Manufacturing DevBlog

Checkout & CheckIn a file in Vault 2014

By Wayne Brill

There have been some questions about using the API to checkout, download and Check in a file. This example is an update to this Vault SDK sample:

C:\Program Files (x86)\Autodesk\Autodesk Vault 2014 SDK\VS10\VB\VaultList

It has two new buttons. One does the checkout and download and the other does the CheckIn. They both use a function that does a search for a file named "12345 Testing XXXX.csv". That function returns a FileIteration object.

Download Vault_List_wB

 

Use VB.NET dialog in iLogic

By Xiaodong Liang

The Form ability of iLogic is helpful in most cases. However, it is not so flexible to design the layout. And textbox does not support multi-lines (iProperties>>Comments cannot be shown) etc.

iLogic bases on VB.NET. Actually it can call native form of VB.NET. Following is the steps of a demo:

Download VBNetFormforiLogic

1) Create a VB.NET class library project. Add one form with single-line textbox to communicate with the parameter which is single value; a combo box for a parameter which is multi values; a multi-line textbox for iProperties>>Comments.

2) In Form_Load, assign the parameters values to the controls. In OK button, update the parameters values with the controls values.

PublicClassMyForm

 

    Public RailHeight AsDouble

    Public Material AsString

    Public Material_List AsArrayList

    Public Comments AsString

    PrivateSub MyForm_Load(sender As System.Object,
              e As System.EventArgs)
                      HandlesMyBase.Load

 

        'param which is single value

        TextBox1.Text = CStr(RailHeight)

        'param which is multi-values

        ForEach Material_val
               AsStringIn Material_List

            ComboBox1.Items.Add(Material_val)

        Next

        ComboBox1.Text = Material

        ' iProperties>>Comments which is multi lines

        TextBox3.Text = Comments

    EndSub

 

    PrivateSub OK_Button_Click(sender As 

                             System.Object,
                        e As System.EventArgs)
                         Handles OK_Button.Click

        RailHeight = CDbl(TextBox1.Text)

        Material = ComboBox1.Text

        Comments = TextBox3.Text

        Me.DialogResult =
                System.Windows.Forms.DialogResult.OK

        Me.Close()

    EndSub

 

    PrivateSub Cancel_Button_Click(sender As 

                                    System.Object, 
                       e As System.EventArgs)
                       Handles Cancel_Button.Click

        Me.DialogResult =
              System.Windows.Forms.DialogResult.Cancel

        Me.Close()

    EndSub

EndClass

3) In Inventor file, prepare the corresponding parameters.

 

 

4) Create a rule as below:

' add the reference of VB.NET dll. change the absolute path of your own

AddReference"C:\VBNetFormforiLogic\VBNetFormforiLogic\bin\Debug\VBNetFormforiLogic1.dll" 
SubMain()

localTrigger = iTrigger0

' create a form of VB.NET 
UsingdlgAsNewVBNetFormforiLogic.MyForm

' assign the param and property to the form

  dlg.RailHeight = Parameter("RailHeight")

    dlg.Material_List = MultiValue.List("Material")

  dlg.Material = Parameter("Material")  
  dlg.Comments = iProperties.Value("Summary", "Comments")

  'show the dialog

  DimiAsInteger = dlg.ShowDialog()

  'update the param and property from the form

  Ifi <> vbOK ThenReturn

     RailHeight =  dlg.RailHeight

     Material =  dlg.Material

     iProperties.Value("Summary", "Comments") = dlg.Comments

EndUsing

iLogicVb.UpdateWhenDone = True

End Sub

 

AddReference could also be relative to the path set in Tools Tab>>Advanced iLogic Configuration>>iLogic Addin Dlls Directory. You can put your dll in the directory and use relative path.

 

 

 

 

 

Constraint an Assembly Workplane with a ComponentOccurence Workplane?

By Augusto Goncalves

The AddFixed method creates a work plane at the specified position in space, but it is not grounded.  Placing a constraint on the work plane could cause it to move depending on what it is being constrained to and the behavior of the solver.  The fact that it is not grounded and still have six degrees of freedom available allows the solver to reposition it as needed.

As a workaround, please set oAssyPlane.Grounded = True before AddMateConstraint and set Grounded back to its original value.

