# ACU-T: 3000 Enclosed Hot Cylinder: Natural Convection

This tutorial provides the instructions for setting up, solving and viewing results for a simulation of a hot cylinder contained within another air-filled cylinder. In this simulation, an internally heated cylinder is surrounded by air which heats up as it comes in contact with the surface of the inner cylinder. The localized heating near the surface induces a buoyancy driven flow in the air, generating convection currents. This tutorial is designed to introduce you to modeling concepts related to natural convection simulations.

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:
• Creating and specifying a new custom material in AcuConsole
• Specifying a volume group as a heat source
• Using the Boussinesq density model in buoyancy driven flows, such as cases involving natural convection
• Set up periodic boundary conditions
In this tutorial you will do the following:
• Analyze the problem
• Start AcuConsole and create a simulation database
• Set general problem parameters
• Set solution strategy parameters
• Create a new custom material model in AcuConsole and assign material properties to it
• Import the geometry for the simulation
• Create a volume group and apply volume parameters
• Create surface groups and apply surface parameters
• Set global and local meshing parameters
• Set periodic boundary conditions
• Generate the mesh
• Set the appropriate boundary conditions
• Run AcuSolve
• Monitor the solution with AcuProbe
• Post-processing the nodal output with AcuFieldView

## 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 twin_cylinder.x_t from AcuConsole_tutorial_inputs.zip.

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.

## Analyze the Problem

An important step in any CFD simulation is to examine the engineering problem at hand and determine the important parameters that need to be provided to AcuSolve. Parameters can be based on geometrical elements (such as 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 system being simulated contains an internally-heated cylinder, which is surrounded by a cylindrical ring of a larger diameter. The annular volume between the two cylinders is filled with a fluid (air). The inner cylinder thus acts a heat source, and the fluid in contact with the surface of this heat source is heated up. This hot fluid, being lower in density than the cold fluid, then rises up to the upper part of the annulus due to buoyancy effects, and displaces the cold fluid at top. At the same time, the film of fluid which was in contact with the heating surface is replaced by the surrounding cold fluid. This new film of cold fluid goes through the same process until eventually a steady state convection current is achieved, or the inner cylinder ceases to generate heat and slowly the whole system achieves an equal temperature.

The system being simulated can be considered similar to a heat exchanger wherein the inner cylinder is akin to a tube through which a hot fluid passes by, and the air which surrounds this inner tube extracts heat from the inner tube. Another analogy can be of a wire carrying high current enclosed in an air cooled chamber. As the current heats up the wire due to resistance, the air around the wire keeps the wire temperature within control by extracting heat from the wire surface.

The schematics of the problem which will be addressed in this tutorial is shown in Figure 1. The inner cylinder is a solid volume with internal heat generation, and the outer cylinder is a fluid volume with air as the fluid. Both cylinders are assumed to be infinitely long and the system will be modeled using half symmetry and periodicity. The cylinders are infinite in z-direction and hence periodicity will be applied along this direction.

## Introduction to Theory

### Natural Convection

Convection is a heat transfer mechanism where the transfer of heat energy happens through the motion of matter. Since the definition of convection involves motion of matter a fluid state is usually present in convection. Usually this type of heat transfer takes place between a hot or a cold surface and a fluid. The film of fluid in contact with the surface absorbs heat from or transfers heat to the surface and is then replaced by a new film. This movement of fluid may either be governed by an external source, such as a fan or pump, or due to internal changes in the fluid properties. When no external sources are responsible for the fluid motion the heat transfer mechanism at work is called the Natural Convection. The driving force for motion of the fluid in a natural convection is density changes in the fluid due to temperature gradients induced in the fluid by heat transfer.

