Macro to suspend graphics update using SOLIDWORKS API

This macro demonstrates how to suspend graphics update while performing operations with feature tree and models (including opening of new documents) using SOLIDWORKS API.

Macro copies the bodies from the external part into the newly created derived configuration of the active part document.

Set the source part path (the part to copy bodies from) via SRC_PART constant

Const SRC_PART As String = "C:\Sample.sldprt"

Try both options to see the difference by changing the SUPPRESS_UPDATES constant

Const SUPPRESS_UPDATES As Boolean = True 'True to suppress updates, False to show the updates (default behavior)

Macro performs the following steps

Opens the model with bodies to copy
Copies all the bodies into the memory
Closes the model
Creates new derived configuration in the original model
Inserts copied bodies
Suppresses the created features in all configurations except of this one
Activates the original configuration

If SUPPRESS_UPDATES option is set to true all of the operations will be hidden and only active state of the model will be shown on screen (i.e. model opening, feature insertion etc. will be invisible)

Const SUPPRESS_UPDATES As Boolean = True

Const SRC_PART As String = "C:\Sample.sldprt"

Dim swApp As SldWorks.SldWorks

Sub main()

    Set swApp = Application.SldWorks
    
    Dim swModel As SldWorks.ModelDoc2
    
    Set swModel = swApp.ActiveDoc
    
    If TypeOf swModel Is SldWorks.PartDoc Then
        
        On Error GoTo End_

        If SUPPRESS_UPDATES Then
            SuppressUpdates swModel, True
        End If
        
        Dim activeConfName As String
        activeConfName = swModel.ConfigurationManager.ActiveConfiguration.Name
        
        Dim vBodies As Variant
        vBodies = GetBodies(SRC_PART)
        
        swModel.ConfigurationManager.AddConfiguration2 activeConfName & "_Merged", "", "", swConfigurationOptions2_e.swConfigOption_LinkToParent, activeConfName, "", True
        
        Dim i As Integer
        
        For i = 0 To UBound(vBodies)
            Dim swBody As SldWorks.Body2
            Set swBody = vBodies(i)
            Dim swFeat As SldWorks.Feature
            Set swFeat = swModel.CreateFeatureFromBody3(swBody, False, swCreateFeatureBodyOpts_e.swCreateFeatureBodySimplify)
            swFeat.SetSuppression2 swFeatureSuppressionAction_e.swUnSuppressFeature, swInConfigurationOpts_e.swThisConfiguration, Empty
        Next
        
        swModel.ShowConfiguration2 activeConfName

End_: 'restore the flag otherwise all files will be opened invisible
    
        If SUPPRESS_UPDATES Then
            SuppressUpdates swModel, False
        End If
        
    Else
        MsgBox "Please open part document"
    End If
    
End Sub

Sub SuppressUpdates(model As SldWorks.ModelDoc2, suppress As Boolean)
    
    Dim enable As Boolean
    enable = Not suppress
    
    Dim swView As SldWorks.ModelView
    Set swView = model.ActiveView
    
    swView.EnableGraphicsUpdate = enable
    
    model.FeatureManager.EnableFeatureTree = enable
    model.FeatureManager.EnableFeatureTreeWindow = enable
        
    swApp.DocumentVisible enable, swDocumentTypes_e.swDocPART
    swApp.DocumentVisible enable, swDocumentTypes_e.swDocASSEMBLY
    swApp.DocumentVisible enable, swDocumentTypes_e.swDocDRAWING
    
End Sub

Function GetBodies(path As String) As Variant
    
    Dim swPart As SldWorks.PartDoc
    Set swPart = swApp.OpenDoc6(path, swDocumentTypes_e.swDocPART, _
        swOpenDocOptions_e.swOpenDocOptions_Silent + swOpenDocOptions_e.swOpenDocOptions_ReadOnly, "", 0, 0)
    
    Dim vBodies As Variant
    vBodies = swPart.GetBodies2(swBodyType_e.swSolidBody, True)
    
    If Not IsEmpty(vBodies) Then
        Dim i As Integer
        For i = 0 To UBound(vBodies)
            Dim swBody As SldWorks.Body2
            Set swBody = vBodies(i)
            Set vBodies(i) = swBody.Copy
        Next
    End If
    
    swApp.CloseDoc swPart.GetTitle()
    
    GetBodies = vBodies
    
End Function