1. Multiphysics Chapter 8

2. Training Manual May 15, 2001 Inventory #001478 8-2 Multiphysics Chapter Goals - –Describe Coupled Analyses - multiphysics See Also: ANSYS Coupled-Field Analysis Guide –Sequential Coupled-Field Analysis –Show Results of some applications –Provide a detailed, step-by-step Tutorial of a fluid structure interaction problem: The Multiphysics Tutorial

3. Training Manual May 15, 2001 Inventory #001478 8-3 Types of Coupled Analyses Indirect Method –Involves two analyses, done in sequence, each belonging to a different field. The fields are coupled by applying results from one analysis as loads for another analysis Direct –Involves a single analysis using a coupled-field element which contains all necessary degrees of freedom (DOF’s) Examples of one way and two way coupling for the indirect method will be shown next

4. Training Manual May 15, 2001 Inventory #001478 8-4 “One-Way” Coupling Examples Fluid-Structure Interaction –CFD results determine pressure loadings –Resulting structural deformations have negligible effect on the flowfield. Fluid-Thermal Interaction (constant property) –CFD flowfield necessary to compute temperatures –CFD properties (sometimes!) unaffected by temperature changes.

5. Training Manual May 15, 2001 Inventory #001478 8-5 LDREAD - load transfers Fluid Analysis Structural Analysis Fluids Results File Structural Results File Performing an Indirect Coupled-Field Analysis

6. Training Manual May 15, 2001 Inventory #001478 8-6 Coupled Valve Analysis * Courtesy of Cybernet Systems Company, Ltd., 1995 Multiphysics Example... 2D flow through a valve Coupled Analysis FLOTRAN used to calculate pressure These pressure loads applied to structural analysis in ANSYS to obtain equivalent stresses

7. Training Manual May 15, 2001 Inventory #001478 8-7 The Basic Procedure Converge Flow Analysis Switch element type to structural (or thermal or magnetic). Note: delete the FLOTRAN element type, NOT the elements. –In this example, the non-fluid elements could be a part of the FLOTRAN solution (as solids). Then the element type number for these elements is assigned to a structural element. Unselect the fluid elements and nodes. Apply structural constraints. Select nodes at the solid-fluid interface and transfer loads from fluid analysis (LDREAD). Run structural analysis.

8. Training Manual May 15, 2001 Inventory #001478 8-8 The FLOTRAN mesh

9. Training Manual May 15, 2001 Inventory #001478 8-9 The FLOTRAN mesh (continued)

10. Training Manual May 15, 2001 Inventory #001478 8-10 Velocity Field

11. Training Manual May 15, 2001 Inventory #001478 8-11 Pressure Field

12. Training Manual May 15, 2001 Inventory #001478 8-12 The Structural Mesh

13. Training Manual May 15, 2001 Inventory #001478 8-13 Loading - Pressure Forces

14. Training Manual May 15, 2001 Inventory #001478 8-14 Displacements

15. Training Manual May 15, 2001 Inventory #001478 8-15 Equivalent Stresses

16. Training Manual May 15, 2001 Inventory #001478 8-16 Fluid - Magnetic Interaction Magnetic phenomena can produce effects that should be accounted for in CFD analyses in several ways –Body forces ( FLOTRAN momentum equation) These can be the result of DC or AC currents (time- averaged). LDREAD,FORCE,… (FLOTRAN converts to Force/vol) Harmonic analyses require the calculation of time averaged JxB cross product from element data. –Electromagnetic fields can also generate heat (Joule Heating) (FLOTRAN energy equation) Occurs through eddy currents LDREAD,HGEN,…..

