1. Wrap up of the thermal and thermo mechanical simulation on the IBL stave Simone Coelli Mauro Monti INFN Milano ATLAS PIXEL Inserted B-Layer Eng. Meeting 3 February 2009

2. EDMS PAGES WITH REPORT ON THE FEM SIMULATIONS ATL-IP-EA-0002 In Work Thermo mechanical simulation of the homogeneous stave 1-REPORT ON THE NEW STAVE THERMO-MECHANICAL FEM SIMULATIONS FOR ATLAS PIXEL DETECTOR B-LAYER REPLACEMENT 2-FINITE ELEMENT METHOD VALIDATION REPORT FOR THERMO-STRUCTURAL SIMULATIONS ON THE NEW STAVE COOLING PIPES Will be soon upgraded with new updated summary report documents on the FEM simulations Inserted B-Layer Eng. Meeting 3 February 20092

3. SUMMARY: Inserted B-Layer Eng. Meeting 3 February 20093 The purpose of this document is to summarize the results of FEM simulations carried out till now on the new B-Layer Stave concept for the Atlas Pixel Detector. Simulation Finite Element Analysis software used is ANSYS code (11.0). Cross-check calculation have been made using the Classical Laminate Theory (CLT). The software ESAComp has been used for a cross-check of some laminate thermal expansion coefficient (CTE). The following subjects have been studied: -VALIDATION OF THE METHOD: comparison of ANSYS and CLT results for easy to handle problems -THERMAL STEADY-STATE: temperature field on the new stave with pipe cooling and power on (max heat flux from modules 7200 W/m 2 ) -STATIC STRUCTURAL MECHANICS: stress and deformation in the composite pipe caused by the internal pressure (design pressure 150 bar) and composites CTE calculation (using a ΔT). -THERMO-MECHANICAL SIMULATION: full length stave (800 mm) stress and deformation induced by the thermal field, cooling down the stave to -40°C from the ambient temperature 20°C, considering both the alternatives with power on modules or not.

4. VALIDATION OF THE METHOD Inserted B-Layer Eng. Meeting 3 February 20094 Comparison of ANSYS and CLT results for easy to handle problems These mechanical simulations were performed with standard load conditions provided by the science of construction and the FEM results were compared with the theoretical calculated values, in order to validate the FE models and the boundary conditions applied. The FE models used have the same characteristics (type of elements, element dimensions, number of elements, etc.) of the components in the Stave FE model We carried out some mechanical simulations on a pipe under different loading conditions. The pipe materials in the simulations are aluminium (isotropic) and composite carbon fiber/epoxy laminate with two different lay-up.

5. VALIDATION OF THE METHOD Inserted B-Layer Eng. Meeting 3 February 20095 Single ply monoaxial stress simulation, changing fibers orientation.

6. Inserted B-Layer Eng. Meeting 3 February 20096 Single ply biaxial stress simulation, changing fibers orientation.

7. Inserted B-Layer Eng. Meeting 3 February 20097 Single ply biaxial stress simulation like in a cylindrical pressure vessel (Mariotte theory) changing fibers orientation.

8. Inserted B-Layer Eng. Meeting 3 February 20098 Single ply shear stress simulation, changing fibers orientation.

9. Inserted B-Layer Eng. Meeting 3 February 20099 Single ply biaxial stress plus shear stress simulation, changing fibers orientation.

10. Inserted B-Layer Eng. Meeting 3 February 200910 Single ply thermal strain due to uniform heating simulation, changing fibers orientation.

11. Inserted B-Layer Eng. Meeting 3 February 200911 Single ply thermal strain due to uniform heating simulation and mechanical stress, changing fibers orientation.

12. Inserted B-Layer Eng. Meeting 3 February 200912 LAMINATE monoaxial stress simulation, changing lay-up.

13. Inserted B-Layer Eng. Meeting 3 February 200913 LAMINATE biaxial stress simulation, changing lay-up.

14. Inserted B-Layer Eng. Meeting 3 February 200914 LAMINATE ply biaxial stress simulation like in a cylindrical pressure vessel (Mariotte theory), changing lay-up.

15. Inserted B-Layer Eng. Meeting 3 February 200915 CARBON FIBER COMPOSITE PIPE biaxial stress simulation as a cylindrical pressure vessel, axial symmetric shell element changing lay-up, OD, thickness.

16. Inserted B-Layer Eng. Meeting 3 February 200916 CARBON FIBER COMPOSITE PIPE biaxial stress simulation as a cylindrical pressure vessel, Looking at the strain and stress of the laminate global and in the single plies.

