• Author / Uploaded
• Pranjal Anand

Citation preview

TRANSPORT PHENOMENA A LABORATORY MANUAL IN CHEMICAL ENGINEERING

DEPARTMENT OF CHEMICAL ENGINEERING R V COLLEGE OF ENGINEERING BANGALORE 560059 2015-2016

R. V. College of engineering Department of Chemical Engineering 12CH62 – Transport Phenomena Lab

Laboratory Manual Academic Year 2015–2016

Name of the Student

:

University Seat No.

:

Semester & Section

:

Batch

:

Vision of RVCE: Leadership in technical education, research & innovation, with a focus on sustainable and inclusive technology

Mission of RVCE: •

To deliver Quality Technical Education, with an equal emphasis on Experiential Learning with the state of the art infrastructure

•

To create an Open, Conducive and Interdisciplinary Environment for faculty and students to learn and carry out Research, consequently excel in their areas of interest

•

To continuously foster Industry – Institution collaboration for Teaching and Research, leading to Innovation and Entrepreneurship

•

To focus on development of technologies that are Sustainable and Inclusive, addressing Social Issues

•

To Nurture Disciplined, Ethical, Socially Concerned and Employable Engineers

•

Vision of the Chemical Engineering department: Imparting quality education that promotes leadership in Research, Innovation and Sustainable Technologies through teamwork and Entrepreneurship in Chemical Processes, Energy, Unit Operations and Computational Chemical Engineering to meet societal requirements Mission of the Chemical Engineering department: education in basic and applied areas of Chemical Engineering

1.

Impart

quality

2. Enable students and faculty to achieve proficiency in the areas of Chemical Processes, Energy, Unit Operations and Computational Chemical Engineering using state-of-the-art laboratories and modern infrastructure 3. Encourage faculty and students to make career in research and contribute towards innovative processes and products 4. Develop inclusive technologies with a focus on new materials and sustainability 5. Collaborate with industries and research institutes for academics and research 6. Inculcate leadership qualities, entrepreneurial skills, societal and ethical values in students and faculty

Program Educational Objectives (PEOs) Graduates will be able to, PEO 1: Comprehend, analyze, design and implement engineering systems by acquiring sound knowledge of Basic Sciences and Chemical Engineering PEO 2: Excel in the areas of Chemical Processes, Energy, Unit Operations and Computational Chemical Engineering with a focus on research and innovation PEO 3: Address industry challenges by providing sustainable engineering solutions and to work in multi disciplinary team with human values PEO 4: Exhibit sound communication skills, leadership qualities and develop into successful entrepreneurs Program Outcomes The graduates in BE of Chemical Engineering are expected to have the following abilities/ qualities PO1. Apply knowledge of mathematics, basic sciences and engineering fundamentals to identify, formulate and solve chemical engineering problems PO2. Design a system, component, or process to meet desired needs with appropriate societal and environmental considerations

PO3. Work in multi-disciplinary teams and develop leadership qualities with effective communication PO4. Engage in life-long learning and follow ethical principles PO5. Identify and use appropriate computational tools in chemical engineering practice PO6. Undertake research leading to innovations, sustainable technologies and entrepreneurship with a focus on project management

Experiment 1: 3D-CAD modelling of cyclone AIM: To create geometry model of cyclone separator using 3D-CAD. Create a 3D-CAD model: 1.Launch STAR-CCM+. 2.Save the simulation under the name cyclone.sim. Launch 3D-CAD and create the geometry: 3.Right-click Geometry > 3D-CAD Models and select New. The 3D-CAD environment launches and a 3D-CAD model is created. Within 3D-CAD, an object

tree

that

is

specific

to

the

3D-CAD

model

is

displayed.

This

tree

contains Bodies, Features, and Design Parameters nodes. A 3D-CAD View scene is also created automatically. Initially, this scene displays three starting sketch planes which are used as a basis for adding features to the model. 4.Rename the 3D-CAD Model 1 node to Cyclone.

Sketching the Cyclone Profile: Create a sketch that contains the profile of the cyclone chamber.

Every 3D-CAD model contains three default sketch planes: XY, YZ, and ZX. Create a sketch on the YZ sketch plane: 1.Right-click the Features > YZ node and select Create Sketch. Creating a sketch activates sketch mode, in which a grid is displayed on the sketch plane in the 3D-CAD View scene, and the Sketch panel opens. This panel contains the tools for creating sketch entities, such as lines, circles, and arcs. The panel also allows you to control the settings for the grid that is displayed in the scene. Each sketch plane has local X and Y axes relative to the position and orientation of the plane in relation to the global coordinate system. 2.Click

(View normal to sketch plane) to align the sketch plane with the plane of the

screen. 3.Click

(Set sketch grid spacing) to specify the distance between the grid lines on the

sketch plane so that the spacing is suitable for the dimensions of the model geometry. 4.In the Grid Spacing dialog, set Grid Spacing to 0.025 m. 5.Click OK. Use the mouse to adjust the position, orientation, and zoom level of the sketch plane. 6. In the 3D-CAD View scene: Left-click and drag the mouse in any direction to rotate the view. While holding down the key, click and drag to roll the view. Right-click and drag to pan the view. Middle-click and drag to zoom in or out. Alternatively, if your mouse has a scroll wheel, turn the mouse wheel to adjust the zoom level. 7.Click

(View normal to sketch plane) to realign the sketch plane with the screen.

8.Adjust the view in the 3D-CAD View scene so that the top half of the grid is shown. Leave some white space above the grid as the sketch will cover some of this space. 9.Click

(Create line) and move the mouse over the grid in the 3D-CAD View scene.

The mouse pointer has a blue square that is attached to it, which indicates the position of the point on the grid. The coordinates of this point are displayed in the Line Properties box of the Sketch panel, and change as you move the mouse. The

(Snap to Grid) option is

enabled by default, so the point jumps to an intersection between two grid lines as it is approaches them. 10.Position the blue square at [0.0, 0.3] m.

11.Click to fix the blue square in position. Create the first set of lines with approximate lengths. To exit the tool while creating a sketch entity, press the key. If you want to reposition any sketch entities while you are sketching, exit the tool first, then click-and-drag the relevant sketch entities to the desired position. To resume sketching, simply select the appropriate tool from the Create Sketch Entities box and continue. 12.Move the mouse pointer to the left. A blue preview is shown to indicate the position of the line. Position the mouse so that the blue line extends horizontally left of the starting point and click the left mouse button. The Line tool creates continuous lines, so the end point of the first line is the start point of the next. The coordinates that are shown in the Line Properties box are automatically updated as each line is defined. 13.Move the mouse pointer into the white space above the grid and notice that it still snaps to grid intersections even though they are not visible. 14.Position the mouse so that the second line is vertical and ends in the white space above the grid. You can adjust the zoom level while you are in the process of creating sketch entities. 15.Left-click to fix the end point of the second line. When you draw sketch entities outside of the grid that is shown in the 3D-CAD View scene, the grid automatically expands. 16.Create a short horizontal line that extends to the left of this point and left-click to fix the end point in position. 17.Move the mouse vertically downwards to create a longer vertical line and click to fix the point. 18.Press the key to exit the line creation tool.

Adding Constraints and Dimensions: Constraints and dimensions are applied to the sketch to control the position and size of the sketch entities on the sketch plane. Apply the constraints first to maintain the current orientation of the lines. Following this, apply the dimensions to define the length of each line. • A

Right-click the first horizontal line and select Apply Horizontal Constraint.

glyph is added to the sketch to show that the constraint has been applied.

