Mod the Machine

Fusion 360 JavaScript API support ending this December

We stopped fully supporting the JavaScript API a few years ago, but your existing add-ins using it kept running.
Not anymore. In December they will stop running, and you need to migrate your add-ins to another programming language: either C++ or Python.

See post from product management: Notice: Javascript API is being fully retired

Edit: looks like now there is also a pop-up dialog warning you if you have a JavaScript add-in installed:

-Adam

Generate flat pattern for 3d folded sheet metal files

I vaguely remember now seeing this before, but could not recall it when someone asked about it the other day, that Inventor can generate flat pattern for any folded sheet metal model, without having to first create all the related sheet metal features (bend, flange, etc) by hand.

In this case I started with opening a STEP file of the 3D folded sheet metal. When I select "Convert To Sheet Metal" then I need to select the base face for the sheet metal, and then the thickness will be automatically populated with the correct value.

There is no dedicated function in the Inventor API for that very last part about finding out the thickness.
However, we can use things like FindUsingRay() to find the face opposite the one we want to use as the base, and then check the distance between them

There are two ways to open a non-Inventor file: simply use the Documents.Open() function, in which case the file will be converted, or through ComponentDefinition.ImportedComponents, in which case you can also decide to reference the file - see Import AnyCAD documents associatively

When doing this whole thing through the API, then you have to find a way to figure out which face should be used as base. One option could be looking for the largest planar face.
Once you have that you need to find the face opposite that and check the distance between them. That should provide the thickness of the sheet metal.

Here is a VBA sample showing this:

Function GetThickness(sb As SurfaceBody) As Double
  ' Find biggest face
  Dim f As Face
  Dim bf As Face
  Dim area As Double
  For Each f In sb.Faces
    ' Only care about planar faces
    If TypeOf f.Geometry Is Plane And f.Evaluator.area > area Then
      Set bf = f
      area = f.Evaluator.area
    End If
  Next
  
  ' Find the opposite face
  Dim p As Plane
  Set p = bf.Geometry
  
  Dim pt1 As Point
  Set pt1 = bf.PointOnFace
  
  Dim tr As TransientGeometry
  Set tr = ThisApplication.TransientGeometry
  
  Dim objs As ObjectsEnumerator
  Dim pts As ObjectsEnumerator
  Dim n As UnitVector
  ' We have to search in the opposite direction
  ' of the face's normal vector
  If bf.IsParamReversed Then 
    Set n = p.Normal 
  Else 
    Set n = tr.CreateUnitVector( _ 
      -p.Normal.x, -p.Normal.y, -p.Normal.z) 
  End If
  ' objs(2) should be the opposite face
  ' but we do not need it, the intersection point
  ' is enough, i.e. pts(2)
  Call sb.FindUsingRay(pt1, n, 0, objs, pts)
  
  ' The first point found will be on the same face
  ' The second one will be on the face opposite
  Dim pt2 As Point
  Set pt2 = pts(2)
  
  GetThickness = pt1.DistanceTo(pt2)
End Function

Sub ConvertToSheetMetal()
  Dim path As String: path = "C:\Temp\SheetMetal_0.05in.stp"
  
  Dim doc As PartDocument
  Set doc = ThisApplication.Documents.Open(path)
  
  ' Turn it into a sheet metal part
  doc.SubType = "{9C464203-9BAE-11D3-8BAD-0060B0CE6BB4}"
  
  Dim cd As SheetMetalComponentDefinition
  Set cd = doc.ComponentDefinition
 
  cd.UseSheetMetalStyleThickness = False
  cd.Thickness.Value = GetThickness(cd.SurfaceBodies(1))
  
  Call cd.Unfold
End Sub

And the result:

If the part is not really a folded sheet metal, then though the Unfold "succeeds", the body of the "Folded Model" and the "Flat Pattern" will be the same.  
You can test this by comparing the bodies:

Sub TestFlatPattern()
  Dim doc As PartDocument
  Set doc = ThisApplication.ActiveDocument
  
  Dim cd As SheetMetalComponentDefinition
  Set cd = doc.ComponentDefinition
  
  Dim tr As TransientBRep
  Set tr = ThisApplication.TransientBRep
  
  Dim objs As ObjectCollection
  Set objs = ThisApplication.TransientObjects.CreateObjectCollection
  Call objs.Add(cd.SurfaceBodies(1))
  Call objs.Add(cd.FlatPattern.SurfaceBodies(1))
  Set objs = tr.GetIdenticalBodies(objs)
  
  If objs.Count > 0 Then
    MsgBox ("The flat pattern body is the same as the original body")
  End If
End Sub

-Adam

Get Named Face of iPartFactory

One enhancement in Inventor 2019 was the ability to Assign Name to objects - see iLogic Enhancements

I wrote about how you could automate that in Automate creation of Named Geometry

This feature is something that you could also use to mark objects in an iPart factory and use that later on to find them when its member is used in an assembly.

Here is an article on the difficulties of finding derived objects in iPart members: Get edge in derived part that drives work point 

Let's say we have these files:

The Named Face in the iPart Factory will not show up in the iPart Member, so we'll have to figure out the connection ourselves using the ReferencedEntity property of the Face in the member document.   

Once we have that we need to also get the Face Proxy representing the specific Face of the iPart Member inside the Assembly, so that we can do things with it, like selecting it in the UI.

We can achieve all that using the following code - this is VBA 

Sub TestSelectNamedFace()
  Dim selSet As SelectSet
  Set selSet = ThisApplication.ActiveDocument.SelectSet

  Dim occ As ComponentOccurrence
  Set occ = selSet(1)
  
  Call selSet.Clear
  
  Call selSet.Select(GetNamedFace(occ, "MyFace"))
End Sub

Function GetNamedFace(occ As ComponentOccurrence, name As String) As Face
  Dim memberDoc As PartDocument
  Set memberDoc = occ.Definition.Document
  
  If Not memberDoc.ComponentDefinition.IsiPartMember Then
    Call MsgBox("Not an iPart member based occurrence")
  End If
  
  Dim factoryDoc As PartDocument
  Set factoryDoc = memberDoc.ComponentDefinition. _
    iPartMember.ReferencedDocumentDescriptor.ReferencedDocument
    
  Dim addin As ApplicationAddIn
  Set addin = ThisApplication.ApplicationAddIns. _
    ItemById("{3BDD8D79-2179-4B11-8A5A-257B1C0263AC}")
  
  Dim iLogicAuto As Object
  Set iLogicAuto = addin.Automation
  
  Dim namedEntities As Object
  Set namedEntities = iLogicAuto.GetNamedEntities(factoryDoc)
  
  Dim f As Face
  Set f = namedEntities.FindEntity(name)
  
  If f Is Nothing Then
    Call MsgBox("Did not find named Face")
  End If
  
  Dim f2 As Face
  For Each f2 In memberDoc.ComponentDefinition.SurfaceBodies(1).Faces
    If f2.ReferencedEntity Is f Then
      ' Get the face into the context of the assembly
      Call occ.CreateGeometryProxy(f2, GetNamedFace)

      Exit Function
    End If
  Next
End Function

First select the relevant occurrence in the assembly then run the code:

You can find info on NamedEntities object and its functions like FindEntity() here 

-Adam