Inventor API Python

[22351396]

I tried to create an assembly joint. It connects the midpoints of the edges of two faces using a rotational joint. I used python. 
My problem is that "Error creating joint definition: (-2147352567, 'Exception occurred.', (0, None, None, None, 0, -2147467259), None)"
Here is my code.

import win32com.client

def AssemblyJoint():
    # Initialize Inventor application
    invApp = win32com.client.Dispatch("Inventor.Application")
    
    # Create a new assembly document
    asmDoc = invApp.Documents.Add(12291, invApp.FileManager.GetTemplateFile(12291, 8962))
    asmDef = asmDoc.ComponentDefinition
    tg = invApp.TransientGeometry
    
    # Place an occurrence into the assembly
    matrix1 = tg.CreateMatrix()
    translation_vector1 = tg.CreateVector(0, 0, 0)
    matrix1.SetTranslation(translation_vector1)
    occ1 = asmDef.Occurrences.Add("C:\\Users\\MINHAZULISLAM\\Desktop\\API Join\\Part1.ipt", matrix1)
    
    matrix2 = tg.CreateMatrix()
    translation_vector2 = tg.CreateVector(8 * 2.54, 6 * 2.54, 2 * 2.54)  # Converting inches to cm
    matrix2.SetTranslation(translation_vector2)
    occ2 = asmDef.Occurrences.Add("C:\\Users\\MINHAZULISLAM\\Desktop\\API Join\\Part2.ipt", matrix2)

    # Print the structure of the first occurrence
    print("Occurrence 1:")
    PrintStructure(occ1)
    print("\nOccurrence 2:")
    PrintStructure(occ2)

    # Get faces and edges by index
    face1 = occ1.SurfaceBodies.Item(1).Faces.Item(1)
    face2 = occ2.SurfaceBodies.Item(1).Faces.Item(1)
    edge1 = occ2.SurfaceBodies.Item(1).Edges.Item(1)
    edge3 = occ1.SurfaceBodies.Item(1).Edges.Item(1)

    # Debugging information
    if not face1:
        print("Face1 not found")
    if not face2:
        print("Face2 not found")
    if not edge1:
        print("Edge1 not found")
    if not edge3:
        print("Edge3 not found")

    # Check if the faces and edges were found
    if not face1 or not face2 or not edge1 or not edge3:
        raise ValueError("One or more named entities could not be found.")

    # Create geometry intents
    edge1Intent = asmDef.CreateGeometryIntent(edge1, 1)
    edge3Intent = asmDef.CreateGeometryIntent(edge3, 1)
    intentOne = asmDef.CreateGeometryIntent(face2, edge1Intent)
    intentTwo = asmDef.CreateGeometryIntent(face1, edge3Intent)

    # Debugging information for intents
    print("Edge1 Intent:", edge1Intent)
    print("Edge3 Intent:", edge3Intent)
    print("Intent One:", intentOne)
    print("Intent Two:", intentTwo)

    # Create a rotation joint between the two parts
    try:
        jointDef = asmDef.Joints.CreateAssemblyJointDefinition(102401, intentOne, intentTwo)  # kRotationalJointType
    except Exception as e:
        print("Error creating joint definition:", e)
        return

    jointDef.FlipAlignmentDirection = False
    jointDef.FlipOriginDirection = True
    joint = asmDef.Joints.Add(jointDef)

    # Make the joint visible
    joint.Visible = True

    # Drive the joint to animate it
    joint.DriveSettings.StartValue = "0 deg"
    joint.DriveSettings.EndValue = "180 deg"
    joint.DriveSettings.GoToStart()
    joint.DriveSettings.PlayForward()
    joint.DriveSettings.PlayReverse()

def PrintStructure(occurrence):
    # Print the structure of the occurrence
    partDef = occurrence.Definition
    surfaceBodies = partDef.SurfaceBodies
    print(f"Number of Surface Bodies: {surfaceBodies.Count}")
    for i in range(1, surfaceBodies.Count + 1):
        surfaceBody = surfaceBodies.Item(i)
        print(f"  Surface Body {i}:")
        print(f"    Number of Faces: {surfaceBody.Faces.Count}")
        for j in range(1, surfaceBody.Faces.Count + 1):
            print(f"      Face {j}")
        print(f"    Number of Edges: {surfaceBody.Edges.Count}")
        for k in range(1, surfaceBody.Edges.Count + 1):
            print(f"      Edge {k}")

# Execute the function
AssemblyJoint()

[YuhanZhang · Accepted solution]

