FEA of Pressure Vessel and Nozzle Junction DHARMIT THAKORE MOONISH ENTERPRISES PTY LTD

Size: px

Start display at page:

Download "FEA of Pressure Vessel and Nozzle Junction DHARMIT THAKORE MOONISH ENTERPRISES PTY LTD"

Jean Waters
6 years ago
Views:

1 2013 FEA of Pressure Vessel and Nozzle Junction DHARMIT THAKORE MOONISH ENTERPRISES PTY LTD

2 Executive Summary The main objective of this project was to understand the Finite Element Analysis capability of Open Source Software Salome for Pre-processing and Post-processing and Code_Aster for analysis of a Pressure Vessel Nozzle junction. To obtain hexahedral mesh for the Pressure Vessel Half geometry. To analyse and compare Deflection and Vonmises stresses for three load cases for the geometry, Internal Pressure only, Force on Nozzle Only and a combination of Internal Pressure and Force on Nozzle. The main goal was to calculate Stresses by hand and compare them with the Finite Element Analysis results. Analysis was carried out on a half section of a pressure vessel with nozzle in the middle of the geometry, with sufficient symmetry and boundary conditions added for stability of the model. Linear analysis using hexahedral elements was carried out for this study. Salome version and Aster version was used for this analysis. From the study it can be seen that hand calculations closely match the Finite Element Analysis results for the geometry away from the Pressure Vessel and Nozzle junction. An effort has been made to calculate Membrane and Bending Stresses for comparison only at two Stress Classification lines at the Nozzle Pressure Vessel Junction. Further studies are required to evaluate stresses and analyse them based on ASME Section VIII Division 2 Part 5 rules and to obtain Membrane, Bending and Peak stresses.

3 Table of Contents Executive Summary... 1 Introduction... 3 Model Geometry... 4 Mesh Loads and Restraints Analysis of results Internal Pressure only Force Only Pressure and Force applied together Conclusions... 37

4 Introduction The main goal of this study was 1. To Model Pressure Vessel with Nozzle Geometry (Show step by step method of how is it done in Salome) 2. Partition it to make it ready for Hexahedral meshing 3. Mesh it with Hexahedral elements 4. Perform Finite Element Analysis with 3 load cases a. Internal pressure (both Hoop and Longitudinal stresses) b. Force of 9000N on Nozzle in Lateral direction to vessel geometry c. Combination of both a and b 5. Study the Stresses developed around the Nozzle Geometry (Discontinuity) 6. Compare the results with Hand Calculations Salome was used to model the geometry. The geometry modelling is carried out in Salome Geometry module, meshing was carried out in Salome Mesh module and then the mesh was exported in.msh format. Finite Element Analysis was carried out in Code_Aster and the results were exported in.msh format. This result mesh was imported in Salome again and Post Processing was carried out where Displacements and Vonmises stresses were evaluated. In this study Static Linear Finite Element Analysis was used to obtain results. Hexahedral mesh was used for this study. Quadratic mesh was not considered for this study. Vonmises stresses were calculated for the 3 load cases above and they were compared with hand calculations using first principles. Membrane and Bending stresses were calculated for two Stress Classification Lines (SCL) for all three load cases and are presented for comparison purposes only.

5 Model Geometry The model geometry is a half section of a Pressure Vessel modelled in positive X-Z zone of the coordinate system. This pressure vessel has a nozzle at the centre of it pointing in positive X direction. Half model of the entire pressure vessel was used in this study as the not-modelled section of the pressure vessel was very remote to the Nozzle geometry. Flange was not modelled on the nozzle end to minimise mesh size and computation time as this is the standard practice used in commercial software packages. Solid modelling was carried out in this study with following parameters.

