AICAD/Text2CAD-Bench huggingface dataset:
Geometric description: The square hole perfectly accommodates the cylinder. The overall appearance is a square frame enclosing a cylinder. The main base feature is a square frame with an outer side length of 60mm and an inner hole side length of 40mm. The extended feature is a cylinder with a diameter of 40mm, centered within the square hole, and with a height of 20mm. The topological logic is that the cylinder's diameter equals the side length of the square hole, so the four generatrices of the cylinder are "tangentially in contact" with the four flat walls of the square hole. In CAD, when this contact is handled as a single entity, the connection is a zero-thickness line. The overall structure is a solid with a cylinder fully inserted into the square hole.

Modeling procedure: Draw a square with a side length of 60 mm in the XY plane and extrude it by 20 mm. On the top face, draw a centered square with a side length of 40 mm and cut through to form a frame. Again on the top face, draw a centered circle with a diameter of 40 mm, extrude it by 20 mm, and check "Merge Results." At this point, the cylindrical side contacts the inner wall of the frame at four tangent points, forming a solid where the frame tightly encloses the cylinder.
Geometric description: This is a heat sink with parallel fins on the top. The overall appearance is a square block that is solid at the bottom and comb-like at the top. The base of the main body is a flat plate measuring 60x60x10mm. The extended features consist of 10 vertical fins arranged along the X-axis above the base. Each fin is 60mm long, 40mm high, and 2mm thick, with a spacing of 4mm between each fin. All the fins are integrated with the base. The whole assembly is a model of a heat sink for electronic devices.

Modeling procedure: Stretch a 60x60x10mm base plate. On the upper surface edge of the base plate, draw the first fin sketch: a 60x2mm rectangle. Extrude the height to 40mm. Use the linear array command to copy 10 instances along the X-axis, setting the spacing to /9 or specifying the spacing to ensure the fins are evenly distributed on the base and merge them into a single body.
Geometric description: This is a flexible hose with a wavy wall. The overall appearance resembles an accordion or the bent part of a straw. The basic characteristics are a 100mm long, thin-walled tube with an average diameter of 40mm and a wall thickness of 2mm. The extended feature is that the tube wall is not straight but fluctuates in a sine wave along the axial direction. The peak diameter is 45mm, the trough diameter is 35mm, the wavelength is 10mm, and there are 10 cycles. The detailed features include the same wavy shape inside the tube, maintaining a uniform wall thickness, with 5mm long straight sections at both ends for connection. Overall, it is a typical hydraulic bellows.

Modeling procedure: In the front view plane, draw the rotational section of the corrugated pipe: Draw a centerline 100mm long. Draw the wavy line for the pipe wall, with the crest 22.5mm from the axis and the trough 17.5mm from the axis, with a wavelength of 10mm, repeated 10 times. Use the offset solid command to create the inner wall profile by offsetting 2mm inward, and close both ends. Rotate 360 degrees around the central axis to generate the solid model of the corrugated pipe.
Geometric description: The two hemispheres are offset and fused. The overall appearance is similar to the shape of a peanut. The main body features two hemispheres with a radius of 30mm each. The extension feature involves the flat surfaces of the two hemispheres facing each other but not overlapping. The center of the left hemisphere is at one point, and the center of the right hemisphere is at another, with a distance of 0 between the two planes. Due to the misalignment of the centers, the overlapping area of the two circular planes is non-circular, and the edge of the fused solid presents an "8"-shaped contour change rather than a smooth spherical surface. Overall, it is a misaligned, joined spherical assembly.

