Manufacturing DevBlog

Inventor API: Change sketch parameters of draft view in drawing document

By Xiaodong Liang

In drawing document, draft view also contains sketch with the similar functionalities of genetic sketch in part or assembly. While it looks the dimension constraint of the sketch entities are not managed by Parameter in the document. 

With API, we can still access these parameters and manipulate them directly.  The VBA code demos a workflow to change a specific parameter of a specific sketch of a specific draft view. Since draft view could have the same name, the code uses index as a unique identification. 

 

 

Sub test()

  Call changeDraftSketchConstaintParam(1, "d0", "200 in")
  
End Sub
Sub changeDraftSketchConstaintParam(draftIndex, paramName, newV)

    Dim oDoc As DrawingDocument
    Set oDoc = ThisApplication.ActiveDocument
    
    Dim oSheet As Sheet
    Set oSheet = oDoc.ActiveSheet
    
    Dim oView As DrawingView
    Set oView = oSheet.DrawingViews(1)
    
    If oView.ViewType = kDraftDrawingViewType Then
        Dim oDraftSketch As Sketch
        Set oDraftSketch = oView.Sketches(draftIndex)
        
        If Not oDoc.ActivatedObject Is oDraftSketch Then
           oDraftSketch.Edit
        End If
        
        Dim oDim As DimensionConstraint
        For Each oDim In oDraftSketch.DimensionConstraints
            Dim oParam As Parameter
            Set oParam = oDim.Parameter
            
            If oParam.Name = paramName Then
                 oParam.Expression = newV
                  
            End If
        Next
        oDraftSketch.Solve
        oDraftSketch.ExitEdit
    End If
    oDoc.Update
End Sub . 

iLogic does not provide a direct module to access these parameters, but the same VBA code could be used in iLogic with just a little bit modification:

Sub Main()

  Call changeDraftSketchConstaintParam(1, "d0", "200 in")
  
End Sub

Sub changeDraftSketchConstaintParam(draftIndex, paramName, newV)

    Dim oDoc As DrawingDocument
    oDoc = ThisApplication.ActiveDocument
    
    Dim oSheet As Sheet
    oSheet = oDoc.ActiveSheet
    
    Dim oView As DrawingView
    oView = oSheet.DrawingViews(1)
    
    If oView.ViewType = kDraftDrawingViewType Then
        Dim oDraftSketch As Sketch
         oDraftSketch = oView.Sketches(draftIndex)
        
        If Not oDoc.ActivatedObject Is oDraftSketch Then
           Call oDraftSketch.Edit()
        End If
        
        Dim oDim As DimensionConstraint
        For Each oDim In oDraftSketch.DimensionConstraints
            Dim oParam As Parameter
            oParam = oDim.Parameter
            
            If oParam.Name = paramName Then
                 oParam.Expression = newV
                  
            End If
        Next
        Call oDraftSketch.Solve()

        Call oDraftSketch.ExitEdit()
    End If
    Call oDoc.Update()
End Sub

  

Inventor API: Detect a Content Center part is inserted as standard or custom

By Xiaodong Liang

When we place a part to the assembly, it could be a common part, or a part from content center yet as standard, or the content center part as custom. Sometimes we would need to know which type part is inserted. 

To differentiate the UI >> [Place] or [Place from Content Center], the first I thought of is the event: UserInputEvents::OnActivateCommand. For UI>>[Place], it can tell a meaningful name, but for UI >> [Place from Content Center], it only tells a command "InteractionEvents"  which will also happen with some other UI operations. It cannot either tell as standard or as custom. In addition, the placing would be performed by an API code, the command name cannot over everything. 

So I turned to check the other event: AssemblyEvents::OnNewOccurrence. It can provide the final component definition after the part is inserted, by the definition, we could check if it is a content center part as standard by PartComponentDefinition::IsContentMember. As to the content center part as custom, it looks we have to check the properties of the document because a content center part will have some special property sets than the common part, even if it has been converted to as custom part. The other blog tells more. 

Based on the investigation, I produced a demo VBA code as below. Hope it helps.

Download TestProject

'module

Dim oClass As TestEvenClass
Sub startEvent()
    Set oClass = New TestEvenClass
    
    oClass.ini
    
    Do While True
        DoEvents
    Loop

End Sub

'event class
Public WithEvents oAssEvents As AssemblyEvents 

Public Sub ini()
  Set oAssEvents = ThisApplication.AssemblyEvents 
End Sub
  

Private Sub oAssEvents_OnNewOccurrence(ByVal DocumentObject As AssemblyDocument, ByVal Occurrence As ComponentOccurrence, ByVal BeforeOrAfter As EventTimingEnum, ByVal Context As NameValueMap, HandlingCode As HandlingCodeEnum)

If BeforeOrAfter = kAfter Then
    
    For Index = 1 To Context.Count

        Dim oContextName As String
        oContextName = Context.Name(Index)
            
        If oContextName = "ComponentDefinition" Then
        
            Dim oDef As ComponentDefinition
            Set oDef = Context.Value(Context.Name(Index))
            
