# ACU-T: 3110 Exhaust Manifold Conjugate Heat Transfer - CFD Data Mapping

## Prerequisites

This tutorial introduces you to setting up and solving a steady state conjugate heat transfer problem using HyperMesh and then using acuOptiStruct to generate an OptiStruct solver deck to perform a thermal stress analysis. 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. To run this simulation, you will need access to a licensed version of HyperMesh 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-T3110_acuOptiStruct.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 an exhaust manifold with four inlets and one outlet. The inlets have flanges with holes for steel bolts to attach the manifold. The body of the manifold is made up of stainless steel.

The diameter of the inlets is 0.036 m; the inlet velocity (v) is 8.0 m/s; and the temperature (T) of the fluid entering the inlets is 700 K. The diameter of the outlet is 0.036 m. The pipe wall has a thickness of 0.003 m and the flanges have a thickness of 0.01 m.

The combustion mixture enters the inlets and heat is transferred through conduction inside the manifold. The heat transfer causes deformations and stress in the manifold body which can be simulated using OptiStruct.

The fluid in this problem is air, which has the following material properties:
Density (ρ)
1.225 kg/m3
Viscosity (μ)
1.781 * 10-5 kg/m-s
Specific Heat (Cp)
1005 J/kg-K
Conductivity (k)
0.0251 W/m-K
The exhaust manifold is designed as Steel which has following material properties:
Density (ρ)
800 kg/m3
Specific Heat (Cp)
500 J/kg-K
Conductivity (k)
16.2 W/m-K

For the AcuSolve simulation, the variation in material properties of air with temperature is ignored.

The AcuSolve simulation will be set up to model steady state heat transfer to determine the temperature and pressure distribution on the walls of the manifold.

The nodal surface output needs to be activated for all the surfaces in order to create the OptiStruct input deck from the acuOptiStruct command.

The temperature distribution and forces on the wetted surfaces are used by OptiStruct to calculate the deformations and stress in the solid body.

The OptiStruct input deck is generated through a utility acuOptiStruct which can be used for a one-way coupled simulation. The following input commands are of importance for this simulation:
-solids
Input name for the solid body/bodies where conduction heat transfer would take place.
-den
Density values for the solid body/bodies.
-spcsurfs
List of surfaces where boundary condition constraints need to be specified.
-spcsurfsdof
List of degrees of freedom for the surfaces.
-spcsurfsdofvals
List of degrees of freedom values for the surfaces which is zero by default.
-type
Stress analysis type for the OptiStruct solver.
For this simulation, the constrained surfaces are the flange bolts and Outlet end of the manifold. These surfaces will be constrained in all six degrees of freedom (Translation and Rotation). The default value of zero is used.

The stress analysis type is selected as steady linear where the deformations are in the elastic range; that is, the stresses, σ, are assumed to be linear functions of the strains, ε, Hooke's law can be used to calculate the stresses.

## Open the HyperMesh Model Database

1. Start HyperMesh Desktop 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-T3110_acuOptiStruct.hm and click Open.
4. Click File > Save As.
The Save Model As dialog opens.
5. Create a new directory named Manifold_TFSI 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 Manifold_TFSI 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, verify that the Analysis type is set to Steady State.
3. Set the Temperature equation to Advective Diffusive.
4. Set the Turbulence model to Spalart Allmaras.

## Assign Material Properties and Boundary Conditions

### 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 8000 kg/m3.
5. Set the Specific heat to 500 J/kg-K.
6. Set the Conductivity to 16.2 W/m-k.

