Test 1

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 Number	Mass (g)
Part 1	2850.16
Part 2	290.79
Part 3	1633.25
Part 4	112.37

Center of Gravity Analysis – Gripper

Configuration	X (mm)	Y (mm)	Z (mm)
Fully Open	-29.15	0.16	19.86
Fully Closed	-25.78	0.06	19.86

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

 

Process of Obtaining the Part

—> 1. Workspace Setup

• Launch SolidWorks and select New Part.

• Click on Piece to start modeling a new piece.

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

• 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.

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—> 2. Sketching the Base Profile

---> a. Create Centerlines

• Click on the Line function.

• 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.

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

---> 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.

• 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.

---> 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.

---> b. Offset the Arc

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

---> c. Mirror the Cutout

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

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

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• Ensure the sketch forms a closed loop.

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—> 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.

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


—> 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.

—> 3. Sketch Creation

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

• 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.

• 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.

• 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.

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

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

• 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.

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

• Click Validate.

—> 6. Mass Properties

• 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


—> 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

  

• Click on the Front Plane, then select Sketch

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—> 2. Creating the Sketch

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

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

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

• 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

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

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

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—> 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

  

• Confirm by clicking OK

---> Cut-Extrude (Material Removal)

• Select Extruded Cut

• Choose the entities to remove

• Set extrusion properties:

  • Direction: Select Mid Plane
  • Depth: 60 mm

  

• 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

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


—> 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

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—> 3. Creating the Sketch

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

• Use Smart Dimension to assign dimensions to the sketch elements

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

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—> 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

---> 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

  

• Validate the extrusion

---> Third Extrusion

• Repeat the previous step

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

  

• 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

  

• 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

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.

—> 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.

—> 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.


2. 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

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Positioning the First Link

• Insert the first biellette (link)
• Apply Coaxial and Coincident constraints to mount it on top of the cylinder rod end


Adding the Second Link

• 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


Creating Symmetry

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


Adding the Jaw Holders

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

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

• Analyze the center of gravity of the entire assembly in this fully open position


Configuration	X (mm)	Y (mm)	Z (mm)
Fully Open	-29.15	0.16	19.86

—> 2. Center of Gravity – Closed Position

• Fix the rod end at the maximum extension

• Analyze the center of gravity in this fully closed configuration


Configuration	X (mm)	Y (mm)	Z (mm)
Fully Closed	-25.78	0.06	19.86

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 SolidWorks Installation Guide (EN)
  Detailed instructions to install SolidWorks on a single computer.

• SolidWorks Admin & Deployment Guides
  For advanced installations, network licenses, and administrative deployments.

• SolidWorks Downloads Portal
  Access to installation files, service packs, and updates (login required).

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Official Tutorials & Manuals

• Student’s Guide to Learning SolidWorks (PDF)
  A comprehensive beginner workbook with hands-on exercises.

• MySolidWorks – Online Training Hub
  Interactive tutorials, certification prep, and beginner-to-advanced courses.

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Beginner-Friendly Video Tutorials

• SolidWorks Tutorial for Beginners #1 – CAD CAM Tutorials (YouTube)
  Start modeling with sketches, constraints, and extrusion.

• SolidWorks 2020 Full Beginner Tutorial – Aryan Fallahi (YouTube)
  A concise intro to interface, part design, and assemblies.

• SolidWorks Tutorials for Beginners (Website)
  Detailed walkthroughs on tools, menus, and modeling strategies.

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Additional Resources

• Last Minute Engineers – CAD & Arduino Projects
  Perfect for blending SolidWorks with real-world embedded projects.

• GrabCAD Library – SolidWorks Files
  Thousands of free SolidWorks models and parts to download and explore.

• SolidWorks Forums (EN)
  Ask questions, get help, and join discussions with the global community.