fluent13共轭传热

Tutorial: Solving a Conjugate Heat Transfer Problem using ANSYS FLUENT Introduction The physics of conjugate heat transfer is common in many engineering applications, includ- ing heat exchangers, HVAC, and electronic component design. The purpose of this tutorial is to provide guidelines and recommendations for setting up and solving a conjugate heat transfer problem using ANSYS FLUENT. The geometry and flow domain consists of a flat circuit board with a heat generating elec- tronic chip mounted on it. Heat is conducted through the source (chip) and the board on which it is mounted. A laminar stream of air flows over the board and the chip, causing si- multaneous cooling of the solid components and heating of the air stream due to convection. Thermal energy is also transported due to the complex flow field. This tutorial demonstrates how to do the following: • Set up appropriate boundary conditions for a conjugate heat transfer simulation in ANSYS FLUENT. • Enable source terms for specified zones. • Perform flow and energy calculations using various materials (both solid and fluid). • Manipulate mesh adaption registers and perform Boolean operations on them. • Perform mesh adaption and verify that the solution is mesh independent. Prerequisites This tutorial assumes that you are familiar with the ANSYS FLUENT interface and that you have a good understanding of the basic setup and solution procedures. Some steps will not be shown explicitly. You will perform postprocessing related only to mesh adaption and verification of a mesh independent solution. For detailed postprocessing of this simulation, refer to the ANSYS FLUENT 13 Tutorial Guide. c© ANSYS, Inc. February 14, 2011 1 Solving a Conjugate Heat Transfer Problem using ANSYS FLUENT Problem Description The problem considered is shown schematically in Figure 1. The configuration consists of a series of heat-generating electronic chips mounted on a circuit board. Air flow, confined between the circuit board and an upper wall, cools the chips and the board. As the air flows over the chips and the board, its temperature rises. Taking the symmetry of the configuration into consideration, the model extends from the middle of one chip to the plane of symmetry between it and the next chip. As shown in Figure 1, each half chip is assumed to generate 1 Watt and have a thermal conductivity of 1.0 W/m-K. The circuit board conductivity is assumed to be one order of magnitude lower, at 0.1 W/m-K. Air enters the system at 298 K with a velocity of 0.5 m/s. The inlet Reynolds number (based on the spacing between the upper and lower walls) is approximately 870 and thus, the flow is treated as laminar. Figure 1: Problem Schematic Setup and Solution Preparation 1. Copy the mesh file, chip3d.msh.gz to your working folder. 2. Use FLUENT Launcher to start the 3D version of ANSYS FLUENT. For more information about FLUENT Launcher refer to Section 1.1.2, Starting ANSYS FLUENT Using FLUENT Launcher in ANSYS FLUENT 13.0 User’s Guide. 2 c© ANSYS, Inc. February 14, 2011 Solving a Conjugate Heat Transfer Problem using ANSYS FLUENT Setup and Solution Step 1: Mesh 1. Read the mesh file (chip3d.msh.gz). File −→ Read −→Mesh... As the mesh file is read, ANSYS FLUENT reports the progress in the console. Step 2: General Settings 1. Retain the default solver settings. General 2. Scale the mesh. General −→ Scale... (a) Select in from the Mesh Was Created In drop-down list. (b) Select in from the View Length Unit In drop-down list. (c) Close the Scale Mesh dialog box. 3. Check the mesh. General −→ Check ANSYS FLUENT will perform various checks on the mesh and report the progress in the console. Make sure the minimum volume reported is a positive number. Figure 2: Mesh Display c© ANSYS, Inc. February 14, 2011 3 Solving a Conjugate Heat Transfer Problem using ANSYS FLUENT Step 3: Models 1. Enable the Energy Equation. Models −→ Energy −→ Edit... 2. Ensure laminar viscous model is selected. Models −→ Viscous −→ Edit... Step 4: Materials Materials −→ Create/Edit... The working fluid is air. You need to specify the materials for the chip and the board. These materials are assumed to have the same density and heat capacity as that of aluminum, but different thermal conductivities. 