First Argument (Point by 3 Co-ordinates) Name: Reference1; X: 0; Y: 0; Z: 1500; Click Apply and Close New Entiry -> Basic -> Vector -> Second Argument

6 OD of Pressure Vessel Shell = 3000mm OD of Nozzle = 300mm Height of the Pressure Vessel Shell = 3000mm ID of Pressure Vessel Shell = 2980mm ID of Nozzle = 280mm Height of the Nozzle = 200mm Modelling steps for the entire geometry are described below Salome -> Geometry Module New Entity -> Basic -> Point -> First Argument (Point by 3 Co-ordinates) Name: Reference1; X: 0; Y: 0; Z: 1500; Click Apply and Close New Entiry -> Basic -> Vector -> Second Argument (Vector by 3 Coordinates) Name: Vx; X: 10; Y: 0; Z: 0; Click Apply Name: Vy; X: 0; Y: 10; Z: 0; Click Apply Name: Vz; X: 0; Y: 0; Z: 10; Click Apply and Close

Argument (Cylinder by Base Point, Vector, Radius and Height) Name: Cyliner_3; Base Point: Reference1; Vector: Vx; Radius:

7 New Entiry -> Primitive -> Cylinder -> Second Argument (Cylinder by Radius and Height) Name: Cylinder_1; Radius: 1500; Height: 3000; Click Apply Name: Cylinder_2; Radius: 1490; Height: 3000; Click Apply Still in Cylinder Modelling Select First Argument (Cylinder by Base Point, Vector, Radius and Height) Name: Cyliner_3; Base Point: Reference1; Vector: Vx; Radius: 150; Height: 1700; Click Apply Name: Cyliner_4; Base Point: Reference1; Vector: Vx; Radius: 140; Height: 1700; Click Apply and Close

8 Operations -> Boolean -> Fuse -> Default Argument Name: Fuse_1; Object 1: Cylinder_1; Object 2: Cylinder_3; Click Apply Name: Fuse_2; Object 1: Cylinder_2; Object 2: Cylinder_4; Click Apply and Close Operations -> Boolean -> Cut -> Default Argument Name: Cut_1; Main Object: Fuse_1; Tool Object: Fuse_2; Click Apply and Close

9 Right Click Cut_1 in Object Browser and Select Show Only

10 New Entiry -> Primitive -> Box - > Second Argument Box by Dimensions at Origin) Name: Box_1; Dx: 1500; Dy: 3000; Dz: 3000; Click Apply and Close Operations -> Transformations -> Translation -> First Argument (By Dx, Dy, Dz) Objects: Box_1; Dx: ; Dy: -1500; Dz:0; Uncheck Create a Copy ; Click Apply and Close

11 Operations -> Boolean -> Cut -> Default Argument Name: Cut_2; Main Object: Cut_1; Tool Object: Box_1; Click Apply and Close Right Click Cut_2 in Object Browser and Select Show Only

Vz; Size of Plane: 7000; Click Apply and Close Operations -> Partition -> First Argument (By Objects

12 New Entiry -> Basic -> Plane -> First Argument (Plane by Point and Vector) Name: Plane_1; Point: Reference1; Vector: Vy; Size of Plane: 7000; Click Apply Name: Plane_2; Point: Reference1; Vector: Vz; Size of Plane: 7000; Click Apply and Close Operations -> Partition -> First Argument (By Objects and Tool Objects) Name: Partition_1; Objects: Cut_2; Tool Objects: Plane_1 & Plane_2; Click Apply and Close

Right Click Partition_1 in Object Browser and Select Show Only Point P1 Point P2 While Partition_1 is selected in Object Browser New Entiry -> Group -> Create -> First Argument (Shape Type Points )

13 Right Click Partition_1 in Object Browser and Select Show Only Point P1 Point P2 While Partition_1 is selected in Object Browser New Entiry -> Group -> Create -> First Argument (Shape Type Points ) Group Name: P1; Main Shape: Partition_1; Select Point on the extreme Z = 1500 (as shown in above figure); Click Add; Click Apply Group Name: P2; Main Shape: Partition_1; Select Point on the extreme Z = 1500 (as shown in above figure); Click Add; Click Apply and Close

New Entity -> Basic -> Point -> First Argument (Point by 3 Co-ordinates) Name: P3; X: 1500; Y: 0; Z: 2250; Click Apply Name: P4; X: 1500; Y: 0; Z: 750; Click Apply and Close New Entiry -> Basic ->