17. Training Manual May 15, 2001 Inventory #001478 8-17 Fluid - Magnetic Interaction (continued) Magnetic phenomena are influenced by fluid phenomena as well... –Properties Electric resistivity of a fluid is an input to the electromagnetic Analysis. It is often temperature dependent. Real constant –Fluid Velocity Part of the Magnetic Reynolds Number Element input (no automatic load transfer exists) –Fluid Surface configuration (shape)

18. Training Manual May 15, 2001 Inventory #001478 8-18 Example of Magnetics-Fluid Analysis: Induction Furnace In this case, the CFD analysis receives the loads, rather than generating them as magnetic effects produce body force terms…. –The model is axisymmetric –Crucible for molten steel at 2500 F –AC current applied to the coils produces eddy currents within the furnace –The eddy currents produce heating (Joule heating) which melts the steel –The interaction of the eddy currents with the Lorentz forces stirs the molten steel

19. Training Manual May 15, 2001 Inventory #001478 8-19 Solid Model

20. Training Manual May 15, 2001 Inventory #001478 8-20 Induction Furnace - The Mesh Note denser mesh around the coils and in the crucible Denser mesh in areas of large gradients, also the areas of interest Coarse mesh with infinite boundary elements at the far-field Approximately 6600 elements

21. Training Manual May 15, 2001 Inventory #001478 8-21 Finite Element Mesh

22. Training Manual May 15, 2001 Inventory #001478 8-22 Emag Solution - Flux First, ANSYS/Emag product is used to solve the electromagnetic field Axisymmetric, time-harmonic analysis This plot shows the electromagnetic flux lines resulting from the magnetically-induced field

23. Training Manual May 15, 2001 Inventory #001478 8-23 EMAG Flux Lines

24. Training Manual May 15, 2001 Inventory #001478 8-24 Emag Solution - Lorentz Forces Lorentz forces also result of the electromagnetic field Strongest closest to the coils Closeup of the Lorentz forces in the crucible These forces are strong enough to stir the molten steel... –Velocities on the order of 3 meters/sec can be produced.

25. Training Manual May 15, 2001 Inventory #001478 8-25 Lorentz forces in molten steelCloseup of Lorentz forces in crucible

26. Training Manual May 15, 2001 Inventory #001478 8-26 FLOTRAN Solution - Velocity Field Lorentz forces induce flow in the molten steel Velocity vectors show the turbulent fluid motion in the crucible Note the two turbulent eddies

27. Training Manual May 15, 2001 Inventory #001478 8-27 The flow field up close…. The Crucible with Flow

28. Training Manual May 15, 2001 Inventory #001478 8-28 “Two-Way” Coupling Necessary when the effects of the second analysis (i.e., structural deformation effects) on the flow field are not negligible and re-analysis of the flow field is required. Solve the initial fluid and structural (or thermal or magnetic) problems following the procedure for one-way coupling. Re-mesh (or perhaps merely move the nodes) the new flow field geometry according to structural /thermal/magnetic analysis deformations.

29. Training Manual May 15, 2001 Inventory #001478 8-29 “Two Way” Coupling (continued) In the two-way coupling analysis involving FLOTRAN, care must be taken to ensure convergence of the flow analysis. –Complete convergence of intermediate FLOTRAN runs is not usually required if a steady state problem is being solved. The entire sequential process may be put in a macro loop.

30. Training Manual May 15, 2001 Inventory #001478 8-30 Fluid is air. Wall is concrete:4 m by 0.25 m Modulus of Elasticity = 1.39x10 8 N/m 2 Poisson’s Ratio = 0.30 V free stream = 200 km/hr P = 0 Ground, no slip wall H = 4 m t = 0.25 m The Wall Exercise Solve the problem of air flow over a “bendable” wall. What is the maximum von Mises stress in the wall? And what is the wall configuation under this load

31. Training Manual May 15, 2001 Inventory #001478 8-31 The Wall Note that a simple version of this problem was solved in the introductory course as a one-way coupling. In this case we relax the Modulus of Elasticity to the point where the deformation of the wall is significant enough to warrant re-analysis of the flow field. The FSSOLVE macro will be used to iterate to a steady state solution.

