1.3-GHz Superconducting
Radio Frequency Cavity
Stress and Buckling Analysis
Ashish KUMAR
CASA, Accelerator Laboratory,
High Energy Accelerator Research Organization (KEK)2021/09/09
2021/09/09

1

Contents
1. Cryomodule Assembly
2. Pressure Vessel Compliance for Cryomodules
3. Structural Analysis using FEA
4. 1.3 GHz 3-Cell SRF Cavity Structural Analysis
5. Eigen value Buckling Analysis
6. 1.3 GHz 3-Cell SRF Cavity Buckling Analysis
7. 1.3 GHz 3-Cell SRF Cavity Non-linear Buckling Analysis
2021/09/09

2

Cryomodule Assembly

2021/09/09

3

ILC Cryomodule

2021/09/094

Cryomodule Cross-sectional View
 2 K two-phase superfluid heliumpipeline

 2 K gas helium return line.
 5 K shield line and 80 K or 40 Kshield line.

 Cold mass at 2 K is enclosed withtwo thermal shields
 No issues with pressure vessel
compliance for these lines.

2021/09/09

5

Pressure Vessel Compliance

2021/09/09

6

1.3 GHz 9-Cell SRF Cavity Assembly
Niobium SRF Cavity with its Titanium
jacket is considered as a pressure vessel
Design must be cleared by high-pressure
gas safety authorities
Determine maximum allowable stressand buckling pressure using ANSYS.
Nb and NbTi not listed as a material forhigh pressure vessel design
2021/09/09

Cited from: The International Linear Collider: A
Global Project, arXiv:1903.01629 [hep-ex]

7

Steps Involved in Preparing
Documentation
 Description of the SRF cavity assembly.
 Mechanical properties of the materials at room and in liquid helium temperatures.
 Mechanical properties of welded joints like Nb-Nb, Nb-Ti, Ti-Ti welds etc.

 Stress and buckling analysis of the cavity assembly using CAE software at maximum
allowable working pressure (0.2 MPa) and tuner displacement.
 Cavity fabrication information.
 Pressure test and examination reports.
 Documentation to summarize above items to be submitted to the high-pressure gas
safety authority.
2021/09/09

8

Structural Analysis

2021/09/09

9

Structural Analysis
 Structural analysis determines the integrity of structure to withstand loads.
 Structural analysis incorporates the fields of mechanics and dynamics as wellas the many failure theories.
 From a theoretical perspective, the primary goal of structural analysis is thecomputation of deformations, internal forces, and stresses.

 In practice, structural analysis reveals the structural performance of theengineering design and ensures the soundness of structural integrity indesign without dependence on direct testing.

2021/09/09

10

A. Bedford and K.M Leichti, Mechanics of materials,
second edition, Springer.

2021/09/09

https://www.mscsoftware.com/product/dytran

11

Finite Element Analysis
 FEA is a powerful computational technique for approximate solutions to a variety of“real-world” problems.
 It relies on decomposition of domain (solid, liquid or gas) into a finite number of subdomains.
 Reduces the problem into finite number of unknowns by dividing the domain intoelements and by expressing the unknown field variable in terms of the assumed
approximating functions within each element.

2021/09/09

12

Finite Element Analysis
 Discretization of the domain into finite number ofsub-domains.
 Selection of interpolating functions.
 Development of the elemental matrix of the subdomain.
 Assembly of the element matrices for each
subdomain to obtain global matrix.
 Imposition of boundary conditions.
 Solution of equations.
 Additional data-analysis if necessary.
Cited from: E Madenci and I Guven., The finite element method andapplications in engineering using ANSYS®, second edition, Springer 2015.
2021/09/09

13

Direct Approach: Linear Spring System Suitable for simpler problems but fundamental
step of a typical FEA.
 Global system of equations can be cast into:

