Tutorial: Simulating a 3D Check Valve Using Dynamic Mesh 6DOF Model And Diffusion Smoothing
|
|
- Job Cole
- 5 years ago
- Views:
Transcription
1 Tutorial: Simulating a 3D Check Valve Using Dynamic Mesh 6DOF Model And Diffusion Smoothing Introduction The purpose of this tutorial is to demonstrate how to simulate a ball check valve with small displacement using the dynamic mesh and 6DOF model in FLUENT. A pressure is applied at the valve inlet that pushes the valve and causes it to move due to the fluid forces applied on the valve. This tutorial uses the workbench workflow for solving the problem. As the displacement of the check valve ball in this case is small, a smoothing approach is suitable for this problem. In this tutorial, the diffusion smoothing algorithm is used. A pure hex mesh is used for this case since only smoothing is used. A dynamic mesh UDF is used to specify the mass properties of the valve for the 6DOF model. This tutorial demonstrates how to do the following: Prerequisites Set up a problem using the dynamic mesh model. Specify dynamic mesh modeling parameters. Specify a rigid body motion zone. Specify a deforming zone. Use the 6DOF model. Perform the calculation with residual plotting. Post process using CFD-Post This tutorial assumes that you are familiar with the FLUENT interface and have completed Tutorial 1 from the FLUENT 13.0 Tutorial Guide. You should also be familiar with the dynamic mesh model. Refer to Section 11.7: Steps in Using Dynamic Meshes in the FLUENT 13.0 User's Guide for more information on the use of the dynamic mesh model. ANSYS, Inc. January 15,
2 Problem Description The problem considered is shown schematically in Figure 1. Check valves are commonly used to enforce unidirectional flow of liquids and act as pressure-relieving devices. The check valve for this tutorial contains a ball connected to a spring with a stiffness constant of 300 N/m. The ball is made of steel with a density of 7800 kg/m3 and is represented as a cavity region in the mesh with a diameter of 4 mm. Initially the center of mass of the ball is located at the coordinate point (0, , 5e-05); this point is the spring origin, and all forces that interact with the ball are assumed to pass through this point. The tank region, located below the valve housing, is filled with Methanol (CH4O) at 25 C. High pressure from the liquid at the tank opening (2 atm) causes the ball to move up, thus allowing the fluid to escape through the valve to the atmosphere at an absolute pressure of 1 atm. The forces on the ball are: the force due to the spring (not shown in the figure) and the force due to fluid flow. Gravity is neglected here for simplicity. Figure 1: Problem schematic ANSYS, Inc. January 15,
3 The spring pushes the ball downward to oppose the force of the pressure when the ball is raised above its initial position. The pressure variation causes the ball to oscillate along the Y-axis as a result of a dynamic imbalance in the forces. The ball eventually stops oscillating when the forces acting on it are in equilibrium. In this tutorial the deformation of the ball itself is not modeled; mesh deformation is employed to modify the mesh as the ball moves. A rigid body simulation is used to predict the motion of the ball, and will be based on the forces that act on it (6DOF). Preparation 1. Open Workbench Unzip the project check_valve_diffusion_3d.wbpz by File -> Restore Archive 3. Double click on the Fluent Setup Cell Figure 2: Workbench project page ANSYS, Inc. January 15,
4 4. From the FLUENT launcher, start FLUENT. Setup and Solution Step 1: Mesh 1. The mesh is automatically read into Fluent and displayed in the graphics window. 2. Note that if you are using standalone Fluent, you can read in the mesh from the File menu: File -> Read -> Mesh. The mesh file for this project can be accessed by navigating the project files to "check_valve_diffusion_3d_files\dp0\fff\mech". The mesh file is named FFF.msh. Figure 3: Fluent window and mesh display 3. Check the mesh by clicking on Mesh -> Check 4. FLUENT will perform various checks on the mesh and report the progress in the console. Make sure that the minimum volume reported is a positive number. ANSYS, Inc. January 15,
5 5. Change the pressure units to atm from Pa (a) Define -> Units (b) Pick pressure in the "Quantities" window (c) Pick atm as the unit (d) Close 6. Note that Most of the Fluent settings can be accessed by navigating the setup tree on the left in the Fluent Window Step 2: General Settings Problem Setup -> General Settings 1. Enable time-dependent calculations. (e) Select Transient from the Time list. ANSYS, Inc. January 15,
6 Figure 4: General settings Step 3: Models Problem Setup -> Models -> Viscous 1. Enable the standard k-epsilon model with standard wall functions. Figure 5: Models options ANSYS, Inc. January 15,
7 Figure 6: Viscous models window Step 4: Materials Problem Setup -> Materials 1. Create/Edit -> Fluent Data Base (a) Pick methyl-alcohol-liquid (b) Copy, Close 2. Close the Materials panel. ANSYS, Inc. January 15,
8 Figure 7: Materials panel Step 5: Cell Zone Conditions Problem Setup -> Cell Zone Conditions 1. Pick each cell zone listed and click Create/Edit 2. In the pop up window, make sure that the material selected is methyl-alcohol-liquid and not air Step 6: Boundary Conditions Problem Setup -> Boundary Conditions In this step, you will set the inlet and outlet conditions. 1. Define boundary conditions for the inlet zone. ANSYS, Inc. January 15,
9 (a) Pick the boundary named as "inlet" and switch the Type to pressure-inlet (b) Enter 2(atm) to be the Gauge total pressure (c) Switch the direction specification method to be Normal to Boundary (d) Select Intensity and Viscosity Ratio from the Specification Method drop-down list (e) In the Turbulence group box, set Turbulent Intensity to 5% and Turbulent Viscosity Ratio to 10%. (f) Click OK to close the Velocity Inlet panel. 2. Similarly pick the outlet zone and click Edit (a) Select Intensity and Viscosity Ratio from the Specification Method drop-down list (b) In the Turbulence group box, set Turbulent Intensity to 5% and Turbulent Viscosity Ratio to 10%. (c) Click OK to close the pressure outlet panel. 3. Close the Boundary Conditions panel. Figure 8: Inlet boundary conditions panel ANSYS, Inc. January 15,
