WS5-1 WORKSHOP 5 AXISYMMETRIC FLOW IN A PIPE NAS104, Workshop 5, March 2004 Copyright 2004 MSC.Software Corporation

WS5-2 NAS104, Workshop 5, March 2004 Copyright 2004 MSC.Software Corporation

WS5-3 NAS104, Workshop 5, March 2004 Copyright 2004 MSC.Software Corporation n Problem Description In this example we will analyze an axisymmetric structure for its temperature distribution. We will use the MSC.Nastran CTRIAX6 axi- symmetric element (in its 3 node configuration) as the heat conduction element. The basic geometry is detailed in the figure below. A section of pipe consisting of composite materials is divided into two different material regions. Region A is from radius 1.5 feet to 3.5 feet. Region B is from radius 3.5 feet to 4.75 feet. The overall pipe section is 5.0 feet long with an inside diameter of 3 feet and an outside diameter of 9.5 feet. Oil flows through the interior with an inlet temperature of 100 o F and a mass flow rate of 2.88E6 lbm/hr. The forced convection heat transfer coefficient between the oil and wall is calculated by MSC.Nastran using the following relationship: Nu=0.023Re 0.8 Pr Thermal conductivity properties for Region A and Region B are 0.2 and 0.5 Btu/hr/(ft* o F). Volumetric internal heat generation occurs in the subregion of Region B (from radius 3.5 feet to feet), and varies based on Z location. The heat generation is 1200*(1-Z/5) Btu/hr/ft 3, where Z is in units of feet. Free convection to an ambient temperature of 100 o F is applied to the exterior surface of the model through a heat transfer coefficient of 3.0 Btu/hr/(ft 2 * o F).

WS5-4 NAS104, Workshop 5, March 2004 Copyright 2004 MSC.Software Corporation

WS5-5 NAS104, Workshop 5, March 2004 Copyright 2004 MSC.Software Corporation n Suggested Exercise Steps 1. Create a new database 2. Set the solver as MSC.Nastran Thermal 3. Create the geometry 4. Mesh the fluid curve and pipe surfaces 5. Specify material 6. Define element properties 7. Define a spatial field 8. Apply volumetric heat generation 9. Apply free convection to outside of model 10. Define the inlet temperature of oil 11. Define coupled flow tube convection 12. All boundary conditions 13. Perform the thermal analysis 14. Attach the results file 15. Display the temperature results 16. Step 16: Quit MSC.Patran

WS5-6 NAS104, Workshop 5, March 2004 Copyright 2004 MSC.Software Corporation Step 1: Create a New Database Create a new database a.File: New b.Enter axisym for File name. c.Click OK. c a b

WS5-7 NAS104, Workshop 5, March 2004 Copyright 2004 MSC.Software Corporation Step 2: Set the Solver as MSC.Nastran Thermal Create the geometry a.Select Default for Tolerance. b.Select MSC.Nastran for Analysis Code. c.Select Thermal for Analysis Type. d.Click OK. c a b d

WS5-8 NAS104, Workshop 5, March 2004 Copyright 2004 MSC.Software Corporation Step 3: Create the Geometry a.Geometry: Create/Curve/XYZ b.Enter for Vector Coordinates List. c.Enter [0 0 0] for Origin Coordinates List. d.Click Apply. e.Click Bottom view Icon c a b d e

WS5-9 NAS104, Workshop 5, March 2004 Copyright 2004 MSC.Software Corporation Step 3: Create the Geometry (Cont.) a.Geometry: Create/Surface/XYZ b.Enter for Vector Coordinates List. c.Enter [ ] for Origin Coordinates List d.Click Apply. e.Enter for Vector Coordinates List. f.Enter [ ] for Origin Coordinates List g.Click Apply. h.Enter for Vector Coordinates List. i.Enter [ ] for Origin Coordinates List j.Click Apply. d b c j h i g e f

WS5-10 NAS104, Workshop 5, March 2004 Copyright 2004 MSC.Software Corporation Step 3: Create the Geometry (Cont.)

