Icem_CFD_CFX流体学习资料 Icem CFD CFX流体学习资料 CFX_ICEMCFD_11_培训教程_2008_04 CFX11_Workshops CFX11_W9_Radiation

1、Fuel Channel Assembly,Workshop 9,Notice,This workshop is meant to be run with ANSYS CFX 11.0 SP1. If running without the service pack, please skip all steps related to the radiometer. Including these steps will result in a solver error.,This case models the heat transfer and thermal radiation in a f

2、uel channel assembly,Nuclear ReactorFuel Channel Assembly,Nuclear ReactorFuel Channel Assembly,The fuel channel assembly comprises of a pressure tube containing the fuel, a Calandria tube containing CO2, two end-fittings (one at each end of the pressure tube), and various internal components. Carbon

3、 dioxide gas passes between the Calandria tube and the pressure tube to insulate the Calandria tube from the thermal radiation emitted by the hot pressure tube. CO2 is used since it is optically thick (it absorbs thermal radiation well). Spacers, positioned along the length of the pressure tube, mai

4、ntain the annular gap and prevent contact between the two tubes. Each end-fitting holds a liner tube, a fuel support plug, and a channel closure. To keep solution time to a minimum the case has been simplified by modeling only the CO2 flow in the annular region of the fuel channel assembly. The spac

5、ers have been ignored.,Assumptions,Inlet for CO2 flow Mass flow rate= 0.02 kg/s,Constant Average Static Pressure outlet,Wall at constant high temperature of 600 K,Wall at constant low temperature of 300 K,Solution Approach,Due to the symmetry of the geometry and flow field, only a quarter of the geo

6、metry is modeled The Discrete Transfer radiation model with Weighted Sum of Grey Gases Radiation will be used to model radiation Post processing of radiometers will be demonstrated,Start Simulation,Start CFX-Pre in a new working directory and create a new simulation using the General Simulation Type

7、 Right-click on Mesh in the Outline tree and import the ICEM CFD mesh annular.cfx5 You will need to change the File Type to ICEM CFD Use the default Mesh Units of m,Hex grid: Inner Diameter = 116 mm Outer Diamter = 160 mm Length = 4m,Examine Mesh Regions,Expand annular.cfx5 and click on the 3D and 2

8、D regions The corresponding mesh is displayed in the Viewer Notice that PER1 and PER2 correspond to the periodic surfaces,Load Material Properties,In the Outline tree, right click on Materials and select Import Library Data In the pop-up window, expand Calorically Perfect Ideal Gases, and select CO2

9、 Ideal Gas Click OK CO2 Ideal Gas will now appear under Materials in the Outline tree,The next step is to load the required material from the material library:,Edit the Fluid Domain,In the Outline tree, right-click Default Domain and select Edit On the General Options tab, set the Fluids List to CO2

10、 Ideal Gas using the icon Switch to the Fluid Models tab Set the Heat Transfer Option to Thermal Energy and leave the Turbulence Option set to the default k-Epsilon model Expand the Thermal Radiation Model frame and set the Option to Discrete Transfer,Edit the Fluid Domain,Set the Spectral Model Opt

11、ion to Gray then click Ok,Load Radiation Template,Click File Import CCL and import the file multigrey_radiation_modi.ccl provided with this workshop Some expressions are generated when the template is loaded. These expressions describe the absorption coefficient of the gases at different spectral ba

12、nds.,The CFX installation includes model templates for various different simulations. The templates can be found in C:Program FilesANSYS Incv110CFXetcmodel-templates. One of the templates is a multigray radiation simulation that uses natural gas. A modified version of this template is provided with

13、this workshop and can be viewed in a text editor. The modified template only includes the weight and absorption coefficients necessary to define the multigray model. In addition, the molar fraction of CO2 has been set to 1 and the molar fraction of other species in the template (CH4, CO, H2O) have b