2.Select one of the horizontal lines, then hold down the key and select the other horizontal line. Right-click and select Apply Parallel Constraint. Apply similar constraints to the vertical lines:

3.Right-click one of the vertical lines and select Apply Vertical Constraint. 4.Using the technique described above, select both of the vertical lines, right-click and select Apply Parallel Constraint. Set the length of each line by applying dimensions: 5.Right-click the first horizontal line and select Apply Length Dimension. 6.In the Dimension dialog, enter a value of 0.075 m. 7. Click OK. 8.Repeat the previous two steps for the remaining lines. Use the values that are displayed in the following sketch: Notice that when you select each line, a list of the constraints and dimensions that are applied to that line is displayed in theConstraints/Dimensions box in the Line Properties. Draw the remainder of the cyclone profile, and use some additional constraints to control its position on the sketch plane: 9.Pan the view down and adjust the zoom level so that the 3D-CAD View scene appears as follows: 10.Click

(Create line) and move the mouse to the starting point for the previous set of

lines. The mouse automatically snaps to existing sketch entities within the sketch, so when the blue square is close to the point, it jumps onto that point. 11.Click the top of the existing point. 12.Move the mouse vertically downward until a line Length of 0.7 m is shown in the Line Properties box. Left-click to fix the point at the grid intersection. 13.Move the mouse to the left and create a short line that extends horizontally from this point. Complete the profile by creating a diagonal line to define the cone shape of the cyclone: 14.Move the mouse pointer to the free end of the first set of lines and click to close the sketch profile. 15.Right-click the longest vertical line and select Apply Vertical Constraint. 16.Right-click the horizontal line at the bottom of the sketch and select Apply Length Dimension. 17.In the Dimension dialog, enter a value of 0.05 m and click OK. Move the axis of the cyclone so that it is aligned with the Y-axis of the sketch plane. To do this you can drag-and-drop the sketch:

18.If necessary, adjust the zoom level. Left-click and hold at any point on the longest vertical line, drag the mouse pointer onto the origin and release the mouse button. Adding a Construction Line A construction line defines the axis around which the cyclone profile revolves. Add a construction line to the profile sketch: 1.Click

(Create line) and create a line that is aligned with the Y-axis as shown below.

The appearance of the line changes from solid to dashed to indicate that it is now a construction line. Upon exiting the sketch, this line is no longer visible, as construction lines are only shown when you are creating or editing a sketch. Apply a constraint between the construction line and the vertical line at the center of the cyclone to make sure that they are collinear: 4.To select the construction line, hold down the key and select the long vertical line on the Y-axis. 5.Right-click either of the lines and select Apply Collinear Constraint. The cyclone profile is now complete and is ready to revolve. 6.Click OK at the bottom of the Sketch panel to exit sketch mode. Revolving the Cyclone Profile: Right-clicking a sketch in the feature tree lets you perform various CAD operations, such as revolving a profile around an axis. Revolve the sketch of the cyclone chamber profile: 1.Rename the Sketch 1 node to Sketch Profile. 2.Right-click Sketch Profile and select Create Revolve. The Revolve panel lets you specify the parameters for the revolved feature. The Direction option defines the direction in which the sketch is revolved. The Body Interaction option specifies how the body that is created from the revolution interacts with any other bodies in the model. In this case, the sketch is revolved through 360 degrees and no other bodies are present. Therefore the Direction and Body Interaction settings do not affect the outcome and can be left as the default. The Axis option lets you choose which construction line to use as the axis of revolution. In this case, the sketch only contains one construction line, so this menu contains a single option, Line 8. A blue preview of the selected axis is shown in the 3D-CAD View scene. 3.In the Revolve panel, click set Angle to 360.0 deg and press . 4.Click OK to confirm the settings and create the revolved feature. A Revolve 1 feature node is added to the feature tree, and the solid body is displayed in the Graphics window. Bodies that form a 3D-CAD model are shown under the Bodies node.

5.Expand the Bodies node and select Body 1. The corresponding body is highlighted in the 3D-CAD View 1 scene. 6.Rename the Body 1 node to Fluid. Creating the Outlet Pipe The outlet pipe has a circular cross-section and is created by sketching a circle and extruding it. The circle that is sketched is slightly smaller in diameter than the hole in the top of the cyclone, and the difference between the two is the thickness of the outlet pipe. Create the sketch for the outlet pipe on an existing face: 1.Rotate the model in the 3D-CAD View 1 scene so that you can see the sunken face in the top of the model. 2.Right-click the sunken face and select Create Sketch. A sketch plane that is defined by the selected face is displayed on the model in the 3D-CAD View scene. 3.Click

(View normal to sketch plane).

4.To see the hole, in the Vis toolbar, click 5.Click

(Make scene transparent).

(Create circle) in the Create Sketch Entities box and click at [0.0, 0.0] m.

The first click positions the circle at the origin of the sketch. The second mouse click lets you specify the radius of the circle. 6. Move the mouse so that the radius is approximately 0.06 m, using the Circle Properties box for reference, and click. You can define the circle radius more accurately by entering an exact value in the Circle Properties box. 7.In the 3D-CAD View 1 scene, click on the circle. 8.Set Radius to 0.07 m 9.Click OK to exit the sketch. 10. In the Vis toolbar, click

(Make Scene Transparent).

Extrude the sketch to form the outlet section of the cyclone geometry: 11.Right-click the Sketch 1 node in the feature tree and select Create Extrude. 12.In the Extrude panel, make sure that Body Interaction is set to the default option of Merge. This option causes it to merge with the Fluid body, resulting in a single body. 13.Set Distance to 0.45 m. 14.Retain the default settings for the other options.

15.Use the mouse to rotate the model and check the preview of the extrusion. 16.Click OK. Creating the Inlet Duct Fluid enters the top of the chamber horizontally through a rectangular inlet duct. Create the inlet duct: 1.Right-click the Features > YZ node and select Create Sketch. 2.Click 3.Click

(View normal to sketch plane). (Make scene transparent).

4.Zoom in on the top left-hand corner of the geometry. 5.Click

(Create rectangle) and click the top left corner of the cyclone.

6.Move the mouse pointer down and to the right until the rectangle Length that is shown in the properties box is 0.05 m and the Width is0.15 m. 7.Left-click to fix the point in position. 8.Click OK. Constraints are applied automatically to a rectangle to make sure that the sides are vertical and horizontal. 9.Click

(Make Scene Transparent).

Extrude the sketch: 10.Right-click the Sketch 2 node and select Create Extrude. 11.In the Extrude panel, set the extrusion Distance to 0.35 m and click OK. Creating a Design Parameter Design parameters allow you to modify an aspect of the geometry from outside 3D-CAD. Create a design parameter to control the position of the outlet pipe: 1.Right-click the Sketch Profile node and select Edit. 2.Click

(View normal to sketch plane).

3.Zoom in on the top of the sketch. 4.Select the vertical line that defines the hole at the top of the cyclone chamber. Right-click the dimension arrow for this line and selectEdit Dimension. 5.In the Dimension dialog, activate the Expose Parameter option. 6.In the Name textbox enter PipeDepth and click OK. To make sure that the changes that are made to the length of this line only affect the depth of the hole into the cyclone chamber, fix the total height of the cyclone using a vertical dimension. Also fix the position of a point at the top of the cyclone.

