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 HyperMesh, 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 HyperMesh and AcuSolve.

Prior to running through this tutorial, click here to download the tutorial models. Extract ACU-T3100_MixingElbowHeatTransfer.hm from HyperMesh_tutorial_inputs.zip.

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 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

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 ACU-T3100_MixingElbowHeatTransfer.hm and click Open.
  4. Click File > Save As.
    The Save Model 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.

Set the General Simulation Parameters

  1. Go to the Solver Browser, expand 01.Global, then click PROBLEM_DESCRIPTION.
  2. In the Entity Editor, set the Turbulence equation to Advective Diffusive.
  3. Set the Turbulence Model to Spalart Allmaras.


    Figure 2.

Set Up Boundary Conditions and Material Model Parameters

In this step, you will start by creating a new material, then you will define the surface boundary conditions for the problem and assign material properties to the fluid and solid volumes.

Create a New Material Model

  1. In the Solver Browser, expand the 02.Materials tree.
  2. Right-click on SOLID and select Create.
  3. In the Entity Editor, change the name to Steel.
  4. Set the Density to 8030 kg/m3.
  5. Set the Specific heat to 500 J/kg-K.
  6. Set the Conductivity to 16.2 W/m-k.


    Figure 3.

Set Up Boundary Conditions

  1. In the Solver Browser, expand 12.Surfaces > WALL.
  2. Click Large_Inlet. In the Entity Editor,
    1. Change the Type to INFLOW.
    2. Set the Inflow type to Average velocity.
    3. Set the Average velocity to 0.4 m/s.
    4. Set the Temperature to 295.0 K.


    Figure 4.
  3. Similarly, click Small_Inlet. In the Entity Editor,
    1. Change the Type to INFLOW.
    2. Set the Inflow type to Average velocity.
    3. Set the Average velocity to 1.2 m/s.
    4. Set the Temperature to 320.0 K.
  4. Click Outflow. In the Entity Editor, change the Type to OUTFLOW.


    Figure 5.
  5. Click Symmetry. In the Entity Editor, change the Type to SYMMETRY.


    Figure 6.
  6. Similarly, click Pipe_Symmetry and change the Type to SYMMETRY.
  7. Click Pipe_OuterWalls. In the Entity Editor,
    1. Verify that the Type is set to WALL.
    2. Set the Convective heat flux coefficient to 100 J/m2-sec-K.
    3. Enter 302.594 K for the Convective heat flux reference temperature.


    Figure 7.
  8. Click Pipe_InnerWalls. In the Entity Editor,
    1. Verify that the Type is set to WALL.
    2. Turn Show advanced features On.
    3. Verify that the Activate Auto Walls option is set to On.
      This surface is an interface between the fluid and solid regions. Auto_Wall is an advanced feature in AcuSolve that automatically detects and splits the internal surface without the user having to do it manually. Hence in this case, the Pipe_InnerWalls surface set will be split into two, one on the fluid region and the other on the solid region.


    Figure 8.
  9. Click Pipe_Ends. In the Entity Editor,
    1. Verify that the Type is set to WALL.
    2. Change the Temperature BC type to None.


    Figure 9.
  10. Click Fluid. In the Entity Editor,
    1. Change the Type to FLUID.
    2. Select Water_HM as the Material.


    Figure 10.
  11. Click Solid. In the Entity Editor, and
    1. Change the Type to SOLID.
    2. Select Steel as the Material.


    Figure 11.
  12. Save the model.

Compute the Solution

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

Run AcuSolve

  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 12.

Post-Process the Results with HyperView

Once the solution has converged, close the AcuProbe and AcuTail windows. Go to the HyperMesh window and close the AcuSolve Control tab.

Open HyperView and Load the Model and Results

  1. In the HyperMesh main menu area, click Applications > 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 and Pipe_Symmetry components to turn off the display of all components in the graphics window except the Symmetry and Pipe_Symmetry components.


    Figure 13.
  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 14.
  9. Click the Legend tab then click Edit Legend. In the dialog, change the Numeric format to Fixed then click OK.


    Figure 15.

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

  10. Turn off the display for all components except Outlet.
  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 16.

Summary

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