14、een set to 0.,Load Radiation Template,The template loads expressions which are used to calculated a weighted absorption coefficient for gases. The weighting compensates for the fact that different gases absorb and emit in different spectral bands. Notice the CH4molf, CO2molf, COmolf and H2Omolf expr

15、essions. CO2molf is the only non-zero molar fraction. You can change the coefficients in the template to match different gases. The table on next page provide the required coefficients.,Calculates overall gas emissivity based on:,Where agi are expressed as functions of T:,Template Background,Templat

16、e explanation,Here Ng is number of bands, theoretically, the more bands we divided, the better representation of the radiative absorption and emission from a gas would be. In the modeltemplate file, there are total 4 bands, then the coefficient in the Ng 4 should match all the coefficients in the mo

17、del template file. User can also modify the template file by change it to the other number of bands, for example 3 or 2, with the corresponding coefficients in the table. For the two equations below the table, the first equation represents the absorption coefficient while the second equation represe

18、nts the weight.,Setting Multigray Options,Double-click on the Default Domain On the Fluid Models tab, change the Spectral Model to Multigray This is the same as a Weighted Sum of Grey Gases model Click on the Add new item icon and accept the default name Gray Gas 1 Enter the expressions weight1 and

19、abscoef1 for Weight and Absorption Coefficient Create Gray Gas 2 and enter the expressions weight2 and abscoef2 for the Weight and Absorption Coefficient,Now edit the domain to use the Multigray model:,Setting Multigray Options,Repeat the last step for Gray Gas 3 and Gray Gas 4, using the expression

20、s weight3, abscoef3, weight4 and abscoef4 Scattering for most clear gases is minimal. Leave the Scattering Model set to None Click Ok,Create Boundary Conditions,Next you will create the boundary conditions shown below,Inlet for CO2 flowMass Flow Rate = 0.005 kg/s,Pressure outlet,Periodic condition,W

21、all at constant temperature 600K,Wall at constant temperature 300K,Create Boundary Conditions,In the Outline tree, right-click on Default Domain and select Insert Boundary. Enter the Name as Inlet then click OK On the Basic Settings tab, set the Boundary Type to Inlet and the Location to INLET On th

22、e Boundary Details tab, set the Mass And Momentum Option to Mass Flow Rate Set Mass Flow Rate to 0.005 kg s-1 Set Static Temperature to 300 K and click Ok,Create Boundary Conditions,Right-click on Default Domain and insert a boundary named Outlet Use the following setting for this boundary: Boundary

23、 Type = Outlet Location = OUTLET Mass And Momentum Option = Average Static Pressure Relative Pressure = 0 Pa Click Ok to create the outlet boundary,Now create the outlet boundary:,Create Boundary Conditions,Insert a boundary named ptubeside into the domain Default Domain Use the following settings f

24、or this boundary: Boundary Type = Wall Location = PTUBE Heat Transfer Option = Temperature Fixed Temperature = 600 K Click Ok to create the wall boundary,Now create the wall boundary for the pressure tube:,Create Boundary Conditions,Insert a boundary named ctubeside into the Default Domain Use the f

25、ollowing settings for this boundary: Boundary Type = Wall Location = CTUBE Heat Transfer Option = Temperature Fixed Temperature = 300 K Click Ok to create the wall boundary,Finally, create the Calandria tube wall boundary:,Create Domain Interface,Select the Domain Interfaces icon from the toolbar an

26、d enter the Name as PerInterface Set the Interface Type to Fluid Fluid For Interface Side 1, pick PER1 from the Region List,Domain Interfaces are used to implement a periodic condition, effectively connecting one side of a domain to another side of the same domain.,Create Domain Interfaces,For Inter

27、face Side 2, pick PER2 from the Region List Set the Interface Model Option to Rotational Periodicity Set the Rotation Axis to Global Z Set the Mesh Connection Method to 1:1 Click Ok,Set Solver Controls,Double-click on the Solver Control entry in the Outline tree Set Convergence Criteria Residual Typ