            If TypeOf oDef Is PartComponentDefinition Then
            
                Dim oPartDef As PartComponentDefinition
                Set oPartDef = oDef
                
                If oPartDef.IsContentMember Then
                    'this is a part from content center in standard way
                    Debug.Print "This is a part from Content Center "
                Else
                
                   ' check if it is common part of custom part of Content Center
                   
                   Dim isCustomPart As Boolean
                   isCustomPart = False
                   
                   Dim oPropertySets As PropertySets
                   Set oPropertySets = oPartDef.Document.PropertySets
                   
                   Dim oEachProSet As PropertySet
                   Dim oEachP As Property

                    For i = 1 To oPropertySets.Count

                        ' use the 6th propertyset of [ContentCenter].
                        ' If it is a Custom part, there is only one property within this property set.
                        ' The name is “IsCustomPart”. While if it is a Standard CC part, there are some properties
                        ' to indicate the information of the CC such as family, member etc..
                        
                        'the internal name of this propertyset is not same across different content center part
                        'so, it looks we have to use display name, which assumes no user defined property set with the same name.

                        Set oEachProSet = oPropertySets(i)
                        'If oEachProSet.InternalName = "{5E21919D-4082-492A-8A30-039424CD07B5}" Then
                        If oEachProSet.DisplayName = "ContentCenter" Then
                     
                            For k = 1 To oEachProSet.Count
                                Set oEachP = oEachProSet(k)
                                If oEachP.Name = "IsCustomPart" Then
                                    Dim oValue As String
                                    oValue = oEachP.Value
                                    
                                    If oValue = "1" Then
                                        isCustomPart = True
                                        Exit For
                                    End If
                                    
                                End If
                            
                            Next
                     
                        End If
                        
                        If isCustomPart Then
                            Exit For
                        End If
                       
                    Next
                    If isCustomPart Then
                        Debug.Print "This is a custom part from content center"
                             
                    Else
                        Debug.Print "This is a common part"
                    End If
                   
                End If
            End If
        End If

    Next
    
End If

End Sub
 

Batch remove FEA links

By Xiaodong Liang

In the same time when I tested the code in the other blog, my colleague Henry Huang in product support team shared a code that can batch delete FEA OLE links. The code is provided by the engineer Paul Zeng. The code is well written. I believe it will be help many other customers. 

Thank you Paul, Henry!

Sub DeleteFEALinksForFolder()
  
    'add search paths
    Dim DicList
    Set DicList = CreateObject("Scripting.Dictionary")
    
    Const SearchPath = "C:\Users\zengp\Desktop\Inv_11229\" 'add more paths if you have
    DicList.Add SearchPath, ""
      
    'collect all folders
    Dim FileList, I
    Set FileList = CreateObject("Scripting.Dictionary")
    
    I = 0
    Do While I < DicList.Count
        Key = DicList.keys
        NowDic = Dir(Key(I), vbDirectory) 'start search folder
        Do While NowDic <> ""
            If (NowDic <> ".") And (NowDic <> "..") And (NowDic <> "OldVersions") Then
                If (GetAttr(Key(I) & NowDic) And vbDirectory) = vbDirectory Then 'find child folder
                    DicList.Add Key(I) & NowDic & "\", ""
                End If
            End If
            NowDic = Dir() 'continue searching
        Loop
        I = I + 1
    Loop
    
    'collect all part/assembly files
    For Each Key In DicList.keys
       NowFile = Dir(Key & "*.ipt")
       Do While NowFile <> ""
            FileList.Add Key & NowFile, "" 'Add(Key,Item)  FileList.Key=file name,FileList.Item=file path
            NowFile = Dir()
       Loop
    Next
    
    For Each Key In DicList.keys
       NowFile = Dir(Key & "*.iam")
       Do While NowFile <> ""
            FileList.Add Key & NowFile, "" 'Add(Key,Item)  FileList.Key=file name,FileList.Item=file path
            NowFile = Dir()
       Loop
    Next

    'delete FEA file links
    ThisApplication.SilentOperation = True
    
    For Each strFileName In FileList.keys
        DeleteFEALinksForSingleFile (strFileName)
    Next

    ThisApplication.SilentOperation = False
    
End Sub

Sub DeleteFEALinksForSingleFile(strFullFileName As String)

    Dim oDoc As Document
    Set oDoc = ThisApplication.Documents.Open(strFullFileName)
    
    Dim bHasFEALinksDeleted As Boolean
    bHasFEALinksDeleted = DeleteFEALinks(oDoc)
    If bHasFEALinksDeleted Then
        Call oDoc.Save
        Debug.Print strFullFileName
    End If
    
    Call oDoc.Close
End Sub


Function DeleteFEALinks(oDoc As Document) As Boolean 'if delete links
    DeleteFEALinks = False
    
    Dim oReferencedOLEFileDescriptors As ReferencedOLEFileDescriptors
    Set oReferencedOLEFileDescriptors = oDoc.ReferencedOLEFileDescriptors
    
