Reconstruction Dataset

The Reconstruction Dataset contains sequential design data from a subset of simple 'sketch and extrude' components that enables final geometry to be reconstructed.

Overview

Reconstruction data is extracted in sequence from CAD modeling operations found in the parametric feature timeline of each Fusion 360 CAD model. Although there are many CAD modeling operations, we intentionally limit the data to the sketch and extrude operations to reduce the complexity of the reconstruction task. By replaying the sequence of modeling operations programmatically in Fusion 360 it is possible to reconstruct the original model.

Sketch

Sketch data is represented as a series of points, that create curves, that in turn create profiles. Curves can range from a simple line, to a circle, to arcs and splines. Profiles are closed loops formed from one or more curves.

Extrude

An extrude operation takes one or more sketch profiles and constructs a 3D shape. Various parameters inform how the extrude operation is created, such as the direction, distance, and operation type. In the example design sequence below, sketch profiles are sequentially extruded to join (Extrude 1, Extrude 2) or cut (Extrude 3) geometry using built in boolean operations. The color coded areas show the sketch profiles that partake in each extrude operation.

Data Formats

The reconstruction dataset contains 3D models in three different representations: B-Rep, mesh, and construction sequence saved in JSON text format. Other representations, such as point clouds or voxels, can be generated using existing data conversion routines and are not included in the dataset. For convenience we include a thumbnail .png image file together with each geometry. Files are provided in a single directory, with a naming convention as follows: XXXXX_YYYYYYYY_ZZZZ[_1234].ext. Here XXXXX represents the project, YYYYYYYY the file, ZZZZ the component, and _1234 the extrude index. If _1234 is absent the file represents the final design.

B-Rep

B-Rep data is provided as .smt files representing the ground truth geometry and .step as an alternate neutral B-Rep file format. The .smt file format is the native format used by Autodesk Shape Manager, the CAD kernel within Fusion 360, and has the advantage of minimizing conversion errors. Additionally the B-Rep entities, such as bodies and faces, can referenced from the construction sequence back to entities in the .smt file.

Mesh

Mesh data is provided in .obj format representing a triangulated version of the B-Rep. Each B-Rep face is triangulated separately and labeled as a group of triangles in the .obj file with the B-Rep face id as the group name. This approach allows the triangles to be traced back to the B-Rep face and associated extrude operation. Note that the .obj meshes provided are not manifold.

Units

All units are provided in cm. Angular units are provided in radians.

Construction Sequence

Construction information is provided in a .json text format that allows for designs to be reconstructed with Fusion 360 to match the original geometry.

Timeline

When a user is designing in Fusion 360, CAD modelling operations are recorded in a timeline along with the parameters specified by the user at each step.

We represent the timeline as a sequantial list with an index and an entity. The index represents when in the overall assembly timeline the sketch or extrude operation was performed. The entity is a uuid value to look up the sketch or extrude data in the entities data structure.

"timeline": [
    {
        "index": 0,
        "entity": "ed84457a-965f-11ea-911a-acde48001122"
    },
    {
        "index": 1,
        "entity": "ed86b6a2-965f-11ea-911a-acde48001122"
    },
    {
        "index": 2,
        "entity": "ed86ca98-965f-11ea-911a-acde48001122"
    },
    {
        "index": 3,
        "entity": "ed8bae3c-965f-11ea-911a-acde48001122"
    }
]

Entities

The entities data structure contains the details of the sketch and extrude operations detailed in the timeline. Each entity has a name and a type. The name is assigned usually assigned automatically in Fusion 360 but could also be in a localized version. The type represents the CAD operation and will be either Sketch or ExtrudeFeature.