14 New Entity -> Basic -> Point -> First Argument (Point by 3 Co-ordinates) Name: P3; X: 1500; Y: 0; Z: 2250; Click Apply Name: P4; X: 1500; Y: 0; Z: 750; Click Apply and Close New Entiry -> Basic -> Plane -> Second Argument (Plane by 3 Points) Name: Plane_3; Point 1: P1; Point 2: P2; Point 3: P3; Size of Plane: 7000; Click Apply Name: Plane_4; Point 1: P1; Point 2: P2; Point 3: P4; Size of Plane: 7000; Click Apply and Close Operations -> Partition -> First Argument (By Objects and Tool Objects) Name: Partition_2; Objects: Partition_1; Tool Objects: Plane_3 & Plane_4; Click Apply and Close Right Click Partition_2 in Object Browser and Select Show Only Right Click Partition_2 -> Transparency: 70%

Right Click Cylinder_1 in Object Browser and Select Show Only New Entiry -> Group -> Create - > Third Argument (Shape Type Faces ) Group Name: PV_OD; Main Shape: Cylinder_1; Select Cylindrical

15 Right Click Cylinder_1 in Object Browser and Select Show Only New Entiry -> Group -> Create - > Third Argument (Shape Type Faces ) Group Name: PV_OD; Main Shape: Cylinder_1; Select Cylindrical Surface of Cylinder_1; Click Add; Click Apply and Close Right Click Cylinder_3 in Object Browser and Select Show Only New Entiry -> Group -> Create -> Third Argument (Shape Type Faces ) Group Name: Nozzle_OD; Main Shape: Cylinder_3; Select Cylindrical Surface of Cylinder_3; Click Add; Click Apply and Close Right Click Partition_2 in Object Browser and Select Show Only Operations -> Partition -> First Argument (By Objects and Tool Objects) Name: PV; Objects: Partition_2; Tool Objects: PV_OD & Nozzle_OD; Click Apply and Close

Right Click PV in Object Browser and Select Show Only Face PrLong Face DxDy Face Dx Face ForceE Face Dz New Entiry -> Group -> Create -> Third Argument (Shape Type Faces ) Group Name: DxDy; Main

16 Right Click PV in Object Browser and Select Show Only Face PrLong Face DxDy Face Dx Face ForceE Face Dz New Entiry -> Group -> Create -> Third Argument (Shape Type Faces ) Group Name: DxDy; Main Shape: PV; Select Right Vertical Face of the PV Shell if you are standing at Origin looking at the Nozzle in +X direction; Click Add; Click Apply Group Name: Dx; Main Shape: PV; Select Left Vertical Face of the PV Shell if you are standing at Origin looking at the Nozzle in +X direction; Click Add; Click Apply

17 Group Name: Dz; Main Shape: PV; Select Bottom Horizontal Face of the PV Shell; Click Add; Click Apply Group Name: PrLong; Main Shape: PV; Select Top Horizontal Face of the PV; Click Add; Click Apply Group Name: IntPress; Main Shape: PV; Select All Inside surfaces of the Pressure Vessel Shell and Nozzle (There should be 20 faces to be selected); Click Add; Click Apply Group Name: ForceE; Main Shape: PV; Select Front face of the Nozzle; Click Add; Click Apply and Close Following step is only required if you want to have a Sub Mesh in the thickness of the Shell and Nozzle. Still in Group Create -> Select Second Argument (Shape Type Wire ) Group Name: Sub5; Main Shape: PV; Select all Edges in the Shell Thickness at the Vertical and Horizontal Faces of the Shell, Select all Edges in the Nozzle Thickness (hdf file for this study is available for download); Click Add; Click Apply Right Click PV in Object Browser and Select Show Only This concludes Modelling exercise for the Pressure Vessel.

