Lab 9: FLUENT: Transient Natural Convection Between Concentric Cylinders

Size: px

Start display at page:

Download "Lab 9: FLUENT: Transient Natural Convection Between Concentric Cylinders"

Maude Booth
6 years ago
Views:

1 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. The specific problem considered is natural convection in the annular space between two concentric cylinders at different temperatures. Concepts introduced in this lab will include modeling options for transient flows, data storage, animations, and using the Boussinesq approximation for natural convection. Laboratory: For this problem we will model transient, two-dimensional flow of air due to natural convection in the annular space between two concentric cylinders as shown in Figure 1. The cylinders are assumed to be very long in the z-direction (into the paper), thus the flow can be modeled as twodimensional. Initially, the air in the gap is at uniform temperature T 0 = 290 K. At time t = 0, the temperature of the inner surface is set to T i = 310 K while the outer surface is kept at T o = 290 K. As the air near the inner cylinder is heated its density decreases inducing an upwards flow. Due to continuity the cold air near the walls must go downwards and a circulating flow develops in the annular space. T o = 290 K g y T i = 310 K air filled space initially at T 0 = 290 K x D i = D o = Figure 1. Schematic diagram of the natural convection flow in the annular space between long, horizontal, concentric cylinders.

2 In order to determine if the flow is laminar or turbulent within the annular space we must calculate the Rayleigh number typically defined for this geometry as Ra Lc = g β T T 3 ( i o) L c ν α = (1) [ ( r i) ] 4 3 L c = 2 ln r o 3 r /5 3 /5 i + r o ( ) 5 /3 = m (2) where g is the gravitational acceleration, β is the thermal expansion coefficient, ν is the kinematic viscosity, and α is the thermal diffusivity at the average temperature in the annular space defined as T m = ( T i + T o ) 2. For this Rayleigh number the flow is well within the laminar region. The total heat transfer rate from one cylinder to the other at steady state has been studied experimentally by Raithby and Hollands [1] and a correlation for the heat transfer rate per unit length is given as a function of an effective thermal conductivity k eff k = Pr Pr Ra 4 Lc = 3.74 (3) ( ) ( ) q ʹ = q L = 2 π k eff T i T o ln r o r i = 7.68 W/m (4) where k is the molecular thermal conductivity. This correlation is good for 0.7 Pr 6000 and Ra Lc Laboratory: ICEM CFD To run ICEM CFD, click on the ICEM CFD icon on the desktop. In the Main Menu, from the Settings pull down menu select Product Solver. In the DEZ verify under Product Setup Output Solver that ANSYS Fluent Solvers - CFD Version is selected. If it is not, do so, click OK, exit the program, and then restart ICEM CFD. Step 1. Select Working Directory and Create New Project Main Menu - From File pull down menu, select Change Working Directory In New Project directory dialog box create a new folder. Do not use a name with spaces, including all the directories in the path. Main Menu - From File pull down menu, select New Project In New Project dialog box create a new project. Again, do not use a name with spaces. 2

3 Step 2. Create Points for Geometry Function Tab - From Geometry select Create Point DEZ - For Create Point enter the following: deselect Inherit Part (NOTE, this is only needed for Windows OS), in Part text edit box click LMB and enter PNT (replacing GEOM), select Explicit Coordinates using LMB, under Explicit Locations ensure Create 1 point is selected from pull down menu, in Y text edit box click LMB and enter 10 for point at (0, 10, 0), click Apply using LMB and verify the Message Done: points pnt.00, in Y text edit box click LMB and enter -10 for point at (0, -10, 0), click Apply using LMB and verify the Message Done: points pnt.01, in Y text edit box click LMB and enter 50 for point at (0, 50, 0), click Apply using LMB and verify the Message Done: points pnt.02, in Y text edit box click LMB and enter -50 for point at (0, -50, 0), click Apply using LMB and verify the Message Done: points pnt.03, in Y text edit box click LMB and enter 0, in X text edit box click LMB and enter 10 for point at (10, 0, 0), click Apply using LMB and verify the Message Done: points pnt.04, in X text edit box click LMB and enter 50 for point at (50, 0, 0), click Apply using LMB and verify the Message Done: points pnt.05, click Dismiss Utilities - Select Fit Window using LMB to verify that six points have been created. DCT - Expand Geometry and Parts menus by using LMB to change + to - for each. Under Model\Geometry use RMB to click on Points and select Show Point Names using LMB. Verify that six points have been created. Step 3. Create Curves for Geometry Function Tab - From Geometry select Create/Modify Curve DEZ - For Create/Modify Curve enter the following: ensure Inherit Part is NOT selected, in Part text edit box click LMB and enter WALL_INNER (replacing PNT), select Arc using LMB, under Method ensure From 3 Points is selected from pull down menu, select Select location(s) using LMB, select pnt.00, pnt.04, and pnt.01 using LMB to create inner arc, verify the Message Done: curves crv.00, in Part text edit box click LMB and enter WALL_OUTER, select pnt.02, pnt.05, and pnt.03 using LMB to create outer arc, verify the Message Done: curves crv.01, 3

select From Points using LMB, in Part text edit box click LMB and enter SYMMETRY, select pnt.00 and pnt.

