Express Introductory Training in ANSYS Fluent Workshop 08 Vortex Shedding

Transcription

1 Express Introductory Training in ANSYS Fluent Workshop 08 Vortex Shedding Dimitrios Sofialidis Technical Manager, SimTec Ltd. Mechanical Engineer, PhD PRACE Autumn School Industry Oriented HPC Simulations, September 21-27, University of Ljubljana, Faculty of Mechanical Engineering, Ljubljana, Slovenia 2012 ANSYS, Inc. September 19, Release 14.5

2 Workshop 7b Vortex Shedding 14.5 Release Introduction to ANSYS Fluent 2012 ANSYS, Inc. September 19, Release 14.5

3 I Introduction Workshop Description: The purpose of this workshop is to introduce good techniques for transient flow modeling. Learning Aims: This workshop teaches skills for running Fluent for time dependant (transient) simulations. Topics covered include: Selecting a suitable timestep. Using Custom Field Functions (CFF). Auto saving results during the simulation. Generating Fast Fourier Transforms (FFT). Generating images during the simulation. Transient post processing in CFD Post. Learning Objectives: To show how to set up, run and post process a transient (time dependant) simulation, as well as additional skills in using custom field functions and Fast Fourier Transforms ANSYS, Inc. September 19, Release 14.5

4 Simulation to be Performed The case considered here is flow around a cylinder with a Reynolds number of 100. Vortex shedding will be observed. However the workshop starts with a steady state analysis assuming that the user didn t anticipate this behavior. This workshop demonstrates iterative and non iterative time advancement, Fast Fourier Transforms (FFT) and animations. The tutorial is carried out using Fluent and CFD Post in standalone mode ANSYS, Inc. September 19, Release 14.5

5 Computational Domain Computational domain created in ANSYS DesignModeler has the following dimensions. Name Location Dimension Cylinder D1 2 m (dia.) Inlet Length D2 20 m = 10 D Outlet Length D3 30 m = 15 D Width D4 40 m = 20 D 2012 ANSYS, Inc. September 19, Release 14.5

6 Reynolds Number Effects Re < 5 Creeping flow (no separation) < Re < 40 A pair of stable vortices in the wake. 40 < Re < 150 Laminar vortex street. 150 < Re < < Re < Laminar boundary layer up to the separation point, turbulent wake. Boundary layer transition to turbulent. Re> Turbulent vortex street, but the separation is narrower than the laminar case ANSYS, Inc. September 19, Release 14.5

7 Start a Fluent Project (Standalone) Launch Fluent from the Start Menu: "Start Menu>ANSYS 14.5>Fluid Dynamics>Fluent". Select "2D" Display Mesh After Reading. Select the working directory you are using on your machine (may be different to that shown here) ANSYS, Inc. September 19, Release 14.5

8 Mesh [1] Read the Fluent mesh file: "vortex shedding coarse.msh" ("File>Read>Mesh"). The mesh will be read in and displayed, and the zones will be shown in the TUI window ANSYS, Inc. September 19, Release 14.5

9 Mesh [2] The mesh needs scaling. Select "Scale" ("Problem Setup>General>Scale"), and enter the values shown, then press "Scale". Be careful only to press "Scale" only once. Final domain extent. Close the scale panel and "Check" the Mesh. "General>Check". "General>Report Quality". Display the grid again once scaling has been performed. "General>Display" ANSYS, Inc. September 19, Release 14.5

10 Select "General" in the navigation pane and keep the "Steady State" "Pressure Based" solver. Keep "Laminar" setting for the "Viscous Model". The properties to be used for the material "air" need to be set. For "Density", enter "1 (kg/m3)". For "Viscosity", enter "0.01 (kg/m s)". Select "Change/Create". Solver & Models Later on we will compare the Fluent results with those from a literature search. We have changed the default material properties for air to aid that comparison ANSYS, Inc. September 19, Release 14.5

11 Boundary Conditions. "Inlet": Boundary Conditions/Solution Methods Select boundary "in". Set velocity to be "1 [m/s]" "normal" to boundary. "Outlet": Select boundary "out". Keep default of "0 [Pa]". "Other boundaries": "cylinder" is set to a "wall", no action needed. "sym1" and "sym2" are set to "symmetry", no action needed. Solution Methods. Select "QUICK" scheme for "Momentum" equation ANSYS, Inc. September 19, Release 14.5

