ACU-T: 3100 Conjugate Heat Transfer in a Mixing Elbow

This tutorial provides the instructions for setting up, solving, and viewing results for a simulation of 3D turbulent-flow with conjugate heat transfer in a mixing elbow. It is designed to introduce you to the AcuSolve tool set with a simple problem.

The basic steps in any CFD simulation are shown in ACU-T: 2000 Turbulent Flow in a Mixing Elbow. The following additional capabilities of AcuSolve are introduced in this tutorial:
  • Simulating heat transfer within a fluid
  • Simulating heat transfer between a fluid and a solid (conjugate heat transfer)
  • Creation of a new material model
  • Modeling of surfaces shared between solid and fluid volumes
  • Propagation (copying) of settings from one surface group to another

Prerequisites

You should have already run through the introductory tutorial, ACU-T: 2000 Turbulent Flow in a Mixing Elbow. It is assumed that you have some familiarity with AcuConsole, AcuSolve, and AcuFieldView. You will also need access to a licensed version of AcuSolve.

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

Analyze the Problem

An important first step in any CFD simulation is to examine the engineering problem to be analyzed and determine the settings that need to be provided to AcuSolve. Settings can be based on geometrical components (such as volumes, inlets, outlets, or walls) and on flow conditions (such as fluid properties, velocity, or whether the flow should be modeled as turbulent or as laminar).

The problem to be addressed in this tutorial is shown schematically in Figure 1. It consists of a mixing elbow made of stainless steel with water entering through two inlets with different velocities and with different temperatures. The geometry is symmetric about the XY midplane of the pipe, as shown in the figure. This symmetry allows the flow to be modeled with the use of a symmetry plane. The use of a symmetry plane leads to reduced computation time while still providing an accurate solution.



Figure 1. Schematic of Mixing Elbow with Stainless-steel Walls

Details of the problem characteristics are shown in the following images extracted from a sample worksheet that was created prior to setting up the case for AcuSolve.

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.



Figure 2.

The fluid in this problem is water, with the following properties that do not change with temperature; a density (ρ) of 1000 kg/m3, a molecular viscosity (μ) of 1 X 10-3 kg/m-sec, a conductivity (k) of 0.598 W/m-K, and a specific heat (cp) of 4183 J/kg-K, as shown in the worksheet.



Figure 3.

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.



Figure 4.

Based on mass conservation, the combined flow rate (Q) yields a velocity of 0.475 m/s downstream of the small inlet. This value is useful in determining the Reynolds number, which in turn can be used to determine if the flow should be modeled as turbulent, or if it should be modeled as laminar.



Figure 5.
In order to determine whether the modeled flow would be turbulent or whether it would be laminar, the Reynolds number (Re) should be calculated. The Reynolds number is given by: (1) Re= ρVD μ MathType@MTEF@5@5@+= feaagKart1ev2aaatCvAUfeBSjuyZL2yd9gzLbvyNv2CaerbuLwBLn hiov2DGi1BTfMBaeXatLxBI9gBaerbd9wDYLwzYbItLDharqqtubsr 4rNCHbGeaGqiVu0Je9sqqrpepC0xbbL8F4rqqrFfpeea0xe9Lq=Jc9 vqaqpepm0xbba9pwe9Q8fs0=yqaqpepae9pg0FirpepeKkFr0xfr=x fr=xb9adbaqaaeGaciGaaiaabeqaamaabaabaaGcbaGaciOuaiaacw gacqGH9aqpdaWcaaqaaiabeg8aYjaadAfacaWGebaabaGaeqiVd0ga aaaa@3DE7@ where ρ is the fluid density, v is the fluid velocity, D is the diameter of the flow region, and μ is the molecular viscosity of the fluid. When the Reynolds number is above 4,000, it is generally accepted that flow should be modeled as turbulent.

The Reynolds numbers of 40,000 at the large inlet, 30,000 at the small inlet, and 47,500 for the combined flow indicate that the flow is turbulent throughout the flow domain.



Figure 6.

The simulation will be set up to model steady state, turbulent flow with varying temperature. In addition, the thermal characteristics of the flow will be modeled using advection and diffusion equations.



Figure 7.

In addition to setting appropriate conditions to capture the physics of the simulation, it is important to generate a mesh that is sufficiently refined to provide good results. In this tutorial the global mesh size is set to provide at least 30 mesh elements around the circumference of the large inlet. For this problem, the global mesh size is 0.0106 m. This mesh size was chosen to provide a quick turnaround time for the model. For real-world simulations, you would modify your mesh settings after an initial solution until a mesh-independent solution is reached (that is, a solution that does not change with further mesh refinement).



Figure 8.

AcuSolve allows for mesh refinements in a user-defined region that is independent of geometric components of the problem such as volumes, model surfaces, or edges. It is useful to refine the mesh in areas where gradients in pressure, velocity, eddy viscosity, and the like are steep. For this problem, the flow entering the large pipe from the side pipe creates large velocity gradients that need to be resolved. A mesh refinement zone is used to capture the flow in this region.



Figure 9.

Once a solution is calculated, the flow properties of interest are the steady state temperature contours on the symmetry plane, velocity vectors on the symmetry plane, temperature contours on the pipe walls, and temperature contours at the pipe outlet.