03 using LMB and then click MMB to create lower boundary, verify the Message Done: curves crv.03, click DISMISS Step 4.

Initialize Blocks Type select 2D Planar from pull down menu, and click Apply and Dismiss Function Tab - From Blocking select Split Block DEZ - For Split Block enter the

05 at ( 0, 50, 0) using LMB to create horizontal split, and click Dismiss NOTE: The block is made up of edges and vertices (in contrast to curves and points for the

$Under Model\Blocking use LMB to check the box for Vertices and then use RMB to click on Vertices and select Numbers Verify that six vertices are now numbered.$

4 select From Points using LMB, in Part text edit box click LMB and enter SYMMETRY, select pnt.00 and pnt.02 using LMB and then click MMB to create upper boundary, verify the Message Done: curves crv.02, select pnt.01 and pnt.03 using LMB and then click MMB to create lower boundary, verify the Message Done: curves crv.03, click DISMISS Step 4. Create Blocking Function Tab - From Blocking select Create Block DEZ - For Create Block enter the following: in Part text edit box click LMB and enter FLUID, under Initialize Blocks Type select 2D Planar from pull down menu, and click Apply and Dismiss Function Tab - From Blocking select Split Block DEZ - For Split Block enter the following: under Split Method select Prescribed point from pull down menu, select Select edge(s) using LMB, select right edge of block using LMB, select pnt.05 at ( 0, 50, 0) using LMB to create horizontal split, and click Dismiss NOTE: The block is made up of edges and vertices (in contrast to curves and points for the geometry). For the block, boundary edges are colored black and the interior edge is light blue. DCT - Expand Blocking menu by using LMB to change + to -. Under Model\Blocking use LMB to check the box for Vertices and then use RMB to click on Vertices and select Numbers Verify that six vertices are now numbered. You may want to make the point names invisible to clearly see the numbers for the vertices. Function Tab - From Blocking select Associate DEZ - For Blocking Associations enter the following: under Edit Associations select Associate Vertex using LMB, select Select vert(s) using the LMB, select Vertex number 33 and then pnt.04 at (10, 0, 0) using the LMB, select Vertex number 13 and then pnt.00 at (0, 10, 0) using the LMB, 4

select Vertex number 11 and then pnt.01 at (0, -10, 0) using the LMB, select Vertex number 21 and then pnt.02 at (0, 50, 0) using the LMB, select Vertex number 19 and then pnt.

under Edit Associations select Associate Edge to Curve using LMB, select Select edge(s) using the LMB, select Edges number 13-33 and 11-33 using LMB and then click MMB, select Curve crv.

01 using LMB and then click MMB, select Edge number 13-21 using LMB and then click MMB, select Curve crv.

03 using LMB and then click MMB, and click Dismiss NOTE: All outer block edge colors will turn to green indicating they are associated with a curve. Step 5.

5 select Vertex number 11 and then pnt.01 at (0, -10, 0) using the LMB, select Vertex number 21 and then pnt.02 at (0, 50, 0) using the LMB, select Vertex number 19 and then pnt.03 at (0, -50, 0) using the LMB, select Vertex number 34 and then pnt.05 at (50, 0, 0) using the LMB, NOTE: All vertex colors will turn from black to red indicating they are associated with a point. under Edit Associations select Associate Edge to Curve using LMB, select Select edge(s) using the LMB, select Edges number and using LMB and then click MMB, select Curve crv.00 using LMB and then click MMB, select Edges number and using LMB and then click MMB, select Curve crv.01 using LMB and then click MMB, select Edge number using LMB and then click MMB, select Curve crv.02 using LMB and then click MMB, select Edge number using LMB and then click MMB, select Curve crv.03 using LMB and then click MMB, and click Dismiss NOTE: All outer block edge colors will turn to green indicating they are associated with a curve. Step 5. Mesh Blocks and Surface Function Tab - From Blocking select Pre-Mesh Params DEZ - For Pre-Mesh Params enter the following: under Meshing Parameters select Edge Params using LMB, scroll down and select Copy Parameters using LMB, under Copy Method ensure To All Parallel Edges is selected from pull down menu, scroll up and select Select Edges(s) using LMB, select Edge number using LMB, under Mesh law select Geometric 1 from pull down menu, under Spacing 1 enter 0.4 for spacing for first nodes from surface, under Nodes enter 41, select Select Edges(s) using LMB, select Edge number using LMB, under Mesh law select Uniform from pull down menu, under Nodes enter 50, select Select Edges(s) using LMB, select Edge number using LMB, under Mesh law select Uniform from pull down menu, under Nodes enter 50, click Dismiss 5

