Mod the Machine

New API's in Inventor 2020.1

For the clearance hole APIs we expose the HoleFeatures.CreateClearanceInfo and also make the HoleFeature.ClearanceInfo writable in Inventor 2020.1 so users now can create a clearance hole via API.

Here is a sample:

Sub test() 
   ' open a part document with a hole feature
   Dim oDoc As PartDocument 
   Set oDoc = ThisApplication.ActiveDocument 
     
   Dim oHole As HoleFeature 
   Set oHole = oDoc.ComponentDefinition.Features.HoleFeatures(1) 
     
   Debug.Print oHole.IsClearanceHole 
   
   ' Create a HoleClearanceInfo(not associative with any HoleFeature) 
   Dim oHCI As HoleClearanceInfo 
   Set oHCI = oDoc.ComponentDefinition.Features.HoleFeatures.CreateClearanceInfo("Ansi Unified Screw Threads", "Flat Head Machine Screw (100)", "#1", kNormalFitType) 
   Debug.Print oHCI.FastenerStandard 
   Debug.Print oHCI.FastenerType 
   Debug.Print oHCI.FastenerSize 
   Debug.Print oHCI.FastenerFitType 
   
   ' we can change the property when the HoleClearanceInfo is not associative with a HoleFeature 
   oHCI.FastenerStandard = "ISO" 
   oHCI.FastenerType = "Countersunk Flat Head Screw ISO 2009/7046" 
   oHCI.FastenerSize = "M1.6" 
   oHCI.FastenerFitType = kCloseFitType 
   
   Debug.Print "----------------------------" 
   Debug.Print oHCI.FastenerStandard 
   Debug.Print oHCI.FastenerType 
   Debug.Print oHCI.FastenerSize 
   Debug.Print oHCI.FastenerFitType 
   
   ' set the hole as a clearance hole 
   oHole.ClearanceInfo = oHCI 
   Debug.Print oHole.IsClearanceHole 
   
   ' retrieve the HoleClearanceInfo from a HoleFeature 
   Set oHCI = oHole.ClearanceInfo 
   
   Debug.Print "----------------------------" 
   Debug.Print oHCI.FastenerStandard 
   Debug.Print oHCI.FastenerType 
   Debug.Print oHCI.FastenerSize 
   Debug.Print oHCI.FastenerFitType 
   
   ' now the oHCI is associative with a HoleFeature, we don't allow to change a property(like FastenerStandard) directly on the property 
   ' but you can call the SetClearanceInfo method to change the properties, and the change will affect the HoleFeature directly 
   Call oHCI.SetClearanceInfo("Ansi Unified Screw Threads", "Flat Head Machine Screw (82)", "#8", kNormalFitType) 
   Debug.Print "----------------------------" 
   Debug.Print oHCI.FastenerStandard 
   Debug.Print oHCI.FastenerType 
   Debug.Print oHCI.FastenerSize 
   Debug.Print oHCI.FastenerFitType 
   
   ' also you can create another HoleClearanceInfo(not associative with any HoleFeature), and assign it to the HoleFeature.ClearanceInfo to change its clearance info 
   Dim onewHCI As HoleClearanceInfo 
   Set onewHCI = oDoc.ComponentDefinition.Features.HoleFeatures.CreateClearanceInfo("DIN", "Countersunk Flat Head Screw DIN EN ISO 2009", "M1.6", kNormalFitType) 
   oHole.ClearanceInfo = onewHCI 
   
   Set oHCI = oHole.ClearanceInfo 
   Debug.Print "----------------------------" 
   Debug.Print oHCI.FastenerStandard 
   Debug.Print oHCI.FastenerType 
   Debug.Print oHCI.FastenerSize 
   Debug.Print oHCI.FastenerFitType 
 
End Sub

 

The new Fusion 360 UI is here!

A new Fusion 360 toolbar UI is becoming official soon, including changes to the existing API. To ensure that your add-ins are still compatible, we highly encourage you to update your add-in using the new API: https://docs.google.com/document/d/174ISmaXs-60JRtn8bt4Sbr6Z3jqzkyoSizVD9YwChOQ/edit?usp=sharing

For convenience I'm also pasting here the content:

Tabbed Toolbar API

UserInterface class changes
http://help.autodesk.com/view/fusion360/ENU/?guid=GUID-52303e26-c1c2-4a1c-8c1a-a3c199e6db63

app = adsk.core.Application.get()
ui  = app.userInterface

Indicates if Fusion 360 is running with in the old toolbar or new toolbar:

# bool isTabbedToolbar { get; }
runningTabbedToolbar = ui.isTabbedToolbar

Gets all of the toolbar tabs. This returns all of the tabs available, regardless of which workspace or product they're associated with.

