This example adds the dimension between 2 selected sketch segments (e.g. sketch lines) using SOLIDWORKS API. The dimension will be placed in the middle of 2 selection points.

Dimension with name
Dimension with name

When adding dimensions programmatically using SOLIDWORKS API it is important to disable the Input Dimension Value option otherwise the macro will be interrupted and will require user inputs.

The example below temporarily removes this option and restores the original value after the dimension inserted so user settings are not affected.

Option to input dimension value on creation
Option to input dimension value on creation
Dim swApp As SldWorks.SldWorks
Dim swModel As SldWorks.ModelDoc2
Dim swSelMgr As SldWorks.SelectionMgr

Sub main()

    Set swApp = Application.SldWorks
    Set swModel = swApp.ActiveDoc
    If Not swModel Is Nothing Then
        Set swSelMgr = swModel.SelectionManager
        If swSelMgr.GetSelectedObjectCount2(-1) = 2 Then
            Dim vPt1 As Variant
            Dim vPt2 As Variant
            vPt1 = swSelMgr.GetSelectionPoint2(1, -1)
            vPt2 = swSelMgr.GetSelectionPoint2(2, -1)
            Dim inputDimDefVal As Boolean
            inputDimDefVal = swApp.GetUserPreferenceToggle(swUserPreferenceToggle_e.swInputDimValOnCreate)
            swApp.SetUserPreferenceToggle swUserPreferenceToggle_e.swInputDimValOnCreate, False

            swModel.AddDimension2 (vPt1(0) + vPt2(0)) / 2, (vPt1(1) + vPt2(1)) / 2, (vPt1(2) + vPt2(2)) / 2
            swApp.SetUserPreferenceToggle swUserPreferenceToggle_e.swInputDimValOnCreate, inputDimDefVal
            MsgBox "Please select sketch segments to add dimension"
        End If
        MsgBox "Please open the model"
    End If
End Sub