1. Model air as an incompressible ideal gas. For this simulation, model air as an incompressible gas because there is a maximum air temperature rise of about 150◦C, but very little pressure change. The incompressible ideal gas option for density treats the fluid density only as a function of temperature. (a) Select fluid from the Material Type drop-down list. (b) Select incompressible-ideal-gas from the Density drop-down list. (c) Click Change/Create. 2. Create the chip material. (a) Select solid from the Material Type drop-down list. (b) Enter chip for Name and delete the entry for Chemical Formula. (c) Enter 1.0 for Thermal Conductivity. (d) Click Change/Create. ANSYS FLUENT displays a question dialog asking whether to overwrite aluminum. Click No. 3. Create the board material. (a) Enter board for Name and delete the entry for Chemical Formula. (b) Enter 0.1 for Thermal Conductivity. (c) Click Change/Create. Do not overwrite aluminum. 4. Close the Create/Edit Materials dialog box. 4 c© ANSYS, Inc. February 14, 2011 Solving a Conjugate Heat Transfer Problem using ANSYS FLUENT Step 5: Cell Zone Conditions 1. Specify the cell zone condition for cont-fluid-air zone. Cell Zone Conditions −→ cont-fluid-air (a) Ensure that fluid is selected from the Type drop-down list. (b) Click Edit... to open the Fluid dialog box. i. Ensure that air is selected from the Material Name drop-down list. ii. Click OK to close the Fluid dialog box. 2. Specify the cell zone condition for cont-solid-board zone. Cell Zone Conditions −→ cont-solid-board (a) Ensure that solid is selected from the Type drop-down list. (b) Click Edit... to open the Solid dialog box. i. Select board from the Material Name drop-down list. ii. Click OK to close the Solid dialog box. 3. Specify the cell zone condition for cont-solid-chip zone. Cell Zone Conditions −→ cont-solid-chip c© ANSYS, Inc. February 14, 2011 5 Solving a Conjugate Heat Transfer Problem using ANSYS FLUENT (a) Ensure that solid is selected from the Type drop-down list. (b) Click Edit... to open the Solid dialog box. i. Select chip from the Material Name drop-down list. ii. Enable Source Terms. iii. Click the Source Terms tab and click the Edit... button to open the En- ergy(w/m3) sources dialog box. A. Set the Number of Energy (w/m3) sources to 1. B. Select constant from the drop-down list and enter 904055. 6 c© ANSYS, Inc. February 14, 2011 Solving a Conjugate Heat Transfer Problem using ANSYS FLUENT C. Click OK to close the Energy(w/m3) sources dialog box. This value, based on the half-volume of the chip, yields a total energy source of 2 Watts in the chip zone. iv. Click OK to close the Solid dialog box. Step 6: Boundary Conditions 1. Define the inflow and outflow boundaries. (a) Set the boundary conditions for the inlet zone. Boundary Conditions −→ inlet −→ Edit... i. Enter 0.5 m/s for Velocity Magnitude. ii. Click the Thermal tab and enter 298 K for Temperature. iii. Click OK to close the Velocity Inlet dialog box. (b) Set the boundary conditions for the outlet zone. Boundary Conditions −→ outlet −→ Edit... i. Retain 0 for Gauge Pressure. ii. Click the Thermal tab and enter 298 K for Backflow Total Temperature. iii. Click OK to close the Pressure Outlet dialog box. 2. Define the thermal boundary conditions. (a) Ensure that the Coupled thermal condition is selected for the following walls: • wall-chip and wall-chip-shadow • wall-chip-bottom and wall-chip-bottom-shadow • wall-duct-bottom and wall-duct-bottom-shadow 3. Set the boundary conditions for the wall-board-bottom zone. Boundary Conditions −→ wall-board-bottom −→ Edit... (a) Click the Thermal tab select Convection from the Thermal Conditions list. (b) Enter 1.5 for Heat Transfer Coefficient. (c) Enter 298 for Free Stream Temperature. (d) Click OK to close the Wall dialog box. 4. Copy the boundary conditions set for the wall-board-bottom zone to the wall-duct-top zone. Boundary Conditions −→ Copy... (a) Select wall-board-bottom from the From Boundary Zone selection list. (b) Select wall-duct-top from the To Boundary Zones selection list. c© ANSYS, Inc. February 14, 2011 7 Solving a Conjugate Heat Transfer Problem using ANSYS FLUENT (c) Click Copy. A Question dialog box is displayed asking if you want to copy wall-board-bottom boundary conditions to wall-duct-top. Click OK. (d) Close the Copy Conditions dialog box. Verify that the boundary conditions were copied correctly. Copying a boundary condition does not create a link from one zone to another. If you want to change boundary conditions on these zones, you will have to change each one separately. Step 7: Solution 1. Define the solution method parameters. Solution Methods (a) Select Green-Gauss Node Based from the Gradient drop-down list. (b) Select Second Order Upwind from the Momentum and Energy drop-down lists. 2. Retain the default under relaxation factors. Solution Controls 3. Ensure the plotting of residuals during the calculation. Monitors −→ Residuals −→ Edit... 8 c© ANSYS, Inc. February 14, 2011 Solving a Conjugate Heat Transfer Problem using ANSYS FLUENT (a) Enter 0.0001 for continuity. (b) Click OK to close the Residual Monitors dialog box. 4. Define a point monitor for the energy equation. You will define a point monitor in the recirculation region behind the chip. The solu- tion convergence is critical in this region. Surface −→Point... (a) Enter 2.85, 0.25, and 0.3 for Coordinates x0, y0, and z0. (b) Enter point-monitor for New Surface Name. (c) Click Create and close the Point Surface dialog box. 5. Enable the plotting of the point monitor. Monitors (Surface Monitors )−→ Create... (a) Enable Plot and Write for surf-mon-1. (b) Select Vertex Average from the Report Type drop-down list. (c) Select Temperature... and Static Temperature from the Field Variable drop-down lists. (d) Select point-monitor from the Surfaces selection list. (e) Click OK to close the Surface Monitor dialog box. 6. Save the case file chip3d.cas.gz. File −→ Write −→Case... 7. Initialize the solution. Solution Initialization (a) Select inlet from the Compute From drop-down list. (b) Click Initialize. c© ANSYS, Inc. February 14, 2011 9 Solving a Conjugate Heat Transfer Problem using ANSYS FLUENT 8. Request 200 iterations (Figures 3 and 4). Run Calculation −→ Calculate The solution converges in approximately 145 iterations. Figure 3: Residual Plot Figure 4: Convergence History of Static Temperature at Monitor Point 10 c© ANSYS, Inc. February 14, 2011 Solving a Conjugate Heat Transfer Problem using ANSYS FLUENT Step 8: Data Analysis 1. Verify that mass is conserved. Reports −→ Fluxes −→ Set Up... (a) Ensure Mass Flow Rate is selected from the Options list. (b) Select inlet and outlet from the Boundaries selection list. (c) Click Compute. ANSYS FLUENT displays the total mass flux across each boundary selected. • The mass flow rate for the inlet should be positive (indicating that mass is entering the domain), while that for the outlet should be negative (indicating that mass is leaving the domain). • The net mass flux appears in the box at the lower right corner of the Flux Reports dialog box. • The net mass flux (inlet plus outlet) should be almost zero, indicating that mass is conserved. 