7.Right-click the point at the top of the PipeDepth line and select Apply Fixation Constraint. 8.Zoom out so that the whole sketch is visible. 9.Select the point at the top of the PipeDepth line, hold down the key and select the point at the bottom-right corner of the sketch. 10.Right-click one of the selected points and select Apply Vertical Distance. 11.In the Dimension dialog, make sure that the value is 0.9 m and click OK. 12.Click OK to exit the sketch. The design parameter is displayed under the Design Parameters node in the object tree: 13.Expand the Design Parameters node and select the PipeDepth node. Specifying Inlet and Outlet Faces The final step in preparing the model geometry is to specify the inlet and outlet faces of the model by setting face names. When the 3D-CAD model is imported into the simulation via geometry parts, faces that have been named are defined as separate part surfaces. Therefore, when the geometry is assigned to a region, these surfaces can easily become separate boundaries. Name the faces for the inlet and outlet: 1.Rotate the model so that the inlet duct is visible. 2.Right-click the rectangular inlet face and select Rename. 3.In the Rename dialog, enter Inlet and click OK. 4.Right-click the circular face at the top of the outlet pipe and select Rename. 5.In the Rename dialog, enter Outlet and click OK. The geometry is now complete and you can exit 3D-CAD. 6.AT the bottom of the object tree, click Close 3D-CAD. When you exit 3D-CAD, the 3D-CAD View 1 scene closes automatically. 7.Save the simulation.

Geometry scene Creating a Geometry Part Create a geometry part from the 3D-CAD model. To use the 3D-CAD model in a simulation, create a geometry part: 1. Right-click the Geometry > 3D-CAD Models > Cyclone node and select New Geometry Part. 2.In the Parts Creation Options dialog, click OK to close the dialog. The default settings are acceptable. 3.Expand the Parts > Fluid > Surfaces node. The inlet and outlet faces that you specified in the previous section are defined as separate surfaces. Assigning a Part to a Region To define the computational domain, assign the cyclone separator part to a region. 1.Right-click the Geometry > Parts > Fluid node and select Assign Parts to Regions. 2.In the Assign Parts to Regions dialog, select: a. Create a Region for Each Part b. Create a Boundary for Each Part Surface 3.Click Apply then Close. A new region is created with boundaries that define the inlet, outlet, and main fluid volume. Check that the region and boundaries are defined correctly: 4.Create a Geometry Scene.

5.Expand the Regions > Fluid > Boundaries node and select each of the boundary nodes to make sure that they are specified correctly. VIVA Questions 1. Why are we creating a design parameter? 2. Why are we assigning parts to each region? 3. What happens if you don’t rename Body 1 to fluid in the earlier step? 4. Enunciate the importance of Grid spacing for creating the cyclone separator sketch. 5. What is the importance of applying vertical, horizontal constraints and collinear constraint? 6. Why are we creating the construct line? 7. What is the importance of Merge option in the “create extrude” dialog box? 8. What is the importance of specifying and renaming the inlet and outlet? 9. What is the relation between assigning parts to each region and renaming the inlet and outlet faces? 10. What is Simulation? 11. What is Modelling? 12. What is the difference between Simulation and Modelling? 13. What is a cyclone separator? Which are the industries it is used? 14. What is vortex separation? 15. What is cut-point of a cyclone? 16. What are the different types of vortex?

Experiment 2: Post processing of cyclone for velocity scalar AIM: To obtain scalar velocity plot for cyclone separator. Selecting Physics Models Physics models define the physical variables and phenomena in the simulation. In this tutorial, the K-Omega turbulence model is used to limit the simulation run time. To select the physics models: 1.Create a physics continuum. 2.For the physics continuum, Continua > Physics 1, select the following models in order: 3.Click Close. 4.To review the models, open the Physics 1 > Models node. 5.Save the simulation. Specifying Boundary Conditions

Specify conditions at the inlet and outlet boundaries: 1.Edit the Regions > Fluid > Boundaries node. 2.Set the following properties: Generating a Mesh Use a polyhedral mesh to analyze the flow patterns in the cyclone separator. 1.Create a mesh continuum. 2.For the mesh continuum, Continua > Mesh 1, select the following models in order: 3.Click Close. Define the mesh settings and generate the volume mesh: 4.Select the Mesh 1 > Reference Values > Base Size node and set Value to 0.01 m. 5.Generate the volume mesh. 6.Create a mesh scene. 7.Save the simulation.

Mesh Scene Preparing a Scalar Scene Use a scalar scene to visualize the vertical velocity on a section through the cyclone chamber. You can use this scene to visualize the solution while the simulation is running. 1.Create a scalar scene. 2.Create a section plane with the following properties: 3.Rotate the view in Scalar Scene 1 so that the plane section is visible. Define the scene settings: 4.Click scene/plot.

5.Edit the Displayers node and set the following properties: 6.Save the simulation.

Scalar Scene Running the Simulation Preparation of the simulation is now complete, and the simulation can be run. 1.Click

(Run) in the Solution toolbar.

2.While the simulation is running, select the Scalar Scene 1 tab at the top of the Graphics window to visualize the solution. 3.When the simulation has finished running, save it.

Scalar scene After Iterations VIVA Questions: •

What is Physics models?

•

What is a continuum?

•

What is K-Omega Turbulence?

•

What is segregated flow?

•

What are the different equations of state you know?

•

What is turbulence suppression?

•

What is the importance of specifying boundary conditions?

•

What is mesh continuum?

•

How would you differentiate mesh and physics continuum?

•

What is the importance of Base size for the polyhedral mesh created?

•

What is scalar scene?

•

How to create a section plane?

•

Why are we creating the section plane?

•

What is iteration with respect to the simulation created?

•

Differentiate the scalar velocity scene and scalar pressure scene?

•

Interpret the pressure scalar scene and velocity scalar scene.

•

Define continuum mechanics.

Experiment 3: Post processing of cyclone for stream lines AIM: To obtain stream lines for cyclone separator. Creating a Streamlines Scene Create a scene to display the streamlines inside the cyclone separator. 1.Create a Geometry Scene. 2.Rename the Geometry Scene 2 node to Streamlines. Use the Create Streamline panel to specify the properties of the streamlines. In this case, the streamlines are grown from the cyclone inlet. 3.Create a Streamline derived part with the following properties: Define the scene settings: 4.Click scene/plot. 5.Edit the Streamlines > Displayers node and set the following properties: To extend the streamlines through the fluid domain up to the outlet, increase the maximum propagation property. This defines how far the streamlines are propagated through the fluid domain from the starting points. A higher value causes the streamlines to extend further. 6.Select the Derived Parts > streamline > 2nd Order Integrator node and set Maximum Propagation to 15.

Animating the Streamlines Animate the streamlines inside the cyclone chamber. To animate streamlines: 1.Click scene/plot. 2.Edit the Displayers node and set he following properties: 3.In the Animation toolbar: a.Click

(Play)

b.To stop the animation, click

(Stop)

Stream lines scene Additional: Modifying the Geometry and Rerunning (Refer the star CCM+ inbuilt manual)

VIVA Questions: •

What is streamlines?

•

What is maximum propagation?

•

Why are we setting scalar field to velocity in K direction?

Experiment 4: Natural convection of heated fin AIM: To obtain temperature profile around fin. Importing the Mesh and Naming the Simulation To set up the STAR-CCM+ simulation, launch a simulation and import the supplied volume mesh. Use the following steps: 1.Launch STAR CCM+. 2.Start a simulation. 3.Select File > Import > Import Volume Mesh. 4.In the Open dialog, navigate to [INSTALL_DIR]/doc/startutorialsdata/heatTransferAndRadiation/data. 5.Select fin.ccm then click Open. STAR-CCM+ provides feedback on the import process in the Output window. Two mesh regions named AIR and AL are created in the Regionsnode representing the grid domain. A geometry scene is created in the Graphics window. 6.Save the simulation as heatedFin.sim.

