Manufacturing DevBlog

Manipulate rows and columns of iPart - 1

By Xiaodong Liang

API provides you to access the iPart table and its existing rows & columns & cells. The object collection of row is iPartTableRows, the object for columns is iPartTableColumns. API allows you delete the row or column by

iPartTableRow.Delete
iPartTableColumn.Delete

Note: The "Member" and "Part Number" columns cannot be deleted.

Following is small demo. It deletes the first row and the column named “param1”.

Sub DeleteIPartRowColumn()

    Dim oPartDoc As PartDocument
    Set oPartDoc = ThisApplication.ActiveDocument
    On Error Resume Next
    Dim oFactory As iPartFactory
    Set oFactory = oPartDoc.ComponentDefinition.iPartFactory
    'Get the iPartTable
    If Err > 0 Or oFactory Is Nothing Then
        MsgBox ("no iPart table!")
        Exit Sub
    End If
    If oFactory.TableRows.Count > 0 Then
      'delete the first row
       oFactory.TableRows(1).Delete
    End If
     If oFactory.TableColumns.Count > 0 Then
     ' Note :The "Member" and "Part Number" columns cannot be deleted.
      'delete the column "param1"
       Dim oEachCol As iPartTableColumn
       For Each oEachCol In oFactory.TableColumns
         If oEachCol.DisplayHeading = "param1" Then
            oEachCol.Delete
         End If
       Next
    End If

End Sub

But how to add rows or columns, and how to configure the rows/columns if we create a new iPart table by code?

Actually, every iPart table links to an Excel file. In UI, you can either add rows/columns by [Edit Table], or edit them by the Excel file.

e.g. Assume the iPart table has some rows and columns as below. One column (Author) is marked as custom column.

Close the table. Now edit the table via spreadsheet. You can see how the columns are defined in the spread sheet.

That is to say: The columns of iProperties are defined as
Property Name [Property Set Name]
The custom column is defined with the XML tag <free></free>
While the common parameters (d0. d1) are defined with their name directly.

Now, add one more column,

Save and close the spreadsheet, open the table again by [Edit Table] in UI, you can see the result:

So, we can edit the rows/columns by editing the spread sheet.

API allows you to access the corresponding spreadsheet: iPartFactory.ExcelWorkSheet

In this post, we firstly see how to configure the rows/columns if we create a new iPart table by code.

VBA
Please note to add reference to Mircrosoft Excel xx(version number,e.g.12) Object Library in this VB project

‘ this sample assumes the part has at least 4 model parameters.

Private Sub CreateNewiPartTable()

    Dim oPartDoc As PartDocument
    Set oPartDoc = ThisApplication.ActiveDocument
    On Error Resume Next
    Dim oFactory As iPartFactory
    Set oFactory = oPartDoc.ComponentDefinition.iPartFactory
    'Get the iPartTable
    If Err > 0 Or oFactory Is Nothing Then
    Set oFactory = oPartDoc.ComponentDefinition.CreateFactory
    Else
    Exit Sub
    End If
    On Error GoTo 0
    Dim oWorkSheet As WorkSheet
    Set oWorkSheet = oFactory.ExcelWorkSheet
    Dim oCells As Range
    Set oCells = oWorkSheet.Cells
    ' Column names...
    'Set the key for the iPartTable, here we use the key 'Part Number"
    With oCells
    .Item(1, 2) = oCells.Item(1, 2) + "0"
    .Item(1, 3) = oPartDoc.ComponentDefinition.Parameters.ModelParameters.Item(1).Name
    .Item(1, 4) = oPartDoc.ComponentDefinition.Parameters.ModelParameters.Item(2).Name
    .Item(1, 5) = oPartDoc.ComponentDefinition.Parameters.ModelParameters.Item(3).Name
    .Item(1, 6) = oPartDoc.ComponentDefinition.Parameters.ModelParameters.Item(4).Name
    End With
    Dim oUM As UnitsOfMeasure
    Set oUM = oPartDoc.UnitsOfMeasure
    Dim oParameter As Parameter
    Set oParameter = oPartDoc.ComponentDefinition.Parameters.ModelParameters.Item(1)
    'The first row is column name in excel table, the first ipart row is the second row in fact
    Dim iInitRow, i As Integer
    iInitRow = 2
    With oCells
        .Item(iInitRow, 3) = _
            oUM.GetStringFromValue( _
                oParameter.Value, oParameter.Units)
        Set oParameter = _
                oPartDoc.ComponentDefinition. _
                Parameters.ModelParameters.Item(2)
        .Item(iInitRow, 4) = _
                oUM.GetStringFromValue( _
                    oParameter.Value, oParameter.Units)
        Set oParameter = _
                oPartDoc.ComponentDefinition. _
                    Parameters.ModelParameters.Item(3)
        .Item(iInitRow, 5) = _
                oUM.GetStringFromValue( _
                    oParameter.Value, oParameter.Units)
        .Item(iInitRow, 6) = _
                oPartDoc.ComponentDefinition. _
                    Parameters.ModelParameters.Item(4).Expression
    End With
    'We need query the part number from iProperties of the part document.
    Dim sPartNumber As String
    sPartNumber = _
        oPartDoc.PropertySets.Item( _
            "{32853F0F-3444-11d1-9E93-0060B03C1CA6}"). _
                ItemByPropId(kPartNumberDesignTrackingProperties).Value
    Dim pos As Integer
    pos = InStrRev(sPartNumber, "-")
    Dim str As String
    str = Left(sPartNumber, pos)
    Dim iNumber As Integer
    iNumber = Right(sPartNumber, Len(sPartNumber) - pos)
    'Assume the offset of the parameter's value _
    ' (between two rows) is equal to 0.5cm
    Dim offset As Double
    offset = 0.5
    'Add 20 rows into the iPartTable
    For i = 1 To 20
        ' Row i values...
        If (iNumber + i) < 10 Then
            sPartNumber = _
                str + "0" + CStr(iNumber + i)
            Else
            sPartNumber = _
                str + CStr(iNumber + i)
        End If
        With oCells
            .Item(iInitRow + i, 1) = _
                sPartNumber
            .Item(iInitRow + i, 2) = _
                sPartNumber
            Set oParameter = _
                oPartDoc.ComponentDefinition. _
                    Parameters.ModelParameters.Item(1)
            .Item(iInitRow + i, 3) = _
                oUM.GetStringFromValue( _
                    oParameter.Value + offset * i, _
                        oParameter.Units)
            Set oParameter = _
                oPartDoc.ComponentDefinition.Parameters. _
                ModelParameters.Item(2)
            .Item(iInitRow + i, 4) = _
                oUM.GetStringFromValue( _
                oParameter.Value + offset * i, _
                oParameter.Units)
            Set oParameter = _
                oPartDoc.ComponentDefinition. _
                Parameters.ModelParameters.Item(3)
            .Item(iInitRow + i, 5) = _
                oUM.GetStringFromValue( _
                oParameter.Value + offset * i, oParameter.Units)
            .Item(iInitRow + i, 6) = _
                oPartDoc.ComponentDefinition. _
                Parameters.ModelParameters.Item(4).Expression
        End With
    Next
    Set oUM = Nothing
    Dim oWB As Workbook
    Set oWB = oWorkSheet.Parent
    oWB.Save
    oWB.Close
End Sub

