Cantilever Beam with 1D Elements

Modified on Thu, 13 Feb at 10:04 AM

What is in this Article?

1. Introduction

2. Problem Description

3. Before We Start

4. Implementation

5. Results Verification


     Terminologies

Collection

The folder containing data of an asset/model on Akselos Cloud or users’ computer

Components

Components created by the componentization process to use with Akselos Integra 

Node port

A mesh node or beam end is used to connect 1D beam elements to other component types 

Nodeset

A mesh node assigned with a certain ID number

Model ribbon

An Akselos Modeler ribbon containing tools for model assembling and management

Ribbons

The top-sided toolbars of Akselos Modeler

Property Tree

A panel at the left bottom of Akselos Modeler, where shows properties of user selection


1. Introduction

This tutorial will guide you through the simulation process of a 1D beam model. You will learn how to create, assign cross-section, merge, split, and handle orientations of 1D beams to create a 1D beam model. You will also learn to apply loads and boundary conditions on 1D beams then solve the model.

Figure 1.1. 1D cantilever beam problem workflow


2. Problem Description

In this tutorial, we use the 1D beam elements to simulate a cantilever beam model which is clamped on 1 side and free on the other side, under a uniformly distributed load W=1000 N/m. The model schematic and beam cross-section are shown in the figure below.

 

Figure 2.1. Cantilever beam with a uniformly distributed load

The beam geometry and beam properties used in this example model are as follows:

  • Total length (L) is 2 (m)
  • Beam cross-section (mm): B = 37.5, b = 4.525, H = 65 and h = 4.525
  • Young’s modulus (E) of material is 200e9 (Pa), Poisson (ν) is 0.3
  • Mass density: 7850 kg/m3

Figure 2.2. The beam Cross-section


3. Before We Start

To follow the instructions below, please notice the point below:

  • A new collection in your Organization is required to store this model on Akselos Portal (https://dashboard.akselos.com). Don’t know how? Read more Start building your asset with a new collection.
  • Akselos Modeler – our simulation is required to build this model.
  • A sample collection has been prepared for you to use as a reference. Find the Steel-Beams here on Akselos Portal.
  • By default, you can use Akselos Cloud (available in Akselos Modeler).

Note: If you have trouble accessing to any of those prerequisites. Please contact us at: support @akselos.com

 

Follow the steps below to import the Steel-Beams collection into Akselos Modeler:

  • In Akselos Modeler, click on the Cloud tab on Ribbons → Authentication  Enter your username and (password or token) → Click on the Check button and wait for Authentication status to turn green and show Authentication successful. 

Figure 3.1. Checking authentication

  • On the Collections tab, click on Import Collection…  On the Import Collection window, find and select Steel-Beams collection Click on the Import button to pull the collection into your computer. You will receive a success message on the Logs screen when the collection is successfully imported.

Figure 3.2. Importing Steel-Beams collection into the local machine

  • On the File tab, click on New Model from Current Collection. The collection is ready to use after this step. 

Figure 3.3. Create a new working space in the Steel-Beams collection


4. Implementation

In the Implementation section, we will show you a step-by-step in detail guide on how to analyze the basic 1D beam problem in Akselos Modeler.

Figure 4.1. 1D cantilever beam problem workflow


Step 1: Create Nodes

Figure 4.2. Create Model – Create Nodes

In Akselos Modeler, we use the Edit Beams tool to create the 1D beam. It is located on the Right Panel.

Figure 4.3. Edit Beams tool interface

  • Click on the '+' icon to add a row to the table, each row corresponds to a node. We will create two nodes with the coordinates as shown below  Click on Create Nodes to add two nodes to the Graphic Window.

Figure 4.4. Adding nodes' coordinates


Step 2: Create Beam model from nodes

Figure 4.2. Create Model – Create Beam model from nodes

After two nodes have been created, we will create a beam from them by clicking on the Create Beam From Nodes button Select two nodes on the Graphic Window.

Figure 4.5. Creating a beam from two nodes


Step 3: Split Beam

Figure 4.6. Create Model – Split Beam

A single beam may not give us good results compared to theoretical results. To increase accuracy, we should split the beam into several sub-beams.

  • In the Edit Beams interface, change to the Split/Merge tab Select the beam on the Graphic Window  Input 4 into the Number of Segment box Leave the default for other options and click on the Split button.