18 Mesh Entire geometry is meshed with 3D Linear Hexahedral elements. Global geometry was meshed with 3D Algorithm of Hexahedron (I,j,k), 2D Algorithm of Quadrangle (Mapping) and 1D Algorithm of Wire Discretisation with Hypothesis of Nb Segments of 50 Equidistant distribution. Following steps assumes that you are in Mesh module of Salome Mesh -> Create Mesh Name: PV; Geometry: PV (Select PV geometry from Geometry Module); 3D Tab: Algorithm: Hexahedron (i,j,k); 2D Tab: Algorithm: Quadrangle (Mapping); 1D Tab: Algorithm: Wire discretisation: Hypothesis: (Click Add Hypothesis Button and select) Nb_Segment; In Hypothesis Construction: Name: (Default) Nb. Segments_1; Number of Segments: 40; Type of distribution: Equidistant distribution; Click Ok; Click Apply and Close

Shell thickness was given a Sub Mesh with 1D Algorithm of Wire discretisation, with Hypothesis of Nb Segments of 5 Equidistant distribution and Additional Hypothesis of Propogation of

Right Click PV in Mesh Module in Object Browser and Select Create Sub-mesh Name: (Default) SubMesh_1; Mesh: PV; Geometry: (Select) Sub5 (from Geometry Module); 1D Tab: Algorithm: Wire

19 Shell thickness was given a Sub Mesh with 1D Algorithm of Wire discretisation, with Hypothesis of Nb Segments of 5 Equidistant distribution and Additional Hypothesis of Propogation of 1D Hypothesis on opposite edge. Right Click PV in Mesh Module in Object Browser and Select Create Sub-mesh Name: (Default) SubMesh_1; Mesh: PV; Geometry: (Select) Sub5 (from Geometry Module); 1D Tab: Algorithm: Wire discretisation: Hypothesis: (Click Add Hypothesis Button and select) Nb_Segment; In Hypothesis Construction: Name: (Default) Nb. Segments_2; Number of Segments: 5; Type of distribution: Equidistant distribution; Click Ok; Add. Hypothesis: (Click Add Hypothesis Button and select) Propagation of 1D Hyp. On opposite edges; Click Apply and Close

20 Right Click PV in Object Browser and Select Compute

21 Close-up of the Nozzle Mesh.

This mesh is suitable for Studying stresses generated in Pressure Vessel Shell. It is good for evaluating Bending, Peak and Membrane stresses in and around the Shell Nozzle junction.

22 This mesh is suitable for Studying stresses generated in Pressure Vessel Shell. It is good for evaluating Bending, Peak and Membrane stresses in and around the Shell Nozzle junction. Better Stress distribution can be obtained by using Quadratic meshing which will be done in future studies. Right Click PV in Object Browser and Select Create Groups from Geometry Mesh:PV; Geometry: (Select DxDy from Geometry Module) DxDy; Click Apply Mesh:PV; Geometry: (Select Dx from Geometry Module) Dx; Click Apply Mesh:PV; Geometry: (Select Dz from Geometry Module) Dz; Click Apply Mesh:PV; Geometry: (Select PrLong from Geometry Module) PrLong; Click Apply Mesh:PV; Geometry: (Select IntPress from Geometry Module) IntPress; Click Apply Mesh:PV; Geometry: (Select ForceE from Geometry Module) ForceE; Click Apply and Close Right Click PV in Object Browser and Select Export to MED file Select a location for the med file and save it.

23 Loads and Restraints To provide Symmetric Boundary Condition to the Pressure Vessel following Boundary Conditions were used. 1. Face DxDy was given Boundary condition of DX = 0.0 and DY = Face Dx was given Boundary condition of DX = Face Dz was given Boundary condition of DZ = 0.0 Three load cases were considered in this analysis 1. Internal Pressure of 0.5MPa applied on the Internal Face of the pressure vessel 2. Force of Fy = 9000N applied on the face of the flange 3. Combined Internal Pressure and Force To account for the discontinuity in the Pressure Vessel shell, force equivalent to the Pressure acting on the inside of the Nozzle was applied in Fx direction on face ForceE. If this balancing force was not applied, Pressure Vessel Ovalization occurred due to un-balanced distribution of the Pressure on internal face..comm file used for analysis with Code_Aster is shown here for easy reference. This file is commented sufficiently to give information on what is going on. DEBUT(); #Define Material Steel Steel=DEFI_MATERIAU(ELAS=_F(E= , NU=0.3,),); #Read the mesh in 'MED' format MAIL=LIRE_MAILLAGE(FORMAT='MED',); #Assign the model Mechanical and in 3D MODE=AFFE_MODELE(MAILLAGE=MAIL, AFFE=_F(TOUT='OUI',

