ACU-T: 3600 Melting of Diesel Exhaust Additive within an Enclosed Tank

This tutorial provides the directions for setting up, solving, and post-processing results for a simulation that models the approximated melting of the common diesel fuel exhaust additive that is contained within a notional tank. 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 HyperWorks CFD and AcuSolve. To run this simulation, you will need access to a licensed version of HyperWorks CFD and AcuSolve.

Before you begin, copy the file(s) used in this tutorial to your working directory.

Problem Description

In this tutorial, a diesel exhaust additive, commonly known as Urea, is initially subjected to freezing conditions dictating that the fluid is frozen, T(Initial)=263.15 K. The fluid is then heated above its defined melting point by imposing a fixed thermal condition on the heating element. As the temperature within the enclosure exceeds the melting temperature of the material, the porosity effectiveness of the fluid decreases to 0.0, allowing the fluid to move under natural convection currents. Eventually the entire fluid volume becomes melted, reaching the temperature of the heating element. The time to melt is computed for the specified heating element temperature of 313.15 K. Note that the interface between the solid/fluid material is captured because of the material definition as defined with a linear temperature gradient spanning 2 degrees at the melting front.


Figure 1.

Start HyperWorks CFD and Open the HyperMesh Database

  1. Start HyperWorks CFD from the Windows Start menu by clicking Start > Altair <version> > HyperWorks CFD.
  2. From the Home tools, Files tool group, click the Open Model tool.


    Figure 2.
    The Open File dialog opens.
  3. Browse to the directory where you saved the model file. Select the HyperMesh file ACU-T3600_UreaTankMelting_TemperatureBasedEffectiveness.hm and click Open.
  4. Click File > Save As.
  5. Create a new directory named MeltingTank 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 MeltingTank as the file name for the database, or choose any name of your preference.
  7. Click Save to create the database.

Validate the Geometry

The Validate tool scans through the entire model, performs checks on the surfaces and solids, and flags any defects in the geometry, such as free edges, closed shells, intersections, duplicates, and slivers.

To focus on the physics part of the simulation, this tutorial input file contains geometry which has already been validated. Observe that a blue check mark appears on the top-left corner of the Validate icon on the Geometry ribbon. This indicates that the geometry is valid, and you can go to the flow set up.


Figure 3.

Set Up Flow

Set Up the Simulation Parameters and Solver Settings

  1. From the Flow ribbon, click the Physics tool.


    Figure 4.
    The Setup dialog opens.
  2. Under the Physics models setting:
    1. Set Time marching to Transient.
    2. Set the Time step size to 0.5 seconds.
    3. Set the Final time to 600.0 seconds (10 minutes).
    4. Select Spalart-Allmaras as the Turbulence model.
    5. Activate Include Gravitational Acceleration and set it to [0.0, -9.81, 0.0] m/s2.
    6. Set the Pressure scale to Absolute.
    7. Active Heat transfer.
    8. Set the Temperature scale to Absolute.


    Figure 5.
  3. Under the Advanced controls setting:
    1. Select Modify flow stagger settings.
    2. Assign Maximum flow stagger settings to 4 iterations.
    3. Select Modify temperature stagger settings.
    4. Assign Maximum temperature stagger settings to 6 iterations.


    Figure 6.

Assign Material Properties

  1. From the Flow ribbon, click the Material Library tool.


    Figure 7.
  2. Under Settings, click Fluid, then click the My Materials tab.
  3. Click to create a new material.
  4. Name the material Urea, set the density (ρ) type to Boussinesq and enter Density (kg/m3) and Reference temperature (K) values as shown below.


    Figure 8.
  5. Click the Specific Heat tab and set the Type to Piecewise Linear Enthalpy.
  6. Verify that the Curve fit variable is set to Temperature.
  7. Enter the values for Latent heat (J), Latent heat temperature (K), and Latent heat temperature interval (K) by referring to the figure below.
  8. Click three times to add three rows to the table and then enter the table values according to the figure below.


