FEA Analysis of the LHCB Velo RF foil Simulations done with Comsol Multiphysics, and Siemens NX CAE (Nastran solver) by Jesse van Dongen Physical comparative tests done on a Half Rf foil test box by Tjeerd Ketel

Disclaimers These are priliminary results, i haven’t done any manual calculations for validation yet, however results have been cross validated in 2 different FEA programs All calculated values are based on linear solutions (stress stiffening or plastic deformation not taken into account, meaning comparing a solution of 10mbar vs -5mbar gives exactly half the stresses and deformation but in opposite directions) Perfect dimensions (effects of slight imperfections in straightness etc not taken into account in buckling analysis). Linear buckling (with instable post bucking behaviour a system could in reality buckle before the calculated value). Ideal material properties, it is assumed that the youngs and poisson ratio are always exactly the same as the bulk material properties. Triangular automatically generated mesh, depending on mesh coarseness can make a structure appear stiffer than in reality

Material Properties Used a generic type of aluminium for material properties Youngs modulus 70e9 Pa Poisson ratio 0.3 Yield 100e6 Pa

0.25 mm 2mm Box modelled using shell elements all material 0.5mm except 0.25 mm 2mm

Constraints Full 6 Dof constraint on the edges connected to the flange

Mesh (free 2d Tetraeder) (General note on tet meshes is that to deform a straight bending line is generally not possible, this means that a structure generally will perform slightly stiffer in simulations). In a similar sense calculated stresses are often higher than reality as well.

Material Material normal direction (grey top / yellow bottom)

10 mbar pressure (applied on the outside) Applied everywhere except for the 2mm ribs

No rounded off inner edges in Comsol model

Linear Buckling pressures Positive - overpressure outside the box Negative - overpressure inside the box -67mbar +100mbar +130mbar -90mbar

Notes on buckling Higher order buckling modes, are unlikely to occur due to lower mode buckling modes changing the structure shape. Buckling calculation was done with a nominal model, assuming for instance perfectly flat horizontal faces on the flat sides of the rffoil. In reality they are likely slightly arched, which means they can snap from one side to the other. A linear buckling analysis was done however as the modes are around a factor 7 away from the nominal buckling pressures, its assumed that this is plenty far away not to need to worry about buckling.

Gravity Sag when horizontal on flange Abs XYZ displacement [m] displacement in gravity direction [m]

Gravity Sag when horizontal with beamline Abs XYZ displacement [m] displacement in gravity direction [m]

Gravity Sag in real orientation Abs XYZ displacement [m] displacement in gravity direction [m]

Displacement 10mbar pressure + gravity sag Outwards applied 10mbar pressure [m]

10mbar pressure + gravity sag Pa

Stresses 10mbar pressure + gravity sag (log scale) Log10( [Pa] )

Detail Simulation of high stress areas Shell model does not take into account rounded off edges on the inside of the real model. Shell model does not take into account the mushrooms on the side Because of this a full 3d-simulation was done with NX Nastran of the side where the biggest stress occurs to get a more realistic number. As a form of validation Tjeerd did a physical test, which was later compared with the calculated solutions of both Comsol and NX

Fine Mesh In this detailed model, it was ensured that there would be at least 2 elements over the width, the mushrooms on the outside and the rounded edges on the inside were taken into account. Only the side was of interest, however a 2cm elongation was added to the system to distance the fixed constraint a bit from the point of interest.

Forces & Constraints Pressure Fixed Constraint

NX Detail Simulation Displacement mm

NX detailed Nodal Stresses Inside MPa MPa Elemental stresses give a value of 80Mpa, Nodal stresses give a value of 120Mpa (highest), this difference is due to triangular elements instead of quad/hexa elements. The real world value should be somewhere inbetween these 2 values.

General Discussion NX and comsol give comparable results, so likely the simulations were done correctly. Depending on the exact type of aluminium the Rfbox might yield slightly at the corner of the sides ( changing the rib design/ layout or overall side thickness could change this) A maximum deformation of ~ 1mm is expected at the side (with 10mbar over/under pressure) and ~0.4mm on top. As critical buckling loads are far enough away from the nominal loads, it assumed to be a non issue.

Real World Comparison

Real world Comparison 3.5 mbar overpressure 0.2 mm deformation Clock force 114g / ~ 1.1 N 0.6mm assumed side thickness

Comsol deformation m 1.1N Load

NX Deformation mm 1.1N Load

2nd Test A second test was performed to investigate the real world deformation performance better.

Maximal displacement is predicted at exit foil Maximal displacement is predicted at exit foil. Measured displacement is 0.25 mm at 4 mbar (4 cm)

Exit foil thickness is 0.57 mm 0.2 - 0.3 mm at 4 mbar

At the large distance slot Thinned foil thickness is 0.27 mm 0.1 – 0.15 mm at 4 mbar

Conclusions Displacement with pressure at exit foil is largest

Secondary FEA Test (NX detail analysis) mm 1.1N Load

Secondary FEA Test (Comsol simplified shell analysis) 1.1N Load

Discussion In general the simulation corresponds within 30% of the real values in terms of displacement. This result is worse than expected but is likely due to the usage of tetraeder elements for meshing. And not exact parameters used. However this still allows the results to be used. Overall both NX and Comsol give similar results to the real world scenario, this means that within the margin of error that it’s likely that the results can be trusted. Measurements were done at the end of the foil due to seeing the biggest stress and deformations there, allowing for more accurate measurement, however the key points of interest are logically near the modules. Based on this the following points can be made

Conclusion Deformation of the nomal box will result in ~1mm displacement at the ends of the RF foil and ~0.4mm displacement at the foil near the modules. The stress at the ends of the RF foil might yield or be close to yielding at 10mbar. This is initially no issue, however over time with this fatigue might be an issue.