Terminologies
| Terminology | Paraphrased Description |
|---|---|
| Collection | A directory that stores all data related to an asset or model, either on the Akselos Cloud or on a local machine. |
| Components | Structural or logical entities generated through the componentization process for use with Akselos Integra. |
| Node port | A mesh node or beam endpoint used to connect 1D beam elements with other component types. |
| Node set | A group of mesh nodes identified and referenced by a specific ID number. |
| Model ribbon | A dedicated ribbon in Akselos Modeler that provides tools for assembling and managing models. |
| Ribbon | The set of toolbars displayed at the top of the Akselos Modeler interface. |
| Property tree | A panel located at the lower-left area of Akselos Modeler that displays properties of the currently selected item. |
1. Introduction
Floating Offshore Wind Turbines (FOWTs) are wind turbines installed on floating platforms that are stabilized by mooring systems rather than fixed foundations. Different floater concepts, such as spar, semi-submersible, and tension leg platforms, lead to significantly different global structural behavior, load transfer mechanisms, and dynamic response. As a result, structural modeling of FOWTs requires a workflow that can consistently represent these characteristics while remaining efficient for engineering assessment.
Figure 1.1: Typical Floating Offshore Wind Turbine floater concepts
Within Akselos, FOWT assessment is performed as part of a structured workflow in SPM, covering model preparation, structural assembly, load definition, simulation, and result evaluation. This tutorial sits within that overall workflow and focuses on one specific stage of the process. Supporting pre-processing steps are demonstrated using Akselos Modeler where appropriate, while the core analysis and evaluation are carried out through SPM and its User Interface.
Figure 1.2: High-level Akselos FOWT workflow in SPM
Problem Description
In the provided DeepCwind 5MW reference model, one structural component is not yet assembled into the overall system. Without this component, the structural model is incomplete and cannot accurately represent the global behavior of the floating wind turbine. The missing component must be properly introduced, configured, and connected so that stiffness, mass, and load paths are transferred correctly throughout the structure.
Figure 1.3: DeepCWind 5MW model and the missing component
This tutorial addresses that gap by guiding users through the assembly of the missing component and its integration into the existing DeepCwind model.
Tutorial Scope
This tutorial covers the model assembly stage of the DeepCwind 5MW Floating Offshore Wind Turbine workflow. By the end of this tutorial, users will be able to:
Import the missing FOWT structural component along with its associated settings.
Define and assign the required 1D cross-section properties.
Assemble the imported component into the full DeepCwind structural model with correct alignment and connectivity.
Prepare the assembled model so it is ready for subsequent steps such as boundary condition definition and load application.
Figure 1.4: DeepCwind 5MW tutorial workflow and user journey
Subsequent tutorials build on this assembled model to complete the remaining stages of the FOWT structural assessment workflow.
2. Before we start
Before configuring cross-sections for 1D stiffeners, access to the required Akselos tools and a suitable baseline model must be in place. The workflow relies on authenticated access to the Akselos Portal, availability of Akselos Modeler, and a pre-prepared reference collection. Ensuring these elements are ready avoids interruptions during the setup process.
To follow the instructions in this tutorial, access to the required Akselos tools and reference data is mandatory.
Akselos Portal account
A valid Akselos account is required to sign in to the Akselos Portal. Portal access allows users to access collections, download sample data and software installers, and connect with Akselos Modeler.
- Install Akselos Modeler
Akselos Modeler is the simulation software used throughout this tutorial. After download and install, authentication the software with your Akselos Portal account is required to import sample collections and data and to open models in Akselos Modeler.
Figure 2.1: Checking authentication
Sample collection
A reference sample collection is provided for this tutorial. After authentication, import the DCW 5MW tutorial 1 sample collection from the Akselos Portal and open it in Akselos Modeler.
Figure 2.2: Importing collection - DCW_5MW_tutorial_1
Ensure that authentication is completed and that access to the sample collection is confirmed before proceeding with the implementation steps. For access requests or assistance, contact [email protected]
3. Implementation
This section details the workflow for importing the raw mesh data, configuring the component logic, and assembling the global model within Akselos Modeler.
STEP 1: Import the Missing Component
In this step, the missing structural component required for the DeepCwind 5MW model is introduced into the existing setup. This ensures that all primary structural parts needed for global assembly are available before defining connectivity and properties.
Figure 3.1: Create Model – Import Mesh files
Akselos Modeler includes a native importer to convert Abaqus Input (.inp) mesh files into compatible Akselos components. The required mesh file for this tutorial is located within the sample collection directory: inp_file/5MW_MC_Middle_new.inp.