32. Training Manual May 15, 2001 Inventory #001478 8-32 Instructor Exercise (continued) Extend the boundaries “far enough away” from the wall in all directions. Make the mesh finer at the wall and ground. Eliminate singularities if possible - round the top of the wall. Apply free stream conditions to the upper boundary and inlet. Treat the ground as a no slip wall. Apply P=0 at the outlet. Set Artificial viscosity =0.1 Set Turbulence Inertia = 1.0

33. Training Manual May 15, 2001 Inventory #001478 8-33 Instructor Exercise (continued) Run the FLOTRAN analysis for 100 iterations. Switch element type 1 from FLUID141 to PLANE42. Input the concrete properties. Unselect the fluid nodes and elements. Fix the bottom of the wall (Set Ux=Uy=0). Select the fluid/solid interface nodes and apply the pressure loads. Solve the static, structural problem.

34. Training Manual May 15, 2001 Inventory #001478 8-34 The Multiphysics Tutorial This tutorial describes in detail the use of various FLOTRAN features in a Multiphysics analysis. –Features... – Advanced turbulence model – SUPG upwinding of advection terms – Modification of CFD mesh using structural approach (UPCOORD) An alternate approach to moving the nodes near the deformed piece involves using MORPHING, a process of remeshing using boundary deformations. – Use of Physics Environments, load transfers to solid and shell elements

35. Training Manual May 15, 2001 Inventory #001478 8-35 A Fluid Structure Analysis With FLOTRAN (Multiphysics)

36. Training Manual May 15, 2001 Inventory #001478 8-36 The Problem Described…. As shown on the previous page, there are two flows (and the nozzle is axisymmetric) that come together. The outer and inner flows are at much different velocities, and are modeled with Flotran 141 elements. The two flows are separated by a thin piece –The effect degree of deformation of this piece on the flowfields, is of interest. –It will be modeled with Solid 42 elements The outer portion of the nozzle,on the right side before the outlet region, is also subject to deformation and will be modeled with Shell 61 elements. The nodes in the fluid regions near the deforming pieces will be moved by considering them part of a “structural fluid”.

37. Training Manual May 15, 2001 Inventory #001478 8-37 Problem Objectives - Step This is a fluid structure analysis where a mixing flow will be calculated while the resulting fluid pressures cause deformation of the boundaries of the flowfield. Milestones in the Analysis Sequence (these will be further subdivided into 14 stages) –Development of the Geometry –Establishment and execution of the meshing strategy –Creation of Physics Environments –Interactive Analysis The student may do the entire exercise interactively or elect to have certain portions performed with input files provided.

38. Training Manual May 15, 2001 Inventory #001478 8-38 Velocity 200 in/sec Velocity 2000 in/sec Axis of Symmetry Separator (moveable) Deformable portion of mixing nozzle Problem - A Mixing Nozzle Axisymmetric geometry. Air Flow (2000 in/sec) through the outer portion mixes with a slower flow (200 in/sec) coming through the inner portion. A solid region separates the flows, and the deformation of this Separator will be calculated. The deformation of the outside of the nozzle is modeled with axisymmetric shell elements.

39. Training Manual May 15, 2001 Inventory #001478 8-39 Summary of Steps Stage 1: Geometry and mapped meshing parameters (mix1) Stage 2: Assign the attributes (mix2) Stage 3. Meshing and Mesh refinement Stage 4: Create CFD environment and write physics file (mix4) Stage 5. Create Structural environment and write physics file (mix5). Stage 6. Activate fluid physics and execute initial FLOTRAN run. Stage 7. Activate alternate advection scheme, extend solution. Stage 8. Examine pressure solution. Stage 9. Activate structural environment. Stage 10. Reading in pressure loads from FLOTRAN. Stage 11. Solve for stresses and displacements. Stage 12. Examine deformations. Stage 13. Update CFD mesh coordinates. Stage 14. Continuing the Sequential solution process