Modeling procedure: Create the first entity: generate a hemisphere with a radius of 30mm, centered at the origin, with the flat face oriented towards the positive Z-axis. Create the second entity: generate a hemisphere with a radius of 30mm, centered at the origin, with the flat face oriented towards the negative Z-axis. Perform a Boolean union operation to merge the two offset hemispheres into a single entity, forming an "8"-shaped waist.
Geometric description: This is a pipe fitting with a central baffle. The overall appearance resembles a bamboo joint. The main body is a tube with an inner diameter of 20mm, an outer diameter of 30mm, and a length of 100mm. At both ends of the tube, there are flanges with a diameter of 50mm and a thickness of 5mm. In the exact center of the tube, there is a central baffle with a diameter of 40mm and a thickness of 5mm. All flanges and the tube are coaxially integrated. The entire assembly is a hydraulic pipe fitting with dual-end and central fixation.

Modeling procedure: Use the revolve command to form the shape in one step. Draw a profile sketch in the front plane: include a tube body contour with a length of 100mm and a wall thickness of 5mm; add flange rectangles with a height of 10mm and a width of 5mm at both ends; add a retaining ring rectangle with a height of 5mm and a width of 5mm in the middle. After closing the profile, revolve it 360 degrees around the central axis to generate the solid.
Geometric description: Study the cross-sectional shape after a sphere is removed from the corner of a cube. The overall appearance is a cube with a missing corner. The main feature is a cube with an edge length of 50 mm. An extended feature is created at one of the eight vertices of the cube, with a sphere of radius 30 mm centered at that vertex. A Boolean subtraction operation is performed, removing the sphere from the cube. The topological logic of the cut is not a flat chamfer but a concave spherical triangle, and since the sphere's radius is less than the edge length, the cut surface appears as a curved depression surrounded by three arcs. The overall shape is a cube with a concave corner.

Modeling procedure: Stretch a cube with an edge length of 50mm. Select one of the vertices and use it as the center to construct a sphere with a radius of 30mm. In the feature options, select "Cut" or "Boolean Subtract" to remove the volume of the sphere from the cube. The result should show that the corner is removed, forming a concave spherical surface.
Geometric description: Two objects are interlocked but not in contact. The overall appearance is a chain structure. The main base feature, Ring A, is a circular ring with an outer diameter of 40 and an inner diameter of 30, placed horizontally. The extended feature, Ring B, has the same dimensions but is placed vertically. Topologically, Ring B passes through the central hole of Ring A, and the two rings do not overlap in any way, but they cannot be separated. This is a typical topologically interlocked structure, considered as one component despite being multiple entities. The whole structure is a two-ring interlock.

Modeling procedure: Create two independent entities. Entity 1: Draw a circle in the front view plane and revolve it around the Y-axis to generate a horizontal ring. Entity 2: Draw the same sectional sketch in the right view plane, adjust the center of the circle so that revolving it around the X-axis generates a vertical ring, ensuring that the ring passes through the inner hole of Entity 1 without interference. This is a multi-entity part modeling.
Geometric description: This is a multi-diameter shaft with a keyway. The overall appearance consists of three cylindrical sections of different thicknesses. The main base features are as follows: the left section has a diameter of 40mm and a length of 30mm, the middle section has a diameter of 30mm and a length of 40mm, and the right section has a diameter of 20mm and a length of 30mm, all coaxially connected. An extended feature is a flat-bottomed keyway on the top of the middle cylindrical section, which is 20mm long, 6mm wide, and 3.5mm deep. Detailed features include a center hole at each end face of the shaft, each with a diameter of 5mm and a depth of 10mm. Overall, it is a standard industrial transmission stepped shaft.

Modeling procedure: Use the revolve command to generate the main body of the stepped shaft. Create a tangent reference plane on the middle cylindrical surface, and draw a straight groove sketch with a length of 20mm and a width of 6mm. Extrude and cut 3.5mm inward. At the center of the left and right end faces of the shaft, draw circles with a diameter of 5mm, and cut to a depth of 10mm.
Geometric description: This is a T-shaped block with extremely rounded edges. The overall appearance resembles three cylinders fused together, but the connections are smooth. The main body consists of two 20x20x60mm rectangular prisms intersecting in a T-shape. All the edges of the T-shaped intersection are rounded with an 8mm radius, making the entire piece appear as if it were smoothly transitioned from cylinders and spheres, with no straight edges remaining. A 5mm diameter hole is drilled at the center of each of the three end faces. The whole piece is a streamlined T-joint.