Define the Simulation Parameters

Start AcuConsole and Create the Simulation Database

In this tutorial, you will begin by creating a database, populating the geometry-independent settings, loading the geometry, creating groups, setting group attributes, adding geometry components to groups, and assigning mesh controls and boundary conditions to the groups. Next you will generate a mesh and run AcuSolve to converge on a steady state solution. Finally, you will visualize the results using AcuFieldView.

In the next steps you will start AcuConsole, create the database for storage of AcuConsole settings and set the location for saving mesh and solution information for AcuSolve.

  1. Start AcuConsole from the Windows Start menu by clicking Start > Altair <version> > AcuConsole.
  2. Click the File menu, then click New to open the New data base dialog.
    Note: You can also open the New data base dialog by clicking on the toolbar.
  3. Browse to the location that you would like to use as your working directory.
    This directory is where all files related to the simulation will be stored. The AcuConsole database file (.acs) is stored in this directory. Once the mesh and solution are created, additional files and directories will be created within this directory.
  4. Create a new folder named Mixing_Elbow_Heat and open this folder.
  5. Enter Mixing_Elbow_Heat as the File name for the database.
    Note: In order for other applications to be able to read the files written by AcuConsole, the database path and name should not include spaces.
  6. Click Save to create the database.

Set General Simulation Parameters

In the next steps you will set parameters that apply globally to the simulation. To simplify this task, you will use the BAS filter in the Data Tree Manager. The BAS filter limits the options in the Data Tree to show only the basic settings.

The general parameters that you will set for this tutorial are for turbulent flow, steady state time analysis and for thermal analysis using advection-diffusion equations.

  1. Click BAS in the Data Tree Manager to switch to basic view in the Data Tree.


    Figure 10.
  2. Double-click the Global Data Tree item to expand it.
    Tip: You can also expand a tree item by clicking next to the item name.


    Figure 11.
  3. Double-click Problem Description to open the Problem Description detail panel.
    Tip: You can also open a panel by right-clicking a tree item and clicking Open on the context menu.
  4. Enter Introductory Tutorial as the Title for this case.
  5. Enter Mixing Elbow – Turbulent with conjugate heat transfer as the Sub title for this case.
  6. Accept the default Analysis type of Steady State.
  7. Set the Temperature equation to Advective Diffusive.
  8. Set the Turbulence equation to Spalart Allmaras.
    The robustness and accuracy of the Spalart-Allmaras turbulence model makes it an excellent choice for simulation of steady state flows.


    Figure 12.

Set Solution Strategy Parameters

In the next steps you will set the parameters that control the behavior of AcuSolve as it progresses during the solution.

  1. Double-click Auto Solution Strategy to open the Auto Solution Strategy detail panel.
  2. Enter 0.4 for the Relaxation factor.
    The relaxation factor is used to improve convergence of the solution. Typically a value between 0.2 and 0.4 provides a good balance between achieving a smooth progression of the solution and the extra compute time needed to reach convergence. Higher relaxation factors cause AcuSolve to take more time steps to reach a steady state solution. A high relaxation factor is sometimes necessary in order to achieve convergence for very complex applications.


    Figure 13.

Set Material Model Parameters

AcuConsole has three pre-defined materials, Air, Aluminum and Water.

In the next steps you will verify that the pre-defined material properties of water match the desired properties for this problem. You will also create a new material, stainless steel, and set the desired material properties.



Figure 14.
  1. Double-click Material Model in the Data Tree to expand it.
  2. Double-click Water in the Data Tree to open the Water detail panel.
    The Material type for water is Fluid. The default material type for any new material created in AcuConsole is Fluid.
  3. Click the Density tab. Verify that the density of water is 1000.0 kg/m3.
  4. Click the Specific Heat tab. Verify that the specific heat of water is 4183.0 J/kg-K.
  5. Click the Viscosity tab. Verify that the viscosity of water is 0.001 kg/m-sec.
  6. Click the Conductivity tab. Verify that the conductivity of water is 0.598 W/m-K.
  7. Create a new material model for stainless steel.


    Figure 15.
    1. Right-click Material Model in the Data Tree.
    2. Click New.
  8. Rename the new material.
    1. Right-click Material Model 1 in the Data Tree.
    2. Click Rename.
    3. Type Stainless Steel and press Enter.
  9. Double-click Steel in the Data Tree to open the Stainless Steel detail panel.
  10. Change the Material type to solid.
    1. Click the drop-down control next to Material Type.
    2. Click Solid.
  11. Set the density to be used for stainless steel in this simulation.
    1. Click the Density tab.
    2. Enter 8030 for Density.
    3. Verify that the units are kg/m3.
  12. Set the specific heat of steel for this simulation.
    1. Click the Specific Heat tab.
    2. Enter 500 for Specific heat.
    3. Verify that the units are J/kg-K.
  13. Set the conductivity of steel for this simulation.
    1. Click the Conductivity tab.
    2. Enter 16.2 for Conductivity.
    3. Verify that the units are W/m-K.
  14. Save the database to create a backup of your settings. This can be achieved with any of the following methods.
    • Click the File menu, then click Save.
    • Click on the toolbar.
    • Click Ctrl+S.
    Note: Changes made in AcuConsole are saved into the database file (*.acs) as they are made. A save operation copies the database to a backup file, which can be used to reload the database from that saved state in the event that you do not want to commit future changes.