### Assign Material Properties and Boundary Conditions

By default, all components are assigned to the wall boundary condition. In this step, you will change them to the appropriate boundary conditions and assign material properties to the fluid volumes.
1. In the Solver Browser, expand 12.Surfaces > WALL.
2. Click Fluid. In the Entity Editor,
1. Change the Type to FLUID.
2. Set the Material to Air_HM.
3. Click Solid. In the Entity Editor,
1. Change the Type to SOLID.
2. Set the Material to Steel.
4. Click Inlets. In the Entity Editor,
1. Change the Type to INFLOW.
2. Set the Inflow type to Velocity.
3. Verify that the Inflow velocity type is set to Normal.
4. Set the Normal velocity to 8.0 m/sec.
5. Set the Temperature to 700 K.
6. Set the Turbulence input type to Viscosity Ratio.
A new field for assigning materials appears above the Simple Boundary Condition tab.
7. Set the Material to Air_HM.
8. Set the Turbulence viscosity ratio to 40.
9. Under the Surface Output tab, set the Nodal time step frequency to 100.
Since this is a steady state simulation, acuOptiStruct needs the nodal surface output for each surface at the final time step. By setting the Nodal time step frequency to 100, AcuSolve will write the nodal surface output at the last time step of the simulation or the 100th time step, whichever is earlier.
5. Click Outlet. In the Entity Editor,
1. Change the Type to OUTFLOW.
2. Under the Surface Output tab, set the Nodal time step frequency to 100.
Since this is a steady state simulation, acuOptiStruct needs the nodal surface output for each surface at the final time step. By setting the Nodal time step frequency to 100, AcuSolve will write the nodal surface output at the last time step of the simulation or the 100th time step, whichever is earlier.
6. Click Outlet_End. 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. Set the Convective heat flux reference temperature to 303 K.
4. Under the Surface Output tab, set the Nodal time step frequency to 100.
Since this is a steady state simulation, acuOptiStruct needs the nodal surface output for each surface at the final time step. By setting the Nodal time step frequency to 100, AcuSolve will write the nodal surface output at the last time step of the simulation or the 100th time step, whichever is earlier.
7. Click Outer_Wall. 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. Set the Convective heat flux reference temperature to 303 K.
4. Under the Surface Output tab, set the Nodal time step frequency to 100.
Since this is a steady state simulation, acuOptiStruct needs the nodal surface output for each surface at the final time step. By setting the Nodal time step frequency to 100, AcuSolve will write the nodal surface output at the last time step of the simulation or the 100th time step, whichever is earlier.
8. Click Inner_Wall_Fluid. In the Entity Editor,
1. Verify that the Type is set to WALL.
2. Under the Surface Output tab, set the Nodal time step frequency to 100.
Since this is a steady state simulation, acuOptiStruct needs the nodal surface output for each surface at the final time step. By setting the Nodal time step frequency to 100, AcuSolve will write the nodal surface output at the last time step of the simulation or the 100th time step, whichever is earlier.
9. Click Inner_Wall_Solid. In the Entity Editor,
1. Verify that the Type is set to WALL.
2. Under the Surface Output tab, set the Nodal time step frequency to 100.
Since this is a steady state simulation, acuOptiStruct needs the nodal surface output for each surface at the final time step. By setting the Nodal time step frequency to 100, AcuSolve will write the nodal surface output at the last time step of the simulation or the 100th time step, whichever is earlier.
10. Click Flange. 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. Set the Convective heat flux reference temperature to 303 K.
4. Under the Surface Output tab, set the Nodal time step frequency to 100.
Since this is a steady state simulation, acuOptiStruct needs the nodal surface output for each surface at the final time step. By setting the Nodal time step frequency to 100, AcuSolve will write the nodal surface output at the last time step of the simulation or the 100th time step, whichever is earlier.
11. Click Flange_Bolts. 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. Set the Convective heat flux reference temperature to 303 K.
4. Under the Surface Output tab, set the Nodal time step frequency to 100.
Since this is a steady state simulation, acuOptiStruct needs the nodal surface output for each surface at the final time step. By setting the Nodal time step frequency to 100, AcuSolve will write the nodal surface output at the last time step of the simulation or the 100th time step, whichever is earlier.
12. On the menu bar, go to BCs > Components > Auto Wall > Deactivate. Make sure that the Auto Wall is deactivated for all the wall surfaces.
To create an OptiStruct solver deck, acuOptiStruct needs a Simple Boundary Condition and Surface Output defined on all the surfaces, including the fluid and solid side of the interfaces. Hence, auto wall should not be used for any wall surfaces while using the acuOptiStruct utility.
13. In the Solver Browser, click the Inner_Wall_Fluid component. In the Entity Editor. activate the Interface Surface Display option and turn On the interface surface.
14. Similarly, click the Inner_Wall_Solid component, activate the Interface Surface Display option, and turn On the interface surface.
15. Save the model.

### Define the Nodal Output Frequency

1. In the Solver Browser, expand 17.Output and then click on NODAL_OUTPUT.
2. In the Entity Editor, verify that the Time step frequency is set to 1000.
This means the nodal output will be stored at the last time step, or the time step at which the solution converges, whichever is earlier.
Note: For transient simulations, the nodal output frequency should be set to 1 for both global nodal output and the individual nodal surface output.
3. Save the model.

## Compute the Solution

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. Activate the Export options checkbox then turn off the Always two layers for interfaces checkbox.
Since you split the interface between the fluid and domain already, this option need not be activated.
5. Leave the remaining options as default and click Launch to start the solution process.
Once you hit the Launch button, the AcuTail and AcuProbe windows are launched automatically. A summary of the run in the AcuTail window indicates that the solver run is complete. Once the run is compete, you can close the AcuTail and AcuProbe windows.

