The post ASME PTB-3 Validation – Fatigue Analysis appeared first on Flexible Shell Elements FEA Software.

]]>Here an ASME PTB-3 Validation for “Example E5.5.3 – Elastic Stress Analysis, and Equivalent Stresses” to check for protection against failure from cyclic loadings per ASME Sec VIII Div 2 is carried out using ANSYS.

Problem Statement:

Evaluate the vessel top head and shell base metal regions given in Example E5.2.1 in accordance with the fatigue methodology provided in paragraph 5.5.3. Note that the nozzle to head weld is machined and subjected to full volumetric examination and both ID and OD surfaces receive MT/PT and VT. The shell to head weld is in the as-welded condition and the OD surface receive the same inspection as above. The ID surface receives only full volumetric examination. The cyclic loading design requirements given in the Users’ Design Specification are provided below:

Operating pressure = 380 psig at 125^{o}F

Corrosion Allowance = 0.125 inches

Cyclic Life Requirement = 20000 full pressure cycles

Number of Shutdowns/Startups = 20

Solution:

Typically before performing a detailed fatigue analysis the equipment is checked to see if it meets fatigue screening criteria per sec 5.5.2. Three methods for fatigue screening criteria are provided in the code. We’ll see each one of them.

Fatigue Analysis Screening Based on Experience With Comparable Equipment.

We’ll assume no such data is available and move to next method.

Fatigue Analysis Screening, Method A.

- The expected (design) number of full-range pressure cycles including startup and shutdown, N
_{ΔFP }= 20000 + 20 = 20020 cycles - Operating pressure cycles (cycles for which range of pressure variation exceeds 20% of the design pressure for integral construction), N
_{ΔPO }= 0 cycles - The effective number of changes in metal temperature difference between any two adjacent points, N
_{ΔTE}= 0 cycles - The number of temperature cycles for components involving welds between materials having different coefficients of thermal expansion that causes the value of thermal strain to exceed 0.00034, N
_{ΔTα}= 0 cycles - Sum total of above calculated cycles N
_{ΔFP}+ N_{ΔPO}+ N_{ΔTE}+ N_{ΔTα}= 20020 which is greater than 1000 (Refer Table 5.9). Hence, Screening Method A is not met. So we proceed to Method B.

Fatigue Analysis Screening, Method B.

- For integral construction with no nozzles or attachments in the knuckle region criteria factors C
_{1}= 3 and C_{2}= 2 (Table 5.10) - N
_{ΔFP }= 20020 cycles as in Method A.

The allowable number of cycles can be obtained as N(C_{1}S) = 10^{X} (3-F.21) where X is obtained from Annex 3-F. A summary is shown in the above table.

Since N_{ΔFP }> N(C_{1}S) for both components, fatigue evaluation for both are required.

Fatigue Evaluation – Elastic Stress Analysis, and Equivalent Stresses

Finite Element Model from Example E5.2.1 is used in this analysis. The only cyclic load here is the pressure load which varies from 0 to 380 psi. Typically to find alternating stress amplitude one needs to solve two load cases:

Case 1: The maximum cyclic load (in our case pressure of 380 psi)

Case 2: The minimum cyclic load (in our case pressure of 0 psi)

Finally stress range is obtained as Case 3 = Case 1 – Case 2.

However for a linear elastic analysis like the one which we would be doing, the response (deformations, stresses) will be directly proportional to the applied loads. Hence Case 3 can be directly obtained by applying ΔP load = P_{max} – P_{min} = 380 – 0 = 380 psi in a single load case. Note, this approach would work even if we had a non zero P_{min}.

ANALYSIS SUMMARY

LOADS & BOUNDARY CONDITIONS

- Internal Pressure of ΔP = 380 psi was applied on the inner surfaces of the model.

- Pressure Thrust of 888.75 psi was applied on the flange face as negative pressure.

- Axial displacement was arrested at the shell base.

ANALYSIS RESULTS

Total Deformation Plot

Von-Mises Stress

Von-Mises Stress from PTB-3 example

SCL Locations

SCL Locations from ASME PTB-3 example

Membrane + Bending stress @ SCLs (The red values are from this analysis, the black values are from ASME PTB-3)

Allowable Primary + Secondary stress, S_{PS} is calculated as max(3S, 2S_{y}) as shown in the table below.

Since Membrane + Bending Stresses are less than S_{PS}, fatigue penalty factor K_{e} = 1

Computation of alternating stresses @ SCLs

S_{alt} = K_{f}*K_{e}*Total Von-Mises Stress Range/2

Here K_{f}, the fatigue strength reduction factor is taken from Tables 5.11 and 5.12.