    Figure 9.
  9. Click the Viscosity tab and set µ (viscosity) to 0.002 kg/m-sec.
  10. Click the Conductivity tab and set k (conductivity) to 0.57 W/m-K.
  11. Close the material creation dialog.
  12. In the Material Library, click Solid under Settings.
  13. Select the My Materials tab then click to create a new material.
  14. Specify two solid material properties for Plastic and Copper using the figure below.


    Figure 10.
  15. From the Flow ribbon, click the Material tool.


    Figure 11.
  16. Assign the Solid material – Plastic – to the outer tank volume and the Fluid material – Urea – to the inner tank volume, as shown in the figure below.


    Figure 12.

Define the Porous Medium

  1. From the Flow ribbon, Porous tool group, click the Cartesian Porous Media tool.


    Figure 13.
  2. Hide the outer volume (Plastic) tank and select the inner volume tank (urea fluid body)
  3. Click Orientation on the guide bar then choose an arbitrary location to define the Porous model orientation
    Any location is acceptable for this model.
  4. Assign the Porous Media values according to the following figure.


    Figure 14.
  5. Click besides Effectiveness type.
  6. In the new dialog, click four time to add four empty rows to the table then enter values according to the figure below.


    Figure 15.
  7. Rename the Porous model.
    1. Double-click on Porous in the legend on the left side of the modeling window.
    2. Type Additive and press Enter.
  8. On the guide bar, click to execute the command and exit the tool.

Assign the Flow Boundary Conditions

  1. From the Flow ribbon, click the No Slip tool.


    Figure 16.
  2. Select the exterior faces of the plastic tank.
    Select a single face then right-click and choose Select > Face. This selects all faces that are connected by shared edges.


    Figure 17.
  3. In the microdialog, click the Temperature tab.
  4. Verify that the Thermal boundary condition is set to Flux.
  5. Set the Convective heat coefficient to 5.0 W/m2K.
  6. Set the Convective heat reference temperature to 263.15 K.


    Figure 18.
  7. Rename the wall boundary.
    1. Double-click on Wall in the legend on the left side of the modeling window.
    2. Type Exterior_Wall and press Enter.
  8. On the guide bar, click to execute the command and remain in the tool.
  9. Hide Exterior_Wall and select the interior faces of the heating element.
  10. In the microdialog, click the Temperature tab.
  11. Change the Thermal boundary condition to Temperature and set the Temperature (K) to 313.15.


    Figure 19.
  12. Click on the guide bar.
  13. From the Flow ribbon, click the Thin tool to define a virtual thin solid.


    Figure 20.
  14. In the modeling window, select the interior faces of the heating element (Wall) in the image above.
  15. In the microdialog, set the layer thickness (m) to 0.002 and the Material to Copper.


    Figure 21.
  16. Click on the guide bar.
  17. From the Flow ribbon, click the arrow next to the Setup tool set, then select Parameters.


    Figure 22.
    The Parameter Manager opens.
  18. Assign variables associated with the problem definition to compute the mesh settings, including the diameter of the heating element (d_line), the number of elements across the diameter (n), the local surface mesh size (dx), the volume mesh size (dx_vol), and the first layer height (flh).


    Figure 23.

Generate the Mesh

The meshing parameters for this tutorial are already set in the input file.
  1. From the Mesh ribbon, click the Surface tool.


    Figure 24.
  2. In the legend, right-click on Heating Element (34), select Edit, and verify that the average element size of Heating Element is set to dx.


    Figure 25.
  3. Similarly, verify that the average element size is set to dx_vol for Other (68).
  4. Click the Boundary Layer tool.


    Figure 26.
  5. In the legend, right-click on BL_Active (66), select Edit, and verify that the values in the following figure.


    Figure 27.
  6. Click the Volume Mesh tool.


    Figure 28.
  7. Define the Solid volume mesh parameters as in the following figure, where dx_vol=0.015m.


    Figure 29.
  8. Define the Fluid volume mesh parameters as in the following figure.


    Figure 30.
  9. Click the Volume tool.


    Figure 31.
  10. Define the mesh operations as shown in the following figure.