6 DCT - Under Model\Blocking use LMB to check the box for Pre-Mesh. In Mesh Dialog Box select Yes to compute mesh. NOTE: You should produce a structured mesh with nodes concentrated near the inner wall. Step 6. Save Files and Export Mesh Main Menu - From File pull down menu, select Blocking -> Save Unstructured Mesh using LMB. Use the Save Mesh as Dialog Box to save the unstructured mesh. Main Menu - From File pull down menu, select Save Project Function Tab - From Output Mesh select Output To Fluent V6 Boundary Cond. In Family Part boundary conditions dialog box: expand Edges and Mixed/unknown menu by using LMB to change + to -, expand SYMMETRY menu by using LMB to change + to -, click Create new to open the Selection dialog box, under Boundary Conditions select symmetry using the LMB, click Okay using LMB to close the Selection dialog box, expand WALL_INNER menu by using LMB to change + to -, click Create new to open the Selection dialog box, under Boundary Conditions select wall using the LMB, click Okay using LMB to close the Selection dialog box, expand WALL_OUTER menu by using LMB to change + to -, click Create new to open the Selection dialog box, under Boundary Conditions select wall using the LMB, click Okay using LMB to close the Selection dialog box, click Accept Function Tab - From Output Mesh select Write Input In Save dialog box click Yes using LMB to Save current project first. In Open dialog box click Open to select unstructured mesh with current project name. In ANSYS Fluent V6 dialog box enter the following: in Grid dimension select 2D using LMB, in Scaling ensure No is selected, in Write binary file ensure No is selected, in Ignore couplings ensure No is selected, in Boco file retain the default file name, in Output file change the file from fluent to a new name for your mesh, and click Done 6

7 FLUENT Step 1. Read In Mesh Import your mesh created using ICEM CFD into FLUENT. Check to make sure the mesh imported correctly and that you scale it correctly from mm to m. Step 2. Problem Setup for Initial Simulation In the Navigation Pane under Problem Setup use the following steps to setup your simulation: General Solver o Type: Pressure-Based o Time: Transient o Velocity Formulation: Absolute o 2D Space: Planar Gravity: ON Gravitational Acceleration o x-direction: 0 m/s 2 o y-direction: m/s 2 Models (remaining models off) Energy: On Viscous: Laminar Materials, Fluid, air (change the properties for air to those at 300 K) Density: Boussinesq (use pull down menu), kg/m 3 Specific Heat: 1,007 J/kg K Thermal Conductivity: W/m K Viscosity: 1.846e-05 kg/m s Thermal Expansion Coefficient: /K (where β = 1/T m for an ideal gas) Cell Zone Conditions Zone: fluid o Type: fluid o Material Name: air Operating Conditions o Operating pressure: 101,325 Pa o Gravity: ON (gravitational acceleration set using Problem Setup: General) o Boussinesq Parameters Operating Temperature: 290 K (use cold temperature for enclosure) Specified Operating Density: ON Operating Density: kg/m 3 7

8 Boundary Conditions Zone: symmetry o Type: symmetry Zone: wall-inner o Type: wall o Edit: Momentum tab Wall Motion: Stationary Wall Shear Condition: No Slip o Edit: Thermal tab Thermal Conditions: Temperature Temperature: 310 K, constant Zone: wall-outer o Type: wall o Edit: Momentum tab Wall Motion: Stationary Wall Shear Condition: No Slip o Edit: Thermal tab Thermal Conditions: Temperature Temperature: 290 K, constant Reference Values Compute from: wall-inner Reference Zone: air-flow Step 3: Solution Setup for Simulation In the Navigation Pane Tree under Solution use the following steps to setup your solution methods, controls, monitors, and initialization: Solution Methods Pressure-Velocity Coupling o Scheme: PISO (more efficient for transient) Spatial Discretization o Gradient: Least Squares Cell Based o Pressure: Body-Force Weighted (good for natural convection flows) o Momentum: Second Order Upwind o Energy: Second Order Upwind Transient Formulation: Second Order Implicit Non-Iterative Time Advancement: ON (again, more efficient option) Solution Controls Non-Iterative Solver Relaxation Factors o Pressure: 1 o Momentum: 1 o Energy: 0.9 (required for natural convection to get convergence) 8