Modeling procedure: Draw a T-shaped sketch and extrude it by 20mm to form a T-shaped block. Use the fillet command, select all edges, and set the radius to 8mm. Since the cross-section is only 20mm, a large fillet will make the block's cross-section nearly circular or elliptical. Finally, draw a 5mm diameter circle at the center of the flat ends on three sides and cut through holes.
Geometric description: This is a square tube structure with a tilted top and hollow interior. The overall appearance is a rectangular shell with a slanted top. The main base feature is a 60x60x100mm rectangular column. The extended feature is cut at the top by a plane at a 45-degree angle to the horizontal, leaving the front wall height at 60mm and the rear wall height at 100mm. The detailed feature is that the interior is hollowed out, with a uniform wall thickness of 5mm, forming an irregular tube that runs through from top to bottom. A 20mm diameter circular hole is drilled in the higher rear wall. The overall structure is a sloped exhaust hood casing.

Modeling procedure: Stretch a 60x60mm rectangle to a height of 100mm. In the front view plane, draw a line from the front edge at Z=60mm to the back edge at Z=100mm, forming a triangular cutting tool, and extrude to cut out the top. Use the shell command to remove the bottom surface with a wall thickness of 5mm. On the higher rear face, draw a circle with a diameter of 20mm and cut out a through hole.
Geometric description: This is a structure where a frame encases a sphere. The overall appearance is a hollow cubic frame with a "floating" sphere in the center. The main base feature is a solid cube with an edge length of 60mm. Extended features involve cutting circular through-holes with a diameter of 40mm at the center of each of the six faces of the cube. The six holes intersect at the center, and the remaining material after cutting forms the frame. The detailed feature is a sphere with a diameter of 30mm placed in the central cavity. If simplified to a single entity, it can be described as: after cutting holes on all six sides, the material left in the center forms a specific geometric structure, or it can be directly described as a frame with a solid sphere of 20mm in diameter at the center, connected to the frame by six thin rods. The overall structure is a complex hollow containment.

Modeling procedure: Stretch a cube with an edge length of 60mm. Draw a circle with a diameter of 40mm on each of the six faces, and completely cut through inwardly. This will form a frame. Create a new solid at the center and rotate it to generate a sphere with a diameter of 30mm. If physical connection is needed, add small connecting columns between the sphere and the inner corners of the frame, or the model can exist as a multi-body component.
Geometric description: Complex openings on the pyramid. The overall appearance is a pyramid with only the edges remaining. The main base feature is a square pyramid with a base edge of 40mm and a height of 40mm. An extended feature involves excavating a smaller square pyramid cavity from the center of the base upwards. Detail features include triangular through-holes on each of the four sides, connecting to the internal cavity. Topological logic transforms the square pyramid into a skeleton composed of four side edges and a base frame. The whole structure is a frame-like pyramid.

Modeling procedure: Draw a 40x40mm square in the XY plane, extrude it to the vertex at Z=40mm, and generate a solid quadrangular pyramid. Draw a 30x30mm square on the base, cut and loft to the vertex at Z=30mm, hollowing out the interior. On each of the four triangular sides, draw smaller triangular contours, perform cut operations to penetrate the side walls, leaving only the edge framework.
Geometric description: The path and cross-section change simultaneously. The overall appearance is a 90-degree elbow, with one end larger and the other smaller. The main base feature scan path is a quarter-circle arc with a radius of 50mm. The extended feature starts with a circular cross-section of 30mm in diameter and ends with a circular cross-section of 15mm in diameter. The topology logic involves tapering while bending, and the pipe wall surface is a complex doubly curved surface rather than a simple part of a torus. The overall shape is a conical bend.