The code below assumes two occurrences in one assembly. The coordinate system of the second occurrence is not aligned with the assembly’s.

Public Sub MateConstraintOfWorkPlanes()

 

  ' get the active component definition

  Dim oAsmCompDef As AssemblyComponentDefinition

  oAsmCompDef = m_inventorApplication. _

    ActiveDocument.ComponentDefinition

 

  ' get the workplane

  Dim oAssyPlane As WorkPlane

  Dim OPt As Point = Nothing

  Dim XV As UnitVector = Nothing

  Dim YV As UnitVector = Nothing

  oAsmCompDef.WorkPlanes(2). _

    GetPosition(OPt, XV, YV)

  ' and add fixed

  oAssyPlane = oAsmCompDef. _

    WorkPlanes.AddFixed(OPt, XV, YV)

 

  ' create geometry proxy

  Dim oOcc1 As ComponentOccurrence

  oOcc1 = oAsmCompDef.Occurrences(2)

  Dim oPartPlaneXZ As WorkPlane

  oPartPlaneXZ = oOcc1.Definition.WorkPlanes(2)

  Dim oPartPlane1 As WorkPlaneProxy = Nothing

  oOcc1.CreateGeometryProxy( _

    oPartPlaneXZ, oPartPlane1)

 

  ' and finally add the constraint

  Dim oldV As Boolean

  oldV = oAssyPlane.Grounded

  oAssyPlane.Grounded = True

  oAsmCompDef.Constraints.AddMateConstraint( _

    oPartPlane1, oAssyPlane, 0)

  oAssyPlane.Grounded = oldV

End Sub

Set Visibility of Sketch in sub assembly

By Adam Nagy

The following blog post talks about ComponentOccurrence contexts, which is relevant in this case as well: http://adndevblog.typepad.com/manufacturing/2012/12/componentoccurrence-contexts-and-reference-keys.html

If you want to set the visibility of an object that can only be reached through a ComponentDefinition (PartComponentDefinition/AssemblyComponentDefinition) object and it resides in a sub assembly, then you need to bring it into the context of the main/top assembly using CreateGeometryProxy. This is what the following code does as well. This will make the sketch highlighted in the picture (Sketch 2) invisible.

Sub HideSubAsmSketch()
    Dim dwg As DrawingDocument
    Set dwg = ThisApplication.ActiveDocument
    
    Dim baseView As DrawingView
    Set baseView = dwg.Sheets(1).DrawingViews(1)
    
    Dim mainAsm As AssemblyDocument
    Set mainAsm = _
      baseView.ReferencedDocumentDescriptor.ReferencedDocument
    
    Dim mainDef As AssemblyComponentDefinition
    Set mainDef = mainAsm.ComponentDefinition
    
    Dim subOcc As ComponentOccurrence
    Set subOcc = mainDef.Occurrences(1)
    
    Dim subDef As AssemblyComponentDefinition
    Set subDef = subOcc.Definition
    ' This does exactly the same as the below code. This
    ' way we'll get outside of the context of the main
    ' assembly and get inside the context of the sub assembly
    ' Set subDef = GetSubAsmDef()
    
    ' Anything we get through subDef will need to be
    ' brought into the context of mainAsm if
    ' that's where we want to set properties
    Dim sk As PlanarSketch
    Set sk = subDef.Sketches("Sketch 2")
    
    ' Let's bring sk into the mainAsm context through the
    ' occurrence object
    Dim skProxy As PlanarSketchProxy
    Call subOcc.CreateGeometryProxy(sk, skProxy)
    
    ' Now we can set the visibility for it
    Call baseView.SetVisibility(skProxy, False)
End Sub

Function GetSubAsmDef() As AssemblyComponentDefinition
  Dim asm As AssemblyDocument
  Set asm = ThisApplication.Documents.Open("SubAsm.iam")
  
  Set GetSubAsmDef = asm.ComponentDefinition
End Function

Create LeaderNote.FormattedText with Document Model properties

By Augusto Goncalves

I would like to set the FormattedText of the LeaderNote to something like:

"<Property Document='model' PropertySet='Design Tracking Properties' Property='Part Number' FormatID='{32853F0F-3444-11D1-9E93-0060B03C1CA6}' PropertyID='5'>PART NUMBER</Property>"

Is there a way to do this? Yes, the code below show a sample.

