Manufacturing DevBlog

Inventor: Change text items in TitleBlockDefinition

by Vladimir Ananyev

Issue

Question: How do I change text items in the TitleBlockDefinition in Inventor?

Solution

Answer: Assuming you have an active drawing document open, first you need to access the TitleBlockDefinitions collection. Step through the collection to find the Title Block of interest, as shown in the following code fragment, the "ANSI - Large" title block definition.

When the TitleBlockDefinition of interest is found, we select the TextBoxes collection. Step through the collection until the TextBox of interest is found. For a TextBox the 'Text' property is a read/write property. The most important code in the following code fragment is placing the TitleBlockDefinition into edit mode with a call to 'Edit' and exiting the edit mode with a call to 'ExitEdit'.

Two code samples and a sample drawing document ("Drawing.zip") demonstrate this.

 Download Drawing

VBA:

Private Sub ChgTitleBlkDef()

 

  Dim objDoc As Document

  Set objDoc = ThisApplication.ActiveDocument

 

  If objDoc Is Nothing Then

    MsgBox "No Active Document"

    Set objDoc = Nothing

    Exit Sub

  End If

 

  'Is the active document a drawing document?

  If objDoc.DocumentType <> kDrawingDocumentObject Then

    MsgBox "Not a drawing document"

    Set objDoc = Nothing

    Exit Sub

  End If

 

  Dim objDrawDoc As DrawingDocument

  Set objDrawDoc = objDoc

 

  Dim colTitleBlkDefs As TitleBlockDefinitions

  Set colTitleBlkDefs = objDrawDoc.TitleBlockDefinitions

 

  Dim objTitleBlkDef As TitleBlockDefinition

 

  For Each objTitleBlkDef In colTitleBlkDefs

    If objTitleBlkDef.Name = "ANSI - Large" Then

      'we have the title blk we want

      Exit For

    End If

  Next objTitleBlkDef

 

  If objTitleBlkDef Is Nothing Then

    MsgBox "ANSI - Large TitleBlockDefinition not found!"

    Set objDrawDoc = Nothing

    Set colTitleBlkDefs = Nothing

    Set objTitleBlkDef = Nothing

    Exit Sub

  End If

 

  ' If we are here we have the title block of interest.

  ' Get the title block sketch and set it active

  Dim objDrwSketch As DrawingSketch

  Call objTitleBlkDef.Edit(objDrwSketch)

 

  Dim colTextBoxes As TextBoxes

  Set colTextBoxes = objDrwSketch.TextBoxes

 

  Dim objTextBox As TextBox

  For Each objTextBox In colTextBoxes

    If objTextBox.Text = "TITLE" Then

      objTextBox.Text = "Captain CAD Engineering"

      Exit For

    End If

  Next objTextBox

 

  Call objTitleBlkDef.ExitEdit(True)

 

  ' Clean up

  Set objDrawDoc = Nothing

  Set colTitleBlkDefs = Nothing

  Set objTitleBlkDef = Nothing

  Set objDrwSketch = Nothing

  Set colTextBoxes = Nothing

  Set objTextBox = Nothing

 

  Beep

End Sub

 

VB .NET:

Sub ChgTitleBlkDef()

 

  Dim objDrawDoc As DrawingDocument _

      = CType(oApp.ActiveDocument, DrawingDocument)

 

  Dim colTitleBlkDefs As TitleBlockDefinitions _

      = objDrawDoc.TitleBlockDefinitions

 

  Dim objTitleBlkDef As TitleBlockDefinition = Nothing

  For Each objTitleBlkDef In colTitleBlkDefs

    If objTitleBlkDef.Name = "ANSI - Large" Then

      'we have the title blk we want

      Exit For

    End If

  Next

 

  ' If we are here we have the title block of interest.

  ' Get the title block sketch and set it active

  Dim objDrwSketch As DrawingSketch = Nothing

  objTitleBlkDef.Edit(objDrwSketch)

 

  Dim colTextBoxes As TextBoxes _

        = objDrwSketch.TextBoxes

 

  For Each objTextBox As TextBox In colTextBoxes

    If objTextBox.Text = "TITLE" Then

      objTextBox.Text = "Captain CAD Engineering"

      Exit For

    End If

  Next

  objTitleBlkDef.ExitEdit(True)

 

  Beep()

End Sub

Inventor: Accessing the views represented by document windows

by Vladimir Ananyev

Issue

How to access the views represented by the document windows open in an Inventor session?

