(Part A) Set up, process, and save an initial fluid field of a Multiphase case in Ansys Fluent that can later be used for 2-Way Fluent coupling with Rocky DEM.
(Part B) Use the .cas and .dat files you created in Part A to set up the Rocky portion of the 2-Way Multiphase simulation, and then run it coupled with Ansys Fluent.
The main purpose of this Tutorial is to set up and process a Multiphase CFD case with Ansys Fluent to be later used in a 2-Way coupling simulation with Rocky.
Important: Even if you are already familiar with CFD, please follow Part A in order to understand the main limitations and needs for coupling a Multiphase case with Rocky.
Part B of this tutorial will cover setting up the Rocky project.
The scenario considered is that of a Mixing Tank into which solid material (particles) fall through air into water that is being mixed by a rotating impeller.
You will learn how to: Set up, process, and save an initial fluid field of a Multiphase case in Ansys Fluent that can later be used for 2-Way Fluent coupling with Rocky.
To complete this tutorial, you are required to have a valid license for Ansys Fluent 2025 R2.
Important: This ADVANCED tutorial assumes that you are already familiar with the Ansys Fluent UI and project workflow.
If that is not the case, please refer to the Ansys Fluent user documentation for basic introduction about Fluent usage before beginning this tutorial.
The geometry in this tutorial is composed of:
(1) Tank walls
(2) Mixing shaft
(3) Mixing impeller
Note: These geometries will come from the Fluent .cas file that you will import as part of this tutorial.
To set up the Fluent Case, do the following:
Open Ansys Fluent.
From the Fluent Launcher, under Dimension, ensure that 3D is selected; also, under Options, ensure that Double Precision is selected (as shown).
Important: Double Precision and 3D are required for coupling with Rocky.
Click Start.
For this tutorial, the tank and the impeller were meshed separately.
This is so the Body of Influence (BOI) region where the air and water meet can have a higher resolution.
Both regions will be solved together by a sliding interface approach in Fluent.
The mesh interface will be defined later on this tutorial. Follow the steps below to open the mesh file and start the setup.
Download the
dem_tut16_files.zipfile here .Unzip
dem_tut16_files.zipto your working directory.From the File menu, point to Read, and then click Case
From the Select File dialog, select Mixing_Tank.msh.h5 from the dem_tut16_files/mesh folder, and then click OK.
Now that the Fluent .cas file is imported, we can start setting up the Fluent case.
Use the information in the table that follows to visualize and set up the mesh.
Tip: If you run into settings or procedures in these tables that you are not yet familiar with, please refer to your Ansys Documentation to find detailed instructions.
Step Location Parameter or Action Settings A Setup | General Display Mesh (impeller, opening, shaft, walls | Display) Check Mesh Time Transient Gravity (Enabled) Gravitational Acceleration -9.81 [m/s2] in the Y direction
For this tutorial, we want two fluid phases representing water and air, respectively, so we will use the Multiphase approach.
Important: Even though we will be simulating only two fluid phases in this tutorial, the number of Eulerian phases will be set to three (number of phases + 1) to account for a required particle phase.
Use the information in the tables that follow to set up the fluid materials.
Note: We will leave the air fluid as it is set by default.
Step Location Parameter or Action Settings A Step | Materials | Fluid Create New Fluid Name particles Chemical Formula particles Constant Density 998.2 [kg/m3] Constant Viscosity 0.001003 [kg/(m s)] Note: This new particles fluid material will be used as the required dispersed phase.
For this material, the properties set in Fluent will be later overridden by Rocky.
To create each new fluid material, from the Create/Edit Materials dialog, click Change/Create and select No if asked to overwrite other material.
Step Location Parameter or Action Settings B Step | Materials | Fluid Create New Fluid Name water-liquid Chemical Formula h20<l> Constant Density 998.2 [kg/m3] Constant Viscosity 0.001003 [kg/(m s)] Next, use the information in the tables that follow to set up the Eulerian Muliphase model, define the three phase materials, and set the interactions between the phases.
Step Location Parameter or Action Settings A Step | Materials | Multiphase Models | Inhomogeneous Models Eulerian … | Number of Eulerian Phases 3 … | Eulerian Parameters (All Cleared) … | Formulation Implicit Important: These first four settings are required for any Rocky coupled Multiphase case.
Step Location Parameter or Action Settings B … | Phases | phase-1 - Primary Phase Name water Phase Material water-liquid ⯆ C … | Phases | phase-2 - Secondary Phase Name air Phase Material air ⯆ Constant Diameter 0.005 [m] D … | Phases | phase-3 - Secondary Phase Name particles Phase Material particles ⯆ Click Apply to update phase names for the next step.