28、e to MAX This is a tighter convergence criteria. Usually a high quality mesh, as used in this workshop, is required to obtain this level of convergence Click on the Advanced Options tab and toggle on Thermal Radiation Control Set Diagnostic Output Level to 1 then click Ok,Radiation Solver Controls,I

29、teration Interval frequency of the radiation calculation with respect to the flow solver. If left unset, radiation will be calculated at each flow solver iteration (i.e., 1). Diagnostic Output Level output is controlled as follows: 0 = Quiet If the solver encounters a fatal error, it will stop autom

30、atically. 1 = Minimal A diagnostic results file is written and warnings are reported. The diagnostic results file includes radiation quantities for each radiation element. 2 = Verbose This level is for debugging purposes only. Target Coarsening Rate (64) radiation is solved on a coarser mesh than th

31、e rest of the equations. This is the (approximate) factor by which the original mesh is coarsened for the solution of the radiation equations. Small Coarse Grid Size (500) minimum number of radiation elements in the coarser mesh. The coarsening algorithm will stop when either this value or the targe

32、t coarsening rate is achieved.,The information on the next two slides details some important radiation solver control parameters available on the Advanced Options tab:,Radiation Solver Controls,Ray Tracing Control ( Discrete Transfer only): Iteration Interval (0) calculation frequency for ray tracks

33、. Default is that tracks are computed only once and stored permanently. Maximum Number of Tracks (9000) rays can be reflected from specular surfaces, giving rise to an infinite number of tracks. Whenever the number of tracks reaches this maximum, the tracing for this ray is halted, and the next ray

34、is started. Maximum Number of Iterations (100) the radiation equations have their own solver, which iterates to a solution each time the equations are solved (every timestep by default). This setting limits the number of iterations in the radiation solver. Usually the first iteration satisfies the c

35、onvergence tolerance (1%) in the radiation solver, but reflective boundaries may prevent this. Ray Reflection Threshold (0.01) for specular boundaries, a ray may get reflected multiple times. When the energy content of the original ray has dropped below this threshold, the tracing is halted.,Creatin

36、g Radiometers,A radiometer is a monitor point that acts like an experimental device to measure radiation Measurement of radiation is directional and ray-based Post-processing of rays is possible in CFX-Post This is a useful tool for measuring the amount of radiation reaching a given location in the

37、solution domain,Next you will create a radiometer. This step requires Service Pack 1 for ANSYS CFX 11.0. If you do not have Service Pack 1 installed please skip to writing the Definition file.,Creating Radiometers,Double-click on Output Control Click on the Monitor tab and toggle on Monitor Options.

38、 Click the Create New icon in the Radiometer section Accept the default name Enter the Cartesian Coordinates for the radiometer as(0.05, 0.05, 2.0) This is in the middle of the domain Set the Temperature to 300 K This is the calibration temperature Set the radiometer to use 8 Quadrature Points (samp

39、ling beams),Creating Radiometers,Set the Diagnostic Output Level to 2 Set the orientation of the radiometer to be facing up a Direction of (0, 0 ,1) Click Apply A yellow cross-hair will appear in the Viewer showing the location of the radiometer,Run the Solution,Save the CFX-Pre simulation as annula

40、r.cfx Select the Write Solver File icon Click Save to write the Definition file annular.def and launch the Solver Manager Click Start Run when the Solver Manager opens Continue with the steps on the next page while the solver is running,You can now save the simulation, write the Definition file and

41、start the Solver,While Running the Solver,By default, the radiation equations are solved once per time step. Diagnostics are reported each time. The %Imbal and %Lost numbers are related if any of the traced rays were terminated it will result in an energy imbalance. An imbalance can also occur if th

42、e radiation solution is not converging. Both these quantities should be near 0 at the end of a run. You should always check this.,Radiometer Diagnostics,Radiometers calculate ray traces and measure the incident radiation. After the second iteration, a Radiometer tab will appear in the Solver Manager