Ku = F𝑢 = 𝑢1 − 𝑢2𝑘−𝑘𝑓1 = ku = k(𝑢1 − 𝑢2 )𝑓2 = −𝑓1

𝑓1−𝑘 𝑢1=𝑜𝑟 𝑘 𝑒 𝑢 𝑒 = 𝑓 𝑒𝑢𝑓2
2𝑘Here, 𝑢 𝑒 is the vector of nodal unknowns representing
displacement, 𝑘 𝑒 is the element (stiffness) matrix and 𝑓 𝑒 isthe element (force) vector. The stiffness matrix can be(𝑒)represented in its indicial form as 𝑘𝑖𝑗 .
2021/09/09

Cited from: E Madenci and I Guven., The finite element method andapplications in engineering using ANSYS®, second edition, Springer 2015.
14

Assembly of Global System Matrix
 Engineering problem model with finite
elements requires the assembly of element
characteristic (stiffness) matrices and element
right-hand-side vectors.

Ku = F𝐸

𝐾 = ෍𝑘 𝑒

𝐸𝐹 = ෍𝑓 𝑒

𝑒=1𝑘111𝑘21𝑒
𝐾=𝑘121𝑘221 + 𝑘112+𝑘113

0𝑘212 + 𝑘21300

𝑒=100𝑘122 + 𝑘123

0𝑘222 + 𝑘223+𝑘114
𝑘21𝑒

1𝑘12𝑒
𝑘224

𝑢1

𝑢1
123𝑢2
𝑢2 = 𝑢1 = 𝑢1
𝑢= 𝑢 =234
3𝑢2 = 𝑢2 = 𝑢1𝑢44𝑢22021/09/09

1𝑓1
𝑓1
1
2
3
𝑓2 + 𝑓1 + 𝑓1
𝑓2
𝐹=
=2
34
𝑓3
𝑓2 + 𝑓2 + 𝑓1
𝑓4
4
𝑓2
Cited from: E Madenci and I Guven., The finite element method andapplications in engineering using ANSYS®, second edition, Springer 2015.
15

Solution of Global Matrix(𝑒)(𝑒)(𝑒) For the specific values 𝑘11 = 𝑘22 = 𝑘 (𝑒) and 𝑘21 =(𝑒)𝑘12 = −𝑘 (𝑒) , the global system matrix becomes
𝐾=𝑘𝑒

1 −1 00−1 3 −2 00 −2 3 −100 −1 1

 The eigenvalues are 𝜆1 = 0, 𝜆2 = 2, 𝜆3 = 3 −5, and 𝜆3 = 3 − 5. The corresponding
eigenvectors are
11112− 52+ 5
1−1
u1 =,u 2 =,u 3 =,u 4 =1−1−2 + 5−2 − 51111

2021/09/09

Cited from: E Madenci and I Guven., The finite element method andapplications in engineering using ANSYS®, second edition, Springer 2015.
16Applying Boundary Condition
 Possible to obtain unique solution with boundary conditions.
 If 𝑢1 = 0, the nodal force 𝑓1 still remains an unknown
and the corresponding nodal forces have values of
𝑓2 = 𝑓3 = 0, and 𝑓4 = 𝐹.
−1
3−200−2
3−1

0
0−1
10
𝑓1
𝑢20
=
𝑢30
𝑢4𝐹𝑘𝑒

1−100

𝑢2 =

𝐹3 𝐹
5 𝐹,
𝑢=,
𝑢=32𝑘 𝑒 4 2𝑘 𝑒𝑘𝑒
Cited from: E Madenci and I Guven., The finite element method andapplications in engineering using ANSYS®, second edition, Springer 2015.
2021/09/0917Stress-strain Relationship in ANSYS Stress-strain relationship in ANSYS for linear materials
is defined as:{𝜎} = 𝐷{𝜀 𝑒𝑙 }{σ} = Stress vector = [𝜎𝑥 𝜎𝑦 𝜎𝑧 𝜎𝑥𝑦 𝜎𝑦𝑧 𝜎𝑥𝑧 ]𝑇[D] = Elasticity or elastic stiffness matrix or stress-strain matrix.
{𝜀 𝑒𝑙 } = 𝜀 − {𝜀 𝑡ℎ } = elastic strain vector
𝜀 = total strain vector = [𝜀𝑥 𝜀𝑦 𝜀𝑧 𝜀𝑥𝑦 𝜀𝑦𝑧 𝜀𝑥𝑧 ]𝑇{𝜀 𝑡ℎ } = thermal strain vector

