In the last post, we introduced how to create chamfer feature in part document. In an assembly document, we have two choices, either create the feature in assembly context, or create the real feature in part context. Actually, this applies to other types of feature which are supported in assembly document.
For choice 1, we need to input the proxy geometries (say EdgeProxy, FaceProxy) to the methods of chamfer feature. e.g. the code below assumes a face is selected in the assembly document. Since it is in the context of assembly, it is FaceProxy already. The same to the edges of the FaceProxy, they are EdgeProxy.
Sub createChamferInAssemblyContext_selectedObject()
Dim oDoc As AssemblyDocument
oDoc = ThisApplication.ActiveDocument
Dim oDef As AssemblyComponentDefinition
oDef = oDoc.ComponentDefinition
'selected face. in assembly this is a proxy face
Dim oSelectedFace As FaceProxy
oSelectedFace = oDoc.SelectSet(1)
Dim oEdgeCol As EdgeCollection
oEdgeCol = ThisApplication.TransientObjects.CreateEdgeCollection()
'method 1: creates a new ChamferFeature defined by a specified distance
'the edge from the FaceProxy is proxy edge already.
oEdgeCol.Add oSelectedFace.Edges(1)
oEdgeCol.Add oSelectedFace.Edges(2)
Call oDef.Features.ChamferFeatures.AddUsingDistance(oEdgeCol, "0.1 in")
'method 2: creates a new ChamferFeature that is defined by a distance and at a specified angle to an input face
'the edge from the FaceProxy is proxy edge already.
oEdgeCol.Clear()
oEdgeCol.Add oSelectedFace.Edges(3)
Call oDef.Features.ChamferFeatures.AddUsingDistanceAndAngle(oEdgeCol, oSelectedFace, "0.2 in", 0.5233)
'creates a new ChamferFeature that is defined by two distances
'the edge from the FaceProxy is proxy edge already.
oEdgeCol.Clear()
oEdgeCol.Add oSelectedFace.Edges(4)
Call oDef.Features.ChamferFeatures.AddUsingTwoDistances(oEdgeCol, oSelectedFace, "0.1 in", "0.2 in")
EndSub
If we get the objects of parts firstly, we can convert them to proxy objects by Occurrence.CreateGeometryProxy. Next, similarly to the above, input the proxy geometries to the methods of chamfer feature.
Sub createChamferInAssemblyContext_objectFromPart()
Dim oDoc As AssemblyDocument
oDoc = ThisApplication.ActiveDocument
Dim oAssDef As AssemblyComponentDefinition
oAssDef = oDoc.ComponentDefinition
Dim oOccurrence1 As ComponentOccurrence
oOccurrence1 = oAssDef.Occurrences(1)
Dim oPart1Def As PartComponentDefinition
oPart1Def = oOccurrence1.Definition
'get face and edge in part context
Dim oFaceInPart As Face
oFaceInPart = oPart1Def.SurfaceBodies(1).Faces(1)
Dim oEdge1 As Edge
oEdge1 = oFaceInPart.Edges(1)
Dim oEdge2 As Edge
oEdge2 = oFaceInPart.Edges(2)
Dim oEdge3 As Edge
oEdge3 = oFaceInPart.Edges(3)
Dim oEdge4 As Edge
oEdge4 = oFaceInPart.Edges(4)
'create the proxy geometries
Dim oFaceProxy As FaceProxy
Call oOccurrence1.CreateGeometryProxy(oFaceInPart, oFaceProxy)
Dim oEdge1Proxy As EdgeProxy
Call oOccurrence1.CreateGeometryProxy(oEdge1, oEdge1Proxy)
Dim oEdge2Proxy As EdgeProxy
Call oOccurrence1.CreateGeometryProxy(oEdge2, oEdge2Proxy)
Dim oEdge3Proxy As EdgeProxy
Call oOccurrence1.CreateGeometryProxy(oEdge3, oEdge3Proxy)
Dim oEdge4Proxy As EdgeProxy
Call oOccurrence1.CreateGeometryProxy(oEdge4, oEdge4Proxy)
Dim oEdgeCol As EdgeCollection
oEdgeCol = ThisApplication.TransientObjects.CreateEdgeCollection()
'method 1: creates a new ChamferFeature defined by a specified distance
Call oEdgeCol.Add(oEdge1Proxy)
Call oEdgeCol.Add(oEdge2Proxy)
Call oAssDef.Features.ChamferFeatures.AddUsingDistance(oEdgeCol, "0.1 in")
'method 2: creates a new ChamferFeature that is defined by a distance and at a specified angle to an input face
oEdgeCol.Clear()
Call oEdgeCol.Add(oEdge3Proxy)
Call oAssDef.Features.ChamferFeatures.AddUsingDistanceAndAngle(oEdgeCol, oFaceProxy, "0.2 in", 0.5233)
'creates a new ChamferFeature that is defined by two distances
oEdgeCol.Clear()
Call oEdgeCol.Add(oEdge4Proxy)
Call oAssDef.Features.ChamferFeatures.AddUsingTwoDistances(oEdgeCol, oFaceProxy, "0.1 in", "0.2 in")
EndSub
For choice 2, we can manipulate the part definition directly and save the part document. In this code, I found an issue: after the face/edge object in part is used by one chamfer method, they seem to be broken. I have to get the objects again.
Sub createChamferInPartContext()
Dim oDoc As AssemblyDocument
oDoc = ThisApplication.ActiveDocument
Dim oAssDef As AssemblyComponentDefinition
oAssDef = oDoc.ComponentDefinition
Dim oOccurrence1 As ComponentOccurrence
oOccurrence1 = oAssDef.Occurrences(1)
Dim oPart1Def As PartComponentDefinition
oPart1Def = oOccurrence1.Definition
'get face and edge in part context
Dim oFaceInPart As Face
oFaceInPart = oPart1Def.SurfaceBodies(1).Faces(3)
Dim oEdge1 As Edge
oEdge1 = oFaceInPart.Edges(1)
Dim oEdge2 As Edge
oEdge2 = oFaceInPart.Edges(2)
Dim oEdgeCol As EdgeCollection
oEdgeCol = ThisApplication.TransientObjects.CreateEdgeCollection()
'method 1: creates a new ChamferFeature defined by a specified distance
Call oEdgeCol.Add(oEdge1)
Call oEdgeCol.Add(oEdge2)
Call oPart1Def.Features.ChamferFeatures.AddUsingDistance(oEdgeCol, "0.1 in")
'method 2: creates a new ChamferFeature that is defined by a distance and at a specified angle to an input face
' after the face/edge object in part is used by one chamfer method, they seem to be broken. have to get the objects again
oEdgeCol.Clear()
oFaceInPart = oPart1Def.SurfaceBodies(1).Faces(3)
Dim oEdge3 As Edge
oEdge3 = oFaceInPart.Edges(3)
Call oEdgeCol.Add(oEdge3)
Call oPart1Def.Features.ChamferFeatures.AddUsingDistanceAndAngle(oEdgeCol, oFaceInPart, "0.1 in", 0.5233)
'creates a new ChamferFeature that is defined by two distances
' after the face/edge object in part is used by one chamfer method, they seem to be broken. have to get the objects again
oEdgeCol.Clear()
oFaceInPart = oPart1Def.SurfaceBodies(1).Faces(3)
Dim oEdge4 As Edge
oEdge4 = oFaceInPart.Edges(4)
Call oEdgeCol.Add(oEdge4)
Call oPart1Def.Features.ChamferFeatures.AddUsingTwoDistances(oEdgeCol, oFaceInPart, "0.1 in", "0.2 in")
Call oPart1Def.Document.Save()
EndSub