Autodesk Inventor Customization

[#1]

Guys,

What if I have 3 views and I need to dimension OAL length on the front view, OAL width on the side view, and lets say a hole on the top view. How to modify the code. I tried to play with it, copiyng the part of the code and changing the view name, but it gives me an error.

Thanks in advance.

[#2]

Hi,

Here you have some code that can do that, only thing what you must have do is give the Drawing View a name and give the user / model parameter the right name.

Sub Main
    Dim oDrawDoc As DrawingDocument = ThisDoc.Document
    Dim oSheet As Sheet = oDrawDoc.ActiveSheet
    RetrieveDimByView(oSheet, "FrontView", "RetD_")
    RetrieveDimByView(oSheet, "RightView", "RetDRight_")
    RetrieveDimByView(oSheet, "TopView", "RetDTop_")
End Sub

Sub RetrieveDimByView(ByVal oSheet As Sheet, ByVal ViewName As String, ByVal PrefixStr As String)
    Dim oDrawView As DrawingView
    For Each oDrawView In oSheet.DrawingViews
        If oDrawView.Name = ViewName Then
            Exit For
        End If
    Next
    Dim oGeneralDimensionsEnum As GeneralDimensionsEnumerator
    oGeneralDimensionsEnum = oSheet.DrawingDimensions.GeneralDimensions.Retrieve(oDrawView)
    Dim oGeneralDimension As GeneralDimension
    For Each oGeneralDimension In oGeneralDimensionsEnum
        Dim oParameter As Parameter
        Try
            oParameter = oGeneralDimension.RetrievedFrom.Parameter
        Catch
            ' Error to set oParameter.
            ' Go further to delete the dimension.
        End Try
        If oParameter.DrivenBy.count <> 0 Then
            Dim oDrivenByParameter As Parameter
            For Each oDrivenByParameter In oParameter.DrivenBy
                If InStr(oDrivenByParameter.Name, PrefixStr) = 0 Then
                    oGeneralDimension.Delete
                End If
            Next
        Else
            If InStr(oParameter.Name, PrefixStr) = 0 Then
                oGeneralDimension.Delete
            End If
        End If
    Next
    oSheet = Nothing
End Sub

[#3]

Excellent works just great.

One more question, is there any chance to offset the dimensions?

Thanks,

[#4]

Hi Marco,

It works fine, but my model is based on a multi body part.

So if i retrieve the dimensions, i get the dimensions from every part from my assembly.

in the standard interface, i can select a part thats part of the view, how can i do this thru the api?

the API help tells me that you can use a "demensionToRetrive":

Sub Retrieve(ViewOrSketch As IDispatch, ByRef DimensionsToRetrieve As [optional] VARIANT, Result As [out, retval] GeneralDimensionsEnumerator*)

I've tried some to create a ObjectCollection with the specific part, but i doesn't seem to work. Do you have any suggestion.

Kind regards,

Theo

[#5]

Hello achmidt,

What you can do is select all dimension and then arrange dimensions.

Start code"

    Dim oCommandMgr As CommandManager = _
    ThisApplication.CommandManager

    oCommandMgr.ControlDefinitions.item("DrawingSelectAllInventorDimsCmd").Execute
    oCommandMgr.ControlDefinitions.item("DrawingArrangeDimensionsCmd").Execute

"End code

Best regards,

[#6]

Hello Theo,

If you want to make a collection of a Part you can do something like this,

Dim oAssemblyDocument As Inventor.AssemblyDocument = _
	oDrawView.ReferencedDocumentDescriptor.ReferencedDocument

Dim oOcc As Inventor.ComponentOccurrence = _
	oAssemblyDocument.ComponentDefinition.occurrences.item(1)

Dim oGeneralDimensionsObj As ObjectCollection = _
	oSheet.DrawingDimensions.GeneralDimensions.GetRetrievableDimensions(oDrawView, oOcc)

The oGeneralDimensionsObj has now the retrieved dimensions form the first Part.

Best regards,

[#7]

Thanks!!!

[#8]

I`d like to share the code I assembled from different pieces (see attached). Configurator works great but I have few problems with the drawing dimensions.

I`m not sure how to place flat pattern OAL dim`s, can`t place bend dim`s, not sure how to modify flat pattern placement code so it shows bend extents.

oView4 = oSheet.DrawingViews.AddBaseView(oPartDoc,oPoint4, ViewScale,kDefaultViewOrientation, kHiddenLineDrawingViewStyle,,, oBaseViewOptions)

 Also I`m not sure how to do ordinate dim`s for the holes (horizontal & vertical).

If you`d like to test it out don`t forget to change the template path and name in the code.

I have an external rule that I run after drawing creation (see below), it places the dimensions I need.

Sub Main
    Dim oDrawDoc As DrawingDocument = ThisDoc.Document
    Dim oSheet As Sheet = oDrawDoc.ActiveSheet
    RetrieveDimByView(oSheet, "VIEW1", "Fr_") ' front view
    RetrieveDimByView(oSheet, "VIEW3", "Rs_") ' right side view
	RetrieveDimByView(oSheet, "VIEW2", "Tv_") ' top view
    'RetrieveDimByView(oSheet, "View3", "RetDTop_")
End Sub

Sub RetrieveDimByView(ByVal oSheet As Sheet, ByVal ViewName As String, ByVal PrefixStr As String)
    Dim oDrawView As DrawingView
    For Each oDrawView In oSheet.DrawingViews
        If oDrawView.Name = ViewName Then
            Exit For
        End If
    Next
    Dim oGeneralDimensionsEnum As GeneralDimensionsEnumerator
    oGeneralDimensionsEnum = oSheet.DrawingDimensions.GeneralDimensions.Retrieve(oDrawView)
    Dim oGeneralDimension As GeneralDimension
    For Each oGeneralDimension In oGeneralDimensionsEnum
        Dim oParameter As Parameter
        Try
            oParameter = oGeneralDimension.RetrievedFrom.Parameter
        Catch
            ' Error to set oParameter.
            ' Go further to delete the dimension.
        End Try
        If oParameter.DrivenBy.count <> 0 Then
            Dim oDrivenByParameter As Parameter
            For Each oDrivenByParameter In oParameter.DrivenBy
                If InStr(oDrivenByParameter.Name, PrefixStr) = 0 Then
                    oGeneralDimension.Delete
                End If
            Next
        Else
            If InStr(oParameter.Name, PrefixStr) = 0 Then
                oGeneralDimension.Delete
            End If
        End If
    Next
    oSheet = Nothing
	
	
	Dim oCommandMgr As CommandManager = _
    ThisApplication.CommandManager

    oCommandMgr.ControlDefinitions.item("DrawingSelectAllInventorDimsCmd").Execute
    oCommandMgr.ControlDefinitions.item("DrawingArrangeDimensionsCmd").Execute
	
End Sub

 Would be great to add a code that automatically scales up/down the views and places them on the sheet.

Any help appreciated. Thanks,