The natural convection mechanism works similarly as described above, whilst discussion of the problem. The fluid which is in contact with the surface absorbs or transfers heat from the surface and becomes hotter or colder than the surrounding fluid. Driven by buoyancy forces due to difference in densities caused by the temperature gradient, the fluid is displaced upwards or downwards. Surrounding fluid fills in the void created by the displaced fluid, which then undergoes the same process again. This gives rise to a convection current which drives the hot fluid to the top and cold fluid to the bottom of the convection cell. Buoyancy effects are driven by gravity, therefore natural convection requires presence of a gravitational force to work. It must be noted, however, that gravity is not the driving force behind the fluid movement. Presence of gravity only enables displacement of the fluid due to the density changes caused by temperature gradients.

Mathematical determination of the onset of natural convection is done through a dimensionless number called the Rayleigh number (Ra). The Rayleigh number is defined as:

where:
• x is the characteristic length (m)
• $R{a}_{x}$ is the Rayleigh number for characteristic length x
• $g$ is acceleration due to gravity (m/s2)
• ${T}_{s}$ is the surface temperature (K)
• ${T}_{\infty }$ is the quiescent temperature (fluid temperature far from the surface of the object) (K)
• $\nu$ is the kinematic viscosity (m2/s)
• α is the thermal diffusivity (m2/s)
• β is the thermal expansion coefficient (equals to $1/T$ for ideal gases where is absolute temperature).

The fluid properties $\nu$, α and β are evaluated at the film temperature, ${T}_{f}$, which is defined as:

${T}_{f}=\frac{{T}_{s}+{T}_{\infty }}{2}$

When the Rayleigh number is below a critical value for the fluid heat transfer is primarily in the form of conduction. When it exceeds this critical value the dominant heat transfer mechanism is convection.

### Boussinesq Density Model

The Boussinesq density model is an approximation method applied to buoyancy driven flows, such as natural convection flows. In the Boussinesq approximation, the density variation terms are neglected everywhere except when multiplied by acceleration due to gravity, $g$. The basis of this approximation is that since temperature changes are small, the resultant changes in density are small as well and thus can be neglected. However, when multiplied by $g$, the resultant term gives rise to forces which no longer are negligible. The Boussinesq approximation is:

where
• $\rho$ is the instantaneous density at temperature $T$ (kg/m3)
• ${\rho }_{0}$ is the density at reference temperature ${T}_{o}$ (kg/m3)
• $\text{Δ}T$ is change in temperature $T-{T}_{o}$ (K)

As stated in the approximation, the Boussinesq density model is only applicable when density variations are small. A general guideline is to check for the condition to be true. This indirectly puts a limitation on this model to be used to only for cases where expected temperature differences within the fluid are not large.

## 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 volume and surface groups, setting group parameters, 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 solve for the number of time steps specified. Finally, you will visualize some characteristics of the results using AcuFieldView.

In the next steps you will start AcuConsole, and create the database for storage of the simulation settings.

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 directory in this location. Name it Natural_convection and navigate into this directory.
5. Enter NaturalConvection as the file name for the database, or choose any name of your preference.
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 next steps you will set parameters that apply globally to the simulation. To make this simple, the basic settings applicable for any simulation can be filtered using the BAS filter in the Data Tree Manager. This filter enables display of only a small subset of the available items in the data tree and makes navigation of the entries easier.

1. Click BAS in the Data Tree Manager to switch to basic view in the Data Tree.
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.
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 AcuSolve Tutorial as the Title.
5. Enter Natural Convection as the Sub title.
6. Change the Analysis type to Steady State.
7. Change the Temperature equation to Advective Diffusive.

### 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 in the Data Tree to open the Auto Solution Strategy detail panel.
2. Check that Analysis type is set to Steady State.
3. Set the Max time steps to 100.
4. Change the Convergence tolerance to 0.0001.
5. Enter 0.25 for the Relaxation factor.
6. Check that Flow and Temperature are set to On.
7. Change the Temperature flow to On.
Changing the Temperature flow flag to On will instruct the solver to solve thermal-flow problems in fully coupled mode. Otherwise these problems are solved with a staggered strategy. In fully-coupled mode, the flow and temperature equations are solved simultaneously, while in the staggered approach, the flow equation will usually be solved first considering constant temperature, and then the temperature equation will be solved as the next step.