10 Step 7: Compile the UDF Note that the tutorial project has the UDF libraries included. The UDF has been compiled in serial on Windows 64 bit machine. To run the tutorial on any other hardware specification, it needs to be recompiled. A 6DOF UDF is used in this example. The DEFINE_SDOF_PROPERTIES macro is used to assign the mechanical properties of the check valve. The motion of the valve is automatically calculated by Fluent from the forces acting on the valve. You will need a c-compiler installed on your machine to be able to compile UDFs. Define -> User Defined -> Functions -> Compiled 1. Click the Add... button in the Source Files group box. 2. The Select File dialog will open. 3. Browse to the folder "check_valve_diffusion_3d_files\dp0\fff\fluent". Select the file check_valve_motion.c and click OK to close the Select File dialog. 4. Click Build to build the library. 5. FLUENT will set up the directory structure and compile the code. The compilation will be displayed in the console. 6. Click Load to load the library. 7. Close the Compiled UDFs panel. ANSYS, Inc. January 15,
11 Figure 9: Compiled UDF panel Step 8: Mesh Motion Setup 1. Enable dynamic mesh motion and specify the associated parameters. (a) Problem Setup -> Dynamic Mesh (b) Enable Dynamic Mesh in the Models group box. (c) Enable Smoothing in the Mesh Methods group box and Six DOF in the Options. (d) Make sure that the Layering and Remeshing options are disabled. (e) Click on Mesh Method Settings to open the Mesh Method Settings panel. Switch method to Diffusion in the Smoothing tab. (f) Click OK to close the Dynamic Mesh Parameters panel. ANSYS, Inc. January 15,
12 Figure 10: Dynamic mesh settings 2. Specify the motion of the check valve ball ANSYS, Inc. January 15,
13 (a) Click on Create/Edit in the Dynamic Mesh Panel. (b) Select ball from the Zone Names drop-down list. (c) Retain the selection of Rigid Body in the Type list. (d) Select spring_check_valve::libudf from the Six DOF UDF drop-down list. (e) Enter Center of Gravity location of the ball as (X, Y, Z) = (0.0, , 5.0e-5) m (f) Make sure the Six DOF Options is turned to On (g) Click Create. Figure 11: Settings for 6DOF ball valve ANSYS, Inc. January 15,
14 (h) FLUENT will create the dynamic zone valve which will be available in the Dynamic Zones list. 3. Specify the motion of the symmetry 1. (a) Select symmetry1 from the Zone Names drop-down list. (b) Select Deforming from the Type list. (c) Click the Meshing Options tab and set the following parameters: (d) Enable Smoothing and disable remeshing in the Methods group box. (e) Retain the default settings for the remaining parameters. (f) Click Create. (g) FLUENT will create the dynamic zone axis1 which will be available in the Dynamic Zones list. 4. Do the same for symmetry2select axis2 from the Zone Names drop-down list. 5. Close the Dynamic Mesh Zones panel. 6. Save the project. Step 9: Solution In a dynamic mesh simulation, the mesh changes are saved in the case files. At any point in the solution, to revert the mesh back to original settings and to start calculation from beginning, close Fluent and click on the Settings cell again in the project page. This will re-launch Fluent with the original mesh but with all the saved settings. To re-start a calculation, always launch Fluent from the Solution cell. This reads in the latest Fluent case and data file. 1. Request saving of case and data files every 25 time steps. (a) Solution -> Calculation Activities -> Autosave (b) Enter 25 for both Autosave Case File Frequency and Autosave Data File Frequency. Clicking on Edit makes more options available. (c) Click OK to close the Autosave panel. ANSYS, Inc. January 15,
15 Note: Fluent case and data files can also be read by CFD-Post for post processing but in the interests of minimizing hard disk space, you have the option to write out light weight files of only the variables that you are interested in for Post processing by following these steps:calculation Activities > Automatic Export > Create > Solution Data Export. Choose file type to be CFD-Post compatible. Select Frequency, give a file name, select variables to post process 2. Solution -> Solution Methods (a) Switch P-V Coupling Scheme to Coupled (b) Switch Spatial Discretization Scheme for Pressure to PRESTO! 3. Retain the default solution control parameters at Solution -> Solution Controls 4. Enable the plotting of residuals during the calculation. (a) Solution -> Monitors -> Residual (b) Enable Plot in the Options group box. (c) Click OK to close the Residual Monitors panel. 5. Initialize the flow field (a) Solution-> Solution Initialization -> Initialize (b) Set TKE value to 0.1. (c) Click Initialize and close the Solution Initialization panel. 6. Save the project. Saving the project after initialization saves the settings file and the first case file. Any subsequent changes to the settings during the run will write out case files appended with an integer number corresponding to the change in settings you make. Resetting any cell in the Workbench project will clear all the corresponding files from the directory. 7. Run the calculation for 150 time steps. (a) Solution -> Run Calculation -> Iterate (b) Enter 5e-5 s for Time Step Size. (c) Enter 150 for Number of Time Steps. (d) Click Iterate. ANSYS, Inc. January 15,
16 (e) Close the Iterate panel. Postprocessing Figure 12: Residual plot You have two options for post processing. One is to use the Fluent post processor Results -> Graphics and Animations/ Plots/ Reports. The other is to use CFD-Post. When you are dealing with transient data and wish to create animations/ plots, CFD-Post offers features that may not be available in Fluent Post. So long as you have written out data files at a frequency, CFD-Post can read in those files and create animations, transient monitors without pre-setting these at the beginning of your simulation. For details on using Fluent Post, please refer tutorial X. Step 1: Launch CFD-Post 1. Close Fluent and double click on the Results cell in workbench. This launches CFD-Post with the last.cas and.dat file read in automatically. ANSYS, Inc. January 15,
17 1. Click on "z-axis" in the display window to see front view of geometry. 2. Click on the clock icon on the menu. This will show the transient sequence of files that has been loaded. (a) Double click on any Step to display results at that time step. Figure 13: Time step selector to display results at any saved simulation time Step 2: Display velocity contours: 1. Insert Contour from the menu. Insert -> Contour 2. Give a name to the contour 3. In the contour details, select location to be symmetry1 tank and symmetry1 valve. 4. Select variable to be velocity ANSYS, Inc. January 15,
18 5. Click apply. This displays the velocity contours in the display window. Note: Other variable contours (e.g Static Pressure etc.) can be set up in similar fashion. As further practice, please try setting up velocity vectors by Insert -> Vector. The Insert menu has also different options such as inserting text, legends and so on. New planes or surfaces for display of data can be created by Insert -> Location. Any feature (contours, vectors, particle tracks) that have been inserted can be turned on or off in the display by clicking on the check box next to the feature. Figure 14: Velocity contours at 1s of flow time Step 3: Creating animations 6. We will animate the mesh deformation. For this, first uncheck the contours created in previous step. ANSYS, Inc. January 15,
