Computational Fluid Dynamics CFD

1
Computational Fluid Dynamics (CFD)

• Using Fluent
• a Brief Tutorial
• For ChFE 3353

2
Steps in CFD problem-solving (1)

• Preprocessing
• Create flowfield geometry combining straight
  lines, arcs, predefined 2D and 3D geometric
  elements
• Subdivide geometry into (small) computational
  volumes (mesh the flowfield)
• Specify fluid properties (e.g. m, r, cp),
  physical model (laminar, turbulent), presence of
  body forces (e.g. gravity), and boundary
  conditions (inlet velocity, flow rate, pressure
  drop, wall roughness)

3
Steps in CFD problem-solving (2)

• Processing
• Choose discretization accuracy
• Initialize properties (specify initial values
  for velocity, pressure, density at all mesh
  points)
• Set the convergence criteria
• Let the calculation run
• Babysit the calculation to see if it converges.
  If not, stop it, reinitialize properties or
  change model/accuracy/convergence criteria and
  let it run again

4
Steps in CFD problem-solving (3)

• Post-Processing
• Examine the results (often not trivial with tens
  of thousands of data points)
• Extract calculated numerical values, or evaluate
  derived values from CFD-generated ones
• Using your ingenuity and presentation skills,
  plot relevant properties and flowfield
  features(this is where CFD is often jokingly
  labeled
  Colorful Fluid Dynamics)

5
In practice

• Place ChFE ICC (MEB 2285) or CADE lab (WEB 210
  or 224)
• Computers Departmental PCs, CADE lab PCs or
  UNIX workstations
• Operating system Windows XP or SunOS (UNIX
  variant)
• Note if you want tutorial instructions for the
  UNIX version of Fluent, let me know
• Software
• Preprocessing GAMBIT
• Processing and postprocessing FLUENT
• Fluent and Gambit manuals are available online if
  you want more detail than is given in this
  tutorial (on PCs look under StartgtProgramsgtFluent
  IncgtFluent 6.0 Help)

6
Basic DOS Commands You Might Need

• Get DOS Command Prompt
• - StartgtProgramsgtAccessoriesgtCommand Prompt
• - or Startgtrungttype cmd and enter
• At DOS prompt
• To see the current folder contents dir
• To create folder mkdir new_folder_name
• To move to subfolder cd subfolder_name
• To move back to parent folder cd .. (no spaces
  between dots)
• To change drive, type drive letter followed by
  colon, e.g.
• To change to C drive C
• To change to T drive T

7
Gambit Tutorial

• (CFD Preprocessing)

8
Problem Statement

• Calculate the pressure drop for the Westfall 2300
  (10a) Venturi Meter

9
Initial Comments

• Disk space
• storage of your work
• Be sure you know where you are storing your files
• Store in your student file space, NOT on the hard
  disk of the computer you are using
• temp folder/directory for later backup, or
• If you store on the hard disk of the specific
  computer you are using, you will need to run your
  cases from the same machine next time
• or back up on flash drive/Zip disk

10
Run Gambit
Note While Gambit can be started from a desktop
shortcut, file management is easier if started
from a DOS prompt.

• First time only StartgtProgramsgtFluent IncgtSet
  Environment
• Get DOS command prompt Startgtrungt type cmd
• Change drive/directory to location where you will
  store files (for example to your space on T )
• Create folder to store specific problem files
• T\your_dirgt mkdir venturi
• Get into newly created folder
• T\your_dirgt cd venturi
• T\your_dir\venturigt
• Start Gambit
• T\your_dir\venturigt gambit venturi

11

• Select the solver (Gambit has different commands
  options for different solvers)

12
Create Geometry (1)
We will be creating the following shapes
Frustum (H0.126 Rb0.12 Rt0.06)
Frustum (truncated cone) (H0.335 Rb0.06
Rt0.12)
Cylinder (H0.08 R0.06)
Cylinder (H1.2 R0.12)
Cylinder (H1.2 R0.12)
13
Create Geometry (2)

• Select Operation Geometry
• Select Geometry Volume
• Select Volume type Cylinder(right-click the
  Create Volume button left-click the Cylinder
  button)

14
Create Geometry (3)

• Create the inlet cylinder
• (Type the data into appropriate fields and
  left-click Apply button)

Enter information here
Make selections here
15
Create Geometry (4)

• Create other 4 objects

Converging pipe
Throat
Diverging pipe
Outlet pipe
16
Create Geometry (5)

• Move object in place

• Select Move/Copy/Allign tool
• Pick the object to move
• (object lines will turn red)
• Specify whether to move or copy
• Specify the type of motion
• Specify the extent of motion
• Left-click Apply

converging
17
Create Geometry (6)

• Move the rest of objects in place

• Move throat_pipe by 1.326 in z-direction
• Move diverging_pipe by 1.406 in z-direction
• Move outlet_pipe by 1.741 in z-direction
• By now, you should have this

Note you can rotate the object using left mouse
button, zoom using the right mouse button, and
translate (slide) the object using the middle
button.
18
Create Geometry (7)

• Unite separate volumes into single flowfield

• Select Boolean Operations tool
• Left-click here to get the list of objects
• Left-click each object
• Left-click here
• Close the pick list
• Left-click Apply