17. Inserted B-Layer Eng. Meeting 3 February 200917 CARBON FIBER COMPOSITE OR METALLIC PIPE MECHANICAL SIMULATIONS FOR VALIDATION PIPE FE MODEL The main characteristics of the pipe FE model are the following: OUTSIDE DIAMETER D = 3.0 mm INNER DIAMETER d = 2.4 mm WALL THICKNESSt = 0.30 mm LENGTHl =100 mm AVERAGE RADIUSR m =1.35 mm FE MODEL ELEMENTSSOLID186 STRUCTURAL for aluminium pipe SOLID186 LAYERED for composite pipe NUMBER OF ELEMENTS3200 (n.32 in the cross section x n.100 along longitudinal axis) ELEMENT DIMENSIONS0.3 x 0.3 x 1 (length) mm COMPOSITE LAMINATE – LAY UP ± 54.7 Carbon Fiber : T-300 (HR) Matrix:Epoxy Lay-up:2 layers -54.7/+54.7 Layer thickness:0.15 mm V f :60% COMPOSITE LAMINATE – LAY UP 0-90-0 Carbon Fiber : T-300 (HR) Matrix:Epoxy Lay-up:3 layers 0-90-0 Layer thickness:0.10 mm V f :60%

18. Inserted B-Layer Eng. Meeting 3 February 200918 F AXIAL TENSILE LOAD FE MODEL CONSTRAINTS Pipe end face 1 (at X=0 mm) : all nodes constrained UX,UY,UZ Nodal solution - displacement vector sum Amplified scale (10) Element solution - stress along fibers in layer 1

19. Inserted B-Layer Eng. Meeting 3 February 200919 SUPPORTED PIPE DEFLECTION DUE TO GRAVITY EFFECT

20. Inserted B-Layer Eng. Meeting 3 February 200920 CANTILEVERED PIPE DEFLECTION DUE TO GRAVITY EFFECT

21. Inserted B-Layer Eng. Meeting 3 February 200921 PIPE INTERNAL PRESSURE Pipe subjected to internal pressure and hydrostatic head pressure. FE MODEL CONSTRAINTS Pipe end face 1 (at X=0 mm): all nodes constrained UX,UY,UZ (see picture 19)

22. Inserted B-Layer Eng. Meeting 3 February 200922 STAVE SIMULATIONS WITH DIFFERENT MESH

23. THERMAL STEADY-STATE SIMULATIONS Inserted B-Layer Eng. Meeting 3 February 200923 THERMAL STEADY-STATE calculation of the temperature field on the new stave with pipe cooling and power on (max heat flux from modules 7200 W/m 2 ). Internal wall pipe temperature set to 0° C. Mono-pipe and bi-pipe cases.

24. THERMAL STEADY-STATE SIMULATIONS Inserted B-Layer Eng. Meeting 3 February 200924 THERMAL STEADY-STATE: temperature field on the new stave with pipe cooling and power on (max heat flux from modules 7200 W/m 2 ). See next table for the results. Thermal simulation with aluminum pipe - nodal temperatures resulting Thermal simulation with carbon pipe - nodal temperatures resulting Thermal simulation with titanium pipe - nodal temperatures resulting Comparison between staves with different pipe materials: -Carbon fiber composite (0.3 mm) -Aluminum (0.3 mm) -Titanium (0.1 mm)

25. THERMAL STEADY-STATE SIMULATIONS Inserted B-Layer Eng. Meeting 3 February 200925 THERMAL STEADY-STATE: temperature field on the new stave with pipe cooling and power on (max heat flux from modules 7200 W/m 2 ). See next table for the results. Thermal simulation with aluminum pipes - nodal temperatures resulting Thermal simulation with carbon pipes - nodal temperatures resulting Thermal simulation with titanium pipes - nodal temperatures resulting Comparison between staves with different pipe materials: -Carbon fiber composite (0.3 mm) -Aluminum (0.3 mm) -Titanium (old value 0.3 mm)

26. THERMAL STEADY-STATE SIMULATIONS summary table Inserted B-Layer Eng. Meeting 3 February 200926

27. 27 COMPOSITE PIPE STATIC STRUCTURAL MECHANICS PIPE 3D FE MODEL PIPE ELEMENTS COORDINATE SYSTEMS FOR LAYERED ELEMENTS ORIENTATION The materials database which we refer for the simulations, is located at the following web address: http://dgiugni.web.cern.ch/dgiugni/upgrade/simulation/ In the database are collected the known materials mechanical and thermal properties. The materials used for the composite pipe simulations are : Carbon fiber: T300 HR Matrix:Epoxy, with two different CTE (70 ppm/C or 110 ppm/C) Volume fiber ratio (V f ) :60% (baseline) or, alternatively, 30% (*) (*) For the carbon pipe with lay-up [54,7 / -54,7] also have been carried out simulations with Vf = 40%, 50% and 70%,only for the calculation of the CTE.

