ACU-T: 3100 Conjugate Heat Transfer in a Mixing Elbow

Prerequisites

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, AcuSolve, and HyperView. Although it is not necessary, it is recommended that you complete ACU-T: 2000 Turbulent Flow in a Mixing Elbow prior to running this simulation. To run this simulation, you will need access to a licensed version of HyperWorks CFD and AcuSolve.

Prior to running through this tutorial, copy HyperWorksCFD_tutorial_inputs.zip from <Altair_installation_directory>\hwcfdsolvers\acusolve\win64\model_files\tutorials\AcuSolve to a local directory. Extract ACU-T3100_MixingElbowHeatTransfer.hm from HyperWorksCFD_tutorial_inputs.zip.

Problem Description

The problem to be addressed in this tutorial is shown schematically in Figure 1. It consists of a mixing elbow made of stainless steel with water entering through two inlets with different velocities and at different temperatures. The geometry is symmetric about the XY midplane of the pipe, as shown in the figure.



Figure 1. Schematic of Mixing Elbow with Stainless-steel Walls

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-T3100_MixingElbowHeatTransfer.hm and click Open.
  4. Click File > Save As.
    The Save File As dialog opens.
  5. Create a new directory named MixingElbow_HeatTransfer 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 MixingElbow_HeatTransfer as the file name for the database, or choose any name of your preference.
  7. Click Save to create the database.

Validate the Geometry

  1. From the Geometry ribbon, click the Validate tool.


    Figure 3.
    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.

    The current model doesn’t have any of the issues mentioned above. Alternatively, if any issues are found, they are indicated by the number in the brackets adjacent to the tool name.

    Observe that a blue check mark appears on the top-left corner of the Validate icon. This indicates that the tool found no issues with the geometry model.


    Figure 4.
  2. Press Esc or right-click in the modeling window and select Exit from the context menu to exit the tool.
  3. Save the database.

Set Up the Problem

Set Up the Simulation Parameters and Solver Settings

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


    Figure 5.
    The Setup dialog opens.
  2. Click the Time setting and ensure that Steady is selected.


    Figure 6.
  3. Click the Flow setting.
  4. Check that the flow type is set to Turbulent.
  5. Select Spalart-Allmaras as the Turbulence model.
    The robustness and accuracy of the Spalart Allmaras turbulence model makes it an excellent choice for simulation of steady state flows.


    Figure 7.
  6. Click the Heat transfer setting then activate the Heat transfer check box.
  7. Click the Solver controls setting and verify that the parameters are set as shown in the figure below.


    Figure 8.
  8. Exit the Setup dialog.

Create a New Material Model

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


    Figure 9.
    The Material Library opens.
  2. Under Settings, click Solid.
  3. Click the My Materials tab then click to create a new solid.
    A material creation dialog opens.
  4. Rename the material.
    1. In the top-left of the dialog, click Solid to edit the name.
    2. Type Steel and press Enter.
  5. Change the Density value to 8030.


    Figure 10.
  6. Click the Specific Heat tab.
  7. Change the Specific heat value to 500.


    Figure 11.
  8. Click the Conductivity tab.
  9. Change the Conductivity value to 16.2.


    Figure 12.
  10. Exit the material creation dialog.


    Figure 13.
  11. Exit the Material Library.

Assign Material Properties

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


    Figure 14.
  2. Select the outer pipe solid.


    Figure 15.
  3. In the dialog that appears, click the drop-down menu next to Material and select Steel.
  4. On the guide bar, click to execute the command and remain in the tool.
  5. Next, select the inner pipe solid.


    Figure 16.
  6. In the dialog that appears, click the drop-down menu next to Material and select Water.
  7. On the guide bar, click to execute the command and exit the tool.

Assign Flow and Thermal Boundary Conditions

Set Boundary Conditions for the Large Inlet

The large inlet of the mixing elbow will be defined as a profiled inlet based on average velocity.
  1. From the Flow ribbon, Profiled tool group, click the Profiled Inlet tool.


    Figure 17.
  2. Click the face of the large inlet.


    Figure 18.
  3. In the dialog that appears, enter a value of 0.4 for Average velocity.
  4. Click to open the temperature tab.
  5. Enter a value of 295 for Temperature.
  6. Rename the inlet.
    1. From the legend on the left side of the modeling window, double-click on Inlet
    2. Type Large_Inlet and press Enter.
  7. On the guide bar, click to execute the command and remain in the tool.
    Note: The number of inlets created appears in parenthesis on the top-right of the Profiled tool icon.

Set Boundary Conditions for the Small Inlet

The small inlet of the mixing elbow will also be defined using average velocity. The guide bar for the Profiled tool should still be open from the last step.
  1. Click the face of the small inlet.


    Figure 19.
  2. In the dialog that appears, enter a value of 1.2 for Average velocity.
  3. Click to open the temperature tab.
  4. Enter a value of 320 for Temperature.
  5. Rename the inlet.
    1. From the legend on the left side of the modeling window, double-click on Inlet
    2. Type Small_Inlet and press Enter.
  6. On the guide bar, click to execute the command and exit the tool.

