Hide Table of Contents

Get Properties of Sketch Pattern Feature Example (VBA)

This example shows how to get the properties of a sketch pattern feature.

'----------------------------------------------------------------
' Preconditions:
' 1. Verify that the specified document exists.
' 2. Open an Immediate window.
'
' Postconditions:
' 1. Creates Boss-Extrude2, Sketch3, and Sketch-Pattern1.
' 2. Inspect the Immediate window.
'
' NOTE: Because the model is used elsewhere, do not save changes.
'----------------------------------------------------------------
Dim swApp                   As SldWorks.SldWorks
Dim Part                    As SldWorks.ModelDoc2
Dim myFeature               As SldWorks.Feature
Dim swSketchPatt            As SldWorks.SketchPatternFeatureData
Dim vBasePt                 As Variant
Dim skPoint                 As Object
Dim vSkLines                As Variant
Dim swSketch                As SldWorks.Sketch
Dim swSketchFeat            As SldWorks.Feature
Dim swPatternTransform      As SldWorks.MathTransform
Dim boolstatus              As Boolean
Dim i                       As Long
Dim longstatus              As Long
Dim longwarnings            As Long

Option Explicit

Sub main()

    Set swApp = Application.SldWorks
    Set Part = swApp.OpenDoc6("C:\Users\Public\Documents\SOLIDWORKS\SOLIDWORKS 2018\samples\tutorial\api\block20.sldprt", 1, 0, "", longstatus, longwarnings)
    swApp.ActivateDoc2 "block20", False, longstatus
   

    boolstatus = Part.Extension.SelectByID2("", "FACE", -4.07921768468213E-02, 3.96239999998329E-02, -4.02814031592129E-02, False, 0, Nothing, 0)
    boolstatus = Part.Extension.SetUserPreferenceToggle(swUserPreferenceToggle_e.swSketchAddConstToRectEntity, swUserPreferenceOption_e.swDetailingNoOptionSpecified, False)
    boolstatus = Part.Extension.SetUserPreferenceToggle(swUserPreferenceToggle_e.swSketchAddConstLineDiagonalType, swUserPreferenceOption_e.swDetailingNoOptionSpecified, True)
    vSkLines = Part.SketchManager.CreateCornerRectangle(-5.18589252521906E-02, 4.51811131877662E-02, 0, -3.57471289475484E-02, 2.86242963995278E-02, 0)
    Part.SketchManager.InsertSketch True
   

    boolstatus = Part.Extension.SelectByID2("Sketch2", "SKETCH", 0, 0, 0, False, 4, Nothing, 0)
    Set myFeature = Part.FeatureManager.FeatureExtrusion2(True, False, False, 0, 0, 0.00254, 0.00254, False, False, False, False, 1.74532925199433E-02, 1.74532925199433E-02, False, False, False, False, True, True, True, 0, 0, False)
   

    Part.SketchManager.InsertSketch True
    boolstatus = Part.Extension.SelectByID2("", "FACE", -7.70328176440671E-03, 3.96239999998897E-02, -7.62437790422155E-03, False, 0, Nothing, 0)
    Set skPoint = Part.SketchManager.CreatePoint(-0.00527, 0.051345, 0#)
    Set skPoint = Part.SketchManager.CreatePoint(-0.005854, 0.025783, 0#)
    Set skPoint = Part.SketchManager.CreatePoint(-0.005888, -0.000009, 0#)
    Set skPoint = Part.SketchManager.CreatePoint(0.019408, 0.051285, 0#)
    Set skPoint = Part.SketchManager.CreatePoint(0.019093, 0.024628, 0#)
    Set skPoint = Part.SketchManager.CreatePoint(0.019629, -0.000148, 0#)
    Set skPoint = Part.SketchManager.CreatePoint(0.043756, 0.051962, 0#)
    Set skPoint = Part.SketchManager.CreatePoint(0.043146, 0.025865, 0#)
    Set skPoint = Part.SketchManager.CreatePoint(0.043401, 0.000225, 0#)
    Part.ClearSelection2 True
    Part.SketchManager.InsertSketch True
   
    boolstatus = Part.Extension.SelectByID2("Boss-Extrude2", "BODYFEATURE", -4.77922378944982E-02, 4.21639999998433E-02, 2.33214950450815E-02, False, 4, Nothing, 0)
    boolstatus = Part.Extension.SelectByID2("Sketch3", "SKETCH", 0, 0, 0, True, 64, Nothing, 0)
   

    Set swSketchFeat = Part.FeatureManager.FeatureSketchDrivenPattern(True, False)
    Set swSketchPatt = swSketchFeat.GetDefinition

    swSketchPatt.AccessSelections Part, Nothing
   

    Set swSketch = swSketchPatt.Sketch
    i = swSketch.GetSketchPointsCount2
   

    Set swPatternTransform = swSketchPatt.GetTransform(i)
   

    vBasePt = swSketchPatt.GetBasePoint

    Debug.Print swSketchFeat.Name
    Debug.Print "  Create pattern using only geometry? " & swSketchPatt.GeometryPattern
    Debug.Print "  Pattern seed coordinates in mm:  (" & vBasePt(0) * 1000# & ", " & vBasePt(1) * 1000# & ", " & vBasePt(2) * 1000# & ")"
    Debug.Print "  Body count: " & swSketchPatt.GetPatternBodyCount
    Debug.Print "  Face count: " & swSketchPatt.GetPatternFaceCount
    Debug.Print "  Feature count: " & swSketchPatt.GetPatternFeatureCount
    Debug.Print "  Reference point type (-1 for centroid): " & swSketchPatt.GetReferencePointType
    Debug.Print "  Use centroid as the reference point? " & swSketchPatt.UseCentroid
    Debug.Print "  Propagate visual properties? " & swSketchPatt.PropagateVisualProperty
   

    swSketchPatt.ReleaseSelectionAccess

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

 
*Email:  
Subject:   Feedback on Help Topics
Page:   Get Properties of Sketch Pattern Feature Example (VBA)
*Comment:  
*   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:



x

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
x

Web Help Content Version: API Help (English only) 2018 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.