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Create Loft Body Example (VBA)

This example shows how to create a loft body using IModeler::CreateLoftBody2.

' ******************************************************************************

' Preconditions:

'       (1) Part document is open.

'       (2) Two closed sketches representing the profiles for the loft body exist.

'       (3) One curve representing a guide curve for the loft body exists.

'

' Postconditions: Loft body is created and displayed.

' ******************************************************************************

Option Explicit

 

Dim swApp As SldWorks.SldWorks

Dim swModel As SldWorks.ModelDoc2

Dim swModelDocExt As SldWorks.ModelDocExtension

Dim swFeatMgr As SldWorks.FeatureManager

Dim count As Long

Dim featArr As Variant

Dim feat1 As SldWorks.Feature

Dim feat2 As SldWorks.Feature

Dim feat3 As SldWorks.Feature

Dim swSelMgr As SldWorks.SelectionMgr

Dim swModeler As SldWorks.Modeler

Dim boolstatus As Boolean

Dim profileIn As Variant

Dim guideCurve As Variant

Dim pProfile(1) As SldWorks.Feature

Dim pGuide(0) As SldWorks.Feature

Dim bValue As Boolean

Dim swBody As SldWorks.Body2

Dim bIsTempBody As Boolean

 

Sub main()

 

Set swApp = Application.SldWorks

Set swModeler = swApp.GetModeler

Set swModel = swApp.ActiveDoc

Set swModelDocExt = swModel.Extension

 

' Select the sketches for the profiles

' for the loft body and make them

' elements of an array to use to

' create the loft body

Set swFeatMgr = swModel.FeatureManager

count = swFeatMgr.GetFeatureCount(False)

featArr = swFeatMgr.GetFeatures(False)

Set swSelMgr = swModel.SelectionManager

boolstatus = swModelDocExt.SelectByID2("Sketch1", "SKETCH", 0.01432052560262, 0.03232526173853, 0, False, 0, Nothing, 0)

Set feat1 = swSelMgr.GetSelectedObject6(1, -1)

Debug.Print "First profile's feature name:       " & feat1.Name

Set pProfile(0) = feat1

boolstatus = swModelDocExt.SelectByID2("Sketch2", "SKETCH", 0, 0, 0, False, 0, Nothing, 0)

Set feat2 = swSelMgr.GetSelectedObject6(1, -1)

Debug.Print "Second profile's feature name:      " & feat2.Name

Set pProfile(1) = feat2

profileIn = pProfile

 

' Select a guide curve for the loft body

' and make it an element of an array

' to use to create the loft body

boolstatus = swModelDocExt.SelectByID2("Curve1", "REFERENCECURVES", 0.1353192072154, 0.1043159291966, 0.09477145953832, False, 0, Nothing, 0)

Set feat3 = swSelMgr.GetSelectedObject6(1, -1)

Debug.Print "Guide curve's feature name:         " & feat3.Name

Set pGuide(0) = feat3

Set guideCurve = feat3

 

' Create the loft body

Set swBody = swModeler.CreateLoftBody2(swModel, profileIn, guideCurve, Nothing, False, 0, 0, 0, True, False, True, False, True, 1, 1, 1, True, True, 1, 1, False)

 

' Test whether the loft body is a temporary body

bIsTempBody = swBody.IsTemporaryBody

Debug.Print "Is the loft body a temporary body?  " & bIsTempBody

 

' Display the loft body

bValue = swBody.Display3(swModel, 256, swTempBodySelectOptionNone)

 

End Sub



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