12 Solution Monitor Set up residual monitors so the convergence can be monitored. "Monitors>Residuals>Edit". Make sure "Plot" is on, then "OK". Create points to monitor quantity. "Surface (top menu)>point". Specify coordinates (2, 1). "Activate" point tool to check location on the grid. (check out point tool before closing panel). "Create" then "Close". Surface monitor on point. "Monitors>Surface Monitors>Create". Select "Vertex Average" on report type and "Velocity" "Y velocity" in field variable. Select "point 6" (the point created above at co ordinates [2,1]). Options: "Print to Console" & "Plot", then "OK" ANSYS, Inc. September 19, Release 14.5

13 Solution Initialization Initialize the flow field based on the far field boundary. Select "Standard Initialization" "Compute from" "in" (inlet zone). "Initialize". Save the case file. "File>Write Case". You can write case and data files with extension.gz, the files will be compressed automatically ANSYS, Inc. September 19, Release 14.5

14 Run Calculation [1] Set the number of requested iterations to "400" then "Calculate". We have tried to solve this vortex shedding problem in a steady state manner. Note that solution is not converging and monitor shows a regular periodic behavior ANSYS, Inc. September 19, Release 14.5

15 Run Calculation [2] Choose Graphics and "Animations>Vectors". Since this is a 2D simulation, there is no need to pick a surface, just "Display". Steady state solution is asymmetric ANSYS, Inc. September 19, Release 14.5

16 Save Case&Data Files and Make Transient Save the Case&Data files. "File>Write Case&Data". You can write case and data files with extension.gz the files will be compressed automatically. To obtain a more realistic solution to this problem we will solve it again, but in a transient (time dependant) manner. Under "Problem Setup>General", change the time option to "Transient" ANSYS, Inc. September 19, Release 14.5

17 Run Calculation For the transient scheme, it is recommended to change Solver Methods. The default pressure velocity coupling (SIMPLE) may require more iterations to converge. Change to the "PISO" scheme and "2 nd Order Implicit" "Transient Formulation" as shown in the image below. Also change the "Under Relaxation Factors" as shown in the image ANSYS, Inc. September 19, Release 14.5

18 Edit the Surface monitor. Solution Monitor Change "Get Data Every" to "Time Step". Also set the "X Axis" to be "Time Step". "OK" 2012 ANSYS, Inc. September 19, Release 14.5

19 Run Calculation [1] Save the transient case file before starting the computation. We need to identify a suitable time step size for this problem. 1) A quick way is to do a hand calculation to see how long it takes for the flow to pass through a typical grid cell. Run this, and check that convergence occurs in less that 20 iterations per timestep. 2) Another approach is to determine the characteristic response of the system. By performing a literature search, we believe that for this problem, the Strouhal number will be approximately at this Reynolds number. From this, we can predict the period of the oscillation: St fd 1 D period 6. s V f St. V 06 For each oscillation cycle, we will aim to solve 60 timesteps. Hence we will run the solver using a timestep size of 0.1s ANSYS, Inc. September 19, Release 14.5

20 Run Calculation [2] Specify "Time Step" ("0.1 s") and "Number of Time Steps" ("120'). Click on the "Extrapolate Variables" option. "Calculate" the solution. Use this option to change the display to show both output Windows. The "Extrapolate Variables" option will speed up convergence. Without this option, each timestep would start with the solution at the previous timestep. This option provides a better starting point for the new timestep based on how the solution is changing with time. Notice that as the solver runs, convergence is attained in 5 10 iterations at each timestep ANSYS, Inc. September 19, Release 14.5

21 Run Calculation [3] Save the transient case&data files. Note if you add the string %t to the filename ("vortex shedding transient %t.gz") then Fluent will append the current time value to the filename. Note also that this file just contains the results at the current timestep. If you require interim results as the solution progresses, use the "Autosave" feature prior to running the model. We will do this shortly. Although we now have simulated a couple of oscillations, in order to obtain a true representation of the vortex shedding we need to simulate many more cycles. With each cycle, the "starting position" converges with time until eventually all cycles are identical. It will take many cycles to achieve this, so we have provided case and data files that has already been converged (simulation time of 84secs). You will then run this on for a further couple of cycles to extract the detail of the fluctuating flow patterns. So, read in the supplied Case and Data file: "vortex shedding converged.cas.gz" and ".dat.gz" ANSYS, Inc. September 19, Release 14.5