Solution

An Inventor session can have one or more documents open. Each of the documents will be displayed in its own window. Also, in addition, you could have one or more views (e.g. top view, right view etc.) of a document being displayed in separate windows. So, each window displays a view of a particular document with the possibility that the source document could be the same for the windows (i.e. the windows are displaying different views of the same document).

The API allows access to these views of the same or different documents that are being displayed in separate windows. From the Application object you could get the ActiveView object (represents the currently active view (might be one of many) of a document). The ActiveView object corresponds to the active window in the Inventor session. The ActiveView object in turn supports the Camera object that helps you set the new orientation using the ViewOrientationType property. Also, if one or more views of a particular document are being displayed in separate windows, they can also be accessed using the Views object obtained from the Document object.

The following is a VBA sample to access and change view orientation:

Public Sub GetViews()

  'access only the currently active view of a document
  Dim oActiveView As View
  Set oActiveView = ThisApplication.ActiveView
 
  Dim oCamera As Camera
  Set oCamera = oActiveView.Camera
 
  oCamera.ViewOrientationType = kIsoBottomRightViewOrientation
  oCamera.Apply

 
  'if you have multiple windows(views) of a document open,

  'you can access all of them
  Dim oDoc As Document
  Set oDoc = ThisApplication.ActiveDocument
  
  Dim oViews As Views
  Set oViews = oDoc.Views
 
  Dim oView As View
  For Each oView In oViews
      Set oCamera = oView.Camera
  Next

End Sub

 

The equivalent C# code:

private void GetViews()

{

    // access only the currently active view of a document

    Inventor.View oActiveView = oApp.ActiveView;          

    Camera oCamera = oActiveView.Camera;

    oCamera.ViewOrientationType =

        ViewOrientationTypeEnum.kIsoBottomRightViewOrientation;

    oCamera.Apply();

 

    // if you have multiple windows(views) of a document open,

    // you can access all of them

    Inventor.Document oDoc = oApp.ActiveDocument;

    Views oViews = oDoc.Views;           

    foreach (Inventor.View oView in oViews)

    {

        oCamera = oView.Camera;

    }       

}

Inventor: DisplayState property of BrowserNodeDefinition.

by Vladimir Ananyev

Issue

BrowserNodeDefinition.DisplayState returns current states for native browser nodes. I find that it returns kDefaultDisplayState unless it was explicitly changed by using BrowserNodeDefinition.DisplayState. Is this assumption correct?

Solution

This is as designed. A return value of kDefaultDisplayState indicates that the browser node’s display state has been decided by Inventor. Other values indicate an override applied by API client. The DisplayState property is intended to be used for browser customization. If you're interested in state of associated object you need to query the object associated with the browser node.

The following samples illustrate this approach:

VBA:

Sub DumpAdaptivityInfo()

  Dim doc As AssemblyDocument

  Set doc = ThisApplication.ActiveDocument

  Call DumpNodes(doc.BrowserPanes.ActivePane.topNode)

End Sub

 

Private Sub DumpNodes(topNode As BrowserNode)

  On Error Resume Next

 

  Dim node As BrowserNode

 

  For Each node In topNode.BrowserNodes

 

    Dim nodeDef As NativeBrowserNodeDefinition

    Set nodeDef = node.BrowserNodeDefinition

 

    Dim nativeObj As Object

    Set nativeObj = nodeDef.NativeObject

 

    If Not nativeObj Is Nothing Then

      If TypeOf nativeObj Is ComponentOccurrence Then

     

        Dim occ As ComponentOccurrence

        Set occ = nodeDef.NativeObject

       

        Debug.Print nodeDef.Label

        Debug.Print Spc(2); "Adaptive: " & occ.Adaptive

       

      End If

    End If

    Call DumpNodes(node)

  Next

 

End Sub

 

VB .NET:

Sub DumpAdaptivityInfo()

  Dim oDoc As AssemblyDocument _

      = CType(oApp.ActiveDocument, AssemblyDocument)

  DumpNodes(oDoc.BrowserPanes.ActivePane.TopNode)

End Sub

 

Private Sub DumpNodes(ByVal topNode As BrowserNode)

  For Each node As BrowserNode In topNode.BrowserNodes

    Dim nodeDef As NativeBrowserNodeDefinition _

        = CType(node.BrowserNodeDefinition, NativeBrowserNodeDefinition)

    Dim nativeObj As Object = Nothing

    Try

      nativeObj = nodeDef.NativeObject

    Catch

    End Try

    If nativeObj IsNot Nothing Then

      If TypeOf nativeObj Is ComponentOccurrence Then

        Dim occ As ComponentOccurrence _

          = CType(nodeDef.NativeObject, ComponentOccurrence)

        Debug.Print(nodeDef.Label)

        Debug.Print(Space(2) + "Adaptive: " & occ.Adaptive)

      End If

    End If

    DumpNodes(node)

  Next

End Sub

Inventor: Create Pattern of Component Occurrences

by Vladimir Ananyev

Issue

How to create a pattern (rectangular/circular) of occurrences in an Inventor assembly?