    Dim oOLEFileDescriptor As ReferencedOLEFileDescriptor
    For Each oOLEFileDescriptor In oReferencedOLEFileDescriptors
        Dim strFileName As String
        strFileName = oOLEFileDescriptor.FullFileName
              
        If (IsFEAOLELinkFile(strFileName)) Then
          'Debug.Print "Break FEA OLE file link: " + strFileName
          DeleteFEALinks = True
          Call oOLEFileDescriptor.Delete
        End If
    Next
    
End Function

Function IsFEAOLELinkFile(strFileName As String) As Boolean
    IsFEAOLELinkFile = False

    Dim FEAFileExtArr() As Variant
    FEAFileExtArr = Array(".fins", ".fsat", ".ftes", ".fwiz", ".fmsh", ".fres")
    
    For Each strFileExt In FEAFileExtArr
      If (InStr(strFileName, strFileExt) > 0) Then
        IsFEAOLELinkFile = True
        Exit For
      End If
    Next

End Function

Remove OLE Links using ReferencedOLEFileDescriptor

By Xiaodong Liang

A few years ago, my colleague Wayne composed a blog on how to remove missing OLE links. Recently, a customer wanted to remove any OLE links when checking in to Vault. Ideally, he needs an iLogic code. So I refactored a little with the code Wayne demoed in VBA and iLogic:

Sub Main()
 
    Dim oDoc As Document
    oDoc = ThisApplication.ActiveDocument
    
    
    If TypeOf oDoc Is AssemblyDocument Then
            Call compositeDoc(oDoc)
    ElseIf TypeOf oDoc Is PartDocument Then
             Call singleDoc(oDoc)
    ElseIf TypeOf oDoc Is DrawingDocument Then
             Call singleDoc(oDoc)
    Else
    	Call MsgBox("wrong file type!") 
    End If
    
    Call oDoc.Update2(True)
     
  
End Sub
 

Sub singleDoc(doc)
        
    Dim oEachOLEDesc As ReferencedOLEFileDescriptor
    For Each oEachOLEDesc In doc.ReferencedOLEFileDescriptors
        oEachOLEDesc.Delete
        doc.Dirty = True
    Next
     
   
End Sub
 
Sub compositeDoc(parentAssDoc)
 
     'remove links of top document
     Call singleDoc(parentAssDoc)

    'remove links of sub document
     For Each oEachDesc In parentAssDoc.ReferencedDocumentDescriptors
        Dim doc As Document
        doc = oEachDesc.ReferencedDocument
        
        Dim oEachOLEDesc As ReferencedOLEFileDescriptor
        For Each oEachOLEDesc In doc.ReferencedOLEFileDescriptors
            oEachOLEDesc.Delete
            doc.Dirty = True
        Next
       
        If TypeOf doc Is AssemblyDocument Then
            Call compositeDoc(doc)
        End If
    Next
   
End Sub

The below code is written in VBA.

Sub breakLinks()
 
    Dim oDoc As Document
    Set oDoc = ThisApplication.ActiveDocument
    
    
    If TypeOf oDoc Is AssemblyDocument Then
            
            
            Call compositeDoc(oDoc)
    ElseIf TypeOf oDoc Is PartDocument Then
             Call singleDoc(oDoc)
    ElseIf TypeOf oDoc Is DrawingDocument Then
             Call singleDoc(oDoc)
    Else
    
        Call MsgBox("wrong file type!")
            
    End If
    
    Call oDoc.Update2(True)
     
  
End Sub
 

Sub singleDoc(doc)
        
    Dim oEachOLEDesc As ReferencedOLEFileDescriptor
    For Each oEachOLEDesc In doc.ReferencedOLEFileDescriptors
        oEachOLEDesc.Delete
        doc.Dirty = True
    Next
     
   
End Sub
 
Sub compositeDoc(parentAssDoc)
 
      'remove links of top document
     Call singleDoc(parentAssDoc)

      'remove links of sub document
     For Each oEachDesc In parentAssDoc.ReferencedDocumentDescriptors
        Dim doc As Document
        Set doc = oEachDesc.ReferencedDocument
        
        Dim oEachOLEDesc As ReferencedOLEFileDescriptor
        For Each oEachOLEDesc In doc.ReferencedOLEFileDescriptors
            oEachOLEDesc.Delete
            doc.Dirty = True
        Next
       
        If TypeOf doc Is AssemblyDocument Then
            Call compositeDoc(doc)
        End If
    Next
   
End Sub

Get Specific Table Row of Content Center Family

By Xiaodong Liang

In general, we call ContentFamily.CreateMember to create the instance of a content family row by inputting index of this row. However, sometimes, we would need to pick one row which has specific cell value such as diameter, radius, length etc. I do not find a direct way to get specific table row. while we could still iterate the table rows and find out the specific item by the cell value(s).

In the other blog, my colleague Adam shared a code demo on how to get specific family. I produced another code based on that. The code tries to get the table row with one column: 'radius is 0.25". 

Note: the method ContentTableRow.GetCellValue accepts the column index, or its internal name. e.g. in this case, the internal name of column 'radius' is 'RR'. In addition,  in this demo code, I input one column only, however obviously, in family 'Bolt GB/T 35', there are many rows whose radius is also '0.25'.  So you would need to input other columns and cell values, in order to get the unique row.