19
Mesh the Geometry

• Select Mesh operation
• Select Mesh Volume
• Select Mesh Volumes
• Pick volume to mesh
• Choose mesh elements type
• Choose faces - inlet and outlet from which to
  create mesh (face outline will turn red in
  graphic window)
• Choose spacing
• Click Apply to mesh the volume

20
Name the Boundary Surfaces (1)

• Select Zones operation
• Select Specify Boundary Types command
• Pick the boundary surface
• Name the surface
• Select Surface Type
• Click Apply

Note Your face may be different from this one.
Selected face will be colored red in graphic
window.
21
Name the Boundary Surfaces (2)

• Repeat the previous step for outlet
• Pick the boundary surface
• Name the surface
• Select Surface Type
• Click Apply

Note Your face may be different from this one.
Selected face will be colored red in graphic
window.
22
Finish Up

• Save the Gambit file
• In main menu, select File Save
• If you need to open a previously-created Gambit
  file
• In main menu, select File Open
• (Note file type .dbs)
• Save the mesh in Fluent-readable format
• In main menu, select File Export Mesh
• Exit the Gambit program
• In main menu, select File Exit

23
Fluent tutorial

• Part 1 CFD processing

24
Running Fluent

• Be sure you have exited Gambit (there is a
  limited number of licenses)
• StartgtProgramsgtFluent IncgtFluent 6.0
• Version for the venturi problem 3d
• Note - it is possible to run more than one Fluent
  case at once however
• There is a limited number of licenses for use by
  the whole college be kind to your classmates
• Two cases running on one CPU will run half as
  fast as one case running on one CPU
• Moral unless you have a dual CPU machine, you
  are probably better off running one at a time

25
Importing mesh

• Read in the mesh fileFile Read CaseLocate
  your working folder (venturi in this case)
• In the list of files select the .msh file, than
  click OK
• Check the meshGrid CheckIf no error messages,
  mesh is OK
• Re-Scale the mesh into metric unitsGrid
  Scale(Dimensions for our grid are already in
  meters, so this step is not necessary for this
  problem)

26
Setting Simulation Parameters (1)

• Select viscosity modelDefine Models
  ViscousSelect k-epsilon (2 eqn), than click
  OK
• Set fluid propertiesDefine Materials
• Name water
• Density 998.2
• Viscosity 0.001002
• Click Change/Create button, than Close

27
Setting Simulation Parameters (2)

• Set boundary conditions
• Define Boundary Conditions
• Select inlet surface, and click Set button
• Enter 1.0 for Velocity Magnitude, than click OK
• Click Close button to close Boundary Conditions
  window
• Set initial values (Initialize the flowfield)
• Solve Initialize
• Enter 0.5 for z-velocity Click Init, than
  Close
• Set convergence criteria
• Solve Monitors Residuals
• Change convergence tolerance if necessary (for
  greater accuracy)
• Use 1.0e-5 for this problem for all residuals
  (note there are 6 residuals when using the k-e
  turbulence model)
• check Plot in Options (upper L.H. corner not
  the Plot button), than click OK

28
Running the Simulation

• Save the parameter set (the Case)
• File Write Case
• Check/change the filename, than click OK
• Start the simulation
• Solve Iterate
• Enter 1000 for Number of Iterations
• Click Iterate and watch the calculation progress

29
Finishing the processing phase

• Once the calculation is complete (message
  solution converged in main Fluent window)
• Save the parameters set and the calculated
  results
• File Write Case and Data
• Check/change the filename, than click OK
• Move on to analyzing results within Fluent
  (postprocessing) or exit Fluent

30
Fluent tutorial

• Part 2 CFD Postprocessing

31
Define a view plane
You can define as many planes as you want they
will be used to visualize the data computed
during the processing stage

• From main menu Surface Plane
• Identify a planar surface in your domain by
  determining any 3 defining points relative to the
  origin
• Enter the 3-D coordinates of those (or any) 3
  points in the plane
• Name the plane
• Click Create, than Close

32
Display velocity vectors

• From main menu choose Display Vectors
• Pick the scalar property to be used
• to color the vectors
• Pick a plane in the flowfield
• Click Display
• If necessary, rotate the image
• Using left mouse button, or
• Choosing from the main menu
• Display
• Views
• Left
• Restore
• Apply
• Note mouse controls are not exactly the same as
  Gambit. Can be changed using Display Mouse
  Buttons

33
Calculate the total pressure drop

• From main menu choose Report Surface
  Integrals
• Choose function to compute
• Choose the variable to integrate
• Choose the surface(s) for integration
• Click Compute
• We actually computed
• and
• Note 1 The above calculated Area-weighted
  average of the surface integral of pressure
  is the average pressure on that surface
• Note 2 Reported Net value is not pressure drop

34
Plot the static pressure changethrough the
venturi tube

• From main menu choose Plot XY Plot
• Choose the plot direction
• Choose the plot direction
• Choose the surface for plotting
• Click Plot

35
Printing graphics

• 1. Save graphics window contents to file
• From main menu choose File Hardcopy
• Choose the JPEG for Format
• Select Reverse Foreground/Background
• Choose 1200 x 800 for Resolution (or whatever you
  would like)
• Click Save, select filename, and click OK, than
  Close Graphics Hardcopy window
• 2. The resulting JPEG file can be imported into
  Word, Powerpoint, or whatever program you desire
  to use for presenting your results.