The below table summarizes the results (values in red are from this analysis and those in black are from ASME PTB-3.

Finally allowable number of cycles, need to be calculated for S_{alt} using Annex 3-F. Calculation for allowable number of cycles are not being done for this analysis, however reference table from ASME PTB-3 is produced below.

Knowing the allowable number of cycles N and the design cycle life of the component n fatigue damage factor can be calculated as D = n/N. In case multiple cyclic loads are present, the miner’s rule D = n_{1}/N_{1} + n_{2}/N_{2} … can be used.

This results in calculated fatigue damage for the limiting region (nozzle outside radius) of 0.073 (from ASME PTB-3). Similarly, a fatigue damage of 0.039 (from ASME PTB-3) is calculated for the head knuckle.

Since D<1, the equipment is safe w.r.t fatigue damage.

The post ASME PTB-3 Validation – Fatigue Analysis appeared first on Flexible Shell Elements FEA Software.

]]>The post ASME PTB-3 Validation – Buckling Analysis appeared first on Flexible Shell Elements FEA Software.

]]>Here an ASME PTB-3 Validation for “Example E5.4 – Protection Against Collapse from Buckling” is carried out per ASME Sec VIII Div 2 using ANSYS.

Problem Statement:

Evaluate the following tower for compliance with respect to the Type-1 buckling criteria provided in paragraph 5.4.1.2.

Material – Shell and Heads = SA-516, Grade 70, Normalized

Design Conditions = -14.7 psig at 300^{o}F

Corrosion Allowance = 0.125 inches

ANALYSIS SUMMARY

- A mid surface shell model was constructed using corroded dimensions from the above figure.
- The model was meshed with higher order shell elements.

- Fixed Support was applied to the base of the skirt.
- External Pressure = 14.7 psi was applied as perturbation load for the static structural analysis.

- The pre-stressed model from static structural analysis was used for eigenvalue buckling analysis. 3 buckling modes were requested using analysis setup and the numerical model was solved.
- Following Eigenvalues were found from the buckling analysis

Mode | Eigenvalues |

1 | 9.0009 |

2 | 9.0016 |

3 | 15.288 |

ASME PTB-3 Eigenvalues

Mode | Eigenvalues |

1 | 7.939 |

2 | 7.940 |

3 | 14.351 |

Note the ASME PTB-3 analysis is carried out using abaqus which calculates Buckling Load as Eigenvalue + Eigenvalue*Perturbation Load. But in ANSYS Buckling Load is calculated as Eigenvalue*Perturbation Load. Hence there is a difference of about 1 between the two eigenvalues.

First Mode Shape Plot

ASME PTB-3 First Mode Shape

The plots are quite similar. Note that values of deformations have no physical meaning for buckling analysis

CRITICAL BUCKLING LOAD EVALUATION

For Type 1 buckling analysis (Elastic Stress Analysis with small deformation theory) performed here ASME SEC VIII Div 2 gives a minimum design factor of \(\Phi_B=\frac{2}{\beta_{cr}}\).

For unstiffened cylinders under external pressure \(\beta_{cr} = 0.80 \) from eq 5.14.

Therefore \(\Phi_B=\frac{2}{\beta_{cr}}=\frac{2}{0.80}=2.5\)

Critical Buckling Load (Mode 1)

= Perturbation Load * Eigenvalue/Design Factor

= 14.7*9.0009/2.5

= 52.9 psi

Critical Buckling Load (Mode 1 ASME PTB-3)

= (Perturbation Load +Perturbation Load* Eigenvalue)/Design Factor

= (14.7 + 14.7*7.939)/2.5

= 52.6 psi

The values compare fairly well.

Since external pressure = 14.7 psi < buckling pressure = 52.9 psi the structure is safe w.r.t buckling under the design conditions.

The post ASME PTB-3 Validation – Buckling Analysis appeared first on Flexible Shell Elements FEA Software.

]]>The post ASME PTB-3 Validation – Protection Against Local Failure appeared first on Flexible Shell Elements FEA Software.

]]>ELASTIC ANALYSIS

Here an ASME PTB-3 Validation for “Example E5.3.2 – Elastic Analysis” to check for protection against local failure per ASME Sec VIII Div 2 is carried out using ANSYS.

The same problem which was analyzed in the post – ASME PTB-3 Validation – Elastic Stress Analysis for protection against plastic collapse will be used to check protection against local failure.