Import the Geometry and Define the Model

Import the Geometry

You will import the geometry in the next part of this tutorial. You will need to know the location of mixingElbowHeat.x_t in order to complete these steps. This file contains information about the geometry in Parasolid ASCII format.
  1. Click File > Import.
  2. Browse to the directory containing mixingElbowHeat.x_t.
  3. Change the file name filter to Parasolid File (*.x_t *.xmt *X_T …).
  4. Select mixingElbowHeat.x_t and click Open to open the Import Geometry dialog.


    Figure 16.

    For this tutorial, the default values for the Import Geometry dialog are used to load the geometry. If you have previously used AcuConsole, be sure that any settings that you might have altered are manually changed to match the default values shown in the figure. With the default settings, volumes from the CAD model are added to a default volume group. Surfaces from the CAD model are added to a default surface group. You will work with groups later in this tutorial to create new groups, set flow parameters, add geometric components, and set meshing parameters.

  5. Click Ok to complete the geometry import.


    Figure 17.

    The color of objects shown in the modeling window in this tutorial and those displayed on your screen may differ. The default color scheme in AcuConsole is "random," in which colors are randomly assigned to groups as they are created. In addition, this tutorial was developed on Windows. If you are running this tutorial on a different operating system, you may notice a slight difference between the images displayed on your screen and the images shown in the tutorial.

Create a Volume Group and Apply Volume Parameters

Volume groups are containers used for storing information about volumes. This information includes the list of geometric volumes associated with the container, as well as parameters such as material models and mesh sizing information.

When the geometry was imported into AcuConsole, all volumes were placed into the "default" volume container.

In the next steps you will create a new group for the steel wall volume; set the material for that group; add the volumes from the geometry to that volume group; rename the default volume group to Fluid and set the material for that group; then add the volumes from the geometry to that group.

  1. Expand the Model tree item.
  2. Expand Volumes.
  3. Toggle the display of the default volume container by clicking and next to the volume name.
    Note: You may not see any change when toggling the display if Surfaces are being displayed, as surfaces and volumes may overlap.
  4. Create a new volume group for the steel pipe walls.
    1. Right-click Volumes.
    2. Click New.
  5. Right-click Volume 1, select Rename and enter Steel Walls .
    Note: When an item in the Data Tree is renamed, the change is not saved until you press Enter. If you move the input focus away from the item without entering it, your changes will be lost.
  6. Set the material model for the volume to use the Stainless Steel.
    1. Expand the Steel Walls volume in the tree.
    2. Double-click Element Set to open the Element Set detail panel.
    3. Change the Medium to Solid to define this volume as a solid.
    4. For Material model, click Stainless Steel.


    Figure 18.
  7. Add the pipe wall components in the geometry to this volume group.
    1. Right-click Steel Walls under Volumes in the Data Tree.
    2. Click Add to.
    3. Click the outer surface of the pipe wall.
      If you rotate the view, by Ctrl + left-clicking, you can see that only the outer volume is highlighted.


      Figure 19.
    4. Click Done to add this geometry volume to the Steel Walls volume group.
      Note: You can also use the middle mouse button to complete the addition of geometry components to a group.
  8. Rename the default volume to Fluid.

    When the geometry was loaded into AcuConsole, all geometry volumes were placed in the default volume group. In the previous steps, you selected a geometry volume to be added to the Steel volume container that you created. At this point, all that is left in the default volume group is the fluid volume. Rather than create a new container, add the fluid volume in the geometry to it, and then delete the default volume container, you will rename the container and modify the attributes for this group.

  9. Set the material model used for the fluid in the simulation.
    1. Expand the Fluid volume in the tree.
    2. Double-click Element Set to open the Element Set detail panel.
      Note: The default Medium for a volume in AcuConsole is Fluid.
    3. Click the drop-down control next to Material model.
    4. Click Water to set this material model for the fluid.


    Figure 20.

Create Surface Groups and Apply Surface Attributes

Surface groups are containers used for storing information about a surface. This information includes the list of geometric surfaces associated with the container, as well as attributes such as boundary conditions, surface outputs, and mesh sizing information.

In the next steps you will define surface groups, assign the appropriate attributes for each group in the problem, and add surfaces to the groups.

Set Inflow Boundary Conditions for the Large Inlet

In the next steps you will define a surface group for the large inlet, set the inlet velocity, and add the main inlet from the geometry to the surface group.



Figure 21.
  1. Create a new surface group.
    1. Right-click Surfaces in the Data Tree.
    2. Click New.
  2. Rename Surface 1 to Large Inlet.
  3. Expand the Large Inlet surface in the tree.
  4. Double-click Simple Boundary Condition under Large Inlet to open the Simple Boundary Condition detail panel.
  5. Change the Type to Inflow.
  6. Change the Inflow type to Average Velocity.
    This type of boundary condition is used by AcuSolve to approximate a fully developed flow with a given average velocity.
  7. Set the Average velocity to 0.4 m/sec.
  8. Set the Temperature to 295 K.


    Figure 22.
  9. Add a geometry surface to the Large Inlet group.
    1. Right-click Large Inlet and click Add to.
    2. Click on the large inlet face.


      Figure 23.

      At this point, the inlet should be highlighted.

    3. Click Done to add this geometry surface to the Large Inlet surface group.
      Note: You can also use the middle mouse button to complete the addition of geometry components to a group.