2. Verify that energy is conserved. (a) Select Total Heat Transfer Rate from the Options list. (b) Deselect the previously selected boundaries (inlet and outlet) from the Boundaries selection list and select wall-chip and wall-chip-bottom. (c) Click Compute . The net heat transfer from the chip should 1 Watt since only half the chip is modeled. c© ANSYS, Inc. February 14, 2011 11 Solving a Conjugate Heat Transfer Problem using ANSYS FLUENT (d) Select surfaces where heat flows into and/or out of the computational domain. (e) Retain the selection of wall-chip and wall-chip-bottom from the Boundaries selec- tion list. (f) Select the convection boundaries, wall-duct-top and wall-board-bottom, and inlet and outlet. The selection of the inlet and outlet surfaces accounts for the heat carried by the air as it enters and leaves the domain. (g) Click the Compute button. The net heat transfer error should be very small, indicating that an overall heat balance has been achieved. It should be less than 1 % of the smallest source. 3. Close the Flux Reports dialog box. Step 9: Postprocessing You will perform postprocessing related to mesh adaption and verification of a mesh inde- pendent solution. 1. Set up line surfaces for plotting. Surface −→Line/Rake... 12 c© ANSYS, Inc. February 14, 2011 Solving a Conjugate Heat Transfer Problem using ANSYS FLUENT (a) Create line surfaces line-xwss and line-cross with end points as follows: Line x0 y0 z0 x1 y1 z1 line-xwss 2.75 0.1001 0 4.75 0.1001 0 line-cross 3.5 0.25 0 3.5 0.25 0.5 (b) Close the Line/Rake Surfacedialog box. 2. Generate an XY plot of the cross-stream temperature profile downstream of the chip along the line surface, line-cross. Plots −→ XY Plot −→ Set Up... (a) Ensure that Node Values and Position on X Axis are enabled from the Options list. (b) Enter 0, 0 and, 1 for X, Y and, Z respectively in the Plot Direction group box. (c) Select Temperature... and Static Temperature from the Y Axis Function drop-down lists. (d) Select line-cross from the Surfaces selection list. (e) Click Plot (Figure 5). Figure 5 shows the predicted cross stream temperature profile behind the block. The effects of the heated block are apparent. The mesh is currently too coarse to resolve the heat transfer details accurately. (f) Enable Write to File from the Options list and click Write... to open the Select File dialog box. (g) Enter temp-0.xy for XY File and click OK. 3. Generate an XY plot of the cross-stream velocity profile downstream of the chip along the line surface line-cross. c© ANSYS, Inc. February 14, 2011 13 Solving a Conjugate Heat Transfer Problem using ANSYS FLUENT Figure 5: Cross-Stream Static Temperature Profile at x = 3.5 in, y = 0.25 in (a) Disable Write to File. (b) Select Velocity... and Velocity Magnitude in the Y Axis Function drop-down lists. (c) Ensure line-cross is selected from the Surfaces selection list and click Plot (Fig- ure 6). Figure 6: Cross-Stream Velocity Magnitude Profile at x = 3.5 in, y = 0.25 in 14 c© ANSYS, Inc. February 14, 2011 Solving a Conjugate Heat Transfer Problem using ANSYS FLUENT Figure 6 shows the predicted cross stream velocity profile behind the block. Flow details are smeared due to the relatively coarse mesh used. The mesh is currently too coarse to resolve the flow details accurately. (d) Write the data to an output file velocity-0.xy. 4. Generate an XY plot of the stream-wise component of wall shear stress in the stream- wise direction along the center of the chip. (a) Disable Node Values and Write to File. (b) Ensure Position on X Axis is enabled from the Options list. (c) Enter 1, 0 and, 0 for X, Y and, Z respectively in the Plot Direction group box. (d) Select Wall Fluxes... and X-Wall Shear Stress in the Y Axis Function drop-down lists. (e) Select line-xwss from the Surfaces selection list and click Plot (Figure 7). (f) Write the data to an output file xwss-0.xy. (g) Close the Solution XY Plot dialog box. Figure 7: X-Wall Shear Stress Profile Downstream of the Chip 5. Save the case and data files (chip3d.cas.gz and chip3d.dat.gz). File −→ Write −→Case & Data... Step 10: Mesh Adaption The solution can be improved by refining the mesh to better resolve the flow details. It is also important to verify if the flow solution is independent of the mesh size used. c© ANSYS, Inc. February 14, 2011 15 Solving a Conjugate Heat Transfer Problem using ANSYS FLUENT 1. Create mesh adaption registers based on gradients of pressure, velocity, and tempera- ture, as well as a region adaption register. An adaption register is a logical collection of cells that have been marked for adaption. 