9 Monitors Residuals - Print, Plot o Options Print to Console: ON Plot: OFF o Equations, Residual, Monitor: ON (all 4 equations) Surface Monitors (click Create to open Surface Monitor Dialog box) o Name: heat_flux_mon (change from default of surf-mon-1) o Options Print to Console: OFF Plot: ON, Window: 1 2 Write: OFF x Axis: Flow Time Get Data Every: 1 Time Step (use pull down menu) o Report Type: Integral o Field Variable: Wall Fluxes, Total Surface Heat Flux o Surfaces: wall-inner NOTE: We are using surface monitors to plot total heat flux from inner cylinder versus time. We will use a second window to make an animation of the solution. Before we set that up below from the Menu Bar select View -> Graphics Window Layout and then an option that allows you to see two panes in the Graphics Window. Solution Initialization (which is actually setting the initial condition) Reference Frame: Relative to Cell Zone Initial Values o Gauge Pressure: 0 Pa o x Velocity: 0 m/s o y Velocity: 0 m/s o Temperature: 290 K Calculation Activities Autosave Every: 10 Time Steps (use Edit button to change file name and location) Solution Animations (click Create/Edit to open Solution Animation Dialog Box) o Animation Sequences: 1 o Name: vectors o Every: 10 Time Step o Define (to open Animation Sequence Dialog Box) Storage Type: Metafile Window: 2 1 (hit Set button) Display Type: Vectors (should open Vectors Dialog Box or hit Edit button) Vectors of: Velocity Color by: Temperature, Static Temperature Options 9

10 o Global Range: ON o Auto Range: OFF o Clip to Range: OFF o Auto Scale: ON o Draw Mesh: OFF Scale: 4, Skip: 2 Min: 290 K, Max: 310 K Click Display button in the Vectors Dialog Box to make a plot of the velocity vector field in window 2. You should see the outline of your domain, but no vectors because your initial velocity field is zero. Hit the Close button to close the Vectors Dialog Box and hit the OK button to close the Animation Sequence Dialog Box. In the Solution Animation Dialog Box verify that the vectors sequence is now checked as Active and hit the OK button to close the Dialog Box. You can now pan or zoom for a different view of the velocity vector field in window 2 1 if desired for your animation, but the default view should be fine. Step 4. Run Calculation Navigation Pane Tree - Under Solution select Run Calculation. Task Page - Under Time Step Size enter s, under Number of Time Steps enter 200 and click Calculate. Next, select the Calculate button in the Task Page. Note that at each time step the solution must iterate until convergence, but this only takes usually 2 iterations for PISO/NITA. The heat transfer from the inner cylinder versus flow time should appear in window 1 2 (use the tab on the top to switch to this window or right click on the tab and select SubWindow View from the pulldown menu to see both window 1 and 2 at the same time). Its value starts out high and then decreases to below 5 W after about 1 second. Every 10 time steps the converged velocity vector field colored by temperature should appear in window 2 1. Notice that a hot plume rises from the inner cylinder and then re-circulates downwards near the outer wall. Step 5. View Solution Animation Navigation Pane Tree - Under Results select Graphics and Animations. Task Page - Under Animations select Solution Animation Playback and select Set Up to open Playback Dialog Box. Use the controls to view the animation. If you want to make an MPEG movie of the animation change WRITE/Record Format to MPEG and click WRITE button. Step 6. View Solution at Each Time Step To display the velocity vector data at any previous time step, from the Main Menu select File\Read\Data and select a data file to read in one that was automatically saved during the run. In the Task Page under Graphics and Animations select Vectors and select Set Up to open the Vectors Dialog Box. Under Vectors of select Velocity and under Color by select Temperature 10

11 and Static Temperature from the pull-down menus. Select Display to see the plot in the Graphics Window. Step 7. Continue Simulation If desired you can solve for velocity and temperature at additional time steps with the same or different time step. To continue make sure that you have open the data file you wish to proceed from. The new plots will be appended to your existing animation by default. If you run the simulation until it reaches steady state the heat flux converges to 7.36 W (which is doubled to include both halves of the annulus). This compares well with the 7.68 W predicted by Equation (4) with an approximately 4% difference (reasonable for an experimental correlation). Assignment There is no written assignment due for this lab so that you can work on the final project (see my webpage at and follow the ME 544 link to a link for the final project assignment and an example validation paper). There is also a link to FLUENT Summary under the General Course Notes section that lists instructions for running a typical simulation. 11

Lab 8: FLUENT: Turbulent Boundary Layer Flow with Convection

Lab 8: FLUENT: Turbulent Boundary Layer Flow with Convection Objective: The objective of this laboratory is to use FLUENT to solve for the total drag and heat transfer rate for external, turbulent boundary