Set Inflow Boundary Conditions for the Small Inlet

In the next steps you will define a surface group for the small inlet, assign the appropriate attributes, and add the small inlet from the geometry to the surface group.



Figure 24.
  1. Create a new surface group and rename the surface to Small Inlet.
  2. Expand the Small Inlet surface in the tree.
  3. Double-click Simple Boundary Condition under Small Inlet to open the Simple Boundary Condition detail panel.
  4. Change the Type to Inflow.
  5. Change the Inflow type to Average Velocity.
  6. Set the Average velocity to 1.2 m/sec.
  7. Set the Temperature to 320 K.


    Figure 25.
  8. Add a geometry surface to the Small Inlet group.
    1. Right-click Small Inlet and click Add to.
    2. Rotate the model to expose the small inlet by Ctrl+left-clicking near the bottom of the geometry and moving the cursor toward the top of the window.
      Note: If you need to zoom in or out, Ctrl+right-click and drag the cursor down or up. You can also restore the initial view by clicking .
    3. Left-click on the small inlet face.


      Figure 26.

      At this point, the small inlet should be highlighted.

    4. Click Done to add this geometry surface to the Small Inlet group.

Set Outflow Boundary Conditions for the Outlet

In the next steps you will define a surface group for the outlet, assign the appropriate attributes and add the outlet from the geometry to the surface group.

  1. Create a new surface group and rename the surface to Outlet.
  2. Expand the Outlet surface in the tree.
  3. Double-click Simple Boundary Condition under Outlet to open the Simple Boundary Condition detail panel.
  4. Change the Type to Outflow.


    Figure 27.
  5. Add a geometry surface to the Outlet surface container.
    1. Right-click Outlet and click Add to.
    2. Rotate the model to expose the outlet by Ctrl+left-clicking near the top of the geometry and moving the cursor toward the bottom of the window.
    3. Click on the outlet face.


      Figure 28.

      At this point, the outlet should be highlighted.

    4. Click Done to associate this geometry surface with the surface settings of the Outlet group.

Set Wall Boundary Conditions for the Steel Pipe Outer Walls

In the next steps you will define a surface group for the steel pipe outer walls, assign the appropriate attributes and add the pipe walls from the geometry to the surface group. In this simulation, you will not be modeling the air surrounding the pipe. However, you will specify a convective heat transfer coefficient and reference temperature to account for heat transfer from the pipe walls to the surroundings.

  1. Create a new surface group and rename the surface to Steel Pipe - Outer Walls.
  2. Double-click Simple Boundary Condition under Steel Pipe - Outer Walls to open the Simple Boundary Condition detail panel.
  3. Enter 100 for the Convective heat flux coefficient and verify that the units are J/m2-sec-K.
    This convective heat transfer coefficient is chosen to model the heat transfer between the steel pipe and the surrounding air.
  4. Enter 302.594 for the Convective heat flux reference temperature and verify that the units are K.
    This temperature value specifies that the surroundings of the pipe are at a constant temperature of 302.594 K.


    Figure 29.
  5. Add a geometry surface to the Steel Pipe - Outer Walls group.
    1. Right-click Steel Pipe - Outer Walls and click Add to.


      Figure 30.

      At this point, the outer pipe walls should be highlighted.

    2. Click Done to associate these geometry surfaces with the surface settings of the Steel Pipe - Outer Walls group.

Set Boundary Conditions for the Steel Pipe Inner Walls

In the next steps you will define a surface group for the steel pipe inner wall, assign the appropriate attributes, and add the pipe walls from the geometry to the surface group.

  1. Create a new surface group and rename the surface to Steel Pipe - Inner Walls.
  2. Disable boundary conditions for this surface.
    For this simulation, no boundary conditions will be used for the inner surface of the steel pipe. Where there is an interface between two volumes (fluid/solid or fluid/fluid), AcuConsole treats the interface as two surfaces. This allows you to set different attributes, such as boundary conditions or local meshing attributes, on either side of the interface. You will set boundary conditions for the large pipe wall (the second surface at this interface) later in this tutorial.
    1. Expand the Steel Pipe - Inner Walls surface in the tree.
    2. Click the check box next to Simple Boundary Condition to disable boundary conditions.
  3. Turn off the display of the Steel Pipe - Outer Walls.
    • Click next to the surface so that it is in the display off state (),

      or,

    • Right-click Steel Pipe - Outer Walls in the tree, and click Display off.
    Turning off the display of the outer walls will make it easier to add geometric surfaces to the inner wall group.
  4. Add geometry surfaces to the Steel Pipe - Inner Walls group.
    1. Right-click Steel Pipe - Inner Walls and click Add to.
    2. Click the pipe near the main inlet, the pipe near the elbow, the pipe near the outlet, and the pipe near the side inlet to select the four surfaces that make up the inner surface of the steel pipe wall.


      Figure 31.

      At this point, the inner walls of the steel pipe should be highlighted.

    3. Click Done to associate these geometry surfaces with the surface settings of the Steel Pipe - Inner Walls group.

Set Wall Boundary Conditions for the Large Pipe

In the next steps you will define a surface group for the pipe walls, assign the appropriate attributes, and add the elbow pipe walls from the geometry to the surface group.

