ACU-T: 6500 Flow Through Porous Medium


This tutorial provides the instructions for setting up, solving and viewing results for simulation of flow through a porous medium. Prior to starting this tutorial, you should have already run through the introductory HyperWorks tutorial, ACU-T: 1000 HyperWorks UI Introduction, and have a basic understanding of AcuSolve, HyperView, and HyperMesh. To run this simulation, you will need access to a licensed version of HyperMesh and AcuSolve.

Prior to running through this tutorial, copy from <Altair_installation_directory>\hwcfdsolvers\acusolve\win64\model_files\tutorials\AcuSolve to a local directory. Extract from

Since the HyperMesh database (.hm file) contains meshed geometry, this tutorial does not include steps related to geometry import and mesh generation.

Problem Description

The problem to be addressed in this tutorial is shown schematically in the figure below. It consists of a cylindrical channel with a porous medium in the flow section. As the flow passes through this section, a pressure drop is observed. In this simulation, an inlet velocity will be assigned to the flow and pressure drop across the porous medium will be calculated. The length of the porous section is 0.06 m and the fluid is an imaginary air-like fluid with a density of 1 kg/m3 and a molecular viscosity of 0.001 kg/m-s. The inlet velocity of the flow is 0.2 m/s.

Figure 1.

Open the HyperMesh Model Database

  1. Start HyperMesh and load the AcuSolve user profile.
    Refer to the HM introductory tutorial, ACU-T: 1000 HyperWorks UI Introduction, to learn how to select AcuSolve from User Profiles.
  2. Click the Open Model icon located on the standard toolbar.
    The Open Model dialog opens.
  3. Browse to the directory where you saved the model file. Select the HyperMesh file and click Open.
  4. Click File > Save As.
    The Save Model As dialog opens.
  5. Create a new directory named PorousMedia and navigate into this directory.
    This will be the working directory and all the files related to the simulation will be stored in this location.
  6. Enter PorousMedia as the file name for the database, or choose any name of your preference.
  7. Click Save to create the database.

Set the General Simulation Parameters

In this step, you will set the simulation parameters that apply globally to the simulation.

  1. Go to the Solver Browser, expand 01.Global, then click PROBLEM_DESCRIPTION.
  2. In the Entity Editor, verify that the Analysis type is set to Steady State and the Turbulence model is set to Laminar.

    Figure 2.

Set Up Boundary Conditions and Material Model Parameters

In this step, you will start by modifying the material properties of Air and then create a material model for the porous medium. Then, you will assign the surface boundary conditions and material properties for all the fluid volumes.

Create the Material Model

  1. In the Solver Browser, expand 02.Materials > FLUID then click on Air_HM.
  2. In the Entity Editor, change the Density to 1 kg/m3 and the Viscosity to 0.001 kg/m-sec.

    Figure 3.
  3. Right-click on Air_HM in the Solver Browser and select Duplicate.
  4. Name the new material Porous.
  5. In the Entity Editor, scroll down to the Porosity tab and set the Porosity type to Constant.
  6. Enter the values 1, 0.001, and 0.001 for the Direction 1 permeability, Direction 2 permeability and Direction 3 permeability, respectively.
  7. Set the value of Darcy coefficient to 4166.67.
  8. Set the Forchheimer coefficient to 8.33.

    Figure 4.
  9. Save the model.

Assign Boundary Conditions and Material Properties

By default, all components are assigned to the wall boundary condition. In this step, you will change them to the appropriate boundary conditions and assign material properties to the fluid volumes.
  1. In the Solver Browser, expand 12.Surfaces > WALL.
  2. Click Inlet. In the Entity Editor,
    1. Change the Type to INFLOW.
    2. Set the Inflow velocity type to Cartesian.
    3. Set the X velocity to 0.2 m/sec

    Figure 5.
  3. Click Outlet. In the Entity Editor, change the Type to OUTFLOW.

    Figure 6.
  4. Click Walls. In the Entity Editor, verify that the Type is set to WALL.

    Figure 7.

    All the internal surfaces, such as the inlet and outlet of the porous section and the external walls of pipe surface, can be grouped into one single surface set. Auto_Wall, which is an advanced feature in AcuSolve, re-groups these elements into internal and external surfaces for each volume and writes the surface output accordingly. This process is done internally, thereby reducing the number of steps in the workflow.

  5. Click Fluid_Upstream. In the Entity Editor,
    1. Change the Type to FLUID.
    2. Select Air_HM as the Material.

    Figure 8.
  6. Click Fluid_Porous. In the Entity Editor,
    1. Change the Type to FLUID.
    2. Select Porous as the Material.

    Figure 9.
  7. Click Fluid_Downstream. In the Entity Editor,
    1. Change the Type to FLUID.
    2. Select Air_Hm as the Material.

    Figure 10.
  8. Save the model.

Compute the Solution

In this step, you will launch AcuSolve directly from HyperMesh and compute the solution.

  1. Turn on the visibility of all mesh components.
    For the analysis to run, the mesh for all active components must be visible.
  2. Click on the ACU toolbar.
    The Solver job Launcher dialog opens.
  3. Optional: For a faster solution time, set the number of processors to a higher number (4 or 8) based on availability.
  4. The Output time steps can be set to All or Final. Since this is a steady state analysis, the Final time step output is sufficient.
  5. Leave the remaining options as default and click Launch to start the solution process.

    Figure 11.

Post-Process the Results

As the solution progresses, AcuProbe is launched automatically. AcuProbe can be used to monitor different variables over solution time. In this step, you will plot the residual ratio values and then compute the pressure drop across the porous section.

  1. In the AcuProbe window, from the Data Tree on the left, expand Residual Ratio.
  2. Right-click on Final and select Plot All.

    Figure 12.
  3. Once the solution is converged, right-click again on Final and select Plot None.
  4. Click the User Function icon from the toolbar.
    The User Function dialog opens.
  5. In the dialog, enter dP as the function name.
  6. In the Function field, type P_In =.
  7. In the Data Tree, expand Surface Output > AUTO Fluid_Porous internal > Pressure.
  8. Right-click on pressure and select Copy name. Paste the value in the Function window after P_In =.

    Figure 13.
  9. On the next line, type P_Out = and repeat the above step for pressure on the AUTO Fluid_Downstream internal surface.
  10. On the next line, type value = P_In - P_Out.
    Note: The word “value” is case sensitive and should always be in lower case. If you use a capital letter, an error window appears.

    Figure 14.
  11. Click Apply to display the plot.
    Note: You might need to click on the toolbar in order to properly display the plot.

    Figure 15.


In this tutorial, you learned how to set up and solve a problem with porous medium. You started by importing the HyperMesh database and then creating a material model for the porous section. Then, you assigned the boundary conditions and material properties and solved by launching AcuSolve directly from HyperMesh. Finally, you created a pressure drop plot using the user function tool in AcuProbe and calculated the drop in pressure between the inlet and outlet surfaces of the porous section.