Place & Constrain to Origin Macro

Anonymous · ‎03-24-2014

Can anyone please send me the vba code to select a part file from a file dialog & then automatically place & constrain to the origin. I currently have a macro that uses commondialog but this doesnt seem to be supported with Inventor 2014.

xiaodong_liang · ‎03-30-2014

Hi,

I'd suggest you post your code for the peers in forum to diagnose why it failed in 2014.

I still wrote a small code which creates a file dialog and asks user to select a file, next places it to the active assembly. it works well in Inventor 2014.

Sub selectPartAndPlace()

    'assume an assembly is opened
     Dim oAssDoc As AssemblyDocument
     Set oAssDoc = ThisApplication.ActiveDocument
        
    ' Create a new FileDialog object.
    Dim oFileDlg As FileDialog
    Call ThisApplication.CreateFileDialog(oFileDlg)

    ' Define the filter to select part and assembly files or any file.
    oFileDlg.Filter = "Inventor Files (*.iam;*.ipt)|*.iam;*.ipt|All Files (*.*)|*.*"

    ' Define the part and assembly files filter to be the default filter.
    oFileDlg.FilterIndex = 1

    ' Set the title for the dialog.
    oFileDlg.DialogTitle = "Open File Test"

    ' Set the initial directory that will be displayed in the dialog.
    oFileDlg.InitialDirectory = "C:\Temp"

    ' Set the flag so an error will be raised if the user clicks the Cancel button.
    oFileDlg.CancelError = True

    ' Show the open dialog.  The same procedure is also used for the Save dialog.
    ' The commented code can be used for the Save dialog.
    On Error Resume Next
    oFileDlg.ShowOpen
'    oFileDlg.ShowSave

    ' If an error was raised, the user clicked cancel, otherwise display the filename.
    If Err Then
        MsgBox "User cancelled out of dialog"
    ElseIf oFileDlg.FileName <> "" Then
        'MsgBox "File " & oFileDlg.FileName & " was selected."
        
        Dim oAssDef As AssemblyComponentDefinition
        Set oAssDef = oAssDoc.ComponentDefinition
        
        Dim oM As Matrix
        Set oM = ThisApplication.TransientGeometry.CreateMatrix()
        
        Dim oNewOcc As ComponentOccurrence
        Set oNewOcc = oAssDef.Occurrences.Add(oFileDlg.FileName, oM)
        
        'if you need to ground it
        'oNewOcc.Grounded = True
        
    End If


End Sub

Anonymous · ‎03-30-2014

Thanks for the code, it works well.

Regards, Peter.

Anonymous · ‎11-25-2014

How can i use this code, but instead of grounding create 3 other constraint?

Assembly Y-axis Mate Sub-assembly Y-axis

Assembly XZ-plane Flush Sub-assembly XZ-axis

Assembly XY-plane 2-angle Sub-assembly XY-axis

This is a constraint that i use very often when placing new parts on a tank so it would be easy if it could be done with placing 🙂

Anonymous · ‎11-25-2014

I am using this code (similar to the one above, but without dialogbox and grounding is default off)

I'm not taking credit for this, I found the code here on the forum, but I slightly modifyed it to suit my needs. 🙂

I created a custom button to run this script...nice and effective 🙂

'get file to place
Dim oFileDlg As inventor.FileDialog = Nothing
InventorVb.Application.CreateFileDialog(oFileDlg)
oFileDlg.Filter = "Inventor Files (*.iam;*.ipt)|*.iam;*.ipt|All Files (*.*)|*.*"
oFileDlg.DialogTitle = "Select a File"
oFileDlg.InitialDirectory = ThisDoc.Path
oFileDlg.CancelError = True
On Error Resume Next
oFileDlg.ShowOpen()
If Err.Number <> 0 Then
MessageBox.Show("File not chosen.", "Dialog Cancellation")
Return
ElseIf oFileDlg.FileName <> "" Then
oFile = oFileDlg.FileName
End If

' set a reference to the assembly component definintion.
' This assumes an assembly document is open.
Dim oAsmCompDef As AssemblyComponentDefinition
oAsmCompDef = ThisApplication.ActiveDocument.ComponentDefinition

' Set a reference to the transient geometry object.
Dim oTG As TransientGeometry
oTG = ThisApplication.TransientGeometry
    