2. Combine the adaption registers using Boolean addition and adapt the mesh using the combination register. 3. Continue with the iterations, examine the results obtained using refined mesh. 4. Determine if the solution is mesh independent or if further adaption is required. Mesh adaption should always be performed until mesh independence is achieved. 1. Create a pressure gradient adaption register. Adapt −→Gradient... (a) Retain the default selection of Curvature from the Method list. (b) Select Pressure... and Static Pressure in the Gradients of drop-down lists. (c) Click Compute. ANSYS FLUENT reports that the maximum adaption function value is approxi- mately 0.000176. (d) Enter 1.76e-5 for Refine Threshold. Coarsen Threshold specifies the threshold values for coarsening the grid. Cells with adaption function values (in this case, pressure gradient) below the Coarsen Threshold will be marked for coarsening. Refine Threshold specifies the threshold values for refining the grid. Cells with adaption function values above the Refine Threshold will be marked for refining. When selecting values for Refine Threshold, a good rule of thumb is to use ap- proximately 10% of the value reported in the Max field (i.e., the maximum value of the adaption function). For more information on adaption, refer to Chapter 30. Adapting the Mesh the ANSYS FLUENT 13.0 User’s Guide. (e) Click Mark. ANSYS FLUENT creates a pressure gradient adaption register. ANSYS FLUENT reports that approximately 150 cells were marked for refinement and no cells were marked for coarsening in the console. (f) View the cells marked for pressure gradient adaption (Figure 8). i. Click the Manage... button to open the Manage Adaption Registers dialog box. ii. Select gradient-r0 from the Registers selection list. iii. Click Display. You can modify the display of the adaption register by setting the respective options in the Adaption Display Options dialog box. You can open this dialog 16 c© ANSYS, Inc. February 14, 2011 Solving a Conjugate Heat Transfer Problem using ANSYS FLUENT Figure 8: Cells Marked (approx. 150) for Pressure Gradient Adaption box by clicking the Options... button in the Manage Adaption Registers dialog box. Figure 8 shows the cells marked for pressure gradient adaption. These cells are concentrated on the front face of the block, where the static pressure is changing abruptly due to stagnation and change in the direction of the air flow. 2. Create a velocity gradient adaption register. (a) Select Velocity... and Velocity Magnitude from the Gradients of drop-down lists. (b) Click Compute. ANSYS FLUENT reports that the maximum adaption function value is approxi- mately 0.00057. (c) Enter a value of 5.7e-5 for Refine Threshold (10% of the maximum value). (d) Click Mark. ANSYS FLUENT creates a velocity gradient adaption register. The ANSYS FLU- ENT console window reports that approximately 1550 cells were marked for re- finement. (e) View the cells marked for velocity gradient adaption (Figure 9). 3. Create a temperature gradient adaption register. (a) Select Temperature... and Static Temperature from the Gradients of drop-down lists. (b) Click Compute. ANSYS FLUENT reports that the maximum adaption function value is approxi- mately 0.0977. c© ANSYS, Inc. February 14, 2011 17 Solving a Conjugate Heat Transfer Problem using ANSYS FLUENT Figure 9: Cells Marked (approx. 1550) for Velocity Gradient Adaption (c) Enter a value of 0.00977 for Refine Threshold (10% of the maximum value). (d) Click Mark. ANSYS FLUENT creates a temp