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1rst Test

Objectives​

  • Produce a batch of parts within a limited time frame while adhering to imposed constraints (materials, dimensions, etc.).
  • Comply with a mass tolerance of ±5% for each manufactured part.
  • Design sketches incorporating basic geometric shapes:
    • Rectangles
    • Circles
    • Polygons
  • Use extrusion and revolution features to model 3D parts based on the sketches.
  • Evaluate the mass of each part.

Summary​

Modeling files​

Access the modeling files by clicking here.

Mass Summary of Part​

Part NumberMass (g)
Part 12850.16
Part 2290.79
Part 31633.25
Part 4112.37

Center of Gravity Analysis – Gripper​

ConfigurationX (mm)Y (mm)Z (mm)
Fully Open-29.150.1619.86
Fully Closed-25.780.0619.86

Materials​

  • Computer
  • Internet connection

Execution​

Modeling of the First Part​

Unit Systems and Material Properties​

  • Unit System: MMGS (Millimeter, Gram, Second)
  • Decimals: 2
  • Hole Specification: All holes are through unless otherwise specified
  • Material: AISI 1020 Steel
  • Density: 0.0079 g/mm³

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Process of Obtaining the Part​

--> 1. Workspace Setup

  • Launch SolidWorks and select New Part.

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  • Click on Piece to start modeling a new piece.

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  • In the design tree, right-click the Front Plane and choose Edit Sketch.

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  • Set the unit system to MMGS (Millimeter, Gram, Second).
  • Ensure decimals are set to 2.
  • Assume all holes are through unless stated otherwise.
  • Assign material as AISI 1020 Steel with a density of 0.0079 g/mm³.

--> 2. Sketching the Base Profile

---> a. Create Centerlines

  • Click on the Line function.

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  • Select the Horizontal Constraint and For Construction in the properties.
  • Position the start and end points, ensuring alignment with the reference frame.
  • Click Validate to confirm.

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  • Click again on the Vertical Constraint to draw the vertical axis, ensuring alignment with the reference frame.
  • Click Validate to confirm.

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---> b. Draw Concentric Circles

  • In the top ribbon, click on "Circle".
  • Click on the intersection point of the two axes (center of the circle).
  • Stretch the circle to any size for now.
  • Enter the circle radius in the properties panel on the left.

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  • Select the "Smart Dimension" tool.
  • Click on the edge of the circle → a diameter dimension will appear.
  • Enter the value 100 mm (since the radius is 50 mm, the diameter is 100 mm).
  • Click Validate to confirm.
  • Draw two other circles centered on the origin:
    • Diameter 135.6 mm
    • Diameter 150 mm
  • Apply concentricity constraints to ensure a common center.

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---> c. Add Offset Circle

  • Create a new circle on the horizontal axis, offset from the origin.
  • Set its diameter to 80 mm (radius = 40 mm).
  • Use Smart Dimension to set the center-to-center distance from the 150 mm circle to 150 mm.

---> d. Add Additional Circle

  • Draw another circle with a diameter of 50 mm, concentric with the 80 mm circle.

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--> 3. Creating Fillet and Cutout

---> a. Create Tangent Arc

  • Use the Perimeter Circle to draw a circle tangent to the 150 mm and 80 mm circles.
  • Set the appropriate diameter to represent a 75 mm fillet.
  • Use the Trim Entities tool to remove excess lines, forming a closed contour.

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---> b. Offset the Arc

  • Select the arc and apply a 10 mm offset using Offset Entities.
  • Trim intersecting entities to clean up the sketch.

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---> c. Mirror the Cutout

  • Use Mirror Entities to duplicate the feature across the horizontal axis.

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  • Then mirror the resulting shapes across the vertical axis for full symmetry.

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  • Ensure the sketch forms a closed loop.

--> Creating the 3D Volume

  • Exit the sketch and switch to the Features tab.

  • Use Extruded Boss/Base:

    • Select the entire sketch.
    • Choose Blind extrusion with a depth of 20 mm.
    • Select only the 100 mm diameter region to extrude the solid part.

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--> 5. Adding the Cut (Counterbore)

  • Use Extruded Cut on the same sketch:
    • Set cut depth to 10 mm.
    • Select the region between 100 mm and 135.6 mm circles as the cut profile.

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--> 6. Mass Evaluation

  • Type Mass in the search bar.
  • Click on Mass Properties.

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The part mass should be 2850.16 grams.


Modeling of the Second Part​

Unit Systems and Material Properties​

  • MMGS (Millimeter, Gram, Second)
  • Decimals: 2
  • Hole Specification: All holes are through unless otherwise specified
  • Material: Aluminum Alloy 1060
  • Density: 0.0027 g/mm³

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--> 1. Modifying Part 2 Parameters

  • Right-click on Material: "Not Specified".
  • Click on Edit Material.
  • The Material tab opens.
  • Navigate to SolidWorks Materials → Aluminum Alloy → Alloy 1060.
  • Click Apply and Close.