One more thing: if you have known the member id of a row, you could also get ContentTableRow by a direct method:ContentCenter.GetContentObject. In the blog, my colleague Wayne introduced it. 

 

Public Function GetFamily( _
name As String, node As ContentTreeViewNode) _
As ContentFamily
  Dim cc As ContentCenter
  Set cc = ThisApplication.ContentCenter
    
  If node Is Nothing Then Set node = cc.TreeViewTopNode
  
  Dim cf As ContentFamily
  For Each cf In node.Families
     
    
    If cf.DisplayName = name Then
      Set GetFamily = cf
      Exit Function
    End If
  Next
  
  Dim child As ContentTreeViewNode
  For Each child In node.ChildNodes
    Set cf = GetFamily(name, child)
    If Not cf Is Nothing Then
      Set GetFamily = cf
      Exit Function
    End If
  Next
End Function

'input: specific content family
'       internal name of specific ContentTableColumn (ContentTableColumn.internalName)
'       the cell value of this column

'Note: you would need to input other columns and cell values, in order to get the unique row.
Public Function GetSpecificRow(cf As ContentFamily, colInternalName As String, cellValue As Variant)

    Dim oRow As ContentTableRow
    Dim oCol As ContentTableColumn
    
    Dim oFound As Boolean
    oFound = False
    For Each oRow In cf.TableRows

        'check the cell value of the specific column
        Dim oCellV As String
        oCellV = oRow.GetCellValue(colInternalName)
        If oCellV = cellValue Then
            oFound = True
            Exit For
        End If
    Next

    If oFound Then
      Set GetSpecificRow = oRow
    Else
      Set GetSpecificRow = Nothing
    End If
    
    
End Function

Public Sub CcTest()
   Dim asm As AssemblyDocument
   Set asm = ThisApplication.ActiveDocument
    
   'get specific family
   Dim cf As ContentFamily
   Set cf = GetFamily("Bolt GB/T 35", Nothing)
   
   'get specific table row
   Dim oOneTableRow As ContentTableRow
   Set oOneTableRow = GetSpecificRow(cf, "RR", "0.25")
   
   'create this member
   Dim member As String
   Dim ee As MemberManagerErrorsEnum
   member = cf.CreateMember(oOneTableRow, ee, "Problem")
   
   Dim tg As TransientGeometry
   Set tg = ThisApplication.TransientGeometry
   
   'inser the member to the assembly
   Call asm.ComponentDefinition.Occurrences.Add( _
    member, tg.CreateMatrix())
End Sub

Fusion 360 API: Work with Custom Palette

By Xiaodong Liang

I played with custom palette these days. I am sharing some practices. 

Firstly, the API help sample is a very good tutorial for us to get started with. Basically, the skeleton of palette is HTML, auxiliary js , css (except the js libraries of Fusion 360), the corresponding Fusion code (Python/C++) that consumes the HTML. 

When I was playing, I happened to hit an issue. The HTML elements were not shown up. It was only a white page. After checking with engineer team, it is addressed as a problem: current API does not encode the path of the local html which contains invalid character(such as space). This fix will be available soon. If you are testing right now, please put the dataset on a path without invalid character.

As said above, the skeleton of palette can include auxiliary js , css, which means we could apply with some nicer UI such as Bootstrap and the frameworks such as Jquery. The usage is simply like what you do in other web application. 

After the HTML is ready, I'd strongly suggest you open it to test it. It will be more easier to find out some problems. e.g. check the basic behavior of buttons, dropdown, checkbox, the workflows. The only that cannot test are the calls of Fusion 360., however you could at least check the parameters that are for communications with Fusion. In my test, I wanted to make a custom Export dialog. I have not made it work with [Choose Path] . The chooser does not show up.  In addition, I am working to add the workflow  [save to cloud]. 

 

When the HTML and its workflow are ready, load the add-in to Fusion. If you do not want to debug, you could still view the HTML source or inspect element exactly like we program in web page. The browser engine Fusion uses is Chrome on Windows OS, Safari on Mac. 

 

 

 

 

 

HTML and Js code

Fusion Add-In code

Fusion 360 API: Transform Component

By Xiaodong Liang

There are some posts on Autodesk forum about translating or rotating component in the assembly. This blog is mainly for sort them out. 

The object Occurrence.transform manages the transformation this component locates relatively to the space of assembly. It is  Matrix3D which is a standard math object. you could either make static method to build the translation, transformBy a matrix (Matrix3D.transformBy, or edit the cells (Matrix3D.setCell). Calling the transform property of the Occurrence object creates a new matrix that contains the current transform information of the occurrence and returns this matrix.  The matrix doesn't have any relationship back to the occurrence so changing information in the matrix has not affect on the occurrence.  So, the correct way to update the transformation is to get the existing transform as a matrix, change data within the matrix and then assign it back to the occurrence.  The matrix being assigned back to the occurrence can come from anywhere.  The assignment then update the internal transform of the occurrence.

