What is in this Article?
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 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
Pushover analysis for beam models is now supported by the Akselos solver. Pushover capabilities within Akselos solver can provide insight into the structural aspects by enabling the users to conduct a full elastoplastic pushover analysis of a structure.
In this tutorial, we will do the pushover analysis for the frame model with the 1D beam element. It will guide you on how to create the beam frame model via the Akselos Modeler tool. You will learn how to create, apply loads, set up time steps, boundary conditions on the model, and solve the simulation step by step.
Figure 1.1. Pushover analysis with 1D beam element workflow
2. Problem Description
In this tutorial, we use the 1D beam element to build the beam frame model which is constrained at 4 legs, under self-weight, and forces applied on 4 points on top. FV is the constant load. FH is the pushover load which is increased by step until any degree-of-freedom displacement first equals or exceeds 0.25m then the solver will terminate. This time also means the structure is considered collapsed. The model schematic and beam cross-section are shown in the figure below.
Figure 2.1. The beam frame problem
The beam geometry, beam properties, and load cases used in this example model are as follows:
- Beam cross-section (m): Tubular with below dimensions:
- Cross-section 1 :
- Diameter: 1.016 m
- Thickness: 0.035 m
- Cross-section 2 :
- Diameter: 1.0 m
- Thickness: 0.04 m
- Cross-section 3 :
- Diameter: 2.0 m
- Thickness: 0.06 m
- Cross-section 1 :
- Material with the below properties:
- Mass density: 8000 kg/m3
- Poisson ratio: 0.3
- Young Modulus: 210 GPa
- Tangent Modulus: 0.42 GPa
- Yield Stress: 330 MPa
- Applied loads:
- Self-weight
- Constant Load: FV = 30 MN (Point Load)
- Pushover Load: FH = 30 MN (Point Load)
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 Pushover Analysis Collection here on Akselos Portal.
- By default, you can use Akselos Cloud (available in Akselos Modeler).
Note:
▶ If you have not installed Akselos Modeler yet, please see Akselos Modeler - Installing, Updating and Managing the Akselos Simulation Software to download and install the software.
▶ If you have trouble accessing to any of those prerequisites. Please contact us at: support.akselos.com
Follow the steps below to import the Pushover 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 Pushover 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 Pushover 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 Pushover collection
4. Implementation
In the Implementation section, we will show you a step-by-step in detail guide on how to analyze the pushover problem in Akselos Modeler.
Figure 4.1. Pushover analysis with 1D beam element workflow
Step 1: Create Nodes
Figure 4.2. Create Model – Create Nodes
Akselos Modeler provides an Edit Beams tool that helps users create nodes and beams. The tool also can modify beams such as split/merge or change the beam type.
- On the left panel, select the Edit Beam tool.
Figure 4.3. The Edit Beams tool interface
To build the beam frame, 13 nodes need to be created first. Akselos Modeler provides tools for manually creating nodes or quickly importing multiple nodes using a CSV file with coordinates. For this tutorial, we have prepared a CSV file available in the collection - Model_Node.csv.
- Option 1 - Create nodes manually from table: Click the + icon to add rows until there are 13 rows in the table. Enter the X, Y, Z coordinates as shown in the figure below, then click the Create Nodes button
Figure 4.4. Creating nodes manually
- Option 2 - Creating nodes from csv file: Click the Import icon shown below, select Model_Node.csv in the collection to import the file. The node coordinates will appear in the table, just like in Option 1. Finally, click the Create Nodes button to generate the nodes.
Figure 4.5. Creating nodes from the csv file
Once the above steps are completed, 13 nodes will appear in the Graphic Window.
Figure 4.6. Thirteen nodes on the Graphic Window after creating
Step 2: Create Beams Model From Nodes
Figure 4.7. Create Model – Create Beams Model From Nodes
From these nodes, you can create the beam frame. Click the Create Beam From Nodes button, then select nodes in the Graphic Window — each pair of selected nodes will form one beam. Repeat this process until all 28 beams are created, completing the model.