TRIAXIAL STRESS

The sum of principal stresses called as the triaxial stress can be found in ANSYS using the expression = S1 + S2 + S3 in a “user defined result”.

From plots its evident that Max(Triaxial Stress) = 72575 psi < 4S = 93200 psi. Hence the components satisfy elastic local failure check criteria and further stress linearization need not be performed. It shall be noted that local failure check is required only for linearized primary stresses for the load case – “Design Pressure + Static Head + Dead Loads” per sec 5.3.2.

ASME PTB-3 TRIAXIAL STRESS

The results compare very well with those provided in ASME PTB-3.

ELASTIC PLASTIC ANALYSIS

To check the above problem using elastic plastic methodology an analysis analogous to that performed in the post ASME PTB-3 Validation – Elastic Plastic Analysis is done but using a load factor of 1.7 instead of 2.4 used for checking protection against plastic collapse. Load factor is selected for local criteria from table 5.5.

Loads used in the model:

Internal Pressure = 1.7P = 714 psi

Pressure Thrust = 1.7 * Pressure Thrust in the Elastic Analysis = – 1669.9 psi

RESULTS

Computation of limiting triaxial strain was done using eq 5.6. The strain limit parameters were calculated from table 5.7 for both materials SA 105 and SA 516 Gr 70. Sample strain limit parameters for SA 516 Gr 70 are:

User Defined Results were used to plot the limiting triaxial strain using eq 5.6

NOTE: Strains above those at ultimate stress are shown in pink.

ASME PTB-3 Triaxial Strain Limit

Equivalent Plastic Strain

ASME PTB-3 Equivalent Plastic Strain

Strain Ratio

There was no forming strain in the components hence the equivalent plastic strain needs to be checked against the limiting triaxial strain. This can be done by computing and plotting strain ratio of the equivalent plastic strain and the limiting triaxial strain.

ASME PTB-3 Strain Ratio

Since the strain ratio < 1, protection against local failure check is satisfied. It shall be noted that though the strain ratio reported by ASME PTB-3 is 2% against 3% obtained from this analysis, we are still talking about very small values, hence the difference looks to be OK. Also the difference might have been due to a more accurate stress strain curve considered in this analysis (75 points) against a crude curve considered by ASME PTB-3 (20 points).

Find PTB-3 Validation for plastic collapse check using Elastic Stress Analysis here

Find PTB-3 Validation for plastic collapse check using Limit Load Analysis here

Find PTB-3 Validation for plastic collapse check using Elastic Plastic Analysis here

The post ASME PTB-3 Validation – Protection Against Local Failure appeared first on Flexible Shell Elements FEA Software.

]]>The post ASME PTB-3 Validation – Elastic Plastic Analysis appeared first on Flexible Shell Elements FEA Software.

]]>- The material model is non-linear and requires true stress strain curve as input. In contrast a linear static analysis just needs Elastic Young’s Modulus to construct the full stress strain curve. The stress-strain curve in this case is simply a line starting from origin with slope equal to the Elastic Young’s Modulus.
- Geometric non-linearity is also considered in an elastic plastic analysis by switching on large deformation effects. This allows the model to incorporate change in structures stiffness with large deformations. To understand this, consider a cantilever loaded at its end. Initially the cantilever will bend relatively easily and deformations will be proportional to the load (δ=PL
^{3}/3EI). However, it becomes more stiff (hard to bend) as deformations become large and the load vs deformation response is no longer linear. These sort of stress stiffening effects are captured by switching on large deformation effects. - The third type of non-linearity which is contact may or may not be present in the model.

Here an ASME PTB-3 Validation for “Example E5.2.3 – Elastic Plastic Analysis” to check for protection against plastic collapse per ASME Sec VIII Div 2 is carried out using ANSYS.

Problem Statement:

Evaluate the vessel top head and shell region given in Example Problem E5.2.1 for compliance with respect to the elastic-plastic analysis criteria for plastic collapse provided in paragraph 5.2.4.

For Vessel Data, Geometry, Mesh Details refer the post – ASME PTB-3 Validation – Elastic Stress Analysis

ANALYSIS SETUP

A static structural analysis was carried out with large deformation effects switched on to capture geometric non-linearities in the model.