22 NITA Enable the "Non Iterative Time Advancement Method" (NITA). With "Fractional Step" for "Pressure Velocity Coupling". NITA is an algorithm used to speed up the transient solution process. NITA runs about twice as fast as the ITA scheme. NITA scheme reduce the splitting error to O(Δt 2 ) by using sub iterations per time step. 2 Overall time discretization error for 2 nd order scheme: O(Dt 2 ) Truncation error: O(Dt 2 ) = + Splitting error (due to eqn segregation): O(Dt n ) Two flavors of NITA schemes available. - PISO (NITA/PISO). - Fractional step method (NITA/FSM). About 20% cheaper than NITA/PISO on a per time step basis ANSYS, Inc. September 19, Release 14.5

23 Result Analysis Save the transient case&data files. One of the ways of quantifying the wake vortices is through the use of the "Q Criterion". The formula for this is below. It is not a standard quantity computed by Fluent, however since we know the formula, we can ask Fluent to compute it at each grid cell. U V U V Q. x y y x "Define>Custom Field Functions" Select solver quantities using the pull down list at the right hand side to construct this function as shown, then press "Define" ANSYS, Inc. September 19, Release 14.5

24 Extracting Transient Data Unless specifically requested, Fluent will not save interim results during a transient simulation. There are two ways you may want to consider doing this: 1) Saving the results data every (n) timesteps to disk. This will give a collection of files that can be post processed at a later date, either using Fluent or CFD Post. However having to load in a large number of files can be time consuming. 2) The alternative is to extract the required result (like an image from which to build an animation) from Fluent during the solution process. Since all the data is in memory at that instant, this is very quick to perform. We will do both in this example ANSYS, Inc. September 19, Release 14.5

25 To save interim results: Save Interim Results Select "Calculation Activities", and save "Every 5 Time Steps". Press "Edit", and specify the name of the file to be saved. Note that the file name will be appended with the current time value (e.g. "transient detail dat.gz"). "OK" ANSYS, Inc. September 19, Release 14.5

26 Saving Images On The Fly [1] Select "Calculation Activities>Solution Animation>Create/Edit". Increase "Number of Sequences" to "1". "Sequence 1", "Every" "2 Time Steps". "Define", which will open the "Animation Sequence" window. Set "Window to 3", press "Set" to enable this window, and "Display Type" to "Contours". Continued on next slide ANSYS, Inc. September 19, Release 14.5

27 Saving Images On The Fly [2] Set up the contour panel as shown in the image below, then "Display". Set the graphics window to display screen "3". Draw a zoom box with the middle mouse button to zoom in on the cylinder. Note that the file name will be appended with the current time value. Close the contour panel, then "OK" to both panels opened on previous slide ANSYS, Inc. September 19, Release 14.5

28 Solution Monitors Edit the Surface monitor again. Check the box next to "Write" and specify a name for the file. This type of file can be used for Fourier Transform analysis. "OK" ANSYS, Inc. September 19, Release 14.5

29 Run the calculation: Run Calculation for Creating Animation Use a smaller timestep for NITA (0.05s). Solve for 240 Time Steps. Calculate (this corresponds to roughly 2 periods). Save the Case and Data File. Remember that if you add the string %t to the filename ("vortex shedding transient %t.gz") then Fluent will append the current time value to the filename ANSYS, Inc. September 19, Release 14.5

30 Post Processing (Fluent) [1] To run the animation (Graphics and Animation in the navigation pane on the left, then choose Solution Animation Playback and Set Up ) Use the Play button to view a movie of the series of images. If required, this can be written out as an mpeg movie ANSYS, Inc. September 19, Release 14.5