The following is a code snippet on translating one component, and rotate another component. It shows a couple ways to update transformation. The comments enclosed explain the corresponding methods. 

Another trick in this demo is: to make an animation of the transforming, you will need to call doEvents after each transformation updates.  doEvents function temporarily halts the execution of the add-in or script and gives Fusion 360 a chance to handle any queued up messages.  

 

 

#Author-
#Description-


import adsk.core, adsk.fusion, adsk.cam, traceback,threading
import math
import time



times = 0


def eachMove():
    ui = None
    try:
        app = adsk.core.Application.get()
        ui  = app.userInterface


        #get product        
        product = app.activeProduct
        design = adsk.fusion.Design.cast(product)
        if not design:
            ui.messageBox('No active Fusion design', 'No Design')
            return


        # Get the root component of the active design.
        rootComp = design.rootComponent
        #get array of occurrences
        occurrences = rootComp.occurrences.asList
        
        #get first component
        occurrence_first = occurrences.item(0)
        
         #get second component
        occurrence_second= occurrences.item(1)
        
        #get thrid component
        occurrence_third= occurrences.item(2)
        
       
        while (times < 20):           
            
            #translate the first component by updating [translation] property

            #wrong way: occurrence.transform will clone and return a matrix
            #so any change on this cloned matrix does not take effect on the 
            #update of component
            #offsetVector = adsk.core.Vector3D.create(5.0, 0, 0)
            #occurrence.transform.translation.add( offsetVector )
        
            # Get the current transform of the first occurrence
            transform = occurrence_first.transform
            
            if times <10:
                # Change the transform data by moving 5.0cm on X+ axis
                transform.translation = adsk.core.Vector3D.create( transform.translation.x +  5.0, 0, 0)
            else:
                # Change the transform data by moving 5.0cm on X- axis
                transform.translation = adsk.core.Vector3D.create( transform.translation.x -  5.0, 0, 0)
                
            # Set the tranform data back to the occurrence
            occurrence_first.transform = transform
            
            # Get the current transform of the second occurrence
            transform = occurrence_second.transform
            
            
            rotX = adsk.core.Matrix3D.create()
            # Change the transform data by rotating around Z+ axis

            rotX.setToRotation(math.pi/4, adsk.core.Vector3D.create(0,0,1), adsk.core.Point3D.create(0,0,0))
            transform.transformBy(rotX)
            
             # Set the tranform data back to the occurrence
            occurrence_second.transform = transform
            
             # Get the current transform of the third occurrence
            transform = occurrence_third.transform
            
            if times <10:
                # Change the transform data by moving 5.0cm on Y+ axis
                transform.setCell(1,3,transform.getCell(1,3) + 5.0)
            else:
                # Change the transform data by moving 5.0cm on Y- axis
                transform.setCell(1,3,transform.getCell(1,3) - 5.0)
                 

            #rotate around Z+ axis
            rotZSin = math.sin(math.pi/4 * times)
            rotZCos = math.cos(math.pi/4 * times)
            
            #change the cells value 
            transform.setCell(0,0,rotZCos)
            transform.setCell(0,1,rotZSin)
            transform.setCell(1,0,-rotZSin)
            transform.setCell(1,1,rotZCos) 
            
             # Set the tranform data back to the occurrence
            occurrence_third.transform = transform
            
            
            global times
            times =times +1 
            time.sleep( 0.1 )

            #Calling doEvents gives it a chance to catch up each time the components are transformed. 
            adsk.doEvents() 

       
        
       
    except:
        if ui:
            ui.messageBox('Failed:\n{}'.format(traceback.format_exc()))


def run(context): 
    global times
    times = 0
    eachMove() 
   

click the picture to see the gif.

Fusion 360 API: Customized Export Dialog

By Xiaodong Liang

This is a solution described in the forum post. The blog is basically for making the related codes be more searchable. 

The built-in dialog of [Export] is not customizable currently. While the API provides an object FileDialog that can be a workaround. i.e. make your own Export dialog and specify the parameters you would like to have such as file path and file type. This dialog is still a traditional type. I will write another blog on how to make an HTML dialog like the same style of built-in Export dialog.

 

 

 

import adsk.core, adsk.fusion, traceback

def run(context):
    ui = None
    try:
        app = adsk.core.Application.get()
        ui = app.userInterface
        filedlg = ui.createFileDialog()
        filedlg.initialDirectory = '/Users'
        filedlg.filter = '*.f3d'
        if filedlg.showSave() == adsk.core.DialogResults.DialogOK:
            design = adsk.fusion.Design.cast(app.activeProduct)
            option = design.exportManager.createFusionArchiveExportOptions(filedlg.filename, design.rootComponent)
            design.exportManager.execute(option)
    except:
      if ui:
          ui.messageBox('Failed:\n{}'.format(traceback.format_exc()))

Fusion API: Add Simple Extrude Feature and Add by Input

By Xiaodong Liang

In the past, when creating the extrude feature, we will need to create an ExtrudeInput firstly, then add the extrude feature with the input. The input is like a definition of the feature, with which, some parameters of the feature can be defined. One of the benefits is the ExtrudeFeatures.Add method would not be changed for long term. When any new parameter of creating feature is appended, the API specifies can only add more properties withExtrudeInput. 