  1. Create a new surface group and rename the surface to Large Pipe.
  2. Expand the Large Pipe surface in the tree.
  3. Double-click Simple Boundary Condition under Large Pipe to open the Simple Boundary Condition detail panel.
    The default wall settings will be used for the pipe wall.
  4. Turn off the display of the Steel Pipe - Inner Walls.
    Turning off the display of the inner walls of the steel pipe will make it easier to add geometric surfaces to the pipe group.
  5. Add geometry surfaces to this group.
    1. Right-click Large Pipe and click Add to.
    2. Click on the pipe near the large inlet, the pipe near the elbow, and the pipe near the outlet to select the three surfaces that make up the main pipe wall.


      Figure 32.

      At this point, the pipe walls should be highlighted.

    3. Click Done to add these geometric surfaces to the Large Pipe group.

Set Wall Boundary Conditions for the Small Pipe

In the next steps you will define a surface group for the side pipe wall, assign the appropriate parameters, and add the side pipe wall from the geometry to the surface group.

  1. Create a new surface group and rename the surface to Small Pipe.
  2. Expand the Small Pipe surface in the tree.
  3. Double-click Simple Boundary Condition under Small Pipe to open the Simple Boundary Condition detail panel.
    As with the large pipe, the default boundary condition Type is Wall. The default is appropriate for this group and no other changes are needed.
  4. Add geometry surfaces to this group.
    1. Right-click Small Pipe and click Add to.
    2. Rotate the model to expose the side pipe by Ctrl+left-clicking near the bottom of the geometry and moving the cursor toward the top of the window.
    3. Click on the pipe near the side inlet.


      Figure 33.

      At this point, the side pipe wall should be highlighted.

    4. Click Done to associate this geometry surface with the Small Pipe surface container.

Set Symmetry Boundary Conditions for the Pipe Symmetry Plane

This geometry is symmetric about the XY midplane, and can therefore be modeled with half of the geometry. In order to take advantage of this, the midplane needs to be identified as a symmetry plane. The symmetry boundary condition enforces constraints such that the flow field from one side of the plane is a mirror image of that on the other side.

In the next steps you will create a surface group for the symmetry plane of the pipe, assign the appropriate attributes, and add the side pipe wall from the geometry to the surface group.
  1. Create a new surface group and rename it to Symmetry.
  2. Expand the Symmetry surface in the tree.
  3. Double-click Simple Boundary Condition under Symmetry to open the Simple Boundary Condition detail panel.
  4. Change the Type to Symmetry.
  5. Turn off the display of all surface items except Symmetry and default.
  6. Add geometric faces to this group.
    1. Right-click Symmetry and click Add to.
    2. Click on the Symmetry plane.


      Figure 34.

      At this point, the symmetry plane should be highlighted.

    3. Click Done to associate this geometry surface with the Symmetry surface container.

Set Boundary Conditions for the Steel Pipe Ends

In the next steps you will define a surface group for the ends of the steel pipe, assign the appropriate attributes, and add the pipe ends from the geometry to the surface group.

  1. Create a new surface group and rename it to Steel Pipe - Ends.
  2. Expand the Steel Pipe - Ends surface in the tree.
  3. Disable boundary conditions for this surface.

    No boundary conditions will be used for the pipe ends for this simulation. AcuSolve will treat the steel wall as if it continues beyond the regions modeled.

  4. Turn off the display of all surface items except Steel Pipe - Ends and default.
  5. Add geometric faces to this group.
    1. Right-click Steel Pipe - Ends and click Add to.
    2. Click on the pipe ends at the large inlet, the small inlet, and the outlet.
      Note: You may need to rotate the graphic to see that the pipe end at the large inlet is highlighted.


      Figure 35.

      At this point, the pipe ends should be highlighted.

    3. Click Done to associate these geometry surfaces with the Steel Pipe - Ends surface container.

Set Symmetry Boundary Conditions for the Steel Pipe Symmetry Plane

  1. Rename the default surface group to Steel Pipe - Symmetry.
  2. Expand the Steel Pipe - Symmetry surface in the tree.
  3. Double-click Simple Boundary Condition under Steel Pipe - Symmetry to open the Simple Boundary Condition detail panel.
  4. Change the Type to Symmetry.
  5. Save the database to create a backup of your settings.

Assign Mesh Controls

Set Global Meshing Parameters

Now that the simulation has been defined, parameters need to be added to define the mesh sizes that will be created by the mesher.

AcuConsole supports three levels of meshing control; global, zone, and geometric.
  • Global mesh controls apply to the whole model without being tied to any geometric component of the model.
  • Zone mesh controls apply to a defined region of the model, but are not associated with a particular geometric component.
  • Geometric mesh controls are applied to a specific geometric component. These controls can be applied to volume groups, surface groups, or edge groups.

In the next steps you will set global meshing parameters. In subsequent steps you will create zone and surface meshing parameters.



Figure 36.
  1. Click MSH in the Data Tree Manager to filter the settings in the Data Tree to show only the controls related to meshing.
  2. Expand the Global Data Tree item.
  3. Double-click Global Mesh Attributes to open the Global Mesh Attributes detail panel.
  4. Change the Mesh size type to Absolute.
  5. Enter 0.0106 m for the Absolute mesh size.
    This absolute mesh size is chosen to ensure that there are at least 30 mesh elements around the circumference of the main pipe.
  6. Turn off the Curvature refinement parameters option.


    Figure 37.