### Set Material Model Parameters

AcuConsole has three pre-defined materials, Air, Aluminum and Water, with standard parameters defined. In the next steps you will check and modify the material characteristics of the predefined Air model to match the desired properties for this problem. Since this a natural convection problem the density type for air will be set to use the Boussinesq approximation. Subsequently, you will create a new custom material and assign relevant material properties to it.
1. Double-click Material Model in the Data Tree to expand it.
2. Double-click Air in the Data Tree to open the Air detail panel.

The material type for air is Fluid. Fluid is the default material type for any new material created in AcuConsole.

3. Click the Density tab. Change the density type to Boussinesq.
4. Click the Viscosity tab. The viscosity of air is 1.781 x 10-5kg/m – sec.
5. Click the Specific Heat tab and make sure the Specific heat value is 1005.0 J/kg-K.
6. Similarly check the Conductivity tab and make sure the values are as follows:
1. Conductivity: 0.02521 W/m-K
2. Turbulent Prandtl number: 0.91
7. 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.
8. Right-click Material Model in the Data Tree and select New from the context menu that appears.
A new entry, Material Model 1, will be created in the Data Tree under the Material Model branch.
9. Right-click Material Model 1 and select Rename in the context menu.
10. Type in Stainless Steel as the name and press Enter.
11. Double-click Stainless Steel in the Data Tree to open the Stainless Steel detail panel.
The Material type is listed as Fluid. This is the default type for any new material created in AcuConsole.
12. Change the Material type for Stainless Steel to Solid.
13. Set the material properties for Stainless Steel as follows by navigating through respective tabs in the detail panel:
1. Density: 8000 kg/m3.
2. Specific Heat: 500.0 J/kg-K
3. Conductivity: 16.2 W/m-K

## 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 twin_cylinder.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 twin_cylinder.x_t.
3. Change the file name filter to Parasolid File (*.x_t *.xmt *X_T …).
4. Select twin_cylinder.x_t and click Open to open the Import Geometry dialog.

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.
6. Rotate the visualization to view the entire model.

### Set the Body Force

The body force commands add volumetric source terms to the governing conservation equations. Two types of body forces will be used in this tutorial.

The first one is the gravitational force on the fluid due to inertia of the fluid. As discussed in Analyze the Problem, gravity is an important aspect of the simulation. In fact, for thermal problems solved in AcuSolve with the Boussinesq approximation, the gravity is scaled by the product of the expansivity and the temperature minus reference temperature, while density remains constant. This variation in the gravitational force on fluid regions with different temperatures is what generated convection currents. For this tutorial gravity is defined as equal to standard gravity (g = 9.81 m/s2) along the negative Y-axis, which is the downward direction in the model.

The second body force which will be used in this model is the volumetric heat source, which specifies the heat energy source term per unit volume. This will be used to simulate the heat-generating inner cylinder in our model.

1. Double-click Body Force in the Data Tree to expand it.
2. Double-click Gravity to open the Gravity detail panel.

The medium for gravity is Fluid. This means that the gravity defined here is applicable only on material models whose material type is fluid.

3. Click Open Array.
4. In the Array Editor dialog, enter:
• X-component: 0.0
• Y-component: -9.81 m/s2
• Z-component: 0.0
5. Click OK to complete the definition of gravity.
Note: The definition of gravity here will have no effect on the simulation unless it is assigned to some volume set in the model.
6. Create a new body force by right-clicking on Body Force in the Data Tree and selecting New in the context menu that appears.
A new entry, Body Force 1, will be created under the Body Force branch.
7. Right-click on Body Force 1, select Rename in the context menu, and type in Heat Source as the entity name.
8. Double-click on Heat Source to open it in the detail panel.
9. Change the Medium to Solid.
10. Click on the drop-down selector next to first Type option and select Per unit volume.
This sets the type of heat source to volumetric heat source.
11. Click on the drop-down selector next to the second Type option and select Constant.
12. Set the Volumetric heat source value to 20000.0 W/m3

### Apply Volume Parameters

Volume groups are containers used for storing information about a volume region. This information includes solution and meshing parameters applied to the volume and the geometric regions that these settings are applied to.