1. Access the Component Creator
Open the Model ribbon in the SPM User Interface.
Navigate to Collections → Create → Component Type.
Figure 3.2: Opening the Component Type creation dialog
2. Load the Mesh Data
In the Create New Component Types window, select Add Meshes.
Browse to and select the
5MW_MC_Middle_new.inpfile from the local machine.Confirm that the file is listed in the Mesh list after loading.
Figure 3.3: Selecting the input mesh file
Figure 3.4: Mesh file displayed in the Mesh list
3. Configure Import Settings
Before creating the component, define the ID ranges used to identify subdomains and connection interfaces.
Open the Settings tab.
Enter the following values to map mesh IDs to logical entities:
Stiffener:
50–100, used to identify the longitudinal stiffener and ring frame stiffener.Port:
120–130, used to identify the port sidesets for structural connection.
Figure 3.5: Configuring ID ranges in the Settings tab
4. Create the Component
Return to the Create tab.
Select Create to generate the component.
Verify that a confirmation message appears in the log indicating successful creation.
Close the dialog once the process is complete.
Figure 3.6: Creating the component and confirmation message
STEP 2: Component Configuration
After creating the component type, additional setup is required to define its structural properties and prepare it for hydrostatic load application. This includes configuring the 1D stiffener cross section, creating a surface boundary set for the outer shell, and assigning this boundary set to a hydrostatic operator.
1. Set Up the Cross Section
The procedure for creating and assigning cross-sections is a standard workflow in Akselos Modeler.
Note on Cross-Sections: For this tutorial, please refer to the Floating Offshore Wind Turbines: Set up cross-section for 1D stiffener guide to correctly configure the stiffeners for the 5MW_MC_Middle component before proceeding.Apply the cross section to the corresponding stiffener entities to ensure correct stiffness and mass representation.
Figure 3.7: Create Model – Component Editor
2. Create a Boundary Set for the Outer Shell Surface
Open the component entity in the model hierarchy using the Component Editor.
Right click on Boundary Sets → Create Boundary Set → Surface.
Figure 3.8: Creating a new surface boundary set
A new surface set named New Surface is created. Rename this boundary set to Wetted_panels or another descriptive name.
Select the entire outer shell surface:
Click on the boundary set in the tree to activate it.
In the viewport, click and hold for approximately 2 seconds on a shell element located on the outer surface.
Select the option to include all connected outer shell elements. The selected surfaces are highlighted in yellow.
Figure 3.9: Selecting all connected outer shell elements
3. Add and Configure the Hydrostatic Operator
Navigate to the Features tab in the ribbon.
Select Hydrostatic Operator to add a new operator to the component.
Figure 3.10: Adding a Hydrostatic Operator
In the Properties panel of the hydrostatic operator, locate the boundary_set field.
Select the boundary set created in Substep 2.2, for example Hydrostatic, to associate the operator with the outer shell surface.
Figure 3.11: Assigning the boundary set to the Hydrostatic Operator
At this stage, the component is fully configured with its cross section and hydrostatic definition and is ready to be positioned and assembled into the full DeepCwind model in the next step.
Optional: A new operator might contain certain parameters used for certain models. Hence, users should delete unused parameters to make the component cleaner and faster in the training process.
After completing all the steps above, save all changes within this component by right-clicking on '5MW_MC_Middle_new' and selecting Save Changes (Component).
Figure 3.12: Saving component changes
STEP 3: Assemble model
In this section, the newly created component is assembled into the global model using the Position and Assemble tool. This step ensures that the imported component is correctly placed and structurally connected to the existing DeepCwind model.
Figure 3.13: Create Model – Assemble Model
1. Open a model
Click on the File tab → Open File from Collection.
In the dialog window, select
5MW_DeepCWind_missing_MC_middle.aksand click Open.
Figure 3.14: Opening aks model
The model is loaded into the Graphic Window, and its structure and properties are displayed in the Structure tree. At this stage, the model contains all previously defined components except the newly created one.
Figure 3.15: Opened model shown in the graphic window
2. Add the missing component
Click the + Add button → Components.
In the Add Component(s) window, select
components/5MW_MC_middle_new.Click Add to insert the missing component into the model. The component is added at the origin position
(0, 0, 0)or at a default location defined by the system.
Figure 3.16: Adding the missing component into the model
Change the Selection Mode to Components, then select the newly added component in the Structure Tree to highlight it in the Graphic Window. This allows the component position and connectivity to be inspected.
