ACU-T: 3300 Modeling of a Heat Exchanger Component


This tutorial provides instructions for running a steady-state simulation of a flow inside a pipe with an interior heat exchanger placed at the middle of the pipe. Prior to starting this tutorial, you should have already run through the introductory tutorial, ACU-T: 1000 HyperWorks UI Introduction, and have a basic understanding of HyperMesh and AcuSolve. To run this simulation, you will need access to a licensed version of HyperMesh and AcuSolve.

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

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 the figure below. It consists of a cylindrical pipe channel with an interior heat exchanger component volume with thickness ‘t’ and radius ‘r’. The heat exchanger component parameters are assigned to the HEX_Inlet surface component. Basically, the heat exchanger model is applied to a surface and the temperature rises across that surface to model the effect of the heat exchanger. Air enters the pipe at a velocity of 0.1 m/sec and flows through the heat exchanger volume and then exits through the outlet.

Figure 1.

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 and click Open.
  4. Click File > Save As.
    The Save Model As dialog opens.
  5. Create a new directory named HeatExchanger 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 HeatExchanger 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

In this step, you will set the simulation parameters that apply globally to the simulation.

  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. Change the Turbulence model to Spalart Allmaras.

    Figure 2.

Set Up Boundary Conditions and Assign Material Model Parameters

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. Select Air_HM as the Material.

    Figure 3.
  3. Similarly, click HEX and change the Type to FLUID and select Air_HM as the Material in the Entity Editor.
  4. Click Inlet. In the Entity Editor,
    1. Change the Type to INFLOW.
    2. Change the Inflow velocity type to Cartesian and set the X velocity to 0.1 m/sec.
    3. Set the Temperature to 273 K.
    4. Change the Turbulence input type to Viscosity Ratio.
    5. For the Turbulent viscosity ratio, enter a value of 40.

    Figure 4.
  5. Click Outlet. In the Entity Editor, change the Type to OUTFLOW.

    Figure 5.
  6. Click HEX_Inlet. In the Entity Editor,
    1. Change the Type to HEAT_EXCHANGER_COMPONENT.
    2. Verify that the Heat exchanger type is set to Constant Coolant Heat Reject.
    3. Set the Coolant Heat Reject to 200 W.
    4. Set the Coolant flow rate to 0.0006309 m3/sec.
    5. Set the Heat exchanger thickness to 0.06 m.
    6. Verify that the Upstream distance is set to 0.
    7. Change the Friction type to Kays London.
    8. Change the Core Friction Constant to 20.
    9. Change the Core Friction Exponent to -0.75.

    Figure 6.
  7. Click Walls. In the Entity Editor, verify that the Type is set to WALL.
    The surface mesh elements on the external wall surfaces and interfaces can be grouped into one single collector. Auto_Wall, which is an advanced feature in AcuSolve, re-groups them into surface sets based on the element set they belong to and whether they are internal or external surfaces. This process is done internally without the user having to do it manually.

    Figure 7.
  8. 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 8.

Post-Process with AcuProbe

As the solution progresses, the AcuTail and AcuProbe windows are launched automatically. The surface output and residual ratios can be monitored using AcuProbe.

  1. In the AcuProbe window, under the Data Tree, expand Residual Ratio, right-click on Final, and select Plot All.
    Note: You might need to click on the toolbar in order to properly display the plot.

    Figure 9.
  2. Once the solution is converged, right-click on Final under Residual Ratio and select Plot None.
  3. Click on the toolbar.
    A User Function dialog opens.
  4. Enter dT as the Name.
  5. Type In = in the Function field.
  6. Expand Heat Exchanger > HEX_Inlet. Right-click on air_temperature and select Copy Name. Paste the value in the function after In =.
  7. Type Out = on a new line in the Function field.
  8. Expand Heat Exchanger > HEX_Inlet. Right-click on coolant_temperature and select Copy Name. Paste the value in the function after Out =.
  9. On the next line, type value = Out - In.

    Figure 10.
    Note: The word “value” is case sensitive and should always be in lowercase characters. If it starts with a capital letter, it will give you an error window.
  10. Click Apply.

    Figure 11.

    You can zoom into the plot by clicking and then defining an area at the end of the curve. As shown in the figure below, for the given problem, the temperature rise is 43.21 K.

    Figure 12.


In this tutorial, you successfully learned how to set up and solve a simulation involving a Heat Exchanger component. You imported the meshed geometry and then assigned the boundary conditions and material properties for all the regions. Once the solution was computed, you defined a user function in AcuProbe in order to create a plot of the temperature rise across the heat exchanger volume.