Converting to a Two-Dimensional Mesh For greater efficiency, convert the mesh region from a one-cell-thick three-dimensional grid to a two-dimensional one. There are special requirements in the STAR-CCM+ product for three-dimensional meshes that are converted to two-dimensional ones. These requirements are: The grid must be aligned with the X-Y plane. The grid must have a boundary plane at the Z = 0 location.

The mesh imported for this tutorial was built with these requirements in mind. Were the grid not to conform to the above conditions, it would have been necessary to realign the region using the transformation and rotation facilities in STAR-CCM+. 1.Select Mesh > Convert To 2D. 2.In the Convert Regions To 2D dialog that appears, make sure that: All regions are selected. The Delete 3D Regions After Conversion option is activated. 3.Click OK. Once you click OK, the mesh conversion takes place. The new two-dimensional mesh is shown, viewed from the z-direction, in the Geometry Scene 1 display which was created after you imported the mesh. The mouse rotation option is suppressed for two-dimensional scenes. 4.Right-click the Continua > Physics 1 continuum node and select Delete. 5.Click Yes in the confirmation dialog. 6.Repeat these steps for the Physics 2 continuum node.

Renaming Regions and Boundaries Change the default region and boundary names to more suitable names. Use the following steps: 1.Rename AIR 2D to Fluid. 2.Rename the boundaries within the Fluid node: Original Name New Name wall

Air-Interface

wall 2

Vertical-Walls

wall 3

Horizontal-Walls

3.Rename AL 2D to Solid. 4.Rename the boundaries within the Solid node: Original Name

New Name

Default_Boundary_Region Fin-Interface

wall

Fin-Bottom

Scaling the Mesh 1.To scale the region, select Mesh > Scale Mesh from the menu bar. 2.In the Scale Mesh dialog, set the Scale Factor to 0.01 for the fluid and solid regions. 3.Click Apply. The mesh region reduces in size. 4.Click Close. 5.To restore the previous viewing distance for the scaled domain in the display, click

(Reset

View) in the toolbar. 6.To verify that scaling has in fact been applied: a.Select Mesh > Diagnostics from the menu bar. b.In the Mesh Diagnostics dialog, click OK for all regions. 7.Check and review the output values.

Visualizing the Interior Two-Dimensional Mesh This part of the tutorial involves examining the interior of the two-dimensional mesh of the heated fin. Use the following steps: 1.Select the Scenes > Geometry Scene 1 > Displayers > Geometry 1 node. 2.Activate the checkbox of the Mesh property. This shows the mesh in the solution domain interior. 3.To get a clearer view of individual mesh regions, highlight them. For example, select the Regions > Fluid node.

Geometry Scene Setting Up the Models

Models define the primary variables of the simulation, including pressure, temperature, velocity, and what mathematical formulation is used to generate the solution. In this example, the flow is turbulent and compressible. The Coupled Flow model is used together with the default K-Epsilon turbulence model. As there are two materials (air and aluminum) present, two regions are required for the analysis. Define two sets of continuum models, each appropriate to a different region. By default, Physics 1 2D and Physics 2 2D are automatically created when the mesh is converted to two-dimensional. Use these continua for the fluid and the solid. 1.Rename the continua: Original Name

New Name

Physics 1 2D Air Physics 2 2D Aluminum Alloy 2.For the physics continuum, Continua > Air, select the following models in order: Group Box

Enabled Models

Model Two Dimensional (Selected automatically) Gradients (Selected automatically)

Time

Steady

Material

Gas

Flow

Coupled Flow

Equation of State

Ideal Gas

Turbulent Viscous Regime

Reynolds-Averaged Turbulence

Reynolds-Averaged NavierStokes (Selected automatically) K-Epsilon Turbulence Realizable K-Epsilon Two-Layer (Selected

automatically) Two-Layer All y+ Wall Treatment (Selected automatically) Optional Models

Gravity

3.Click Close. The color of the Air node turns from gray to blue to indicate that models have been activated. 4.To review the models, open the Air > Models node. 5.For the continuum of the solid region, Continua > Aluminum Alloy, select the following models in order: Group Box

Model Two Dimensional (Selected automatically)

Enabled Models

Gradients (Selected automatically)

Material

Solid

Optional Models

Coupled Solid Energy

Equation of State

Constant Density

Time

Steady

6.Click Close. The color of the Aluminum Alloy node turns from gray to shaded gray to indicate that models have been activated. 7.To review the models, open the Aluminum Alloy > Models node. 8.Save the simulation.

Setting Material Properties This part of the tutorial involves changing the solid material properties for the aluminum alloy fin. The fin has a density of 2800 kg/m3, a specific heat of 880 J/kg-K and a thermal conductivity of 180 W/m-K. The surrounding air is considered compressible based on the Ideal Gas Law. By default it has a variable density, a molecular weight of 28.9664

kg/kg.mol, a specific heat of 1003.62 J/kg-K, a thermal conductivity of 0.0260305 W/m-K, and a molecular viscosity of 1.85508E-5 Pa-s. 1.Navigate to the Continua > Aluminum Alloy > Models > Solid > Al node. 2.Edit the Material Properties node and set the following properties: Node

Property Setting

Density > Constant

Value

2800 kg/m^3

Specific Heat > Constant

Value

880 J/kg-K

Thermal Conductivity > Constant Value

180 W/m-K

3.Save the simulation.

Setting Initial Conditions and Reference Values This part of the tutorial involves setting the direction and magnitude of the gravity vector and the reference density for the simulation. Start with the acceleration force in the negative y-direction. 1.Edit the Continua > Air > Reference Values node and set the following properties: Node

Property Setting

Gravity

Value

Reference Density Value

[0.0, -9.81, 0.0] m/s^2

1.27588 kg/m^3

2.Edit the Continua > Air > Initial Conditions > Static Temperature > Constant node and set Value to 293 K. 3.Edit the Continua > Aluminum Alloy > Initial Conditions > Static Temperature > Constant node and set Value to 343 K. This temperature is close to the final expected temperature of the solid region. 4.Save the simulation.

Creating Interfaces STAR-CCM+ requires the existence of an interface between all regions to transfer the appropriate mass and energy quantities during the calculation. For this example, create a contact-type interface between the fluid and solid regions. This procedure involves creating a so-called “in-place interface” between the wall boundaries

enclosing each of the two regions, and then defining this interface as being of an appropriate “contact” type for fluid-solid heat transfer. 1.Using the multi-select method, select the following nodes: Regions > Fluid > Boundaries > Air-Interface Regions > Solid > Boundaries > Fin-Interface 2.Create an in-place interface. This step creates the following new nodes: Fluid > Boundaries > Air-Interface [In-place 1] Solid > Boundaries > Fin-Interface [In-place 1] When you initialize the flow, these boundaries form the connection between the fluid and solid regions, superseding the original wall boundaries. In addition to the new in-place boundaries, a folder node named Interfaces appears in the object tree. It contains an interface node called In-place 1. 3.Edit the Interfaces > In-place 1 node and set the following properties: Property

Setting

Type

Contact Interface

Topology

In-place

4.Save the simulation.

Setting Boundary Conditions and Values The heated fin consists of an inverted “T” shape placed in a closed box. The only boundary specifications required for this analysis are wall thermal conditions. Apply a fixed temperature of 343 K to the base of the solid fin to provide the heat source. Set the vertical sides of the fluid-containing box to a fixed temperature of 293 K. All other wall boundary conditions are considered to be adiabatic. Use a contact-type conducting boundary at the solid-fluid interface. Start with the wall boundary definitions for the fluid region. 1.Navigate to the Regions > Fluid > Boundaries > Vertical-Walls > Physics Conditions node. 2.Select the Thermal Specification node and set Condition to Temperature. The temperature value for this boundary can now be set. 3.Select the Vertical-Walls > Physics Values > Static Temperature > Constant node and set Value to 293 K.

