topic Re: How dont export hole with thread? in Inventor Programming Forum

How dont export hole with thread?

Leonardo_Czuy — Thu, 14 Dec 2023 11:47:46 GMT

Hello Everyone,

I am trying to make a code to automatize export to DXF Flat Sheet Metal.
When i export a Sheet with thread hole.
This holes have M12, when i export with DN 12mm.

In this case, if hole have thread I would like these holes not to be exported.

For Each oRefDoc In oRefDocs iptPathName = Left(oRefDoc.FullDocumentName, Len(oRefDoc.FullDocumentName) - 3) & "ipt" If (Not System.IO.File.Exists(iptPathName)) Then Continue For Dim oDrawDoc As PartDocument oDrawDoc = ThisApplication.Documents.Open(iptPathName, True) oFileName = Left(oRefDoc.DisplayName, Len(oRefDoc.DisplayName)) Dim quantidadeDePecas As String = "QTDE: " & oAsmDoc.ComponentDefinition.Occurrences.AllReferencedOccurrences(oRefDoc).Count 'Set the DXF target file name Try Dim CustomName As String Try CustomName = iProperties.Value(oFileName, "Project", "Part number") CustomName = CustomName.replace("/", "-") Catch CustomName = oFileName End Try oDataMedium.FileName = oFolder & "\" & CustomName & ".dxf" Dim oCompDef As SheetMetalComponentDefinition oCompDef = oDrawDoc.ComponentDefinition If oCompDef.HasFlatPattern = False Then oCompDef.Unfold Else oCompDef.FlatPattern.Edit End If For Each oFeature As PartFeature In oCompDef.Features If oFeature.Type = kThreadFeatureObject Then End If Next Dim sOut As String sOut = "FLAT PATTERN DXF?AcadVersion=2004&" & _ "OuterProfileLayer=CONTORNI&OuterProfileLayerColor=255;255;0&" & _ "InteriorProfilesLayer=CONTORNI&InteriorProfilesLayerColor=255;255;0&" & _ "TangentLayer=SOTTILI&TangentLayerColor=255;0;0&" & _ "BendLayer=SOTTILI&BendLayerColor=255;0;0&" & _ "BendUpLayerColor=255;0;0&BendDownLayerColor=255;0;0&" & _ "InvisibleLayers=IV_ARC_CENTERS;IV_FEATURE_PROFILES;IV_FEATURE_PROFILES_DOWN" oCompDef.DataIO.WriteDataToFile(sOut, oDataMedium.FileName) AddDXFProperties(oDrawDoc, oDataMedium.FileName, quantidadeDePecas ,False) oCompDef.FlatPattern.ExitEdit Catch End Try oDrawDoc.Close Next

回复： How dont export hole with thread?

yuzeaa — Thu, 14 Dec 2023 12:56:55 GMT

This method may not look good, but it may be feasible. You can try it out

Dim threadHoles As New List(Of HoleFeature) For Each Hole As HoleFeature In refdoc.ComponentDefinition.Features.HoleFeatures If Hole.HealthStatus = HealthStatusEnum.kSuppressedHealth Then Continue For If Hole.TapInfo IsNot Nothing Then threadHoles.Add(Hole) Hole.Suppressed = True End If Next 'start 'export dxf 'end For Each hole As HoleFeature In threadHoles hole.Suppressed = False Next

Re: How dont export hole with thread?

JelteDeJong — Thu, 14 Dec 2023 13:34:43 GMT

It's possible to add attributes to edges. With those attributes, you can control the layer that the edge will get during export. So if assign an attribute to the edges of holes with thread, then you control the layer of those edges. If you hide those layers during export then you get what you want.

The following iLogic rule will add attributes to edges that belong to holes with thread. You should see that they get exported to the layer "HideFromExport"

Dim setName As String = "FlatPatternAttributes" Dim attName As String = "LayerName" Dim attValue As String = "HideFromExport" Dim doc As PartDocument = ThisDoc.Document Dim def As SheetMetalComponentDefinition = doc.ComponentDefinition Dim flatPattern = def.FlatPattern Dim topFace = flatPattern.TopFace Dim circuarEdges = topFace.Edges.Cast(Of Edge).Where(Function(e) e.GeometryType = CurveTypeEnum.kCircleCurve) Dim foundEdges = ThisApplication.TransientObjects.CreateObjectCollection For Each edge As Edge In circuarEdges For Each face As Face In edge.Faces Dim feature As PartFeature = face.CreatedByFeature If (TypeOf feature Is HoleFeature) Then Dim hole As HoleFeature = feature If (hole.HoleType = HoleTypeEnum.kDrilledHole) Then foundEdges.Add(edge) Dim attSet As AttributeSet = Nothing If (edge.AttributeSets.NameIsUsed(setName)) Then attSet = edge.AttributeSets.Item(setName) Else attSet = edge.AttributeSets.Add(setName) End If If (attSet.NameIsUsed(attName)) Then Dim attribute = attSet.Item(attName).Value = attValue Else attSet.Add(attName, ValueTypeEnum.kStringType, attValue) End If End If End If Next Next doc.SelectSet.Clear() doc.SelectSet.SelectMultiple(foundEdges) MsgBox("Found edges: " & foundEdges.Count)

There are some disadvantages to using attributes.

There is no way of viewing attributes with the Inventor. You need an addin to view them (like 'Nifty Attributes') or you can use my iLogic rule to change layer names. "Setting Extra Layers In DXF Exports"
This rule will add attributes to edges but will never remove them. So I'm not sure what would happen if you change your hole type from a hole with thread and then remove the thread. It's possible that the attribute stays and your hole without thread is still removed from export.

Re: How dont export hole with thread?

Leonardo_Czuy — Thu, 14 Dec 2023 15:26:38 GMT

Hello @JelteDeJong and @JelteDeJong, thanks a lot for helping, but have one problem

What can i do when hole is draw in sketch?

Re: How dont export hole with thread?

jeremy.goenen — Fri, 15 Dec 2023 12:17:14 GMT

Hi, if you can commit to make the holes with a feature, be it hole, cut, extrusion or else, you could add a tag to the featurename, like "suppress" or "nodxf" and then suppress all features that include this tag like @yuzeaa proposed

Maybe you could use a punchtool for these holes, in this case you can define how the holes are shown in the flatpattern

https://help.autodesk.com/view/INVNTOR/2022/ENU/?guid=GUID-1A5F9CD1-80A8-4462-894A-4D8C9DFCDB51