Modeling procedure: Use the loft command. First, draw the path in the front view plane: a 90-degree arc with a radius of 50 mm. Create two reference planes: one at the start point of the path and one at the end point. Draw a circle with a diameter of 30 mm on the start plane and a circle with a diameter of 15 mm on the end plane. Execute the loft, select the centerline parameter, and pick the arc path to generate the variable-diameter elbow solid.
Geometric description: The intersection of two hollow tubes, with an overall appearance of a cross-shaped pipe fitting. The base feature consists of two cylinders with a diameter of 40mm and a length of 100mm, orthogonally fused. The extended feature involves shelling the entire merged solid, with a wall thickness of 2mm, and removing all four end faces. The topological challenge lies internally: the tube walls at the intersection of the two cylinders are removed, forming a fully connected cross-shaped internal cavity, rather than two separate tubes inserted into each other. It is necessary to understand the post-processing effect of the shelling operation on the Boolean union. The overall structure is a cross-shaped pipe with uniform wall thickness.

Modeling procedure: Draw a cross sketch on the front plane: extrude a cylinder with a diameter of 40mm and a length of 100mm along the X-axis; extrude another cylinder with a diameter of 40mm and a length of 100mm along the Y-axis, and perform a Boolean union at the intersection of the two cylinders. Use the shell command, set the wall thickness to 2mm, select and remove the four end faces of the cylinders. The system will automatically calculate and remove the material in the internal intersecting area, forming a fully connected hollow cross tube.
Geometric description: This is a thick disc with semicircular grooves on the edges. The overall appearance resembles a simplified plum blossom. The main body feature is a cylinder with a diameter of 100mm and a thickness of 30mm. The extended features are eight semicircular grooves with a radius of 10mm, evenly distributed on the outer circumference of the cylinder. The axes of the grooves are parallel to the main axis of the cylinder and run through the entire thickness. The detailed feature is a central hole with a diameter of 30mm, and a keyway with a width of 8mm and a depth of 4mm is cut into the side wall of the hole. The whole structure is a typical half of an elastic coupling.

Modeling procedure: Stretch a cylinder with a diameter of 100 mm and a height of 30 mm. Draw a circle with a radius of 10 mm on the top edge, with its center located on the edge of the cylinder, and cut through. Use a circular array to replicate the cut 8 times. Draw a circle with a diameter of 30 mm at the center of the cylinder and a connected keyway rectangle of 8x4 mm, and cut through.
Geometric description: The appearance is simple, with a hole that turns inside. The overall appearance is a solid rectangular prism. The main body has a basic feature of a rectangular prism measuring 80mm in length, 40mm in width, and 40mm in height. The detailed feature includes an L-shaped circular passage inside: one segment enters horizontally from the center of the left side, 40mm deep; the other segment enters vertically from the center of the top surface, 20mm deep. The topology ensures that the two segments of the hole intersect precisely inside, forming a 90-degree bend flow channel, and the flow channel does not penetrate the opposite surface. Overall, it is a module containing a right-angle bend hole.

Modeling procedure: Stretch an 80x40x40mm rectangular prism. Select the left side, draw a circle with a diameter, and cut to a depth of 40mm. Select the center of the top surface, draw a circle with the same diameter, and cut to a depth of 20mm. Ensure that the depth parameters of the two holes are such that they intersect precisely and connect internally, forming an L-shaped blind hole channel.
Geometric description: Two holes intersect but do not appear to be through. The overall appearance is a cube. The main feature is a 50mm cube. Detailed features include a 15mm diameter blind hole along the X-axis, 30mm deep, and a 15mm diameter blind hole along the Z-axis, 30mm deep. Topologically, the two holes intersect in the central region, forming an L-shaped internal space. Since both are blind holes, they do not appear to be connected from the outside, but the internal spaces merge. The whole is a dual-blind hole block with internal connectivity.