40. Training Manual May 15, 2001 Inventory #001478 8-40 Read in the input file that creates the solid model. Utility Menu: File > Read Input from... Choose mix1 (This completes Stage 1 completely) OK ( Then close the warning box about deactivating element shape checking) 1 2 1 2 Perform This Step to Bypass Interactive Creation of Stage 1

41. Training Manual May 15, 2001 Inventory #001478 8-41 The Geometry

42. Training Manual May 15, 2001 Inventory #001478 8-42 Working Plane and Parameter Settings Utility Menu > Work Plane > Display Utility Menu > Work Plane > Settings Utility Menu > Parameters > Scalar Parameters

43. Training Manual May 15, 2001 Inventory #001478 8-43 Basic Geometry Preprocessor > Create Open the Scalar Parameter file just created –Utility > Scalar Parameters Click on the desired parameter, move to the field in the command, then hit the middle mouse button… –(Or just type it in…)

44. Training Manual May 15, 2001 Inventory #001478 8-44 The Other Rectangles Click Apply to get the box back…Last one gets OK

45. Training Manual May 15, 2001 Inventory #001478 8-45 Resulting Basic Areas

46. Training Manual May 15, 2001 Inventory #001478 8-46 Connect the Dots... Preprocessor > Numbering Ctrls > Merge Items Pull down menu for label, Choose ALL Then zoom on the open space between the rectangles….

47. Training Manual May 15, 2001 Inventory #001478 8-47 Operate on the Model Preprocessor >Create>Lines>Tan to 2 Lines Get the Picker and Choose Lines: –First Line –Point of Tangency –Second Line –Point of Tangency –Oks all along...

48. Training Manual May 15, 2001 Inventory #001478 8-48 Create the remaining areas Create Arbitrary Areas - Through KPs First Area: Second Area

49. Training Manual May 15, 2001 Inventory #001478 8-49 The Areas are Complete (The keypoint numbers are turned on)

50. Training Manual May 15, 2001 Inventory #001478 8-50 Establish Line Divisions - Lengthwise Mesh Tool - Size Control - Lines –Outlet: 25, Ratio 3 –Use Flip Bias on line 16 –Transition Region (2 lines) Use 20 –Beam Use 14 –Inlet Region (4 lines) Use 20, Ratio -3

51. Training Manual May 15, 2001 Inventory #001478 8-51 Mesh Tool

52. Training Manual May 15, 2001 Inventory #001478 8-52 Transverse Lines Utility Menu > Plot Ctrl > Size and Shape –X distortion factor is 5 Inlet /Outlet: –Use 12, Ratio -2 Outer Inlet: –Use 10, Ratio -2 Separator –Use 3, Ratio -2

53. Training Manual May 15, 2001 Inventory #001478 8-53 Details... Add two areas….. –Preprocessor>Operate>Add>Areas –Areas 5 and 6 This completes Stage 1 (I.e. what is accomplished by the file “mix1”).

54. Training Manual May 15, 2001 Inventory #001478 8-54 Stage 2 Before the Meshing Step, Element types must be assign and attributes must be set Elements will change between the two different physics, so the initial assignment is arbitrary Review –ANSYS Coupled-Field Analysis Guide Sequential Coupled-Field Analysis The input file for Stage 2 is “mix2” Set –Element types –Attributes The Interactive Steps for Stage 2 follow the diagrams which illustrate attribute assignment.

55. The areas will be assigned attribute numbers based on the physics that will be modeled. The table on the following slide shows how the attributes are to be assigned Fluid Only Area 4 Area 1 Area 2 Area 7 Line 8 Line 10 Area 3 Fluid and then “structural fluid” Shell elements on these lines (NOT TO SCALE!)

