Mate 2 parts in assembly, one by face name and one by clicking it
Hi @valyyg. Here is something you may be able to use. I kept it fairly brief, since that appears to be the theme. There are 2 main ways to get 'named entities' from a document. One is by using the iLogic specific 'NamedEntities' interface. The other is a much longer and more complex bit of code that filters through all the Attributes in the document, looking for the ones with specific names and values. There are two ways to access the NamedEntities interface...one way is shown above, the other is 'ThisDoc.NamedEntities', but that one will only work on the 'active/local' document, not some other document.
Dim componentA = Components.Add("perete_intermediar", "perete_intermediar.ipt", position := Nothing, grounded := False, visible := True, appearance := Nothing)
Dim oCompADoc As Document = componentA.Occurrence.ReferencedDocumentDescriptor.ReferencedDocument
oNEs = iLogicVb.Automation.GetNamedEntities(oCompADoc)
oEntity = oNEs.TryGetEntity("edge_jos ")
If IsNothing(oEntity) Then Exit Sub
Dim oFace1 As Face = oEntity
Dim oFace2 As Face = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kPartFacePlanarFilter, "Pick a face. press Esc to cancel")
Dim oAsm As AssemblyDocument = ThisDoc.Document
oAsm.ComponentDefinition.Constraints.AddMateConstraint(oFace1, oFace2, 0)
Wesley Crihfield
(Not an Autodesk Employee)
OK. You may have an older version of Inventor, where that specific method under the NamedEntities interface did not exist yet. That's OK, because there are is another method under it you should be able to use. You can use oNEs.FindEntity("edge_jos ") instead of TryGetEntity(). But that one may throw an error if the object is not found. There is also a method under the NamedEntities interface called NameExists("EntityName"), which can be used to check if that name can be found, before using the other method which might throw the error if not found. But I'm not sure which version of Inventor that NameExists method was introduced.
Wesley Crihfield
(Not an Autodesk Employee)
That error message indicates that the code is encountering the error at the line where it is trying to create the Mate constraint, so that would be the last line. Here try this version of the code (below). I added in several bits of code to try to catch the error, or find out why it is failing.
Dim componentA = Components.Add("perete_intermediar", "perete_intermediar.ipt", position := Nothing, grounded := False, visible := True, appearance := Nothing)
Dim oCompADoc As Document = componentA.Occurrence.ReferencedDocumentDescriptor.ReferencedDocument
oNEs = iLogicVb.Automation.GetNamedEntities(oCompADoc)
Dim oEntityName As String = "edge_jos"
Dim oEntity As Object = Nothing
If oNEs.NameExists(oEntityName) = False Then
MsgBox("Could not find any entity in the document named: " & oEntityName, vbCritical, "")
Exit Sub
Else
Try
oEntity = oNEs.FindEntity(oEntityName)
Catch
MsgBox("Error trying to retrieve named entity from document.", vbCritical, "")
Exit Sub
End Try
End If
If IsNothing(oEntity) Then
MsgBox("No entity was retrieved from the document.", vbCritical, "")
Exit Sub
End If
Dim oFace1 As Face = oEntity
Dim oFace2 As Face = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kPartFacePlanarFilter, "Pick a face. press Esc to cancel")
Dim oAsm As AssemblyDocument = ThisDoc.Document
Try
oAsm.ComponentDefinition.Constraints.AddMateConstraint(oFace1, oFace2, 0)
Catch oEx As Exception
MsgBox("AddMateConstraint method failed" & vbCrLf & _
oEx.Message & vbCrLf & oEx.StackTrace, vbCritical, "")
End TryWesley Crihfield
(Not an Autodesk Employee)
Ohhh... I forgot that the face it is retrieving from the other document, is in the context of that other document, and the assembly constraint needs a reference to that face in the context of the main assembly...so it needs a FaceProxy, instead of a regular Face. I think I know what it is missing now. My brain is getting tired today.😪
Here try this:
Dim componentA = Components.Add("perete_intermediar", "perete_intermediar.ipt", position := Nothing, grounded := False, visible := True, appearance := Nothing)
Dim oCompADoc As Document = componentA.Occurrence.ReferencedDocumentDescriptor.ReferencedDocument
oNEs = iLogicVb.Automation.GetNamedEntities(oCompADoc)
Dim oEntityName As String = "edge_jos"
Dim oEntity As Face = Nothing
If oNEs.NameExists(oEntityName) = False Then
MsgBox("Could not find any entity in the document named: " & oEntityName, vbCritical, "")
Exit Sub
Else
Try
oEntity = oNEs.FindEntity(oEntityName)
Catch
MsgBox("Error trying to retrieve named entity from document.", vbCritical, "")
Exit Sub
End Try
End If
If IsNothing(oEntity) Then
MsgBox("No entity was retrieved from the document.", vbCritical, "")
Exit Sub
End If
'create the variable to hold the FaceProxy that the method below will get the reference to
Dim oFace1 As FaceProxy = Nothing
'now use this method to set the value to that variable we just created
componentA.Occurrence.CreateGeometryProxy(oEntity, oFace1)
Dim oFace2 As Face = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kPartFacePlanarFilter, "Pick a face. press Esc to cancel")
Dim oAsm As AssemblyDocument = ThisDoc.Document
Try
oAsm.ComponentDefinition.Constraints.AddMateConstraint(oFace1, oFace2, 0)
Catch oEx As Exception
MsgBox("AddMateConstraint method failed" & vbCrLf & _
oEx.Message & vbCrLf & oEx.StackTrace, vbCritical, "")
End Try
Wesley Crihfield
(Not an Autodesk Employee)