Step Location Parameter or Action Settings E … | Phase Interaction | Forces | water : air Surface Tension Force Modeling (Enabled) Surface Tension Coefficient constant ⯆ 0.072 [N/m] F … | Phase Interaction | Interfacial Area Interfacial Area [m-1] (all the three) ia-particle ⯆ Note: Fluid-particle interphase transfers are calculated on the Rocky side and not in Fluent, so we do not need to worry about setting values for this third phase (particles).
Fluid-particle momentum exchange terms are calculated on the Rocky side and not in Fluent, so we need only to define the interactions between the fluid phases.
The only interaction you must define between fluids is Drag. For this tutorial, the Drag Coefficient was left as default (Schiller-Naumann) and the Interfacial Area parameters were defined in Step F.
Since this tutorial includes a free surface problem, we have also chosen to consider surface tension.
Use the information in the table that follows to set up the turbulence model.
Step Location Parameter or Action Settings A Setup | Models | Viscous Model k-epsilon (2-eqn) Near-Wall Treatment Scalable Wall Functions Options | Production Limiter (Enabled) Turbulence Multiphase Model Per Phase Note: The choice of turbulence model depends upon the application.
Since for this problem fluid phases are completely segregated, the Turbulent Multiphase Model should be set to Per Phase.
To account for the impeller rotation, we need to define a mesh motion.
Use the information in the table that follows to set up the cell zone conditions.
Step Location Parameter or Action Settings A Setup | Cell Zone Conditions | Operating Conditions... Operating Density Method user-input⯆ | 0 [kg/m³] B Setup | Cell Zone Conditions | Fluid | movingregion Mesh Motion (Enabled) Speed 12 [rad/s] Rotation-Axis Direction 0, -1, 0 [ - ] Note: If moving meshes are prescribed for any Zone in Fluent, the Zone Name defined here (movingregion) will become a new Motion Frame in Rocky once the Fluent .cas file is imported. (We will cover this later in Part B of this tutorial.)
Use the information in the table that follows to set up the boundary conditions on the shaft component.
Step Location Parameter or Action Settings A Setup | Boundary Conditions | shaft Wall Motion Moving Wall Motion Absolute Rotational Speed 12 [rad/s] Rotation-Axis Direction 0, -1, 0 [ - ] Note: This should match the rotation we defined for the movingregion zone earlier.
Now, a pressure outlet condition must be set to the top opening.
With Boundary Conditions selected, from the Task Page, double-click the opening component and do the following:
Keep the default settings for water and particles Phases. (No backflow volume fraction).
For air Phase, on the Multiphase tab, change the Backflow Volume Fraction to 1.
For air Phase, on the Momentum tab, set Backflow Turbulent Intensity to 1 [%].
Note: Every remaining surface is modeled as a non-slipping boundary.
Use the information in the table below to define a mesh interface for the different mesh regions.
Step Location Parameter or Action Settings A Setup | Mesh Interface Create new mesh interface Zones | interface_mr and interface_tank (selected) Create
Use the information in the table that follows to define the solution methods.
Step Location Parameter or Action Settings A Solution | Methods Pressure-Velocity Coupling Scheme Phase Coupled SIMPLE Transient Formulation First Order Implicit High Order Term Relaxation (Enabled) View Relaxation Options B Relaxation Options (dialog box) Relaxation Factor 0.6 [ - ] Note: For all Multiphase coupling simulations, the Pressure-Velocity Coupling Scheme must be set to Phase Coupled SIMPLE.
In addition, for all 2-Way coupling simulations, First Order Implicit must be set for Transient Formulation.
Relaxation is used only to help make this example simulation run easier for tutorial purposes.
For the purposes of this tutorial only, we'll modify the controls to increase stability.
Use the information in the table that follows to define the Under-Relaxation Factors.
Step Location Parameter or Action Settings A Solution | Controls Pressure 0.2 [ - ] Momentum 0.5 [ - ] Volume Fraction 0.7 [ - ] Turbulent Kinetic Energy 0.7 [ - ] Turbulent Dissipation Rate 0.7 [ - ] Turbulent Viscosity 0.7 [ - ]
It is important to provide Rocky with the correct initial volume fraction fields.
For this tutorial:
air phase is initialized with a volume fraction of 1.0 in the entire domain and then it is patched to a volume fraction of zero in the water region.
Also, air turbulence quantities are patched to zero inside water region and vice-versa. This is done by two cell register regions.