' Create a matrix.  
Dim oMatrix As Matrix
oMatrix = oTG.CreateMatrix

'place an instance of the component 
Dim oOccurrence As ComponentOccurrence
oOccurrence = oAsmCompDef.Occurrences.Add(oPath & oFile, oMatrix) 
' Set the translation portion of the matrix so the part will be 
'positioned at the co-ordinates
oMatrix.SetTranslation(oTG.CreateVector(0, 0, 0)) 

 'Iterate through all of the occurrences and ground them.
For Each oOccurrence In oAsmCompDef.Occurrences
'check for and skip virtual components
If Not TypeOf oOccurrence.Definition Is VirtualComponentDefinition Then
oOccurrence.Grounded = False
Else
End If
Next

'Get the plane from the selected part.
' The work plane obtained is in the context of the part, not the assembly.
Dim oPartPlane1 As WorkPlane
Dim oPartPlane2 As WorkPlane
Dim oPartPlane3 As WorkPlane
 oPartPlane1 =  oOccurrence.Definition.WorkPlanes.Item(1) 'Component YZ Plane
 oPartPlane2 =  oOccurrence.Definition.WorkPlanes.Item(2) 'Component XZ Plane
 oPartPlane3 =  oOccurrence.Definition.WorkPlanes.Item(3) 'Component XY Plane

 'Get the plane from the assembly
Dim oAsmPlane1 As WorkPlane
Dim oAsmPlane2 As WorkPlane
Dim oAsmPlane3 As WorkPlane
 oAsmPlane1 = oAsmCompDef.WorkPlanes.Item(1) 'Assembly YZ Plane
 oAsmPlane2 = oAsmCompDef.WorkPlanes.Item(2) 'Assembly XZ Plane
 oAsmPlane3 = oAsmCompDef.WorkPlanes.Item(3) 'Assembly XY Plane

' Create proxies for the work planes of the part.
' The proxies represent the part work planes in the context of the assembly.
Dim oAsmPlane4 As WorkPlaneProxy
Dim oAsmPlane5 As WorkPlaneProxy
Dim oAsmPlane6 As WorkPlaneProxy
oOccurrence.CreateGeometryProxy(oPartPlane1, oAsmPlane4)
oOccurrence.CreateGeometryProxy(oPartPlane2, oAsmPlane5)
oOccurrence.CreateGeometryProxy(oPartPlane3, oAsmPlane6)

' Create the constraint using the part work plane proxies.
oConstraint = oAsmCompDef.Constraints.AddFlushConstraint(oAsmPlane1, oAsmPlane4, 0)
oConstraint = oAsmCompDef.Constraints.AddFlushConstraint(oAsmPlane2, oAsmPlane5, 0)
oConstraint = oAsmCompDef.Constraints.AddFlushConstraint(oAsmPlane3, oAsmPlane6, 0)

Anonymous · ‎11-25-2014

I use flushing to 1 or 2 origin planes myself, so I modifyed the script to work in "different levels of flushing" I even created new buttons for them 🙂

check out the attached zip file and use the scripts you need 🙂

GeorgK · ‎05-08-2015

Hello itjelta,

is it possible to get the icons for your scripts?

Thanks

Georg

Anonymous · ‎05-08-2015

Hello i tried this rule again as is so just pasted it and i get 2x error on this code what am i doing wrong?

Error1 (on the last 3 lines)

Argument not specified for parameter 'EntityTwo' of 'Public function AddFlushConstraint...

Error2 (on the last 3 lines)

Comma,'(', or a valid expression continuation expected.

'get file to place
Dim oFileDlg As inventor.FileDialog = Nothing
InventorVb.Application.CreateFileDialog(oFileDlg)
oFileDlg.Filter = "Inventor Files (*.iam;*.ipt)|*.iam;*.ipt|All Files (*.*)|*.*"
oFileDlg.DialogTitle = "Select a File"
oFileDlg.InitialDirectory = ThisDoc.Path
oFileDlg.CancelError = True
On Error Resume Next
oFileDlg.ShowOpen()
If Err.Number <> 0 Then
MessageBox.Show("File not chosen.", "Dialog Cancellation")
Return
ElseIf oFileDlg.FileName <> "" Then
oFile = oFileDlg.FileName
End If

' set a reference to the assembly component definintion.
' This assumes an assembly document is open.
Dim oAsmCompDef As AssemblyComponentDefinition
oAsmCompDef = ThisApplication.ActiveDocument.ComponentDefinition