56. Training Manual May 15, 2001 Inventory #001478 8-56 Definition of Physics Regions

57. Training Manual May 15, 2001 Inventory #001478 8-57 Area Attributes Since properties have not been defined yet, the GUI is not used to set the attributes…. Select the Areas associated with a Physics Region and then assign attribute via the command line. For Example, the Structural Fluid region: –Select Areas 1,3,7 as shown AATT,mat,real,element type number –AATT,1,1,2 Use LATT for shells Define Initial element types: –et,1,42 –et,2,42 –et,3,42 –et,4,61

58. Training Manual May 15, 2001 Inventory #001478 8-58 Area plot, colors assigned to element types This is the completion of Stage 2: after element types and attributes are set

59. Training Manual May 15, 2001 Inventory #001478 8-59 Stage Three - Meshing There is no input file for this step ! Mapped meshes are used where possible Free meshing with quads is used in the central region Mesh refinement where necessary Note that we mesh with arbitrary elements assigned to the attribute numbers. What actual ANSYS element is assigned to “num” in the command ET,2,”num”, for example, will vary with the particular physics being solved. It is assigned in the physics environment file (later).

60. Training Manual May 15, 2001 Inventory #001478 8-60 Activate the Mesh Tool Main Menu: PreProcessor > Mesh Tool 1 3 Use a mapped quadrilateral meshfor the upper and lower portions 2 4 2 Pick these three Pick this one 4 1 Choose Quad elements Mapped mesh Mesh Pick these four areas OK 4 3 5 5 (Close any warning boxes that arise during the meshing steps!) Mesh the Model

61. Training Manual May 15, 2001 Inventory #001478 8-61 6 8 7 9 7 Central Area 6 Choose Quad elements Free Mesh Mesh Pick the Centerl area 9 8 10 OK Mesh the Central Region Create a free mesh of quads for this

62. Training Manual May 15, 2001 Inventory #001478 8-62 13 12 Pick this one 15 11 Choose Quad elements Free Mesh Refine at areas Click Refine Pick Area OK OK (minimal refinement) 14 13 14 16 17 11 12 15 16 17 Refine the Mesh in the Central Area

63. Training Manual May 15, 2001 Inventory #001478 8-63 18 20 Create shell elements on the outside of the nozzle 19 20 Pick lines Lines Mesh Pick these lines OK Close 21 19 21 18 22 Mesh the Shell elements on the outside

64. Training Manual May 15, 2001 Inventory #001478 8-64 Stage Four - Fluid Physics Environment File “mix4” creates fluid physics environment (File shown at the end of the stage). Input the file or perform the steps interactively. Physics Environment files contain: –Element assignments used for the element type numbers. –Boundary Conditions –Solid Material Properties –FLOTRAN settings Solution options Stability Parameters Fluid Properties

65. Training Manual May 15, 2001 Inventory #001478 8-65 Element Types Make these changes on the command line (GUI only allows certain element switching) Assign Element 141 (axisymmetric about Y) to element type numbers 1,2 –et,1,141,,,1 –et,2,141,,,1 Assign Null Element Type to Shells and the Solid regions –et,3,0 –et,4,0

66. Training Manual May 15, 2001 Inventory #001478 8-66 FLOTRAN Boundary Conditions Symmetry Conditions VX = 0 Inlet VY = 200,VX=0 Inlet VY = 2000, VX=0 Walls: VX,VY=0 More Walls Pressure: PRES=0

67. Training Manual May 15, 2001 Inventory #001478 8-67 Application of Boundary Conditions Use Solid Model Boundary Conditions for Velocity and Pressure –Solution>Loads> Apply>Velocity

68. Training Manual May 15, 2001 Inventory #001478 8-68 FLOTRAN Solution Options

69. Training Manual May 15, 2001 Inventory #001478 8-69 FLOTRAN Properties Use AIR-IN for everything on the pull-down menu

70. Training Manual May 15, 2001 Inventory #001478 8-70 Flow Environment Flow Environment >Reference Conditions Always make sure that the reference conditions are consistent with the property type used.