Modeling procedure: Stretch a 50mm cube. Select the front face, draw a circle with a diameter of 15mm, and cut to a depth of 30mm. Select the top face, draw a circle with a diameter of 15mm, and cut to a depth of 30mm. The two holes will spatially overlap in the central area of the cube, achieving internal connectivity.
Geometric description: This is a part with holes on both the cylindrical surface and the end face. The overall appearance is a thick-walled ring with multiple holes. The main base feature is a ring with an outer diameter of 90mm, an inner diameter of 40mm, and a thickness of 25mm. Extended feature 1: On the outer cylindrical surface of the ring, there are 6 through-holes with a diameter of 10mm, evenly distributed radially. These holes penetrate the wall and lead to the central hole inside. Extended feature 2: On the upper end face of the ring, there are 6 countersunk holes with a diameter of 8mm, evenly distributed on a circle with a diameter of 65mm. The radial holes and the axial countersunk holes are staggered in their circumferential positions, with the radial holes located at 0, 60, 120... degrees, and the axial holes at 30, 90, 150... degrees. The topological logic ensures that the two sets of holes do not intersect, adding to the complexity of machining and the geometric aesthetics of the part. Overall, it is a complex flange model.

Modeling procedure: First, draw two concentric circles with an outer diameter of 90mm and an inner diameter of 40mm in the top view plane. Extrude 25mm to create the base ring. Next, create radial holes: select the front view plane, and at Z=12.5mm, draw a circle with a diameter of 10mm, with its center on the outer side. Use the extrude cut command, directing towards the center, and choose "cut to the next face" to penetrate the wall. Use the circular array feature to array this cut feature 6 times around the Z-axis. Then, create axial holes: select the top surface of the ring, and draw a construction circle with a diameter of 65mm. On the construction circle, draw a hole location point, rotated 30 degrees relative to the X-axis. Use the non-standard hole wizard or revolve cut to create a countersunk hole. Finally, use the circular array to array this countersunk hole feature 6 times around the Z-axis.
Geometric description: The model is an optical surface for a car headlight reflector, with its geometric essence being a paraboloid of revolution. The vertex of the reflective surface is precisely located at the point (100, 75, 0) in the global coordinate system. This paraboloid has a rotation axis that passes through the vertex and is parallel to the X-axis, with the opening facing the positive direction of the X-axis. Its optical properties are uniquely determined by the focal length, with the focus located 50 millimeters in front of the vertex, at the coordinates (150, 75, 0). This means the focal length f of the paraboloid is 50 millimeters (corresponding to the parabolic equation parameter p=100, i.e., the standard equation $Y^2+Z^2 = 200(X-100)$). The entire reflective surface extends along the positive direction of the X-axis, with a total depth of 100 millimeters, extending from the vertex at X=100 to a plane at X=200, forming a circular opening boundary. This surface is used to reflect the light emitted from a point source placed at the focus into a parallel beam.

Modeling procedure: First, initialize the modeling environment and ensure the use of a standard Cartesian coordinate system. Select the XY plane (top view) as the sketch reference plane. In the sketch environment, draw a horizontal construction line through Y=75 to serve as the rotation axis for subsequent steps. Next, use the parabola tool to draw a parabolic arc opening to the right. Add geometric constraints to fix the vertex of the parabola at the coordinate point (100, 75, 0). To precisely define the curvature, place a point 50.0 mm to the right of the vertex on the axis of the parabola and constrain it as the focus of the parabola (or annotate the horizontal distance from the vertex to the focus as 50.0 mm). Then, draw a vertical line at x=200 to truncate the parabola, ensuring the axial depth of the reflective surface is 100.0 mm. Trim the excess parabolic segment beyond x>200. After completing the sketch, exit. Invoke the "revolve surface" command, select the drawn parabolic arc as the profile, and choose the horizontal construction line at Y=75 as the rotation axis. Rotate 360 degrees to generate the final parabolic reflector solid.