Cited from: P. Kohnke, ANSYS® Mechanical APDL theoryreference, ANSYS® Inc.

 Also,𝛼𝑥𝑠𝑒 = Secant coefficient of thermal expansion in the 𝑥 direction

ε = 𝜀 𝑡ℎ + [𝐷]−1 {𝜎}, For the 3-D case, the thermal strain vector is:
𝜀 𝑡ℎ = ∆𝑇[𝛼𝑥𝑠𝑒 𝛼𝑦𝑠𝑒 𝛼𝑧𝑠𝑒 0 0 0]𝑇 ,2021/09/09∆𝑇 = 𝑇 − 𝑇𝑟𝑒𝑓
𝑇 = current temperature at the point in question

𝑇𝑟𝑒𝑓 = reference strain free temperature
18

Stress-strain Relationship in ANSYS The flexibility or compliance matrix for the linear material is:

D−1=1𝐸𝑥−𝜈𝑦𝑥𝐸𝑦−𝜈𝑧𝑥𝐸𝑧−𝜈𝑥𝑦𝐸𝑥1𝐸𝑦−𝜈𝑧𝑦𝐸𝑧−𝜈𝑥𝑧
𝐸𝑥−𝜈𝑦𝑧𝐸𝑦1
𝐸𝑧

000000000000001
𝐺𝑥𝑦000001𝐺𝑦𝑧

000001𝐺𝑥𝑧

Where the typical terms are:
𝐸𝑥 = Young’s modulus in the x direction, 𝜈𝑥𝑦 = major Poisson’s ratio
𝜈𝑦𝑥 = minor Poisson’s ratio, 𝐺𝑥𝑦 = Shear modulus in the xy plane

Cited from: P. Kohnke, ANSYS® Mechanical APDL theoryreference, ANSYS® Inc.

For isotropic materials (𝐸𝑥 = 𝐸𝑦 = 𝐸𝑧 𝑎𝑛𝑑 𝜈𝑥𝑦 = 𝜈𝑦𝑧 = 𝜈𝑥𝑧 )2021/09/09

19

1.3-GHz 3-Cell SRF Cavity
Stress Analysis

2021/09/09

20

Note The results presented here are just an example and the results presented
here are not supposed to be considered for 9-Cell SRF Cavity structure.

2021/09/09

21

SRF Cavity Assembly

2021/09/09

22

Mechanical Properties
Properties

UnitNiobium

Titanium

Young’s Modulus

GPa

103

107

Poisson’s Ratio

-0.38

0.32

Coefficient of ThermalExpansion

× 10−6 /℃

4.87

5.22

 Elastic properties of the materials will be considered for structure and buckling analysis.
 Coefficient of thermal expansion necessary to include contraction of material during
cooldown.

2021/09/09

23

Case Structure in ANSYS

Case Study

PressureTuner Displacement

Temperature

Case A

0.2 MPa

0.65 mm

40 °C

Case B

0.2 MPa

0.65 mm-271.4 °C

Case C

0.2 MPa

3 mm-271.4 °C

2021/09/09

24

Engineering Data
Niobium Properties

2021/09/09

Titanium Properties

25

Geometry CAD Model is uploaded to Geometry
 Topology is set to Share2021/09/09

26

Model – Material Assignment

 Material is assigned to each geometry.
 Stiffness behavior is set to Flexible.
2021/09/09

27

Model – Symmetry

 Model symmetry along z-axis defined.
 Faces in Red specifies the symmetry region.
2021/09/09

28

Model – Virtual Spring A virtual spring replaces Ti bellow between Ti
jacket with stiffness of 206.7 N/mm.