However, quoted from the latest news of Fusion 360 API: With the recent changes to the Extrude feature the API to create extrusions got quite a bit more complicated. However, we recognized that even though the feature is more powerful and provides a lot more capabilities, the majority of the time people still create simple finite extrusions. To make this more common workflow easier, we've added a new addSimple. method to the ExtrudeFeatures collection. This makes creating an extrusion much simpler than it ever was before with a single API call.

So, you could decide to use the previous way or the simple way based on your requirement. The following is a code snippets from the API sample on the two scenarios. 

Python

#Author-
#Description-

import adsk.core, adsk.fusion, adsk.cam, traceback

def run(context):
    ui = None
    try:
        app = adsk.core.Application.get()
        ui  = app.userInterface
        
        #crreate a document
        doc = app.documents.add(adsk.core.DocumentTypes.FusionDesignDocumentType)
        
        product = app.activeProduct
        design = adsk.fusion.Design.cast(product)
        
        #get the root component of the active design
        rootComp = design.rootComponent
        
        # Get extrude features
        extrudes = rootComp.features.extrudeFeatures  
        
        # create a sketch
        sketches = rootComp.sketches
        sketch1 = sketches.add(rootComp.xZConstructionPlane)
        sketchCircles = sketch1.sketchCurves.sketchCircles
        centerPoint = adsk.core.Point3D.create(0, 0, 0)
        sketchCircles.addByCenterRadius(centerPoint, 3.0)

        # Get the profile defined by the circle.
        prof_simple = sketch1.profiles.item(0) 
        
        # Extrude Sample 1: A simple way of creating typical extrusions (extrusion that goes from the profile plane the specified distance).
        # Define a distance extent of 5 cm
        distance = adsk.core.ValueInput.createByReal(5) 
        extrude_simple = extrudes.addSimple(prof_simple, distance, adsk.fusion.FeatureOperations.NewBodyFeatureOperation) 
        # Get the extrusion body
        body_simple = extrude_simple.bodies.item(0) 
        body_simple.name = "simple extrude feature" 
        
        #Create another sketch
        sketch2 = sketches.add(rootComp.xZConstructionPlane) 
        sketchCircles2 = sketch2.sketchCurves.sketchCircles 
        sketchCircles2.addByCenterRadius(centerPoint, 13.0) 
        sketchCircles2.addByCenterRadius(centerPoint, 15.0) 
        prof_for_input = sketch2.profiles.item(1) 
        
        # Create taper angle value inputs
        deg0 = adsk.core.ValueInput.createByString('0 deg') 
        deg2 = adsk.core.ValueInput.createByString('2 deg') 
        deg5 = adsk.core.ValueInput.createByString('5 deg') 
        
        #Create distance value inputs
        mm10 = adsk.core.ValueInput.createByString('10 mm') 
        mm100 = adsk.core.ValueInput.createByString('100 mm') 

        # Extrude Sample 2: Create an extrusion that goes from the profile plane with one side distance extent
        extrudeInput = extrudes.createInput(prof_for_input, adsk.fusion.FeatureOperations.NewBodyFeatureOperation) 
        # Create a distance extent definition
        extent_distance = adsk.fusion.DistanceExtentDefinition.create(mm100) 
        extrudeInput.setOneSideExtent(extent_distance, adsk.fusion.ExtentDirections.PositiveExtentDirection) 
        # Create the extrusion
        extrude_by_input = extrudes.add(extrudeInput) 
        # Get the body of extrusion
        body_by_input = extrude_by_input.bodies.item(0) 
        body_by_input.name = "extrude feature by input" 
        

    except:
        if ui:
            ui.messageBox('Failed:\n{}'.format(traceback.format_exc()))

 

JavaScript

function run(context) {

    "use strict";
    if (adsk.debug === true) {
        /*jslint debug: true*/
        debugger;
        /*jslint debug: false*/
    }
 
    var ui;
    try {
        var app = adsk.core.Application.get();
        ui = app.userInterface;
        
        // Create a document.
        var doc = app.documents.add(adsk.core.DocumentTypes.FusionDesignDocumentType);
 
        var product = app.activeProduct;
        var design = adsk.fusion.Design(product);

        // Get the root component of the active design
        var rootComp = design.rootComponent;
        
        // Get extrude features
        var extrudes = rootComp.features.extrudeFeatures; 
        
        // Create sketch
        var sketches = rootComp.sketches;
        
        var sketch1 = sketches.add(rootComp.xZConstructionPlane);
        var sketchCircles = sketch1.sketchCurves.sketchCircles;
        var centerPoint = adsk.core.Point3D.create(0, 0, 0);
        var circle = sketchCircles.addByCenterRadius(centerPoint, 5.0);
        
        // Get the profile defined by the circle
        var prof_simple = sketch1.profiles.item(0);
        
