1 / 78

Heating Coil Simulation

Heating Coil Simulation. Workshop 12 ANSYS CFX 5.7. Introduction. The objective is to set up, solve and post-process a simplified CFD problem which illustrates fluid flow and conjugate heat transfer.

pata
Download Presentation

Heating Coil Simulation

An Image/Link below is provided (as is) to download presentation Download Policy: Content on the Website is provided to you AS IS for your information and personal use and may not be sold / licensed / shared on other websites without getting consent from its author. Content is provided to you AS IS for your information and personal use only. Download presentation by click this link. While downloading, if for some reason you are not able to download a presentation, the publisher may have deleted the file from their server. During download, if you can't get a presentation, the file might be deleted by the publisher.

E N D

Presentation Transcript

  1. Heating Coil Simulation Workshop 12 ANSYS CFX 5.7

  2. Introduction • The objective is to set up, solve and post-process a simplified CFD problem which illustrates fluid flow and conjugate heat transfer. • The mesh resolution used in this workshop will not necessarily obtain accurate results, but will enable the participants to work through test cases in the limited time available.

  3. Workshop Outline • Analysis of a heating coil surrounded by moving fluid • Open an existing workbench project containing the Design Modeler geometry • Open CFX Mesh: Set mesh parameters and create mesh • Preprocess: set fluid domain physics, boundary conditions, initial conditions, solver parameters • Solution: monitor residuals, review out files • Post-process

  4. Heating Coil Workshop Double click on to start the CFX5.7 launcher ...

  5. Getting Started • Ensure that the Working Directory is set • Copy the following files to your working directory • HeatCoil.wbdb & HeatCoil.agdb • Click on the CAD2Mesh icon to start the ANSYS Workbench environment

  6. Starting CFX Mesh • Select Open Project and open the HeatCoil.wbdb database. • On the project page, select on the Design Modeler database HeatCoil.agdb • With the Design Modeler database selected, click on Generate CFX Mesh.

  7. Mesher Environment • Mesher window appears as tab on the Project Page • Layout is similar to Design Modeler with parts tree on left • Meshing Progress from top to bottom of Tree • Feedback from mesher appears at bottom left

  8. Mesher Environment • Perform tree functions by right-clicking on objects • Suppress or unsuppress geometry parts/bodies for easier viewing • Mouse Usage: • to rotate (default) • + shift to zoom • + ctrlto translate

  9. Mesher Environment • Left clicking on selected objects in the tree allows you to change attributes of that object • To change the geometry view from solid (opaque) to transparent mode, left click on Geometry • Set % Transparency to 67 using the slider bar or by typing in a number. Experiment with different transparencies and shine

  10. 2D Region Creation 1 • Define 2D regions for placement of CFD boundary conditions • Right-click on Regions to Insert a new Composite 2D Region • Composite regions can consist of one or more surfaces

  11. 2D Region Creation 2 • Create the 2D Region “cinlet” to define the nearest end of the cylinder • To select a location on the geometry, click None under Composite 2D Region at bottom left • Pick the nearest end of the cylinder

  12. Save Often • Save your work often ! • Save after each significant change to the mesh definition • Click Save As … and save in your working directory • For subsequent saves, simply click Save

  13. 2D Region Creation 3 • Surfaces selected for 2D regions will appear as green in the viewer window • Unfinished region definitions appear with a red-circled exclamation mark • Click Apply to finish defining the new 2D region. Marks should disappear

  14. 2D Region Creation 4 • Create 3 more 2D regions: • coutlet for the far end of the cylinder • hinlet for the end of the coil nearest to the inlet • houtlet for far end of the coil

  15. 2D Region Creation 7 • We will now create a region coil thatdefines the surfaces of the coil which will be in contact with the fluid. • Set the display to transparent so that the interior structures of the geometry become visible • Left click the Geometry object in the tree • Use the slider bar to adjust the transparency

  16. 2D Region Creation 9 • Orient the geometry so that you are viewing the side of the cylinder • Insert a new 2D Region “coil” • Click on None to set the Location • Box select the coil to include all the coil surfaces. Note that the ends of the coil have already been assigned to hinlet and houtlet