# ToolbarTabList allToolbarTabs { get; }
Similar example:  see commandDefinitions, like:  ui.commandDefinitions
allToolbarTabsList = ui.allToolbarTabs

this gets all of the toolbar tabs associated with the specified product. The full list of available products can be obtained by using the Application.supportedProductTypes property.

# ToolbarTabList toolbarTabsByProductType(string productType);
supportedProductTypesList = app.supportedProductTypes
print(supportProductTypesList)
# Example output:  ('CAMProductType', 'AnimationProductType', 'DesignProductType', 'FusionDrawingProductType', 'SimStudiesProductType')
tabsListForProduct = ui.toolbarTabsByProductType('DesignProductType')

New! ToolbarTabList class

This is a collection of ToolbarTab objects

Returns the specified tab using an index into the collection.
# ToolbarTab item(uint index);

Returns the ToolbarTab of the specified ID.
# ToolbarTab itemById(string id);

Gets the number of toolbar tabs in the collection.
# uint count { get; }

Try to get the Solid tab:
solidTab = allToolbarTabsList.itemById('SolidTab')

New! ToolbarTab class

Gets ID of tab:
# string id { get; }

Get position of this tab within its toolbar:
# uint index { get; }

Gets whether this tab is currently being displayed in the user interface
# bool isVisible { get; }

Gets the name of the tab as seen in the user interface.
# string name { get; }

Gets the collection containing the panels associated with this tab.
It's through this collection that you can add new toolbar panels.
# ToolbarTabPanels toolbarPanels { get; }

Gets the parent UserInterface object.
# UserInterface parentUserInterface { get; }    

# Returns the name of the product this toolbar tab is associated with.
# string productType { get; }   

# Make sure that it isn't null
if solidTab:
    # Found solidTab!  Ok to use it now!
    isSolidTabVisible = solidTab.isVisible
    allSolidTabPanels = solidTab.toolbarPanels

New! ToolbarTabPanels class 

Collection of ToolbarPanel objects (ToolbarPanel is existing class) 
Unlike ToolbarPanels, ToolbarTabPanels class lets you position the panel in a specific tab in relation to other panels in the toolbar. 
 
Creates a new ToolbarPanel. The panel is initially empty.
# ToolbarPanel add(string id, string name, [Optional] string positionID = "", [Optional] bool isBefore = true);

Returns the specified toolbar panel using an index into the collection.
# ToolbarPanel item(uint index);

Returns the ToolbarPanel at the specified ID.
ToolbarPanel itemById(string id);

Gets the number of panels.
# uint count { get; }

Add a new panel to a particular tab:
fancyAddinToolbarPanel = allSolidTabPanels.add('JenCompanyAddin', 'DoImportantFusionThingPanel')

ToolbarPanel class (existing class, but 1 new method)
http://help.autodesk.com/view/fusion360/ENU/?guid=GUID-0ca48ac9-da95-4623-bf87-150f3729717a

# string id { get; }
# uint index { get; }
# bool isVisible { get; }
# string name { get; }
# bool deleteMe();
# ToolbarControls controls { get; }
# UserInterface parentUserInterface { get; }
# ToolbarControlList promotedControls { get; }
# ObjectCollection relatedWorkspaces { get; set; }
# productType { get; }

New method - Gets the position this panel is in within the toolbar tab.
# uint indexWithinTab(string tabId); 

Add a control to the initially empty new toolbar panel:
ToolbarControls class:  https://help.autodesk.com/view/fusion360/ENU/?guid=GUID-df24e158-40e0-4aed-9990-97c470935dbb

fancyAddinToolbarPanelControls = fancyAddinToolbarPanel.controls

Assume JenFancyCommmandDef created already....
https://help.autodesk.com/view/fusion360/ENU/?guid=GUID-1ed0cfb5-2ad4-4285-9eec-484ef19f2729
doSomethingAmazingCmdControl = fancyAddinToolbarPanelControls.addCommand(JenFancyCommmandDef, '', False)

Workspace class (existing class, but 1 new method)

Gets the collection containing the tabs associated with this workspace.
# ToolbarTabs toolbarTabs { get; }

Get a list of all workspaces:
https://help.autodesk.com/view/fusion360/ENU/?guid=GUID-75ac7274-735c-4a61-af57-1d837c4df217

workspacesList = ui.workspaces
print (workspacesList.count)    

The above example prints 29 total workspaces in Fusion.
Note from Jennifer:  With 29 workspaces that don't match up with the new Tabbed Toolbar 
"Workspaces" as shown in the Workspace Switcher, I'm not sure how valuable 
workspaces will be for new API writers and tabbed toolbar?