Figure 4.7. Steps to split beam

Figure 4.8. A beam with four equal elements after splitting

Optional: We also have the Merge Beams tool that allows merging two selected beams together into a single beam. If we select more than two beams, we will receive a message on the Logs that we can not merge more than two elements.

Figure 4.9. Steps to merge beams

Figure 4.10. A beam after merging two elements


Step 4: Add Cross-section

Figure 4.11. Assign Properties – Add Cross-section

In this step, we will guide you in creating and defining a cross-section. Then the process of applying it to the beam model.

  • In the Model Tree on the left panel, right-click on Model  Add Property  Cross-Sections. The group of cross-sections will be created with one default item. You can add more Cross-sections in the group by right-clicking on the group → Add Property  Crosssectiongroupitem or delete them by clicking on then pressing the Delete button. 

Figure 4.12. Creating CrossSectionGroup

  • Click on Cross-Section 1 then see the Property Tree→ Choose IbeamCrossSection in the cross_section box Define the dimensions (height = H + 2*h = 65 + 2*4.525 =74.05 mm). 

Figure 4.13. Defining Cross-section properties

After this step, the cross-section has been created but is not yet assigned to the beam. We will proceed to Step 5, and once it is completed, the software will automatically assign both the cross-section and material to the beam. At that point, we will review where to modify them if needed.


Step 5: Add Material

Figure 4.14. Assign Properties – Add  Material

  • In the Model Tree on the left panel, right-click on Model Add Property Materials. The group of materials will be created with one default item. You can add more items by right-clicking on the group → Insert Property Materialgroupitem or delete them by clicking on then pressing the Delete button.

Figure 4.15. Creating MaterialGroup

    • Click on Material 1 then see the Property Tree  Define the parameters for material.

Figure 4.16. Defining material properties

As mentioned at the end of Step 4, once the material is created, the software will automatically assign both the material and cross-section to the beam. To verify this, switch to Mesh Elements Selection mode, select any element on the Graphic Window, and expand the Properties section in the Property Tree. There, you will see the assigned items for that element.

Figure 4.17. A place to check material/cross-section items that are assigned to the beam

Akselos Modeler provides a tool to visualize the beam's cross-section. In the Graphic Window, open the Configure View Settings menu and enable the Show Beam Cross-section option.

Figure 4.18. Showing beam model with cross-section on the Graphic Window


Note: This tool will not function if the beam has not been assigned both a material and a cross-section.


Step 6: Constrain Model

Figure 4.19. Model Set-Up - Constrain model

Before we solve the model, we need to apply boundary conditions. Boundary conditions specify how the beam is supported or fixed at its ends or along its length. In this tutorial, we will apply the boundary condition by fixing the node at the end of the beam.

A related article that is useful for you to know and implement in this section: Boundary Conditions.


  • To visualize the model's ports and boundaries in the Graphic Window, enable the Unconnected Ports and Boundary Conditions options in the Configure view settings.

Figure 4.20. Turning on Unconnected Ports and Boundary Conditions options

  • In the Mesh Elements selection mode, select the node at the beam end Right-click on the Graphic Window → Create Node Port.

Figure 4.21. Creating Node Port

  • To constrain the node port, select it Then go to the Property Tree and choose (x. y, z, theta_x, theta_y, theta_z) in Constraint Type. Once applied, a black point will appear at the port, indicating that it has been successfully constrained.

Figure 4.22. Constraining node port

Figure 4.23. The beam model with the constrained node


Step 7: Apply Loads

Figure 4.24. Model Set-Up - Apply loads

In this step, we will apply load on the model. For beams, we can apply four types of loads: Point load, Linear distributed load, Partial distributed load, and Self-weight. For this example, the model only has one uniformly distributed load = 1000 N/m, therefore we can choose the Linear distributed load type.

Some articles are useful for you to implement in this section: Stored Selection, Create Load Case and Load.
  • Stored Selection: Firstly, we need to have a stored selection to apply load on. Change to Subdomains selection mode Select the beam on the Graphic Window Right-click then press Store current selection. The stored selection item will appear under Stored Selection on the left panel.