WS5-11 NAS104, Workshop 5, March 2004 Copyright 2004 MSC.Software Corporation Step 4: Mesh the Fluid Curve and Pipe Surfaces Mesh the curve representing the fluid(oil) and surfaces for the pipe. a.Element: Create/Mesh Seed/One Way Bias. b.Enter 10 for Number. c.Enter 2.0 for L2/L1. d.Enter Curve 1 Surface for Curve List. e.Click Apply. f.Element: Create/Mesh/Surface. g.Select Tria for Elem Shape. h.Enter IsoMesh for Mesher. i.Enter Tria3 for Topology. j.Enter Surface 1:3 for Surface List. k.Enter 0.25 for Value of Global Edge Length. l.Click Apply. c a b j i g h f d e k l

WS5-12 NAS104, Workshop 5, March 2004 Copyright 2004 MSC.Software Corporation Step 4: Mesh the Fluid Curve and Pipe Surfaces a.Elements: Create/Mesh/Curve. b.Select Bar2 for Topology. c.Enter Curve 1 for Curve List. d.Enter 0.25 for Value of Global Edge Length. c a b d e

WS5-13 NAS104, Workshop 5, March 2004 Copyright 2004 MSC.Software Corporation Step 4: Remove Coincident Nodes Connect elements a.Elements: Equivalence/All Tolerance Cube. b.Enter c.Click Apply. c a b

WS5-14 NAS104, Workshop 5, March 2004 Copyright 2004 MSC.Software Corporation Step 5: Specify Material Create isotropic material property for Region A. a.Materials: Create/Isotropic/Manual Input. b.Enter mat_a for Material Name. c.Click Input Properties… d.Select Solid properties for Constitutive Model. e.Enter 0.2 for Thermal Conductivity. f.Click OK. g.Click Apply. c a b g f d e

WS5-15 NAS104, Workshop 5, March 2004 Copyright 2004 MSC.Software Corporation Step 5: Specify Material (Cont.) Specify isotropic material property for Region B. a.Materials: Create/Isotropic/Manual Input. b.Enter mat_b for Material Name. c.Click Input Properties… d.Select Solid properties. e.Enter 0.5 for Thermal Conductivity. f.Click OK. g.Click Apply. c a b f d e

WS5-16 NAS104, Workshop 5, March 2004 Copyright 2004 MSC.Software Corporation Step 5: Specify Material (Cont.) Specify material property for oil a.Materials: Create/Isotropic/Manual Input. b.Enter oil for Material Name. c.Click Input Properties… d.Select Fluid properties for constitutive Model. e.Enter 0.77 for Thermal Conductivity. f.Enter 0.44 for Specific Heat. g.Enter 56.8 for Density. h.Enter for Dynamic Viscosity. i.Click OK j.Click Apply. c a b j i g h f d e ??

WS5-17 NAS104, Workshop 5, March 2004 Copyright 2004 MSC.Software Corporation Step 6: Define Element Properties Define axisymmetric element properties for Region A. a.Properties: Create/2D/ Axisym Solid. b.Enter pipe_a for Property Set Name. c.Click Input Properties… d.Click in Material Name box and select mat_a under Material Property Sets. e.Click OK. f.Enter Surface 1 for Select Members. g.Click Add h.Click Apply c a b g h f d e

WS5-18 NAS104, Workshop 5, March 2004 Copyright 2004 MSC.Software Corporation Step 6: Define Element Properties (Cont.) Define axisymmetric element properties for Region B. nProperties: Create/2D/Axisym Solid. nEnter pipe_b for Property Set Name. nClick Input Properties… nClick in Material Name box and select mat_b for Material Property Sets. nClick OK. nEnter Surface 2 3 for Select Members. nClick Add. nClick Apply. c a b g h f d e

WS5-19 NAS104, Workshop 5, March 2004 Copyright 2004 MSC.Software Corporation Step 6: Define Element Properties (Cont.) Define element properties for Bar2- s representing the oil. a.Properties/Create/1D/Flow Tube. b.Enter oil for Property Set Name. c.Click Input Properties.. d.Click in Material Name box and select oil under Material Property Sets. e.Enter 3.0 for Hydraulic Diam. at Node f.Click OK. g.Enter Curve 1 for Select Members. h.Click Add. i.Click Apply. c a b i g h f d e

WS5-20 NAS104, Workshop 5, March 2004 Copyright 2004 MSC.Software Corporation Step 7: Define a Spatial Field Define a spatial field for heat generation. a.Fields: Create/Spatial/PCL Function. b.Enter qvol_z for Field Name. c.Enter 1200*(1.0-Z/5.0) for Scalar Function. d.Click Apply. c a b d