Get a single workspace:
oneWorkspace = workspacesList.itemById('FusionModelingEnvironment') 

https://help.autodesk.com/view/fusion360/ENU/?guid=GUID-33f9ed37-e5c7-4153-ba85-c3254a199dd1

# Gets the collection containing the tabs associated with this workspace.
# ToolbarTabs toolbarTabs { get; }
modelingEnvToolbarTabs = oneWorkspace.toolbarTabs

New! ToolbarTabs class

Collection of ToolbarTab objects

Returns the specified toolbar tab using an index into the collection.
#  ToolbarTab item(uint index);

Returns the ToolbarTab at the specified ID.
# ToolbarTab itemById(string id);

# Gets the number of ToolbarTabs.
# uint count { get; }

In the August Update (coming around mid August), we will be making the new toolbar UI the default toolbar for Fusion 360. Users will have the option to revert back to the old toolbar, however this option will only be available for a limited period of time. The current plan is to completely transition over to the new toolbar UI by the September Update. 

If you haven’t tried out the new toolbar UI yet, you can turn it on by going to the Preferences > Preview section and checking the UI Preview option.
Here is a video of the top 5 changes to look for when using the new toolbar UI. 

The commands of existing add-ins will be redirected to the most appropriate place, but it's not always possible. In that case the command buttons will be placed in the Tools tab as a default location under the new toolbar UI. 
It's better to use the new API's to make sure your command button goes exactly where you want it 😀

Mirror Sketch Geometry

In the Sketch environment there is a Mirror command in the Pattern palette:

Unfortunately, its functionality is not directly exposed in the API. 
However, we can check what it does and try to replicate it.

When I mirror sketch geometry, I can see that the Mirror command basically copies all the sketch points and lines, and then sets up a symmetry constraint between the original and copied sketch points.

Here is a VBA sample which achieves this for sketch lines - for other geometry you would have to implement the functionality in a similar fashion:

Function CopyAndConstrainPoint(pt As SketchPoint, ln As SketchLine, pts As Dictionary) As SketchPoint
  ' The sketch we are working in
  Dim sk As PlanarSketch
  Set sk = pt.Parent
     
  ' Check if we already copied this
  ' sketch point
  If Not pts.Exists(pt) Then
    ' Create new point
    Set CopyAndConstrainPoint = sk.SketchPoints.Add(pt.Geometry, False)
    Call pts.Add(pt, CopyAndConstrainPoint)
    ' Constrain it
    Call sk.GeometricConstraints.AddSymmetry(pt, CopyAndConstrainPoint, ln)
  Else
    Set CopyAndConstrainPoint = pts(pt)
  End If
End Function

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

  ' The first selected item needs to be the
  ' mirror line
  Dim mirrorLine As SketchLine
  Set mirrorLine = selSet(1)
  
  ' The sketch we are working in
  Dim sk As PlanarSketch
  Set sk = mirrorLine.Parent
  
  ' Let's get the lines we need to mirror
  ' We need to copy the lines, the sketch points
  ' and set up a symmetry constraint between the
  ' points and the mirror line
  Dim mirroredSketchPoints As New Dictionary
  Dim sketchLines As ObjectCollection
  Set sketchLines = ThisApplication.TransientObjects.CreateObjectCollection()
  
  ' First store the selection set
  ' because it might get reset when adding new
  ' sketch entities and setting up constraints
  Dim i As Integer
  For i = 2 To selSet.Count
    If TypeOf selSet(i) Is SketchLine Then
      Call sketchLines.Add(selSet(i))
    End If
  Next
      
  Dim line As SketchLine
  For Each line In sketchLines
    ' Get the copied points
    Dim sp As SketchPoint
    Set sp = CopyAndConstrainPoint(line.StartSketchPoint, mirrorLine, mirroredSketchPoints)
    
    Dim ep As SketchPoint
    Set ep = CopyAndConstrainPoint(line.EndSketchPoint, mirrorLine, mirroredSketchPoints)
    
    ' Create the new line using the copied and constrained
    ' sketch points
    Call sk.sketchLines.AddByTwoPoints(sp, ep)
  Next
End Sub

When running it, make sure that you first select the mirror line, and then the rest of the geometry:

-Adam