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 using HyperMesh CFD and AcuSolve. 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 CFD and AcuSolve. The introductory tutorial, ACU-T: 1000 Basic Flow Set Up, gives a basic introduction to AcuSolve and HyperView.

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

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.


Start HyperMesh CFD and Open the HyperMesh Database

  1. Start HyperMesh CFD from the Windows Start menu by clicking Start > Altair <version> > HyperMesh CFD.
  2. From the Home tools, Files tool group, click the Open Model tool.
    Figure 4.


    The Open File 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.
  5. Create a new directory named MixingElbow_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 MixingElbow_Transient_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 input file provided.

  1. From the Solution ribbon, click the Run tool.
    Figure 5.


    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. Expand the Default initial conditions drop-down and deactivate the Pre-compute flow option.
  6. Set the x-velocity to 0 and the Temperature to 300.
  7. Click Run to launch AcuSolve.
    Figure 6.


  8. In the Run Status dialog, right-click on the AcuSolve run and select View log file.
  9. Once the solver run is complete, close the Run Status dialog.
    Figure 7.


Set the Transient Simulation Parameters

  1. From the Flow ribbon, click the Physics tool.
    Figure 8.


    The Setup dialog opens.
  2. Under the Physics models setting:
    1. Set Time marching to Transient.
    2. Set the Time step size to 0.053 and the Final time to 4.5.
    Figure 9.


  3. Click the Solver controls setting.
  4. Set the Minimum and Maximum stagger iterations to 2 and 5, respectively.
  5. De-activate the Flow and Turbulence equations.
    By turning these options off, AcuSolve will not update the solution to these equations. Instead, the current flow and turbulence values (generated from the steady state solution for this tutorial) will be used throughout the simulation, and AcuSolve will only solve for the temperature field.
    Figure 10.


  6. Close the dialog and save the model.

Specify the Transient Inflow Boundary Conditions

  1. From the Flow ribbon, Profiled tool group, click the Profiled Inlet tool.
    Figure 11.


  2. In the modeling window Boundaries legend, right-click Large Inlet and select Edit from the context menu.
    Figure 12.


  3. In the microdialog, click multiplier function drop-down menu next to Temperature and select Create new.
    Figure 13.


  4. In the dialog that appears, edit the name of the multiplier function by clicking in the top-left corner. Set the name to Large Inlet.
  5. Set the Type to Piecewise Linear.
  6. Verify that the Variable is set to Time and Evaluation is set to Time Step.
  7. Click four times to add four new rows to the bottom of the table.
  8. Enter the table values for the multiplier function as shown in the image below.
    Figure 14.


  9. Close the dialog.
  10. On the guide bar, click to execute the command and remain in the tool.
  11. In the Boundaries legend, right-click Small Inlet and select Edit from the context menu.
  12. In the microdialog, click multiplier function drop-down menu next to Temperature and select Create new.
  13. In the dialog that appears, edit the name of the multiplier function by clicking in the top-left corner. Set the name to Small Inlet.
  14. Set the Type to Piecewise Linear.
  15. Verify that the Variable is set to Time and Evaluation is set to Time Step.
  16. Click four times to add four new rows to the bottom of the table.
  17. Enter the table values for the multiplier function as shown in the image below.
    Figure 15.


  18. Close the dialog.
  19. On the guide bar, click to execute the command and exit the tool.
  20. Save the model.

Compute the Solution

Define Nodal Outputs

  1. From the Solution ribbon, click the Field tool.
    Figure 16.


    The Field Output dialog opens.
  2. Activate the Write initial conditions option and set the Time step interval to 3 for the Solution variables.
    Figure 17.


Launch AcuSolve

  1. From the Solution ribbon, click the Run tool.
    Figure 18.


    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. Expand the Restart menu and activate the Restart from previous solution option.
  6. Set the Problem name to MixingElbow_Transient (if not set already).
  7. Verify that the Run number is set to 1 and the Reset time step option is activated.
  8. Click Run to start the transient run.
    Figure 19.


  9. In the Run Status dialog, right-click on the second AcuSolve run and select View log file.
  10. Once the solver run is complete, close the Run Status dialog.

Post-Process the Results with HM-CFD Post

  1. Once the solution is completed, navigate to the Post ribbon.
  2. From the menu bar, click File > Open > Results.
  3. Select the AcuSolve .log file in your problem directory to load the results for post-processing.
    The solid and all the surfaces are loaded in the Post Browser.
  4. Isolate the Pipe_Symmetry and Symmetry flow boundaries in the Post Browser.
    Figure 20.


  5. Click the Boundary Groups tool.
    Figure 21.


  6. Select all visible surfaces in the modeling window.
  7. In the display properties microdialog, set the display to temperature.
  8. Activate the Legend toggle and click to reset the range.
  9. Click and set the Colormap Name to Rainbow Uniform.
    Figure 22.


  10. Click on the guide bar.
  11. Click at the bottom of the modeling window to view an animation of the transient flow with respect to the temperature contour.
    Figure 23.


  12. Save the animation.
    1. Go to File > Screen Capture > Advanced Capture.
    2. Click on the toolbar.
    3. Uncheck Include mouse cursor.
    4. Set the frame rate to 50.
    5. Click on the toolbar then drag over the area you want to record.
    6. Click to start recording and the same button to stop recording.
    7. Name the file and save it.

Summary

In this tutorial, you learned how to set up and run a transient conjugate heat transfer simulation using HyperMesh CFD and AcuSolve. You started by importing the input file, which had the conjugate heat transfer setup for the steady state run. Once the steady state solution was computed, you set the transient simulation parameters and applied the transient conditions at the inlets. Once the transient solution was computed, you post-processed the results using the Post ribbon.