  17. 2D Region Creation 6 • All the selected coil surfaces should turn green. • Holding down the control key select the two end surfaces of the coil (previously defined as hinlet and houtlet) to deselect them • Click on apply to assign the selected surfaces

  18. Mesh Controls 1 • Some parameters are required to control the density of the tetrahedral mesh produced by CFX-Mesh • Under Mesh in the Object Tree, click on Default body spacing and set to 0.12 mm. • Click on Default Face Spacing. Set Angular resolution to 30 Degrees, Minimum and Maximum Edge Lengths to 0.006 and 0.12 mm respectively

  19. Mesh Controls 2 • Click on Inflation. Set the number of Inflated Layers to 3. Set the Expansion Factor to 1.7. • Inflation controls the mesh near the walls of the geometry (more later …) • Click on Options. Set Overwrite Existing GTM file to Yes.

  20. Mesh Controls 3 • Click on Preview. This section of the tree controls mesh visualization. Set Mesh Render Mode to Wireframe • Set the mesh Face Colour Mode to Uniform and choose a color by clicking on the colored bar • Next, we will select the surfaces on which to display the finished mesh.

  21. Mesh Preview 1 • Mesh Preview allows the definition of surfaces on which to view the mesh before exporting to CFD • Right click on Preview and Insert a Preview Group. Label the group “coilsurface”. • Click on None under Preview Group to select surfaces and box select the entire Coil • Click Apply to accept the selection

  22. Mesh Preview 2 • Create a second Preview Group called “all” • Click on None to select the defining surfaces • Box Select the entire geometry • Click Apply to accept the selection

  23. Mesh Generation 1 • CFX Mesh generates surface meshes first, then makes the volume mesh • To generate a surface mesh for the coil, left-click on the coilsurface Preview region and select Generate This Surface Mesh • A progress bar appears at the bottom of the window. • When the coil surface mesh is complete, it appears in the viewer

  24. Mesh Generation 2 • To generate a surface mesh for the coil, left-click on the all Preview region and select Generate This Surface Mesh • A progress bar appears at the bottom of the window. • When the surface mesh is complete, it appears in the viewer

  25. Mesh Generation 3 • Next we will define the characteristics of the mesh near the walls of the geometry • Insert Inflated Boundary “cylinder” and set the maximum thickness to 0.12 mm • Click on None next to Location box and select, the inner and outer cylinders. (Note: Use the control key for multiple selections) • Click on Apply to accept

  26. Mesh Generation 4 • Now we will view the changes produced by defining inflation. • Click on Preview and Set Mesh Render Mode to Solid Face • Right-click on Preview region all and generate the surface mesh • Mesh appears as solid and shaded. The meshed surfaces shown represent the interface between the inflation layer and the tetrahedral mesh

  27. Mesh Generation 5 • Generate the volume mesh (this step writes out a mesh *.gtm file) • Use the icon at the top right corner of the meshing window, • Or right click on the Mesh object in the tree • Volume meshing uses the constraints created during surface meshing • A progress bar will appear at the bottom left of the mesher window

  28. Saving the Mesh file • Save the CFX Mesh database. • Return to the Project Page by clicking the Project Tab • Save the project and exit Workbench

  29. Starting CFX-5 Pre • Click on CFX-Pre 5.7 • The CFX-Pre Splash Screen should appear

  30. Starting CFX-5 Pre • Click on Open Simulation • Set the file type to be GTM Database • Select the GTM file written out by CFX Mesh (HeatCoil.gtm) • Click on Open to start CFX Pre.

  31. Preprocessing 1 • Click on the Physics Tab to start defining the problem parameters • Click Create, Flow Objects and select Simulation Type. • Set the Simulation Type to Steady State. • Click Ok

  32. Preprocessing 2 • Next we will define the working fluid around the coil • Click Create, Flow Objects and select Domain. • Call the Domain “fluid” • Click Ok to Edit the Domain

  33. Preprocessing 3 • The Edit Domains Form has three sections • Under General Options set the location to B2.P3, the fluid to Water and the reference Pressure to 1 atm • Under Fluid Models, set the Heat Transfer Model to Thermal energy and the Turbulence Model to k-Epsilon