"entities": {
    "ed84457a-965f-11ea-911a-acde48001122": {
        "name": "Sketch1",
        "type": "Sketch"
    },
    "ed86b6a2-965f-11ea-911a-acde48001122": {
        "name": "Extrude1",
        "type": "ExtrudeFeature"
    }
}

Sketch

Sketch entities reflect the Fusion API Sketch. A high level overview of the data structure is provided below, but please refer to the Fusion API documentation for low level details. A sketch entity contains the following top level data structures:

"ed84457a-965f-11ea-911a-acde48001122": {
    "name": "Sketch1",
    "type": "Sketch",
    "points": { },
    "curves": { },
    "constraints": { },
    "profiles": { },
    "transform": { },
    "reference_plane": { }
}

Points

Each point is provided with a uuid key and a Point3D data structure. Sketch data is drawn in a local coordinate system, so only the x and y values will be populated.

"ed85d386-965f-11ea-911a-acde48001122": {
    "type": "Point3D",
    "x": 4.0,
    "y": 2.0,
    "z": 0.0
}

Curves

Each curve has a uuid key and a SketchCurve that can represent a number of different curve types:

• SketchArc
• SketchCircle
• SketchConicCurve
• SketchEllipse
• SketchEllipticalArc
• SketchFittedSpline
• SketchFixedSpline
• SketchLine

Shown below is a simple example of a SketchLine that has a start_point and end_point uuid referencing the points data structure.

"ed85413c-965f-11ea-911a-acde48001122": {
    "type": "SketchLine",
    "construction_geom": false,
    "fixed": false,
    "fully_constrained": false,
    "reference": false,
    "visible": true,
    "start_point": "ed85e27c-965f-11ea-911a-acde48001122",
    "end_point": "ed85f460-965f-11ea-911a-acde48001122"
}

Constraints

Constraints are used to control how the sketch is generated when parameters are changed. Each constraint has a uuid key and a GeometricConstraint that can represent a number of different constraint types that are applied to curves:

• CircularPatternConstraint
• CoincidentConstraint
• CollinearConstraint
• ConcentricConstraint
• EqualConstraint
• HorizontalConstraint
• HorizontalPointsConstraint
• MidPointConstraint
• OffsetConstraint
• ParallelConstraint
• PerpendicularConstraint
• PolygonConstraint
• RectangularPatternConstraint
• SmoothConstraint
• SymmetryConstraint
• TangentConstraint
• VerticalConstraint
• VerticalPointsConstraint

"ed866d8c-965f-11ea-911a-acde48001122": {
    "line": "ed85413c-965f-11ea-911a-acde48001122",
    "type": "HorizontalConstraint"
}

Dimensions

Dimensions are defined by the user to set angles, diameters, distances etc... between sketch geometry to constraint the sketch as it is edited. Each dimension has a uuid key and a SketchDimension representing a dimension type such as:

• SketchAngularDimension
• SketchConcentricCircleDimension
• SketchDiameterDimension
• SketchEllipseMajorRadiusDimension
• SketchEllipseMinorRadiusDimension
• SketchLinearDimension
• SketchOffsetCurvesDimension
• SketchOffsetDimension
• SketchRadialDimension

The example below describes a linear dimension of 5.27 cm between two points.

"6bac825c-c842-11ea-af4b-54bf646e7e1f": {
    "parameter": {
        "type": "ModelParameter",
        "value": 5.27451897,
        "name": "d2",
        "role": "Linear Dimension-2"
    },
    "text_position": {
        "type": "Point3D",
        "x": -6.666826879191981,
        "y": -3.1769168442187983,
        "z": 0.0
    },
    "is_driving": true,
    "entity_one": "6bab9808-c842-11ea-8db0-54bf646e7e1f",
    "entity_two": "6babbf08-c842-11ea-8cac-54bf646e7e1f",
    "orientation": "AlignedDimensionOrientation",
    "type": "SketchLinearDimension"
}

Profiles

Profiles represent a collection of curves that joint together to make a closed loop. In Fusion 360 profiles are automatically generated from arbitrary curves that don't necessarily connect at the end points. In the example below two profiles (pr1 and pr2) are generated when the line crosses the triangle. We provide both the original curves used to generate the profiles (bottom left) and the trimmed profile information containing just the closed profile loop (bottom right).

