After teaching 1000’s of students and writing about SOLIDWORKS and SOLIDWORKS Simulation for over 25 years, David Planchard, emeritus WPI, is exploring 3DEXPERIENCE Simulation and the Abaqus solver. Through the SOLIDWORKS and 3DEXPERIENCE Simulation Lesson series, David helps educators understand 3DEXPERIENCE Simulation fundamentals through simple examples and industry practices.
In this lesson, learn the proper workflow to upload a SOLIDWORKS assembly to the 3DEXPERIENCE platform and perform a Linear Structural Simulation study using the Abaqus solver.
Open a SOLIDWORKS assembly that has not been saved to the 3DEXPERIENCE platform. Identify your Collaborative space in the MySession panel.
Upload the SOLIDWORKS assembly to the 3DEXPERIENCE platform. Save the assembly in your Collaborative space. Use an existing Bookmark. Return to your SOLIDWORKS desktop. Lock the assembly and all reference components.
Launch the Linear Structural Validation App from the SOLIDWORKS Task Pane. View and set Simulation study preferences.
Set study conditions: Global mesh (Tetrahedron second-order elements), Material (AISI 1020 Steel), Contact (Linear Structural Validation frictionless), Fixed Displacement Restraints (2) and Load (Pressure 3.5 × 106N/m2).
Run the Simulation study. Use the Physics Results Explorer App. Create three Simulation study contour plots: Von Mises Stress, Displacement and Factor of Safety (FOS). Review the Simulation contour plots to interpret the results.
Save the Simulation study in your Collaborative space and Bookmark.
Play a Simulation study contour plot animation.
Before we start, there are a few items that you need to know.
In this lesson, use your default Collaborative space. An internet connection is required. A 3DEXPERIENCE ID is required.
The Simulation lesson provides a foundation to users who are new to using simulation to solve real-word engineering and design problems. A Solid body is used. You should have a basic understanding of Stress and Finite Element Method (FEM).
3DEXPERIENCE Launcher and SOLIDWORKS Desktop
3DEXPERIENCE Launcher needs to be installed. 3DEXPERIENCE Works Lesson 1: Getting Started with SOLIDWORKS.
The 3DEXPERIENCE platform is browser driven. Your existing cookies and cache determine what you will see on your computer desktop or during a SOLIDWORKS login. A full installation of SOLIDWORKS 2019 SP0 or later is required
Start a SOLIDWORKS session from your desktop.
Double-click the SOLIDWORKS icon.
View the illustration below. Depending on your system setup, cookies, and cache, it will be different. Read the provided information.
Input the requested data. Click Accept All.
The Welcome – SOLIDWORKS dialog box is displayed.
You are logged into the 3DEXPERIENCE platform.
Close the Welcome dialog box.
Click the 3DEXPERIENCE icon in the Task Pane. The MySession panel is displayed. This displays the two-way communication between SOLIDWORKS running on your desktop and the 3DEXPERIENCE platform running in the cloud.
In this lesson, I’m using a Collaborative space named Quick Start xDesign.
Note: If you do not see the 3DEXPERIENCE icon, click the Options drop-down arrow, click Add-Ins, check the 3DEXPERIENCE box, click OK, from the SOLIDWORKS Main menu.
Click Accept All.
Two Ring SOLIDWORKS Assembly
Download the SOLIDWORKS assembly, Two Rings to follow along with the lesson.
Open the Two Rings assembly and reference components that have not been previously uploaded or saved to the 3DEXPERIENCE platform.
Expand the Task Pane bar. The MySession panel displays a tree view of the active file and a list of commands that can be accessed through the Action bar and context menu. The orange save Status icon for the Two Rings assembly informs you that the assembly and the reference components on your computer have not been saved to the 3DEXPERIENCE platform.
Confirm the name of your Collaborative space.
Click the drop-down arrow in the MySession panel as illustrated.
Click the Preferences icon.
In this example, my Collaborative space is named Quick Start xDesign.
Save the assembly to the 3DEXPERIENCE platform.
Click Save Active Window from the Lifecycle tab in the Action bar.