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

In the next steps you will create volume groups for each volume in the model, assign volumes to the respective volume groups, rename the default volume group container, and set the materials and other properties for each volume group.

1. Expand the Model Data Tree item.
2. Create a new volume group for the solid inner cylinder.
1. Right-click on Volumes.
2. Click New.
3. Rename the new volume group to solid.
4. Add the solid component in the geometry to this group.
1. Right-click solid under Volumes in the Data Tree.
3. Click the heating element portion of the geometry in the Visualization Area. Refer to the following figure to identify the correct portion.
Follow the instructions in the Add to dialog if you need to manipulate the display to select the correct portion of the geometry.
4. Click Done to add the selected volume to the solid volume group.
5. Set up the solid volume element set.
The material model for this volume will be set to Stainless Steel, which is the custom material model you created earlier in this tutorial, specifically for this solid volume. Also the solid volume is to be set up as the heat source
1. Expand the solid volume group in the tree.
2. Double-click Element Set to open the Element Set detail panel.
3. Change the Medium to Solid.
4. Change the Material model to Stainless Steel.
5. Change the Body force to Heat Source.
6. In the Data Tree, right-click on default and rename it to fluid.
7. Set up the Fluid volume element set.
1. Expand the fluid volume group in the tree.
2. Double click Element Set under fluid to open it in the detail panel.
3. Ensure that the Medium for the volume is set to Fluid. If not, change it to Fluid.
4. Change the Material model to Air.
5. Change the Body force to Gravity.

### Create Surface Groups and Apply Surface Parameters

Surface groups are containers used for storing information about a surface, including solution and meshing parameters, and the corresponding surface in the geometry that the parameters will apply to.

In the next steps you will define surface groups, assign the appropriate settings for the different characteristics of the problem, and add surfaces to the group containers.

In the process of setting up a simulation, you need to move into different panels for setting up the boundary conditions, mesh parameters, and so on, which can sometimes be cumbersome, especially for models with too many surfaces. To make it easier, less error prone, and to save time, two new dialogs are provided in AcuConsole. Use the Volume Manager and Surface Manager to verify and provide the information for all surface or volume entities at once. In this section some features of Surface Manager are exploited.

1. Turn-off display for Volumes by right-clicking on Volumes and selecting Display off .
2. Right-click on Surfaces in the Data Tree and select Surface Manager.
3. In the Surface Manager dialog, click New six times to create six new surface groups.

If you cannot see the Simple BC Active and Simple BC Type columns, click on Columns , select these two columns from the list and click Ok.

4. Turn off the display for all surfaces except for the default surface.
5. Rename the default surface to inner_wall.
6. Rename Surface 1 through Surface 6 according to the image below.
7. Set the Simple BC Active and Simple BC Type columns as per Figure 14.
8. Assign the periodic surfaces to the respective surface groups.
As mentioned earlier, the cylinders are assumed to be infinitely extended in z-direction. Hence periodicity will be applied in this direction.
1. In the solid_pos_z row in the Surface Manager, click Add to .
2. Select the planar symmetry surfaces as shown in Figure 15 and click Done.
3. Follow the procedure to assign all the surfaces that will extend in the z-direction to respective surface collectors.
9. Assign the outer wall of the geometry to the outer_wall surface group. Use Figure 16 as the reference for selecting the required surfaces.
10. Assign the surface for symmetry_plane.