Set Zone Meshing Parameters

In addition to setting meshing characteristics for the whole problem, you can assign meshing parameters to a zone within the problem where you want to be able to resolve flow with a mesh that is more refined than the global mesh. A zone mesh refinement can be created using basic shapes to control the mesh size within that shape. These types of mesh refinement are used when refinement is needed in an area that does not correspond to a geometric item.

In the next steps you will define mesh controls for a region around the small pipe and extending into the main pipe by using a zone mesh control. The region of interest for this refinement is a cylinder that encloses the small pipe and extends into the main pipe.



Figure 38.
  1. Turn off the display of Volumes.
  2. Turn off the display of all surfaces except Symmetry.
  3. Restore the initial view by clicking on the View Manager toolbar.
  4. Right-click Zone Mesh Attributes under the Global branch in the Data Tree and click New.
  5. Rename Zone Mesh Attributes 1 to Small pipe refinement.
  6. Double-click Small pipe refinement to open the Zone Mesh Attributes detail panel.
  7. Change the Mesh zone type to Cylinder.
  8. Enter 0.0254 m for the Radius.
    This radius is used to define a cylinder that is larger than the small inlet.
  9. Enter 0.0053 m for the Mesh size.
    This will result in a zone where the mesh size is half of the mesh size in the rest of the pipe.


    Figure 39.
    Note: When setting mesh size for refinement zones, the best practice is to choose a value that is the global mesh size divided by a power of 2, that is, 1/2, 1/4, 1/8, and the like.
  10. Set the location of the mesh refinement by defining the center points of the end faces of the cylinder.
    1. Click Open Array to open the Array Editor dialog.
    2. Enter 0.143 for X-coordinate 1 and 2.
    3. Enter -0.232 for Y-coordinate 1.
    4. Enter -0.025 for Y-coordinate 2.
    5. Enter 0.0 for Z-coordinate 2.
    6. Click OK.


      Figure 40.


    Figure 41.

Set Meshing Attributes for Surface Groups

In the following steps you will set meshing attributes that will allow for localized control of the mesh size on surface groups that you created earlier in this tutorial. Specifically, you will set local meshing attributes that control the growth of boundary layer elements normal to the surfaces of the main pipe and of the side pipe.

Set Meshing Parameters for the Large Pipe

In the next steps you will set parameters that control the mesh size normal to the large pipe wall (boundary layer mesh controls).
  1. Expand the Model > Surfaces > Large Pipe tree item.
  2. Click the check box next to Surface Mesh Attributes to enable the settings and open the Surface Mesh Attributes detail panel.
  3. Change the Mesh size type to None.
    This option indicates that the mesher will use the global meshing attributes when creating the mesh on the surface of the pipe walls.
  4. Turn on the Boundary layer flag option.
    This option allows you to define how the meshing should be handled in the direction normal to the walls.
  5. Set the Resolve option to Total Layer Height.
    Mesh elements for a boundary layer are grown in the normal direction from a surface to allow effective resolution of the steep gradients near no-slip walls. The layers can be specified using a number of different options. In this tutorial you will specify the height of the first layer, a stretch ratio for successive layers (growth rate), and the total number of layers to generate. AcuConsole will resolve the total layer height from the attributes that you provide. That is, total layer height will be computed based on the height of the first element, the growth rate, and the number of layers that you provide in the next few steps.
  6. Keep the default value, 0.001 m, for First element height
  7. Enter 1.3 for the Growth rate.
  8. Enter 4 for the Number of layers.


    Figure 42.

Propagate Meshing Parameters to the Small Pipe

The local mesh settings for the small pipe are the same as for the large pipe. AcuConsole has the capability to propagate, or "copy and paste," settings from one group to another. In the following steps you will propagate the local mesh settings from the large pipe surface group to the small pipe surface group.

  1. Right-click Surface Mesh Attributes under Large Pipe and click Propagate.
  2. Scroll down the list of surfaces and click Small Pipe.


    Figure 43.
  3. Click Propagate to paste the settings for the Large Pipe surface to the Small Pipe surface.
If you examine the Surface Mesh Attributes for the Small Pipe, you will see that the settings are the same as those for the Large Pipe.

Set Meshing Parameters for the Steel Pipe Outer Walls

In the following steps you will set meshing parameters that will allow for localized control of the mesh size near the outer walls of the steel pipe.

  1. Expand the Model > Surfaces > Steel Pipe - Outer Walls tree item.
  2. Click the check box next to Surface Mesh Attributes to enable the settings and open the Surface Mesh Attributes detail panel.
  3. Change the Mesh size type to None.
    This option indicates that the mesher will use the global meshing parameters when creating the mesh on the surface of the pipe walls.
  4. Turn on the Boundary layer flag option.
    This option allows you to define how the meshing should be handled in the direction normal to the walls. For the inner and outer walls of the steel pipe, you will set parameters to create a mesh one layer thick with a height of 0.002 m.
  5. Set the Resolve option to Total Layer Height.
  6. Enter 0.002 m for First element height.
  7. Enter 1 for the Number of layers.


    Figure 44.

Propagate Meshing Attributes to the Steel Pipe Inner Walls

The local mesh settings for the inner walls of the pipe are the same as for the outer walls. In the following steps you will propagate the local mesh settings from the surface group containing the steel pipe outer walls to the surface group containing the steel pipe inner walls.