19 7. Display the mesh on symmetry1 tank and symmetry1 valve. For this, check the box next to the required locations in the loaded data file boundaries displayed in the tree view on the left. 8. Double click on symmetry1 tank. This brings up the details panel on the left bottom corner of CFD-Post. 9. In the "Render" tab check the box next to "Show Mesh Lines". This displays the mesh in symmetry 1 tank. 10. Do the same for symmetry1 valve. ANSYS, Inc. January 15,
20 Figure 15: Displaying mesh on symmetry planes 11. Click on the animation icon. This brings up the animation panel. 12. Select Time steps as the object to animate. 13. You can adjust the slider to make the animation fast or slow. 14. Clicking on the downfacing arrow brings up a few more details. 15. Check the box next to "Save Movie". 16. Browse to the required folder and give a name. 17. Then click on the play button. 18. This animates the mesh motion and save it into a wmv file. The animation file format is flexible and many options are available. ANSYS, Inc. January 15,
21 Figure 16: Animation panel in CFD-Post 19. Contours, iso-surfaces, streamlines etc. can be animated in similar fashion. Step 4: Creating transient XY plots 1. Create a point on a node attached to the check valve 2. Insert -> Location -> Point 3. Check the box adjacent to the boundary called "ball" in the tree view of the loaded data file on the left Figure 17: Displaying the ball valve and creating a point ANSYS, Inc. January 15,
22 4. In the point details window, set method to be "XYZ" and click on the co-ordinates window 5. You can now pick your XYZ location with your mouse pointer on the 3D viewer. Select a point on the Valve close to the top 6. Clicking "Apply" in the point details displays the nearest node location to the selected XYZ location 7. Switch Domains to "valve" 8. Now, switch the method to Node Number and enter the node number obtained from previous step. This will ensure that the point is hooked to the mesh node. If the node is displaced by mesh motion, the point is displaced as well. Click "Apply" Figure 18: Point details menu 9. From the Insert menu, select Insert -> Chart. 10. In the details of the chart, set type to be "XY-Transient or sequence". Enter a title for the chart. 11. Go to the "Data Series" tab. Under Data Source, pick Point 1 as the location. ANSYS, Inc. January 15,
23 12. Under "Y Axis" tab, pick X as the plot variable and click apply 13. The transient variation of the node location defined by Point 1 is plotted on a chart in the chart window. Figure 19: Tracking the motion of the valve (point attachhed to node on valve) in x- direction Note: Instead of a point, create a line location. XY solution data can be plotted on the line to analyze your result. Step 5: Automatic Reports 1. Right click on the 3D viewer and select "Copy to New Figure". The figure is automatically inserted into the automatically generated report. 2. Any charts that were created are also inserted automatically into the report. ANSYS, Inc. January 15,
24 3. Click on the Report viewer tab on the bottom to access the automatically generated report. Step 6: Expressions CFD-Post allows creation of expressions to evaluate quantitative data from flow results. The expressions can also be used to create XY plot and creating tables. 1. Select the Expression tab on the top left. 2. Right click on Expressions and click on "New" Figure 20: Creating expressions 3. Enter a name for the Expression 4. Right click on the blank details panel that opens up 5. This opens up the CEL expressions drop down list. All the accessible functions, expressions, variables, boundary locations and constants are listed 6. Choose functions -> CFD-Post -> massflow 7. The CEL syntax for massflow is inserted as massflow()@ 8. With the mouse pointer resting after symbol, Choose Locations -> outlet 9. The entire syntax for calculation mass flow at the boundary named as the outlet is massflow()@outlet ANSYS, Inc. January 15,
25 10. Click Apply to see the calculated value in the box 11. Expressions can be used in XY plots, tables and in creating custom variables. Figure 21: Writing CEL expressions Step 7: Custom Variables 1. Create another expression for velocity magnitude as sqrt(velocity u^2+velocity v^2+velocity w^2). 2. This can be done as in previous step by right click on the details window and selecting from the menu that opens up. Flow variable names are listed under "Variables". ANSYS, Inc. January 15,
26 3. Go to the Variable tab 4. Right click in the window, click on New 5. Enter a name for the custom variable (e.g VelMag) > ok 6. In the details window, under Expressions select the expression for velocity magnitude that you created 7. Apply 8. This creates a new flow variable called VelMag that can be used in contour plots and so on just like any other flow variables. Step 8: Creating Tables 1. Insert -> Table 2. This opens the table viewer 3. Click on any cell in the table. Entries in the table (text etc.) can be typed in the entry box that appears. 4. Functions, expressions etc. can be inserted in the table by selecting relevant data from the drop down lists that appear at the top. Figure 22: Using the table viewer ANSYS, Inc. January 15,
27 Figure 23: Case comparison Step 9: Case Comparison (a) Go back to the 3D viewer and display the velocity contours. (b) You may have to turn on the contour you inserted in Step 2. (c) Now load one of the data files in the sequence again by File -> Load Results and navigating to check_valve_diffusion_3d_file\dp0\fff\fluent and picking FFF dat.gz (d) Now you will see the two Cases listed in the tree view on the left as Case 1 and Case 2 (e) Double click on Case Comparison, which is the first item in the tree. ANSYS, Inc. January 15,
28 Summary (f) In the Details menu that appears, you can now pick Case 1 and Case 2 as required. The entire time history is available to pick. (g) Double click on Step 150 for Case 1 and Step 50 for Case 2. (h) Apply. (i) This shows the contours plotted on Case 1, Case 2 and the difference between the two in the viewer on the right. In this tutorial, you used the diffusion smoothing option for the dynamic mesh feature in FLUENT. The motion was limited to small distances. 6DOF model was used to calculate valve motion under the action of fluid forces. Post processing is shown using CFD-Post to detail some of the features of the post processing tool. ANSYS, Inc. January 15,
Use 6DOF solver to calculate motion of the moving body. Create TIFF files for graphic visualization of the solution.