The overall structure for a profile is as follows. Inside profile_curves the reference to the curve uuid points to the original curve that created the profile. The remaining data specifies the trimmed curve segments that form a connected loop.

"0e0d3220-8e8c-3fd7-b7ad-cba4eca5ed74": {
    "loops": [
        {
            "is_outer": true,
            "profile_curves": [
                {
                    "type": "Line3D",
                    "start_point": {
                        "type": "Point3D",
                        "x": 4.000000059604645,
                        "y": 3.0000000447034836,
                        "z": 0.0
                    },
                    "end_point": {
                        "type": "Point3D",
                        "x": 4.000000059604645,
                        "y": 0.0,
                        "z": 0.0
                    },
                    "curve": "ea667aee-e6ef-11ea-8960-acde48001122"
                },
                {
                    ...
                }
            ]
        }
    ],
    "properties": { }
}

Transform

The transform of the sketch with respect to model space. See Sketch.transform. Provided as a coordinate system.

Reference Plane

The reference plane the sketch is associated to. See Sketch.referencePlane. The refererence plane can originate from a ConstructionPlane (such as a canonical XY, YZ, or YZ construction plane), a planar BRepFace, or a Profile.

Extrude

Extrude entities reflect the Fusion API ExtrudeFeature. A high level overview of the data structure is provided below, but please refer to the Fusion API documentation for low level details. An extrude entity contains the following top level data structures:

"ea69e774-e6ef-11ea-8960-acde48001122": {
    "name": "Extrude1",
    "type": "ExtrudeFeature",
    "profiles": [ ],
    "operation": "NewBodyFeatureOperation",
    "start_extent": { },
    "extent_type": "OneSideFeatureExtentType",
    "extent_one": { },
    "faces": { },
    "bodies": { },
    "extrude_bodies": [ ],
    "extrude_faces": [ ],
    "extrude_side_faces": [ ],
    "extrude_end_faces": [ ],
    "extrude_start_faces": [ ]
},

Profiles

The sketch profiles used to define the shape of the extrude. Each entry contains a reference to the sketch in the entities data structure and to the profile within that sketch.

"profiles": [
    {
        "profile": "5bebd271-f2be-3fbf-80e0-072256cd8723",
        "sketch": "ea635c7e-e6ef-11ea-8960-acde48001122"
    }
]

Operation

The operation defines the type of operation performed by the extrude. The operation type is defined by ExtrudeFeature.operation and can be one of the following types, as illustrated in the figure below:

• NewBodyFeatureOperation
• JoinFeatureOperation
• CutFeatureOperation
• IntersectFeatureOperation

Start Extent

The start_extent defines the "extent" used to define the start of the extrude. See ExtrudeFeature.startExtent. Can be one of ProfilePlaneStartDefinition or OffsetStartDefinition. With ProfilePlaneStartDefinition the extrude starts at the sketch profile, while with OffsetStartDefinition it is offset by a given distance from the sketch profile.

Extent Type

The extent_type defines the type of "extent" used for with the extrude. See ExtrudeFeature.extentType. The image below shows how an extrude can be expressed in several different ways: perpendicular from a sketch for a set distance along one side (OneSideFeatureExtentType), a symmetrical distance along both sides (SymmetricFeatureExtentType), or separate distances along two sides (TwoSidesFeatureExtentType).

Extent One/Two

Both extent_one and extent_two define the distance and taper of the extrude. See ExtrudeFeature.extentOne / extentTwo. For OneSideFeatureExtentType and SymmetricFeatureExtentType only extent_one will be present. The taper_angle is provided in radians and illustrated on the right in the above image.

"extent_one": {
    "distance": {
        "type": "ModelParameter",
        "value": -1.2,
        "name": "d3",
        "role": "AlongDistance"
    },
    "taper_angle": {
        "type": "ModelParameter",
        "value": 0.0,
        "name": "d4",
        "role": "TaperAngle"
    },
    "type": "DistanceExtentDefinition"
}

Faces

The faces data structure contains a list of all B-Rep faces in the design at this point in the timeline. The index value can be used to reference the face when imported into Fusion 360 from the .smt file generated at this step in the timeline. The surface_type indicates the type of underlying surface represented by the face, see SurfaceTypes. point_on_face is a 3D point at or near the center of the face.