        // Extrude Sample 1: A simple way of creating typical extrusions (extrusion that goes from the profile plane the specified distance).
        // Define a distance extent of 5 cm
        var distance = adsk.core.ValueInput.createByReal(5);
        var extrude_simple = extrudes.addSimple(prof_simple, distance, adsk.fusion.FeatureOperations.NewBodyFeatureOperation);
        // Get the extrusion body
        var body_simple = extrude_simple.bodies.item(0);
        body_simple.name = "simple extrude feature";
        
       // Create another sketch
        var sketch2 = sketches.add(rootComp.xZConstructionPlane);
        var sketchCircles2 = sketch2.sketchCurves.sketchCircles;
        sketchCircles2.addByCenterRadius(centerPoint, 13.0);
        sketchCircles2.addByCenterRadius(centerPoint, 15.0);
        var prof_for_input = sketch2.profiles.item(1);
        
        // Create taper angle value inputs
        var deg0 = adsk.core.ValueInput.createByString('0 deg');
        var deg2 = adsk.core.ValueInput.createByString('2 deg');
        var deg5 = adsk.core.ValueInput.createByString('5 deg');
        // Create distance value inputs
        var mm10 = adsk.core.ValueInput.createByString('10 mm');
        var mm100 = adsk.core.ValueInput.createByString('100 mm');

        // Extrude Sample 2: Create an extrusion that goes from the profile plane with one side distance extent
        var extrudeInput = extrudes.createInput(prof_for_input, adsk.fusion.FeatureOperations.NewBodyFeatureOperation);
        // Create a distance extent definition
        var extent_distance = adsk.fusion.DistanceExtentDefinition.create(mm100);
        extrudeInput.setOneSideExtent(extent_distance, adsk.fusion.ExtentDirections.PositiveExtentDirection);
        // Create the extrusion
        var extrude_by_input = extrudes.add(extrudeInput);
        // Get the body of extrusion
        var body_by_input = extrude_by_input.bodies.item(0);
        body_by_input.name = "extrude feature by input";
        

        
    } 
    catch (e) {
        if (ui) {
            ui.messageBox('Failed : ' + (e.description ? e.description : e));
        }
    }

    adsk.terminate(); 
}
 

 

 

Fusion API: Manage Participant Bodies

By Xiaodong Liang

This is mainly quoted from Fusion 360 help document:

In the recent update in Jan, Fusion added the ability to choose which bodies will be affected when creating certain features; extrude, hole, loft, revolve, and sweep. The input objects for each of those features and the feature objects themselves all now support a "participantBodies" property that lets you specify the set of bodies that will participate in the feature. The default is that all visible bodies that intersect the feature will be used, which was also the previous default so existing programs shouldn't see any change of behavior.

The codes below is a simple sample on how this new property works. It creates some bodies, then creates a cut feature. With participantBodies, only some of the bodies are cut. 

 

Python:

 

#Author-
#Description-

import adsk.core, adsk.fusion, adsk.cam, traceback

def run(context):
    ui = None
    try:
        app = adsk.core.Application.get()
        ui  = app.userInterface
        
        #crreate a document
        doc = app.documents.add(adsk.core.DocumentTypes.FusionDesignDocumentType)
        
        product = app.activeProduct
        design = adsk.fusion.Design.cast(product)
        
        #get the root component of the active design
        rootComp = design.rootComponent
        
        # create a sketch
        sketches = rootComp.sketches
        sketch = sketches.add(rootComp.xZConstructionPlane)
        sketchCircles = sketch.sketchCurves.sketchCircles
        centerPoint = adsk.core.Point3D.create(0, 0, 0)
        sketchCircles.addByCenterRadius(centerPoint, 3.0)

        # Get the profile defined by the circle.
        prof = sketch.profiles.item(0)

	  # Create sketch for Cut
        sketchForCut = sketches.add(rootComp.xZConstructionPlane)
        sketchForCutCircles = sketchForCut.sketchCurves.sketchCircles
        sketchForCutCircles.addByCenterRadius(centerPoint, 1.5)

        # Get the profile defined by the circle.
        profForCut = sketchForCut.profiles.item(0)

        # Create an extrusion input
        extrudes = rootComp.features.extrudeFeatures
        extInput = extrudes.createInput(prof, adsk.fusion.FeatureOperations.NewBodyFeatureOperation)

        # Define that the extent is a distance extent of 5 cm.
        distance = adsk.core.ValueInput.createByReal(5)
        extInput.setDistanceExtent(False, distance)

        # Create the extrusion.
        ext = extrudes.add(extInput)

        # Get the body created by extrusion
        body = ext.bodies.item(0)

        # Create input entities for rectangular pattern
        inputEntites = adsk.core.ObjectCollection.create()
        inputEntites.add(body)

        # Get x and y axes for rectangular pattern
        xAxis = rootComp.xConstructionAxis
        yAxis = rootComp.yConstructionAxis

        # Quantity and distance
        quantityOne = adsk.core.ValueInput.createByString('0')
        distanceOne = adsk.core.ValueInput.createByString('0 cm')
        quantityTwo = adsk.core.ValueInput.createByString('6')
        distanceTwo = adsk.core.ValueInput.createByString('15 cm')

