ACU-T: 3101 Transient Conjugate Heat Transfer in a Mixing Elbow

Prerequisites

This tutorial provides you instructions for running a transient simulation of a 3D turbulent flow with conjugate heat transfer in a mixing elbow. You should have already run through the ACU-T: 3100 Conjugate Heat Transfer in a Mixing Elbow tutorial and have a basic understanding of HyperMesh, AcuSolve and HyperView. The HyperWorks introductory tutorial, ACU-T: 1000 HyperWorks UI Introduction, gives a basic introduction to HyperWorks and AcuSolve.

Prior to running through this tutorial, copy HyperMesh_tutorial_inputs.zip from <Altair_installation_directory>\hwcfdsolvers\acusolve\win64\model_files\tutorials\AcuSolve to a local directory. Extract ACU-T3101_MixingElbowTransient.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

This problem is divided into two components, a steady state solution and a transient solution. The schematic of the steady state component is shown below.



Figure 1.

The diameter of the large inlet is 0.1 m, the inlet velocity (v) is 0.4 m/s and the temperature (T) of the fluid entering the large inlet is 295 K. The diameter of the small inlet is .025 m, the velocity is 1.2 m/s, and the temperature of the fluid entering the small inlet is 320 K. The pipe wall has a thickness of 0.005 m. The fluid in this problem is water and the pipe walls are made of stainless steel with a density of 8030 kg/m3, a conductivity of 16.2 W/m-K, and a specific heat of 500 J/kg-K.

The model file for the steady state part of the problem is provided as the input file. Once the steady state solution is computed, it is projected on to the mesh and used as the initial state for the transient simulation. The starting point for the transient portion of the problem is shown schematically in the figure below.



Figure 2.

At 0.2s into the simulation, a cold slug of water is injected at both the inlets and the temperature is ramped down to 283.15 K starting from 0.2 s to 0.4 s. Then it is maintained constant at 283.15 K for 1 sec and then ramped up to initial states from 1.4s to 1.6s. Given a flow path of 0.6356 m, the transit time for the slug is approximately 1.6s. Therefore, our simulation time should be at least 3.2 s to factor in the duration of the slug and transit time. The total simulation time will be 4.5s to allow time for the thermal conditions to return to a steady state.

The temperature change at the large inlet is from 295 K to 283.15 K. At the small inlet, the temperature changes from 320 K to 283.15 K. The ratio of the cold slug temperature to the initial temperature of the large inlet flow is 0.9598. The ratio of the cold slug temperature to the initial temperature of the small inlet flow is 0.8848. These values will be used in creating multiplier functions to model the transient temperatures at the inlets.



Figure 3.

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-T3101_MixingElbowTransient.hm and click Open.
  4. Click File > Save As.
    The Save Model As dialog opens.
  5. Create a new directory named ConjugateHeatTransfer_Transient 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 ConjugateHeatTransfer_Transient as the file name for the database, or choose any name of your preference.
  7. Click Save to create the database.

Run the Steady State Simulation

In this step, you will run the steady state simulation with the model file provided and then create the nodal initial condition files needed for the transient simulation. Make sure that the visibility of the mesh for all the components is on.

  1. Click on the ACU toolbar.
    The Solver job Launcher dialog opens.
  2. Optional: For a faster solution time, set the number of processors to a higher number (4 or 8) based on availability.
  3. Once the solution is converged, close the AcuProbe and AcuTail windows. In addition, close the Solver job Launcher and AcuSolve Control tabs.
  4. Start AcuSolve Command Prompt from the Windows Start menu by clicking Start > All Programs > Altair <version> > AcuSolve Cmd Prompt .
  5. In the Command Prompt, change the directory to the working directory by using the cd command.
  6. Type the command acuProj -crd HYPERMESH.DIR\ConjugateHeatTransfer_Transient.crd -run 1 and press Enter.
  7. Verify that the working directory is now populated with the new files.

    ConjugateHeatTransfer_Transient.pres.nic
    ConjugateHeatTransfer_Transient.vel.nic
    ConjugateHeatTransfer_Transient.temp.nic
    ConjugateHeatTransfer_Transient.eddy.nic

  8. Move the .nic files in the working directory into the HYPERMESH.DIR folder.

Set the Transient Simulation Parameters

Set the Analysis Parameters

  1. Go to the Solver Browser, expand 01.Global, then click PROBLEM_DESCRIPTION.
  2. Change the Analysis type to Transient in the Entity Editor.


    Figure 4.

Specify the Solver Settings

  1. In the Solver Browser, click 02.SOLVER_SETTINGS under 01.Global.
  2. In the Entity Editor, set the Max time steps to 0.
  3. Set the Final time to 4.5 sec.
  4. Set the Initial time increment to 0.053 sec.
  5. Verify that the Convergence tolerance is set to 0.001.
  6. Set the Min stagger iterations to 2 and Max stagger iterations to 5.
  7. Change the Relaxation factor to 0.0.
  8. Turn Off the Flow and Turbulence fields.


    Figure 5.