MATERIAL PROPERTIES

An elastic plastic material model was set-up by defining true stress strain curves for the given materials using Annex 3-D of ASME Sec VIII Div 2. A multilinear isotropic hardening plasticity material model was used for this analysis. Here multilinear means the program will join the user input stress strain points on the curve with straight lines to complete the continuous curve. Isotropic Hardening means the strain hardening in the model is assumed to be same for both tension and compression. This model holds good for large strain applications such as the ones dealt with for plastic collapse analysis.

The curve is generated by defining Elastic Young’s Modulus for the linear portion of the curve (upto proportional limit). For the non-linear portion (the curve beyond proportional limit) stress vs plastic strain needs to be defined upto the ultimate stress. Beyond this point the curve is assumed to be perfectly plastic, indicating rupture failure.

Stress Strain Curve for SA 105

NOTE: Typically FEA softwares require stress vs plastic strain as input to generate this sort of curve with the plastic strain starting at zero. Here the plastic strain starts at 0.00002 which is small enough to be taken as zero.

Stress Strain Curve for SA 516 Gr 70

NOTE: Typically FEA softwares require stress vs plastic strain as input to generate this sort of curve with the plastic strain starting at zero. Here the plastic strain starts at 0.00002 which is small enough to be taken as zero.

LOADS & BOUNDARY CONDITIONS

- Factored Internal Pressure of 2.4P = 1008 psi was applied on the inner surfaces of the model as per table 5.4, ASME Sec VIII Div 2.

- Pressure Thrust of 2357.5 psi was applied on the flange face as negative pressure.

- Axial displacement was arrested at the shell base

ANALYSIS RESULTS

The analysis converged for the given load and thereby satisfy the global acceptance criteria for elastic plastic analysis as per para 5.2.4.3 of ASME Sec VIII Div 2. No service criteria was provided in this problem hence they are not checked here.

Von-Mises Stress

Von-Mises Stress from PTB-3 example

Equivalent Plastic Strain

Equivalent Plastic Strain from PTB-3 example

The results obtained shows a very good match with PTB-3 values.

Find PTB-3 Validation Elastic Stress Analysis here

Find PTB-3 Validation Limit Load Analysis here

The post ASME PTB-3 Validation – Elastic Plastic Analysis appeared first on Flexible Shell Elements FEA Software.

]]>The post ASME PTB-3 Validation – Limit Load Analysis appeared first on Flexible Shell Elements FEA Software.

]]>Here an ASME PTB-3 Validation for “Example E5.2.2 – Limit Load Analysis” to check for protection against plastic collapse is carried out using ANSYS.

Problem Statement:

Evaluate the vessel top head and shell region for the vessel for compliance with respect to the limit load analysis criteria for plastic collapse provided in paragraph 5.2.3 of ASME Sec VIII Div 2.

For Vessel Data, Geometry, Mesh Details refer the post – ASME PTB-3 Validation – Elastic Stress Analysis

ANALYSIS SETUP

A static structural analysis was carried out with large deformation effects switched off as limit load analysis is done with the assumption that the strain-displacement relations are those of small displacement theory (Refer para 5.2.3.1(c)(2) of ASME Sec VIII Div 2)

MATERIAL PROPERTIES

- An elastic-perfectly plastic material model was used for the analysis. This can be done by selecting bi-linear isotropic hardening model and entering the tangent modulus as zero. Note that since strain hardening is not being considered here both isotropic and kinematic hardening models are fine.
- Yield strength defining the plastic limit shall equal 1.5S as per para 5.2.3.5 step 3 of ASME Sec VIII Div 2.

Yield Strength for SA-105 = 34950 psi

Yield Strength for SA-516-70N = 36825 psi

Young’s Modulus was taken from table TM-1, ASME II D at design temperature while poisson’s ratio was taken from table PRD, ASME II D. Yield Stress was computed as 1.5S, where S was taken from table 1A, ASME II D.

Stress Strain Curve for SA-105

Stress Strain Curve for SA-516-70N

LOADS & BOUNDARY CONDITIONS

- Factored Internal Pressure of 1.5P = 630 psi was applied on the inner surfaces of the model as per table 5.4, ASME Sec VIII Div 2.

- Pressure Thrust of 1473.45 psi was applied on the flange face as negative pressure.

- Axial displacement was arrested at the shell base

ANALYSIS RESULTS

The analysis converged for the given load and thereby satisfy the global acceptance criteria for limit load analysis as per para 5.2.3.4 of ASME Sec VIII Div 2. No service criteria was provided in this problem hence they are not checked here.