Solution

The sample code below shows how you could pattern occurrences in the x and y direction. The value no_x_rect  refers to the number of occurrences in the x direction, no_y_rect refers to the number of occurrences in  the y direction.  This example just creates a pattern along the x and y directions, you could modify this code to create patterns along any desired directions (e.g. you may pass in an EdgeProxy to define the directions). Similarly, you could also create circular patterns except that you would be dealing with angular co-ordinates.

 

VBA sample code:

Sub CreatePatternsInAssembly()

 

  'open an assembly with at least two components and run this sample

 

  Dim oAssyDoc As AssemblyDocument

  Set oAssyDoc = ThisApplication.ActiveDocument

 

  Dim oAssyDef As AssemblyComponentDefinition

  Set oAssyDef = oAssyDoc.ComponentDefinition

 

  If oAssyDef.Occurrences.Count < 2 Then

    MsgBox "Assembly must have 2 components"

    Exit Sub

  End If

 

  'base work axes

  Dim XAxis As WorkAxis

  Dim YAxis As WorkAxis

  Dim Zaxis As WorkAxis

  With oAssyDef

    Set XAxis = .WorkAxes(1)

    Set YAxis = .WorkAxes(2)

    Set Zaxis = .WorkAxes(3)

  End With

 

  'Create an object collection

  Dim objCol As ObjectCollection

  Set objCol = ThisApplication _

    .TransientObjects.CreateObjectCollection

 

  'add the desired occurrence to be patterned

  objCol.Add oAssyDef.Occurrences.Item(1)

 

  'set the number of patterns in the x direction

  Dim no_x_rect As Integer

  no_x_rect = 3

 

  'set the number of patterns in the y direction

  Dim no_y_rect As Integer

  no_y_rect = 3

  'Creating a Rectangular pattern

  Call oAssyDef.OccurrencePatterns _

        .AddRectangularPattern(objCol, _

          XAxis, True, 10, no_x_rect, _

          YAxis, True, 10, no_y_rect)

 

 

  'Creating a Circular pattern

  objCol.Clear

  objCol.Add oAssyDef.Occurrences.Item(1)

  Call oAssyDef.OccurrencePatterns _

        .AddCircularPattern(objCol, _

          Zaxis, True, "45 deg", 5)

 

End Sub

 

 

C# sample code:

 

private void CreatePatternsInAssembly()

{ //open an assembly with at least two components and run this sample

   

    AssemblyDocument oAssyDoc = (AssemblyDocument)oApp.ActiveDocument; 

    AssemblyComponentDefinition oAssyDef = oAssyDoc.ComponentDefinition;

 

  if (oAssyDef.Occurrences.Count < 2)

  {

    MessageBox.Show("Assembly must have 2 components");

    return;

  }

 

    //base work axes

    WorkAxis XAxis = oAssyDef.WorkAxes[1];

    WorkAxis YAxis = oAssyDef.WorkAxes[2];

    WorkAxis ZAxis = oAssyDef.WorkAxes[3];

 

    //Create an object collection

    ObjectCollection objCol = oApp

        .TransientObjects.CreateObjectCollection();

 

    //add the desired occurrence to be patterned

    objCol.Add(oAssyDef.Occurrences[1]);

 

    //set the number of patterns in the x direction

    int no_x_rect = 3; 

    //set the number of patterns in the y direction

    int no_y_rect = 3;

 

    //Creating a Rectangular pattern

    oAssyDef.OccurrencePatterns.AddRectangularPattern(

        objCol, XAxis, true, 10, no_x_rect,

                YAxis, true, 10, no_y_rect); 

 

    //Creating a Circular pattern

    objCol.Clear();

    objCol.Add(oAssyDef.Occurrences[1]);

    oAssyDef.OccurrencePatterns.AddCircularPattern(

        objCol, ZAxis, true, "45 deg", 5);

}

CheckoutFile / CheckinFile - avoid warnings in Vault Explorer

By Wayne Brill

If you have used the Vault API to Check-out / Check-in a file you may have noticed a status on the file of "Incorrect version Refresh the file" or “Edited out of turn” in Vault Explorer.