        # Create the input for rectangular pattern
        rectangularPatterns = rootComp.features.rectangularPatternFeatures
        rectangularPatternInput = rectangularPatterns.createInput(inputEntites, xAxis, \
            quantityOne, distanceOne, adsk.fusion.PatternDistanceType.SpacingPatternDistanceType)

        # Set the data for second direction
        rectangularPatternInput.setDirectionTwo(yAxis, quantityTwo, distanceTwo)

        # Create the rectangular pattern
        rectangularFeature = rectangularPatterns.add(rectangularPatternInput)

        patBodies = rectangularFeature.bodies

        body0 = patBodies.item(0)
        face0 = body0.faces.item(0)

        extCutInput = extrudes.createInput(profForCut, adsk.fusion.FeatureOperations.CutFeatureOperation)

	  # Set the extrude input
        distanceForCut = adsk.core.ValueInput.createByString('90 cm')
        extCutInput.setDistanceExtent(False, distanceForCut)

        # set bodies to participate
        extCutInput.participantBodies = [patBodies.item(0), patBodies.item(2), patBodies.item(4)]

        extrudes.add(extCutInput)        
        

    except:
        if ui:
            ui.messageBox('Failed:\n{}'.format(traceback.format_exc()))

JavaScipt:

 

function run(context) {

    "use strict";
    if (adsk.debug === true) {
        /*jslint debug: true*/
        debugger;
        /*jslint debug: false*/
    }

    var ui;
    try {
        var app = adsk.core.Application.get();
        ui = app.userInterface;

        // Create a document.
        var doc = app.documents.add(adsk.core.DocumentTypes.FusionDesignDocumentType);

        var product = app.activeProduct;
        var design = adsk.fusion.Design(product);

        // Get the root component of the active design.
        var rootComp = design.rootComponent;

        // Create sketch
        var sketches = rootComp.sketches;
        var sketch = sketches.add(rootComp.xZConstructionPlane);
        var sketchCircles = sketch.sketchCurves.sketchCircles;
        var centerPoint = adsk.core.Point3D.create(0, 0, 0);
        sketchCircles.addByCenterRadius(centerPoint, 3.0);

        // Get the profile defined by the circle.
        var prof = sketch.profiles.item(0);

		// Create sketch for Cut
        var sketchForCut = sketches.add(rootComp.xZConstructionPlane);
        var sketchForCutCircles = sketchForCut.sketchCurves.sketchCircles;
        sketchForCutCircles.addByCenterRadius(centerPoint, 1.5);

        // Get the profile defined by the circle.
        var profForCut = sketchForCut.profiles.item(0);

        // Create an extrusion input
        var extrudes = rootComp.features.extrudeFeatures;
        var extInput = extrudes.createInput(prof, adsk.fusion.FeatureOperations.NewBodyFeatureOperation);

        // Define that the extent is a distance extent of 5 cm.
        var distance = adsk.core.ValueInput.createByReal(5);
        extInput.setDistanceExtent(false, distance);

        // Create the extrusion.
        var ext = extrudes.add(extInput);

        // Get the body created by extrusion
        var body = ext.bodies.item(0);

        // Create input entities for rectangular pattern
        var inputEntites = adsk.core.ObjectCollection.create();
        inputEntites.add(body);

        // Get x and y axes for rectangular pattern
        var xAxis = rootComp.xConstructionAxis;
        var yAxis = rootComp.yConstructionAxis;

        // Quantity and distance
        var quantityOne = adsk.core.ValueInput.createByString('0');
        var distanceOne = adsk.core.ValueInput.createByString('0 cm');
        var quantityTwo = adsk.core.ValueInput.createByString('6');
        var distanceTwo = adsk.core.ValueInput.createByString('15 cm');

        // Create the input for rectangular pattern
        var rectangularPatterns = rootComp.features.rectangularPatternFeatures;
        var rectangularPatternInput = rectangularPatterns.createInput(inputEntites, xAxis,
            quantityOne, distanceOne, adsk.fusion.PatternDistanceType.SpacingPatternDistanceType);

        // Set the data for second direction
        rectangularPatternInput.setDirectionTwo(yAxis, quantityTwo, distanceTwo);

        // Create the rectangular pattern
        var rectangularFeature = rectangularPatterns.add(rectangularPatternInput);

		var patBodies = rectangularFeature.bodies;

        var body0 = patBodies.item(0);
        var face0 = body0.faces.item(0);

		var extCutInput = extrudes.createInput(profForCut, adsk.fusion.FeatureOperations.CutFeatureOperation);

		// Set the extrude input
        var distanceForCut = adsk.core.ValueInput.createByString('90 cm');
        extCutInput.setDistanceExtent(false, distanceForCut);

        //set bodies to participate
        extCutInput.participantBodies = [patBodies.item(0), patBodies.item(2), patBodies.item(4)];

		extrudes.add(extCutInput);

    }
    catch (e) {
        if (ui) {
            ui.messageBox('Failed : ' + (e.description ? e.description : e));
        }
    }

    adsk.terminate();
}