The conditions for the Horizontal-Walls boundary (upper and lower walls of the fluid region) can remain at the default adiabatic setting. You can now set the solid wall boundary conditions and values in a similar way to those of the fluid. 4.Navigate to the Regions > Solid > Boundaries > Fin-Bottom > Physics Conditions node. 5.Select the Thermal Specification node and set Method to Temperature. The temperature value for this boundary can now be set. 6.Select the Fin-Bottom > Physics Values > Static Temperature > Constant node and set Value to 343 K. 7.Save the simulation. Visualizing the Solution This part of the heated fin tutorial involves setting up a scene for displaying scalars and vectors of the solution. To view the temperature of the fluid and solid regions as the solution develops: 1.Create a scalar scene. This scene includes both the fluid and solid regions. 2.Set the scalar value to Temperature. The velocity vectors for the fluid can also be included in the scene by adding a vector displayer to the scalar scene. 3.Create a vector displayer. 4.Edit the Scenes > Vector Scene 1 > Displayers > Vector 1 > Parts node and select the fluid region. 5.Save the simulation. Reporting and Monitoring with Plots STAR-CCM+ can dynamically monitor virtually any quantity while the solution develops. To monitor a quantity, set up a report which defines the quantity of interest and the region parts to monitored. Define a monitor based on the report, which controls the update frequency and normalization characteristics. Finally, create an X-Y graph plot can from the monitor. Use a report monitor to track the heat flux at the interface of the heated fin and surrounding air: 1.Create a heat transfer report. 2.Edit the Reports > Heat Transfer 1 node and select the Solid > Boundaries > FinInterface [In-place 1] node. The setup for the report is now complete, and a monitor can be made from that report.

3.Create a monitor from the report. 4.Create a plot from the monitor 5.Save the simulation. Initializing and Running the Simulation To verify that the initial conditions for the regions are correct before you run the simulation, STAR-CCM+ allows you simply to perform solver initialization and then view the results using an appropriate scene. Use the following steps: 1.Initialize the simulation. 2.To see the initialization result, look at the scalar scene display.

Scalar scene—before running As the colors show, the solid fin is at 343 K while the surrounding air is at 293 K. The velocity value for each cell is 0. The simulation can now be run. 3.Run the simulation. 4.To watch the solution being updated while the simulation is running, look at the scalar scene display. 5.When the simulation has finished running, save it. Visualizing the Results After the solution finishes, you can examine results in plots and scenes. Click the tab of each display that you set up before the run.

1.To view the heat transfer variation at the solid-fluid interface, activate the Heat Transfer 1 Monitor Plot display. 2.To see the temperature and velocity vector results, click the tab for the Scalar Scene 1 display. By default, filled cell values are shown. To make the display smoother: 3.Select the Scenes > Scalar Scene 1 > Displayers > Scalar 1 node and set Contour Style to Smooth Filled. The contours of the scalar display now appear smooth as seen in the following zoomed-in screenshot. Additionally, the temperature solution of each region can be viewed by selecting the appropriate part. 4.Select the Displayers > Scalar 1 > Parts node and deselect the Fluid region.

Scalar Scene--Final

Experiment 5: Conjugate heat transfer AIM: To obtain velocity field around fin. Adding Streamlines In this part of the heated fin tutorial, use streamlines to depict flow paths. Streamlines can be added into any of the scalar or geometry scene plots with the creation of a “streamline” derived part. 1.Make the Geometry Scene 1 display active. 2.Create a new streamline derived part. 3.To select input parts, click Select. 4.In the object selector, select only the Fluid region. 5.In the Create Streamline panel, make the following settings: a.For the seed mode, select Line Seed. b.Activate the display tool option, and set the resolution to 15. The streamline line seed tool appears in the display. 6.Work with the tool in the scene as follows: a.Using the mouse buttons, zoom-in and position the part as shown below. b.Click the sphere at the end of the tool. c.Adjust the line so that it is approximately half a cell above the top of the solid fin. To adjust the line, simply grab the sphere and drag the mouse to its new position.

Placing the probe in between two cells 7.Click Create and then Close. 8.Click

(Reset View) in the toolbar.

The streamlines are generated and shown in the display.

9.Position the part as shown below.

Geometry Scene The streamline part can now be added to any suitable scene or be displayed in its own scene if desired. 10.Create a scalar scene. 11.Set the scalar value to Temperature. 12.By default, the regions Fluid and Solid are included in the scene. To display the streamlines only: a.Edit the Scenes > Scalar Scene 2 > Displayers > Scalar 1 > Parts node. b. Deselect the regions and select the derived part. 13. Edit the Scenes > Scalar Scene 2 > Displayers > Scalar 1 > Parts > Scalar Field node: a. Set Min to 300. b.Set Max to 343. Streamlines colored according to the local temperature appear in the Scalar Scene 2 display.

Second Scalar scene 14. Save the simulation.

Experiment 6: Flow through a pipe with sudden expansion AIM: To obtain stream lines Create a 3D-CAD model:

in a pipe with sudden expansion.

1.Launch STAR-CCM+. 2.Save the simulation under the name expp.sim. Launch 3D-CAD and create the geometry: 3.Right-click Geometry > 3D-CAD Models and select New. The 3D-CAD environment launches and a 3D-CAD model is created. Within 3D-CAD, an object

tree

that

is

specific

to

the

3D-CAD

model

is

displayed.

This

tree

contains Bodies, Features, and Design Parameters nodes. A 3D-CAD View scene is also created automatically. Initially, this scene displays three starting sketch planes which are used as a basis for adding features to the model. 4.Rename the 3D-CAD Model 1 node to expp.

Sketching the Cyclone Profile: Create a sketch that contains the profile of the cyclone chamber. Every 3D-CAD model contains three default sketch planes: XY, YZ, and ZX. Create a sketch on the YZ sketch plane: 1.Right-click the Features > YZ node and select Create Sketch. Creating a sketch activates sketch mode, in which a grid is displayed on the sketch plane in the 3D-CAD View scene, and the Sketch panel opens. This panel contains the tools for creating sketch entities, such as lines, circles, and arcs. The panel also allows you to control the settings for the grid that is displayed in the scene. Each sketch plane has local X and Y axes relative to the position and orientation of the plane in relation to the global coordinate system. 2.Click

(View normal to sketch plane) to align the sketch plane with the plane of the

screen. 3.Click

(Set sketch grid spacing) to specify the distance between the grid lines on the

sketch plane so that the spacing is suitable for the dimensions of the model geometry. 4.In the Grid Spacing dialog, set Grid Spacing to 0.025 m. 5.Click OK. Use the mouse to adjust the position, orientation, and zoom level of the sketch plane. 6. In the 3D-CAD View scene:

Left-click and drag the mouse in any direction to rotate the view. While holding down the key, click and drag to roll the view. Right-click and drag to pan the view. Middle-click and drag to zoom in or out. Alternatively, if your mouse has a scroll wheel, turn the mouse wheel to adjust the zoom level. 7.Click

(View normal to sketch plane) to realign the sketch plane with the screen.

8.Adjust the view in the 3D-CAD View scene so that the top half of the grid is shown. Leave some white space above the grid as the sketch will cover some of this space. 9.Click

(Create line) and move the mouse over the grid in the 3D-CAD View scene.