"Incorrect version Refresh the file"

In vault explorer a file is checked out to the working folder, modified there, and then checked in. Because of this, the latest checked in file matches the file in the working folder. If your code puts the file in a different directory the version in your working folder is never updated and the status is telling you that what you have on disk is not the latest version in vault. 

“Edited out of turn”

The “Edited out of turn”  status occurs when the create date of the local file does not match the create date of the File object in the vault. This blog post has more detail about this.

Example code:

Download Vault_CheckIn_CheckOut

 

Below is code from this project that avoids both of these conditions. To use this example the first file in the root folder of the vault needs to be a txt file. (or change the code so that it uses a txt file).

private void button2_Click(object sender, EventArgs e)

{

    if (m_serviceManager != null )

    {

 

        Folder rootFolder =

     m_serviceManager.DocumentService.GetFolderRoot();

        File[] rootFolderFiles =

            m_serviceManager.DocumentService.

        GetLatestFilesByFolderId(rootFolder.Id, true);

 

        if (rootFolderFiles == null ||

               rootFolderFiles.Length == 0)

            return;

 

        File file = rootFolderFiles[0];

        ByteArray byteArray;

 

        string localPath =

       m_vaultExplorer.GetWorkingFolder(rootFolder);

 

        //Check out the file

        m_serviceManager.DocumentService.

            CheckoutFile(rootFolder.Id,

            file.Id,

            CheckoutFileOptions.Master,

            Environment.MachineName,

            localPath, "test check-out",

        DownloadOptions.Download,

                 false, out byteArray);

 

        string filePath =

      System.IO.Path.Combine(localPath, file.Name);

 

        //Make readonly false for file

        System.IO.FileInfo localFileInfo =

             new System.IO.FileInfo(filePath);

        localFileInfo.IsReadOnly = false;

 

        // edit the file

        System.IO.File.WriteAllBytes

                  (filePath, byteArray.Bytes);

        System.IO.File.AppendAllText

           (filePath, Environment.NewLine +

                          "Hello World_wB!");

 

        // check in the file.

        byteArray.Bytes =

       System.IO.File.ReadAllBytes(filePath);

 

        file = m_serviceManager.DocumentService.

            CheckinFile(file.MasterId,

            "test check-in wB", false,

            System.IO.File.GetLastWriteTime

              (filePath), null, null, true,

                 file.Name, file.FileClass,

                    file.Hidden, byteArray);

 

        // avoid the "Edited-out-of-turn"

        // icon in Vault Explorer

        System.IO.FileInfo info =

            new System.IO.FileInfo(filePath);

        info.CreationTime = file.CreateDate;

        info.Attributes =

          info.Attributes |

           System.IO.FileAttributes.ReadOnly;

    }

}

Inventor: Create Sculpt Feature

by Vladimir Ananyev

Issue

How can I create a sculpt feature programmatically?

Solution

The following is a sample illustrating the way of creating a sculpt feature.

  

Please download the attached sample file before running the code:  Download part model

VB .NET sample code:

Sub RunSculptDemo()

  'reference to the part document

  Dim oDoc As PartDocument _

      = TryCast(oApp.ActiveDocument, PartDocument)

  If oDoc Is Nothing Then Exit Sub

  Dim oDef As PartComponentDefinition _

      = oDoc.ComponentDefinition

 

  'features collection

  Dim oFeatures As PartFeatures = oDef.Features

  'surfaces collection

  Dim oSurfaces As ObjectCollection = _

    oApp.TransientObjects.CreateObjectCollection()

  For Each osurface As WorkSurface In oDef.WorkSurfaces

    oSurfaces.Add(oFeatures.SculptFeatures _

      .CreateSculptSurface(osurface, _

        PartFeatureExtentDirectionEnum.kNegativeExtentDirection))

  Next

  'create sculpt feature

  Dim oSculpt As SculptFeature = oFeatures _

    .SculptFeatures.Add(oSurfaces, _

        PartFeatureOperationEnum.kCutOperation)

End Sub

 

C# sample code:

void RunSculptDemo()

{

  //get reference to active part document

  PartDocument oDoc = (PartDocument)oApp.ActiveDocument;

  PartComponentDefinition oDef = oDoc.ComponentDefinition;

  //features collection

  PartFeatures oFeatures = oDef.Features;