VB.NET

remember to add the reference of Excel.

 

  Private Sub CreateNewiPartTable()

        Dim oPartDoc As PartDocument

        oPartDoc = ThisApplication.ActiveDocument

 

        Dim oFactory As iPartFactory

        'Get the iPartTable

        Try

            oFactory = oPartDoc.ComponentDefinition.iPartFactory

        Catch ex As Exception

            oFactory = oPartDoc.ComponentDefinition.CreateFactory

        End Try

 

        If oFactory Is Nothing Then

            Exit Sub

        End If

 

 

        Try

            Dim oWorkSheet As WorkSheet

            oWorkSheet = oFactory.ExcelWorkSheet

 

            Dim oCells As Range

            oCells = oWorkSheet.Cells

 

            ' Column names...

            'Set the key for the iPartTable, here we use the key 'Part Number"

            With oCells

                .Item(1, 2) = oCells.Item(1, 2) + "0"

                .Item(1, 3) = oPartDoc.ComponentDefinition.Parameters.ModelParameters.Item(1).Name

                .Item(1, 4) = oPartDoc.ComponentDefinition.Parameters.ModelParameters.Item(2).Name

                .Item(1, 5) = oPartDoc.ComponentDefinition.Parameters.ModelParameters.Item(3).Name

                .Item(1, 6) = oPartDoc.ComponentDefinition.Parameters.ModelParameters.Item(4).Name

            End With

 

            Dim oUM As UnitsOfMeasure

            oUM = oPartDoc.UnitsOfMeasure

 

            Dim oParameter As Parameter

            oParameter = oPartDoc.ComponentDefinition.Parameters.ModelParameters.Item(1)

 

            'The first row is column name in excel table, the first ipart row is the second row in fact

            Dim iInitRow, i As Integer

            iInitRow = 2

 

            With oCells

                .Item(iInitRow, 3) =

                    oUM.GetStringFromValue(oParameter.Value,

                                           oParameter.Units)

                oParameter =

                    oPartDoc.ComponentDefinition.

                        Parameters.ModelParameters.Item(2)

                .Item(iInitRow, 4) =

                    oUM.GetStringFromValue(oParameter.Value,

                                           oParameter.Units)

                oParameter =

                    oPartDoc.ComponentDefinition.

                    Parameters.ModelParameters.Item(3)

                .Item(iInitRow, 5) =

                    oUM.GetStringFromValue(

                        oParameter.Value, oParameter.Units)

                .Item(iInitRow, 6) =

                    oPartDoc.ComponentDefinition.

                    Parameters.ModelParameters.Item(4).Expression

            End With

 

            'We need query the part number from iProperties of the part document.

            Dim sPartNumber As String

            sPartNumber =

                oPartDoc.PropertySets.Item(

                    "{32853F0F-3444-11d1-9E93-0060B03C1CA6}").

                ItemByPropId(

                    PropertiesForDesignTrackingPropertiesEnum.

