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

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-T3101_MixingElbowTransient.hm from HyperWorksCFD_tutorial_inputs.zip.

## 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.

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.

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.

## 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.
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.
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.
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.

## Set the Transient Simulation Parameters

1. From the Flow ribbon, click the Physics tool.
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.
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.
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.
2. In the modeling window Boundaries legend, right-click on Large Inlet and select Edit from the context menu.
3. In the microdialog, click the Temperature tab (), then click the drop-down menu for multiplier functions and select Create new.
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.
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 on Small Inlet and select Edit from the context menu.
12. In the microdialog, click the Temperature tab (), then click the drop-down menu for multiplier functions 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.
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.
The Field Output dialog opens.
2. Activate the Write initial conditions option and set the Time step interval to 3 for the Solution variables.

### Launch AcuSolve

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

Once the solver run is complete, you will use HyperView to process the results.

### 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_Transient_Transient.2.log.
4. Click Open.
5. Click Apply in the panel area to load the model and results.

### Create a Temperature Distribution Animation

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.
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.
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 5 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 5 fps.
3. Set the JPEG quality to 99 and click OK.
4. On the ImageCapture toolbar, make sure that the Save Image to File option is On.
5. Click the Capture Graphics Area Video icon .
The Save Graphics Area Video As dialog opens.
6. 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 HyperWorks 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 HyperView.