The files are temporarily being saved to a local cache area. The platform is checking for out of date components, modified components from the last save to the platform, different revisions, missing components, etc. The Save to 3DEXPERIENCE dialog box and PLM attributes are displayed.
Bookmark and Save to the Platform
Save the model. Use your existing Collaborative space. Use an existing Bookmark. Note: if needed view 3DEXPERIENCE Works Lesson 3: SOLIDWORKS Bookmarks, Share and Delete.
Click the Select Bookmark down arrow.
Click Select Bookmark. The Select a Bookmark dialog box is displayed.
In the below example, I selected Design Project 103 as my bookmark.
Click Apply to All from the Select Bookmark dialog box.
Click Save from the Save to 3DEXPERIENCE dialog box.
The model is directly loaded into your Collaborative space and Bookmarked on the 3DEXPERIENCE platform. You return back into your SOLIDWORKS desktop session.
View the Status column in the updated MySession panel. The Status icon displays three green check marks. This means that the Two Rings assembly and the reference components on your SOLIDWORKS desktop are updated and saved to the platform. The default Revision is A.
Lock the assembly and reference components. This prevents anyone in making a change to them.
Right-click Two Rings in the MySession panel.
Click Lock. The lock icon is displayed.
Lock Part1-Large Ring and Part2-Small Ring.
Click Two Rings in the MySession panel.
Click the center of the Compass. Use the Linear Structural Validation App. Think of this App as the SOLIDWORKS Simulation Add-in inside of SOLIDWORKS. Most of the 3DEXPERIENCE Apps run in your web browser. 3DEXPERIENCE Simulation Apps perform a small installation on your windows machine. Both types of Apps are linked to your PLM data on the platform. The Linear Structural Validation App provides the ability to run Linear Structural, Buckling, Frequency, and Thermal studies.
Drag the slider downward to view the Linear Structural Validation App.
Linear Structural Validation App
Launch the Linear Structural Validation App. Note: If this is your first time using a 3DEXPERIENCE Simulation App or an update is available, download the needed App information on your computer. It is reccommended to restart your SOLIDWORKS session after an update.
This may take 10 – 15 seconds.
The 3DEXPERIENCE | SIMULIA Linear Structural Validation App is displayed.
Default Product Name: Two Rings A.
Except the default Simulation title.
Select Structural for Analysis type from the drop-down menu.
Click OK from the Simulation Initialization dialog box. In a Linear analysis, there is a linear relationship between the applied loads and the induced response of the component. In a Nonlinear analysis the response of the component is not a linear function of the magnitude of the applied loads.
View the Orientation of the Triad.
View the Action bar.
Rename the default Simulation title.
Click Simulation Properties from the Setup tab in the Action bar.
The Properties dialog box is displayed. The default Title is Physics Simulation#########.
Enter Two Ring Assembly for new Title.
View your options for input.
Click OK from the Properties dialog box.
Use the Assistant. The Assistant is a useful tool if you are a beginner or experienced in simulation. The Assistant helps the user understand what conditions are required for the study.
Right-click in the Graphics area.
The Assistant dialog box is displayed.
Click Setup from the Assistant dialog box. View the two mesh options in the Assistant dialog box. Apply a Global mesh. Use the default element type (Tetrahedron second-order elements).
Mesh refinement is very important in regions of high stress concentrations such as regions of contact or sharp corners. Typically a smaller element size yields more accurate results, but increases the run time.
Mesh the model.
Click Mesh Specifications from the Commands box.
The Mesh Specifications dialog box is displayed.
Click Part1-Large Ring.
Hover over the various Mesh options and commands.
Click the Edit Mesh Specifications icon. View the default Mesh size (length of one side of a tetrahedron in a mesh) The default Mesh elements per hole is 8. Accept the default sizes at this time. Click Cancel.
Click OK from the Mesh Specifications dialog box.
The Mesh is generated for the assembly.
Click Materials (0/2) from the Assistant dialog box.
Apply material to both parts. Apply AISI 1020 Steel.