                        kPartNumberDesignTrackingProperties).Value

 

            Dim pos As Integer

            pos = InStrRev(sPartNumber, "-")

            Dim str As String

            str = sPartNumber.Substring(0, pos)

            Dim iNumber As Integer

            iNumber = sPartNumber.Substring(

                    sPartNumber.Length - pos, sPartNumber.Length)

 

            'Assume the offset of the parameter's value

            '(between two rows) is equal to 0.5cm

            Dim offset As Double

            offset = 0.5

 

            'Add 20 rows into the iPartTable

            For i = 1 To 20

                ' Row i values...

                If (iNumber + i) < 10 Then

                    sPartNumber = str + "0" + CStr(iNumber + i)

                Else

                    sPartNumber = str + CStr(iNumber + i)

                End If

 

                With oCells

                    .Item(iInitRow + i, 1) = sPartNumber

                    .Item(iInitRow + i, 2) = sPartNumber

 

                    oParameter =

                        oPartDoc.ComponentDefinition.Parameters.

                        ModelParameters.Item(1)

                    .Item(iInitRow + i, 3) =

                        oUM.GetStringFromValue(

                            oParameter.Value + offset * i,

                            oParameter.Units)

 

                    oParameter =

                        oPartDoc.ComponentDefinition.

                        Parameters.ModelParameters.Item(2)

                    .Item(iInitRow + i, 4) =

                        oUM.GetStringFromValue(

                            oParameter.Value + offset * i,

                            oParameter.Units)

 

                    oParameter =

                        oPartDoc.ComponentDefinition.Parameters.

                        ModelParameters.Item(3)

                    .Item(iInitRow + i, 5) =

                        oUM.GetStringFromValue(

                            oParameter.Value + offset * i,

                            oParameter.Units)

 

                    .Item(iInitRow + i, 6) =

                        oPartDoc.ComponentDefinition.Parameters.

                        ModelParameters.Item(4).Expression

                End With

            Next

 

            oUM = Nothing

 

            Dim oWB As WorkBook

            oWB = oWorkSheet.Parent

            oWB.Save()

            oWB.Close()

        Catch ex As Exception

 

        End Try

 

 

 

    End Sub

After the code , the result is:

Vault – use SetSystemACLs to set permissions on files

By Wayne Brill

The Vault API has several functions for setting security permissions on things in the Vault. The example on this blog post should be very helpful if you are trying to learn how to set permissions: Effective Permissions 2013

One thing that may not be obvious is that UpdateSystemACL() is not supported for files. Instead you can use SetSystemACL(). Here is an update to the VaultFileBrowser SDK C# sample that uses this function. (replaces FindButton_Click in FinderForm.cs). With this additional code a file that is found will have permissions set for it.

private void FindButton_Click

      (object sender, System.EventArgs e)

{

    //make sure search conditions

    //have been added

    if (m_criteriaListBox.Items.Count > 0)

    {

        //clear out previous search

        //results if they exist

      m_searchResultsListBox.Items.Clear();

 

      //build our array of SearchConditions

      // to use for the file search

        SrchCond[] conditions =

 new SrchCond[m_criteriaListBox.Items.Count];

 

        for (int i = 0; i <

         m_criteriaListBox.Items.Count; i++)

        {

         conditions[i] =((ListBoxSrchCondItem)

         m_criteriaListBox.Items[i]).SrchCond;

        }

 

        string bookmark = string.Empty;

        SrchStatus status = null;

 

   // added to existing SDK sample VaultFileBrowser

   // (around line #196 in FinderForm.cs file.

        try

        {

            File[] myFiles = m_serviceManager.

     DocumentService.FindFilesBySearchConditions

           (conditions, null, null, false, true,

                      ref bookmark, out status);

 

            Group group = m_serviceManager.

         AdminService.GetGroupByName("Everyone");

 

           // Could use this to get existing

           // permissions on the file

           // ACL[] acls = m_serviceManager.

           //   SecurityService.GetACLsByEntityIds

           //(new long[] { myFiles[0].MasterId });

           // ACE[] aces = acls[0].ACEArray;

 

            ACE ace = new ACE();

            ace.UserGrpId = group.Id;

 

            AccessPermis readAccessPermis =

                          new AccessPermis();

            readAccessPermis.Id = 1;

            readAccessPermis.Val = true;

 

            AccessPermis writeAccessPermis =

                         new AccessPermis();

            writeAccessPermis.Id = 2;

            writeAccessPermis.Val = true;

 

            AccessPermis deleteAccessPermis =

                         new AccessPermis();

            deleteAccessPermis.Id = 3;

            deleteAccessPermis.Val = true;

 

         ace.PermisArray = new AccessPermis[]

       { readAccessPermis, writeAccessPermis,

                       deleteAccessPermis };

 

         ACE[] aces = new ACE[1];

            aces[0] = ace;

 

            ACL myAcl = m_serviceManager.

          SecurityService.AddSystemACL(aces);

 

          m_serviceManager.SecurityService.

                  SetSystemACLs(new long[]

         { myFiles[0].MasterId }, myAcl.Id);

        }

        catch (Exception ex)

        {

            Debug.Print(ex.ToString());

 

        }

        // End Added for setting ACL

 

        //search for files

     List<File> fileList = new List<File>();

 

     while (status == null || fileList.Count

            < status.TotalHits)

        {

          File[] files = m_serviceManager.