Sub CreateLN()

  If m_inventorApplication.Documents.Count = 0 Then Exit Sub

 

  If m_inventorApplication.ActiveDocument.DocumentType _

    <> DocumentTypeEnum.kDrawingDocumentObject Then Exit Sub

 

  Dim oDoc As DrawingDocument

  oDoc = m_inventorApplication.ActiveDocument

  Dim s As String

  s = "<Property Document='model' " _

    & "PropertySet='Design Tracking Properties' " _

    & "Property='Part Number' " _

    & "FormatID='{32853F0F-3444-11D1-9E93-0060B03C1CA6}' " _

    & "PropertyID='5'>PART NUMBER</Property>"

 

  ' Create a DrawingView on this Sheet and 

  ' the first DrawingCurve is line curve.

  Dim oGI As GeometryIntent

  oGI = oDoc.ActiveSheet.CreateGeometryIntent( _

    oDoc.ActiveSheet.DrawingViews(1). _

    DrawingCurves.Item(1), _

    PointIntentEnum.kStartPointIntent)

  Dim oObjCol As ObjectCollection

  oObjCol = m_inventorApplication.TransientObjects. _

    CreateObjectCollection

  oObjCol.Add(oGI)

 

  Dim oLN As LeaderNote

  oLN = oDoc.ActiveSheet.DrawingNotes. _

    LeaderNotes.Add(oObjCol, s)

End Sub

Use | “OR” with DefaultAcquisitionOption to Download & CheckOut with AcquireFiles

By Wayne Brill

The Vault 2014 API documentation does not explicitly describe how to  download and checkout a file using AcquireFiles. To do this you can "OR" together the AcquisitionOption enumeration Checkout and Download .

Here is an update to the downloadFile function in the VaultBrowser SDK sample that does a checkout and download.

 

private static void downloadFile

    (VDF.Vault.Currency.Connections.Connection

                                   connection,

    VDF.Vault.Currency.Entities.FileIteration

                                        file,

                           string folderPath)

{

    VDF.Vault.Settings.AcquireFilesSettings

        settings = new VDF.Vault.Settings.

           AcquireFilesSettings(connection);

 

    settings.AddEntityToAcquire(file);

 

    settings.DefaultAcquisitionOption =

     VDF.Vault.Settings.AcquireFilesSettings.

              AcquisitionOption.Checkout |

     VDF.Vault.Settings.AcquireFilesSettings.

                 AcquisitionOption.Download;

 

        settings.LocalPath =  new VDF.Currency.

        FolderPathAbsolute(folderPath);

 

    connection.FileManager.AcquireFiles(settings);

}

Create PDF C++ Example

By Wayne Brill

There is a VBA example that uses the PDF translator in the Inventor API help file. Here is an example in C++. You can  replace the code in the SimpleExe SDK example to test this code.  (At this location on my system)  

"C:\Users\Public\Documents\Autodesk\Inventor 2014\SDK\DeveloperTools\Samples\VC++\Standalone Applications\Inventor\SimpleExe"

It creates a pdf for each sheet and one PDF with all the sheets.

<code_begin>
// SimpleExe.cpp : Defines the entry point for the console application.

#include "stdafx.h"

// Forward declarations
static HRESULT PrintPDF();

// Main. Note that all COM related activity (including the automatic 'release' within smart
// pointers) MUST take place BEFORE CoUnitialize(). Hence the function 'block' within which
// the smart-pointers construct and destruct (and AddRef and Release) keeping the CoUnitialize
// safely out of the way.

int _tmain(int argc, _TCHAR* argv[])
{
HRESULT Result = NOERROR;

Result = CoInitialize (NULL);

if (SUCCEEDED(Result))
Result = PrintPDF();

CoUninitialize();

return 0;
}

static HRESULT PrintPDF()
{
HRESULT Result = NOERROR;

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"));
return Result;
}

CComPtr<Application> pInvApp;
Result = pInvAppUnk->QueryInterface (__uuidof(Application), (void **) &pInvApp);
if (FAILED(Result)) return Result;

CComPtr<Document> pDoc;
Result = pInvApp->get_ActiveDocument(&pDoc);
if (FAILED(Result)) return Result;

