Open Parameter Dialog box with code

[grim2020]

Hi,

I'm using VBA in Inventor 2010.  I want to create a macro that adds 3 fields to a part for LRNGTH, WIDTH and THICKNESS, as well as comments and setting the export to be export out.  My program is below and works well.  However i would like to end the macro with the parameter dialog box open.  What code do i need to do this?

Sub AddBomFields()
   
    'adds LENGTH, WIDTH and THICKNESS user parameters to part
   
    Dim oPartDoc As PartDocument
    Set oPartDoc = ThisApplication.ActiveDocument
  
    Dim oCompDef As PartComponentDefinition
    Set oCompDef = oPartDoc.ComponentDefinition

    Dim oUserParam As UserParameter
    Set oUserParam = oCompDef.Parameters.UserParameters.AddByValue("LENGTH", 0, kInchLengthUnits)
    Set oUserParam = oCompDef.Parameters.UserParameters.AddByValue("WIDTH", 0, kInchLengthUnits)
    Set oUserParam = oCompDef.Parameters.UserParameters.AddByValue("THICKNESS", 0, kInchLengthUnits)
   
    ' Get the Parameters object. Assumes a part or assembly document is active.
    Dim oParameters As Parameters
    Set oParameters = ThisApplication.ActiveDocument.ComponentDefinition.Parameters

    ' Get the parameter named "LENGTH".
    Dim oLengthParam As Parameter
    Set oLengthParam = oParameters.Item("LENGTH")
    oLengthParam.Comment = "BOM LENGTH"
    oLengthParam.ExposedAsProperty = True
   
    ' Get the parameter named "WIDTH".
    Dim oWidthParam As Parameter
    Set oWidthParam = oParameters.Item("WIDTH")
    oWidthParam.Comment = "BOM WIDTH"
    oWidthParam.ExposedAsProperty = True
       
    ' Get the parameter named "THICKNESS".
    Dim oThicknessParam As Parameter
    Set oThicknessParam = oParameters.Item("THICKNESS")
    oThicknessParam.Comment = "BOM THICKNESS"
    oThicknessParam.ExposedAsProperty = True
   
    ThisApplication.ActiveDocument.Update
   
    Dim Msg, Style, Title, Help, Ctxt, Response
    Msg = "Length, Width and Thickness parameters added."    ' Define message.
    Style = vbOKOnly    ' Define buttons.
    Title = "Parameter Addition Complete"    ' Define title.
   
    ' Display message.
    Response = MsgBox(Msg, Style, Title)
       
    End Sub

[barbara.han · Accepted solution]

To fire a command, you need to find the internal name of that command, then call the Execute method on the corresponding ControlDefinition object.

Here is the code to fire Parameters dialog:   

ThisApplication.CommandManager.ControlDefinitions.Item("AppParametersCmd").Execute

You can use the following code to get all internal names of all commands:

Sub test()

    Dim oControlDef As ControlDefinition

    Open "c:\1.txt" For Output As #1

    Dim s As String

    For Each oControlDef In ThisApplication.CommandManager.ControlDefinitions

        s = oControlDef.InternalName & ":" & oControlDef.DescriptionText

        Write #1, s

    Next

    Close #1

End Sub

Barbara Han

Developer Technical Services

Autodesk

[grim2020]

Excellent.  Thank you.

[grim2020]

Is there a way to condense my code to allow the export and comments to be added at the same time as the parameter is created?

[barbara.han · Accepted solution]

I finally got time to look into this thread again. You can simplify your code so that there is no need to read the parameter later in order to change its properties. Here is the simplified version:

Sub AddBomFields()

    'adds LENGTH, WIDTH and THICKNESS user parameters to part
   
    Dim oPartDoc As PartDocument
    Set oPartDoc = ThisApplication.ActiveDocument
   
    Dim oCompDef As PartComponentDefinition
    Set oCompDef = oPartDoc.ComponentDefinition
   
    Dim oUserParam As UserParameter
    Set oUserParam = oCompDef.Parameters.UserParameters.AddByExpression("LENGTH", 0, kInchLengthUnits)
    oUserParam.Comment = "BOM LENGTH"
    oUserParam.ExposedAsProperty = True
   
    Set oUserParam = oCompDef.Parameters.UserParameters.AddByValue("WIDTH", 0, kInchLengthUnits)
    oUserParam.Comment = "BOM WIDTH"
    oUserParam.ExposedAsProperty = True
   
    Set oUserParam = oCompDef.Parameters.UserParameters.AddByValue("THICKNESS", 0, kInchLengthUnits)
    oUserParam.Comment = "BOM THICKNESS"
    oUserParam.ExposedAsProperty = True
   
    ThisApplication.CommandManager.ControlDefinitions.Item("AppParametersCmd").Execute
  
End Sub

[grim2020]

Thank you Barbara,  I understand VB well enough, it's just getting the Inventor sysntax down.

[barbara.han]

Yes, it would be even simpler if AddByVaule or an other API has more parameters to set all those properties in a line of code, but unluckily no that API. How it should not be difficult to use currect way to do the same. 

[grim2020]

Barbara,

I have the following code to add a length field.  How do I set the unit string to off so the "in" does not display?

Sub AddBomFieldsL()

    'adds LENGTH, WIDTH and THICKNESS user parameters to part
  
    Dim oPartDoc As PartDocument
    Set oPartDoc = ThisApplication.ActiveDocument
  
    Dim oCompDef As PartComponentDefinition
    Set oCompDef = oPartDoc.ComponentDefinition
  
    Dim oUserParam As UserParameter
    Set oUserParam = oCompDef.Parameters.UserParameters.AddByExpression("LENGTH", 0, kInchLengthUnits)
    oUserParam.Comment = "BOM LENGTH"
    oUserParam.ExposedAsProperty = True
  
    ThisApplication.CommandManager.ControlDefinitions.Item("AppParametersCmd").Execute
 
End Sub

[grim2020]

Answered my own question:

    oUserParam.CustomPropertyFormat.ShowUnitsString = False
    oUserParam.CustomPropertyFormat.Precision = kTwoDecimalPlacesPrecision