                DocumentService.

            FindFilesBySearchConditions

      (conditions, null, null, true, true,

                ref bookmark, out status);

 

            if (files != null)

                fileList.AddRange(files);

        }

 

        if (fileList.Count > 0)

        {

            //iterate through found files

            //and display them in the search

            //results list box

            foreach (File file in fileList)

            {

                //create the list item that

                //will wrap the File

                ListBoxFileItem fileItem =

                 new ListBoxFileItem(file);

 

                m_searchResultsListBox.

                    Items.Add(fileItem);

            }

        }

 

        //update the items count label

        m_itemsCountLabel.Text =

            (fileList.Count > 0) ?

   fileList.Count + " Items" : "0 Items";

    }

}

Set Description property of McadAttributeField when using AddAttributeClass

By Wayne Brill

If you are using AddAttributeClass() an error: “Generic failure to execute operation with the provided arguments” occurs if the description property is not set for the McadAttributeField objects that are added to the McadAttributeFields collection that is passed into AddAttributeClass().

The documentation does not state that the Description property has to be set when AddAttributeClass() is called. Here is an excerpt from the AutoCAD Mechanical ActiveX and VBA reference: 

IMcadAttributeField::Description Property

Remarks
This property is a String.
Setting or changing the field description only has an effect when the McadAttributeField is used to define an attribute class.

Here is a VB.NET example that avoids the error:

  <CommandMethod("AttTest")> _

    Public Sub McadAttTest()

        Dim acadApp As AcadApplication =

            Autodesk.AutoCAD.ApplicationServices.

                      Application.AcadApplication

 

        Dim AcadMApp As AcadmAuto.AcadmApplication

        AcadMApp = acadApp.GetInterfaceObject _

                   ("AcadmAuto.AcadmApplication.2")

 

        Dim mcadUtil As McadUtility =

                   AcadMApp.ActiveDocument.Utility

 

        Dim attFields As McadAttributeFields =

                       mcadUtil.CreateCollection _

            (McadCollectionType.mcAttributeFields)

 

        Dim attField As McadAttributeField =

                   mcadUtil.CreateAttributeField()

 

        attField.Name = "InnerDiameter"

        attField.FieldType = McadFieldType.mcDouble

        ' If this is not set an error occurs

        ' when AddAttributeClass() is called

        attField.Description = "Some description"

 

        attFields.Add(attField)

 

        AcadMApp.AddAttributeClass _

                  ("myAttributeClass", attFields)

 

    End Sub

Pick a point

By Adam Nagy

If you'd like to pick a point in the model then you can use the InteractionEvents.MouseEvents.OnMouseMove/OnMouseClick events. In these the ModelPosition parameter will give you a 3d point in the Target plane of the camera based on the mouse location. However, you may want to get back a point on the face under the cursor. In that case you could use the FindUsingRay/FindUsingVector functions.

I extended the sample code from Brian Ekins, which was for picking 2d points in a drawing, with the function that can transform the point from the Target plane onto the face. Since the Target plane could even be beyond the face that logically the point should be picked on, therefore first we'll transform the ModelPosition to the Screen plane, and then use that along with the view direction vector inside the FindUsingRay function to get back the face and the intersection point.

Here is the class that provides the functionality:

Option Explicit

' Declare the event objects
Private WithEvents oInteractEvents As InteractionEvents
Private WithEvents oMouseEvents As MouseEvents

' Declare a flag that's used to determine when selection stops.
Private bStillSelecting As Boolean
Private modelPoint As Point

Public Function GetPoint() As Point
    ' Initialize flag.
    bStillSelecting = True

    ' Create an InteractionEvents object.
    Set oInteractEvents = _
        ThisApplication.CommandManager.CreateInteractionEvents

    ' Ensure interaction is enabled.
    oInteractEvents.InteractionDisabled = False

    ' Set a reference to the mouse events.
    Set oMouseEvents = oInteractEvents.MouseEvents

    oMouseEvents.MouseMoveEnabled = True

    ' Start the InteractionEvents object.
    oInteractEvents.Start

    ' Loop until a (3D) point in the model is selected.
    Do While bStillSelecting
        DoEvents
    Loop

    ' Stop the InteractionEvents object.
    oInteractEvents.Stop

    ' Clean up.
    Set oMouseEvents = Nothing
    Set oInteractEvents = Nothing
    
    Set GetPoint = modelPoint
End Function

Private Sub oInteractEvents_OnTerminate()
    ' Set the flag to indicate we're done.
    bStillSelecting = False
End Sub

Private Function MovePtToFace(pt As Point, v As View) As Point
    ' Get the view direction, i.e. the vector pointing
    ' from the Eye to the Target
    Dim e2t As Vector
    Set e2t = v.Camera.eye.VectorTo(v.Camera.Target)
    
    ' The vector that will take the Model Point from the
    ' Target plane to the Screen plane is the opposite of e2t
    Dim m2s As Vector
    Set m2s = e2t.Copy
    m2s.ScaleBy (-1)
    Call pt.TranslateBy(m2s)
    