When the geometry was loaded into AcuConsole, all geometry surfaces were placed in the default surface group container. This default surface group was renamed to inner_walls. In the previous steps, you assigned some surfaces to various other surface groups that you created. At this point, all that is left in the inner_walls surface group are the surfaces which make up the contact boundary between the inner cylinder and the fluid volume.

1. Close the Surface Manager.

### Assign Surface Parameters

The modeling for this simulation was done using half symmetry. The model is only a partial representation of the system, the complete geometry of which is a cylinder. Hence it is appropriate to set the surface that you chose as symmetry_plane with a symmetry boundary condition to simulate that effect.

This change was completed using the Surface Manager in the last section. The following steps are thus optional.

1. Update symmetry_plane.
1. Expand the symmetry_plane surface in the tree.
2. Double-click Simple Boundary Condition under symmetry_plane to open the Simple Boundary Condition detail panel.
3. Ensure that the Type is set to Symmetry.
2. Update outer_wall.
1. Expand the outer_wall surface group in the tree.
2. Double click Simple Boundary Condition under outer_wall to open the Simple Boundary Condition detail panel.
3. Ensure that the Type is set to Wall.
4. Verify that the Wall velocity type is set to Match Mesh Velocity.
5. Change Temperature BC type from Flux to Value.
6. Set the Temperature to 25° C.
The default unit for temperature input is K. You can change the unit for temperature by clicking on the unit button at the right of the input field, and selecting oC from the appearing menu.
3. Update inner_wall
The inner walls form the boundary surface of the inner cylinder volume, and enclose the fluid volume on the inside. Since the inner cylinder is a solid medium, this contact boundary will be a wall.
1. Expand the inner_wall surface group in the tree.
2. Double click Simple Boundary Condition under inner_wall to open the Simple Boundary Condition detail panel.
3. Ensure that the Type is set to Wall.
4. Verify Wall velocity type is set to Match Mesh Velocity.
4. Update the periodic surfaces solid_pos_z, solid_neg_z, fluid_pos_z, and fluid_neg_z
Physically the simulation domain is assumed to extend infinitely in the z-direction. However, only a small section of the cross section is being modelled and the solution is assumed to be consistent along the z-direction. Thus, these periodic surfaces are not physical boundaries but the solution on these surfaces is constrained to be equal by periodicity. This is achieved via a periodic boundary condition in AcuConsole, which links the corresponding pairs of nodes on the two surfaces which are to be constrained with a periodic boundary condition.

Periodicity can be defined before proceeding with mesh generation. With this workflow, when the mesh is generated, AcuMeshSim, which is the mesh generation engine for AcuSolve, will read the defined periodicity constraints and ensure a periodic mesh on the specified surface pairs.

1. Expand the Model Data Tree item, and right-click on Periodics.
2. Select New from the context menu to create a new entity, Periodic 1.
3. Repeat the above step to create a second entity Periodic 2.
4. Rename the two new entities as periodicity_fluid and periodicity_solid.
5. Right-click on periodicity_fluid and select Define from the context menu.
6. In the Periodic BC dialog, make the following settings.
• Use the drop-down arrow to select the surfaces for Side 1 and Side 2 as fluid_neg_z and fluid_pos_z, respectively
• Check that the Type is set to Translational.
• Set X, Y and Z-offset as 0.0, 0.0, 0.01 respectively.
Use the following figure for reference for setting up the periodic BC.
7. Click OK to close the dialog.
8. Using the same figure as reference, similarly define the periodic BC for the entity periodicity_solid, with only the following changes:
• Use the drop down arrows for Side 1 and Side 2 and select solid_neg_z and solid_pos_z, respectively.

### Create Time History Output Points

Time History Output commands enables you to extract the nodal solution at any point within the domain.