Figure 4.8. Creating beams from nodes
Step 3: Split Beams
Figure 4.9. Create Model – Split Beams
- In the Edit Beams tool, navigate to the Split/Merge tab. Select all beams in the Graphic Window, enter 8 in the Number of Segments box, and choose the Equal Parts option. Then, click the Split button
Figure 4.10. Splitting beams
Figure 4.11. The model after splitting
Step 4: Add Cross-sections
Figure 4.12. Assign Properties – Add Cross-sections
In this step, we will guide you to create and define three cross-sections and then apply them to the model.
- In the Model Tree on the left panel, right-click on Model → Insert Property → Cross-Sections. The group of cross-sections will be created with one default item. You can add more Cross-sections by right-clicking on the group → Insert Property → Crosssectiongroupitem or delete them by clicking on then pressing the Delete button.
Figure 4.13. Creating CrossSectionGroup
- Click on Cross-Section 1 then see the Property Tree → Define the dimensions.
Figure 4.14. Defining Cross-section properties
- Insert two more cross-section items and define them.
Figure 4.15. Defining Cross-sections 2 & 3
After this step, three cross-sections have been created but they are not yet assigned to the beams. We will proceed to Step 5, and once it is completed, the software will automatically assign both the first cross-section item and material to the beams. At that point, we will review where to modify them to correct the model.
Step 5: Add Materials
Figure 4.16. Assign Properties – Add Materials
- In the Model ribbon on the left panel, right-click on Model → Insert Property → Materials. The group of materials will be created with one default item. You can add more Materials by right-clicking on the group → Insert Property → Materialgroupitem or delete them by clicking on then pressing the Delete button.
Figure 4.17. Creating MaterialGroup
- Click on Material 1 then see the Property Tree → Define the properties of elasticity.
Figure 4.18. Defining elasticity properties of Material 1
- In the Property Tree of Material 1, right-click on value → Insert New… → plasticity → Expand hardening_model and input values to tangent_modulus and yield_stress.
Figure 4.19. Inserting and defining plasticity properties of Material 1
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 4.20. A place to check material/cross-section items that are assigned to the beam
The model is currently assigned the first cross-section item as in the figure above. We need to update the cross-section for the four legs and the upper beams to match the given specifications.
- Select the elements of the upper beams, then go to the Property Tree and choose Cross-Section 2.
- Select the elements of the four support legs, then go to the Property Tree and choose Cross-Section 3.
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 4.21. Showing beam model with cross-section on the Graphic Window
Step 6: Constrain Model
Figure 4.22. Model Set-up – Constrain model
In this tutorial, four legs of the frame are constrained. We will constrain 4 nodes at the bottom of the model. Before doing it, we need to create a Node Port at these nodes and then fix them.
- Firstly, we need to turn on the Unconnected Ports and Boundary Conditions options in Configure view settings. The ports and boundaries of the model are visualized on the Graphic Window.
Figure 4.23. Turning on Unconnected Ports and Boundary Conditions options
- Select the bottom node, then right-click in the Graphic Window and choose Create Node Port. Repeat this process for the remaining three nodes. Note: Nodes must be selected one by one, as the tool does not support multiple selections.
Figure 4.24. Creating Node Port

- To constrain them, select the four newly created node ports, then go to the Property Tree and choose (x, y, z, theta_x, theta_y, theta_z) under Constraint Type. The software will automatically apply the same constraints to all selected ports. Once completed, black points will appear at the four ports, indicating they have been successfully constrained.
Figure 4.26. Constraining node ports
Figure 4.27. The model with four constrained nodes
Step 7: Set Time Array & Time Steps
Figure 4.28. Model Set-up – Set Time Array & Time Steps
The incremental steps in pushover analysis represent the progression of loading from one limit state to another as the applied lateral forces increase. The magnitude of these increments depends on factors like the required accuracy, the complexity of the structure, and the specific objectives of the analysis. Smaller increments generally provide more precise results but lead to longer computation. In this step, we will guide you on how to set up time steps in Akselos Modeler for the load applied in the next step.