    Dim doc As PartDocument
    Set doc = v.Document
    
    ' Now we can shoot a ray from the Screen plane
    ' towards the model along the view direction to
    ' find the first object it hits and the intersection point
    Dim objects As ObjectsEnumerator
    Dim pts As ObjectsEnumerator
    Call doc.ComponentDefinition.FindUsingRay( _
        pt, e2t.AsUnitVector(), _
        0.001, objects, pts)
    
    If pts.Count > 0 Then
        Set MovePtToFace = pts(1)
    End If
End Function

Private Sub oMouseEvents_OnMouseClick( _
ByVal Button As MouseButtonEnum, _
ByVal ShiftKeys As ShiftStateEnum, _
ByVal ModelPosition As Point, _
ByVal ViewPosition As Point2d, _
ByVal View As View)
    bStillSelecting = False
    
    ' ModelPosition will be on the Target Plane
    ' which is a plane parallel to the screen's plane
    ' but instead of including the Camera.Eye position
    ' this includes the Camera.Target position
      
    Set modelPoint = MovePtToFace(ModelPosition, View)
End Sub

Private Sub oMouseEvents_OnMouseMove( _
ByVal Button As MouseButtonEnum, _
ByVal ShiftKeys As ShiftStateEnum, _
ByVal ModelPosition As Point, _
ByVal ViewPosition As Point2d, _
ByVal View As View)
    Dim newPos As Point
    Set newPos = MovePtToFace(ModelPosition, View)
    
    If Not newPos Is Nothing Then Set ModelPosition = newPos

    ThisApplication.StatusBarText = _
        ModelPosition.x & " : " & _
        ModelPosition.y & " : " & _
        ModelPosition.z
End Sub

And here is the code that is using the above class:

Sub Get3dPoint()
    Dim oSelectedPoint As New clsGetPoint
    Dim modelPoint As Point
    Set modelPoint = oSelectedPoint.GetPoint
    
    If Not modelPoint Is Nothing Then
        Dim doc As PartDocument
        Set doc = ThisApplication.ActiveDocument
    
        Call doc.ComponentDefinition.WorkPoints.AddFixed(modelPoint)
    End If
End Sub

Here is a picture of the tests I've done with the code, which places work points at the picked positions

Get Edge direction

By Adam Nagy

If you need to get the direction of an Edge on a given Face in a consistent manner, then you need to use the EdgeUse object. The Evaluator of this object will retrieve information in the parametric space of the Face in a way that when the normal of the Face is pointing towards you then the outer loop's edges will go anti-clockwise, whereas the internal edges around the holes will go clockwise.

You can take advantage of the EdgeUse object in two ways:

1. Use the EdgeUse.Evaluator to return information in the parametric space of the Face and then translate that information to model space if needed - e.g. in case of a point you could use Face.GetPointAtParam()
2. And/Or use the EdgeUse.Edge.Evaluator to return information in the model space and remember that its parameters are reversed compared to the EdgeUse if EdgeUse.IsOpposedToEdge = True

In the following VBA sample I'll use the latter. This code iterates through all the EdgeLoop's and Edge's of the selected Face and places UserCoordinateSystem objects at the middle of each of them in a way that X is showing the topological direction of the Edge in context of the selected Face, Z is the same as the Face's normal vector, and so Y is pointing towards the inside of the Face.

Function GetMidParam(oEval As CurveEvaluator) As Double
    Dim min As Double
    Dim max As Double
    Call oEval.GetParamExtents(min, max)
    
    ' Since we just want the middle point, we do not
    ' have to consider EdgeUse.IsOpposedToEdge
    GetMidParam = min + (max - min) / 2
End Function

Function GetPointAtParam(oEdgeUse As EdgeUse, p As Double) As Point
    ' The EdgeUse geometry is in the parametric space of the face
    ' whereas EdgeUse.Edge geometry is in model space
    Dim oEval As CurveEvaluator
    Set oEval = oEdgeUse.Edge.evaluator
    
    Dim param(0) As Double
    Dim pt(2) As Double
    param(0) = p
    Call oEval.GetPointAtParam(param, pt)
    
    Dim oTG As TransientGeometry
    Set oTG = ThisApplication.TransientGeometry
    
    Set GetPointAtParam = oTG.CreatePoint(pt(0), pt(1), pt(2))
End Function

Function GetTangentAtParam(oEdgeUse As EdgeUse, p As Double) _
As UnitVector
    ' The EdgeUse geometry is in the parametric space of the face
    ' whereas EdgeUse.Edge geometry is in model space
    Dim oEval As CurveEvaluator
    Set oEval = oEdgeUse.Edge.evaluator

    Dim param(0) As Double
    Dim v(2) As Double
    param(0) = p
    Call oEval.GetTangent(param, v)
    
    Dim oTG As TransientGeometry
    Set oTG = ThisApplication.TransientGeometry
    
    ' If the edge is not following the direction around the face
    ' then the direction is opposite
    If oEdgeUse.IsOpposedToEdge Then
        Set GetTangentAtParam = _
            oTG.CreateUnitVector(-v(0), -v(1), -v(2))
    Else
        Set GetTangentAtParam = _
            oTG.CreateUnitVector(v(0), v(1), v(2))
    End If
End Function