1. In the tree, double-click on Output, then right-click on Time History Output, and select New.
A new entry, Time History Output 1, will be created in the Data Tree under the Time History Output branch.
2. Right-click on Time History Output 1, select Rename, and type in Monitor points as the entity name.
3. Double click Monitor points to open the detail panel. In the detail panel,
1. Change the Type to Coordinates.
2. Click Open Array.
3. In the Array Editor, add a new row by clicking Add Row.
4. Fill in the values as follows:
4. Click OK.
5. Set Time step frequency to 1.
This will save the results for the defined time history points at every time step.
6. Save the database.

### Set the Initial Conditions

1. Double-click on Nodal Initial Condition in the Data Tree to open the detail panel.
2. Set the Temperature to 80° C.
1. The default unit for temperature input is K. You can change the unit for temperature by clicking on unit to the right of the input field, and selecting oC from the appearing menu.
2. Alternatively, enter 353.15 K in the temperature field.

## Assign Mesh Controls

### Set Global Mesh Parameters

Now that the flow characteristics have been set for the whole problem, a sufficiently refined mesh has to be generated.

Global mesh attributes are the meshing parameters applied to the model as a whole without reference to a specific geometric volume, surface, edge, or point. Local mesh attributes are used to create mesh generation controls for specific geometry components of the model.

In the next steps you will set the global mesh attributes.

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. Double-click the Global Data Tree item to expand it.
3. Double-click Global Mesh Attributes to open the Global Mesh Attributes detail panel.
4. Change the Mesh size type to Absolute.
5. Enter 0.005 m for the Absolute mesh size.

### Set Surface Mesh Parameters

Surface mesh attributes are applied to a specific surface in the model. It is a type of local meshing parameter used to create targeted mesh controls for one or more specific surfaces.

Setting local mesh attributes, such as surface mesh attributes, is not mandatory. When a local mesh attribute is not found for a component, the global attributes are used as the mesh generation control for that component. If a local mesh attribute is present, it will take precedence over the global setting.

In the next steps you will set the surface meshing attributes.

1. Go to the Solver Browser, expand 01.Global, then click PROBLEM_DESCRIPTION.
2. Expand the Model Data Tree item.
3. Under the Model branch, expand the Surfaces. Under Surfaces, expand the inner_wall surface group.
4. If necessary, check the box next to Surface Mesh Attributes to activate it. Double-click it to open the Surface Mesh Attributes detail panel.
The detail panel should now be populated with options related to the local surface meshing controls.
5. Ensure that the Mesh size type is set to Absolute.
6. Enter 0.002 m for the Absolute mesh size.
7. Switch the Boundary layer flag to On.
Mesh controls related to boundary layer meshing become visible.
8. Check the Boundary layer type is set to Full Control.
9. Set Resolve to Total Layer Height.
This sets the total layer height based on the other settings you provide.
10. Set the remaining settings as follows:
Option Description
First element height 0.0001
Growth rate 1.2
Number of layers 8
Boundary layer elements type Tetrahedron

Instead of repeating the above steps for the outer_wall surface, you can choose to propagate the mesh attribute settings for inner_wall surface group to outer_wall surface group.

1. Under the inner_wall surface, right-click Surface Mesh Attributes and select Propagate.
2. In the Propagate dialog, select the surface outer_wall and click Propagate.

### Define Mesh Extrusion

The present simulation is equivalent to a 2D representation of the model, which actually extends infinitely in both sides along the z-direction. In AcuSolve, 2D models are simulated by having just one element across the faces of the cross section. Thus when these faces are set up with a similar boundary condition, it coerces the corresponding nodes across the faces to have same results. In this problem, these faces are the negative and positive z-surfaces. This kind of mesh is achieved in AcuSolve with mesh extrusion process. In the following steps, the process of extrusion of the mesh between these surfaces is defined.