Figure 3.17: Newly added component in Graphic Window
3. Connect the missing component to the model
At this stage, the newly added component is not yet connected to the rest of the structure. Zooming into the center column reveals two green dots, which represent open connection ports.
Figure 3.18: Unconnected ports
Open the Position and Assemble tool from the Right panel.
Click Auto-Connect Close Ports to automatically identify and connect matching ports between components.
Once connected, the green dots change to red dots, indicating that the ports are closed and the component is now structurally connected to the global assembly.
Figure 3.19: Using Auto-Connect Close Ports for connecting unconnected ports to the model
STEP 4: Apply loads
This section defines the hydrostatic pressure load case applied to the wetted surfaces of the assembled DeepCwind model. 
Figure 3.20: Model Set-up – Apply Loads
This load represents the static pressure distribution caused by the surrounding seawater and provides a baseline load case for further analysis.
1. Create Stored Selection
- Create stored selection for surface: Right-click on the Stored Selection in the Structure Tree → Add Boundary Sets Selection. You will see that a Boundary Sets selection named Boundary Sets Selection 1 is created under Stored Selection:
Figure 3.21: Adding new Boundary Sets Selection
- Akselos Modeler provides a tool called Selection Editor that helps users quickly select entities to add to the stored selection item. This tool is located in the Right panel.
Figure 3.22: Selection Editor tool
- Now we need to select all surfaces named Wetted_panels within the model. In the tool UI, select Boundary Sets Selection 1 → Type Wetted_panels in the Boundary Set name box. The below table will be filtered and show all components that contained boundary set named Wetted_panels.
Figure 3.23: Filtering Wetted_panels surface in all components
- Now click on the Select all items in the table button, all filtered Boundary Set will be added to the Boundary Sets Selection 1 store selection. Also, all selected Boundary sets will be shown in the Graphic Window.
Figure 3.24: Selecting all filtered surfaces
2. Create Hydrostatic load case
In this step, we will guide you on how to create a simple hydrostatic load case.
- Right-click on Load Cases in the structure tree → Add Load Case. The new load case named Load Case 1 will be created.
Figure 3.25: Adding new load case
- You can rename the load name by clicking on Load Case 1 then pressing F2 or right-clicking → Rename this Load Case → Input a new name - Hydrostatic load
Figure 3.26: Renaming the load case
- Add hydrostatic load: right-click on Hydrostatic load → Add load, and a new window named New Load Case/Load will appear.
Figure 3.27: Renaming the load case
- Input Floater Hydrostatic Pressure in the Filter box → Select Floater Hydrostatic Pressure in the Load Type panel → Click on the Add button. A new Floater Hydrostatic Pressure 1 load will be added under the Hydrostatic load.
- Click on Floater Hydrostatic Pressure 1 and consult the Property Tree to set the load's properties and parameters.
Setup parameters: The user needs to delete some well-defined parameters in the component, If you don’t delete those parameters, it will cause a conflict error since 2 parameters have been defined in 2 places. In this load case, fields hydrodynamic_properties and rotation_order should be deleted by selecting those fields → Right-clicking → Delete.
Figure 3.28: Deleting parameters in load properties to avoid the conflict error
Setup Stored selection: on the Stored Selection field, select Boundary Sets Selection 1.
Figure 3.29: Selecting the stored boundary set selection
Setup Other Properties, in the dynamic simulation, we all know that the position of the floater always changes in time series therefore affecting the hydrostatic pressure on the floater. In this case, we will assume that the floater is stable at the seawater level (heave = 0, roll = 0, pitch =0, yaw = 0). Other properties are (extracted from Akselos’s DCW model in OrcaFlex):
- center_of_rotation_x: 0 m
- center_of_rotation_y: 0 m
- center_of_rotation_z: 0 m
- Fluid_density: 1025 kg/m3
- Gravity_constant: 9.80665 m/s2
- Mean_water_level: 0 m
Figure 3.30: Defining load’s properties and parameters
4. Conclusion
The structural assembly of the DeepCwind 5MW foundation is now complete. The missing component has been successfully imported, configured with the appropriate cross sections and hydrostatic definitions, and rigidly connected to the global model. In addition, a baseline hydrostatic pressure load case has been defined on the wetted surfaces.
The model is now ready for the Solving and Studying phases of the engineering workflow, where structural response, stress distribution, and code checks can be evaluated under defined loading conditions.