71. Training Manual May 15, 2001 Inventory #001478 8-71 Turbulence Model Choose the RNG Turbulence Model.. Solution > FLOTRAN Set Up > Turbulence Model –Use default parameters for RNG

72. Training Manual May 15, 2001 Inventory #001478 8-72 Create FLUID PHYSICS file Solution > Physics Environment This completes what is accomplished by the file “mix4”

73. Training Manual May 15, 2001 Inventory #001478 8-73 File “mix4” Result of Physics,Write

74. Training Manual May 15, 2001 Inventory #001478 8-74 Stage Five - Structural Physics Environment File “mix5” (file shown at end of Stage 5) performs Stage 5. Details of Stage 5 are now shown. –First Clear Existing Physics Information

75. Training Manual May 15, 2001 Inventory #001478 8-75 Element Types ET,1,0 –Give most of the fluid region the null element type ET,2,42 –This is the “structural fluid” ET,3,42 –The deformable piece separating the two inlets ET,4,61 –The shell element on the outer surface

76. Training Manual May 15, 2001 Inventory #001478 8-76 Properties Preprocessor > Material Props > Isotropic Material 1 is the structural fluid with “artificial properties” –EX:1.E-2 –NUXY:0.000 Making the fluid region a part of the structural solution will enable us to move the nodes via UPCOORD as the structure of interest deforms in the flowfield.

77. Training Manual May 15, 2001 Inventory #001478 8-77 More Properties…... The bendable (deformable) separator –Thermoplastic elastomer –Material Number 2 EX:2.3x10 4 NUXY:0.3000 The Elastic Boundary Shell element –More plastic –Material Number 3 EX:4.0x10 2 NUXY:0.3000

78. Training Manual May 15, 2001 Inventory #001478 8-78 Real Constants Thickness of the Shell Elements –.01

79. Training Manual May 15, 2001 Inventory #001478 8-79 Constraints on the structural problem Centerline Radial Constraint, UX = 0 Axial and Radial Constraints at the bottom, UX,UY=0 Axial Constraint Top of Domain UY = 0 Eliminate Twisting UZ=0

80. Training Manual May 15, 2001 Inventory #001478 8-80 Create Structural Physics File Select everything Title is “struc” This completes what is accomplished by the file “mix5”

81. Training Manual May 15, 2001 Inventory #001478 8-81 The Structural Physics Environment Input

82. Training Manual May 15, 2001 Inventory #001478 8-82 Stage Six: Initial Execution 1. Read in Fluid Physics Choose Read Choose Fluid OK 3 2 1 2. Solve: Main Menu: Solution > Run FLOTRAN 1 2 3 Close any warning boxes that may arise regarding boundary conditions.

83. Training Manual May 15, 2001 Inventory #001478 8-83 Convergence Monitors The first ten global iterations provide an approximate solution suitable for switching to the SUPG advection algorithm

84. Training Manual May 15, 2001 Inventory #001478 8-84 Stage 7: Extend case to Activate New Features Solution > FLOTRAN Setup –After the first 10 global iterations, access FLOTRAN Setup to Change solution options

85. Training Manual May 15, 2001 Inventory #001478 8-85 Solution > FLOTRAN Setup Choose Advection Choose SUPG for turbulence Choose SUPG for momentum OK 8 7 6 5 5 6 7 8 Activate SUPG Advection Scheme

86. Training Manual May 15, 2001 Inventory #001478 8-86 Solution > FLOTRAN Setup Choose Execution Ctrl Set 90 global iterations OK 10 6 9 11 9 10 11 Execution Control 90 more global iterations

87. Training Manual May 15, 2001 Inventory #001478 8-87 Execute ! Solution > Run FLOTRAN The Analysis will end after 100 Global Iterations