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--> 2. Preparing the Workspace

  • Click on Front Plane.

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--> 3. Sketch Creation

  • Click on the Circle tool and draw concentric circles with diameters 20 mm and 38 mm, centered on the vertical axis.

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  • Click on Smart Dimension:
    • Select the 64 mm and 38 mm diameter circles.
    • Specify the center distance as 75 mm and validate.
  • Right-click on the Circle tool and select Perimeter Circle.
  • Select the entities:
    • Click on the 64 mm and 38 mm diameter circles.
    • Click on an external point (the created circle will be tangent to the selected circles).
  • Specify the fillet radius as R64.

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  • Click on the Trim Entities tool to remove overlapping sketch parts and create a closed sketch.
  • Select the Trim tool properties.
  • Click on the entities to remove.

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  • Apply the dimensioning to the fillet.
  • Click on the Symmetry tool.
  • Select the entities to symmetrize: R64 fillet.
  • Select the symmetry axis: Vertical axis.

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--> 3. Creating the Volume

  • Click on Features → Extruded Boss/Base.
  • Select the entities to extrude.

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  • Click Validate.
  • Click on Boss/Base → Sketch.

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  • Click on Features → Extruded Boss/Base.
  • Select the entities to extrude.

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  • Click Validate.
  • Click on Boss/Base → Sketch → Extruded Boss/Base.
  • Select the entities to extrude: 43 mm and 34 mm diameter circles.
  • In the parameters, select Direction 1 and Direction 2.
  • Specify the extrusion distances: 15 mm and 30 mm.

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  • Click Validate.
  • Click on Boss/Base → Sketch → Extruded Cut.
  • Select the entities to cut: 43 mm and 55 mm diameter circles.

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  • Click Validate.

--> 6. Mass Properties

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  • Mass Calculation: Use the Mass Properties tool to determine the part's mass.

The part mass is : 290.79 gramms


Modeling of the Third Piece​

Unit System​

  • MMGS (Millimeter, Gram, Second)
  • Decimals: 2
  • Hole Specification: All holes are through unless otherwise specified
  • Material: AISI 1020 Steel
  • Density: 0.0079 g/mm³

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--> 1. Modifying Part 3 Parameters

  • Right-click on Material: "Not Specified"

  • Select Edit Material

  • In the Material tab:

    • Browse to SolidWorks Materials > Steel > AISI 1020
    • Click Apply, then Close

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  • Click on the Front Plane, then select Sketch

--> 2. Creating the Sketch

  • Use the Line tool to draw a trapezoid (initial dimensions can be arbitrary)
  • Use Smart Dimensioning to set precise dimensions

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Tip: Reference the origin to fix the sketch and improve stability

  • Use the Offset Entities tool to offset the trapezoid 10 mm inward

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  • If the offset direction is incorrect, reverse it in the Property Manager

  • Use the Line tool again to draw a vertical line starting from the base of the 150 mm horizontal segment

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  • Apply Smart Dimensioning to position this line relative to a fixed reference point

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  • Verify that the sketch is fully constrained
    • If not, apply necessary constraints to stabilize the geometry
  • Exit the sketch

--> 3. Creating the 3D Volume

---> Boss-Extrude (Solid)

  • Navigate to Features > Extruded Boss/Base

  • Select the sketch entities to extrude

  • Set extrusion properties:

    • Direction: Select Mid Plane
    • Depth: 100 mm

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  • Confirm by clicking OK

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---> Cut-Extrude (Material Removal)

  • Select Extruded Cut

  • Choose the entities to remove

  • Set extrusion properties:

    • Direction: Select Mid Plane
    • Depth: 60 mm

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  • Confirm by clicking OK

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--> 4. Evaluating Part Mass

  • Type "Mass" in the search bar
  • Click on Mass Properties
  • Review the calculated mass based on geometry and material assignment

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The piece mass is : 1633.25 gramms


Modeling of the Fourth Piece​

Unit System​

  • MMGS (Millimeter, Gram, Second)
  • Decimals: 2
  • Hole Specification: All holes are through unless otherwise specified
  • Material: Aluminum Alloy 1060
  • Density: 0.0027 g/mm³
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--> 1. Updating Material Settings

  • Right-click on Material: “Not Specified”
  • Select Edit Material
  • In the Material tab:
    • Navigate to SolidWorks Materials > Aluminum Alloys > 1060 Alloy
    • Click Apply, then Close

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--> 2. Preparing the Workspace

  • Select the Front Plane and click Sketch

--> 3. Creating the Sketch

  • Use the Line tool to draw a profile similar to the front view of the part

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  • Use Smart Dimension to assign dimensions to the sketch elements

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  • Reference the origin wherever possible for stability
  • Exit the sketch

