Sketch using curve generated by intersection of Surface and a face

[Anonymous]

I have a face "f", which can be assumed to be planar.

I have a SurfaceBody, which is a Surface, called "midsurface"

I wish to create a Sketch containing curve generated by intersection of "f" and "midsurface", placed at "f". (Pic attached)

Following is my attempt, which fails at various places. Sketch is not created. Then I am not able to find type of Intersection curve, so as to cast it and then add it to Sketch.

Public Sub fillMidcurvesData(ByRef nd As Node, ByRef transGeom As TransientGeometry, ByRef oCompDef As PartComponentDefinition)
'Find Interface Face's plane
Dim pt1 As Point = f.Vertices(1).Point()
Dim pt2 As Point = f.Vertices(2).Point()
Dim pt3 As Point = f.Vertices(3).Point()
Dim plane As Plane = transGeom.CreatePlaneByThreePoints(pt1, pt2, pt3)

Dim otherNode As Node = getOtherNode(nd)
Dim otherMidsurface = otherNode.midsuface
If Not otherMidsurface Is Nothing Then
Dim out1 As ObjectsEnumerator = transGeom.SurfaceSurfaceIntersection(plane, otherMidsurface.Faces.Item(1).Geometry(), 0.01) ' plane.IntersectWithSurface(otherMidsurface.Faces(1).Geometry())
If out1.Count > 0 Then
Dim workplane As WorkPlane = oCompDef.WorkPlanes.AddByPlaneAndOffset(plane, 0.0)

Dim sketch As PlanarSketch = oCompDef.Sketches.Add(workplane, False)
Dim line As Line = out1.Item(1)
midcurveProfile = sketch.Profiles.Item(1)
End If
End If
End Sub

[Vladimir.Ananyev]

You may consider oSketch3d.IntersectionCurves.Add method that is the most powerful if you need to get the intersection of two surfaces.

The following sample creates 3d intersection curve that could be a) used as is or b) projected to the planar sketch created on the top face.

Sub SketchWithIntersectionCurve()

    Dim oDoc As PartDocument
    Set oDoc = ThisApplication.ActiveDocument
    Dim oDef As PartComponentDefinition
    Set oDef = oDoc.ComponentDefinition
    
    'top face (in this sample - by index)
    Dim oFace As Face
    Set oFace = oDef.SurfaceBodies.Item(1).Faces.Item(4)
    'cutting surface
    Dim oSurf As WorkSurface
    Set oSurf = oDef.WorkSurfaces.Item(1)
    
    '3d intersection curve with the top face
    Dim oSketch3d As Sketch3D
    Set oSketch3d = oDef.Sketches3D.Add
    Dim oIntersectionCurve  As IntersectionCurve
    Set oIntersectionCurve = oSketch3d.IntersectionCurves _
            .Add(oSurf.SurfaceBodies.Item(1), oFace)
    'it is possible to project all intersection surve
    'segments to the planar sketch
    Dim oSketch2d As PlanarSketch
    Set oSketch2d = oDef.Sketches.Add(oFace, False)
    Dim oEntity3d As SketchEntity3D
    Dim oEntity2d As SketchEntity
    For Each oEntity3d In oIntersectionCurve.SketchEntities
        Set oEntity2d = oSketch2d.AddByProjectingEntity(oEntity3d)
    Next
    Beep
End Sub

 

cheers,

[Vladimir.Ananyev]

I've attached the part model that was used for this demo.

[Anonymous]

I have uploaded my project and a video describing problem at

https://drive.google.com/file/d/0B9ZSXyeZHd37M1FJTi0ydk1MZzA/view?usp=sharing
https://drive.google.com/file/d/0B9ZSXyeZHd37YTNwT25hRUFjX3c/view?usp=sharing

Can you have a look at the function fillMidcurvesData() and let me know if I am doing something wrong?

[Vladimir.Ananyev · Accepted solution]

The first problem with your code – IntersectionCurves.Add() method does not accept Face.Geometry type argument.  This can be one of the following: SurfaceBody, Face, WorkPlane or 2D sketch curve object. Seehelp for further details.