  1. Right-click Surface Mesh Attributes under Steel Pipe - Outer Walls and click Propagate.
  2. Scroll down the list of surfaces and click Steel Pipe - Inner Walls.
  3. Click Propagate to paste the settings for the Steel Pipe - Outer Walls surface to the Steel Pipe - Inner Walls surface.
    If you examine the Surface Mesh Attributes for the Steel Pipe - Inner Walls, you will see that the settings are the same as those for the Steel Pipe - Outer Walls.
  4. Save the database to create a backup of your settings.

Generate the Mesh

In the next steps you will generate the mesh that will be used when computing a solution for the problem.

  1. Click on the toolbar to open the Launch AcuMeshSim dialog.
  2. Click Ok to begin meshing.

    During meshing an AcuTail window opens. Meshing progress is reported in this window. A summary of the meshing process indicates that the mesh has been generated.



    Figure 45.
  3. Display the mesh on surfaces.
    1. Right-click Zone Mesh Attributes under Global in the Data Tree and click Display off.
    2. Right-click Volumes in the Data Tree and click Display off.
    3. Right-click Surfaces in the Data Tree and click Display on.
    4. Right-click Surfaces in the Data Tree, select Display type and click solid & wire.
  4. Rotate, move, or zoom the view to examine the mesh.
  5. Turn off the display of small pipe refinement under Global > Zone Mesh Attributes by clicking next to the surface so that it is in the display off state ().

    Details of the mesh on the side pipe are shown in Figure 46. This view was obtained by turning off the display of all surfaces except Symmetry and Steel Pipe - Symmetry, then zooming in on the region where the small pipe joins the large pipe.



    Figure 46. Mesh Details Around the Pipe Intersection Viewed on the Symmetry Plane

    Note that the mesh size in the main pipe decreases from left to right in the transition from a region where global settings determine the size to the zone around the small pipe where the settings are for a finer mesh.

  6. Save the database to create a backup of your settings.

Compute the Solution and Review the Results

Run AcuSolve

In the next steps you will launch AcuSolve to compute the solution for this case.

  1. Click on the toolbar to open the Launch AcuSolve dialog.

    For this case, the default values will be used.

    Based on these settings, AcuConsole will generate the AcuSolve input files, then launch the solver. AcuSolve will run using four processors to calculate the steady state solution for this problem.

  2. Click Ok to start the solution process.

    While computing the solution, an AcuTail window opens. Solution progress is reported in this window. A summary of the solution process indicates that the run has been completed.

    The information provided in the summary is based on the number of processors used by AcuSolve. If you use a different number of processors than indicated in this tutorial, the summary for your run may be slightly different than the summary shown.



    Figure 47.
  3. Close the AcuTail window and save the database to create a backup of your settings.

View Results with AcuFieldView

Now that a solution has been calculated, you are ready to view the flow field using AcuFieldView. AcuFieldView is a third-party post-processing tool that is tightly integrated toAcuSolve. AcuFieldView can be started directly from AcuConsole, or it can be started from the Start menu, or from a command line. In this tutorial you will start AcuFieldView from AcuConsole after the solution is calculated by AcuSolve.

In the next steps you will start AcuFieldView, manipulate the view of the model, display temperature contours and velocity vectors on the symmetry plane, display temperature contours on the pipe wall symmetry plane and display temperature contours at the outlet.

Start AcuFieldView

  1. Click on the AcuConsole toolbar to open the Launch AcuFieldView dialog.
  2. Click Ok to start AcuFieldView.
    When you start AcuFieldView from AcuConsole, the results from the last time step of the solution that were written to disk will be loaded for post-processing.

Manipulate the Model View in AcuFieldView

When AcuFieldView is started directly from AcuConsole, the model will be displayed in an isometric view with a Boundary Surface dialog open. The initial view is shown in perspective, with an outline around the model. You will manipulate the view in the next steps, and in later steps will view different flow characteristics using the Boundary Surface dialog.



Figure 48.
  1. Change the background color to white.
    1. Click on the View menu.
    2. Click Background / Environment.
    3. Click the white swatch, then click Close.


      Figure 49.
  2. Turn off the display of the outline around the model by clicking on the toolbar.
  3. Change the view from perspective to orthographic.
    1. Click on the View menu.
    2. Click Perspective to disable this option.


    Figure 50.
  4. Orient the model to view it from the positive Z direction (+Z).
    1. Click on the toolbar to open the Defined Views dialog.
    2. Click .

      You will see the view change as soon as you click a button in the Defined Views dialog.

    3. (Optional) Close the dialog.

    You can move, zoom, and rotate the view in AcuFieldView in a similar fashion as in AcuConsole. AcuFieldView uses a different mapping for mouse-button actions.

    Action Mouse Button
    move (pan) left
    rotate middle
    zoom right

Display Contours of Fluid Temperature on the Symmetry Plane

In the next steps you will create a boundary surface to display contours of fluid temperature on the symmetry plane.

  1. Click to open the Boundary Surface dialog.
    Note: The dialog may already be open. This step will put the focus on the dialog.
  2. Disable the Show Mesh option.
  3. Set temperature as the scalar property to display.
    1. Click Select in the Scalar Function control group to open the Function Selection dialog.
    2. Select temperature from the list.
    3. Click Calculate.
  4. Set the symmetry plane as the location for display of the contours.
    1. Click OSF: Symmetry in the list of Boundary Types.
    2. Click OK.