' Set a reference to the transient geometry object.
Dim oTG As TransientGeometry
oTG = ThisApplication.TransientGeometry
    
' Create a matrix.  
Dim oMatrix As Matrix
oMatrix = oTG.CreateMatrix

'place an instance of the component 
Dim oOccurrence As ComponentOccurrence
oOccurrence = oAsmCompDef.Occurrences.Add(oPath & oFile, oMatrix) 
' Set the translation portion of the matrix so the part will be 
'positioned at the co-ordinates
oMatrix.SetTranslation(oTG.CreateVector(0, 0, 0)) 

 'Iterate through all of the occurrences and ground them.
For Each oOccurrence In oAsmCompDef.Occurrences
'check for and skip virtual components
If Not TypeOf oOccurrence.Definition Is VirtualComponentDefinition Then
oOccurrence.Grounded = False
Else
End If
Next

'Get the plane from the selected part.
' The work plane obtained is in the context of the part, not the assembly.
Dim oPartPlane1 As WorkPlane
Dim oPartPlane2 As WorkPlane
Dim oPartPlane3 As WorkPlane
 oPartPlane1 =  oOccurrence.Definition.WorkPlanes.Item(1) 'Component YZ Plane
 oPartPlane2 =  oOccurrence.Definition.WorkPlanes.Item(2) 'Component XZ Plane
 oPartPlane3 =  oOccurrence.Definition.WorkPlanes.Item(3) 'Component XY Plane

 'Get the plane from the assembly
Dim oAsmPlane1 As WorkPlane
Dim oAsmPlane2 As WorkPlane
Dim oAsmPlane3 As WorkPlane
 oAsmPlane1 = oAsmCompDef.WorkPlanes.Item(1) 'Assembly YZ Plane
 oAsmPlane2 = oAsmCompDef.WorkPlanes.Item(2) 'Assembly XZ Plane
 oAsmPlane3 = oAsmCompDef.WorkPlanes.Item(3) 'Assembly XY Plane

' Create proxies for the work planes of the part.
' The proxies represent the part work planes in the context of the assembly.
Dim oAsmPlane4 As WorkPlaneProxy
Dim oAsmPlane5 As WorkPlaneProxy
Dim oAsmPlane6 As WorkPlaneProxy
oOccurrence.CreateGeometryProxy(oPartPlane1, oAsmPlane4)
oOccurrence.CreateGeometryProxy(oPartPlane2, oAsmPlane5)
oOccurrence.CreateGeometryProxy(oPartPlane3, oAsmPlane6)

'' Create the constraint using the part work plane proxies.
oConstraint = oAsmCompDef.Constraints.AddFlushConstraint(oAsmPlane1, oAsmPlane4, 0)
oConstraint = oAsmCompDef.Constraints.AddFlushConstraint(oAsmPlane2, oAsmPlane5, 0)
oConstraint = oAsmCompDef.Constraints.AddFlushConstraint(oAsmPlane3, oAsmPlane6, 0)

Anonymous · ‎05-08-2015

Hi,

i'm trying to edit the code provided here to make a MATE constraint for the Yaxis of assembly & Yaxis of part.

I tried this but my result is negative 🙂

'get file to place
Dim oFileDlg As inventor.FileDialog = Nothing
InventorVb.Application.CreateFileDialog(oFileDlg)
oFileDlg.Filter = "Inventor Files (*.iam;*.ipt)|*.iam;*.ipt|All Files (*.*)|*.*"
oFileDlg.DialogTitle = "Select a File"
oFileDlg.InitialDirectory = ThisDoc.Path
oFileDlg.CancelError = True
On Error Resume Next
oFileDlg.ShowOpen()
If Err.Number <> 0 Then
MessageBox.Show("File not chosen.", "Dialog Cancellation")
Return
ElseIf oFileDlg.FileName <> "" Then
oFile = oFileDlg.FileName
End If

' set a reference to the assembly component definintion.
' This assumes an assembly document is open.
Dim oAsmCompDef As AssemblyComponentDefinition
oAsmCompDef = ThisApplication.ActiveDocument.ComponentDefinition

' Set a reference to the transient geometry object.
Dim oTG As TransientGeometry
oTG = ThisApplication.TransientGeometry
    
