UG二次开发源码-链轮齿轮标准件创建VB源码

admin · 发表于 2014-4-25 20:51:15

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UG二次开发源码-链轮齿轮标准件创建VB源码
感觉还不错，VB写的分享下，只是这里没有使用渐开线的方式画齿轮！

[code] Private Function CreateChainGear(ByVal ChainType As String, ByVal Z As Integer) As Integer
      Dim errorCode As Integer = 0
      Dim p, dr, d, r1, r2, r3, da, d_cut As Double
      Dim alf, Beta, Gama As Double
      Dim M, T, V, W As Double
      Dim DtoR As Double = PI / 180
      Try
         Select Case ChainType
            Case "06B"
                  p = 9.525
                  dr = 6.35
            Case "08A"
                  p = 12.7
                  dr = 7.95
            Case "08B"
                  p = 12.7
                  dr = 8.51
            Case "10A"
                  p = 15.875
                  dr = 10.16
         End Select

         alf = (55 - 60 / Z) * DtoR
         Beta = (18 - 56 / Z) * DtoR
         Gama = (17 - 64 / Z) * DtoR
         r1 = 0.5025 * dr + 0.05
         r2 = 1.3025 * dr + 0.05
         r3 = dr * (1.3 * Cos(Gama) + 0.8 * Cos(Beta) - 1.3025) - 0.05
         M = 0.8 * dr * Sin(alf)
         T = 0.8 * dr * Cos(alf)
         W = 1.3 * dr * Cos(180 / Z * DtoR)
         V = 1.3 * dr * Sin(180 / Z * DtoR)
         d = p / Sin(180 / Z * DtoR)
         da = p * (0.54 + 1 / Tan(180 / Z * DtoR))
         d_cut = p * (1 + 1 / Tan(180 / Z * DtoR))

         Dim Point_O, Point_O2, Point_O3, Point_A, Point_B, Point_C, Point_D, Point_E, Point_cut As Point3d
         Dim Y_o As Double = d / 2

         Point_O = New Point3d(0, Y_o, 0)
         Point_O2 = New Point3d(-M, Y_o + T, 0)
         Dim point_O2_neg As Point3d = New Point3d(M, Y_o + T, 0)

         Point_O3 = New Point3d(W, Y_o - V, 0)
         Dim point_O3_neg As Point3d = New Point3d(-W, Y_o - V, 0)

         Point_A = New Point3d(r1 * Sin(alf), Y_o - r1 * Cos(alf), 0)
         Dim Point_A_neg As Point3d = New Point3d(-r1 * Sin(alf), Y_o - r1 * Cos(alf), 0)

         Point_B = New Point3d(-M + r2 * Sin(alf + Beta), Y_o + T - r2 * Cos(alf + Beta), 0)
         Dim Point_B_neg As Point3d = New Point3d(M - r2 * Sin(alf + Beta), Y_o + T - r2 * Cos(alf + Beta), 0)

         Point_C = New Point3d(W - r3 * Sin(alf + Beta), Y_o - V + r3 * Cos(alf + Beta), 0)
         Dim Point_C_neg As Point3d = New Point3d(-W + r3 * Sin(alf + Beta), Y_o - V + r3 * Cos(alf + Beta), 0)

         Dim X_d As Double = W - r3 * Cos(90 * DtoR - alf - Beta + Gama)
         Dim Y_d As Double = Y_o - V + r3 * Sin(90 * DtoR - alf - Beta + Gama)
         Point_D = New Point3d(X_d, Y_d, 0)
         Dim Point_D_neg As Point3d = New Point3d(-X_d, Y_d, 0)

         Dim Ld As Double = Y_d - X_d / Tan(180 / Z * DtoR)
         Dim Le As Double = Ld * Cos(180 / Z * DtoR)

         Point_E = New Point3d(X_d + Le * Sin(180 / Z * DtoR), Y_d - Ld + Le * Cos(180 / Z * DtoR), 0)
         Dim Point_E_neg As Point3d = New Point3d(-X_d - Le * Sin(180 / Z * DtoR), Y_d - Ld + Le * Cos(180 / Z * DtoR), 0)

