DeepCWind 5MW Part 1 - Model Assemble

Modified on Thu, 16 May at 5:16 PM

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 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, which shows the properties of user selection.

1. Introduction

The Floater offshore wind turbine is the concept model of wind turbine(s) placed on a floating platform that is stabilized by moorings and anchors. There are numerous floating platforms for wind turbines:

A diagram of a wind turbine

Description automatically generated

Figure 1.1: General floater types

Akselos developed a full procedure to work on the assessment (fatigue and buckling check) of semi-submersible. Akselos’ workflow for FOWT is shown below:

A screenshot of a computer

Description automatically generated

Figure 1.2: Akselos’ FOWT workflow

In this tutorial, we will guide you through the following steps:

Import a FOWT component and settings.
Create and set up a 1D cross-section.
Assemble the newly imported component into the whole DCW model.
Set up floater hydrostatic pressure load.

The next articles will guide the next parts (Training – Solve – Validate) of the User Journey.

Figure 1.3: User Journey – DeepCWind 5MW tutorial 1 workflow

2. Problem Description

In this tutorial, we have a DeepCWind model missing 1 component. We need to import, configure, and assemble the missing component into the model.

Figure 2.1: DeepCWind 5MW model and the missing component

3. Before We Start

To follow the instructions below, please note the points below:

Akselos Modeler is the simulation software used in this tutorial.
A sample collection, DCW 5MW tutorial 1, has been prepared for your reference and is available on the Akselos Dashboard.

Follow the steps below to import the DeepCWind 5MW tutorial 1 collection into your computer via 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 the Authentication status to turn green, indicating successful authentication.

Figure 3.1: Checking authentication

4. Implementation

In the Implementation section, we will guide you through importing, configuring, and assembling the model in Akselos Modeler.

A screen shot of a computer

Description automatically generated

Figure 4.1: User Journey – DeepCWind 5MW tutorial 1 workflow

STEP 1: Import Collection

Figure 4.2: Prepared collection – Import Collection

On the File tab, click Import Collection… → On the Import Collection window, find and select DCW_5MW_tutorial_1 collection → Click on the Import button to pull the collection into your computer. A success message will confirm the collection has been imported into your computer.

Figure 4.3: Importing DCW_5MW_tutorial_1 collection

STEP 2: Import Mesh files

Figure 4.4: Create Model – Import Mesh files

Akselos Modeler provides an importer to convert inp mesh file format into Akselos’ components. The prepared inp file is located inside the collection, you can find it in inp_file/5MW_MC_Middle_new.inp

In the Model Ribbons, click on Collections → Create → Component Type.

Figure 4.5: Opening Component Type

A new window named Create New Component Types will appear → Click on the Add Meshes button → Select the inp file mentioned above on your local machine. A new mesh file will appear in the Mesh list.

Figure 4.6: Opening inp file

Figure 4.7: Mesh file is shown on Mesh list after opening

Next, we need to configure specific settings for the import. For this tutorial, adjust the following two fields:

Stiffener: 50-100. The prepared mesh file contains two 1D stiffener subdomains: a longitudinal stiffener (ID=50) and a ring frame stiffener (ID=51)

Port: 120-130. The prepared mesh file contained two port sidesets with ID = 120, 121

Click on the Settings tab → Input the corresponding numbers in the Stiffener and Port fields:

Figure 4.8: Editing ID settings

Import component: Return to the Create tab → Click the Create button, a successful message will appear on the log screen to let us know the component created → Click on the X button to close the window.

Figure 4.9: Adding mesh file and creating component

STEP 3: Component Editor

Figure 4.10: Create Model – Component Editor

In this section, we will guide you on how to:

Create and set up a Cross-section, then assign it to a 1D subdomain of the component.
Create a boundary set for the outer surface.
Create a hydrostatic pressure operator and assign the boundary set to this operator.

Create and set up Cross-section then assign to 1D subdomain:

The section for creating and setting up Cross-section is a general feature in Akselos Modeler. You can refer to Floating Offshore Wind Turbines: Set up cross-section for 1D stiffener tutorial to set up the newly imported component.

Create a boundary set for the outer shell surface:

To create a new surface set, right-click on Boundary Sets specification of components/5MW_MC_Middle_new → Create Boundary Set → Surface → A new surface set named New Surface will be created under Boundary Sets.