Function GetFaceNormal(oFace As Face, oPoint As Point) As UnitVector
    Dim pt(2) As Double
    Dim n(2) As Double
    
    pt(0) = oPoint.x: pt(1) = oPoint.y: pt(2) = oPoint.z
    Call oFace.evaluator.GetNormalAtPoint(pt, n)
    
    Dim oTG As TransientGeometry
    Set oTG = ThisApplication.TransientGeometry
    
    Set GetFaceNormal = oTG.CreateUnitVector(n(0), n(1), n(2))
End Function

Sub CreateUcs(oEdgeUse As EdgeUse, doc As PartDocument)
    Dim oEdge As Edge
    Set oEdge = oEdgeUse.Edge
    
    Dim mid As Double
    mid = GetMidParam(oEdgeUse.Edge.evaluator)
   
    Dim mp As Point
    Set mp = GetPointAtParam(oEdgeUse, mid)
    
    Dim x As UnitVector
    Set x = GetTangentAtParam(oEdgeUse, mid)
    
    Dim z As UnitVector
    Set z = GetFaceNormal(oEdgeUse.EdgeLoop.Face, mp)
    
    Dim y As UnitVector
    Set y = z.CrossProduct(x)
    
    Dim oUCSS As UserCoordinateSystems
    Set oUCSS = doc.ComponentDefinition.UserCoordinateSystems
    
    Dim oUCSD As UserCoordinateSystemDefinition
    Set oUCSD = oUCSS.CreateDefinition
    
    Dim mx As Matrix
    Set mx = ThisApplication.TransientGeometry.CreateMatrix
    Call mx.SetCoordinateSystem(mp, _
        x.AsVector(), y.AsVector(), z.AsVector())
    
    oUCSD.Transformation = mx
    
    Dim oUCS As UserCoordinateSystem
    Set oUCS = oUCSS.Add(oUCSD)
    
    oUCS.XAxis.Visible = False
    oUCS.YAxis.Visible = False
    oUCS.ZAxis.Visible = False
    oUCS.XYPlane.Visible = False
    oUCS.XZPlane.Visible = False
    oUCS.YZPlane.Visible = False
    oUCS.Origin.Visible = False
End Sub

Sub ShowEdgeDirections()
    Dim doc As PartDocument
    Set doc = ThisApplication.ActiveDocument

    Dim oFace As Face
    Set oFace = doc.SelectSet(1)
    
    Dim oEdgeLoop As EdgeLoop
    For Each oEdgeLoop In oFace.EdgeLoops
        Dim oEdgeUse As EdgeUse
        For Each oEdgeUse In oEdgeLoop.EdgeUses
            Call CreateUcs(oEdgeUse, doc)
        Next
    Next
End Sub

Intercept click event on a ribbon tab

By Xiaodong Liang
We got a question on the forum. The customer has a custom ribbon tab on the Assembly and ZeroDoc ribbons, those have panels and buttons.The custom buttons have OnExecute event that can have custom actions added. But Inventor API does not provide the ability to intercept the event when user is clicking on the ribbon tab.

Currently all Autodesk products use the same core of ribbon (AIR Look), which provides some underlying API to get access to that notification. You would need to reference the AdWindows.dll in order to use that code. AdWindows.dll  can be found at <Inventor Installation Path>\bin

The following is the code snippet of a plugin.

using Autodesk.Windows;

       public void Activate(Inventor.ApplicationAddInSite addInSiteObject, bool firstTime)

        {

    // Initialize AddIn members.

            m_inventorApplication = addInSiteObject.Application;

 

            

//delegate the event when the ribbon is initialized

            Autodesk.Windows.ComponentManager.ItemInitialized +=

                new EventHandler<RibbonItemEventArgs>(

                    ComponentManager_ItemInitialized);

        }

 

//delegate the tab event when the ribbon is initialized

        void ComponentManager_ItemInitialized(object sender, RibbonItemEventArgs e)

        {

            //now one Ribbon item is initialized, but the Ribbon control

//may not be available yet, so check before

            if (Autodesk.Windows.ComponentManager.Ribbon != null)

           {

                foreach (Autodesk.Windows.RibbonTab Tab in Autodesk.Windows.ComponentManager.Ribbon.Tabs)

                {

                    if (Tab.Id == "id_TabTools")

                   {

                        Tab.Activated += new EventHandler(Tab_Activated);

                    }

                }

 

                //and remove the event handler

Autodesk.Windows.ComponentManager.ItemInitialized -=

new EventHandler<RibbonItemEventArgs>(ComponentManager_ItemInitialized);

            }

        }

 

        // when the tab is activated

        void Tab_Activated(object sender, EventArgs e)

        {

            System.Windows.Forms.MessageBox.Show(

                "Tab " + ComponentManager.Ribbon.ActiveTab.Id + " Activated!");

        }

Replace Object Defaults Style

By Adam Nagy

In the Style and Standard Editor dialog you can do a Replace Style on an Object Defaults Style. This will go through all the standards and check if any of them uses the selected style as the Active Object Defaults. If so, then it will activate the other Object Defaults Style that you provide in the Replace Style dialog. Once it's not used anywhere you may as well purge it / delete it.