         Point_cut = New Point3d(d_cut / 2 * Sin(180 / Z * DtoR), d_cut / 2 * Cos(180 / Z * DtoR), 0)
         Dim Point_cut_neg As Point3d = New Point3d(-d_cut / 2 * Sin(180 / Z * DtoR), d_cut / 2 * Cos(180 / Z * DtoR), 0)

         theSession.Preferences.SkeTCh.CreateInferredConstraints = False
         theSession.Preferences.Sketch.ContinuousAutoDimensioning = False
         Dim workPart As Part = theSession.Parts.Work
         Dim nullSketch As Sketch = Nothing
         Dim sketchInPlaceBuilder1 As SketchInPlaceBuilder
         sketchInPlaceBuilder1 = workPart.Sketches.CreateNewSketchInPlaceBuilder(nullSketch)
         Dim Cut_sketch As Sketch
         Cut_sketch = sketchInPlaceBuilder1.Commit()
         Cut_sketch.SetName("Sketch_ChainGear")
         Cut_sketch.Activate(Sketch.ViewReorient.False)

         Dim NXMatrix1 As NXMatrix
         nXMatrix1 = theSession.ActiveSketch.Orientation
         Dim arc As Arc
         arc = workPart.Curves.CreateArc(Point_O, nXMatrix1, r1, -90 * DtoR - alf, -90 * DtoR + alf)
         theSession.ActiveSketch.AddGeometry(arc, Sketch.InferConstraintsOption.InferNoConstraints)

         arc = workPart.Curves.CreateArc(Point_O2, nXMatrix1, r2, -90 * DtoR + alf, -90 * DtoR + alf + Beta)
         theSession.ActiveSketch.AddGeometry(arc, Sketch.InferConstraintsOption.InferNoConstraints)

         arc = workPart.Curves.CreateArc(point_O2_neg, nXMatrix1, r2, -90 * DtoR - alf - Beta, -90 * DtoR - alf)
         theSession.ActiveSketch.AddGeometry(arc, Sketch.InferConstraintsOption.InferNoConstraints)

         arc = workPart.Curves.CreateArc(Point_O3, nXMatrix1, r3, 90 * DtoR + alf + Beta - Gama, 90 * DtoR + alf + Beta)
         theSession.ActiveSketch.AddGeometry(arc, Sketch.InferConstraintsOption.InferNoConstraints)

         arc = workPart.Curves.CreateArc(point_O3_neg, nXMatrix1, r3, 90 * DtoR - alf - Beta, 90 * DtoR - alf - Beta + Gama)
         theSession.ActiveSketch.AddGeometry(arc, Sketch.InferConstraintsOption.InferNoConstraints)

         Dim line1 As Line

         line1 = workPart.Curves.CreateLine(Point_B, Point_C)
         theSession.ActiveSketch.AddGeometry(line1, Sketch.InferConstraintsOption.InferNoConstraints)
         line1 = workPart.Curves.CreateLine(Point_B_neg, Point_C_neg)
         theSession.ActiveSketch.AddGeometry(line1, Sketch.InferConstraintsOption.InferNoConstraints)

         line1 = workPart.Curves.CreateLine(Point_D, Point_E)
         theSession.ActiveSketch.AddGeometry(line1, Sketch.InferConstraintsOption.InferNoConstraints)
         line1 = workPart.Curves.CreateLine(Point_D_neg, Point_E_neg)
         theSession.ActiveSketch.AddGeometry(line1, Sketch.InferConstraintsOption.InferNoConstraints)

         line1 = workPart.Curves.CreateLine(Point_E, Point_cut)
         theSession.ActiveSketch.AddGeometry(line1, Sketch.InferConstraintsOption.InferNoConstraints)
         line1 = workPart.Curves.CreateLine(Point_E_neg, Point_cut_neg)
         theSession.ActiveSketch.AddGeometry(line1, Sketch.InferConstraintsOption.InferNoConstraints)

