Description
This macro for SOLIDWORKS automates a repetitive and frequent task for engineers: changing and exiting sketches. Following the provided code, it is capable of automatically determining and adjusting the view to normal for an active sketch or exiting the sketch if the view is already normal. Also, when to open a sketch, when to normalize a view, and when to exit from the sketch is needed. The macro can also deal with suppressed subcomponents automatically, as well as navigate complex feature trees. This makes a VBA macro to automate sketch editing in SOLIDWORKS a potent addition to your design process and productivity.
System Requirements
- SOLIDWORKS Version: SOLIDWORKS 2014 or newer
- Operating System: Windows 7 or later
Pre-Conditions
- Active Document: An active part (.sldprt) or assembly (.sldasm) document must be open in SOLIDWORKS.
- Selection: For the macro to operate correctly, a feature, face, edge, or sketch must be selected.
Results
- Automated View & Sketch Access: Edits the driving sketch of the selected feature/geometry, while also orienting the view normal to the sketch plane.
- Efficient Sketch Exits: Exits from the active sketch if the view is already oriented normal, streamlining the completion of a sketching session.
- Component & Hierarchy Handling: Automatically resolves the selected subcomponents and navigates into the selected sketch hierarchy of more complex features, ensuring a seamless operation.
Process to Implement the Macro
- Execute the Macro: Execute the macro in an open SOLIDWORKS document. The associated document must be a valid document type (part or assembly), and the appropriate items must be selected.
- Behavior Based on Selection:
○ If the user has selected a feature or geometry, the macro will open the driving sketch and view the model in a different view.
○ If no entities are selected and the user is in an active sketch, the macro will set the view to normal.
○ If the user is already viewing in a normal view, the macro will exit the sketch and end.
VBA Macro Code
|
1 2 3 4 5 6 7 8 9 10 11 12 13 14 15 16 17 18 19 20 21 22 23 24 25 26 27 28 29 30 31 32 33 34 35 36 37 38 39 40 41 42 43 44 45 46 47 48 49 50 51 52 53 54 55 56 57 58 59 60 61 62 63 64 65 66 67 68 69 70 71 72 73 74 75 76 77 78 79 80 81 82 83 84 85 86 87 88 89 90 91 92 93 94 95 96 97 98 99 100 101 102 103 104 105 106 107 108 109 110 111 112 113 114 115 116 117 118 119 120 121 122 123 124 125 126 127 128 129 130 131 132 133 134 135 136 137 138 139 140 |
' Disclaimer: ' The code provided should be used at your own risk. ' Blue Byte Systems Inc. assumes no responsibility for any issues or damages that may arise from using or modifying this code. ' For more information, visit [Blue Byte Systems Inc.](https://bluebyte.biz). Option Explicit ' Define a structure for storing view data Type ViewData ViewScale As Double ' Scale of the view Orientation As SldWorks.MathTransform ' Orientation transformation matrix Translation As SldWorks.MathVector ' Translation vector End Type ' Enum for comparison results between two views Enum CompareViewResult_e Same = 0 ' Views are identical DiffOrientation = 2 ^ 0 ' Different orientations difftranslation = 2 ^ 1 ' Different translations diffscale = 2 ^ 2 ' Different scales End Enum ' Debugging constants and tolerance Const Bug As Boolean = False ' Debug output flag Const Tol As Integer = 2 ' Tolerance for comparisons Sub main() On Error Resume Next Dim swApp As SldWorks.SldWorks Dim swDoc As SldWorks.ModelDoc2 Dim SelMgr As SldWorks.SelectionMgr Dim swFeat As SldWorks.Feature Dim swSelType As Long Dim StartView As ViewData Dim CurView As ViewData Dim compRes As CompareViewResult_e ' Initialize SolidWorks objects Set swApp = Application.SldWorks Set swDoc = swApp.ActiveDoc Set SelMgr = swDoc.SelectionManager StartView = GetViewData(swDoc.ActiveView) ' Check if a sketch is active If Not swDoc.GetActiveSketch2 Is Nothing Then ' No selection: Align view "normal to" the sketch If SelMgr.GetSelectedObjectCount2(-1) < 1 Then swDoc.ShowNamedView2 "*Normal To", -1 CurView = GetViewData(swDoc.ActiveView) compRes = CompareViewData(StartView, CurView, Tol) If compRes = Same Then swDoc.SketchManager.InsertSketch True Exit Sub End If Else swDoc.SketchManager.InsertSketch True End If End If ' Resolve selected feature or entity swSelType = SelMgr.GetSelectedObjectType3(1, -1) Select Case swSelType Case swSelFACES, swSelEDGES Set swFeat = SelMgr.GetSelectedObject6(1, -1).GetFeature If swFeat Is Nothing Then Exit Sub Case swSelBODYFEATURES, swSelSKETCHES Set swFeat = SelMgr.GetSelectedObject6(1, -1) Case Else Exit Sub End Select ' Edit sketch or feature If swFeat.GetTypeName = "ProfileFeature" Then swDoc.EditSketchOrSingleSketchFeature Else swDoc.FeatEdit End If ' Align view to "normal to" if a sketch is active If Not swDoc.GetActiveSketch2 Is Nothing Then swDoc.ShowNamedView2 "*Normal To", -1 End If ' Clear selections swDoc.ClearSelection2 True End Sub ' Function to get view data (scale, orientation, translation) Private Function GetViewData(view As SldWorks.ModelView) As ViewData Dim data As ViewData Set data.Orientation = view.Orientation3 ' Get orientation matrix Set data.Translation = view.Translation3 ' Get translation vector data.ViewScale = view.Scale2 ' Get view scale GetViewData = data End Function ' Function to compare two sets of view data Private Function CompareViewData(firstViewData As ViewData, secondViewData As ViewData, Tol As Integer) As CompareViewResult_e Dim res As CompareViewResult_e res = Same ' Compare orientation If Not CompareArrays(firstViewData.Orientation.ArrayData, secondViewData.Orientation.ArrayData, Tol) Then res = res + DiffOrientation End If ' Compare translation If Not CompareArrays(firstViewData.Translation.ArrayData, secondViewData.Translation.ArrayData, Tol) Then res = res + difftranslation End If ' Compare scale If Not TolerantEqual(firstViewData.ViewScale, secondViewData.ViewScale, Tol) Then res = res + diffscale End If CompareViewData = res End Function ' Function to compare arrays with tolerance Private Function CompareArrays(firstArr As Variant, secondArr As Variant, Tol As Integer) As Boolean If UBound(firstArr) = UBound(secondArr) Then Dim i As Integer For i = 0 To UBound(firstArr) If Not TolerantEqual(firstArr(i), secondArr(i), Tol) Then CompareArrays = False Exit Function End If Next CompareArrays = True Else CompareArrays = False End If End Function ' Function to compare two numbers with tolerance Private Function TolerantEqual(a As Variant, b As Variant, Tol As Integer) As Boolean TolerantEqual = Abs(a - b) <= Abs(a / 10 ^ Tol) ' Compare within tolerance End Function |
Macro
You can download the macro from here.
Customization of The Macro
For engineering teams who have special workflow requirements, please reach out, and we will be sure to provide you with our modified version to meet your immediate needs. Regardless of your level of customization needs to maximize your design process, we can help!
Custom development of SOLIDWORKS macros and add-ins is our specialty at Blue Byte Systems Inc. However, we also specialize in seamless integration with existing systems, specific file types or multi-body part tasks are always in mind.
Please contact us to discuss how we can help you reach a more efficient and productive workflow with our custom solutions.