28. Composite pipe CTE evaluation using a ΔT as input to derive the lengthening Vf=30% 28

29. Composite pipe CTE evaluation using a ΔT as input to derive the lengthening Vf=60% 29

30. 30 - Max stress - safety factor (Tsai-Hill failure criterium) - strain (using transversal strain for tightness verification) Ply calculation for a composite pipe with internal pressure (design pressure 150 bar)

31. 31 Optimization of the carbon pipe The design of the laminate of the pipe should satisfy three basic criteria: -150 bar test pressure with minimum safety factor SF = 4 - Stay tight under pressure, transversal plies strains ε T 0.1%, in order to avoid the microcracks growth - Match the longitudinal CTE of the other materials (about -2 ppm/C for the CFRP Omega support with lay-up [0/60/-60] S2 and -0.7/+0.6 ppm/C for the carbon foam). From the simulation results the best lay-up matching the three criteria are: [45 / -45] or [±55/±40]

32. THERMO-MECHANICAL SIMULATIONS 32 Constraints diagram 3D FE MODELS CHARACTERISTICS All the simulations have been executed with 3D FE models, for both the different geometries (mono-pipe and bi-pipes stave). The 3D FE models main characteristics are the following: Model length [mm]800 Elements typesHexahedral 20 nodes bricks For Thermal analysis:element Solid90 For Structural analysis:element Solid186 structural type for isotropic materials layered type for composite materials Number of elements94,750 for mono-pipe stave geometry 88,000 for bi-pipes stave geometry Elements typical dimensions [mm]0.3 x 0.3 (sides) x 3.2 longitudinal length Ratio length/side 10 Meshing techniques Pipes and omega support: mapped mesh in volume Carbon Foam: free extruded mesh Elements coordinate system orientedCarbon pipes and omega (composite materials) Contacts between parts: Merged nodes

33. THERMO-MECHANICAL SIMULATIONS: to determine the behavior (deformation and stress) of the full length stave subjected to a temperature decrement as: 1- A fixed ΔT = -60 C° 2- The nodal thermal field from the previous thermal analysis (assuming the temperature of the inner surface of the cooling pipes as 0°C). The ΔT value of -60 C° is determined by the difference between the minimum temperature value of the cooling fluid in the pipes (-40 °C) and the environment temperature, that we assume as 20 °C. So, having fixed to 0°C the temperature of the inner surface of the cooling pipes in the thermal analysis, we consider 60°C the temperature of the non deformed stave FE model in the mechanical environment. 33 RESULTS EVALUATED IN THERMO-MECHANICAL SIMULATIONS We want evaluate the following things: -Maximum stave bow in the middle length – UZ [µm] -Maximum stave deformation – USUM [µm] -Maximum Von Mises stress in the carbon foam – SEQV [MPa] -Maximum compression stress in the carbon foam – SX [MPa] -Maximum shear stress in the carbon foam – SXY [MPa]

34. THERMO-MECHANICAL SIMULATIONS 34 Thermo-mechanical simulation with carbon pipe: Stave bow Thermo-mechanical simulation with carbon pipe: carbon foam Von Mises stress Thermo-mechanical simulation of the stave with one carbon pipe

35. THERMO-MECHANICAL SIMULATIONS 35 Thermo-mechanical simulation with Titanium pipe: Stave bow Thermo-mechanical simulation with Titanium pipe: carbon foam Von Mises stress Thermo-mechanical simulation of the stave with one Titanium pipe

36. THERMO-MECHANICAL SIMULATIONS 36 Thermo-mechanical simulation with Aluminum pipe: Stave bow Thermo-mechanical simulation of the stave with one Aluminum pipe

37. THERMO-MECHANICAL SIMULATIONS 37 Thermo-mechanical simulation with carbon pipes: Stave bow Thermo-mechanical simulation with carbon pipes: carbon foam Von Mises stress Thermo-mechanical simulation of the stave with two carbon pipes

38. THERMO-MECHANICAL SIMULATIONS summary table 38

39. THERMO-MECHANICAL SIMULATIONS 39