Set Boundary Conditions for the Outlet

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


    Figure 20.
  2. Click the face of the outlet.


    Figure 21.
  3. In the dialog that appears, make sure both Static pressure and Pressure loss factor are 0.


    Figure 22.
  4. On the guide bar, click to execute the command and exit the tool.

Set Boundary Conditions for the Symmetry Planes

This geometry is symmetric about the XY midplane, and can therefore be modeled with half of the geometry. In order to take advantage of this, the midplane needs to be identified as a symmetry plane. The symmetry boundary condition enforces constraints such that the flow field from one side of the plane is a mirror image of that on the other side.

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


    Figure 23.
  2. Click the face of the symmetry plane.


    Figure 24.
  3. In the dialog that appears, accept the default symmetry conditions.


    Figure 25.
  4. On the guide bar, click to execute the command and remain in the tool.
  5. Next, select the faces for the pipe wall symmetry.


    Figure 26.
  6. In the dialog that appears, accept the default symmetry conditions.
  7. Rename the boundary.
    1. From the legend on the left side of the modeling window, double-click on Symmetry 1
    2. Type Pipe_Symmetry and press Enter.
  8. On the guide bar, click to execute the command and exit the tool.

Set Boundary Conditions for the Outer Pipe Walls

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


    Figure 27.
  2. Click the faces of the outer pipe walls.


    Figure 28.
  3. In the dialog that appears, click to open the temperature tab.
  4. Change the Convective heat coefficient value to 100.
  5. Change the Convective heat resistance temperature value to 302.594.


    Figure 29.
  6. Rename the boundary.
    1. From the legend on the left side of the modeling window, double-click on Wall
    2. Type Pipe_OuterWalls and press Enter.
  7. On the guide bar, click to execute the command and exit the tool.
  8. Save the database.

Generate the Mesh

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


    Figure 30.
    The Meshing Operations dialog opens.
    Note: If the model has not been validated, you are prompted to create the simulation model before running the batch mesh.
  2. Check that the Average element size is 0.03606.
  3. Accept all other default parameters.


    Figure 31.
  4. 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.
  5. Observe the refined mesh around the pipe walls.


    Figure 32.

Run AcuSolve

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


    Figure 33.
    The Launch AcuSolve dialog opens.
  2. Set the Parallel processing option to Intel MPI.
  3. Optional: Set the number of processors to 4 or 8 based on availability.
  4. Deactivate the Automatically define pressure reference option.
  5. Leave the remaining options as default and click Run to launch AcuSolve.


    Figure 34.
    The Run Status dialog opens. Once the run is complete, the status is updated and you can close the dialog.
    Tip: While AcuSolve is running, right-click on the AcuSolve job in the Run Status dialog and select View Log File to monitor the AcuSolve solution process.

Post-Process the Results with HyperView

This part of the tutorial shows you how to work with steady state analysis data in HyperView once the solution has converged.

Open HyperView and Load the Model and Results

  1. Start HyperView from the Windows Start menu by clicking Start > All Programs > Altair <version> > HyperView.
    Once the HyperView window is loaded, the Load model and results panel should be open by default. If you do not see the panel, click File > Open > Model.
  2. In the Load model and results panel, click next to Load model.
  3. In the Load Model File dialog, navigate to your working directory and select the AcuSolve .Log file for the solution run that you want to post-process. In this example, the file to be selected is MixingElbow_HeatTransfer.1.Log.
  4. Click Open.
  5. Click Apply in the panel area to load the model and results.
    The model is colored by geometry after loading.

Create Contours for Temperature Distribution

In this step, you will display temperature contours on the symmetry plane and the outlet surface.
  1. In the Results Browser, expand the list of Components.
  2. Click the Isolate Shown icon then hold Ctrl and select the Symmetry - Output and Pipe_Symmetry - Output components to turn off the display of all components in the graphics window except the Symmetry and Pipe_Symmetry.


    Figure 35.
  3. Orient the display to the xy-plane by clicking on the Standard Views toolbar.
  4. Click on the Results toolbar to open the Contour panel.
  5. Under result type, select Temperature(s).
  6. Click the Components entity selector. In the Extended Entity Selection dialog, select Displayed.
  7. Click Apply.
  8. In the panel area, under the Display tab, turn off the Discrete color option.


    Figure 36.
  9. Click the Legend tab then click Edit Legend. In the dialog, change the Numeric format to Fixed then click OK.


    Figure 37.

    Next, you will display temperature contours on the outlet surface.

  10. Turn off the display for all components except Outlet - Output.
  11. Click on the Standard Views toolbar.
  12. In the panel area, click on the Components entity selector and select Displayed.
  13. In the panel area, click Apply.
    The contour plot on the outlet surface is displayed.


    Figure 38.

Summary

In this tutorial, you learned how to set up a conjugate heat transfer simulation using HyperWorks CFD and how to create a new material model. You launched AcuSolve directly from HyperWorks CFD to compute the solution and then post-processed the results using HyperView.