CComQIPtr<DrawingDocument> pDrawDoc = pDoc;

// Get the PDF translator Add-In.
CComPtr<ApplicationAddIns> pAddIns;
Result = pInvApp->get_ApplicationAddIns(&pAddIns);

CComPtr<ApplicationAddIn> pAddIn;
Result = pAddIns->get_ItemById(_bstr_t("{0AC6FD96-2F4D-42CE-8BE0-8AEA580399E4}"), &pAddIn);
 
CComQIPtr<TranslatorAddIn> pTransAddIn = pAddIn;

CComPtr<TransientObjects> pTransObjects;
Result = pInvApp->get_TransientObjects(&pTransObjects);

// Create the context.
CComPtr<TranslationContext> pContext;
Result = pTransObjects->CreateTranslationContext(&pContext);
Result = pContext->put_Type(kFileBrowseIOMechanism);

// Create a NameValueMap object
CComPtr<NameValueMap> pOptions;
Result = pTransObjects->CreateNameValueMap(&pOptions);

// Create a DataMedium object
CComPtr<DataMedium> pDataMedium;
Result = pTransObjects->CreateDataMedium(&pDataMedium);

// Check whether the translator has 'SaveCopyAs' options
VARIANT_BOOL hasOptions;
Result = pTransAddIn->get_HasSaveCopyAsOptions(pDrawDoc, pContext, pOptions, &hasOptions);
if (Result == S_OK)
{
CComPtr<Sheets>pSheets;
Result = pDrawDoc->get_Sheets(&pSheets);

long sheetCount;
Result = pSheets->get_Count(&sheetCount);

if (true)
{
for( int i=1; i<=sheetCount; ++i)
{
Result = pOptions->put_Value(_bstr_t("Vector_Resolution"), CComVariant(400));

Result = pOptions->put_Value(_bstr_t("Sheet_Range"), CComVariant(kPrintSheetRange));
Result = pOptions->put_Value(_bstr_t("Custom_Begin_Sheet"), CComVariant(i));
Result = pOptions->put_Value(_bstr_t("Custom_End_Sheet"), CComVariant(i));

//Set the destination file name
char filename[100];
sprintf_s(filename, "c:\\temp\\test%d.pdf", i);

pDataMedium->put_FileName(_bstr_t(filename));

// Publish document.
Result = pTransAddIn->SaveCopyAs(pDrawDoc, pContext, pOptions, pDataMedium);

}
  
Result = pOptions->put_Value(_bstr_t("Sheet_Range"), CComVariant(kPrintAllSheets));
Result = pOptions->put_Value(_bstr_t("Custom_Begin_Sheet"), CComVariant(1));
Result = pOptions->put_Value(_bstr_t("Custom_End_Sheet"), CComVariant(sheetCount));
pDataMedium->put_FileName(_bstr_t("c:\\temp\\testPDF_all_Sheets_in_one.pdf"));

// Publish document.
Result = pTransAddIn->SaveCopyAs(pDrawDoc, pContext, pOptions, pDataMedium);
}
else
{
Result = pOptions->put_Value(_bstr_t("Vector_Resolution"), CComVariant(400));
Result = pOptions->put_Value(_bstr_t("Sheet_Range"), CComVariant(kPrintSheetRange));
Result = pOptions->put_Value(_bstr_t("Custom_Begin_Sheet"), CComVariant(1));
Result = pOptions->put_Value(_bstr_t("Custom_End_Sheet"), CComVariant(sheetCount));
 
//Set the destination file name
char filename[500];
sprintf_s(filename, "c:\\temp\\testAll.pdf");

pDataMedium->put_FileName(_bstr_t(filename));

// Publish document.
Result = pTransAddIn->SaveCopyAs(pDrawDoc, pContext, pOptions, pDataMedium);
}
}

return Result;
}

<code_end>

Create simplified part by API

by Xiaodong Liang

The [Create Simplified Part] actually creates a derived assembly for the new part document. You will firstly create DerivedAssemblyDefinition, and configure the relevant options, finally add it to the new part by DerivedAssemblyComponents.Add.

 

The following is a small code demo. 