2021/09/09

29

Model – Meshing Model is discretized in this step.
 Meshing generated using Adaptive size control.
2021/09/09

30

Setup – Analysis Settings

 Set number of steps, sub-steps etc.
 Set Large deflection to ON, when non-linear analysis
is expected.
2021/09/09

31

Setup – Pressure Boundary Condition

 Pressure boundary condition (BC) to simulate pressurized
helium between SRF cavity and Ti jacket at 0.2 MPa.
 Surfaces in RED are provided with pressure boundarycondition.
2021/09/09

32

Setup – Displacement Boundary Condition

 Displacement BC to simulate tuner movement.

 Displacement in X-direction and movement in otheraxis are not constrained.
2021/09/09

33

Setup – Remote Displacement
Boundary Condition

 Remote Displacement BC is similar to displacement
but with more control on DOF.

 Line contact on end flanges movement is fixed in Yaxis and no rotation is allowed along any direction.
2021/09/09

34

Setup – Temperature BoundaryCondition

 Applied for Case B and C to simulate cooldown
from room temperature to -271.4 °C.

 All bodies are selected.
2021/09/09

35

Solution - Case A
 Solution -> insert -> Stress intensity -> select bodies or surface to show Stress intensity is the largest of absolute value of difference in principle stresses (σ1 - σ2, σ2 - σ3, or σ3 - σ1).

2021/09/09

36

Solution - Case B
 Solution -> insert -> Stress intensity -> select bodies or surface to show Stress intensity is the largest of absolute value of difference in principle stresses (σ1 - σ2, σ2 - σ3, or σ3 - σ1).

2021/09/0937

Solution - Case C
 Solution -> insert -> Stress intensity -> select bodies or surface to show Stress intensity is the largest of absolute value of difference in principle stresses (σ1 - σ2, σ2 - σ3, or σ3 - σ1).

2021/09/0938

Solution: Maximum Stress Intensity
Case

Nb Half Cells[MPa]

Ti Tank[MPa]

Nb-Ti weld
[MPa]

Case

A

70

512A

147

2212B

76

523B

161

2414C

300

1865C668

11167Stiffener Ring Iris Weld Equator Region
Weld [MPa][MPa]weld [MPa] For the high-pressure gas safety regulations, the mechanical properties of thematerials should be > 1.5 times the maximum stress intensity for 0.2% Y.S, and > 4times the maximum stress intensity for T.S, on individual components.
 Data is different for 9-Cell SRF cavity structure, the stress values are lower.
2021/09/09

39

Eigenvalue Buckling Analysis

2021/09/09

40

What is Buckling?
 It is a sudden change of shape of a structural component undercompressive or its own load.
 It can occur even though the stresses that develop in the structure are
well below those needed to cause failure in the material.
 Further loading may cause significant and somewhat unpredictable
deformations.
 Excess loading might or might not lead to complete loss of the structure’s
load-carrying capacity.
2021/09/09

41

Buckled Structures

https://www.structuresinsider.com/post/thedifference-between-buckling-compression-shear
2021/09/09

https://www.volpe.dot.gov/infrastructure-systems-andtechnology/structures-and-dynamics/track-buckling-research
42Buckling of a Solid Columnd = 5 mm

F = 100 N
2 𝐸𝐼𝜋Euler ′ s Critical Load, 𝑃𝑐𝑟 =𝐾𝐿 2

 Where ‘E’ is Young's modulus, ‘I’ is moment ofinertia, ‘K’ is column effective length factor.
 Stainless Steel E = 200 GPa, Ixx = b*d3/12
2021/09/09