Introduction The purpose of this tutorial is to provide guidelines and recommendations for setting up and solving a moving deforming mesh (MDM) case along with the six degree of freedom (6DOF) solver and
More informationCalculate a solution using the pressure-based coupled solver.
Tutorial 19. Modeling Cavitation Introduction This tutorial examines the pressure-driven cavitating flow of water through a sharpedged orifice. This is a typical configuration in fuel injectors, and brings
More informationTutorial: Hydrodynamics of Bubble Column Reactors
Tutorial: Introduction The purpose of this tutorial is to provide guidelines and recommendations for solving a gas-liquid bubble column problem using the multiphase mixture model, including advice on solver
More informationUsing Multiple Rotating Reference Frames
Tutorial 10. Using Multiple Rotating Reference Frames Introduction Many engineering problems involve rotating flow domains. One example is the centrifugal blower unit that is typically used in automotive
More informationAuto Injector Syringe. A Fluent Dynamic Mesh 1DOF Tutorial
Auto Injector Syringe A Fluent Dynamic Mesh 1DOF Tutorial 1 2015 ANSYS, Inc. June 26, 2015 Prerequisites This tutorial is written with the assumption that You have attended the Introduction to ANSYS Fluent
More informationUsing the Eulerian Multiphase Model for Granular Flow
Tutorial 21. Using the Eulerian Multiphase Model for Granular Flow Introduction Mixing tanks are used to maintain solid particles or droplets of heavy fluids in suspension. Mixing may be required to enhance
More informationUsing a Single Rotating Reference Frame
Tutorial 9. Using a Single Rotating Reference Frame Introduction This tutorial considers the flow within a 2D, axisymmetric, co-rotating disk cavity system. Understanding the behavior of such flows is
More informationTutorial: Riser Simulation Using Dense Discrete Phase Model
Introduction The purpose of this tutorial is to demonstrate the setup of a dense discrete phase model (DDPM) with the example of 2D riser. DDPM is used for the secondary phase that has a particle size
More informationModeling Evaporating Liquid Spray
Tutorial 17. Modeling Evaporating Liquid Spray Introduction In this tutorial, the air-blast atomizer model in ANSYS FLUENT is used to predict the behavior of an evaporating methanol spray. Initially, the
More informationSimulation of Flow Development in a Pipe
Tutorial 4. Simulation of Flow Development in a Pipe Introduction The purpose of this tutorial is to illustrate the setup and solution of a 3D turbulent fluid flow in a pipe. The pipe networks are common
More informationSimulation of Laminar Pipe Flows
Simulation of Laminar Pipe Flows 57:020 Mechanics of Fluids and Transport Processes CFD PRELAB 1 By Timur Dogan, Michael Conger, Maysam Mousaviraad, Tao Xing and Fred Stern IIHR-Hydroscience & Engineering
More informationUsing Multiple Rotating Reference Frames
Tutorial 9. Using Multiple Rotating Reference Frames Introduction Many engineering problems involve rotating flow domains. One example is the centrifugal blower unit that is typically used in automotive
More informationTutorial: Modeling Liquid Reactions in CIJR Using the Eulerian PDF transport (DQMOM-IEM) Model
Tutorial: Modeling Liquid Reactions in CIJR Using the Eulerian PDF transport (DQMOM-IEM) Model Introduction The purpose of this tutorial is to demonstrate setup and solution procedure of liquid chemical
More informationModeling Unsteady Compressible Flow
Tutorial 4. Modeling Unsteady Compressible Flow Introduction In this tutorial, FLUENT s density-based implicit solver is used to predict the timedependent flow through a two-dimensional nozzle. As an initial
More informationFlow in an Intake Manifold
Tutorial 2. Flow in an Intake Manifold Introduction The purpose of this tutorial is to model turbulent flow in a simple intake manifold geometry. An intake manifold is a system of passages which carry
More informationExpress Introductory Training in ANSYS Fluent Workshop 07 Tank Flushing
Express Introductory Training in ANSYS Fluent Workshop 07 Tank Flushing Dimitrios Sofialidis Technical Manager, SimTec Ltd. Mechanical Engineer, PhD PRACE Autumn School 2013 - Industry Oriented HPC Simulations,
More informationThis tutorial illustrates how to set up and solve a problem involving solidification. This tutorial will demonstrate how to do the following:
Tutorial 22. Modeling Solidification Introduction This tutorial illustrates how to set up and solve a problem involving solidification. This tutorial will demonstrate how to do the following: Define a
More informationAppendix: To be performed during the lab session
Appendix: To be performed during the lab session Flow over a Cylinder Two Dimensional Case Using ANSYS Workbench Simple Mesh Latest revision: September 18, 2014 The primary objective of this Tutorial is
More informationSimulation and Validation of Turbulent Pipe Flows
Simulation and Validation of Turbulent Pipe Flows ENGR:2510 Mechanics of Fluids and Transport Processes CFD LAB 1 (ANSYS 17.1; Last Updated: Oct. 10, 2016) By Timur Dogan, Michael Conger, Dong-Hwan Kim,
More informationModeling Evaporating Liquid Spray
Tutorial 16. Modeling Evaporating Liquid Spray Introduction In this tutorial, FLUENT s air-blast atomizer model is used to predict the behavior of an evaporating methanol spray. Initially, the air flow
More informationTutorial 1. Introduction to Using FLUENT: Fluid Flow and Heat Transfer in a Mixing Elbow
Tutorial 1. Introduction to Using FLUENT: Fluid Flow and Heat Transfer in a Mixing Elbow Introduction This tutorial illustrates the setup and solution of the two-dimensional turbulent fluid flow and heat
More informationSolving FSI Applications Using ANSYS Mechanical and ANSYS Fluent
Workshop Transient 1-way FSI Load Mapping using ACT Extension 15. 0 Release Solving FSI Applications Using ANSYS Mechanical and ANSYS Fluent 1 2014 ANSYS, Inc. Workshop Description: This example considers
More informationThe purpose of this tutorial is to illustrate how to set up and solve a problem using the. Moving Deforming Mesh (MDM) using the layering algorithm.