"faces": {
    "eab25b94-e6ef-11ea-8960-acde48001122": {
        "index": 0,
        "surface_type": "PlaneSurfaceType",
        "point_on_face": {
            "type": "Point3D",
            "x": 2.0000000298023224,
            "y": 0.30000000447034836,
            "z": 1.6
        }
    },
    ...
}

Bodies

The bodies data structure contains a list of all B-Rep bodies in the design at this point in the timeline. The index value can be used to reference the body when imported into Fusion 360 from the .smt file generated at this step in the timeline. Each body has a list of faces, containing uuids, that reference the faces list at the above level.

"bodies": {
    "ea7d4e36-e6ef-11ea-8960-acde48001122": {
        "index": 0,
        "name": "Body1",
        "faces": [
            "eab25b94-e6ef-11ea-8960-acde48001122",
            ...
        ]
    }
}

Extrude Bodies and Faces

The extrude_bodies and extrude_faces lists contain references to the subset of B-Rep bodies and faces that were created from the current extrude. The extrude_side_faces, extrude_end_faces, and extrude_start_faces lists indicate the role of each face in the extrude. Side faces are those running perpendicular to the extrude direction. Start faces cap the end of the extrusion and are coincident with the sketch plane. End faces cap the end of the extrusion, opposite the start faces.

"extrude_bodies": [
    "ea7d4e36-e6ef-11ea-8960-acde48001122"
],
"extrude_faces": [
    "eab25b94-e6ef-11ea-8960-acde48001122",
    "eab2ce80-e6ef-11ea-8960-acde48001122",
    ...
],
"extrude_side_faces": [
    "eab25b94-e6ef-11ea-8960-acde48001122",
    "eab2ce80-e6ef-11ea-8960-acde48001122",
    ...
],
"extrude_end_faces": [
    "eab5f0a6-e6ef-11ea-8960-acde48001122"
],
"extrude_start_faces": []

Sequence

The sequence data structure contains a list of files and data references that are using during reconstruction. A new sequence item is added when a curve or an extrude is added to the design. Note that the as-designed ordering of sketch operations is not stored in the native design files, however this sequence represents a consistent ordering derived by traversing the sketch profiles in sequence.

"sequence": [
    {
        "index": 1,
        "type": "Sketch",
        "entity": "7bb3de62-cad8-11ea-a448-acde48001122",
        "curve": "7bb7cd38-cad8-11ea-a448-acde48001122",
        "timeline": 0
    },
    ...
    {
        "index": 9,
        "type": "ExtrudeFeature",
        "entity": "7bbbdbb2-cad8-11ea-a448-acde48001122",
        "timeline": 1,
        "png": "File_12a12060_0000_0009.png",
        "smt": "File_12a12060_0000_0009.smt",
        "obj": "File_12a12060_0000_0009.obj"
    }
]

Each sequence item has:

• index: The index in the sequence
• type: Either Sketch or ExtrudeFeature, indicating the modeling operation used.
• entity: The uuid key to access the entity in the entities data structure.
• timeline: The index in the timeline of the modeling operation.

Additionally curves have the following:

• curve: The uuid key to access the curve in the sketch data structure.

Additionally extrudes have the following:

• png: A png screen capture of the design at this point in the sequence.
• smt: A B-Rep file in smt format of the design at this point in the sequence.
• step: A B-Rep file in step format of the design at this point in the sequence.
• obj: A mesh file in obj format of the design at this point in the sequence.

Statistics

Please see the reconstruction dataset statistics page for overview statistics describing the dataset distribution.

Train/Test Split

The official train/test split is contained in the file train_test.json. The 80:20 split consists of 6,900 and 1,725 designs respectively