- Time Array: The model has both constant loads and pushover loads, time_array should be an array with two entries: e.g. "time_array": "step_array([0.0, 1.5])*s". The solver initializes constant loads in the first step (at t = 0), and the pushover loads are added to the model in the second step.
- To create a time array property, right-click on Model on the left pannel →Insert New→Generic Property →Property.
Figure 4.29. Inserting Model Property
- Rename the recently created property to time_array, and enter into the box as in the figure below.
Figure 4.30. Time array property
- Time Steps:
- There are three child items in this property tree: load_substep_type, number_of_substeps, and time. The load_substep_type can be changed from a drop-down list of options, but the number_of_substeps must be given by the users. It should be noted that the time_array established previously is used to enter time.
- There are three child items in this property tree: load_substep, number_of_substeps, and time.
- The default value of max_arclen_substep is 100, which is sufficient in most cases. However, for some test cases, this value may need to be increased for the solver to trace a complete load-displacement curve.
- The max_displacement_size stopping control method is optional, it uses the user input value as a criterion to stop solving. This input value represents the maximum allowable displacement (of any node in the structure) before the structure is considered collapsed.
- To change the time steps settings, select default_time_stepping on the left panel.
Figure 4.31. Default_time_stepping
- In the Property Tree, right-click on default_time_step → Insert new → number_of_substeps (InPropertyArray).
Figure 4.32. Inserting number_of_substeps
- Change load_substep_type to ArcLengthContinuationProperties.
Figure 4.33. Setting load_substep_type
- Right-click on load_substep_type → Insert new → path_predictor_type (PathPredictorType).
Figure 4.34. Inserting path_predictor_type
- Right-click on auto_step_properties → Insert New → max_displacement_size (m).
Figure 4.35. Inserting max_displacement_size
- Right-click auto_step_properties → Insert New → max_substeps (PropertyArray).
Figure 4.36. Inserting max_substeps
- Change all values as in the figure below.
Figure 4.37. Setting default_time_stepping properties
Step 8: Apply Loads
Figure 4.38. Model Set-Up – Apply Loads
In this tutorial, there are three load cases applied to the mode (Self-Weight, Point-Load-Constant, Point-Load-Pushover). Self-Weight is applied on a subdomain selection and two Point-Load are applied on four nodes. To create a load applying on the node, we need to create Node Set and store them in Stored Selection.
- Create Node Set:
- Change to the Collection ribbon → Show component tree → Right-click on Boundary Sets → Create Boundary Set → Node.
Figure 4.39. Creating Node Set
- Click on New Node → Select four nodes on top as the figure below.
Figure 4.40. Selecting four nodes for Node Set
- We need to turn on the PointLoad operator for this Node Set. Click on New Node → see the Property Tree and turn on PointLoad in Operators.
Figure 4.41. Turning on the PointLoad operator
- After all, we need to save the change of component. Right-click on the component → Save Changes
Figure 4.42. Saving component
- Stored Selection for Self-Weight Load Case:
- Change to the Model ribbon → On the left panel, right-click on Stored Selections → Create Subdomains Selection.
Figure 4.43. Creating Subdomains Selection
- Click on Subdomain Selection 1 → Select the model on the Graphic Window.
Figure 4.44. Storing Subdomain for Self-Weight load case
- Stored Selection for Point-Load Load Case:
- Right-click on Stored Selections → Create Boundary Sets Selection.
Figure 4.45. Creating Boundary Set Selection
- Click on Subdomain Selection 1 → Select node-set (New Node created in the previous step) on the Graphic Window. Because the position of this node set coincides with another one, to select the right node-set, move the mouse to one of its nodes, use the Tab button to change to the right name shown at the bottom of the Graphic Window then click once.