         Dim Point_center As Point3d = New Point3d(0, 0, 0)
         arc = workPart.Curves.CreateArc(Point_center, nXMatrix1, d_cut / 2, (90 - 180 / Z) * DtoR, (90 + 180 / Z) * DtoR)
         theSession.ActiveSketch.AddGeometry(arc, Sketch.InferConstraintsOption.InferNoConstraints)

         theSession.ActiveSketch.Update()
         theSession.ActiveSketch.Deactivate(Sketch.ViewReorient.False, Sketch.UpdateLevel.Model)

         sketchInPlaceBuilder1 = workPart.Sketches.CreateNewSketchInPlaceBuilder(nullSketch)
         Dim Circle_sketch As Sketch
         Circle_sketch = sketchInPlaceBuilder1.Commit()
         Circle_sketch.SetName("Sketch_Circle")
         Circle_sketch.Activate(Sketch.ViewReorient.False)
         arc = workPart.Curves.CreateArc(Point_center, nXMatrix1, da / 2, 0, 360 * DtoR)
         theSession.ActiveSketch.AddGeometry(arc, Sketch.InferConstraintsOption.InferNoConstraints)
         theSession.ActiveSketch.Update()
         theSession.ActiveSketch.Deactivate(Sketch.ViewReorient.False, Sketch.UpdateLevel.Model)

         sketchInPlaceBuilder1.Destroy()

         Dim nullFeatures_Feature As Features.Feature = Nothing
         Dim nullNXObject As NXObject = Nothing
         Dim nullPoint As Point = Nothing

         Dim extrudeBuilder1 As Features.ExtrudeBuilder
         extrudeBuilder1 = workPart.Features.CreateExtrudeBuilder(nullFeatures_Feature)
         extrudeBuilder1.Limits.StartExtend.Value.RightHandSide = "0"
         extrudeBuilder1.Limits.EndExtend.Value.RightHandSide = "5"

         Dim targetBodies1(0) As Body
         Dim nullBody As Body = Nothing
         targetBodies1(0) = nullBody
         extrudeBuilder1.BooleanOperation.SetTargetBodies(targetBodies1)
         extrudeBuilder1.BooleanOperation.Type = GeometricUtilities.BooleanOperation.BooleanType.Create

         Dim section2 As Section
         section2 = workPart.Sections.CreateSection(0.02413, 0.0254, 0.5)
         extrudeBuilder1.Section = section2
         Dim features2(0) As Features.Feature
         Dim sketchFeature2 As Features.SketchFeature = Circle_sketch.Feature
         features2(0) = sketchFeature2
         Dim curveFeatureRule2 As CurveFeatureRule
         curveFeatureRule2 = workPart.ScRuleFactory.CreateRuleCurveFeature(features2)
         Dim rules2(0) As SelectionIntentRule
         rules2(0) = curveFeatureRule2
         Dim sketch2 As Sketch = Circle_sketch
         Dim helpPoint2 As Point3d = New Point3d(0, 0, 0)
         section2.AddToSection(rules2, Circle_sketch.GetAllGeometry(0), nullNXObject, nullNXObject, helpPoint2, Section.Mode.Create, False)

         Dim direction2 As Direction
         direction2 = workPart.Directions.CreateDirection(sketch2, Sense.Forward, SmartObject.UpdateOption.WithinModeling)
         extrudeBuilder1.Direction = direction2

         Dim ExtrudeFeature As Features.Feature
         ExtrudeFeature = extrudeBuilder1.CommitFeature()
         ExtrudeFeature.SetName("Circle")

         extrudeBuilder1.Destroy()

         extrudeBuilder1 = workPart.Features.CreateExtrudeBuilder(nullFeatures_Feature)
         extrudeBuilder1.Limits.StartExtend.Value.RightHandSide = "0"
         extrudeBuilder1.Limits.EndExtend.Value.RightHandSide = "5"