Set the Nodal Output Frequency

  1. In the Solver Browser, expand 17.Output then click NODAL_OUTPUT.
  2. In the Entity Editor, set the Time step frequency to 3 and the Time frequency to 0.
  3. Turn On the Output initial condition field.


    Figure 6.
  4. Save the model.

Specify the Transient Inflow Boundary Conditions and Nodal Initial Conditions

In this step, you will start by creating Multiplier Functions and then specify the transient boundary conditions for both the inlets. Then you will specify the Nodal Initial Conditions for the flow and thermal fields.

Create Multiplier Functions

First, you will create curves for the scaling function to be used for the Multiplier Function type.

  1. Right-click on empty space in the Model Browser and select Create > Curve.
    The Curve editor dialog opens.
  2. Click New and enter Large_Inlet as the name in the panel area.
  3. Click Proceed.
  4. In the Curve editor dialog, enter the following values for the curve array.


    Figure 7.
  5. Click Update.
  6. Click again on New and enter Small_Inlet as the name of the second curve, then click Proceed.
  7. In the Curve editor dialog, click on Small_Inlet in the top-left corner and enter the following values for the array.
    Make sure that the Current curves is showing Small_Inlet.


    Figure 8.
  8. Click Update.
    Both the curves should be displayed, as shown in the figure below.
    Figure 9.
    Note: The default color for the curves is grey, which can be changed using the Color option on the bottom left corner of the Curve editor dialog

    Next, you will create the Multiplier Functions for both the Inlets.

  9. In the Solver Browser, right-click on 05.Multiplier_Function and select Create.
  10. Set the Name of the function to Large_Inlet.
  11. Select Piecewise Linear for the Multiplier Function Type.
  12. Select the Curve Large_Inlet.


    Figure 10.
  13. Repeat the previous four steps to create a Multiplier Function named Small_Inlet with Small_Inlet as the Curve.

Specify the Nodal Initial Conditions

In this step, first you will specify the initial values of Pressure, Velocity, Temperature and Eddy Viscosity at all nodes and then Transient BCs for both the inlets.

  1. In the Solver Browser, expand 01.Global then click 03.NODAL_INITIAL_CONDITION.
  2. In the Entity Editor, under the Pressure tab, change the Type to Nodal Values and Select nodes by to NIC file.
  3. Click on the select file icon in the value field of NIC file, browse to your working directory, and select the ConjugateHeatTransfer_Transient.pres.nic file.


    Figure 11.
  4. Repeat the steps 2 and 3 for the Velocity, Temperature, and Eddy Viscosity fields and select the ConjugateHeatTransfer_Transient.vel.nic, ConjugateHeatTransfer_Transient.temp.nic, and ConjugateHeatTransfer_Transient.eddy.nic files respectively.

Specify the Transient Inlet Boundary Conditions

  1. In the Solver Browser, expand 12.Surfaces > INFLOW.
  2. Click Large_Inlet. In the Entity Editor, under the Simple Boundary Condition tab,
    1. Turn On the Show advanced features field.
    2. Click on the entity collector in the Value field of the Temperature multiplier function and select Large_Inlet. Click OK to close the dialog.


    Figure 12.
  3. Similarly, click on Small_Inlet component and turn On the Show advanced features field. Select Small_Inlet as the Temperature multiplier function.
  4. 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. Set the Output time steps to All if it's not already set.
  5. Leave the remaining options as default and click Launch to start the solution process.


    Figure 13.

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 ConjugateHeatTransfer_Transient.2.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 a Temperature Distribution Animation

In this step, you will create an animation of the temperature distribution with time on the Symmetry surface.
  1. In the Results Browser, expand the list of Components.
  2. Click the Isolate Shown icon then hold Ctrl and click the Symmetry and Pipe_Symmetry components to turn off the display of all components in the graphics window except the Symmetry and Pipe_Symmetry.
  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. Select Temperature (s) as the Result type.
  6. Click the Components entity selector. In the Extended Entity Selection dialog, select Displayed.
  7. Click Apply to display the Temperature contour on the Symmetry plane at the first-time step.
  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.
  10. In the Edit Legend dialog, change the Type to Dynamic Scale and the Numeric format to Fixed then click OK.
  11. On the Animation toolbar, click the Animation Controls icon .
  12. Drag the Max frame Rate slider to 1 fps.
  13. Click the Start/Pause Animation icon to play the animation in the graphics area.

Save the Animation

  1. In the menu area, select Preferences > Export Settings > AVI.
  2. In the Export Settings AVI dialog, set the Frame rate to 1 fps and click OK.
  3. On the ImageCapture toolbar, make sure that the Save Image to File option is On.


  4. Click the Capture Graphics Area Video icon .
    The Save Graphics Area Video As dialog opens.
  5. Navigate to the location where you want to save the file, enter a name of your choice, and click Save.

Summary

In this tutorial, you learned how to set up and run a transient conjugate heat transfer simulation using HyperMesh and AcuSolve. You learned how to specify Nodal Initial Conditions and how to create multiplier functions for setting up the transient boundary conditions. Finally, you used HyperView to create and save an animation of the results of the transient simulation.