topic Re: Make feature sketch invisible in an assembly in Inventor Programming Forum

Make feature sketch invisible in an assembly

Hubert_Los — Tue, 13 Jun 2023 06:53:10 GMT

Hi,
How to make invisible all the feature sketches that are make visible in the assembly?

Re: Make feature sketch invisible in an assembly

Andrii_Humeniuk — Tue, 13 Jun 2023 07:07:07 GMT

Hi @Hubert_Los . Try this iLogic code. It makes all sketches in all components of the main assembly invisible.

Private Sub Main() Dim oDoc As AssemblyDocument = ThisApplication.ActiveDocument Dim oTrans As Transaction = ThisApplication.TransactionManager.StartTransaction(oDoc, "SetVisibleSketch") For Each oRefDoc As Document In oDoc.AllReferencedDocuments If TypeOf oRefDoc Is PartDocument And oRefDoc.IsModifiable Then Dim oPDoc As PartDocument = oRefDoc Call SetVisibleSketch(oPDoc.ComponentDefinition.Sketches) End If Next oTrans.End() End Sub Private Function SetVisibleSketch(oSkets As PlanarSketches, Optional bVisible As Boolean = False) For i As Integer = 1 To oSkets.Count If oSkets.Item(i).Visible Then oSkets.Item(i).Visible = bVisible Next End Function

Re: Make feature sketch invisible in an assembly

Hubert_Los — Tue, 13 Jun 2023 09:26:20 GMT

Hi @Andrii_Humeniuk ,

Unfortunately your code only works on "shered skeches" I have a different situation. I enable sketch editing from the assembly level and this sketch is not share.

Re: Make feature sketch invisible in an assembly

Andrii_Humeniuk — Tue, 13 Jun 2023 10:39:17 GMT

Not sure I understood you correctly, but made the changes to the code. Now the visibility of sketches is turned off in the main assembly and in subassemblies and in details. The code also includes a check for the ability to modify documents.

Private Sub Main() Dim oDoc As AssemblyDocument = ThisApplication.ActiveDocument Dim oTrans As Transaction = ThisApplication.TransactionManager.StartTransaction(oDoc, "SetVisibleSketch") If oDoc.IsModifiable Then Call SetVisibleSketch(oDoc.ComponentDefinition.Sketches) For Each oRefDoc As Document In oDoc.AllReferencedDocuments If oRefDoc.IsModifiable Then Call SetVisibleSketch(oRefDoc.ComponentDefinition.Sketches) End If Next oTrans.End() End Sub Private Function SetVisibleSketch(oSkets As PlanarSketches, Optional bVisible As Boolean = False) For i As Integer = 1 To oSkets.Count On Error Resume Next If oSkets.Item(i).Visible Then oSkets.Item(i).Visible = bVisible Next i End Function

Re: Make feature sketch invisible in an assembly

Hubert_Los — Fri, 16 Jun 2023 07:09:19 GMT

Sorry, but it doesn't work. I'm sending a video of what sketch I mean

(view in My Videos)

Re: Make feature sketch invisible in an assembly

Andrii_Humeniuk — Fri, 16 Jun 2023 08:53:42 GMT

Hi @Hubert_Los . I finally understood you. Thanks for the video explaining what you need it really helped. Here is the code that determines the visibility of all proxy skeaths and makes them invisible:

Private Sub Main() Dim oDoc As AssemblyDocument = ThisApplication.ActiveDocument Dim oTrans As Transaction = ThisApplication.TransactionManager.StartTransaction(oDoc, "SetVisibleSketch") Call SetVisibleSketch(oDoc.ComponentDefinition.Occurrences) oTrans.End() End Sub Private Function SetVisibleSketch(oOccs As ComponentOccurrences, Optional bVisible As Boolean = False) For Each oOcc As ComponentOccurrence In oOccs If oOcc.DefinitionDocumentType = DocumentTypeEnum.kPartDocumentObject Then On Error Resume Next Dim oOccDef As PartComponentDefinition = oOcc.Definition For Each oSketch As PlanarSketch In oOccDef.Sketches Dim oSketchProxy As PlanarSketchProxy : oOcc.CreateGeometryProxy(oSketch, oSketchProxy) If oSketchProxy.Visible Then oSketchProxy.Visible = False Next Else If oOcc.DefinitionDocumentType = DocumentTypeEnum.kAssemblyDocumentObject Then If oOcc.SubOccurrences.Count > 0 Then Call SetVisibleSketch(oOcc.SubOccurrences) End If End If Next End Function

Re: Make feature sketch invisible in an assembly

Hubert_Los — Fri, 16 Jun 2023 09:15:34 GMT

Now it works, thank you 🙂