Figure 4.11: Creating surface boundary set

Select the entire outer shell element, click on New Surface → Click and hold for 2 seconds on a random element on the outer shell. You will set the option for all outer elements to be selected (highlighted in yellow).

Figure 4.12: Assigning surface

You can rename the surface by right-clicking on New Surface → Rename this Named Geom Type → Input Wetted_panels. This step is necessary because we can quickly select these surfaces by filtering their name in the further step below.

Figure 4.13: Renaming surface boundary set

Create Hydrostatic pressure operator:

Right-click on Source Operators → Create Source Operator Type(s), then a Create Operator Type window will appear. In the Filter, enter hydrostatic, then select Floater Hydrostatic Load Pressure → Click on the Add button to insert this operator.

Figure 4.14: Adding Floater Hydrostatic Load Pressure operator

Under Source Operators, a new operator named New Floater Hydrostatic Load Pressure will be created. Click on it to see the Targets in the Property Tree screen → Tick the Wetted_panels check box to assign the surface boundary set to this operator.

Figure 4.15: Assigning Wetted_panels surface to the operator

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 4.16. Saving component changes

STEP 4: Assemble Model

Figure 4.17: Create Model – Assemble Model

In this section, we will show you how to assemble newly created components to a prepared model by using the Position and Assemble tool.

In this section, you can use the setup component in the section above or you can use component 5MW_MC_Middle_with_hydrostatic_operator and proceed with all steps below.

Open a model:

Click on the File tab → Open File from Collection → A window will appear to open the aks model, select 5MW_DeepCWind_missing_MC_middle.aks → Open.

Figure 4.18: Opening aks model

Then, you can see the model opened in the Graphic Window and the model properties loaded into the Structure tree.

Figure 4.19: Opened model is shown in the graphic window

Add the missing component:

Click the + Add button → Components, then the Add Component(s) window will appear. In this window, select components/5MW_MC_middle_new → Click the Add button to insert this missing component into the model. The newly inserted component will appear in the random position on the Graphic Window.

Figure 4.20: Adding the missing component into the model

You can see the new component added to the Graphic window and Structure tree. You can change the Selection Mode to Components then select the newly added component in the Structure Tree to highlight the component.

Figure 4.21: Newly added component in Graphic Window

Select component → Right-click on the Graphic Window → Reset to original position, the component will be reset into its original position.

Figure 4.22: Resetting component to the original position

Connect the mis component to the model:

Now, the component is added and reset to the origin position in the model, when you zoom to the center column on the model, you will see that there are 2 green dots which represent 2 ports opening which means the added component has not been connected to the model.

Figure 4.23. Unconnected ports

We will show you how to connect the component to the model by the Position and Assemble tool. This tool is located on the Right panel. On this tool UI, click on the Auto-Connect Close Ports button. You will see two green dots above now change to two red dots. This means the missing component is connected to the model.

Figure 4.24: Using Auto-Connect Close Ports for connecting unconnected ports to the model

STEP 5: Apply Loads

Figure 4.25: Model Set-up – Apply Loads

In this section, we will show you how to:

Create store selection for Wetted_panel sidesets.
Create a simple hydrostatic pressure load case.

You can continue with the model in the section above or you can use the prepared model 5MW_DeepCWind_Assembly and proceed with all the steps below.

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 4.26: 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 4.27: 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 4.28: 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 4.29: Selecting all filtered surfaces

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 4.30: 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 4.31: 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 4.32: 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.

Figure 4.33: Adding Floater Hydrostatic Pressure load to the current model

Click on Floater Hydrostatic Pressure 1 and consult the Property Tree to set the load's properties and parameters.
1. 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 4.34: Deleting parameters in load properties to avoid the conflict error

Setup Stored selection: on the Stored Selection field, select Boundary Sets Selection 1.

Figure 4.35: 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 4.36: Defining load’s properties and parameters

Congratulations! You've successfully built your model and applied a load case. This is a necessary first step to get familiar with Akselos Modeler! In the next installments of this tutorial series, we'll delve into Training, Solving, Studying steps in User Journey.

Stay tuned for these next tutorials.