Tutorial: Introduction The purpose of this tutorial is to illustrate how to set up and solve a problem using the following two features in FLUENT. Moving Deforming Mesh (MDM) using the layering algorithm.
More informationModeling Flow Through Porous Media
Tutorial 7. Modeling Flow Through Porous Media Introduction Many industrial applications involve the modeling of flow through porous media, such as filters, catalyst beds, and packing. This tutorial illustrates
More informationSolution Recording and Playback: Vortex Shedding
STAR-CCM+ User Guide 6663 Solution Recording and Playback: Vortex Shedding This tutorial demonstrates how to use the solution recording and playback module for capturing the results of transient phenomena.
More informationSimulation of Turbulent Flow over the Ahmed Body
1 Simulation of Turbulent Flow over the Ahmed Body ME:5160 Intermediate Mechanics of Fluids CFD LAB 4 (ANSYS 18.1; Last Updated: Aug. 18, 2016) By Timur Dogan, Michael Conger, Dong-Hwan Kim, Maysam Mousaviraad,
More informationLab 9: FLUENT: Transient Natural Convection Between Concentric Cylinders
Lab 9: FLUENT: Transient Natural Convection Between Concentric Cylinders Objective: The objective of this laboratory is to introduce how to use FLUENT to solve both transient and natural convection problems.
More informationUsing the Discrete Ordinates Radiation Model
Tutorial 6. Using the Discrete Ordinates Radiation Model Introduction This tutorial illustrates the set up and solution of flow and thermal modelling of a headlamp. The discrete ordinates (DO) radiation
More informationCold Flow Simulation Inside an SI Engine
Tutorial 12. Cold Flow Simulation Inside an SI Engine Introduction The purpose of this tutorial is to illustrate the case setup and solution of the two dimensional, four stroke spark ignition (SI) engine
More informationVerification of Laminar and Validation of Turbulent Pipe Flows
1 Verification of Laminar and Validation of Turbulent Pipe Flows 1. Purpose ME:5160 Intermediate Mechanics of Fluids CFD LAB 1 (ANSYS 18.1; Last Updated: Aug. 1, 2017) By Timur Dogan, Michael Conger, Dong-Hwan
More informationSimulating Sinkage & Trim for Planing Boat Hulls. A Fluent Dynamic Mesh 6DOF Tutorial
Simulating Sinkage & Trim for Planing Boat Hulls A Fluent Dynamic Mesh 6DOF Tutorial 1 Introduction Workshop Description This workshop describes how to perform a transient 2DOF simulation of a planing
More informationSimulation of Turbulent Flow around an Airfoil
Simulation of Turbulent Flow around an Airfoil ENGR:2510 Mechanics of Fluids and Transfer Processes CFD Pre-Lab 2 (ANSYS 17.1; Last Updated: Nov. 7, 2016) By Timur Dogan, Michael Conger, Andrew Opyd, Dong-Hwan
More informationIntroduction to CFX. Workshop 2. Transonic Flow Over a NACA 0012 Airfoil. WS2-1. ANSYS, Inc. Proprietary 2009 ANSYS, Inc. All rights reserved.
Workshop 2 Transonic Flow Over a NACA 0012 Airfoil. Introduction to CFX WS2-1 Goals The purpose of this tutorial is to introduce the user to modelling flow in high speed external aerodynamic applications.
More informationNon-Newtonian Transitional Flow in an Eccentric Annulus
Tutorial 8. Non-Newtonian Transitional Flow in an Eccentric Annulus Introduction The purpose of this tutorial is to illustrate the setup and solution of a 3D, turbulent flow of a non-newtonian fluid. Turbulent
More informationFLUENT Secondary flow in a teacup Author: John M. Cimbala, Penn State University Latest revision: 26 January 2016
FLUENT Secondary flow in a teacup Author: John M. Cimbala, Penn State University Latest revision: 26 January 2016 Note: These instructions are based on an older version of FLUENT, and some of the instructions
More informationExpress Introductory Training in ANSYS Fluent Workshop 08 Vortex Shedding
Express Introductory Training in ANSYS Fluent Workshop 08 Vortex Shedding Dimitrios Sofialidis Technical Manager, SimTec Ltd. Mechanical Engineer, PhD PRACE Autumn School 2013 - Industry Oriented HPC Simulations,
More informationRevolve 3D geometry to display a 360-degree image.