Try below updated code to check if the result is as expected:

import win32com.client

def AssemblyJoint():
    # Initialize Inventor application
    invApp = win32com.client.Dispatch("Inventor.Application")
    
    # Create a new assembly document
    asmDoc = invApp.Documents.Add(12291, invApp.FileManager.GetTemplateFile(12291, 8962))
    asmDef = asmDoc.ComponentDefinition
    tg = invApp.TransientGeometry
    
    # Place an occurrence into the assembly
    matrix1 = tg.CreateMatrix()
    translation_vector1 = tg.CreateVector(0, 0, 0)
    matrix1.SetTranslation(translation_vector1)
    occ1 = asmDef.Occurrences.Add("C:\\Users\\MINHAZULISLAM\\Desktop\\API Join\\Part1.ipt", matrix1)
    
    matrix2 = tg.CreateMatrix()
    translation_vector2 = tg.CreateVector(8 * 2.54, 6 * 2.54, 2 * 2.54)  # Converting inches to cm
    matrix2.SetTranslation(translation_vector2)
    occ2 = asmDef.Occurrences.Add("C:\\Users\\MINHAZULISLAM\\Desktop\\API Join\\Part2.ipt", matrix2)

    # Print the structure of the first occurrence
    print("Occurrence 1:")
    PrintStructure(occ1)
    print("\nOccurrence 2:")
    PrintStructure(occ2)

    # Get faces and edges by index
    face1 = occ1.SurfaceBodies.Item(1).Faces.Item(1)
    face2 = occ2.SurfaceBodies.Item(1).Faces.Item(1)
    edge1 = occ2.SurfaceBodies.Item(1).Edges.Item(1)
    edge3 = occ1.SurfaceBodies.Item(1).Edges.Item(1)

    # Debugging information
    if not face1:
        print("Face1 not found")
    if not face2:
        print("Face2 not found")
    if not edge1:
        print("Edge1 not found")
    if not edge3:
        print("Edge3 not found")

    # Check if the faces and edges were found
    if not face1 or not face2 or not edge1 or not edge3:
        raise ValueError("One or more named entities could not be found.")

    # Create geometry intents
    #edge1Intent = asmDef.CreateGeometryIntent(edge1, 1)
    edge3Intent = asmDef.CreateGeometryIntent(edge3, 1)
    
    intentOne = asmDef.CreateGeometryIntent(face2, 57867)
    intentTwo = asmDef.CreateGeometryIntent(face1, edge3.StopVertex.Point)

    # Debugging information for intents
    # print("Edge1 Intent:", edge1Intent)
    print("Edge3 Intent:", edge3Intent)
    print("Intent One:", intentOne)
    print("Intent Two:", intentTwo)

    # Create a rotation joint between the two parts
    try:
        jointDef = asmDef.Joints.CreateAssemblyJointDefinition(102401, intentOne, intentTwo)  # kRotationalJointType
    except Exception as e:
        print("Error creating joint definition:", e)
        return

    jointDef.FlipAlignmentDirection = False
    jointDef.FlipOriginDirection = True
    joint = asmDef.Joints.Add(jointDef)

    # Make the joint visible
    joint.Visible = True

    # Drive the joint to animate it
    joint.DriveSettings.StartValue = "0 deg"
    joint.DriveSettings.EndValue = "180 deg"
    joint.DriveSettings.GoToStart()
    joint.DriveSettings.PlayForward()
    joint.DriveSettings.PlayReverse()

def PrintStructure(occurrence):
    # Print the structure of the occurrence
    partDef = occurrence.Definition
    surfaceBodies = partDef.SurfaceBodies
    print(f"Number of Surface Bodies: {surfaceBodies.Count}")
    for i in range(1, surfaceBodies.Count + 1):
        surfaceBody = surfaceBodies.Item(i)
        print(f"  Surface Body {i}:")
        print(f"    Number of Faces: {surfaceBody.Faces.Count}")
        for j in range(1, surfaceBody.Faces.Count + 1):
            print(f"      Face {j}")
        print(f"    Number of Edges: {surfaceBody.Edges.Count}")
        for k in range(1, surfaceBody.Edges.Count + 1):
            print(f"      Edge {k}")

# Execute the function
AssemblyJoint()

You used a cylindrical Face to create a GeometryIntent, that you can below Intent values (from PointIntentEnum) to specify which point on the cylindrical axis will be used:

kAxisEndPointIntent 57867  
kAxisMidPointIntent 57866  
kAxisStartPointIntent 57865

Thanks,

Rocky

[22351396]

Thank You