1. Expand the Model Data Tree item.
2. Right-click Mesh Extrusions and select New from the context menu to create a new entity, Mesh Extrusion 1.
3. Repeat the above step to create a second entity, Mesh Extrusion 2.
4. Rename the two entities as extrusion_fluid and extrusion_solid.
5. Right-click extrusion_fluid and select Define from the context menu.
6. In the Mesh Extrusion dialog, make the following settings.
1. Check that the Geometry type is set to surface.
2. Use the drop down arrows to select the surfaces for Side 1 and Side 2 as fluid_neg_z and fluid_pos_z, respectively.
3. Check that the Extrusion type is set to Number of layers.
4. Set Number of layers equal to 1.
5. Set Extrusion options to All tets.
Use the following figure for reference for setting up the mesh extrusion for extrusion_fluid.
7. Click OK to close the dialog.
8. Using the same figure as reference, similarly define the mesh extrusion for the entity extrusion_solid, with only the following changes:
1. Use the drop down arrows to select the surfaces for Side 1 and Side 2 as solid_neg_z and solid_pos_z, respectively

### 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.
For this case, the default settings will be used.
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.

Note: The actual number of nodes and elements, and memory usage may vary slightly from machine to machine.
3. Visualize the mesh in the modeling window. Turn on the display of surfaces and set the display type to solid and wire.
4. Rotate and zoom in the model to analyze the various mesh regions.

### Assign Reference Pressure

The present case does not have any inlet or outlet surfaces to define any boundary condition that sets the pressure level inside the domain. To make the solution more robust, you will set a pressure reference point using a nodal boundary condition. The following steps will show how to setup the reference pressure inside the CFD domain.

1. Click BAS in the Data Tree Manager to switch to basic view in the Data Tree.
2. Expand the Model Data Tree item.
3. Right-click on Nodes and select New to create a new entity, Node 1.
4. Rename Node 1 to Fixed Pressure Node.
5. Right-click Fixed Pressure Node and select Define.
6. In the Node Define Dialog Box, set Selection Type to Pressure Point and Volumes to fluid.
7. Click OK.
8. Expand Fixed Pressure Node and enable Pressure.
The single node will now act as the pressure reference point for the simulation. The default Type of Zero sets the nodes in this set to pressure = 0.0.
9. Examine the location of the reference pressure node and check that it is inside the domain.
1. Right-click on Fixed Pressure Node and select Display on.
2. Right-click on Surfaces and set Display type to outline.
3. Right-click Periodics and select Display off.
You should be able to see the fixed pressure node as a point, as shown in the figure below.

## 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.
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.

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

### Post-Process with AcuProbe

AcuProbe can be used to monitor various variables over solution time.

Note: This solution was obtained by running AcuSolve
with four processors.
1. Open AcuProbe by clicking on the toolbar.
2. In the Data Tree on the left, expand Residual Ratio. Right-click on Final and select Plot All.
This will plot the residuals for the three variables, pressure, temperature and velocity, in the plot area.
Note: You might need to click on the toolbar in order to properly display the plot.
3. Right-click on Final under Residual Ratio and select Plot None.
4. Expand Time History > Monitor Points.
5. Expand node 1 and node 2.
6. One node at a time, right-click on temperature and select Plot.
Note: You might need to click on the toolbar in order to properly display the plot.

The node 1 lies in the bottom half of the model and the node 2 in the upper half. The temperature distribution in the above plot shows that in steady state upper half of the cylinder annulus is occupied by the hotter air and lower half has the colder air.

7. In the menu area, click the surfs collector and select all.
8. The time series data of the variables can also be exported as a text file for further post-processing.
1. Right-click on the variable that you want to export and click Export.
2. Enter a File name and choose .txt for the Save as type.
3. Click Save.

### View Results with AcuFieldView

The tutorial has been written with the assumption that you have become familiar with the AcuFieldView interface and basic operations. In general, it will be helpful to understand the following basics:
• How to find the data readers in the File menu and open up the desired reader panel for data input.
• How to find the visualization panels either from the toolbar or the Visualization panels from the main menu to create and modify surfaces in AcuFieldView.
• How to move the data around the modeling window using mouse actions to translate, rotate and zoom in to the data.
This tutorial shows you how to work with steady state analysis data.