    Figure 32.
  11. Click Mesh.
    The Run Status dialog opens. Once the run is complete, the status is updated and you can close the dialog.
    Tip: Right-click on the mesh job and select View log file to view a summary of the meshing process.

Define a Surface Monitor and Run AcuSolve

  1. While in idle mode, set the entity selector to Solids then right-click and select Show All or press A to show all bodies.
  2. Hide the plastic tank by clicking on the exterior tank and then pressing H.
  3. Form the Solution ribbon, click the Surfaces tool.


    Figure 33.
  4. Select by Face after selecting a single face on the interior tank walls.
    This will select all faces that are shared.


    Figure 34.
  5. On the guide bar, click to execute the command and exit the tool.
  6. Rename the surface output.
    1. Double-click on Surface Output in the legend on the left side of the modeling window.
    2. Type Wall-Output and press Enter.
  7. From the Solution ribbon, click the Run tool.


    Figure 35.
    The Launch AcuSolve dialog opens.
  8. Set the Parallel processing option to Intel MPI.
  9. Optional: Set the number of processors to 4 or 8 based on availability.
  10. Set the Default initial conditions as in the following figure.


    Figure 36.
  11. Leave the remaining default options then click Run to launch AcuSolve.

Post-Process the Results

Post-Process with the Plot Tool

  1. From the Solution ribbon, click the Manage tool.


    Figure 37.
  2. In the Run Status dialog, right-click on the AcuSolve run and select Plot time history to launch the Plot Manager.
    The residual and solution ratios for pressure, velocity, eddy viscosity, and temperature are shown.


    Figure 38.
  3. Expand Integrated Surface Output > Temperature and select heat flux.
  4. Select the Wall – Output to plot the heat flux entering the domain from the heating element.
    Note: The value stabilizes near the end of the simulation, indicating that the model is approaching the prescribed thermal boundary conditions.


    Figure 39. Integrated heat flux entering the domain from the heating element surface
  5. Expand the Integrated Surface Output > Temperature > temperature.
  6. Select the Interior Wall – Output to plot the temperature increase of the inside wall of the tank.
    Note: The value is not stabilized by the end of the simulation, indicating that the model has not reached the final temperature to balance the prescribed thermal boundary conditions. After 10 minutes of physical time, approximately 35% of the additive has been melted.


    Figure 40. Integrated temperature on the interior surface of the tank wall

Post-Process with HyperWorks CFD Post

  1. In the Run Status dialog, right-click on the AcuSolve run and select Visualize results to launch HyperWorks CFD Post.
  2. From the Post ribbon, click the Boundary Groups tool.


    Figure 41.
  3. Click on the guide bar to open the Advanced Selection dialog.
  4. Select Exterior_Wall - Output then close the dialog.


    Figure 42.
  5. Set the transparency of the Boundary Group to approximately 75%.
  6. On the guide bar, click to execute the command and exit the tool.
  7. From the Post ribbon, click the Iso-Surfaces tool.


    Figure 43.
  8. Select temperature as the Iso Variable and set the Iso Value of temperature (K) to 261.15.


    Figure 44.
  9. Click Calculate.
  10. In the display properties microdialog, define the Display as constant and select a color of choice.


    Figure 45. Transparent boundary of the tank, showing an Iso-Surface of temperature T=261.15 K, Time=0.0 sec
  11. Using the results animation toolbar, skip to the end of the simulation results.


    Figure 46. Transparent boundary of the tank, showing an Iso-Surface of temperature T=261.15 K, Time=600.0 sec

Summary

In this tutorial, you learned how to set up and solve a flow and thermal simulation with temperature dependent porous media effectiveness. Utilizing the proposed implementation allowed you to specify the melting point of a fluid and compute the melted region of the fluid. You started by importing the HyperWorks CFD input database and then you defined the porous medium to control the melting point of the fluid. Next, you assigned the thermal boundary conditions and generated the mesh using the parametric variable definitions. Once the solution was computed, you created a plot of the heat flux and temperature for the critical surfaces with the model using HyperWorks CFD Plot Manager.