Sub CreateSimplifiedPart()

' Set a reference to the active assembly document
Dim oDoc As AssemblyDocument
Set oDoc = ThisApplication.ActiveDocument

Dim oDef As AssemblyComponentDefinition
Set oDef = oDoc.ComponentDefinition

' Create a new part document that will derive the assembly
Dim oPartDoc As PartDocument
Set oPartDoc = ThisApplication.Documents.Add(kPartDocumentObject, , True)

Dim oPartDef As PartComponentDefinition
Set oPartDef = oPartDoc.ComponentDefinition

Dim oDerivedAssemblyDef As DerivedAssemblyDefinition
Set oDerivedAssemblyDef = oPartDef.ReferenceComponents.DerivedAssemblyComponents.CreateDefinition(oDoc.FullDocumentName)

' Set various related options
oDerivedAssemblyDef.DeriveStyle = kDeriveAsSingleBodyNoSeams
oDerivedAssemblyDef.IncludeAllTopLevelWorkFeatures = kDerivedIncludeAll
oDerivedAssemblyDef.IncludeAllTopLevelSketches = kDerivedIncludeAll
oDerivedAssemblyDef.IncludeAllTopLeveliMateDefinitions = kDerivedExcludeAll
oDerivedAssemblyDef.IncludeAllTopLevelParameters = kDerivedExcludeAll
oDerivedAssemblyDef.ReducedMemoryMode = True
Call oDerivedAssemblyDef.SetHolePatchingOptions(kDerivedPatchAll)
Call oDerivedAssemblyDef.SetRemoveByVisibilityOptions(kDerivedRemovePartsAndFaces, 25)

' Create the shrinkwrap component
Dim oDerivedAssembly As DerivedAssemblyComponent
Set oDerivedAssembly = oPartDef.ReferenceComponents.DerivedAssemblyComponents.Add(oDerivedAssemblyDef)

 'save the new part file
Call oPartDoc.SaveAs("c:\temp\newpart.ipt", False)
  
End Sub

 

 

Why can I not convert linear Edges to Lines?

By Augusto Goncalves

Why can I not convert linear Edges to Lines? Perhaps the name is a bit misleading, but Line in Inventor API represents a straight line with infinite length. It only has a 'RootPoint' and a 'Direction'. In most scenarios, the LineSegment object can do the trick.

Dim oDoc As PartDocument

oDoc = m_inventorApplication.ActiveDocument

Dim oEdge As Edge

oEdge = oDoc.ComponentDefinition.SurfaceBodies(1).Faces(1).Edges(1)

Dim oLineSeg As LineSegment

If TypeOf oEdge.Geometry Is LineSegment Then

  oLineSeg = oEdge.Geometry

End If

Insert Content Center Part

By Adam Nagy

You can insert Content Center parts programmatically. The following sample is looking through the whole Content Center content in order to find a specific part based on its display name.

Public Function GetFamily( _
name As String, node As ContentTreeViewNode) _
As ContentFamily
  Dim cc As ContentCenter
  Set cc = ThisApplication.ContentCenter
    
  If node Is Nothing Then Set node = cc.TreeViewTopNode
  
  Dim cf As ContentFamily
  For Each cf In node.Families
    If cf.DisplayName = name Then
      Set GetFamily = cf
      Exit Function
    End If
  Next
  
  Dim child As ContentTreeViewNode
  For Each child In node.ChildNodes
    Set cf = GetFamily(name, child)
    If Not cf Is Nothing Then
      Set GetFamily = cf
      Exit Function
    End If
  Next
End Function

Public Sub CcTest()
   Dim asm As AssemblyDocument
   Set asm = ThisApplication.ActiveDocument
   
   Dim cf As ContentFamily
   Set cf = GetFamily("CCPart", Nothing)
   
   Dim member As String
   Dim ee As MemberManagerErrorsEnum
   member = cf.CreateMember(1, ee, "Problem")
   
   Dim tg As TransientGeometry
   Set tg = ThisApplication.TransientGeometry
   
   Call asm.ComponentDefinition.Occurrences.Add( _
    member, tg.CreateMatrix())
End Sub

The API Help File (C:\Users\Public\Documents\Autodesk\Inventor 2017\Local Help\admapi_21_0.chm) also contains a couple of samples concerning this topic:
- Place Content Center Parts API Sample
- Replace content center part API Sample