43

Results – First Mode of buckling

PinnedFixedPcr from ANSYS = 4603.6 N

Pcr from ANSYS = 1154.9 N

Pcr from Theory = 4605.8 N

Pcr from Theory = 1151.5 N

Pinned-Pinned Column
2021/09/09

Fixed-Free Column
44Results – First Mode of buckling

FixedFixedPcr from ANSYS = 9414.8 N

Pcr from ANSYS = 18360 N

Pcr from Theory = 9423.5 N

Pcr from Theory = 18423.3 N

Fixed-Pinned Column

Fixed-fixed Column

2021/09/09

45

Modes of Pinned-Pinned Column Buckling

1st Mode

Pcr = 4603.9 N

2nd Mode

Pcr = 18387 N (~ 4 times)

3rd Mode

Pcr = 41268 N (~ 9 times)
2021/09/09

46

Eigen value Buckling Analysis
for 1.3 GHz SRF Cavity

2021/09/09

47

Eigenvalue Buckling of SRF Cavity
 Goal is to determine the pressure at which the cavity structure will buckle.
 Here only two Eigen modes will be determined.
 For this analysis, Case B is taken into consideration for buckling analysis.
 Cavity structure is easier to buckle in Case B rather than Case C due to lower
tuner displacement.

2021/09/09

48

Case Structure Same Geometry is transferred by linking.

 Model with the meshing is also linked.
 Setup is transferred, although pressure boundary condition is suppressed.
2021/09/09

49

Eigenvalue Buckling – Analysis Setting

 Nodal pressure condition is provided.
 0.2 MPa pressure acts on each nodes.

2021/09/09

50

SolutionEigen
mode

LoadMultiplier

BucklingPressure

1st385.2

77.04

2nd386.6

77.32

 Eigenvalue buckling pressure
is higher than therequirement (> 4*0.2 MPa).
 For 9-Cell SRF cavity it has
been calculated to be 33 MPa.

2021/09/09

51

Non-linear Structure Analysis

2021/09/09

52

Non-linear Buckling Analysis
 Continuation of the Eigen value buckling analysis.
 Buckled structure can be transferred for a static structure analysis.

 Possible to control the level of buckling in the structure that would betransferred with scale factor, which can be varied from 0 to > 1.
 Original structure scale factor is 0 and 1 being the buckled structure thatwould be transferred to the static structure analysis.
 Effect of structural deformities on buckling pressure can be determined.
 1st Eigen mode was transferred to four static structure analysis studies withthe scale factors being varied from 0.005, 0.01, 0.1 and 1.
2021/09/09

53

Non-linear Structure Analysis

 1st Eigen mode was transferred to four static structure
analysis studies with the scale factors varied from 0.005,0.01, 0.1 and 1.
2021/09/09

54

Setup – Boundary Condition

 Boundary conditions remains the same as in Case B, except pressure.
 Pressure (faces in Red) is increased incrementally in steps.

 Pressure increased from 0 – 80 MPa in 8 steps.
2021/09/09

55

Solution – Buckling Pressure Buckling pressure was determined by placing a total deformation probe on a point on thecavity structure where the maximum buckling occurs.
 The total deformation obtained from the deformation probe was plotted against thepressure condition for various scaling factors.
2021/09/09

56

Buckled Structures for Scale factors

Scale Factor – 0.005

Scale Factor – 0.1

Scale Factor – 0.01

Scale Factor – 1

2021/09/09

57

Results and Discussions
 Buckling pressure was 74 MPa for scale factor of0.005, similar to Eigenvalue buckling analysis.
 Buckling pressure reduces to 54 MPa for thescale factor of 1.
 For elastic material properties, the 3-Cell cavity
will not buckle upto 54 MPa pressure.

 Buckling pressure usually should be > 4 times theMAWP, and in this case the cavity structure has
sufficient strength to qualify for that criterion.

2021/09/09

58

Thank you for your attention!

2021/09/09

59