  //surfaces collection

  ObjectCollection oSurfaces =

      oApp.TransientObjects.CreateObjectCollection();

  foreach (WorkSurface osurface in oDef.WorkSurfaces)

  {

    oSurfaces.Add(oFeatures.SculptFeatures

      .CreateSculptSurface(osurface,

        PartFeatureExtentDirectionEnum.kNegativeExtentDirection));

  }   

  //create sculpt feature

  SculptFeature oSculpt = oFeatures

    .SculptFeatures.Add(oSurfaces,

        PartFeatureOperationEnum.kCutOperation);

}

 

VBA sample code:

Sub RunSculptDemo()

 

  Dim oDoc As PartDocument

  Set oDoc = ThisApplication.ActiveDocument

  Dim oDef As PartComponentDefinition

  Set oDef = oDoc.ComponentDefinition

 

  Dim oFeas As PartFeatures

  Set oFeas = oDef.Features

 

  Dim oSurfaces As ObjectCollection

  Set oSurfaces = ThisApplication _

        .TransientObjects.CreateObjectCollection

 

  Dim osurface As WorkSurface

  For Each osurface In oDef.WorkSurfaces

    oSurfaces.Add oFeas.SculptFeatures _

      .CreateSculptSurface(osurface, _

          kNegativeExtentDirection)

  Next

 

  Dim oSculpt As SculptFeature

  Set oSculpt = oFeas.SculptFeatures _

        .Add(oSurfaces, kCutOperation)

 

End Sub

 

ComponentOccurrence contexts and Reference keys

by Vladimir Ananyev

Issue

I seem to have some problems with Occurrences, SubOccurrences and Definitions. E.g. why is the reference key different for an Occurrence depending on how I get to it?

Solution

In our example we'll use the following document structure:

Asm1
+ SubAsm1:1
      + Part1
+ SubAsm1:2
      + Part1

Whenever you use the Definition property of a ComponentOccurrence, it takes you out of the context of the Document where the ComponentOccurrence resides and has the same effect as opening the Document the ComponentOccurrence references and using that Document's ComponentDefinition directly.

Asm1.ComponentDefinition.Occurrences(1).Definition = SubAsm1.ComponentDefinition

When a ComponentOccurrence is reached directly from a Definition and not from an Occurrence of that Definition, then it does not have any information about any assemblies that contain it, and therefore the ComponentOccurrence's Parent property returns Nothing or Null. Only SubOccurrences have Parents.

As an example if you want to get the transformation matrix of SubAsm1:1->Part1 that shows how this instance of Part1 is placed inside Asm1's coordinate system, then you should not break the Occurrences.SubOccurrences chain with a reference to a Definition property. Instead do it like this: Asm1.ComponentDefinition.Occurrences(1).SubOccurrences(1).Transformation

NOTE: As an alternative, you can also use Definition property in combination with the CreateGeometryProxy function.

The same applies to all other ComponentOccurrence properties including GetReferenceKey(). If you get a reference key for the Part1 occurrence in SubAsm1's context, it provides a key that is suitable to identify Part1 inside SubAsm1. This is not the same key that you get for SubAsm1:1->Part1 in Asm1, which obviously needs to be different from SubAsm1:2->Part1 as well, since this is for identifying a given instance of Part1 in Asm1 and not only in SubAsm1.

Base view of isometric view

by Vladimir Ananyev

Issue

I need to find the base view of all projected views in the drawing. I use the DrawingView.ParentView however the ParentView is nothing if the view is an isometric view. Is there a way to get the baseview?

Solution

Isometric projected views are not associated with the base views. You can see this in the browser. When you create an isometric projected view, it is not nested under the base view. Also deleting the base view does not delete the isometric view. There is no a property that could return the projected view from the base view. A solution is to check the ReferencedDocumentDescriptor.FullDocumentName property – both views should reference the same document.

The following VB .NET function uses this approach:

Private Function IsProjectedView( _

      oBaseView As DrawingView, _

      oIsoView As DrawingView) As Boolean

     

  Return ((oIsoView.ViewType = _

           DrawingViewTypeEnum.kProjectedDrawingViewType) _

  And (oBaseView.ReferencedDocumentDescriptor.FullDocumentName _

     = oIsoView.ReferencedDocumentDescriptor.FullDocumentName))

 

End Function

Edge or Face by point coordinates

by Vladimir Ananyev

Issue

How to find an Edge in the model given a point coordinate that lies on the Edge ?

Solution

This can be determined by using the 'LocateUsingPoint' method of the SurfaceBody object as shown in the following sample code: Point is defined by workpoint with hardcoded name.