    Figure 51.
  5. Add a legend to the view.
    1. Click the Legend tab in the Boundary Surface dialog.
    2. Enable the Show Legend option.
    3. Enable the Frame option.
    4. Click the white color swatch next to Geometric in the Color group and set the color for the legend values to black.
    5. Click the white color swatch next to the Title field and set the color for the title to black.
    6. Move the legend by Shift+left-clicking and dragging the legend to the left.


    Figure 52.

Add Velocity Vectors to the View

In the next steps you will create a new boundary surface and display velocity vectors on that surface.

  1. Click Create on the Surface tab of the Boundary Surface dialog.
    The new Surface ID will be 2.
  2. Click the Geometric radio button in the Coloring group.
    This sets the color of the vectors to a constant color. By default, the color is black.
  3. Set vector options.
    1. Click the Vectors radio button.
    2. Click Options next to Vectors to open the Vector Options dialog.
    3. Enable Head Scaling and set it to 0.5.
      This option determines the size of the arrow head compared to the vector.
    4. Set the Length Scale to 2.
      The length scale determines the length of the vectors.
    5. Enable the Skip option and set it to 37.5%.
      The Skip option determines the percentage of vectors to skip from being displayed. The setting of 37.5% will result in 62.5% of the vectors being displayed.


      Figure 53.
    6. Close the dialog.
  4. Set the symmetry plane as the location for display of the vectors.
    1. Click OSF: Symmetry in the list of Boundary Types.
    2. Click OK.


    Figure 54.
  5. Zoom in on the junction of the small inlet with the main pipe to view details of velocity vectors.
    1. Click on the toolbar.
    2. Draw a box around the junction of the two pipes.


    Figure 55.
    Note: The Show Legend option for the temperature contour (Surface ID 1) is disabled in order to capture this image.
    The velocity vectors indicate the direction of flow. The vector length indicates the magnitude of the flow velocity. Adding velocity vectors to a view with temperature contours allows you to visualize temperature and velocity simultaneously.

Display Contours of Temperature on the Steel Pipe Walls

In the next steps you will create a boundary surface to display contours of temperature on the stainless steel pipe walls at the symmetry plane.

  1. Click on the Transform Controls toolbar to center the visible surfaces and to fit the view in the window.
  2. Click to open the Boundary Surface dialog.
    Note: The dialog may already be open. This step will put the focus on the dialog.
  3. Disable the visibility of the temperature contours on the symmetry plane and of the velocity vectors.
    1. Set the Surface ID to 1.
    2. Disable the Visibility option on the Surface tab.
    3. Set the Surface ID to 2.
    4. Disable the Visibility option on the Surface tab.
  4. Click Create on the Surface tab of the Boundary Surface dialog.
    The new Surface ID will be 3.
  5. Enable the Smooth option in the Display Type control group.
  6. Enable the Scalar option in the Coloring control group.
  7. Set temperature as the scalar property to display.
    1. Click Select in the Scalar Function control group to open the Function Selection dialog.
    2. Select temperature from the list.
    3. Click Calculate.
  8. Set the stainless-steel pipe symmetry plane as the location for display of the contours.
    1. Scroll up in the list of Boundary Types and click OSF:Steel Pipe - Symmetry.
    2. Click OK.


    Figure 56.

Display Contours of Temperature at the Outlet

In the next steps you will create a boundary surface to display contours of temperature at the outlet.

  1. Click to open the Boundary Surface dialog.
  2. Click Create on the Surface tab of the Boundary Surface dialog.
    The new Surface ID will be 4.
  3. Enable the Smooth option in the Display Type control group.
  4. Enable the Scalar option in the Coloring control group.
  5. Set temperature as the scalar property to display.
    1. Click Select in the Scalar Function control group to open the Function Selection dialog.
    2. Select temperature from the list.
    3. Click Calculate.
  6. Set the outlet as the location for display of the contours.
    1. Click OSF: Outlet in the Boundary Types list.
    2. Click OK.
  7. Turn off the Visibility option for surfaces 1, 2, and 3.
  8. Orient the view so that you can see the contours on the outlet.
    1. Click on the Transform Controls toolbar.
    2. Set the Viewing Direction to -Y.
    3. Click on the Transform Controls toolbar to center the visible surfaces and to fit the view in the window.


    Figure 57.
  9. Change the color scale to better resolve differences in the temperature contours.
    When the scalar function for temperature is calculated by AcuFieldView, minimum and maximum values are calculated for use in a colormap for the contour display. You can edit the coloring to better resolve differences in the pressure distribution.
    1. Set the Surface ID to 4 in the Boundary Surface dialog.
      Note: You could also make this the current surface by double-clicking the surface in the modeling window.
    2. Click the Colormap tab.


      Figure 58.

      Notice that the Min: and Max: values for the Function Range change when the Local option is toggled.

    3. Enable the Local option.


      Figure 59.

Summary

In this tutorial, you worked through a basic workflow to set up a simulation of conjugate heat transfer in a mixing elbow. Once the case was set up, you generated a mesh and generated a solution using AcuSolve. Results were post-processed in AcuFieldView to allow you to create contour and vector views along the symmetry plane of the model. New features introduced in this tutorial include: flows of different temperatures, simulating heat transfer within a fluid, simulating heat transfer between a fluid and a solid (conjugate heat transfer), creation of a new material model, modeling of shared surfaces at fluid/solid interfaces, and copying and pasting (propagation) of settings from one surface group to another.