Tutorial 24. Turbo Postprocessing Introduction This tutorial demonstrates the turbomachinery postprocessing capabilities of FLUENT. In this example, you will read the case and data files (without doing
More informationSupersonic Flow Over a Wedge
SPC 407 Supersonic & Hypersonic Fluid Dynamics Ansys Fluent Tutorial 2 Supersonic Flow Over a Wedge Ahmed M Nagib Elmekawy, PhD, P.E. Problem Specification A uniform supersonic stream encounters a wedge
More informationExpress Introductory Training in ANSYS Fluent Workshop 06 Using Moving Reference Frames and Sliding Meshes
Express Introductory Training in ANSYS Fluent Workshop 06 Using Moving Reference Frames and Sliding Meshes Dimitrios Sofialidis Technical Manager, SimTec Ltd. Mechanical Engineer, PhD PRACE Autumn School
More informationCompressible Flow in a Nozzle
SPC 407 Supersonic & Hypersonic Fluid Dynamics Ansys Fluent Tutorial 1 Compressible Flow in a Nozzle Ahmed M Nagib Elmekawy, PhD, P.E. Problem Specification Consider air flowing at high-speed through a
More informationMiddle East Technical University Mechanical Engineering Department ME 485 CFD with Finite Volume Method Fall 2017 (Dr. Sert)
Middle East Technical University Mechanical Engineering Department ME 485 CFD with Finite Volume Method Fall 2017 (Dr. Sert) ANSYS Fluent Tutorial Developing Laminar Flow in a 2D Channel 1 How to use This
More informationIsotropic Porous Media Tutorial
STAR-CCM+ User Guide 3927 Isotropic Porous Media Tutorial This tutorial models flow through the catalyst geometry described in the introductory section. In the porous region, the theoretical pressure drop
More informationTutorial 17. Using the Mixture and Eulerian Multiphase Models
Tutorial 17. Using the Mixture and Eulerian Multiphase Models Introduction: This tutorial examines the flow of water and air in a tee junction. First you will solve the problem using the less computationally-intensive
More informationWorkbench Tutorial Minor Losses, Page 1 Tutorial Minor Losses using Pointwise and FLUENT
Workbench Tutorial Minor Losses, Page 1 Tutorial Minor Losses using Pointwise and FLUENT Introduction This tutorial provides instructions for meshing two internal flows. Pointwise software will be used
More informationANSYS AIM Tutorial Turbulent Flow Over a Backward Facing Step
ANSYS AIM Tutorial Turbulent Flow Over a Backward Facing Step Author(s): Sebastian Vecchi, ANSYS Created using ANSYS AIM 18.1 Problem Specification Pre-Analysis & Start Up Governing Equation Start-Up Geometry
More informationVerification and Validation of Turbulent Flow around a Clark-Y Airfoil
1 Verification and Validation of Turbulent Flow around a Clark-Y Airfoil 1. Purpose ME:5160 Intermediate Mechanics of Fluids CFD LAB 2 (ANSYS 19.1; Last Updated: Aug. 7, 2018) By Timur Dogan, Michael Conger,
More informationExpress Introductory Training in ANSYS Fluent Workshop 02 Using the Discrete Phase Model (DPM)
Express Introductory Training in ANSYS Fluent Workshop 02 Using the Discrete Phase Model (DPM) Dimitrios Sofialidis Technical Manager, SimTec Ltd. Mechanical Engineer, PhD PRACE Autumn School 2013 - Industry
More informationA B C D E. Settings Choose height, H, free stream velocity, U, and fluid (dynamic viscosity and density ) so that: Reynolds number
Individual task Objective To derive the drag coefficient for a 2D object, defined as where D (N/m) is the aerodynamic drag force (per unit length in the third direction) acting on the object. The object
More informationPrerequisites: This tutorial assumes that you are familiar with the menu structure in FLUENT, and that you have solved Tutorial 1.
Tutorial 22. Postprocessing Introduction: In this tutorial, the postprocessing capabilities of FLUENT are demonstrated for a 3D laminar flow involving conjugate heat transfer. The flow is over a rectangular
More informationTutorial 2. Modeling Periodic Flow and Heat Transfer
Tutorial 2. Modeling Periodic Flow and Heat Transfer Introduction: Many industrial applications, such as steam generation in a boiler or air cooling in the coil of an air conditioner, can be modeled as
More informationIntroduction to ANSYS CFX
Workshop 03 Fluid flow around the NACA0012 Airfoil 16.0 Release Introduction to ANSYS CFX 2015 ANSYS, Inc. March 13, 2015 1 Release 16.0 Workshop Description: The flow simulated is an external aerodynamics
More informationANSYS AIM Tutorial Steady Flow Past a Cylinder
ANSYS AIM Tutorial Steady Flow Past a Cylinder Author(s): Sebastian Vecchi, ANSYS Created using ANSYS AIM 18.1 Problem Specification Pre-Analysis & Start Up Solution Domain Boundary Conditions Start-Up
More informationNovember c Fluent Inc. November 8,
MIXSIM 2.1 Tutorial November 2006 c Fluent Inc. November 8, 2006 1 Copyright c 2006 by Fluent Inc. All Rights Reserved. No part of this document may be reproduced or otherwise used in any form without
More informationµ = Pa s m 3 The Reynolds number based on hydraulic diameter, D h = 2W h/(w + h) = 3.2 mm for the main inlet duct is = 359
Laminar Mixer Tutorial for STAR-CCM+ ME 448/548 March 30, 2014 Gerald Recktenwald gerry@pdx.edu 1 Overview Imagine that you are part of a team developing a medical diagnostic device. The device has a millimeter
More informationSIMCENTER 12 ACOUSTICS Beta
SIMCENTER 12 ACOUSTICS Beta 1/80 Contents FEM Fluid Tutorial Compressor Sound Radiation... 4 1. Import Structural Mesh... 5 2. Create an Acoustic Mesh... 7 3. Load Recipe... 20 4. Vibro-Acoustic Response
More informationSimulation of Turbulent Flow over the Ahmed Body
Simulation of Turbulent Flow over the Ahmed Body 58:160 Intermediate Mechanics of Fluids CFD LAB 4 By Timur K. Dogan, Michael Conger, Maysam Mousaviraad, and Fred Stern IIHR-Hydroscience & Engineering
More informationTUTORIAL#4. Marek Jaszczur. Turbulent Thermal Boundary Layer on a Flat Plate W1-1 AGH 2018/2019
TUTORIAL#4 Turbulent Thermal Boundary Layer on a Flat Plate Marek Jaszczur AGH 2018/2019 W1-1 Problem specification TUTORIAL#4 Turbulent Thermal Boundary Layer - on a flat plate Goal: Solution for Non-isothermal
More informationSimulation of Turbulent Flow around an Airfoil
1. Purpose Simulation of Turbulent Flow around an Airfoil ENGR:2510 Mechanics of Fluids and Transfer Processes CFD Lab 2 (ANSYS 17.1; Last Updated: Nov. 7, 2016) By Timur Dogan, Michael Conger, Andrew
More informationSteady Flow: Lid-Driven Cavity Flow
STAR-CCM+ User Guide Steady Flow: Lid-Driven Cavity Flow 2 Steady Flow: Lid-Driven Cavity Flow This tutorial demonstrates the performance of STAR-CCM+ in solving a traditional square lid-driven cavity
More informationModeling Supersonic Jet Screech Noise Using Direct Computational Aeroacoustics (CAA) 14.5 Release
Modeling Supersonic Jet Screech Noise Using Direct Computational Aeroacoustics (CAA) 14.5 Release 2011 ANSYS, Inc. November 7, 2012 1 Workshop Advanced ANSYS FLUENT Acoustics Introduction This tutorial
More informationTutorial: Modeling Domains with Embedded Reference Frames: Part 2 Sliding Mesh Modeling
Tutorial: Modeling Domains with Embedded Reference Frames: Part 2 Sliding Mesh Modeling Introduction The motion of rotating components is often complicated by the fact that the rotational axis about which
More informationTutorial: Heat and Mass Transfer with the Mixture Model
Tutorial: Heat and Mass Transfer with the Mixture Model Purpose The purpose of this tutorial is to demonstrate the use of mixture model in FLUENT 6.0 to solve a mixture multiphase problem involving heat
More informationModule D: Laminar Flow over a Flat Plate
Module D: Laminar Flow over a Flat Plate Summary... Problem Statement Geometry and Mesh Creation Problem Setup Solution. Results Validation......... Mesh Refinement.. Summary This ANSYS FLUENT tutorial
More informationSTAR-CCM+ User Guide 6922
STAR-CCM+ User Guide 6922 Introduction Welcome to the STAR-CCM+ introductory tutorial. In this tutorial, you explore the important concepts and workflow. Complete this tutorial before attempting any others.