Important: For particles phase, volume fraction MUST be initialized as zero everywhere.
Before initializing, use the information in the table that follows to define the two new cell registers.
Step Location Parameter or Action Settings A Solution | Cell Registers Create New Region B Region Register (dialog box) Name air Input Coordinates | Min -1, 0.1, -1 [m] Input Coordinates | Max 1, 1, 1 [m] C Solution | Cell Registers Create New Region D Region Register (dialog box) Name water Input Coordinates | Min -1, -1, -1 [m] Input Coordinates | Max 1, 0.1, 1 [m]
Then, use the information in the table that follows to initialize, and then patch the phases.
Step Location Parameter or Action Settings A Solution | Initialization Reference Frame Relative to Cell Zone air Volume Fraction 1 [ - ] Initialize Patch B Patch (dialog box) Phase air ⯆ Variable Volume Fraction Value 0 [ - ] Registers to Patch water Patch C Patch (dialog box) Phase air ⯆ Variable Turbulent Kinetic Energy Value 0 [m2/s2] Registers to Patch water Patch D Patch (dialog box) Phase water ⯆ Variable Turbulent Kinetic Energy Value 0 [m2s2] Registers to Patch air (only) Patch
Finally, use the information in the table that follows to set up the calculation.
Step Location Parameter or Action Settings A Run Calculation Time Advancement Type Fixed Number of Time Steps 50 [ - ] Time Step Size 0.005 [s] Max Iterations/Time Step 50 [ - ] Important: Fixed should always be selected for the Time Stepping Method.
Ensure the Time Step Size value you set matches the minimum initial Output Frequency value you want for your Rocky and Fluent files.
Tip: You can change the outputs to be less frequent than this minimum in your Rocky setup later.
At this point in your Fluent setup, your program screen should look similar to the image shown.
From the Run Calculation Task Page, click Calculate.
Let the simulation run for a few time steps until you can confirm that it is converging (as shown).
Stop processing the case.
It is important to have stabilized CFD results to use as initial conditions in Rocky.
These CFD results will be imported as an Initialization file when we define the CFD Coupling in Rocky in Part B.
Write the Case & Data to a file named Mixing_Tank_B.cas.h5
Close Fluent.
This concludes Part A of this tutorial, in which Ansys Fluent was used to set up a Multiphase CFD simulation that will later be used for 2-Way coupling with Rocky.
During this tutorial, it was possible to:
Use Ansys Fluent to set up and process an initial fluid field of a CFD case involving two fluids (water and air) and a particulate phase (particles).
Understand what Fluent settings are required when coupling Multiphase cases with Rocky.
What's Next?
You are ready to move on to Part B and create the Rocky project and 2-way couple it with this CFD case.
The main purpose of this Tutorial is to use the .cas and .dat files we created in Part A to set up the Rocky portion of the 2-Way Multiphase simulation, and then run it coupled with Ansys Fluent.
As a reminder, the scenario considered is that of a Mixing Tank into which solid material (particles) fall through air into water that is being mixed by a rotating impeller.
You will learn how to:
Import geometry components from a Fluent .cas file
Import geometry motions from a Fluent .cas file
Enable the collection of CFD Coupling Particle Statistics data
Set up and run a Multiphase 2-Way Fluent coupled simulation in Rocky
And you will use these features:
CFD Coupling Particle Statistics Module
Custom Geometry Import
Motion Frames
2-Way Fluent CFD Coupling
To complete this tutorial, you are required to have both of the following on the same machine upon which you will be running the coupled simulation:
(1) A valid license for Ansys Fluent 2025 R2.
(2) A license of Rocky 2025 R2.
Important: This ADVANCED tutorial assumes that you are already familiar the the following programs and resources:
The Rocky 2025 R2 program.
If this is not the case, it is recommended that you complete at least Tutorials 01- 05 before beginning this tutorial.
The Ansys Fluent program.
If this is not the case, please refer to the Ansys Fluent user documentation for a basic introduction about Fluent usage before beginning this tutorial.
The geometry in this tutorial is composed of:
(1) Tank walls
(2) Mixing shaft
(3) Mixing impeller
Note: These geometries will come from the Fluent .cas file that you exported out of Fluent in Part A.
Do one of the following:
If you completed Part A of this tutorial, ensure you have available the Mixing_Tank_B.cas.h5 and Mixing_Tank_B.dat.h5 files you exported. (Part B will make use of those files.)
If you did not complete the project from Part A, ensure you have downloaded and extracted the dem_tut16_files zip folder that was provided along with this PDF.
