Hide Table of Contents

Create Solid Bodies using Geometry and Topology APIs Example (VBA)

This example shows how to create a solid body using these geometry and topology APIs:

  • IBody2::Check3

  • IBody2::Operations2

  • IModeler::CreateBodyFromBox

  • IModeler::CreateBodyFromCone

  • IPartDoc::CreateFeatureFromBody3



' Problem:

'       This example shows how to use some of

'       the geometry and topolgy APIs to

'       construct temporary API bodies, perform

'       a boolean addition, and then create a solid

'       body feature from the result.


' Preconditions: None


' Postconditions: A new part is created containing a single solid

'           body feature that is the union of a box and

'           a cone.



Option Explicit

Const SWBODYINTERSECT           As Integer = 15901

Const SWBODYCUT                 As Integer = 15902

Const SWBODYADD                 As Integer = 15903

Public Enum swBodyOperationError_e

    swBodyOperationUnknownError = -1

    swBodyOperationNoError = 0

    swBodyOperationNonApiBody = 1

    swBodyOperationWrongType = 2

    swBodyOperationBooleanFail = 1058

    swBodyOperationNoIntersect = 1067

    swBodyOperationNonManifold = 547

    swBodyOperationPartialCoincidence = 1040

    swBodyOperationIntersectSolidWithSheets = 972

    swBodyOperationUniteSolidSheet = 543

    swBodyOperationMissingGeom = 96

    swBodyOperationSameToolAndTarget = 545

    swBodyOperationFailGeomCondition = 3

    swBodyOperationFailToCutBody = 4

    swBodyOperationDisjointBodies = 5

    swBodyOperationEmptyBody = 6

    swBodyOperationEmptyInputBody = 7

End Enum

Public Enum swCreateFeatureBodyOpts_e

    swCreateFeatureBodyCheck = &H1

    swCreateFeatureBodySimplify = &H2

End Enum

Sub main()

    Dim swApp                           As SldWorks.SldWorks

    Dim swModel                         As SldWorks.ModelDoc2

    Dim swModeler                       As SldWorks.Modeler

    Dim swFeat                          As SldWorks.feature


    Dim nConeParam(8)                   As Double

    Dim vConeArr                        As Variant

    Dim swConeBody                      As SldWorks.body2


    Dim nBoxParam(8)                    As Double

    Dim vBoxArr                         As Variant

    Dim swBoxBody                       As SldWorks.body2


    Dim vNewBodyArr                     As Variant

    Dim vNewBody                        As Variant

    Dim swNewPart                       As SldWorks.PartDoc

    Dim swNewBody                       As SldWorks.body2

    Dim swFaultEnt                      As SldWorks.FaultEntity


    Dim nRetVal                         As Long

    Dim bRet                            As Boolean

    Dim nCount                          As Long


    ' Form cone


    ' Face center

    nConeParam(0) = 0#

    nConeParam(1) = 0.1

    nConeParam(2) = 0#


    ' Axis

    nConeParam(3) = 0#

    nConeParam(4) = 0#

    nConeParam(5) = 1#


    ' Base radius

    nConeParam(6) = 0.2


    ' Top radius

    nConeParam(7) = 0.1


    ' Height

    nConeParam(8) = 0.3


    vConeArr = nConeParam



    ' Form box


    ' Face center

    nBoxParam(0) = 0#

    nBoxParam(1) = 0.1

    nBoxParam(2) = 0.2


    ' Axis

    nBoxParam(3) = 0#

    nBoxParam(4) = 0#

    nBoxParam(5) = 1#


    ' Width

    nBoxParam(6) = 0.3


    ' Length

    nBoxParam(7) = 0.25



    nBoxParam(8) = 0.4

    vBoxArr = nBoxParam



    Set swApp = CreateObject("SldWorks.Application")

    Set swModeler = swApp.GetModeler


    Set swConeBody = swModeler.CreateBodyFromCone((vConeArr))

    Set swBoxBody = swModeler.CreateBodyFromBox((vBoxArr))


    ' Must be valid because parameters were specified

    Debug.Assert Not swConeBody Is Nothing


    Set swFaultEnt = swConeBody.Check3

    nCount = swFaultEnt.Count

    If nCount <> 0 Then

        Debug.Print "Faulty cone!"

        Exit Sub

    End If


    ' Must be valid because parameters were specified

    Debug.Assert Not swBoxBody Is Nothing


    Set swFaultEnt = swBoxBody.Check3

    nCount = swFaultEnt.Count

    If nCount <> 0 Then

        Debug.Print "Faulty box!"

        Exit Sub

    End If



    ' Must work because both bodies were created

    vNewBodyArr = swConeBody.Operations2(SWBODYADD, swBoxBody, nRetVal)

    Debug.Assert swBodyOperationNoError = nRetVal



    Set swNewPart = swApp.NewPart


    For Each vNewBody In vNewBodyArr

        Set swNewBody = vNewBody


        ' Force creation of a solid body feature

        Set swFeat = swNewPart.CreateFeatureFromBody3(swNewBody, False, _

                        swCreateFeatureBodyCheck + swCreateFeatureBodySimplify)


        ' Must be able to create a solid body feature from a solid body

        Debug.Assert Not swFeat Is Nothing


End Sub


Provide feedback on this topic

SOLIDWORKS welcomes your feedback concerning the presentation, accuracy, and thoroughness of the documentation. Use the form below to send your comments and suggestions about this topic directly to our documentation team. The documentation team cannot answer technical support questions. Click here for information about technical support.

* Required

Subject:   Feedback on Help Topics
Page:   Create Solid Bodies using Geometry and Topology APIs Example (VBA)
*   I acknowledge I have read and I hereby accept the privacy policy under which my Personal Data will be used by Dassault Systèmes

Print Topic

Select the scope of content to print:


We have detected you are using a browser version older than Internet Explorer 7. For optimized display, we suggest upgrading your browser to Internet Explorer 7 or newer.

 Never show this message again

Web Help Content Version: API Help (English only) 2012 SP05

To disable Web help from within SOLIDWORKS and use local help instead, click Help > Use SOLIDWORKS Web Help.

To report problems encountered with the Web help interface and search, contact your local support representative. To provide feedback on individual help topics, use the “Feedback on this topic” link on the individual topic page.