88. Training Manual May 15, 2001 Inventory #001478 8-88 Convergence Behavior

89. Training Manual May 15, 2001 Inventory #001478 8-89 Stage 8: Examine the Pressure Solution 1 2 2 OK Pressure Distribution 1 General Postprocessor > Last Set > Plot Results > Nodal Solu

90. Training Manual May 15, 2001 Inventory #001478 8-90 Stage 9: Read in Structural physics Once the CFD analysis is complete, the resulting pressures will be applied to the Separator in the nozzle and the outside 3 2 1 Solution > Physics Environ 1 Read Choose struc OK 2 3 Close boxes that arise

91. Training Manual May 15, 2001 Inventory #001478 8-91 1 2 3 4 1 2 3 4 Select Elements By Attributes Choose Material 2 OK Elements Stage 10: Reading In pressure loads from FLOTRAN Apply fluid pressures to the Separator : Select elements of Material 2 and associated nodes: Utility Menu: Select > Entities

92. Training Manual May 15, 2001 Inventory #001478 8-92 Pressure Load From FLOTRAN (continued) 9 10 11 Where to get pressures Solid for Elements Loads from (jobname).rfl file OK 12 9 10 11 12 10 11 Solution > Loads -Apply- > - Structural -Pressure

93. Training Manual May 15, 2001 Inventory #001478 8-93 Now apply pressure loads to the shell elements. 17 Select the Shell elements: Utility Menu: Select > Entities –Elements –By Attributes –Element type number –Shell elements have previously been defined as 4. –OK 13 14 15 16 13 14 15 1617

94. Training Manual May 15, 2001 Inventory #001478 8-94 181920 21 18 21 19 20 Pressure Load Transfer to Shells (continued) Where to get pressures Shell Face 1 for Shell 61s Loads from jobname (mix).rfl file OK

95. Training Manual May 15, 2001 Inventory #001478 8-95 Select Everything Utility Menu > Select > Everything Solve - Current load step Read and close any boxes that arise when solution is started. 1 1 Stage 11: Solve the StructuralProblem

96. Read in the last set of results: Main Menu: General Post Processor > Last Set Select elements by Type Number Utility Menu > Select > Entities Elements By Attributes Element type 2 and 4 OK Select Nodes associated with the elements Utility Menu > Select > Entities Nodes Attached to Elements OK 1254687 9 3 6 7 8 9 1 2 3 4 5 Stage 12: Post Process - Examine the deformation

97. PlotCtrls > Style > Disp Scaling Set displacment scaling to 1.0 OK Plot Results > Deformed Shape Deformed + Undeformed OK 1 2 3 4 4 3 2 1 Post Process (continued) - Plot Actual Deformed Shape

98. Training Manual May 15, 2001 Inventory #001478 8-98 Post Process (continued) - The Deformed shape resulting from pressure loads

99. Training Manual May 15, 2001 Inventory #001478 8-99 Solution > -Load Step Options - Other Updt Node Coord… Set to 1.0: Use all of the displacement Do not zero displacements OK 4 2 3 1 1 2 3 4 First select everything: Utility Menu > Select > Everything Stage13: Update the Nodal Coordinates with the deformed mesh

100. Training Manual May 15, 2001 Inventory #001478 8-100 Stage 14: Continuing the Sequential Solution Process Execution of the “new” CFD problem domain would result in a slightly different pressure distribution since the mesh has changed. The structural problem can then be solved again to see if the new pressure distribution results in significantly different displacements. Continued sequential solution can be done interactively or in a batch environment. The CFD analysis may be continued: –The Fluid Physics environment is activated as in Step 6 –Solve as in Step 7 If the structural analysis is repeated, the nodes should be returned to their original locations with the upcoord command. –Read in Structural physics environment as in Step 9 –Update nodal coordinates as in Step 13, with FACTOR set to -1 –Apply new pressure loads as in Step 10 –Re-solve structures as in Step 11