If Not otherMidsurface Is Nothing Then
   Dim oSketch3d As Sketch3D = oCompDef.Sketches3D.Add
   Dim oIntersectionCurve As IntersectionCurve = oSketch3d.IntersectionCurves _
          .Add(otherMidsurface.Faces.Item(1).Geometry(), f.Geometry())

The second potential problem you should check – if both arguments are valid faces for this operation.  (I can’t verify this).

If I interrupt execution of your code just before Sketch3D creation and then run my VBA test with acceptable SurfaceBody objects then I get correct 3d sketch intersection lines.

Sub SketchWithIntersectionCurve_2()

    Dim oDoc As PartDocument
    Set oDoc = ThisApplication.ActiveDocument
    Dim oDef As PartComponentDefinition
    Set oDef = oDoc.ComponentDefinition
    
    'Blue box surface body
    Dim oBlueBoxBody As SurfaceBody
    Set oBlueBoxBody = oDef.SurfaceBodies.Item(1)
    
    '3d intersection curve with the top face
    Dim oSketch3d As Sketch3D
    Set oSketch3d = oDef.Sketches3D.Add

    'vertical cutting surface
    Dim oSurf1 As WorkSurface
    Set oSurf1 = oDef.WorkSurfaces.Item(1)
    'horizontal cutting surface
    Dim oSurf2 As WorkSurface
    Set oSurf2 = oDef.WorkSurfaces.Item(2)

    Dim oIntersectionCurve1  As IntersectionCurve
    Set oIntersectionCurve1 = oSketch3d.IntersectionCurves _
            .Add(oSurf1.SurfaceBodies.Item(1), oBlueBoxBody)
            
    Dim oIntersectionCurve2  As IntersectionCurve
    Set oIntersectionCurve2 = oSketch3d.IntersectionCurves _
            .Add(oSurf2.SurfaceBodies.Item(1), oBlueBoxBody)
    Beep
End Sub

Here are both intersection lines:

cheers,

[Anonymous]

Your post provided me with a good solution. Thank you very much! But I have a question. When I defined "Dim oIntersectionCurve As IntersectionCurve" and used “oSketch3D.IntersectionCurves.Add（）” method, there is a error showing that "user-defined type not defined"? My Inventor edition is "Autodesk Inventor Professional 2012". The following is the code. 

Sub blade()
 Dim oapp As Inventor.Application
 Set oapp = ThisApplication
 
 Dim oDoc As PartDocument
 Set oDoc = oapp.ActiveDocument
 
 Dim oCompDef As ComponentDefinition
 Set oCompDef = oDoc.ComponentDefinition
 
 Dim otg As TransientGeometry
 Set otg = oapp.TransientGeometry
 
 Dim oSketch3D As Sketch3D
 Set oSketch3D = oCompDef.Sketches3D.Add
 
 Dim oFace As Face
 Set oFace = oCompDef.Features.Item(1).SurfaceBodies.Item(1).Faces.Item(3)
 
 Dim oWorkPlane5 As WorkPlane
 Set oWorkPlane5 = oCompDef.WorkPlanes.Item(5)
 oWorkPlane5.Visible = True
 
 Dim oWorkPlane6 As WorkPlane
 Set oWorkPlane6 = oCompDef.WorkPlanes.Item(6)
 oWorkPlane6.Visible = True
 
 Dim Distance As Double
 Distance = 5
 
 Dim InsertWorkPlane As WorkPlane
 Set InsertWorkPlane = oCompDef.WorkPlanes.AddByPlaneAndOffset(oWorkPlane5, Distance)
 
 Dim oIntersectionCurve As IntersectionCurve
 Set oIntersectionCurve = oSketch3D.IntersectionCurves.Add(oCompDef.Features.Item(1).SurfaceBodies.Item(1).Faces.Item(3), _
                                                           oWorkPlane5)

End Sub

 

Thank you very much!!