Macro Breakdown
UserForm
This macro starts by opening a Userform. In this form the user has the ability to choose the diameter of one strand in the braid and the total length of the braid, although in this version of the macro the total length of the braid cannot be changed all it does is create one link of the braid.
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| Braid Macro UserForm |
Create Planes
Next the macro inserts 3 3D sketches and draws a spline in each of the sketches. The points of the sketches are determined by multiple of the inputted diameter measurements. Below is an example of the spline creation:
Public Sub Create_Spline_1(Diameter As Double)
Set swApp = Application.SldWorks
Set Part = swApp.ActiveDoc
Part.SketchManager.Insert3DSketch True
' Create Spline
Dim pointArray As Variant
Dim points() As Double
ReDim points(0 To 17) As Double
points(0) = -1 * Diameter
points(1) = -1 * (Diameter / 1.5)
points(2) = 0
points(3) = -1 * Diameter
points(4) = -1 * (Diameter / 1.5)
points(5) = Diameter / 8
points(6) = -1 * (Diameter)
points(7) = Diameter / 1.5
points(8) = Diameter * 2
points(9) = 0
points(10) = 0
points(11) = (Diameter * 4)
points(12) = Diameter
points(13) = (Diameter / -1.5)
points(14) = (Diameter * 6) - (Diameter / 8)
points(15) = Diameter
points(16) = Diameter / -1.5
points(17) = Diameter * 6
pointArray = points
Dim skSegment As Object
Set skSegment = Part.SketchManager.CreateSpline((pointArray))
Part.SketchManager.Insert3DSketch True
Part.ClearSelection2 True
End Sub
Circle Sketches
In order to create a swept braid strand later it needs a sketch to sweep a long the spline. The macro then creates 3 sketches on the front plane with their center points intersecting with end points of the splines and the diameter set to the value taken in the UserForm. Below is an example of the code:
Public Sub Draw_Circles(Diameter As Double)
Set swApp = Application.SldWorks
Set Part = swApp.ActiveDoc
' Cirlce 1
Part.SketchManager.InsertSketch True
boolstatus = Part.Extension.SelectByID2("Plane1", "PLANE", -5.10703921288805E-03, -2.59649850538866E-03, -4.90350149461128E-03, False, 0, Nothing, 0)
Part.ClearSelection2 True
Dim skSegment As Object
Set skSegment = Part.SketchManager.CreateCircle(-1 * Diameter, -1 * (Diameter / 1.5), 0#, -1 * Diameter, (Diameter / -1.5) - (Diameter / 2), 0#)
Part.ClearSelection2 True
Part.SketchManager.InsertSketch True
Part.ClearSelection2 True
' Circle 2
Part.SketchManager.InsertSketch True
boolstatus = Part.Extension.SelectByID2("Plane1", "PLANE", -5.10703921288805E-03, -2.59649850538866E-03, -4.90350149461128E-03, False, 0, Nothing, 0)
Part.ClearSelection2 True
Set skSegment = Part.SketchManager.CreateCircle(0#, 0#, 0#, 0#, Diameter / 2, 0#)
Part.ClearSelection2 True
Part.SketchManager.InsertSketch True
Part.ClearSelection2 True
' Circle 3
Part.SketchManager.InsertSketch True
boolstatus = Part.Extension.SelectByID2("Plane1", "PLANE", -5.10703921288805E-03, -2.59649850538866E-03, -4.90350149461128E-03, False, 0, Nothing, 0)
Part.ClearSelection2 True
Set skSegment = Part.SketchManager.CreateCircle(Diameter, Diameter / 1.5, 0#, Diameter, (Diameter / 1.5) + (Diameter / 2), 0#)
Part.ClearSelection2 True
Part.SketchManager.InsertSketch True
Part.ClearSelection2 True
End Sub
Swept Boss\ Base
The final step is to create the strands. the macro selects 1 spline and 1 circle and preforms a swept boss. This process is repeated 3 times to make all the strands. Below is an example of the code:
boolstatus = Part.Extension.SelectByID2("Sketch1", "SKETCH", 7.11112277789861E-03, 1.27021790098527E-03, 0, False, 1, Nothing, 0)
boolstatus = Part.Extension.SelectByID2("3DSketch1", "SKETCH", 6.81458693163701E-03, 4.54305795442467E-03, 4.79044795270839E-03, True, 4, Nothing, 0)
Dim swFeat As Object
Dim swFeatMgr As Object
Set swFeatMgr = Part.FeatureManager
Dim swFeatData As Object
Set swFeatData = swFeatMgr.CreateDefinition(swFeatureNameID_e.swFmSweep)
swFeatData.AdvancedSmoothing = False
swFeatData.AlignWithEndFaces = 0
swFeatData.AutoSelect = True
swFeatData.D1ReverseTwistDir = False
swFeatData.Direction = -1
swFeatData.EndTangencyType = 0
swFeatData.FeatureScope = True
swFeatData.MaintainTangency = False
swFeatData.Merge = True
swFeatData.MergeSmoothFaces = True
swFeatData.PathAlignmentType = 10
swFeatData.StartTangencyType = 0
swFeatData.ThinFeature = False
swFeatData.ThinWallType = 0
swFeatData.TwistControlType = 0
swFeatData.SetTwistAngle 0
swFeatData.SetWallThickness True, 0
Set swFeat = swFeatMgr.CreateFeature(swFeatData)
Part.ClearSelection2 True
Future Plans
- Add the ability to chose the length of the braid.
- Create the braid with a taper
- Braid in a circle
- Transpose the braid onto different surfaces
- Create the a braided tube
Macro File