WS5-21 NAS104, Workshop 5, March 2004 Copyright 2004 MSC.Software Corporation Step 8: Apply Volumetric Heat Generation Apply heat to elements in part of Region B. a.Loads/BCs: Create/Applied Heat/Element Uniform. b.Select Volumetric Generation for Option. c.Enter qvol for New Set Name. d.Select 2D for Target Element Type. e.Click Input Data… f.Select Basic for Form Type. g.Click in the Volumetric Heat Generation and select qvol_z under Spatial Fields. h.Click OK i.Click Select Application Region.. j.Enter Surface 2 for Select Surfaces. k.Click Add. l.Click OK. m.Click Apply. c a b j i g h f d e k l m

WS5-22 NAS104, Workshop 5, March 2004 Copyright 2004 MSC.Software Corporation Step 9: Apply Free Convection to Outside of Model Define convection on outside of Region B. a.Loads/BCs: Create/Convection/Element Uniform. b.Select To Ambient for Option. c.Enter conv for New Set Name. d.Select 2D for Target Element Type. e.Click Input Data… f.Enter 3.0 for Edge Convection Coef. g.Enter 100 for Ambient Temperature. h.Click OK. i.Click Select Application Region… j.Enter Surface 3.2 for Select Surfaces or Edges. k.Click Add. l.Click OK. m.Click Apply c a b j i g h f d e k l m

WS5-23 NAS104, Workshop 5, March 2004 Copyright 2004 MSC.Software Corporation Step 10: Define the Inlet Temperature of Oil Define the inlet temperature. a.Loads/BCs: Create/Temp(Thermal)/Nodal. b.Enter inlet_temp for New Set Name. c.Click Input Data.. d.Enter 100 for Boundary Temperature. e.Click OK. f.Click Select Application Region.. g.Enter Point 1 for Select Geometry Entities. h.Click Add. i.Click OK. j.Apply. c a b j i g h f d e

WS5-24 NAS104, Workshop 5, March 2004 Copyright 2004 MSC.Software Corporation Step 11: Define Coupled Flow Tube Convection Create convection for oil flow. nLoads/BCs: Create/Convection/Element Uniform. nSelect Coupled Flow Tube. nEnter coup_flow_tube for New Set Name. nTarget Element Type: 1D nRegion 2: 2D nClick Input Data… nSelect Advanced for Form Type. nEnter 2.88e6 for Mass Flow Rate. nEnter 0.23 for Heat Transfer Coefficient nSelect h=k/d*coef*Re**Eqpr*Pr** for Formula Type Option. nEnter 0.8 for Reynolds Exponent. nEnter for Prandtl Exponent, Heat in. nClick OK. nClick Select Application Region… nEnter Curve 1 for Select Curve. nClick Add. nClick Active List of Companion Region. nEnter Surface 1.4 for Select Surfaces or Edges. nClick Add nClick OK nClick Apply c a b l k i j h f g m n o p q m t u d e o r

WS5-25 NAS104, Workshop 5, March 2004 Copyright 2004 MSC.Software Corporation Step 12: All Boundary Conditions

WS5-26 NAS104, Workshop 5, March 2004 Copyright 2004 MSC.Software Corporation Step 13: Perform the Thermal Analysis Perform the steady-state thermal analysis a.Analysis: Analyze/Entire Model/Full Run. b.Enter axisym for Job Name. c.Click Apply. c a b

WS5-27 NAS104, Workshop 5, March 2004 Copyright 2004 MSC.Software Corporation Step 14: Attach the Results File Attach the results file a.Analysis: Attach XDB/Result Entities/Local. b.Click Select Results File… c.Select axisym.xdb for File name. d.Click OK. e.Click Apply. b a e c d

WS5-28 NAS104, Workshop 5, March 2004 Copyright 2004 MSC.Software Corporation Step 15: Display the Temperature Results Display the result a.Results:Create/Quick Plot. b.Select SC1DEFAULT,A1.. for Select Result Cases. c.Select Temperatures for Select Fringe Result. d.Click Apply. c a b d

WS5-29 NAS104, Workshop 5, March 2004 Copyright 2004 MSC.Software Corporation Step 16: Quit MSC.Patran Quit MSC.Patran a.Select File on the Menu Bar and select Quit from the drop down menu a

WS5-30 NAS104, Workshop 5, March 2004 Copyright 2004 MSC.Software Corporation