch.SketchLines.AddAsTwoPointRectangle(
oTG.CreatePoint2d(0, 0),
oTG.CreatePoint2d(6, 3))
Dim oProfile As Profile =
oSketch.Profiles.AddForSolid()
Dim oBaseExtrude As ExtrudeFeature =
oDef.Features.ExtrudeFeatures.
AddByDistanceExtent(
oProfile,
4, PartFeatureExtentDirectionEnum.kPositiveExtentDirection,
PartFeatureOperationEnum.kJoinOperation)
oSketch =
oDef.Sketches.Add(oDef.WorkPlanes.Item(3))
Dim oLine As SketchLine =
oSketch.SketchLines.AddByTwoPoints
(oTG.CreatePoint2d(2, -1),
oTG.CreatePoint2d(3, 2))
oLine =
oSketch.SketchLines.AddByTwoPoints
(oLine.EndSketchPoint,
oTG.CreatePoint2d(2, 4))
oProfile =
oSketch.Profiles.AddForSurface()
Dim oCutExtrude As ExtrudeFeature =
oDef.Features.ExtrudeFeatures.
AddByDistanceExtent(
oProfile,
5, PartFeatureExtentDirectionEnum.kPositiveExtentDirection,
PartFeatureOperationEnum.kSurfaceOperation)
Dim oWorkSurface As WorkSurface =
oCutExtrude.SurfaceBody.Parent
Dim oSplit As SplitFeature
'before Inventor 2010
'Set oSplit = oDef.Features.SplitFeatures.SplitPart(oWorkSurface)
'From Inventor 2010
' e.g. split the first body
oDef.Features.SplitFeatures.TrimSolid(
oWorkSurface,
oDef.SurfaceBodies(1),
False)
Catch ex As Exception
MsgBox(ex.ToString())
End Try
End Sub
This second example passes in a 2D Path as the input to create a SplitFeature. Before running this sample, please confirm that the sketch with some SketchSpline exists and there is the part that can be split. You can use the attached part document "partTobeSplit.ipt" for the test.
Sub splitByPath()
Try
Dim oPart As PartDocument =
_InvApplication.ActiveDocument
Dim oDocDef = oPart.ComponentDefinition
' assume there is a sketch named 'sketch2'
Dim oSketch As Sketch =
oDocDef.Sketches.Item("sketch2")
' find a spline in the sketch
Dim oSkSpLine As SketchSpline
If oSketch.Consumed = False Then
Dim findit As Boolean
findit = False
For Each oSkSpLine In oSketch.SketchSplines
If oSkSpLine.Construction = False Then
findit = True
Exit For
End If
Next
If findit Then
Dim oPath As Inventor.Path
oPath =
oDocDef.Features.
CreatePath(oSkSpLine)
'before Inventor 2010
'oPart.ComponentDefinition.
'Features.SplitFeatures.SplitPart oPath, False
'From Inventor 2010
'just split second surface body
oDocDef.Features.SplitFeatures.
TrimSolid(oPath,
oDocDef.SurfaceBodies(2),
False)
End If
End If
Catch ex As Exception
MsgBox(ex.ToString())
End Try
End Sub
In the assembly context there is not much difference, you just need to pass in the NativeObject of the proxy object in the assembly environment to the CreatePath method when retrieving the SpitTool object. Here is an example that demonstrates how to split a part after the user selects a SketchSpline in the assembly document. Moreover, you can change the side of an existing split feature by deleting and re-creating the SplitFeature and passing in the new side parameter as shown by the last several lines.
Private Function getPath(invApp As Inventor.Application,
ByVal oPrtDoc As PartDocument ) _
As Inventor.Path
Dim oSks As SketchSplineProxy
'We assume the user selected the sketch spline
' in the assembly context
oSks =
invApp.ActiveDocument.SelectSet(1)
Dim oPrtFeats As PartFeatures =
oPrtDoc.ComponentDefinition.Features
getPath =
oPrtFeats.SplitFeatures.CreatePath(oSks.NativeObject)
End Function
private Sub SplitPartInAssembly()
' assume we have had Inventor application
Try
Dim oAss As AssemblyDocument =
_InvApplication.ActiveDocument
'Get the first component to be split
Dim oSelectedOcc As ComponentOccurrence =
oAss.ComponentDefinition.Occurrences(1)
Dim oPrtDoc As PartDocument =
oSelectedOcc.Definition.Document
'Get the 2D path SplitTool
Dim oSelectedTool As Inventor.Path =
getPath(_InvApplication,oPrtDoc)
Dim oPrtFeats As PartFeatures =
oPrtDoc.ComponentDefinition.Features
''**************before Inventor 2010***********
'Create Split Part with negative side
'Dim spFeature As SplitFeature =
'oPrtFeats.SplitFeatures.SplitPart(oSelectedTool, False)
''Change the negative side to positive side
'Dim skObj As Object = spFeature.SplitTool
'spFeature.Delete(True, True, True)
'spFeature =
'oPrtFeats.SplitFeatures.SplitPart(oSelectedTool, True)
'**************
'********from Inventor 2010**********
'Create Split Part with negative side
Dim spFeature As SplitFeature =
oPrtFeats.SplitFeatures.TrimSolid(
oSelectedTool,
oSelectedOcc.Definition.SurfaceBodies(1),
False)
'Change the negative side to positive side
Dim skObj As Object =
spFeature.SplitTool
spFeature.Delete(True, True, True)
spFeature = oPrtFeats.SplitFeatures.TrimSolid(
oSelectedTool,
oSelectedOcc.Definition.SurfaceBodies(1),
True)
'************************************
Catch ex As Exception
MsgBox(ex.ToString())
End Try
End Sub