24 PHENOMENE='MECANIQUE', MODELISATION='3D',),); #Assign the material Steel previously defined MATE=AFFE_MATERIAU(MAILLAGE=MAIL, AFFE=_F(TOUT='OUI', MATER=Steel,),); #Boundary Condition 'Base' is Fixed in all directions BCs=AFFE_CHAR_MECA(MODELE=MODE, FACE_IMPO=(_F(GROUP_MA='Dx', DX=0.0,), _F(GROUP_MA='DxDy', DX=0.0, DY=0.0,), _F(GROUP_MA='Dz', DZ=0.0,),),); #To Balance Internal Pressure at Nozzle Junction Press1 = 0.5; NozOR = 150.0; NozIR = 140.0; NozArIR = 3.14 * NozIR * NozIR; ForceBal = NozArIR * Press1; ForceBal = ForceBal / (3.14 * (NozOR * NozOR - NozIR * NozIR)); #To apply Longitudinal Stress PVOR = ; PVIR = ; PVArIR = 3.14 * PVIR * PVIR;

25 LongStr = PVArIR * Press1; #Pressure is applied on 1/2 Area for Hoop and is resisted by 1/2 Area so 1/2 cancels out LongStr = LongStr / (3.14 * (PVOR * PVOR - PVIR * PVIR)); #Force of 9000N is distributed over the Area of Nozzle Tip ForceY = / (3.14 * (NozOR * NozOR - NozIR * NozIR)); Loads=AFFE_CHAR_MECA(MODELE=MODE, PRES_REP=_F(GROUP_MA=('IntPress'), PRES=Press1,), FORCE_FACE=(_F(GROUP_MA='PrLong', FZ=LongStr,), _F(GROUP_MA='ForceE', FY=ForceY,), _F(GROUP_MA='ForceE', FX=ForceBal,),),); RESU=MECA_STATIQUE(MODELE=MODE, CHAM_MATER=MATE, EXCIT=(_F(CHARGE=BCs,), _F(CHARGE=Loads,),),); #Calculate fields on Elements RESU=CALC_ELEM(reuse =RESU, RESULTAT=RESU, OPTION=('SIEF_ELNO','SIEQ_ELNO','SIGM_ELNO'),); #Calculate fields on Nodes RESU=CALC_NO(reuse =RESU, RESULTAT=RESU, OPTION=('SIGM_NOEU','SIEQ_NOEU','REAC_NODA',),);

26 #Dump the entire result in a text file IMPR_RESU(FORMAT='RESULTAT', RESU=_F(MAILLAGE=MAIL, RESULTAT=RESU, NOM_CHAM=('SIEQ_ELNO','SIEQ_NOEU','DEPL','REAC_NODA','SIGM_NOEU'),),); #Dump the result in.med file that can be read by Salome IMPR_RESU(FORMAT='MED', UNITE=80, RESU=_F(MAILLAGE=MAIL, RESULTAT=RESU, NOM_CHAM=('SIEQ_ELNO','SIEQ_NOEU','DEPL','REAC_NODA','SIGM_NOEU'),),); FIN(); The output from the analysis is saved as a.med file that can be read by Salome and used for Post processing.

The displacement and VonMises stresses are shown below Below is the snapshot of displacement with scale factor of 100.

27 Analysis of results - Present the displacement and Stress results (Including plots and animation) Internal Pressure only The first of the three cases analysed was Internal Pressure only Internal Pressure of 0.5MPa is applied to the inside of the Pressure Vessel and Nozzle. The displacement and VonMises stresses are shown below Below is the snapshot of displacement with scale factor of 100. Maximum displacement is 1.2mm. This is inline with the growth of diameter of the vessel as calculated manually. Below is the displacement upclose near the nozzle.