The mouse pointer has a blue square that is attached to it, which indicates the position of the point on the grid. The coordinates of this point are displayed in the Line Properties box of the Sketch panel, and change as you move the mouse. The

(Snap to Grid) option is

enabled by default, so the point jumps to an intersection between two grid lines as it is approaches them. Create the below given geometry with appropriate length and diameter as required.

10. The constraints and dimensions were added as per requirement. (Refer expt 1) 11. The construction line was added as shown in the above diagram. (Refer expt 1) 12. The profile was revolved using create revolve option. (Refer expt 1) 13. Design parameter if any was created for later modifications. (Refer expt 1) 14. The Inlet and Outlet of the Pipe was renamed by selecting. (Refer expt 1) 15. Simulation was saved. 16. A new geometry part was created. (refer expt 1)

17. Parts were assigned to each region. (refer expt 1) 18. Physics continuum was created and the required models for liquid as fluid was chosen. (refer expt 2) 19. The boundary conditions were specified. (refer expt 2)

Geometry scene after adding boundary conditions 20. A mesh continuum was created with required models as mentioned in expt 2 and a new mesh scene was created after generating the mesh volume. (refer expt 2)

Mesh Scene 21. A scalar scene was created with a section plane of desired coordinates. (refer expt 2) 22. Run the simulation and wait for iterations to complete. Save the simulation after running it.

Scalar scene

23. Streamlines was created and animated. (refer expt 3)

Streamlines NOTE: When Referring to the previous experiments, please don’t use the exact steps, but change as per your geometry and apply. NOTE: This experiment is same as the flow through sudden contraction experiment, but with inlet and outlet interchanged. NOTE: Set the velocity of the order 10-4 example 5*10-4. Only if velocity is less, the contraction can be observed in the streamlines scene.

Experiment 7: Flow through a pipe with sudden contraction AIM:

To obtain stream lines in a pipe with sudden contraction.

Create a 3D-CAD model: 1.Launch STAR-CCM+. 2.Save the simulation under the name contr.sim. Launch 3D-CAD and create the geometry: 3.Right-click Geometry > 3D-CAD Models and select New. The 3D-CAD environment launches and a 3D-CAD model is created. Within 3D-CAD, an object

tree

that

is

specific

to

the

3D-CAD

model

is

displayed.

This

tree

contains Bodies, Features, and Design Parameters nodes. A 3D-CAD View scene is also created automatically. Initially, this scene displays three starting sketch planes which are used as a basis for adding features to the model. 4.Rename the 3D-CAD Model 1 node to contr.

Sketching the Cyclone Profile: Create a sketch that contains the profile of the cyclone chamber. Every 3D-CAD model contains three default sketch planes: XY, YZ, and ZX. Create a sketch on the YZ sketch plane: 1.Right-click the Features > YZ node and select Create Sketch. Creating a sketch activates sketch mode, in which a grid is displayed on the sketch plane in the 3D-CAD View scene, and the Sketch panel opens. This panel contains the tools for creating sketch entities, such as lines, circles, and arcs. The panel also allows you to control the settings for the grid that is displayed in the scene. Each sketch plane has local X and Y axes relative to the position and orientation of the plane in relation to the global coordinate system. 2.Click

(View normal to sketch plane) to align the sketch plane with the plane of the

screen. 3.Click

(Set sketch grid spacing) to specify the distance between the grid lines on the

sketch plane so that the spacing is suitable for the dimensions of the model geometry. 4.In the Grid Spacing dialog, set Grid Spacing to 0.025 m.

5.Click OK. Use the mouse to adjust the position, orientation, and zoom level of the sketch plane. 6. In the 3D-CAD View scene: Left-click and drag the mouse in any direction to rotate the view. While holding down the key, click and drag to roll the view. Right-click and drag to pan the view. Middle-click and drag to zoom in or out. Alternatively, if your mouse has a scroll wheel, turn the mouse wheel to adjust the zoom level. 7.Click

(View normal to sketch plane) to realign the sketch plane with the screen.

8.Adjust the view in the 3D-CAD View scene so that the top half of the grid is shown. Leave some white space above the grid as the sketch will cover some of this space. 9.Click

(Create line) and move the mouse over the grid in the 3D-CAD View scene.

The mouse pointer has a blue square that is attached to it, which indicates the position of the point on the grid. The coordinates of this point are displayed in the Line Properties box of the Sketch panel, and change as you move the mouse. The

(Snap to Grid) option is

enabled by default, so the point jumps to an intersection between two grid lines as it is approaches them. Create the below given geometry with appropriate length and diameter as required.

10. The constraints and dimensions were added as per requirement. (Refer expt 1)

11. The construction line was added as shown in the above diagram. (Refer expt 1) 12. The profile was revolved using create revolve option. (Refer expt 1) 13. Design parameter if any was created for later modifications. (Refer expt 1) 14. The Inlet and Outlet of the Pipe was renamed by selecting. (Refer expt 1) 15. Simulation was saved. 16. A new geometry part was created. (refer expt 1) 17. Parts were assigned to each region. (refer expt 1) 18. Physics continuum was created and the required models for liquid as fluid was chosen. (refer expt 1) 19. The boundary conditions were specified. (refer expt 1)

Geometry scene after adding boundary conditions 20. A mesh continuum was created with required models as mentioned in expt 1 and a new mesh scene was created after generating the mesh volume. (refer expt 1)

Mesh Scene 21. A scalar scene was created with a section plane of desired coordinates. (refer expt 1) 22. Run the simulation and wait for iterations to complete. Save the simulation after running it.

Scalar scene 23. Streamlines was created and animated. (refer expt 1)

Streamlines NOTE: When Referring to the previous experiments, please don’t use the exact steps, but change as per your geometry and apply. NOTE: This experiment is same as the flow through sudden expansion, but with inlet and outlet interchanged. NOTE: Set the velocity of the order 10-4 example 5*10-4. Only if velocity is less, the contraction can be observed in the streamlines scene.

Experiment 8: Flow through annulus AIM: To obtain velocity profile Create a 3D-CAD model: 1.Launch STAR-CCM+.

in radial direction in the annulus.

2.Save the simulation under the name annulus.sim. Launch 3D-CAD and create the geometry: 3.Right-click Geometry > 3D-CAD Models and select New. The 3D-CAD environment launches and a 3D-CAD model is created. Within 3D-CAD, an object

tree

that

is

specific

to

the

3D-CAD

model

is

displayed.

This

tree

contains Bodies, Features, and Design Parameters nodes. A 3D-CAD View scene is also created automatically. Initially, this scene displays three starting sketch planes which are used as a basis for adding features to the model. 4.Rename the 3D-CAD Model 1 node to annulus.

Sketching the Cyclone Profile: Create a sketch that contains the profile of the cyclone chamber. Every 3D-CAD model contains three default sketch planes: XY, YZ, and ZX. Create a sketch on the YZ sketch plane: 1.Right-click the Features > YZ node and select Create Sketch. Creating a sketch activates sketch mode, in which a grid is displayed on the sketch plane in the 3D-CAD View scene, and the Sketch panel opens. This panel contains the tools for creating sketch entities, such as lines, circles, and arcs. The panel also allows you to control the settings for the grid that is displayed in the scene. Each sketch plane has local X and Y

axes relative to the position and orientation of the plane in relation to the global coordinate system. 2.Click

(View normal to sketch plane) to align the sketch plane with the plane of the

screen. 3.Click

(Set sketch grid spacing) to specify the distance between the grid lines on the

sketch plane so that the spacing is suitable for the dimensions of the model geometry. 4.In the Grid Spacing dialog, set Grid Spacing to 0.025 m. 5.Click OK. Use the mouse to adjust the position, orientation, and zoom level of the sketch plane. 6. In the 3D-CAD View scene: Left-click and drag the mouse in any direction to rotate the view. While holding down the key, click and drag to roll the view. Right-click and drag to pan the view. Middle-click and drag to zoom in or out. Alternatively, if your mouse has a scroll wheel, turn the mouse wheel to adjust the zoom level. 7.Click

(View normal to sketch plane) to realign the sketch plane with the screen.