Von-Mises Stress

Von-Mises Stress from PTB-3 example

The result plot compares pretty well with those provided in PTB-3 (ASME Sec VIII Div 2 – Example Problem Manual)

Note that deformations and strains computed in a limit load analysis have no physical meaning and are therefore not been plotted here.

Though convergence is achieved its always a good idea to find the actual limiting load for which plastic collapse occurs. This kind of gives a feel of additional margin above the applied factored load. This can be done by taking a large factor on the load say 10P and subsequently checking the load step upto which convergence is achieved. Say convergence upto a max time of 0.7 will imply 0.7*10P is the limit load.

A load (Internal Pressure in this example) vs max deformation is plotted here to get an idea of the limit load.

Load vs Deformation curve from PTB-3 example

Again the plots compare fairly well and gives an estimate of the limit collapse pressure load of 818 psi vs applied factored pressure load of 630 psi.

Find PTB-3 Validation Elastic Stress Analysis here

Find PTB-3 Validation Elastic Plastic Analysis here

The post ASME PTB-3 Validation – Limit Load Analysis appeared first on Flexible Shell Elements FEA Software.

]]>The post ASME PTB-3 Validation – Elastic Stress Analysis appeared first on Flexible Shell Elements FEA Software.

]]>Problem Statement:

Evaluate the vessel top head and shell region for compliance with respect to the elastic stress

analysis criteria for plastic collapse provided in paragraph 5.2.2. Do not include the standard flanges

or NPS 6 piping in the assessment for compliance to allowable stresses. Internal pressure is the only

load that is to be considered. Relevant design data and geometry are provided below and in Figures

E5.2.1-1 and E5.2.1-2.

Vessel Data

Material – Shell and Heads = SA-516, Grade 70, Normalized

Material – Forgings = SA-105

Design Conditions = 420 psig at 125oF

Corrosion Allowance = 0.125 inches

PWHT = Yes

ANALYSIS STEPS:

An axi-symmetric geometry model was constructed with shell (length > \(5\sqrt{Rt}\)), nozzle and attached weld neck flange using corroded dimensions as shown in sketch below.

MATERIAL PROPERTIES

A small deformation, linear elastic, static structural analysis was carried out using the following material properties.

Young’s Modulus was taken from table TM-1, ASME II D at design temperature while poisson’s ratio was taken from table PRD, ASME II D.

MESH

A fine 2nd order quad dominant mesh was used for analysis purpose with global element sizing set to 0.15 in to get adequate number of elements across thicknesses required for stress linearization. From my experience 3 elements across thickness generally gives acceptable converged linearized results.

MESH @ Nozzle Shell Junction

MESH @ Head Shell Junction

LOADS & BOUNDARY CONDITIONS

- Internal Pressure of 420 psi was applied on the inner surfaces of the model

- Pressure Thrust of 982.3 psi was applied on the flange face as negative pressure

- Axial displacement was arrested at the shell base

ANALYSIS RESULTS

Total Deformation Plot

Note that PTB-3 does not provide a deformation plot for comparision.

Von-Mises Stress

Von-Mises Stress from PTB-3 example

The result plot compares pretty well with those provided in PTB-3 (ASME Sec VIII Div 2 – Example Problem Manual)

SCL Locations

Stress Classification lines were taken at deemed critical locations similar to those given by PTB-3.

STRESS ANALYSIS SUMMARY

Stresses were evaluated at the SCL Locations and were compared against allowables. The below table is reproduced from PTB-3 in which comparitive results from this analysis have been put in orange.

The analysis results are generally within 5% of PTB-3 values. The cases with slightly more error are those of relatively smaller stress, therefore actual difference between the reported stresses for these cases are generally of the order of few MPa. Also it shall be noted that the stress linearization carried out by ansys is not compliant with ASME Sec VIII Div 2 procedure. For more on this read here.

Find PTB-3 Validation Limit Load Analysis here

Find PTB-3 Validation Elastic Plastic Analysis here

The post ASME PTB-3 Validation – Elastic Stress Analysis appeared first on Flexible Shell Elements FEA Software.

]]>The post Shell Elements for Pressure Vessel Design appeared first on Flexible Shell Elements FEA Software.

]]>However though shell models are computationally efficient, their results are not as robust as solid elements and involves additional complexities in model setup. Some key points to consider while setting up a shell model are:

- For shells with R/t < 10 i.e. for thick shells, solid models shall be usually preferred as they give more realistic results.
- The shell normals shall be carefully oriented so that pressure loads get applied on the correct side.
- If a mid-surface model is used, the surfaces should be extended at junctions as required to achieve a shell to shell connection even if it results in an overlap of thicknesses.
- Fillet welds at a T-Junction or a similar junction can be modelled as shell elements with a thickness equal to the weld throat. The weld leg locations on the mid-surface model can be found by projecting normals from actual weld leg locations on to the mid-surfaces. The above two points are nicely illustrated in the following figure from ASME Sec VIII Div 2.