31 From the Plot Menu, select "FFT" then "Setup". From the Fourier Transform Window, "Load Input File" and pick the supplied file "fft data 2000 timesteps.out"(this file was generated after running the simulation for 2000 timesteps. Tip: You may need to alter the file selection filter to "All Files" to see this). Pick "Magnitude" for "Y Axis Function". Pick "Strouhal Number" for "X Axis Function". Continued on next slide Post Processing (Fluent) [2] 2012 ANSYS, Inc. September 19, Release 14.5

32 Post Processing (Fluent) FFT [1] Pick "Axes", and for the "X Axis" turn off "Auto Range". Set bounds from "0.05" to "1". "Apply", then "Close". Select "Plot FFT". Continued on next slide 2012 ANSYS, Inc. September 19, Release 14.5

33 Post Processing (Fluent) FFT [2] You may need to change the graphic window so that "Spectral Analysis" is visible. The peak Strouhal number is 0.171, which is close to the that was suggested by the literature search. To extract the exact peak value from this graph, enable "Write FFT to file" and look at the text file on disk. The second peak is a harmonic as the input signal is not perfectly sinusoidal ANSYS, Inc. September 19, Release 14.5

34 Close Fluent. Open a CFD POST session. Close Fluent Run CFD Post We will create an animation ANSYS, Inc. September 19, Release 14.5

35 Post Processing (CFD Post) [1] Animation in CFD post can be done based on all the data files already saved Thus, you can create any animation once calculation is finished. "File>Load Results". Select last time step data file (Make sure you select the files generated from the autosave feature, with a filename "transient detail 1 nnnnn.dat.gz", rather than the results that you have saved manually whilst working though the instructions. Select "Load complete history as": "A single case" ANSYS, Inc. September 19, Release 14.5

36 Insert a vector. Open a CFD POST session. Keep default name "Vector 1". Location "Symmetry 1". "Apply". Post Processing (CFD Post) [2] Click on the "Z" axis to align the view angle ANSYS, Inc. September 19, Release 14.5

37 Post Processing (CFD Post) [3] Activate Timestep Selector panel. Pick a time value from the list then Apply to see the result at that timestep. Click on the film icon, then the play button, for a quick animation of all saved timesteps. Recall that in Fluent, we generated a contour plot every 2 timesteps. We saved the data files used here every 5 timesteps ANSYS, Inc. September 19, Release 14.5

38 Optional Further Work There are many ways the simulation in this tutorial could be extended. Mesh independence. Check that results do not depend on mesh. Re run simulations with finer mesh(es). Generated in ANSYS Meshing application, or, from adaptive meshing in Fluent. Reynolds number effects. You can investigate other flow pattern by changing the Reynolds number. For lower Reynolds number, steady state analysis with laminar model is possible. For higher Reynolds numbers, unsteady transitional turbulent models (k kl omega, SST) have to be considered. While for Reynolds number higher than , the standard or SST k omega turbulence models would be used ANSYS, Inc. September 19, Release 14.5

39 Wrap Up This workshop has shown the basic steps that are applied in all CFD simulations: Setting boundary conditions and solver settings. Running steady and transient models. Using iterative and non iterative advancement schemes. Postprocessing the results, both in Fluent and CFD Post for transient cases. One of the important things to remember in your own work is, before even starting the ANSYS software, is to think WHY you are performing the simulation: What information are you looking for. What do you know about the boundary conditions. In this case we were interested in calculating flow around a cylinder, and assessing the vortex shedding frequency. We checked with FFT analysis that predicted frequency is in good agreement with results from literature. Knowing your aims from the start will help you make sensible decisions of how much of the part to simulate, the level of mesh refinement needed, and which numerical schemes should be selected ANSYS, Inc. September 19, Release 14.5

40 References Braza, M., Chassaing, P., & Minh, H. H., "Numerical Study and Physical Analysis of the Pressure and Velocity Fields in the Near Wake of a Circular Cylinder", J. Fluid Mech., 165:79 130, Coutanceau, M. & Defaye, J. R., "Circular Cylinder Wake Configurations A Flow Visualization Survey", Appl. Mech. Rev., 44(6), June Williamson, C. H. K, "Vortex Dynamics in The Cylinder Wake", Annu. Rev. Fluid Mechanics, 28: , ANSYS, Inc. September 19, Release 14.5