Click Material Palette from the Commands box.
The Material Palette dialog box is displayed. The Material Palette enables you to browse from materials, research their attributes, compare them and apply them to components in the model.
Select All. Display the available materials. Enter AISI 1020 in the Filter Search box.
Drag and drop AISI 1020 Steel on the first part.
Click the green check mark.
Drag and drop AISI 1020 Steel on the second part.
Click the green check mark.
Close the Material Palette dialog box.
Display the Simulation study tree.
Right-click in the Graphics area.
Click Display, Tree Display. The Simulation study tree displays the Structural Simulation Process. Model (Geometry, Meshing (Element Family), and Property Definition). Scenario (Simulation Type, Solution Method, Element Type, Boundary Conditions, Loads, and Solver). Result (Types of plots, Animations and Tools).
Contact between Surfaces
Display the Assistant dialog box.
Apply a General Contact to the assembly.
Click Contact from the Assistant dialog box.
Click General Contact. The General contact method defines the default behavior for contacting surfaces thoughout an assembly. The benefit of the General contact method is that it detects contact interactions between surfaces automatically. The General contact method in Linear Structural Validation is frictionless.
The General Contact dialog box is displayed. Accept the default name.
Click OK from the General Contact dialog box.
No Connections (Bolts, Springs, Pins, etc.) are required in this study.
Boundary Conditions – Fixed Displacement
Apply two restraints to restrict the motion of the assembly at two different locations.
Click Boundary Conditions from the Assistant dialog box.
Click Fixed Displacement from the Commands box.
The Fixed Displacement dialog box is displayed. Apply the first restraint.
Click the flat face of Part1-Large ring as illustrated.
Select Translation: X, Y, Z to prevent movement along the X-, Y- and Z- axes.
Click OK from the Fixed Displacement dialog box.
Apply the second restraint. Restrain the motion of the assembly normal to the direction of the applied load.
Click Fixed Displacement from the Assistant dialog box. The Fixed Displacement dialog box is displayed.
Rotate the model and select the four flat faces of the Part2-Small Ring plate.
Select Translation: Y, Z as illustrated to prevent movement along the Y- and Z- axes.
Click OK from the Fixed Displacement dialog box.
Loads – Pressure
Apply a pressure load to the assembly. The default solver units are N/m2.
Note: To modify the default solver units, click the Avatar, Preferences from the top menu bar. Expand Parameters, Measures, and Units. Click Units. Reset default solver units from the drop-down menu. Click Apply. Click OK.
Click Loads from the Assistant dialog box.
Click Pressure from the Commands box. A pressure is a distributed load applied normal to a surface. A pressure definition consists of two components: Transmission surface and Magnitude.
The Pressure dialog box is displayed.
Click the back flat face of the Part2-Small Ring plate. Apply pressure normal to the surface.
Enter -3500000N-m2. The negative value represents a pulling load.
Click OK from the Pressure dialog box.
Run the Simulation study. Use the Physics Results Explorer App to manage results data from Simulations performed within the 3DEXPERIENCE platform.
Click Simulate from the Assistant dialog box.
Click Simulate from the Commands box.
The Simulate dialog box is displayed. For a new user, it is recommended to run the Simulation using Local interactive. Local interactive is set by default using an embedded license. The Simulation is excuted on your computer and the user interface is locked while the Simulation is in process. Using an Educational license, up to 4 physical cores are supported.
Click OK from the Simulate dialog box.
Expand and read the Warnings.
Close the Simulation Status dialog box.
Close the Assistant dialog box.
Analyze the simulation results to understand the stress and displacement patterns that develop as the load deforms the model. The Von Mises Stress plot is displayed by default.
In this example, use the results plots for the Von Mises stress, Displacement, and Factor of Safety (FOS). Verify that the Von Mises stresses do not exceed the material’s yield strength. For most metals, the yield strength is defined as the stress point at 0.2% strain offset. For AISI 1020 Steel this is (3.516 × 108N/m2). The maximum Von Mises stress (5.28 × 108N/m2) is above the material yield strength of (3.516 × 108N/m2). Basics of Stress Limits for 3DEXPERIENCE – YouTube
The mouse cursor automatically acts as a probe.