#### Start AcuFieldView

1. Click on the AcuConsole toolbar to open the Launch AcuFieldView dialog.
2. Click Ok to start AcuFieldView.
You will see that the temperature contours have already been displayed on all the boundary surfaces with mesh.

#### Manipulate the Model View in AcuFieldView

1. Close the Boundary Surface dialog.
2. Click Viewer Options.
3. Turn off perspective view by deselecting the Perspective check box.
4. Disable axis markers by clicking on the Axis Markers button.
5. Close the Viewer Options dialog.
6. Click on the Colormap Specification icon on the toolbar.
7. Click on Background in the Scalar Colormap Specification dialog and select white from the color palette that opens.
8. Close both dialogs.
9. Click on the Toggle Outline icon on the toolbar to turn off the outline display.
Your AcuFieldView display should now look like this.

#### Create the Boundary Surface Showing Temperature for the Outer Surfaces with Mesh

1. Orient the geometry as shown in the figure below, so that the symmetry plane and periodic surfaces are visible.
2. Click to open the Boundary Surface dialog.
3. Click the Legend tab and check the Show Legend check box.
4. Change the color of labels to black from the color palette.
5. If desired, change the number of labels to show more labels.
6. Change the Annotation title color to black.
Note: You can move the legend using Shift + left click, and resize it using Shift + right click.

#### Coordinate the Surface Showing Temperature on the Mid-Coordinate Surface

1. In the Surface tab in the Boundary Surface dialog box, click Visibility to turn it off.
2. Click Create to create a new Boundary Surface set.
3. Check Visibility to turn it on.
4. Set the Display Type to Outlines.
5. Under Boundary Types, click Select All, and click Ok.
6. Click to open the Coordinate Surface dialog.
7. Click Create to create a new Coordinate Surface.
8. Set the Coord Plane to Z.
The coordinate surface created is the mid plane between the two periodic surfaces in the model.
9. Change the Coloring to Scalar.
10. Set the Display Type to Smooth.
11. In the Scalar Function list, select Temperature as the scalar function to be displayed.
12. In the Colormap tab, change Scalar Coloring to Local.
13. In the Legend tab, check the Show Legend check box to display the temperature values on the coordinate plane.
14. From the Defined Views, select viewing direction as +Z.

#### Coordinate the Surface Showing Vectors of Velocity on the Mid-Coordinate Surface

1. In the Surface tab in the Coordinate Surface dialog box, click Create to create a new Coordinate Surface set.
2. Set the Display Type to Vectors.
3. Change the Coloring to Scalar.
4. In the Scalar Function list, select Velocity Magnitude as the scalar function to be displayed.
5. Next to Vectors, click Options.
6. Activate Head Scaling and set it at 1.
7. Set the Length Scale to 4.
8. Activate the Skip option, and set the value to 50%.

## Summary

In this AcuSolve tutorial, you successfully set up and solved a natural convection problem. The problem simulated a hot cylinder placed in the center of another air-filled cylindrical volume. Air was modeled using a Boussinesq density approximation model, which is used for buoyancy driven flows, such as those involving natural convection. As the film of air in vicinity of the surface of the hot inner cylinder heated up, it generated convection currents within the annular volume.

You started the tutorial by creating a database in AcuConsole, importing and meshing the geometry and setting up the basic simulation parameters. The hot inner cylinder was represented by a solid volume also acting as a heat source. Once the case was setup, the solution was generated with AcuSolve.

Results were post-processed in AcuFieldView where you generated a temperature profile, and a velocity vector profile, on a cross-section of the model.

New features that were introduced in this tutorial include creating and specifying a new custom material in AcuConsole, specifying a volume group as a heat source using the Boussinesq density model and setting up periodic boundary conditions.