' Create a matrix.  
Dim oMatrix As Matrix
oMatrix = oTG.CreateMatrix

'place an instance of the component 
Dim oOccurrence As ComponentOccurrence
Dim Total As Integer
Total = InputBox("Type How Many", "Insert", "1")

If Err.Number <> 0 Then  'if there is an error it returns out
Return
ElseIf Err.Number = 0 Then 'if there is no error, it keeps working, else returns out

For X = 1 To Total 
oOccurrence = oAsmCompDef.Occurrences.Add(oPath & oFile, oMatrix) 
' Set the translation portion of the matrix so the part will be 
'positioned at the co-ordinates
oMatrix.SetTranslation(oTG.CreateVector(0, 0, 0)) 


'Get the plane from the selected part.
' The work plane obtained is in the context of the part, not the assembly.
Dim oPartAxis1 As WorkAxis
 oPartAxis1 =  oOccurrence.Definition.WorkAxis.Item(2) 'Component Y Axis
 
Dim oAsmAxis1 As WorkAxis
 oAsmAxis1 = oAsmCompDef.WorkAxis.Item(2) 'Assembly Y Axis
 
Dim oAsmAxis4 As WorkAxisProxy
 oOccurrence.CreateGeometryProxy(oPartAxis1, oAsmAxis4)
 
 oConstraint = oAsmCompDef.Constraints.AddMateConstraint(oAsmAxis1, oAsmAxis4, 0)

Any ideas?

Anonymous · ‎05-08-2015

I adjusted my code a little but still no succes.

Just aiming for the axis constraint here. and made some change in the defenition names.

'get file to place
Dim oFileDlg As inventor.FileDialog = Nothing
InventorVb.Application.CreateFileDialog(oFileDlg)
oFileDlg.Filter = "Inventor Files (*.iam;*.ipt)|*.iam;*.ipt|All Files (*.*)|*.*"
oFileDlg.DialogTitle = "Select a File"
oFileDlg.InitialDirectory = ThisDoc.Path
oFileDlg.CancelError = True
On Error Resume Next
oFileDlg.ShowOpen()
If Err.Number <> 0 Then
MessageBox.Show("File not chosen.", "Dialog Cancellation")
Return
ElseIf oFileDlg.FileName <> "" Then
oFile = oFileDlg.FileName
End If

' set a reference to the assembly component definintion.
' This assumes an assembly document is open.
Dim oAsmCompDef As AssemblyComponentDefinition
oAsmCompDef = ThisApplication.ActiveDocument.ComponentDefinition

' Set a reference to the transient geometry object.
Dim oTG As TransientGeometry
oTG = ThisApplication.TransientGeometry
    
' Create a matrix.  
Dim oMatrix As Matrix
oMatrix = oTG.CreateMatrix

'place an instance of the component 
Dim oOccurrence As ComponentOccurrence
Dim Total As Integer
Total = InputBox("Type How Many", "Insert", "1")

If Err.Number <> 0 Then  'if there is an error it returns out
Return
ElseIf Err.Number = 0 Then 'if there is no error, it keeps working, else returns out

For X = 1 To Total 
oOccurrence = oAsmCompDef.Occurrences.Add(oPath & oFile, oMatrix) 
' Set the translation portion of the matrix so the part will be 
'positioned at the co-ordinates
oMatrix.SetTranslation(oTG.CreateVector(0, 0, 0)) 


'Get the plane from the selected part.
' The work plane obtained is in the context of the part, not the assembly.
Dim oPartAxis1 As WorkAxis
 oPartAxis1 =  oOccurrence.Definition.WorkAxes.Item(2) 'Component Y Axis


 'Get the plane from the assembly
Dim oAsmAxis1 As WorkAxis

 oAsmAxis1 = oAsmCompDef.WorkAxes.Item(2) 'Assembly Y Axis


' Create proxies for the work planes of the part.
' The proxies represent the part work planes in the context of the assembly.
Dim oAsmAxis4 As WorkAxisProxy

oOccurrence.CreateGeometryProxy(oPartAxis1, oAsmAxis4)


' Create the constraint using the part axis proxies.
oConstraint = oAsmCompDef.Constraints.AddMateConstraint(oAsmAxis4, oPartAxis1, 0)


Next
End If

Anonymous · ‎05-11-2015

sure 🙂

https://www.dropbox.com/s/tzpicyltujtv0h4/iLogic%20buttons.zip?dl=0

xiaodong_liang · ‎05-18-2015

Hi,

After a couple of test, it looks a problem to me. in UI, it works well. I also checked the constraint that is created by UI, EntityOne and EntityTwo same to what the API code gets. I also tried to create a copy of Y axis of assembly and constrain it with Y axis of part, no help.