         Dim CircleBody As Features.BodyFeature = ExtrudeFeature
         Dim body1() As Body = CircleBody.GetBodies()

         targetBodies1(0) = body1(0)
         extrudeBuilder1.BooleanOperation.SetTargetBodies(targetBodies1)
         extrudeBuilder1.BooleanOperation.Type = GeometricUtilities.BooleanOperation.BooleanType.Create

         section2 = workPart.Sections.CreateSection(0.02413, 0.0254, 0.5)
         extrudeBuilder1.Section = section2
         sketchFeature2 = Cut_sketch.Feature
         features2(0) = sketchFeature2
         curveFeatureRule2 = workPart.ScRuleFactory.CreateRuleCurveFeature(features2)
         rules2(0) = curveFeatureRule2
         sketch2 = Cut_sketch
         section2.AddToSection(rules2, Circle_sketch.GetAllGeometry(0), nullNXObject, nullNXObject, helpPoint2, Section.Mode.Create, False)

         direction2 = workPart.Directions.CreateDirection(sketch2, Sense.Forward, SmartObject.UpdateOption.WithinModeling)
         extrudeBuilder1.Direction = direction2

         Dim CutFeature As Features.Feature
         CutFeature = extrudeBuilder1.CommitFeature()
         CutFeature.SetName("Cut")

         extrudeBuilder1.Destroy()

         Dim geomcopyBuilder1 As Features.GeomcopyBuilder
         geomcopyBuilder1 = workPart.Features.CreateGeomcopyBuilder(nullFeatures_Feature)
         geomcopyBuilder1.Type = Features.GeomcopyBuilder.TransformTypes.Rotation

         geomcopyBuilder1.RotateDistance.RightHandSide = 0
         geomcopyBuilder1.RotateAngle.RightHandSide = 360 / Z
         geomcopyBuilder1.NumberOfCopies.RightHandSide = Z
         Dim datumAxis1 As DatumAxis = CType(workPart.Datums.FindObject("DATUM_CSYS(0) Z axis"), DatumAxis)

         Dim direction1 As Direction
         direction1 = workPart.Directions.CreateDirection(datumAxis1, Sense.Forward, SmartObject.UpdateOption.WithinModeling)
         Dim axis1 As Axis
         axis1 = workPart.Axes.CreateAxis(nullPoint, direction1, SmartObject.UpdateOption.WithinModeling)

         geomcopyBuilder1.RotationAxis = axis1

         Dim CutBody As Features.BodyFeature = CutFeature
         body1 = CutBody.GetBodies()

         Dim added1 As Boolean
         added1 = geomcopyBuilder1.GeometryToInstance.Add(body1(0))
         Dim GeomCopyFeature As Features.Feature
         GeomCopyFeature = geomcopyBuilder1.CommitFeature()

         Dim nullFeatures_BooleanFeature As Features.BooleanFeature = Nothing

         Dim booleanBuilder1 As Features.BooleanBuilder
         booleanBuilder1 = workPart.Features.CreateBooleanBuilderUsingCollector(nullFeatures_BooleanFeature)

         booleanBuilder1.Operation = Features.Feature.BooleanType.Subtract
         body1 = CircleBody.GetBodies()

         Dim added2 As Boolean
         added2 = booleanBuilder1.Targets.Add(body1(0))

         Dim features1(0) As Features.Feature
         Dim geomcopy1 As Features.Geomcopy = GeomCopyFeature

         features1(0) = geomcopy1
         Dim bodyFeatureRule1 As BodyFeatureRule
         bodyFeatureRule1 = workPart.ScRuleFactory.CreateRuleBodyFeature(features1)

         Dim rules4(0) As SelectionIntentRule
         rules4(0) = bodyFeatureRule1
         Dim scCollector2 As ScCollector
         scCollector2 = workPart.ScCollectors.CreateCollector()
         scCollector2.ReplaceRules(rules4, False)

         booleanBuilder1.ToolBodyCollector = scCollector2
         Dim nXObject1 As NXObject
         nXObject1 = booleanBuilder1.Commit()

         booleanBuilder1.Destroy()

         Dim objects2(0) As DisplayableObject
         objects2(0) = CutBody.GetBodies(0)
         theSession.DisplayManager.BlankObjects(objects2)
      Catch ex As Exception
         errorCode = 1
         theUI.NXMessageBox.Show("Block Styler", NXMessageBox.DialogType.Error, ex.ToString)

      End Try
      CreateChainGear = errorCode
End Function

End Class[/code]

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[二次开发源码] UG二次开发源码-链轮齿轮标准件创建VB源码

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