More informationProblem description. The FCBI-C element is used in the fluid part of the model.
Problem description This tutorial illustrates the use of ADINA for analyzing the fluid-structure interaction (FSI) behavior of a flexible splitter behind a 2D cylinder and the surrounding fluid in a channel.
More informationand to the following students who assisted in the creation of the Fluid Dynamics tutorials:
Fluid Dynamics CAx Tutorial: Channel Flow Basic Tutorial # 4 Deryl O. Snyder C. Greg Jensen Brigham Young University Provo, UT 84602 Special thanks to: PACE, Fluent, UGS Solutions, Altair Engineering;
More informationAdvanced ANSYS FLUENT Acoustics
Workshop Modeling Flow-Induced (Aeroacoustic) Noise 14.5 Release Advanced ANSYS FLUENT Acoustics 2011 ANSYS, Inc. November 7, 2012 1 Introduction This tutorial demonstrates how to model 2D turbulent flow
More informationAutomotive Fluid-Structure Interaction (FSI) Concepts, Solutions and Applications. Laz Foley, ANSYS Inc.
Automotive Fluid-Structure Interaction (FSI) Concepts, Solutions and Applications Laz Foley, ANSYS Inc. Outline FSI Classifications FSI Solutions FSI Modeling Approaches ANSYS Workbench for FSI System
More informationDMU Engineering Analysis Review
DMU Engineering Analysis Review Overview Conventions What's New? Getting Started Entering DMU Engineering Analysis Review Workbench Generating an Image Visualizing Extrema Generating a Basic Analysis Report
More informationand to the following students who assisted in the creation of the Fluid Dynamics tutorials:
Fluid Dynamics CAx Tutorial: Pressure Along a Streamline Basic Tutorial #3 Deryl O. Snyder C. Greg Jensen Brigham Young University Provo, UT 84602 Special thanks to: PACE, Fluent, UGS Solutions, Altair
More informationDMU Engineering Analysis Review
Page 1 DMU Engineering Analysis Review Preface Using This Guide Where to Find More Information Conventions What's New? Getting Started Inserting a CATAnalysis Document Using DMU Space Analysis From CATAnalysis
More informationTUTORIAL#3. Marek Jaszczur. Boundary Layer on a Flat Plate W1-1 AGH 2018/2019
TUTORIAL#3 Boundary Layer on a Flat Plate Marek Jaszczur AGH 2018/2019 W1-1 Problem specification TUTORIAL#3 Boundary Layer - on a flat plate Goal: Solution for boudary layer 1. Creating 2D simple geometry
More informationRBF Morph An Add-on Module for Mesh Morphing in ANSYS Fluent
RBF Morph An Add-on Module for Mesh Morphing in ANSYS Fluent Gilles Eggenspieler Senior Product Manager 1 Morphing & Smoothing A mesh morpher is a tool capable of performing mesh modifications in order
More informationSwapnil Nimse Project 1 Challenge #2
Swapnil Nimse Project 1 Challenge #2 Project Overview: Using Ansys-Fluent, analyze dependency of the steady-state temperature at different parts of the system on the flow velocity at the inlet and buoyancy-driven
More informationModeling External Compressible Flow
Tutorial 3. Modeling External Compressible Flow Introduction The purpose of this tutorial is to compute the turbulent flow past a transonic airfoil at a nonzero angle of attack. You will use the Spalart-Allmaras
More informationWall thickness= Inlet: Prescribed mass flux. All lengths in meters kg/m, E Pa, 0.3,
Problem description Problem 30: Analysis of fluid-structure interaction within a pipe constriction It is desired to analyze the flow and structural response within the following pipe constriction: 1 1
More informationShape optimisation using breakthrough technologies
Shape optimisation using breakthrough technologies Compiled by Mike Slack Ansys Technical Services 2010 ANSYS, Inc. All rights reserved. 1 ANSYS, Inc. Proprietary Introduction Shape optimisation technologies
More informationFirst Steps - Conjugate Heat Transfer
COSMOSFloWorks 2004 Tutorial 2 First Steps - Conjugate Heat Transfer This First Steps - Conjugate Heat Transfer tutorial covers the basic steps to set up a flow analysis problem including conduction heat
More informationSimCafe. ANSYS WB - Airfoil - Setup (Physics) Added by Benjamin J Mullen, last edited by Benjamin J Mullen on Apr 29, :18
Page 1 of 5 Search Cornell SimCafe Home Edit Browse/Manage Login Simulation > > ANSYS WB - Airfoil - Setup (Physics) Search ANSYS WB - Airfoil - Setup (Physics) Added by Benjamin J Mullen, last edited
More informationANSYS AIM Tutorial Flow over an Ahmed Body
Author(s): Sebastian Vecchi Created using ANSYS AIM 18.1 ANSYS AIM Tutorial Flow over an Ahmed Body Problem Specification Start Up Geometry Import Geometry Enclose Suppress Mesh Set Mesh Controls Generate
More informationAero-Vibro Acoustics For Wind Noise Application. David Roche and Ashok Khondge ANSYS, Inc.
