Include all surface

[rgruychev]

When I have part  with surface and make drawing  Inventor shows surface -  tag Include all surface is default.

 I want exclude Include all surface tag  by default  and tag when I need.

[jdkriek]

When a file contains only surfaces they are automatically included in drawing views.

When a file contains surfaces, but also at least one solid body then they are automaticly exluded from the drawing views.

[rgruychev]

In Inventor 2013 this function doesn't work

When a file contains surfaces, but also at least one solid body then they are automaticly exluded from the drawing views.

I try with part and assembly consist  solid body and surface tag is included from the drawing views.

[rgruychev]

Does anyone have a similar problem ?

[hjvcan]

yes, i have a very similar problem.

any surface in a model is always visible by default, sometimes I have to make the surfaces invisible in the model before I can even use the option of un-including all surfaces.

this has only started since going to IV2013

[Gene.R]

I am seeing the same problem too, only in 2013.  even when I open an old drawing and change the view scale the surfaces come in, then I have to check the "include all surfaces" from the model tree and then immediately uncheck the "include all surfaces" to turn them off.

is there a default setting somewhere that I am missing?

Gene 

[rschader]

I have this same issue since moving to iv2013, and it is making a ton of extra work for me!

[ic198]

I have the same problem too, and only since moving to 2013.

I think it is something to do with the fact Inventor now implements View Reps for Parts, albeit in a very messy and barely workable fashion.

I do have some assemblies that behave when a drawing is created of them and I've just been experimenting with them and trying to work out a pattern. I'm not sure if this is the final answer:-

I think it is the Master View Rep of the assembly that misbehaves. No matter what you have displayed when viewing the Master in assembly view, when you create a drawing of it it will display all surfaces. Create a new View Rep of the assembly and get this set up correctly with no surfaces or only certain surfaces displayed. A drawing of this new View Rep should (hopefully!) come in correctly. Note that you can update current drawings by changing which View Rep is displayed in the Edit View dialog. You might also need to force this to update sometimes- right-click on the drawing View in the browser and select Apply Design View.

[Gene.R]

it seems to me that the ipt master view rep and the idw view rep does not maintain accosiative beyond initial view placement.

1. create a part
2. copy object as a surface and uncheck associative.
3. turn the visibility of that surface off
4. create a drawing view of that part using the master view rep
5. in the drawing browser right click on the ipt.(notice include all surfaces is not checked).
6. now edit the solid and copy object as a surface, and edit agin so that the soilid will be different than the surface.
7. Turn the visibility of that surface off
8. now when the drawing updates it shows the most recent copy object surface evn though the visibility is off in the master view rep of the ipt.
9. in the drawing browser right click on the ipt (notice include all surfaces now has a black check box next to it) this indicates to me that some of the "include all surfaces" are included in the drawing view but not all.

Now I have to select "include all surfaces" which turns them all on, and immediately select include all surfaces again to turn them off, and I have to do this for every view that is on the drawing regardless of accosiativity to the Base view, and this is really causing a lot of work.

yes creating a new view rep does hide the surfaces if you check the drawing view rep associative link, but I have over 10 years of drawings that were created using the master view representation,

a workflow that I have promoted here at wipaire is to make a copy object surface of a part solid before revising any geometry. then rename the surface as Rev A, Rev B...ect, this provides revision history right in the model. it also helps to make the drafter aware of any geometry that might have changed inadvertently.

[rschader]

With some help from the customization group (I think it was an Autodesk employee), I managed to put together the following macro which iterates through all the views on the active sheet and turns of all surface visibility in each view. Not sure it will work in all cases, but I made sure it works when there are parts suppressed in the active LOD rep for each view. It definately makes my job a bit easier:

Public Sub SetSurfaceVisibilityOff()
    ' Set a reference to the currently active drawing document.
    Dim oDrawDoc As DrawingDocument
    Set oDrawDoc = ThisApplication.ActiveDocument
    
    ' Get the active sheet.
    Dim oSheet As Sheet
    Set oSheet = oDrawDoc.ActiveSheet
    
    ' Get the selected view.
    Dim oDrawView As Inventor.DrawingView
    Dim oNumViews As Integer
    'Set oDrawView = oDrawDoc.ActiveSheet.DrawingViews.Item(1)
    Dim oAsmDoc As AssemblyDocument
    Dim oCompDef As AssemblyComponentDefinition
    Dim oLeafOccs As ComponentOccurrencesEnumerator
    Dim oOcc As ComponentOccurrence
    Dim oWorkSurface As WorkSurface
    Dim oSurface As SurfaceBody
    Dim oFeature As PartFeature
    Dim oFeatureProxy As Object
    oNumViews = oDrawDoc.ActiveSheet.DrawingViews.Count
    Dim oProgBar As ProgressBar
    Set oProgBar = ThisApplication.CreateProgressBar(False, oNumViews, "View Processing Progress")
    oProgBar.Message = "Processing " & oNumViews & " Views"
    
    For Each oDrawView In oDrawDoc.ActiveSheet.DrawingViews
        ' Get the assembly shown in the view.
        Debug.Print "Processing View: " & oDrawView.Name
        oProgBar.Message = "Processing View: " & oDrawView.Name
        oProgBar.UpdateProgress
        Set oAsmDoc = oDrawView.ReferencedDocumentDescriptor.ReferencedDocument
        ' Get the component defenition
        Set oCompDef = oAsmDoc.ComponentDefinition
        ' Get all of the leaf occurrences of the assembly.
        Set oLeafOccs = oCompDef.Occurrences.AllLeafOccurrences
        For Each oOcc In oLeafOccs
            ' We are only interested in PartComponentDefinition's
            ' because only they can have WorkSurfaces
            ' In theory not even an empty assembly could be considered a
            ' leaf occurrence, but we check anyway
            If oOcc.Suppressed = False Then
                If TypeOf oOcc.Definition Is PartComponentDefinition Then
                    For Each oWorkSurface In oOcc.Definition.WorkSurfaces
                        For Each oSurface In oWorkSurface.SurfaceBodies
                            Set oFeature = oSurface.CreatedByFeature
                            Call oOcc.CreateGeometryProxy(oFeature, oFeatureProxy)
                            Call oDrawView.SetVisibility(oFeatureProxy, False)
                        Next
                    Next
                End If
            End If
        Next
    Next
    oProgBar.Close
End Sub

[391-56586451]

Hi there,

I'm not very familiar with VB, but managed to make the macro with the script. It does work untill a view of a IPN is reached then it stops with a error in the following line:

Set oAsmDoc = oDrawView.ReferencedDocumentDescriptor.ReferencedDocument

What can I do to add or fix?

[stevec781]

I posted about this a while ago, the only solution was to go into every part and delete the  construction surfaces with delete face - lump.  But now I have another problem.

I dervied in a solid to many parts to use as a boolean cut, the model is correct but the cutting part shows in the drawing and there is no way to get rid of it.

Guess I have to go into autocad as usual to clean up inventors mess.