C#

private void button1_Click(object sender, EventArgs e)

{

  //get reference to active part document

  PartDocument oDoc = (PartDocument)_InventorApp.ActiveDocument;

  //get some workpoint in model by its name

  WorkPoint wp = oDoc.ComponentDefinition.WorkPoints["wp4"];  

  try

  {

    //coordinate 3d-point

    Inventor.Point pt = wp.Point;

 

    // try to find edge

    Object obj = oDoc.ComponentDefinition.SurfaceBodies[1]

        .LocateUsingPoint(ObjectTypeEnum.kEdgeObject, pt, 0.1);

 

    //// try to find face

    //Object obj =  oDoc.ComponentDefinition.SurfaceBodies[1]

    //    .LocateUsingPoint(ObjectTypeEnum.kFaceObject, pt, 0.1);

 

    // visualize found object using document select set

    oDoc.SelectSet.Select(obj); 

  }

  catch

  {

    MessageBox.Show("Nothing selected at the specified point!",

                    "Find Edge or Face");

  } 

}

 

VB .NET

Private Sub Button1_Click(sender As System.Object, _

                          e As System.EventArgs) _

                        Handles Button1.Click

  ' get reference to active part document

  Dim oDoc As PartDocument = TryCast(oApp.ActiveDocument, PartDocument)

 

  ' get some workpoint in model by its name

  Dim wp As WorkPoint = oDoc.ComponentDefinition.WorkPoints.Item("wp1")

 

  Try

    ' coordinate 3d-point

    Dim pt As Inventor.Point = wp.Point

   

    ' try to find edge

    Dim obj As Object = oDoc.ComponentDefinition.SurfaceBodies.Item(1) _

               .LocateUsingPoint(ObjectTypeEnum.kEdgeObject, pt, 0.1)

   

    '' try to find face

    'Dim obj As Object = oDoc.ComponentDefinition.SurfaceBodies.Item(1) _

    '      .LocateUsingPoint(ObjectTypeEnum.kFaceObject, pt, 0.1)

   

    ' visualize found object using document select set

    oDoc.SelectSet.Select(obj)

  Catch ex As Exception

    MessageBox.Show("Nothing selected at the specified point!",

                    "Find Edge or Face")

  End Try

End Sub

 

VBA

Sub Find_EdgeByPoint()

 

  Dim oDoc As PartDocument

  Set oDoc = ThisApplication.ActiveDocument

 

  Dim wp As WorkPoint

  Set wp = oDoc.ComponentDefinition.WorkPoints.Item("wp4")

 

  Dim pt As Point

  Set pt = wp.Point

 

  On Error Resume Next

  Dim Obj As Object

  Set Obj = oDoc.ComponentDefinition.SurfaceBodies.Item(1) _

    .LocateUsingPoint(kEdgeObject, pt, 0.1)

   

'  Set Obj = oDoc.ComponentDefinition.SurfaceBodies.Item(1) _

'    .LocateUsingPoint(kFaceObject, pt, 0.1)

 

  If Err.Number <> 0 Then

    MsgBox "Nothing selected at the specified point!"

  Else

    oDoc.SelectSet.Select Obj

  End If

   

End Sub

SaveAs with SaveCopyAs False

By Adam Nagy

If you want to save the document with a new file name and make it appear so in the user interface as well, just like in case of Inventor Menu >> Save As >> Save As,

then you need to create a copy of the file with the new name using SaveAs(..., SaveCopyAs=True), open this file and close the original one.

This is exactly what Inventor is doing as well in the background.

Note that SaveAs(..., SaveCopyAs=False) should only be used in case of a new file which has not been saved yet, as it is pointed out in the API help file too:

"SaveCopyAs: Input Boolean that indicates whether the file to be saved is new or is a copy of a previously existing file."

Here is also a table my colleague created describing the behaviour of the save functions in the API:

API	Expected Usage	Note	UI
Save/Save2	If the document was saved onto disk, this is just like you click the Save button in UI, it will save the changes in memory to the file on disk. If the document is unsaved, this will pop up the Save As dialog.		Save
SaveAs(,False)	This is for unsaved/new document only, and similar to the Document.Save but provide the full filename for unsaved document so no Save As dialog will pop up.	Don’t call this for a saved document, because this behaves different from the UI Save As function. The UI Save As will create a copy and then close the current open file and open the copied file, but the API won’t.	Save
SaveAs(,True)	Just save a copy of the document no matter the document is unsaved or saved.		Save Copy As