Figure 4.46. Storing node sets for Point-Load load case
- Create Self-Weight Load Case:
- Right-click on Load Cases → Create Load Case
Figure 4.47. Creating Load Case
- Right-click on Load Case 1 → Create Load
Figure 4.48. Creating load in load case
- Click on Load 1 → see the Property Tree and set them as in the figure below.
Figure 4.49. Defining Self-Weight load
Figure 4.50. The load vector of self-weight appeared after applying
- Create Point-Load-Constant Load Case:
- Right-click on Load Cases → Create Load Case.
Figure 4.51. Creating Load Case
- Right-click on Load Case 2 → Create Load
Figure 4.52. Creating load in load case
- Click on Load 1 of Load Case 2 → see the Property Tree and set them as in the figure below.
Figure 4.53. Defining Point-Load
Figure 4.54. The load vectors of the point load (constant load) appeared after applying
- Create Point-Load-Pushover Load Case: We can copy from Load Case 2 and modify some values to use.
- Right-click on Load Case 2 → Clone.
Figure 4.55. Creating load case by cloning from another one
- Expand Load Case 3 → click on Load 1 → Modify the values in the Property Tree as in the figure below.
Figure 4.56. Creating load in load case
To easily manage the load cases, we should rename them following the load (Right-click on it → Rename this Load Case or click on it → press F2 button)
- Load Case 1 = Self-Weight
- Load Case 2 = Point-Load-Constant
- Load Case 3 =Point-Load-Pushover
Figure 4.57. Renaming three load cases
Step 9: Create Solver Option
Figure 4.58. Solve – Create Solver Option
For the 1D beam element problem, we can only solve it with the FEA solver.
- Under Solver Options on the left panel, there is RB-FEA Options, it is the default and can be used 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 4.59. Setting FEA Solver
- In the Solver Option, 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, Bending Moments, and Plastic Indicator. Turning on three options as in the figure below.
Figure 4.60. Adding some fields on Solver Option
Step 10: Create Scenario 
Figure 4.61. Solve – Create Scenario
- Under Scenario on the left panel, there is Default Scenario and we can use it. Click on Default Scenario → See the Property Tree and set the coefficients of Point-Load and Self-Weight to 1.0.
Figure 4.62. 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 4.63. Setting Solve list
Step 11: Sync Collection and Solve
Figure 4.64. Solve – Sync collection & Solve
Now you can proceed to solve the model. First, you have to save aks file to save all setting up the model → sync the collection to Akselos Dashboard → Run solving.
- Save aks File:
- Click on the File tab →Save.
Figure 4.65. Saving aks file
- The Select destination to save the file window appears, 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 4.66. Naming and saving aks file
- Sync Collection:
- Change to the Collection ribbon → Click on Repository... → Sync.
Figure 4.67. Syncing collection
- Click the Commit button when this window appears.
Figure 4.68. 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 4.69. Solving model
Figure 4.70. Solution after solving.
5. Results
Figure 5.1. Validate – Compare with theoretical results.
After receiving the solution, you can study its solution fields. There are some solution fields (visualization & results). You can review it to compare it with yours.
Figure 5.2. Axial Force result
Figure 5.3. Displacement x-direction result
Figure 5.4. Displacement y-direction result
Figure 5.5. Displacement z-direction result
Figure 5.6. Plastic Indicator result
Figure 5.7. Shear Force results
Figure 5.8. Bending Moment results
- Validation:
The horizontal response calculated by the Akselos solver for the current jacket structure is compared to reference results [1] in the figure below. In terms of ultimate load capacity, the results appear to be in good agreement.
Figure 5.9. Load-displacement curves for the Four-legged jacket structure
[1] Engseth, A. Finite Element Collapse Analysis of Tubular Steel Offshore Structures, Div. of Marine Structures, The University of Trondheim, The Norwegian Institute of Technology, Trondheim, 1984.
Was this article helpful?
That’s Great!
Thank you for your feedback
Sorry! We couldn't be helpful
Thank you for your feedback
Feedback sent
We appreciate your effort and will try to fix the article