8.Adjust the view in the 3D-CAD View scene so that the top half of the grid is shown. Leave some white space above the grid as the sketch will cover some of this space. 9.Click

(Create line) and move the mouse over the grid in the 3D-CAD View scene.

The mouse pointer has a blue square that is attached to it, which indicates the position of the point on the grid. The coordinates of this point are displayed in the Line Properties box of the Sketch panel, and change as you move the mouse. The

(Snap to Grid) option is

enabled by default, so the point jumps to an intersection between two grid lines as it is approaches them. Create the below given geometry with appropriate length and diameter as required.

10. The constraints and dimensions were added as per requirement. (Refer expt 1) 11. The construction line was added as shown in the above diagram. (Refer expt 1) 12. The profile was revolved using create revolve option. (Refer expt 1) 13. Design parameter if any was created for later modifications. (Refer expt 1) 14. The Inlet and Outlet of the Pipe was renamed by selecting. (Refer expt 1) 15. Simulation was saved. 16. A new geometry part was created. (refer expt 1) 17. Parts were assigned to each region. (refer expt 1) 18. Physics continuum was created and the required models for liquid as fluid was chosen. (refer expt 2) 19. The boundary conditions were specified. (refer expt 2)

Geometry scene after specifying boundary conditions 20. A mesh continuum was created with required models as mentioned in expt 2 and a new mesh scene was created after generating the mesh volume. (refer expt 2)

Mesh Scene 21. A scalar scene was created with a section plane of desired coordinates. (refer expt 2) 22. Run the simulation and wait for iterations to complete. Save the simulation after running it.

Scalar scene 23. Streamlines was created and animated. (refer expt 3)

Streamlines Creating Vector scene: 24.Create a new vector scene.

25.From derived part select new part then probe then line. A line is created along the axis. 26. It is adjusted to be cover only the cross sectional area as shown.

Line Probe

Adjusted Probe line 26.Under display, select existing displayer under which select vector 1.click on create. Vector line probe is created as shown below.

Vector scene NOTE: When referring to the previous experiments, please don’t use the exact steps, but change as per your geometry and apply. NOTE: Set the velocity of the order 10-4 example 5*10-4. Only if velocity is less, the contraction can be observed in the streamlines scene.

Experiment 9: 3D-CAD Modelling of S-Bend AIM: To create geometry model of S-Bend using 3D-CAD. Creating the S-Bend Geometry: Create a new simulation and use 3D-CAD to set up the geometry. Use the following steps: 1. Start up STAR-CCM+ in a manner that is appropriate to your working environment and create a New Simulation. 2. Save the new simulation to disk with the file name sBend.sim. The geometry is created using 3D-CAD, which is the parametric solid modeler available within STAR-CCM+.

3. To activate 3D-CAD, right-click the Geometry > 3D-CAD Models node and select New. Start by renaming the 3D-CAD model. 4. Rename the 3D-CAD Model 1 node to S-Bend.

Creating the Geometry Create the geometry of the s-bend pipe, including the circular inlet face. Use the following steps: 1. Create a sketch on the YZ plane by right-clicking the Features > YZ node and selecting Create Sketch. 2. Click

(Set sketch grid spacing) and change the Grid Spacing to 0.0025 m.

3. Click

(View normal to sketch plane) to bring the sketch plane into view.

4. Use the

(Create circle) tool to draw a circle with a radius of 0.01 m and whose center

is on the origin, position [0, 0]. 5. Click OK to exit the sketch. To create the profile of the pipe along its length: 6. Create a sketch on the XY plane. 7. Click 8. Use the

(View normal to sketch plane). (Create line) tool to draw a line of length 0.035 m starting at the origin and

extending in the positive x direction. 9. Press Esc to exit the line tool. 10. Use the

(Center point circular arc) tool to draw an arc with a radius of 0.02 m.

Three mouse clicks are required: a.Click position [0.035 m, 0.02 m] to define the center point. b.Click position [0.035 m, 0.0 m] to define the start point. c.Click position [0.055 m, 0.02 m] to define the end point. To create a second arc to complete the “S” shape: 11. Use the

(Center point circular arc) tool to create the second arc. The coordinates for

the three clicks are listed below: a.Center: [0.075 m, 0.02 m].

b.Start point: [0.075 m, 0.04 m]. c.End point: [0.055 m, 0.02 m]. Draw the final section of the pipe. 12. Draw a line with start point [0.075 m, 0.04 m] that extends 0.065 m in the positive x direction. 13. Click OK to exit the sketch. Create the solid body of the pipe using the sweep feature. A sweep requires two sketches: one to act as the profile being swept; the other to act as the path for the sweep. 14. Select both sketches from the 3D-CAD object tree, holding down the Shift key to select multiple items. 15. Right-click one of the highlighted nodes and select Create Sweep. The Sweep dialog appears. 16. Accept the default settings and click OK. A new body node, Body 1, is added below the Bodies node in the object tree. 17. Rename the Bodies > Body 1 node to Fluid. 18. Position the geometry as shown below. Specifying Inlet and Outlet Faces: The final step in preparing the model geometry is to specify the inlet and outlet faces of the model by setting face names. Use the following steps: 1. Zoom in to the pipe end, right-click the circular face and select Rename 2. Enter Inlet in the Rename dialog and click OK. The benefit of renaming the face in the 3D-CAD model is that it retains its unique identity when the 3D-CAD model is converted to a geometry part. To rename the outlet: 3. Position the geometry so that the outlet face on the other end of the pipe is visible. 4. Right-click the circular face at the other end of the pipe, select Rename, and enter Outlet in the Rename dialog. Click OK to complete the action. The geometry is now complete and you can exit 3D-CAD. 5. Click the Close 3D-CAD button at the bottom of the object tree. 6. Save the simulation. Creating a Geometry Part A new geometry part is created using the 3D-CAD model. Use the following stesp: 1. Right-click the Geometry > 3D-CAD Models > S-Bend node and select New Geometry Part.

2. Click OK to accept the default settings. 3. To see the surfaces, expand the Parts > Fluid > Surfaces node. The inlet and outlet faces in Specifying Inlet and Outlet Faces are defined as separate surfaces. Assigning a Part to a New Region Assign the geometry part to a region. The inlet and outlet surfaces have been renamed in 3D-CAD, and are automatically assigned to separate boundaries. 1. Right-click the Parts > Fluid node and select Assign Parts to Region. 2. In the Assign parts to region dialog set: Region Mode (top drop-down) to Create a Region for Each Part. Boundary Mode (middle drop-down) to Create a Boundary for Each Part Surface. 3. Click Apply and then Close. A new region has been created with boundaries defining the inlet, outlet, and main fluid volume. 4. Create a geometry scene. Use the mouse to rotate the model in the Graphics window to set up the view shown below.