Open Rocky 2025 R2.
Create a new project.
Save the empty project to a location of your choosing.
For this tutorial, we want to do all of the following:
Enable Coarse Grain Modeling (CGM) to help with simulating micron-sized particles.
Tip: For a walk-through example using CGM, refer to Tutorial 17 - Mixing Tee.
Use the CFD Coupling Particle Statistics module to collect particle-fluid interaction statistics for later post-processing.
Tip: For a walk-through example using this module, refer to Tutorial 13 - Windshifter.
Import the same geometries motion definitions that we used in the Multiphase Fluent case.
Use the information in the table that follows to start setting up your Rocky project.
Tip: If you run into settings or procedures in these tables that you are not yet familiar with, please refer to the Rocky User Manual and/or other Tutorials (via the Tutorial Index) to find the detailed instructions you need.
Step Data Entity Editors Location Parameter or Action Settings A Study Study Study Name Mixing Tank B Physics Physics | Coarse-Graining Enable Coarse-Graining (Enabled) C Modules Modules CFD Coupling Particle Statistics (Enabled) D Modules ﹂CFD Coupling Particle Statistics
CFD Coupling Particle Statistics Drag Force (Enabled) Pressure Gradient Force (Enabled) E Geometries Import Wall Mixing_Tank_B.cas.h5 with "m" for Import Unit
After importing the .cas file, there are three geometry components we do not need for the Rocky simulation that we can remove.
We will also create an Inlet from which to inject particles.
Use the information in the table that follows to continue setting up your Rocky project.
Step Data Entity Editors Location Parameter or Action Settings A Geometries ﹂interface_mr
Remove Geometry B Geometries ﹂interface_tank
Remove Geometry C Geometries ﹂opening
Remove Geometry D Geometries Create Circular Surface E Geometries ﹂Circular Surface <01>
Circular Surface Center Coordinates 0, 0.125, 0 [m] Max Radius 0.07 [m] Min Radius 0.008 [m]
In order for our coupled simulation to work properly, the impeller and shaft geometries in the DEM portion need to rotate with the same velocity and position as in the CFD solver.
To ensure that the motions are identical and remain in sync, Rocky will automatically create a new Motion Frame based on the motion information Fluent saved in the .cas file.
This Motion Frame will appear once we set up the CFD Coupling portion of the project, which isn't until later in this tutorial.
For now, we will skip the Motion Frames step and will come back to it later.
For this tutorial, we will have two Particle groups and we want each group to have different Materials.
Therefore, we will modify the Default Particles Material, and then create a duplicate of it for the second Particle group.
Use the information in the table that follows to continue setting up your Rocky project.
Step Data Entity Editors Location Parameter or Action Settings A Materials ﹂Default Particles
Material Use Bulk Density (Cleared) Density 1100 [kg/m3] Young's Modulus 1e+06 [N/m2] Duplicate B Materials ﹂Default Particles <01>
Material Density 1300 [kg/m3]
Note: We will leave all the Material Interactions as they are set by default.
Next, let's create the two Spherical-shaped particle groups making use of the same CGM Scale Factor, but with different Materials.
We can also define the Input from which to release these two Particle groups, and reduce the injection time to only the very beginning of the simulation.
Use the information in the table that follows to continue setting up your Rocky project.
Step Data Entity Editors Location Parameter or Action Settings A Particles Create Particle B Particles ﹂Particle <01>
Particle | Size CGM Scale Factor 3 [ - ] Size 0.0005 [m] @ 100 % C Particles Create Particle D Particles ﹂Particle <02>
Particle Material Default Particles <01> ⯆ Particle | Size CGM Scale Factor 3 [ - ] Size 0.0005 [m] @ 100% E Inlets and Outlets Create Particle Inlet F Inputs ﹂Particle Inlet <01>
Particle Inlet Entry Point Circular Surface <01> ⯆ Particle Inlet | Particles Add row (x2) (1) Particle | Mass Flow Rate Particle <01> ⯆ @ 0.15 [t/h] (2) Particle | Mass Flow Rate Particle <02> ⯆ @ 0.15 [t/h]
For the CFD Coupling step, we will select the Fluent option under 2-Way.
This option in Rocky takes into account fluid forces acting on particles and transfers particle information back to Fluent.
Choosing this option will enable us to select the same .cas file that we created in Part A of this tutorial.
Important: A validation step immediately following this selection requires that a valid and active version Ansys Fluent be available on the same machine that we are doing the Rocky setup.