Rotate the assembly to view the highest stress area.
Click a point on the model as illustrated. View the Von Mises Stress at that point. A Pop-up menu is displayed.
Click the Show Min/Max Values icon from the Pop-up menu. If a part sustains high stress values that exceed the material’s yield strength (3.516 × 108N/m2), you need to validate that the part is safe from material failure.
View the location of the Global Min and Global Max values.
The maximum stress occurs in the region where the two rings come into contact. If these were the operational loading conditions, you need to increase the contact surface by enlarging the diameters of the two rings or by using a softer material that would result in larger ring deformation. By increasing the contact surface area between the two rings, you reduce the localized contact stresses.
Softer materials deform easily under external forces, such as stress, strain, temperature, or light. They have low elastic moduli, high strain limits and viscoelastic behavior. Example: Elastic Modulus of AISI 1020 Steel is (2 × 1011N/m2). Yield strength of AISI 1020 Steel is (3.516 × 108N/m2). Compare to 6061, Alloy Elastic Modulus is (6.9 × 1010N/m2). Yield strength is (5.515 × 107N/m2).
Click Hide Max or Min values and close from the Pop-up menu.
Create a Displacement contour plot. Note: In SOLIDWORKS Simulation the URES Resultant Displacement and the Displacement in 3DEXPERIENCE Simulation represent the same displacement components. Displacement Component 1, 2 and 3 in 3DEXPERIENCE Simulation represent the same displacement components as UX, UY and UZ in SOLIDWORKS Simulation.
Notice the low displacement (9.48 × 10-32 mm) in the area of Part1-Large Ring which is fixed.
Part2-Small Ring has the highest displacement values due to the action of the applied pressure.
The pulling, due to the pressure (3500000N-m2) applied to Part2-Small Ring, affects the displacement of Part1-Large Ring displayed in red, yellow and green.
Factor of Safety
Review the Factor of Safety (FOS) contour plot to identify the critical regions of the model.
The FOS plot displays how close a material is to yielding. The factor of safety is calculated by dividing the material’s Proof (Yield) Strength by the Allowable stress.
Create a Factor of Safety (FOS) contour plot.
The FOS plot has a maximum limit of 2 by default. Regions of the model with a FOS larger than 2 are displayed in gray. Regions of the model with a FOS less than 1 develop stresses above the material’s yield strength under the current loading conditions.
The smallest factors of safety occur in the localized regions where the highest Von Mises stresses occur.
Create a Contour plot animation.
Click Play Animation from the Results tab in the Action bar.
View the animation.
Click Stop and Rewind.
Save and Close
Save the Simulation study.
Click the Share icon as illustrated.
Click Save. Model and Scenario data is always stored on the 3DEXPERIENCE server in your Collaborative space.
Results data may be stored on the server or in a local directory on your machine. Local data is masked, encrypted and only accessible by the owner of the data.
The default option is Server on the platform. Saving the Simulation Results data from a Simulation on the server allows other users in your Collaborative space to access that data and archive the data for future reference.
Close the Simulation study.
Click Close on the Two Ring Assembly A tab.
We are finished with this lesson.
Academic Community: After you create a 3DEXPERIENCE ID, Educators, can get more information on xDesign and SOLIDWORKS. Request to join the 3DEXPERIENCE Academic Community for free at go.3ds.com/academiccommunity.
Student Community: Students, join the student community for free at go.3ds.com/studentcommunity. Check out great posts on Mechanism Mondays, FEA Fridays, Solid Saturdays (animations), Formula Student and Formula SAE exercises.
Additional Lessons in 3DEXPERIENCE Simulation Series:
Additional Lessons in this series on 3DEXPERIENCE Works:
Additional Lessons in this series on SOLIDWORKS xDesign:
More lessons and learning paths on SOLIDWORKS, SOLIDWORKS Simulation and 3DEXPERIENCE Simulation can be found at My.SOLIDWORKS.com.
Design well. Marie