insert an instance of a component and constrain
You need to define the edge in the context of the assembly, not the part. In other words, you need a full path to the edge. As you said, you now have two of these parts in your assembly so if you just specify the edge in the part, how does Inventor know which edge you're referring to? The "full path" to the edge means also specify which occurrence and all of that information is packaged in an EdgeProxy. So the solution is to create a proxy to the edge. The changes to your code are highlighted in red below.
If oRad1 = oRad Then
' take a copy of part and insert
Dim oOccurence As ComponentOccurrence
Set oOccurence = oOccurences.Add(oPath, Omatrix)
Set oDoc2 = oOccurence.Definition.Document
Set oEdge = oDoc2.AttributeManager.FindObjects("iSert")
Dim newEdge as EdgeProxy
call oOccurrence.CreateGeometryProxy(oEdge, newEdge)
Set oInsert = AssmDoc.ComponentDefinition.Constraints.AddInsertConstraint(newEdge, oEdgeH, True, 0)
Set oEdge = Nothing
Set oDoc2 = Nothing
End If
Ahh!
It's failing here, that's why the constraint doesn't work.
The code to add the attibute is:
Dim oEdge As Edge
Set oEdge = ThisApplication.CommandManager.Pick( _
kPartEdgeCircularFilter, _
"Select the circular edge")
Dim oDoc1 As Document
Set oDoc1 = oEdge.Parent.ComponentDefinition.Document
Dim oPath As String
oPath = oDoc1.FullFileName
Dim oAttribSets As AttributeSets
Set oAttribSets = oDoc1.AttributeSets
Dim oAttribset As AttributeSet
On Error Resume Next
Set oAttribset = oEdge.AttributeSets.Add("iSert")
Call oDoc1.Update
It's difficult to tell exactly what's going on with the information you've provided. An attribute to the edge can exist in the part document, but it can also exist in the assembly, where it would actually be an attribute to the edge proxy. I assume you're creating the attribute within the part. oDoc2 is being set to the part document and querying for the attribute there, so it should find it. The edge you'll get back will be in the context of the part so a proxy will need to be constructed to use it in the assembly, but you have the code to do that too so it looks like it should be working.
Attributes can sometimes be tricky to work with because it's hard to see what's actually going on. If you don't have it already I recommend getting the Attribute Manager utility. You can get it here: http://modthemachine.typepad.com/my_weblog/2015/08/attribute-helper-update.html
I think you're on the right track. There's one thing that you might be getting hung up on though. If you have the user pick a face of a part while he's in the assembly, what's returned from the selection is a FaceProxy. If you iterate over the edges of that face, EdgeProxy objects are returned so you don't need to create a proxy for those. You're code looks correct where you're inserting the bolt and then going to the bolt document to query for attributes to find the edge of the bolt. The attribute should exist in the part and so you need to do the query there. But what's returned is the edge in the part so you'll need to create a proxy for the edge to be able to use it in the assembly.
If you still have problems, if you can post a simple test case of code and part and assembly files that can be used to reproduce it I can take a look to see where you're getting hung up.