Geometry scene-After assigning parts to region 5. Expand the Regions > Fluid > Boundaries node and select each of the boundary nodes to make sure that they have been specified correctly. Setting Up the Case

In this first part of the tutorial, run the simulation using a steady state laminar flow (Re = 500). By default, all boundaries are set to be walls. Modify the boundary type for the Inlet and Outlet: 1. Select the Regions > Fluid > Boundaries > Inlet node and set the Type to Velocity Inlet. The icon next to the Inlet boundary changes, indicating that it is now a velocity inlet boundary. 2. Select the Outlet boundary node and set the Type to Pressure Outlet. Generating a Surface Mesh Generate a polyhedral mesh using the generalized cylindrical mesher. This meshing model is suited to pipe flow. Define a prism layer mesh along the wall boundary, to assure that near wall effects are adequately resolved. 1. Right-click the Continua node and select New > Mesh Continuum. 2. Right-click the Mesh 1 > Models node and select the following models, in order: 3. Click Close. To define the mesh settings: 4. Select the Mesh 1 > Reference Values > Base Size node. 5. Set the Value to 0.0008 m. 6. Continuing with the reference values section, set the following properties Generate and check the surface mesh before running the generalized cylinder mesher. A good quality surface mesh is needed before the volume mesh can be generated. 7. Click

(Generate Surface Mesh).

8. Create a mesh scene and examine the surface mesh. Generating a Volume Mesh Before generating the volume mesh, define the boundaries that form the cylindrical geometry. Use the following steps: 1. Right-click the Mesh 1 > Models > Generalized Cylinder and select Manage Cylinders. 2. Make sure the Default cylinder is selected, then click OK. 3. Select the Regions > Fluid > Boundaries > Default > Mesh Conditions > Generalized Cylinder Extrusion Type node. Verify that the Extrusion law property was set to Constant. 4. Within the same Default boundary, select the Default > Mesh Values > Generalized Cylinder Parameters node. Notice that the Number of Layers property was set to 82. STAR-CCM+ calculates this value from the geometry model.

The volume mesh can now be generated. 5. Click the

(Generate Volume Mesh) button.

6. Right-click a blank space in Mesh Scene 1 and select Apply Representation > Volume Mesh. 7. Examine the final volume mesh.

Volume Mesh 8. Save the simulation.

Experiment 10: Analysis of flow through S-Bend AIM: To obtain velocity profile and stream line in the S-Bend. Selecting Physics Models Select the models for the incompressible fluid. A physics continuum was automatically created during the mesh generation process. To select the physics models: •

Right-click the Continua > Physics 1 > Models node and select the following models, in order: Group Box

Model

Time

Steady

Material

Gas

Flow

Segregated Flow

Equation of State Constant Density Viscous Regime

Laminar

2. Click Close. Modifying Material Properties Set the values for the dynamic viscosity and density of air. Use the following steps: 1. Select the Models > Gas > Air > Material Properties > Density > Constant node and set the Value to 1 Kg/m^3. 2. Select the Dynamic Viscosity > Constant node and set the Value to 1.716E-5 Pa-s. Setting Initial Conditions and Boundary Settings

To achieve a Reynolds number of 500 for this gas and pipe diameter, you require a mean velocity of 0.429 m/s. To assist solution convergence, define the initial condition for velocity: 1. Select the Physics 1 > Initial Conditions > Velocity > Constant node and set the Value to [0.429, 0.0, 0.0] m/s. Set the same velocity on the Inlet boundary. 2. Select the Regions > Fluid > Boundaries > Inlet > Physics Values > Velocity Magnitude > Constant node and set the Value to0.429 m/s. Preparing a Scalar Scene A scalar scene is created to show the velocity magnitude on a section plane through the center of the s-bend. Use this scene to visualize the solution while the simulation is running. Use the following steps: 1. Create a scalar scene. 2. Right-click the Derived Parts node and select New Part > Section > Plane 3. In the Create Section panel, set the following values 4.Click Create and then Close. 5. Click the scene/plot button. 6. Select the Displayers > Scalar 1 > Scalar Field node and set the Function to Velocity > Magnitude. 7. Select the Displayers > Scalar 1 node and set the Contour Style to Smooth Filled.

Scalar scene 8. Click the Simulation button to return to the STAR-CCM+ simulation object tree. A vector plot displaying the velocity magnitude is created.

9. Create a vector plot. 10. Using the drag-and-drop method, add the section plane from the Derived Parts node to the scene. Setting Up Stopping Criteria Limit the number of iterations for the solver to 500. 500 iterations are sufficient for the solution to converge. Use the following steps: 1. Select the Stopping Criteria > Maximum Steps node and set the Maximum Steps to 500. 2. Save the simulation. Running the Simulation The simulation is now ready to be run. Use the following steps: 1. Click

(Run).

While the simulation is running, you can click the tabs at the top of the Graphics window to view each of the scalar scenes. During the run, it is also possible to stop the process by clicking you do halt the simulation, it can be continued later by clicking

(Stop) on the toolbar. If (Run). If left alone, the

simulation continues until 500 iterations are complete. The Residuals display is created automatically and shows the progress of the solvers. 2. While the simulation is running, select the Scalar Scene 1 tab at the top of the Graphics window to visualize the solution. 3. When the simulation has finished running, save it. Visualizing the Results Examine the scalar and vector scenes. The scalar scene is shown below.

Scalar scene—Laminar

Vector Scene—Laminar Changing to a Turbulent Flow Edit the models, initial conditions, and boundary conditions to simulate a turbulent flow (Reynolds number = 50,000). First, save the state of the simulation as developed so far: • Save the simulation as sBendTurbulent.sim. Modifying the Physics Continuum Edit the physics models to represent turbulent flow. Disable the laminar model and enable the turbulent and K-epsilon models. 1. For the physics continuum Continua > Physics 1, deselect Laminar in the Enabled Models box.

2. Select the required models, in order. 3. Click Close. Modifying Initial Conditions and Boundary Settings To achieve a turbulent flow (Re = 50,000) in the existing pipe, increase the velocity of the air to 42.9 m/s at the Initial Conditions node and at the Inlet boundary condition. Change the Turbulence Specification so that the turbulence intensity and length scale can be defined. Use the following steps: 1. Select the Continuum > Physics 1 > Initial Conditions > Velocity > Constant node and set the Value to [42.9, 0.0, 0.0] m/s. 2. Select the Turbulence Specification node and set its Method to Intensity + Length Scale. The Turbulent Length Scale node is added to the object tree. 3.Set the following values:

Use the same values at the Inlet boundary. Start by setting the Turbulence Specification to use Intensity + Length Scale. 4. Select the Regions > Fluid > Boundaries > Inlet > Physics Conditions > Turbulence Specification node and set the Method toIntensity + Length Scale. 5.Set the following values: Node

Property

Value

Physics Values > Turbulent Length Scale> Constant

Value

0.0014 m

Regions > Fluid > Boundaries > Inlet >Physics Values

Velocity Magnitude > Constant

Value

42.9 m/s

Turbulence Intensity > Constant

Value

0.12

Extending the Stopping Criteria The turbulent flow requires a longer time to converge. Increasing the number of iterations to 1000 gives the solver sufficient time to converge. 1. Select the Stopping Criteria > Maximum Steps node and set the Maximum Steps to 1000. 2. Save the simulation. Clearing the Solution and Running the Simulation Clear the solution from the laminar flow before running the solver. Use the following steps: 1. Select Solution > Clear Solution from the menu. The Clear Solution dialog appears. 2. Accept the default settings and click OK. The simulation is now ready to be run. 3. Click

(Run).

4. While the simulation is running, select the Scalar Scene 1 tab at the top of the Graphics window to visualize the solution. 5. When the simulation has finished running, save it. Visualizing the Results for the Turbulent Flow

Scalar Scene—Turbulent

Vector scene--Turbulent