You can achieve the above using the API as well.

VBA

Sub ReplaceObjectDefaultsStyle( _
    ByVal stylesMgr As DrawingStylesManager, _
    ByVal replaceStyle As ObjectDefaultsStyle, _
    ByVal withStyle As ObjectDefaultsStyle, _
    purge As Boolean)
    
    ' Go through each standard and replace the
    ' Active Defaults with withStyle if currently
    ' replaceStyle is being used as Active Defaults
    
    Dim oDwgStd As DrawingStandardStyle
    For Each oDwgStd In stylesMgr.StandardStyles
        If oDwgStd.ActiveObjectDefaults Is replaceStyle Then
            oDwgStd.ActiveObjectDefaults = withStyle
        End If
    Next
    
    ' If it is (or is also) local then we can delete it
    ' i.e. not library only
    
    If purge And replaceStyle.StyleLocation <> kLibraryStyleLocation _
    Then
        replaceStyle.Delete
    End If
    
End Sub

Sub TestReplace()

    Dim oDwg As DrawingDocument
    Set oDwg = ThisApplication.ActiveDocument
    
    Dim oStlMgr As DrawingStylesManager
    Set oStlMgr = oDwg.StylesManager
    
    ' The style we want to replace
    Dim oDefStyle1 As ObjectDefaultsStyle
    Set oDefStyle1 = oStlMgr.ObjectDefaultsStyles(3)
    
    ' The style we want to replace the active style with
    Dim oDefStyle2 As ObjectDefaultsStyle
    Set oDefStyle2 = oStlMgr.ObjectDefaultsStyles(1)
    
    ReplaceObjectDefaultsStyle oStlMgr, oDefStyle1, oDefStyle2, True

End Sub

C#

static void ReplaceObjectDefaultsStyle(

  DrawingStylesManager stylesManager,

  ObjectDefaultsStyle replaceStyle,

  ObjectDefaultsStyle withStyle,

  bool purge)

{

  foreach (DrawingStandardStyle standardStyle

    in stylesManager.StandardStyles)

  {

    if (standardStyle.ActiveObjectDefaults == replaceStyle)

      standardStyle.ActiveObjectDefaults = withStyle;

  }

 

  if (purge && replaceStyle.StyleLocation !=

    StyleLocationEnum.kLibraryStyleLocation)

    replaceStyle.Delete();

}

 

static private void test()

{

  Application app = (Application)

    System.Runtime.InteropServices.Marshal.

    GetActiveObject("Inventor.Application");

 

  DrawingDocument dwg = (DrawingDocument)app.ActiveDocument;

  DrawingStylesManager stylesManager = dwg.StylesManager;

  ObjectDefaultsStyle style1 = stylesManager.ObjectDefaultsStyles[1];

  ObjectDefaultsStyle style2 = stylesManager.ObjectDefaultsStyles[2];

  ReplaceObjectDefaultsStyle(stylesManager, style1, style2, true);

}

 

And you could also do it from an iLogic Rule - see Convert VBA to .NET / iLogic

Sub Main()
    Dim oDwg As DrawingDocument
    oDwg = ThisApplication.ActiveDocument
    
    Dim oStlMgr As DrawingStylesManager
    oStlMgr = oDwg.StylesManager
    
    ' The style we want to replace
    Dim oDefStyle1 As ObjectDefaultsStyle
    oDefStyle1 = oStlMgr.ObjectDefaultsStyles(3)
    
    ' The style we want to replace the active style with
    Dim oDefStyle2 As ObjectDefaultsStyle
    oDefStyle2 = oStlMgr.ObjectDefaultsStyles(1)
    
    ReplaceObjectDefaultsStyle(oStlMgr, oDefStyle1, oDefStyle2, True)
End Sub

Sub ReplaceObjectDefaultsStyle(
    stylesMgr As DrawingStylesManager, 
    replaceStyle As ObjectDefaultsStyle, 
    withStyle As ObjectDefaultsStyle, 
    purge As Boolean)
    
    ' Go through each standard and replace the
    ' Active Defaults with withStyle if currently
    ' replaceStyle is being used as Active Defaults
    
    Dim oDwgStd As DrawingStandardStyle
    For Each oDwgStd In stylesMgr.StandardStyles
        If oDwgStd.ActiveObjectDefaults Is replaceStyle Then
            oDwgStd.ActiveObjectDefaults = withStyle
        End If
    Next
    
    ' If it is (or is also) local then we can delete it
    ' i.e. not library only
    
    If purge And replaceStyle.StyleLocation <> kLibraryStyleLocation _
    Then
        replaceStyle.Delete
    End If
End Sub

Get ActiveX/COM class properties and methods from .NET

By Adam Nagy

If you are using the COM interface of e.g. AutoCAD or Inventor from a .NET AddIn or application and you want to be able to find out what properties and methods are available for the object, then here is a nice post which shows excactly that. It works even if your project is not referencing the relevant type library/interop assembly and so you are using late binding:
Obtain Type Information of IDispatch-Based COM Objects from Managed Code