For this tutorial, we want Rocky to consider drag and turbulent dispersion interactions.
We will also make use of the .dat file we exported in Part A to start the simulation with an initial fluid field.
Use the information in the table that follows to set your 2-Way Fluent coupling options.
Note: Fot this step, you must use the same .cas file that you used to import geometries when setting up the project.
Step Data Entity Editors Location Parameter or Action Settings A CFD Coupling Coupling Mode 2-Way | Fluent ⯆ Slect Fluent CAS file Mixing_Tank_B.cas.h5 B CFD Coupling ﹂2-Way Fluent
2-Way Fluent | Interactions Turbulent Dispersion (Enabled) 2-Way Fluent | Coupling Solids Maximum Volume Fraction Target 0.7 2-Way Fluent | Fluent Rocky Phase particles ⯆ Use Data Initialization (Enabled) Import File (button) Load File Mixing_Tank_B.dat.h5 Execution mode Local Parallel ⯆ Solver Processes 6 [ - ] Keep all files (Cleared) Files to keep 2 [ - ] Additional Args -g Note: For Solver Processes, enter a value based upon how many processors you have available.
The Additional Argument is optional but enables the Fluent portion of the coupled simulation to run in batch mode (i.e., without the GUI), which can result in faster processing.
Click Open.
Now that the .cas file is imported, we can see a new entry in the Data panel under Motion Frames called "movingregion" Motion Frame.
This item is automatically named for the Zone Name we set for the mesh motion in Fluent (Part A).
When this item is viewed in the Data Editors panel, a Rotation motion is already defined (as shown).
Note that the options are all disabled. This is to ensure that the motion in Rocky matches exactly the motion in Fluent.
Even though the Motion Frame is automatically created, we must still manually assign it to the geometries we want to move.
For this tutorial, we want only the impeller and shaft to rotate, so we will assign the new motion only to these two components.
Use the information in the table that follows to assign your geometry motions.
Step Data Entity Editors Location Parameter or Action Settings A Geometries ﹂impeller
Wall Motion Frame "movingregion" Motion Frame ⯆ B Geometries ﹂shaft
Wall Motion Frame "movingregion" Motion Frame ⯆ Tip: Once assigned, you can preview these motions in a Motion Preview window.
Lastly, we need to define the Solver setup.
For this tutorial, it is important to note the Fluent Outputs Multiplier, which enables you to change the frequency of outputs.
Tip: A higher multiplier will result in fewer Rocky and Fluent files.
Use the information in the table that follows to finish your Rocky setup.
Step Data Entity Editors Location Parameter or Action Settings A Solver Solver | Time Simulation Duration 3 [s] Output Settings | Fluent Outputs Multiplier 2 [s] Solver | General Simulation Target CPU ⯆ Solver | Advanced Use 2023R2 Cell Volume Fraction Update Approach (does not displace fluid) (Enabled) Tip: When you are making CPU selections, remember that some CPUs have been allocated to the CFD solver. Select only the ones you want Rocky to use here.
With a 3D View window opened, your Data panel and Workspace should look similar to the below image.
Close Fluent if it is opened, and from the Solver entity, click Start.
The Simulation Summary screen appears (as shown), then processing begins.
A new dialog also appears due to the 2-Way Fluent coupling calculations (as shown).
Tip: After getting all information from Fluent, the black dialog closes. In Rocky you can use the Auto Refresh checkbox to view the results in a 3D View window during processing.
Once your simulation has finished processing, you can choose to post-process the results in several ways, as explained below.
In Rocky, you can post-process the CFD and DEM results of the simulation by following the same steps as listed in the following Tutorials:
Tutorial 13 - Windshifter | Part C: One-Way Coupling (Workbench)
Tutorial 14 - Fluidized Bed | Part C: Post-Processing Rocky
In Fluent, you can post-process the CFD results of the simulation using the tools included in that program, or you can use other programs such as Ansys CFD-Post or Ansys EnSight.
Tip: Refer to your Ansys Documentation to learn more about how to use these tools.
This concludes Part B of this tutorial.
The .cas and .dat files we created in Part A were used to set up the Rocky portion of the 2-Way Multiphase simulation, and then run it coupled with Ansys Fluent.
During this tutorial, it was possible to:
Import geometry components from a Fluent .cas file into Rocky
Import Mesh Motions from a CFD .cas file into Rocky and assign them to geometries
Use Rocky to set up and run a 2-Way coupled Multiphase simulation with Fluent
What's Next? If you completed this tutorial successfully, then you are ready to move on to next tutorial.