ANSYS simulation of carbon fiber and anisotropic materials

The ATLAS Pixel Detector during construction. Here we can see one of the cylindrical shells of Pixel detectors formed by the longitudinal cooled supports called staves.

Introduction
The scope of this R&D is to develop a new support, with an integrated cooling system, for the replacement of the inner layer of the Silicon Pixel Detector installed into the ATLAS Experiment, working on the Large Hadron Collider at CERN; for details, we ask our readers to visit: www.atlas.ch/pixel-detector.html. This replacement will become necessary because of the radiation damage, with the detector being very close, about 50 mm, to the high-energy proton-proton interaction point.

The task of the support system is to hold the detector modules in positions with high accuracy, minimizing the deformation induced by the cooling; this must be done with the lowest possible mass because there are tight requirements in terms of material budget. An evaporative boiling system to remove the power dissipated by the sensors is incorporated in the support: thermal contact is made through a very conductive light carbon foam to maintain the sensor temperature sufficiently low, to limit the leakage currents and hence the thermal run-away. The coolant should be a fluorocarbons blend or CO2. The worst case is imposing a cooling pipe design pressure of 10 MPa. The number of pipes could be 1 or 2 and the pipe material should be carbon fiber or titanium. The structural strength of the 800 mm long support stave is given from a carbon fiber “omega” shaped laminate.

Summary of the work
The design is based on thermal, mechanical and thermo-structural analyses of assemblies made of carbon fiber composites. Calculation of the Tsai-Hill safety factors and transversal strains in the plies are required for tightness assessment of the pipe. Moreover, the pipe lay-up optimization against the internal pressure has been made together with estimations of the thermal expansion coefficient of the pipe and omega laminates.

Prototype of a stave with 2 carbon fiber pipes integrated into the carbon foam and attached to the structural omega shaped laminate.

We used ANSYS and ESAComp; input figures for the ply properties, starting from fiber and matrix values, are provided by a dedicated spreadsheet. To validate the FEM simulations both Composite Laminate Theory hand-made calculations on cross-check simple models and experimental tests are used. Work is still in progress to measure material characteristics and FEM results: pull test on pipes performed with “braided” technology, burst pipe pressure, thermal transmission coefficient K of the carbon pipe, CTE and deformations induced by the cooling using a Coordinate Measuring Machine.
The R&D key element is the production of the CF pipe and of the relative joints versus the external connecting piping, having suitable mechanical and tightness properties.

FEM of composite materials

Some assumptions are taken up in building the model and some parameters needed to run the software should be guessed as they are absent in literature (i.e. ply out-of-plane moduli and Poisson coefficient). A major problem found in building the models is the necessity to correctly orient the layered elements for the composites which turns out to be very time consuming. Moreover, in the multi-physics, during the switching from structural to thermal analysis automatically a different orientation of the thermal element coordinate systems is set; the use of dedicated APDL macro routines can be useful to optimize the FEM workflow. We used several meshing techniques: mapped mesh for composites materials and free mesh in 2D or extruded mesh in 3D for the anisotropic materials. Geometry of the anisotropic carbon foam has been carefully conditioned in order to avoid degenerated shape elements. We have chosen to assemble models, avoiding the use of contact elements between the meshed parts in order to obtain a practicable linear solution method, merging the interfacing nodes and reducing both the number of elements and the run-time. Comparisons between different sized meshes, with aspect ratio ranging from 1 to 10, and between 2D cross section and 3D solutions have been judged for time optimization and control purposes.

Carbon fiber pipe production test using braiding technology, before impregnation with resin

The use of brick elements for thin solids was driven by our specific multi-physics needs.

Note that the composite pipe produced by the “braiding” technology can only in first approximation be simulated by the laminate multi-ply hypothesis, like those implemented in the layered elements available at present. This could be an interesting ANSYS product development. We are also in contact with the DIGIMAT micro-mechanics developers to study the problem.

Thermal performance
The thermal performances of the different configurations proposed are studied with steady-state 2D simulations. Heat flux is applied while the BC is the temperature setting of the cooling pipes inner surface. We collected the resulting max ΔT across the staves in a table, using a performance parameter obtained by dividing ΔT by the thermal power flux imposed as load.

Cross section example of a finite element model. Note the mapped mesh for the laminate pipe and omega, whose one possible stacking sequence is showed.

Evaluation of the thermal expansion coefficients
Longitudinal CTE is calculated for the possible configurations; the simulations are executed with the volume fiber percentage measured on the samples, ranging from 30% to 60%. The calculation procedure is to build a model and increase the nodal temperature in order to have a ΔT: the nodal displacement is evaluated and the relative CTE is then calculated. ESAComp has been used for cross check.

Internal pressure and longitudinal stress applied to the pipe

Pressurized pipe lay-up optimization
The design of the pipe laminate should satisfy these criteria: withstanding a pressure test of 15 MPa, having a safety factor of 4 on the design pressure against a Tsai-Hill failure criterion, matching the longitudinal CTE of the other materials, remaining tight under pressure with maximum transversal ply strain ≤ 0.1%. This is the parameter that controls the micro-cracks growth. Pipe is modelled using the element layered-type Solid186. Pressurized vessel conditions are simulated with axial force on the pipe extremities. Different pipe stacking sequences are considered for these structural simulations; for each ply longitudinal, transversal and shear stresses and strains are extracted for the result analysis, used directly or combined in the failure criteria.
Comparison between the stress values or Tsai-Hill index resulting from the simulation and the corresponding rupture stress values of the ply is done. Lastly, the best lay-up, matching the requirements and including technological feasibility, is [45/-45]s.

Thermal solution example

Deformations induced from gravity, cooling and pipe pressurization
To understand the thermo-mechanical effects, we first performed 3D thermal simulations using 20 node Solid90 elements, in order to determine the temperature field under defined heat flux. The resulting nodal temperatures have been imported, node to node, in the structural environment, using Solid186 elements to determine the deformations and stress of the stave components due to the thermal induced deformation, related to the different CTE values of the materials. Coefficients of thermal expansion of the ply are calculated by the Schapery formulas. In the following study the loads applied to analyse the behavior of the stave are: 1) cooling-down: ΔT = -60°C, that is the ΔT between the assembling temperature and the minimum evaporation temperature; 2) static gravity to evaluate the maximum deformation due to the weight; 3) pressure 10 MPa inside the cooling pipe.

Thermo-mechanical simulation results for a given configuration.

Conclusions
A number of considerations have been taken into account in the frame of this collaboration with regard to all ANSYS silmulation results and other parameters, such as the global radiation length, to optimize the assembly properties. The final choice to be made will also depend on the measurements in progress on the real prototypes.

The ANSYS software can be used as a useful tool for the model analysis with composite and anisotropic materials. A lot of work has been devoted to understanding the method, and then to building the required models in a proper way, for achieving the various simulation goals. The real measurement performed on a pipe prototype, actually the CTE of a CF pipe, provides a first positive feedback from the R&D work which is still in progress.

Acknowledgments
Thanks to the colleagues of the INFN Milano Mechanical Design and Workshop Department, in particular Mauro Monti, the responsible for the simulations and to Danilo Giugni and the whole ATLAS Insertable B-Layer Collaboration.

Ing. Simone Coelli
Istituto Nazionale di Fisica Nucleare
Sez. di Milano