I tested it with both Inventor and AutoCAD and it seemed to work fine - I got back all the items shown under Dynamic View inside the Watch window:

 

Calling translator add-in from external application C++

By Adam Nagy

This is the C++ version of this blog post: http://adndevblog.typepad.com/manufacturing/2013/01/calling-translator-add-in-from-external-application.html

static HRESULT SaveToIges()

{

  HRESULT Result = NOERROR;

 

  // Access Inventor

 

  CLSID InvAppClsid;

  Result = CLSIDFromProgID (L"Inventor.Application", &InvAppClsid);

  if (FAILED(Result)) return Result;

 

  CComPtr<IUnknown> pInvAppUnk;

  Result = ::GetActiveObject (InvAppClsid, NULL, &pInvAppUnk);

  if (FAILED (Result))

    _tprintf_s(_T("*** Could not get hold of an active Inventor application ***\n"));

  if (FAILED(Result)) return Result;

 

  CComPtr<Application> pInvApp;

  Result = pInvAppUnk->QueryInterface(

    __uuidof(Application), (void **) &pInvApp);

  if (FAILED(Result)) return Result;

 

  // Get current document

 

  CComPtr<Document> pDoc;

  pInvApp->get_ActiveDocument(&pDoc);

 

  // Find the translator addin

 

  CComPtr<ApplicationAddIns> pAddIns;

  pInvApp->get_ApplicationAddIns(&pAddIns);

 

  CComPtr<TranslatorAddIn> pAddIn;

  pAddIns->get_ItemById(

    _bstr_t("{90AF7F44-0C01-11D5-8E83-0010B541CD80}"),

    (ApplicationAddIn**)&pAddIn);

 

  if (pAddIn == NULL)

  {

    _tprintf_s(_T("*** Could not find the translator addin ***\n"));

    return E_FAIL;

  }

 

  // Set it up

 

  CComPtr<TransientObjects> pTr;

  pInvApp->get_TransientObjects(&pTr);

 

  CComPtr<TranslationContext> pContext;

  pTr->CreateTranslationContext(&pContext);

  pContext->put_Type(IOMechanismEnum::kFileBrowseIOMechanism);

 

  CComPtr<DataMedium> pMedium;

  pTr->CreateDataMedium(&pMedium);

  pMedium->put_FileName(_bstr_t("c:\\temp\\file.igs"));

 

  CComPtr<NameValueMap> pOptions;

  pTr->CreateNameValueMap(&pOptions);

 

  VARIANT_BOOL hasOptions;

  pAddIn->get_HasSaveCopyAsOptions(

    pDoc, pContext, pOptions, &hasOptions);

  if (hasOptions == VARIANT_TRUE)

  {

    CComVariant num1(1, VT_I4);

    pOptions->put_Value(_bstr_t("GeometryType"), num1);

    CComVariant num0(0, VT_I4);

    pOptions->put_Value(_bstr_t("SolidFaceType"), num0);

    pOptions->put_Value(_bstr_t("SurfaceType"), num0);

  }

 

  pAddIn->SaveCopyAs(pDoc, pContext, pOptions, pMedium);

 

  return Result;

}

 

int _tmain(int argc, _TCHAR* argv[])

{

  HRESULT Result = NOERROR;

 

  Result = CoInitialize (NULL);

 

  if (SUCCEEDED(Result))

    Result = SaveToIges();

 

  CoUninitialize();

 

  return 0;

}

 

Detecting Tab Activated Event in the Ribbon

By Philippe Leefsma

I was recently working on an ADN case where the developer wanted to react to his custom tab being activated. The Inventor Ribbon API itself doesn’t provide this kind of notification, however the underlying Ribbon API does.

You need to add a reference to AdWindows.dll (located in Inventor Bin install folder) to your .Net project in order to compile that code:

//Your Add-In activate method, for example

public void Activate(

    ApplicationAddInSite addInSiteObject,

    bool firstTime)

{

   

    Autodesk.Windows.ComponentManager.ItemInitialized

+= new EventHandler<RibbonItemEventArgs>(

            ComponentManager_ItemInitialized);

}

 

void ComponentManager_ItemInitialized(

    object sender,

    RibbonItemEventArgs e)

{

    // Now one Ribbon item is initialized,

    // but the Ribbon control may not be available 

    // yet, so check before

    if (Autodesk.Windows.ComponentManager.Ribbon

        != null)

    {

        foreach (Autodesk.Windows.RibbonTab Tab

            in

        Autodesk.Windows.ComponentManager.Ribbon.Tabs)

        {

            // Replace with the id of the target tab

            if (Tab.Id == "id_TabTools")

            {

                Tab.Activated +=

                    new EventHandler(Tab_Activated);

            }

        }

 

        //and remove the event handler

        Autodesk.Windows.ComponentManager.

        ItemInitialized –=

            new EventHandler<RibbonItemEventArgs>

               (ComponentManager_ItemInitialized);

    }

}

 

void Tab_Activated(object sender, EventArgs e)

{

    System.Windows.Forms.MessageBox.Show(

        "Tab " + ComponentManager.Ribbon.ActiveTab.Id

        + " Activated!");

}