Aero-Vibro Acoustics For Wind Noise Application David Roche and Ashok Khondge ANSYS, Inc. Outline 1. Wind Noise 2. Problem Description 3. Simulation Methodology 4. Results 5. Summary Thursday, October
More informationFirst Steps - Ball Valve Design
COSMOSFloWorks 2004 Tutorial 1 First Steps - Ball Valve Design This First Steps tutorial covers the flow of water through a ball valve assembly before and after some design changes. The objective is to
More informationWorkbench Tutorial Flow Over an Airfoil, Page 1 ANSYS Workbench Tutorial Flow Over an Airfoil
Workbench Tutorial Flow Over an Airfoil, Page 1 ANSYS Workbench Tutorial Flow Over an Airfoil Authors: Scott Richards, Keith Martin, and John M. Cimbala, Penn State University Latest revision: 17 January
More informationTryItNow! Step by Step Walkthrough: Spoiler Support
TryItNow! Step by Step Walkthrough: Spoiler Support 1 2015 ANSYS, Inc. March 28, 2016 TryItNow! Step by Step Walkthrough: Spoiler Support ANSYS designed this TryItNow! experience to give you quick access
More informationWorkshop 3: Cutcell Mesh Generation. Introduction to ANSYS Fluent Meshing Release. Release ANSYS, Inc.
Workshop 3: Cutcell Mesh Generation 14.5 Release Introduction to ANSYS Fluent Meshing 1 2011 ANSYS, Inc. December 21, 2012 I Introduction Workshop Description: CutCell meshing is a general purpose meshing
More informationequivalent stress to the yield stess.
Example 10.2-1 [Ansys Workbench/Thermal Stress and User Defined Result] A 50m long deck sitting on superstructures that sit on top of substructures is modeled by a box shape of size 20 x 5 x 50 m 3. It
More informationIntroduction to ANSYS FLUENT Meshing
Workshop 04 CAD Import and Meshing from Conformal Faceting Input 14.5 Release Introduction to ANSYS FLUENT Meshing 2011 ANSYS, Inc. December 21, 2012 1 I Introduction Workshop Description: CAD files will
More informationExpress Introductory Training in ANSYS Fluent Workshop 04 Fluid Flow Around the NACA0012 Airfoil
Express Introductory Training in ANSYS Fluent Workshop 04 Fluid Flow Around the NACA0012 Airfoil Dimitrios Sofialidis Technical Manager, SimTec Ltd. Mechanical Engineer, PhD PRACE Autumn School 2013 -
More informationIn this problem, we will demonstrate the following topics:
Z Periodic boundary condition 1 1 0.001 Periodic boundary condition 2 Y v V cos t, V 1 0 0 The second Stokes problem is 2D fluid flow above a plate that moves horizontally in a harmonic manner, schematically
More informationComputational Fluid Dynamics autumn, 1st week
Computational Fluid Dynamics 2016 autumn, 1st week 1 Tamás Benedek benedek [at] ara.bme.hu www.ara.bme.hu/~benedek/cfd/icem The most important rule: Dont use space or specific characters in: File names,
More informationStep 1: Create Geometry in GAMBIT
Step 1: Create Geometry in GAMBIT If you would prefer to skip the mesh generation steps, you can create a working directory (see below), download the mesh from here (right click and save as pipe.msh) into
More informationLecture 5 Two-way FSI Solving and Post Processing. Solving FSI Applications Using ANSYS Mechanical and ANSYS CFX Release. Release 14.
Lecture 5 Two-way FSI Solving and Post Processing 14. 5 Release Solving FSI Applications Using ANSYS Mechanical and ANSYS CFX 1 2011 ANSYS, Inc. July 26, 2013 Outline Solution Process Here we discuss starting
More informationc Fluent Inc. May 16,
Tutorial 1. Office Ventilation Introduction: This tutorial demonstrates how to model an office shared by two people working at computers, using Airpak. In this tutorial, you will learn how to: Open a new
More informationNaysEddy ver 1.0. Example MANUAL. By: Mohamed Nabi, Ph.D. Copyright 2014 iric Project. All Rights Reserved.
NaysEddy ver 1.0 Example MANUAL By: Mohamed Nabi, Ph.D. Copyright 2014 iric Project. All Rights Reserved. Contents Introduction... 3 Getting started... 4 Simulation of flow over dunes... 6 1. Purpose of
More informationBioIRC solutions. CFDVasc manual
BioIRC solutions CFDVasc manual Main window of application is consisted from two parts: toolbar - which consist set of button for accessing variety of present functionalities image area area in which is
More informationThe second part of the tutorial continues with the subsequent ANSYS Mechanical simulation steps:
Tutorial: Simulation of aero-vibro-acoustic phenomena using ANSYS Fluent and ANSYS Mechanical. Test case: Noise inside a cavity with a vibrating wall, caused by the external turbulent flow. Introduction
More informationIntroduction to ANSYS Fluent Meshing
Workshop 06: Mesh Creation Including Removal of Gaps and Baffle Thickness 14.5 Release Introduction to ANSYS Fluent Meshing 1 2011 ANSYS, Inc. December 21, 2012 I Introduction Workshop Description: Fluent
More informationThe viscous forces on the cylinder are proportional to the gradient of the velocity field at the
Fluid Dynamics Models : Flow Past a Cylinder Flow Past a Cylinder Introduction The flow of fluid behind a blunt body such as an automobile is difficult to compute due to the unsteady flows. The wake behind
More informationWorkshop 1: Basic Skills
Workshop 1: Basic Skills 14.5 Release Introduction to ANSYS Fluent Meshing 2011 ANSYS, Inc. December 21, 2012 1 I Introduction Workshop Description: This workshop shows some of the clean up tools in Tgrid
More informationDam removed at start of analysis. Air g = 9.8. Water SI units used. Water: Air: = 10, = Slip walls are used to model the basin.
Problem description It is desired to analyze the motion of water within a basin. Initially, the basin contains a dam, and the water is confined by the dam as shown. At the start of the analysis, the dam
More information