Note: A complete work procedure, with example datasets and conditions is available under Fluent Icing in the Fluent Tutorial Guide.
To Set-up a Case for Icing Simulations
Launch Fluent on your computer. In the Fluent Launcher window, set the Capability Level to and then select the Icing workspace. Set an appropriate number of Solver Processes and click to launch Fluent Icing.
In the Project ribbon, select Project → , choose an appropriate name and location for the Project file, and click .
Go to Simulation → and select a suitable case (.cas, .cas.h5) file.
Note: The case must contain a 3D mesh without polyhedral or adapted elements. The reference conditions and material type (Air) should be suitable for icing conditions. Use the tutorial of Fluent Icing to get familiar with the typical airflow, particle and icing settings.
A new simulation is created. When prompted, choose an appropriate name for the new simulation, and select . A simulation folder with the chosen name is then created inside the project, and a remote solver session is loaded with the number of CPUs set earlier and listed in Preferences.
Once Fluent is started, the mesh is displayed and the Outline View panel presents the available settings for your simulation. Use Fluent Icing to review the conditions and solver settings:
Outline View → Setup
Enable the type of simulation to conduct such as Airflow, Particles and Ice. All modules must be enabled for a complete icing simulation.
Setup → Airflow
Review the airflow conditions and configure them if necessary.
Setup → Particles → Droplets
Set the conditions and default settings, which will be used for the particles simulation.
Setup → Ice
Set the conditions and default settings, which will be used for the ice simulation.
Setup → Boundary Conditions → Walls→ wall
Set temperature to adiabatic + 10 by using the button at the bottom of the panel for each wall subject to icing. Activate High roughness for Icing in Wall Roughness within its properties window.
In Outline View → Solution:
In the Solution → Airflow mode, the number of iterations for the Airflow solver can be configured.
Use the button at the bottom of the Airflow panel.
A window will appear. Provide an appropriate name for the new Airflow run. A run folder of this name will appear in the inside the current simulation folder.
The Airflow solver runs and produces an airflow solution.
The number of iterations for the Particles solver can be configured in the Solution → Particles.
Use the button at the bottom of the Particles panel.
A window will appear. Provide an appropriate name for the new Particles run. A run folder of this name will appear in the inside the current simulation folder.
The Particles solver runs and produces a droplet solution.
Use the ribbon and click Results → Quick-View → Contour → Collection efficiency (walls) option to view the water catch on the walls, the solution is displayed in the Graphics window.
In the Solution → Ice node, the total time of ice accretion can be configured.
Use the button at the bottom of the Ice panel.
A window will appear. Provide an appropriate name for the new Ice run. A run folder of this name will appear in the inside the current simulation folder.
The Ice solver runs and produces an ice solution, which is composed of scalar values on walls and the ice shape.
Use the ribbon and click Results → Quick-View → Ice Cover options to view the scalars of the ice solution as well as the ice shape using CFD-Post.