--> 4. Creating the Volume – Extrusions

---> First Extrusion

  • Click Features > Extruded Boss/Base
  • In the Feature Manager:
    • Set extrusion direction to Mid Plane
    • Set Depth to 50 mm
  • Select the appropriate contour and confirm

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---> Second Extrusion

  • Return to the same sketch

  • Click Extruded Boss/Base

    • Set an offset of 15 mm
    • Define the direction carefully (flip if needed)
    • Choose Up to Surface as the end condition if required, and select the target face

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  • Validate the extrusion

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---> Third Extrusion

  • Repeat the previous step

    • Again, pay attention to offset direction
    • Use Up to Surface for precise alignment

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  • Confirm the operation

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--> 5. Revolved Feature

  • In the sketch, select Revolved Boss/Base

    • Specify the revolution angle
    • Select the profile to revolve
    • Choose the axis of revolution

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  • Confirm the feature

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--> 6. Adding Fillets

  • Use the Fillet tool to apply a 2 mm radius to the designated edge(s)
  • Validate the fillet

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--> 7. Evaluating the Part's Mass

  • Type "Mass" in the search bar
  • Click on Mass Properties
  • Review the calculated mass value

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The piece mass is : 112.37 gramms


Assembly – Mechanical Gripper​

Objective​

This stage of the test involves assembling various components to form a mechanical gripper. After downloading the provided .zip file, the goal is to assemble the given parts using appropriate constraints.

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Constraints and Functions Used in the Gripper Assembly​

--> 1. Coaxial Constraint This constraint aligns two cylindrical or circular axes (holes, shafts, cylinders) to share the same center axis.
Example: Aligning a shaft with its corresponding hole ensures proper axial alignment.

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--> 2. Coincident Constraint This constraint forces two planar or linear surfaces to touch, making them coplanar or flush.
Usage: Used to attach one part directly against another.

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--> 3. Symmetric Components Function Under the Linear Component Pattern feature, this function generates a mirrored component from a parent part across a defined reference plane.

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Assembly Steps​

  1. Open SolidWorks, then open the file ASSEMBLAGE PINCE.
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  1. Insert the following parts to complete the mechanical gripper:
    • Connecting Links (Biellettes)
    • Jaw Holders (Porte Mâchoire)
    • Left and Right Jaws (Mâchoire Gauche & Droite)
    • Link Axles (Axe de Biellette)
    • Jaw Holder Axles (Axe Porte Mâchoire)
    • M5×16 Screws
    • M5×25 Screws
    • Circlips
  • Insert the first biellette (link)
  • Apply Coaxial and Coincident constraints to mount it on top of the cylinder rod end
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  • Insert the second biellette underneath the first one, with the rod end in between
  • Use Coaxial and Coincident constraints for alignment
  • Add a Coincident constraint between the two link faces for perfect overlap
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Creating Symmetry​

  • Use the Top Plane and the Symmetric Components tool to mirror and complete all four links required for the gripper
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Adding the Jaw Holders​

  • Insert the Jaw Holder using Coaxial and Coincident constraints
  • Apply symmetry with respect to the Top Plane, as done previously

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Finalizing Assembly​

  • Insert the jaws (left and right)
  • Add all fasteners and fixings:
    • M5×16 screws
    • M5×25 screws
    • Link and jaw axles
    • Circlips for locking
  • This results in the complete mechanical gripper

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Complementary Tasks​

--> 1. Center of Gravity – Open Position

  • Fix the rod end at the minimum extension

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  • Analyze the center of gravity of the entire assembly in this fully open position
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ConfigurationX (mm)Y (mm)Z (mm)
Fully Open-29.150.1619.86

--> 2. Center of Gravity – Closed Position

  • Fix the rod end at the maximum extension

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  • Analyze the center of gravity in this fully closed configuration
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ConfigurationX (mm)Y (mm)Z (mm)
Fully Closed-25.780.0619.86

Errors Encountered​

Problem​

During the installation of SolidWorks, I encountered an issue that initially prevented successful setup.

Solution​

The problem was resolved after watching a step-by-step tutorial video that clearly demonstrated the correct installation procedure and highlighted settings we had previously overlooked.


Perspectives​

  • Part Optimization: Future versions of the mechanical components could explore new materials or lightweight geometries to reduce mass and improve energy efficiency.

  • Smarter Gripping Mechanisms: Integration of force sensors, soft grippers, or motor feedback could make the gripper more adaptive to different object shapes and textures.

  • System Integration: The validated modules can be scaled into more complex robotic systems, such as mobile manipulators or industrial automation platforms.

  • Simulation Before Prototyping: Leveraging SolidWorks Motion Studies, MATLAB/Simulink, or ROS-based environments for dynamic testing and control strategy validation before fabrication.


Resources​

Installation Guides​

Official Tutorials & Manuals​

Beginner-Friendly Video Tutorials​

Additional Resources​