## Use acuOptiStruct to Generate the OptiStruct Solver Deck

Now that the AcuSolve solution has been calculated, you are ready to use the utility ‘acuOptiStruct’ to generate the OptiStruct input deck and run the case using HyperWorks Solver Run Manager. HyperWorks Solver Run Manager is a simple utility which allows to launch any HW solver by selecting appropriate input file(s) and typing any options (if needed) in the field displayed. OptiStruct is an industry proven, modern structural analysis solver for linear and nonlinear structural problems under static and dynamic loadings. OptiStruct can be started directly from the Start menu.

acuOptiStruct uses the flow and thermal data from an AcuSolve conjugate heat transfer CFD simulation to specify the temperature and pressure loads and generates the files necessary to perform a thermal stress analysis using OptiStruct. Executed after the completion of the AcuSolve simulation, acuOptiStruct writes out the solid element mesh data from the AcuSolve run as well as the convective heat transfer information on the wetted surfaces of the solid mesh. Data is written directly in OptiStruct format, both eliminating data loss due to projecting results from one mesh to another and adding fidelity with spatial variation of temperatures and heat transfer coefficients.

In the next steps, you will execute the acuOptiStruct command with the necessary options, which will generate a .fem file. Then you will use OptiStruct to solve the structural problem.

1. Start AcuSolve Command Prompt from the Windows Start menu by clicking Start > Altair <version> > AcuSolve Cmd Prompt .
2. Browse to your working directory where AcuSolve results are stored by using the cd command.
3. Execute the following command:

acuOptiStruct -solids Solids -spcsurfs Flange_Bolts,Outlet_End -spcsurfsdof 123456,123456 -spcsurfsdofvals 0,0 -type sl

This command will generate an OptiStruct input deck from the temperature filed of the flow solution by using the specified constraint surfaces and their degrees of freedom. The analysis type is set to steady linear.
4. Start OptiStruct from the Windows Start menu by clicking Start > Altair <version> > OptiStruct.
5. Click the next to Input File(s).
6. Browse to the location that you use as your working directory.
7. Select the .fem file.
8. Click Run to run the case.
Once the run is complete, the HyperWorks Solver View will show “OptiStruct Job Completed” in the Run summary window.

## Post-Process the Results with HyperView

Once the OptiStruct run is complete, close the HyperWorks Solver View dialog. In the HyperMesh Desktop window, close the AcuSolve Control and Solver job Launcher dialogs. In the next few steps, you will plot the contour plot of temperature and pressure on the fluid domain and the displacement and stress contours on the solid domain.

### Switch to the HyperView Interface and Load the AcuSolve Model and Results

1. In the HyperMesh Desktop window, click the ClientSelector drop-down in the bottom-left corner of the graphics window.
2. Select HyperView from the list.
3. In the pop-up dialog that appears, click Yes.
The interface is changed to HyperView.

Once HyperView is loaded, the Load model and results panel should be open by default. If you do not see the panel, click File > Open > Model.

4. In the Load model and results panel, click next to Load model.
5. 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 Manifold_TFSI.1.Log.
6. Click Open.
7. Click Apply in the panel area to load the model and results.

### Create a Contour Plot of Temperature and Pressure

1. Click on the Results toolbar to open the Contour panel.
2. In the panel area, set the Result type to Temperature (s).
3. In the panel area, click Apply to plot the temperature contours.
4. In the Results Browser, expand the list of Components.
5. Click the Isolate Shown icon then click the Inner_Wall_Fluid component to turn off the display of all components in the graphics window except the Inner Wall component.
6. In the panel area, change the Result type to Pressure (s).
7. Click Apply to plot the pressure contours.

1. Click on the drop-down beside the Page Window Layout icon on the PageControls toolbar.
2. In the drop-down menu, select the vertical 2-window layout icon.
3. Click in the newly created graphics window then click the Load Results icon.
4. In the Load model and results panel, click next to Load model.
6. Click Open.
7. Click Apply in the panel area to load the model and results from the OptiStruct results file.
Observe that this model contains only the solid domain since only the solid is included while generating the OptiStruct solver deck.

### Create a Contour Plot of Displacement and Element Stresses

1. Click on the Results toolbar to open the Contour panel.
2. In the panel area, set the Result type to Displacement (v).
3. Click Apply to plot the displacement magnitude contours.
4. In the panel area, change the Result type to Element Stresses (2D & 3D) (t) and select vonMises from the drop-down below.
5. Click Apply.

## Summary

In this tutorial you learned how to set up a conjugate heat transfer problem using HyperMesh and solve it using AcuSolve. Once you computed the solution, you used acuOptiStruct to generate the input deck for OptiStruct. Once the solution for the structural analysis was computed, you post-processed the results using HyperView and created contour plots of Temperature, Pressure, Displacement and Stress.