Sorry I have not got any workaround this moment. I logged this issue with our engineer team: #70587

GeorgK · ‎05-18-2015

Thank you very much.

Georg

xiaodong_liang · ‎06-09-2015

Hi Georg,

Our engineer checked the test code. She found I made a mistake. I still used part axis as the parameter of AddMateConstraint 😞

after modification, the code works well. I tested a lot and modified a lot… strange I made such stupid mistake. Could you check if it can work at your side?

   Private Sub Button6_Click(sender As Object, e As EventArgs) Handles Button6.Click
        Dim oInventorApplication As Inventor.Application
        Try
            oInventorApplication = System.Runtime.InteropServices.Marshal.GetActiveObject("Inventor.Application")
        Catch
        End Try

        Dim ThisDoc As Document = oInventorApplication.ActiveDocument

        'get file to place
        Dim oFileDlg As Inventor.FileDialog = Nothing
        oInventorApplication.CreateFileDialog(oFileDlg)
        oFileDlg.Filter = "Inventor Files (*.iam;*.ipt)|*.iam;*.ipt|All Files (*.*)|*.*"
        oFileDlg.DialogTitle = "Select a File"
        oFileDlg.InitialDirectory = System.IO.Path.GetFullPath(ThisDoc.FullFileName)
        oFileDlg.CancelError = True
        oFileDlg.ShowOpen()

        Dim oFile As String
        If Err.Number <> 0 Then
            MessageBox.Show("File not chosen.", "Dialog Cancellation")
            Return
        ElseIf oFileDlg.FileName <> "" Then
            oFile = oFileDlg.FileName
        End If

        ' set a reference to the assembly component definintion.
        ' This assumes an assembly document is open.
        Dim oAsmCompDef As AssemblyComponentDefinition
        oAsmCompDef = oInventorApplication.ActiveDocument.ComponentDefinition

        ' Set a reference to the transient geometry object.
        Dim oTG As TransientGeometry
        oTG = oInventorApplication.TransientGeometry

        ' Create a matrix.  
        Dim oMatrix As Matrix
        oMatrix = oTG.CreateMatrix

        'place an instance of the component 
        Dim oOccurrence As ComponentOccurrence
        Dim Total As Integer
        Total = InputBox("Type How Many", "Insert", "1")

        If Err.Number <> 0 Then  'if there is an error it returns out
            Return
        ElseIf Err.Number = 0 Then 'if there is no error, it keeps working, else returns out

            For X = 1 To Total
                oOccurrence = oAsmCompDef.Occurrences.Add(oFile, oMatrix)
                ' Set the translation portion of the matrix so the part will be 
                'positioned at the co-ordinates
                oMatrix.SetTranslation(oTG.CreateVector(0, 0, 0))


                'Get the plane from the selected part.
                ' The work plane obtained is in the context of the part, not the assembly.
                Dim oPartAxis1 As WorkAxis
                oPartAxis1 = oOccurrence.Definition.WorkAxes.Item(2) 'Component Y Axis
                 


                'Get the plane from the assembly
                Dim oAsmAxis1 As WorkAxis
                oAsmAxis1 = oAsmCompDef.WorkAxes.Item(2) 'Assembly Y Axis 
 
                ' Create proxies for the work planes of the part.
                ' The proxies represent the part work planes in the context of the assembly.
                Dim oObj As Object = Nothing
                oOccurrence.CreateGeometryProxy(oPartAxis1, oObj)

                Dim oAsmAxis4 As WorkAxisProxy
                oAsmAxis4 = oObj


                'oNewAxis.Grounded = True
                Dim oConstraint As AssemblyConstraint
                ' Create the constraint using the part axis proxies.
               
                'oConstraint = oAsmCompDef.Constraints.AddMateConstraint(oNewAxis, oPartAxis1, 0)
                 oConstraint = oAsmCompDef.Constraints.AddMateConstraint(oAsmAxis1, oObj, 0)

                'oNewAxis.Grounded = False

            Next
        End If
    End Sub

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Place &amp; Constrain to Origin Macro