Description

You can utilize the tool for the purpose of creating a rectangle that is centered about the origin, on a selected plane or face.

System Requirements

• SolidWorks Version: SolidWorks 2014 or newer
• Operating System: Windows 7 or later

Pre-requisites

• A plane or face must be pre-selected prior to starting the macro.
• SolidWorks must have an active document.

Results

• A centered rectangle will be drawn on the specified plane or face.
• The opposite corners of the rectangle will have a construction line drawn between them, which will be constrained to the origin.
• The rectangle’s width and height will be created.

Steps to Set Up the Macro

1. Choose a Plane or Face: In your SolidWorks document, pre-select the plane (e.g., Right Plane) or planar face on which the rectangle will be sketched.
2. Execute the Macro: Now run the macro (preferably via an assigned keyboard shortcut for maximum speed). The centered rectangle and all related features will be completely created on the selected geometry. This SOLIDWORKS macro for instant centered rectangle sketching ensures that the sketch is generated quickly and precisely without manual alignment.

VBA Macro Code

' 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

Dim swApp As Object                          ' SolidWorks application object
Dim Part As Object                           ' Active document object
Dim SelMgr As Object                         ' Selection manager for the active document
Dim boolstatus As Boolean                    ' Boolean status for operations
Dim longstatus As Long, longwarnings As Long ' Long status for warnings/errors
Dim Feature As Object                        ' Feature object
Dim CurSelCount As Long                      ' Count of selected items

Sub main()

    ' Initialize SolidWorks application and active document
    Set swApp = Application.SldWorks
    Set Part = swApp.ActiveDoc

    ' Ensure there is an active document
    If Part Is Nothing Then
        MsgBox "No active document found. Please open a part or assembly and try again.", vbCritical, "Error"
        Exit Sub
    End If

    ' Initialize the selection manager
    Set SelMgr = Part.SelectionManager

    ' Disable input dimensions on creation
    swApp.SetUserPreferenceToggle swInputDimValOnCreate, False

    ' Check if a plane or face is preselected
    CurSelCount = SelMgr.GetSelectedObjectCount
    If CurSelCount = 0 Then
        MsgBox "Please preselect a plane or face before running the macro.", vbExclamation, "No Selection"
        Exit Sub
    End If

    ' Insert a new sketch on the selected plane or face
    boolstatus = Part.Extension.SelectByID2("", "PLANE", 0, 0, 0, False, 0, Nothing, 0)
    Part.InsertSketch2 True
    Part.ClearSelection2 True

    ' Create a rectangle centered about the origin
    Part.SketchRectangle -0.037, 0.028, 0, 0.015, -0.019, 0, True

    ' Clear selection and add a diagonal construction line
    Part.ClearSelection2 True
    Dim Line As Object
    Set Line = Part.CreateLine2(-0.037, -0.019, 0, 0.015, 0.028, 0)
    Line.ConstructionGeometry = True

    ' Add midpoint constraints to ensure the rectangle is centered
    boolstatus = Part.Extension.SelectByID2("Point1@Origin", "EXTSKETCHPOINT", 0, 0, 0, True, 0, Nothing, 0)
    Part.SketchAddConstraints "sgATMIDDLE"
    Part.ClearSelection2 True

    ' Add dimensions to the rectangle
    boolstatus = Part.Extension.SelectByID2("Line1", "SKETCHSEGMENT", -0.001, 0.027, 0, False, 0, Nothing, 0)
    Dim Annotation As Object
    Set Annotation = Part.AddDimension2(-0.0004, 0.045, 0) ' Horizontal dimension
    Part.ClearSelection2 True

    boolstatus = Part.Extension.SelectByID2("Line2", "SKETCHSEGMENT", -0.030, 0.001, 0, False, 0, Nothing, 0)
    Set Annotation = Part.AddDimension2(-0.061, -0.001, 0) ' Vertical dimension
    Part.ClearSelection2 True

    ' Re-enable input dimensions on creation
    swApp.SetUserPreferenceToggle swInputDimValOnCreate, True

    ' Inform the user that the macro is complete
    MsgBox "Rectangle sketch created successfully.", vbInformation, "Success"

Macro

You can download the macro from here.