28 The Vonmises stress snapshot is shown below Below is the Vonmises stresses upclose

29 Vonmises stresses on the inside of the Pressure Vessel Vonmises stresses on the inside upclose

Force Only Force of 9000N is applied on the face of the Nozzle in

30 Vonmises stresses remote to the nozzle is 65MPa which is inline with the hand calculation. Force Only Force of 9000N is applied on the face of the Nozzle in Fy direction. The displacement and Vonmises stresses for Force Only case is shown below. Displacement upclose

31 Vonmises stresses for the Force only is shown below Vonmises stresses upclose

32 Vonmises on the inside of the Pressure Vessel Vonmises on the inside upclose

pressure vessel remote to the nozzle should remain unchanged and that is what

33 Pressure and Force applied together The combination of Pressure and Force will see some stresses around the nozzle increase but the overall stresses in the pressure vessel remote to the nozzle should remain unchanged and that is what is seen in the analysis. Displacement for Pressure and Force. Displacement upclose

34 Vonmises stresses Vonmises upclose

35 Vonmises on the inside of the pressure vessel Vonmises stresses on the inside of the pressure vessel upclose

36 As can be seen above in the Vonmises stresses on the inside of the Pressure Vessel, the equivalent stresses have fallen from 231 MPa in Pressure Only case to 198 MPa in Pressure and Force case. For evaluation and comparison purposes, Bottom Negative Y Quarter section of the nozzle is shown with VonMises Stresses for all three load cases. First Column is for Pressure Only Load case, Second Column is for Force Only Load Case and Third Column is for combined case. First Row is showing complete Clipped Model, Second Row is showing SCL2 and Third row is showing SCL1. Pressure Only Force Only Pressure and Force

37 Two stress Classification Lines were taken for this study and the tabulated SIXX, SIYY, SIZZ, SIXY, SIYZ, SIZX, Vonmises total along with Membrane and Bending stresses are presented here Pressure Only Force Only Pressure and Force Only SCL1 SCL1 SCL1 Membrane Bending Membrane Bending Membrane Bending Stress (MPa) Stress (MPa) Stress (MPa) Stress (MPa) Stress (MPa) Stress (MPa) SIXX SIYY SIZZ SIXY SIYZ SIZX Total SCL2 SCL2 SCL2 Membrane Bending Membrane Bending Membrane Bending Stress (MPa) Stress (MPa) Stress (MPa) Stress (MPa) Stress (MPa) Stress (MPa) SIXX SIYY SIZZ SIXY SIYZ SIZX Total Evaluation of the stresses is left to the reader. Future aspirations from this analysis are to perform FEA based on ASME Section VIII Division 2 Part 5 rules. Use Stress Classification line to find out Membrane, Bending and Peak stresses which shall be carried out in future analysis and documented in a report. Vonmises stresses were used as a criteria to determine equivalent stress for comparison.

38 Conclusions From this study it can be concluded that Finite Element analysis results match that of hand calculations at location remote to the Nozzle Pressure Vessel junction. This study is not exhaustive and was conducted to try modelling Pressure Vessel geometry and partition it to make it ready for meshing, To mesh the Pressure Vessel geometry with Hexahedral mesh, To carry out Finite Element analysis of a Pressure Vessel Nozzle section using Code_Aster for analysis, And to perform Post Processing using Salome. Outcome of the analysis can be summarised as 1. Salome can be used as a competent software to model the geometry, Mesh it and perform Post Processing on the results 2. Code_Aster is a powerful software but due to it being in Non-english format is a restriction. 3. Open Source softwares can be used for performing FEA based on ASME Section VIII Division 2 Part 5. This study is just a preliminary analysis. For further study following actions are recommended 1. Use of 2 nd order or Higher order elements 2. Mesh refinement around the nozzle shell junction 3. Evaluate Stresses based on ASME Section VIII Division 2 Part 5 rules.

MAE 323: Lab 7. Instructions. Pressure Vessel Alex Grishin MAE 323 Lab Instructions 1

MAE 323: Lab 7. Instructions. Pressure Vessel Alex Grishin MAE 323 Lab Instructions 1 Instructions MAE 323 Lab Instructions 1 Problem Definition Determine how different element types perform for modeling a cylindrical pressure vessel over a wide range of r/t ratios, and how the hoop stress