  34. Preprocessing 4 • Under Initialization, set the fluid Relative Pressure to 0 Pa. This is the pressure relative to the reference pressure set for the domain • Click on the checkbox next to Turbulence Eddy Dissipation to set it • Leave the initialization as automatic • Click OK to save all the Domain settings and close the form Click on initial conditions checkbox to activate initialization

  35. Preprocessing 5 • Note that the Tree at the left now has a new object called fluid • This is the domain created in the last few steps • Create a second domain and call it coil • Click OK to edit the coil domain

  36. Preprocessing 6 • Set the Location to B1.P3. This should highlight the coil mesh in the viewer window • Set the Domain Type to Solid and select Copper from the Solids List • Under the Solid Models tab, note the the Heat Transfer Option is already set to Thermal Energy • Leave the Radiation Model as None

  37. Preprocessing 7 • Click on Initial Conditions to Activate initialization • Set the Temperature Option to Automatic (this is default if the Initialization is not activated) • Click OK to save the domain settings and exit the form

  38. Preprocessing 8 • Next we will specify a heat source in the coil location • Create a Subdomain • Label it “heatsource” • Make sure the Domain is set to coil • Click OK to accept the selection

  39. Preprocessing 9 • Set the location to B1.P3 (Note: the heat source will be specified for the entire volume of the coil) • Under The Sources Tab, set the Energy Sources Option to Total Source • Specify a total heat source of 50 kg m^2 s^-3 (50 W) • Click OK to save the subdomain setting and exit the form

  40. Preprocessing 10 • Next, we will create inlet and outlet boundary conditions to the fluid domain • Create a boundary condition called “inlet” • Make sure that the domain is set to fluid • Click OK to accept and specify the inlet conditions

  41. Preprocessing 11 • Edit the inlet boundary conditions • Under Basic Settings, set the Boundary Type to Inlet and the Location to cinlet • Under Boundary Details, set the Normal Speed to 0.1 m/s and the Temperature to 300 K • Click OK to save the boundary settings and exit the form

  42. Preprocessing 12 • Note that creating objects automatically adds them to the tree at left • To make changes to any object, simply double click to bring up the appropriate form • The inlet boundary is shown as flow arrows in the viewer • Create a second boundary condition called “outlet” for the domain fluid and click OK to edit it

  43. Preprocessing 13 • Edit the outlet boundary conditions • Under Basic Settings, set the Boundary Type to Outlet and the Location to coutlet • Under Boundary Details, set the Mass and Momentum Option to Average Static Pressure • Set the Relative Pressure to 0 Pa • Click OK to save the boundary settings and exit the form

  44. Preprocessing 14 • We are now ready to set the CFD Solver Specifications • Create a Solver Control Flow Object • This will bring up a form on which the discretization scheme and fluid/solid time scales can be set

  45. Preprocessing 15 • For most problems, only the Basic Settings Tab is used • The default discretization is High Resolution and is also most accurate and robust. • The fluid will have a much shorter timescale than the solid • Use a physical timescale of 0.01 s for the fluid and 5 s for the solid • Set the Conservation target for equation balances to 0.01 • Click OK to save and exit the form

  46. Preprocessing 16 (optional) • Click on File -- Export ccl to save the problem setup • Turn off ‘Save All Objects’ and select the Flow & Library objects. • Save the setup as coil.ccl • Saving setup files will allow the boundary conditions to be read in quickly if the grid is changed • The .ccl file is a text file that can be edited using any text editor

  47. Preprocessing 17 • Click on File -- Write Solver (.def) file to write a file to the solver • Save the setup as HeatCoil.def • Set the Operation to Start Solver Manager and turn ON the Report Summary Interface Connections option. • Click OK to save and exit the form

  48. Preprocessing 18 • Minimize the Solver Manager window. • Notice that a domain interface has been automatically created by PRE, to connect the fluid and solid domains. • Click OK on the information window. • Save the CFX Pre database and exit. • Restore the Solver Manager window.

  49. Starting the Solver • On the Define Run form click on Start Run to start the solver

  50. The Solver Manager Workspace • All the functions available from the icons at the top of the Solver Manager window are also available from the Workspace menu • Use the Workspace menu or the icon tool tips to see what various icons do • Note that once a workspace has been changed, this custom setting can be saved and recalled when needed

More Related