43、 showing the value of each Radiometer that was created in CFX-Pre. The value should level off as the solution converges. You can click on the curve to see the iteration number and the incident radiation at that location in W m-2 ,Post-Processing Radiometers,When the solver has finished proceed to CF

44、X-Post Select Location Polyline Select the Method to be From File Click on the File icon and browse to the radiometer output. The file will be in the solver run directory (annular_001) and named pflux.csv Click on Open to load the file,To view the sampling rays for the radiometer you will create a P

45、olyline in CFX-Post:,Post-Processing Radiometers,Click Apply to create the Polyline radiometer plot,Side view,Variables for Radiation,Click on Variables tab. There are some additional variables due to radiation: Wall Radiative Heat Flux: this represents the net radiative energy flux leaving the boun

46、dary. It is computed as the difference between the radiative emission and the incoming radiative flux (Wall Irradiation Flux). Wall Irradiation Flux: this represents the incoming radiative flux. It is computed as the solid angle integral of the incoming Radiative Intensity over a hemisphere on the b

47、oundary. For simulations using the multiband model, the Wall Irradiation Flux for each spectral band is also available for post-processing. The summation of Wall Radiative Heat Flux and the Wall Convective Heat Flux is Wall Heat Flux. For an adiabatic wall, the sum should be zero.,Heat Transfer Coef

48、ficient,The solver calculates a Heat Transfer Coefficient, hc, from the following equation: Qwall = hc(Twall Tnear wall) Where Qwall is the calculated Wall Heat Flux, Twall is the wall temperature and Tnear wall is the temperature in the control volume next to the wall. Often Tnear wall is not appro

49、priate for your particular application. You can specify your own constant value for Tnear wall in CFX-Pre using the Expert Parameter tbulk for htc. However, you may want to use the Temperature at a set distance from the wall as Tnear wall. Next you will calculate your own Heat Transfer Coefficient u

50、sing the Temperature at a fixed distance from the wall. This distance should usually be outside of the thermal boundary layer so that the temperature is representative of the far field temperature.,Heat Transfer Coefficient,Click Locations User Surface. Name the new user surface offset Set the Metho

51、d to Offset from Surface Select the Surface Name to be the region of interest, in this case, ptubeside Set Mode to Uniform and Distance to -0.005 m This offsets the User Surface -0.005 m from the selected region Click the Colour Tab and use Temperature as the Variable Click Apply,Start by creating a

52、n offset surface in CFX-Post at a fixed distance from the wall of interest:,Heat Transfer Coefficient,Edit Ptubeside and click on the Render tab Set the Transparency to about 0.6 and click Apply,To better view the offset surface, edit the Render settings for Ptubeside:,Heat Transfer Coefficient,Sele

53、ct File Export Set the File as Toffset.csv Pick the Locations as offset In the Select Variable(s) list, pick Temperature and click Save The .csv file is written to the working directory and can be opened in Excel,Now you will export Wall Heat Flux and Temperature data from the Ptubeside boundary and

54、 also Temperature data from the offset surface. You can then import this data into Excel and calculate a new Heat Transfer Coefficient.,Heat Transfer Coefficient,Select File Export Set the File as ptubeside.csv Pick the Locations as ptubeside In the Select Variable(s) list, pick Temperature and Wall

55、 Heat Flux (use the Ctrl key) then click Save,The new heat transfer coefficient is calculated as: Qwall / (Twall Tnear wall) Qwall and Twall were exported from ptubeside and Tnear wall was exported from the offset surface.,Heat Transfer Coefficient,Open both csv files in Excel and align the data. Us

56、e the above equation to calculate a new Heat Transfer Coefficient,Monte Carlo Model (Optional),Return to CFX-Pre and double-click on Default Domain In the Fluid Models tab, change Discrete Transfer to Monte Carlo 10,000 is the default Number of Histories. Often more histories are required to produce a “smooth” radiation field, but this increases computational time Write a Definition file and start the run in the Solver Manager,Time permitting, you may want to re-run the simulation using the Monte Carlo radiation model. Note that this model is not inc