Figure 4.25. Steps to store model for applying loads

  • Load Case: On the left panel, right-click on Load Cases Add Load Case  Right-click on Load Case 1 Add load...  The  New Load Case / Load window will appear, search and select Linear Distributed Load With Moment  Click on the Add button.

Figure 4.26. Creating Load Case and Load

  • Click on Linear Distributed Load With Moment  In the Property Tree, select the Stored Selection which is stored above   Enter the value for force as shown below.

Figure 4.27. Creating Linear Distributed Load

Figure 4.28. Load visualization


Step 8: Create Solver Option

Figure 4.29. Solve - Create Solver Option

For the 1D beam element problem, we can only solve it with the FEA solver.

  • Set Solver Option:
    • Under Solver Options on the left panel, there is the default - RB-FEA OptionsWe can use it with some changes. Click on RB-FEA Options → See the Property Tree and change Solver Strategy to FEA. After changing, the name of the default solver will automatically change to FEA Options.

Figure 4.30. The default Solver Option

Figure 4.31. Setting FEA Solver

    • In the Property Tree of FEA Options, you can choose the result fields that you want to visualize. The default results of the solution are displacements in x, y, z-directions. In this example, we choose some additional fields which are Axial Force, Shear Forces and Bending Moments. Turning on two options as in the figure below

Figure 4.32. Adding more solution fields on the Solver Option


Step 9: Create Scenario

Figure 4.33. Solve - Create Scenario

  • Under Scenario on the left panel, there is Default Scenario and we use it. Click on Default Scenario  See the Property Tree and set the coefficients of Load Case 1 to 1.0.

Figure 4.34. Setting Scenario

  • Set Solve List: Since there is only one scenario, select the default in Solve List to check that the default scenario is turned on.

Figure 4.35. Setting Solve list


Step 10: Sync Collection & Solve

Figure 4.36. Solve - Sync collection & Solve

Now you can proceed to solve the model. Firstly, you have to save the aks file to save all settings of the model Sync the collection to Akselos Portal  Run solving.

  • Save aks File:
    • Click on the File tab Save

Figure 4.37. Saving aks file

    • The Select destination to save the file window will appear, enter the name into the File name box then click the Save button. You will receive a success message when the file is successfully saved. 

Figure 4.38. Naming and saving aks file

  • Sync Collection:
    • Change to the Collection ribbon Click on Repository...  Sync

Figure 4.39. Syncing collection

    • Click the Commit button when this window appears.

Figure 4.40. Committing for synchronization

  • Run Solving:
    • Change to the Solutions ribbon Click on the Solve button. The solving request will be submitted to Akselos Cloud. You will see the status of this request on the Solution tree. You can see the results once the solving is done, which is usually within seconds with Akselos solver. 

Figure 4.41. Solving model

After a few seconds, you should receive the solution as shown in Figure 4.52. To visualize the solution, you need to change the Solution Field on the Graphic Window.

 Figure 4.42. The Solution returned after solving


5. Results Verification

Figure 5.1. Validate - Compare with theoretical results

There are some solutions of the model after solving:

  • Displacement z: maximum = 0.01953 (m)

Figure 5.2. Displacement z

  • Shear force: maximum = 2000 (N)

Figure 5.3. Shear force

  • Bending moment: maximum = 2000 (Nm)

Figure 5.4. Bending moment

To validate the results obtained from Akselos' solution, we compared Akselos's results with theoretical results, which turned out to match each other as shown in the following table.

The maximum deflection of the beam is given by the formula:

Where I is the moment of inertia. For the beam cross-section considered here, I = 514247 mm4.

Table 5.1. Comparison between Akselos's solution and analytical solution


Analytical solution
Akselos Solution
Error
Maximum Displacement
Max = w.L^4/(8.E.I) = 0.01945 (m)
0.01953 (m)
0.4%
Shear forces shapeLinearLinear
Maximum shear forceV = w.L = 2000 (N)2000 (N)0%
Bending moments shapeQuadraticQuadratic
Maximum bending momentsM = w.L^2/2 = 2000 (Nm)2000 (Nm)0%

Related Articles & Similar Case Studies:


Was this article helpful?

That’s Great!

Thank you for your feedback

Sorry! We couldn't be helpful

Thank you for your feedback

Let us know how can we improve this article!

Select at least one of the reasons
CAPTCHA verification is required.

Feedback sent

We appreciate your effort and will try to fix the article