- While stress linearization requires identifying critical junctions and creating paths (Stress Classification Lines) in the solid model at these junctions, finding membrane and membrane + bending stresses in a shell model is a trivial process. The middle surface stress at any stress evaluation point (typically weld toes are critical points as shown in the above figure) gives the membrane stress, while the stress at the Top/Bottom surface gives the membrane + bending stress.
- To model a lap weld simply draw a shell from edge of the top plate to point of intersection of the normal through the weld toe to the mid-surface of the bottom plate as shown by orange lines in the figure below.

- Two parallel shell plates like that shown in the above lap joint arrangement if required to be modelled as integral can be joined using bonded contacts between the offset modelled mid-surfaces

These were some pointers to be considered while going for a shell model. Please let me know through comments any other important pointers which I might have missed.

The post Shell Elements for Pressure Vessel Design appeared first on Flexible Shell Elements FEA Software.

]]>The post Flanged and Flued Expansion Joint appeared first on Flexible Shell Elements FEA Software.

]]>Sample this – For a typical heat exchanger there will be 8 load cases (4 design, 4 operating) for each of startup, shut-down, operation, upset conditions etc. Also the analysis needs to be carried out for corroded and uncorroded models for minimum as well as nominal thickness of the expansion joint. For all these conditions TEMA recommends to check for stresses across 10 to 15 SCLs (stress classification lines) as shown below.

8 load cases * 4 design conditions *4 models (nominal uncorroded, minimum corroded etc) * 13 SCLs say = 1664, which means evaluating and checking stresses against allowable for a phenomenal 1664 cases.

Sometimes users wonder that carrying out analysis in the minimum corroded condition shall be conservative. This however may not be true always. A thinner expansion joint leads to higher pressure stress in the longitudinal (PD/4t) and hoop direction (PD/2t), however at the same time thinner joints are more flexible (smaller spring rate) and thus allow displacement loads much easily with lower axial stress. Hence design of expansion joints are always an optimization problem between strength and flexibility and the thickness for these joints shall not be too high than required to sustain pressure loads.

The FSE software comes in handy in analyzing all the requisite cases fairly quickly and without much FEA know-how for the user. I have made it publicly available for free for both educational as well commercial use.

The post Flanged and Flued Expansion Joint appeared first on Flexible Shell Elements FEA Software.

]]>The post Curtain Rod – A Simply Supported Beam appeared first on Flexible Shell Elements FEA Software.

]]>Here is a picture of the initially straight curtain rod without curtains.

And here is a picture of the bent curtain rod when curtains were hung from it.

I analyzed this scenario as a linear, elastic, small deformation simply supported beam problem with uniformly distributed loads on it to check whether the maximum deformation (sagging) of the beam (curtain rod) at its center matches with theoretical calculations.

Though the problem appears to be a pretty straight forward one, the challenge was to measure or estimate physical quantities (dimensions, weight, material properties) with reasonable accuracy to validate the actual results theoretically.

1st I measured the dimensions. The span length of the beam was easy to measure using an inch tape. It turned out to be \(L=2884\) mm.

Next I needed the cross-section dimensions with reasonable accuracy (something like \(\frac{1}{10}\)th of an mm). Additionally the OD of the rod was corrugated which prompted me to find out the mean OD to simplify the analysis. Here’s a picture of the cross-section (The ends are slightly worn out here, but still you’ll get the idea.)

To measure the OD I rolled up three rounds of thread on the outer surface of the rod, unrolled it, measured its length and divided by \(3\pi\). Next using a scale I visually estimated the height of the corrugations to be around 0.8 mm. Using the measured outside OD and approximate height of corrugations I calculated the mean OD of the rod which turned out to be \(OD_{mean}=238/3\pi-0.8=24.45\) mm.

Here’s a picture showing thread rolled over the rod.

To estimate the ID, I inserted a sheet of rolled paper inside the hole of the rod to match its ID. Then repeated a similar procedure, this time rolling thread over the paper to estimate the ID as \(ID=211/3\pi=22.39\) mm.

Here’s a picture of the thread rolled over the paper inserted inside the curtain rod hole.

The curtain rod was made of Aluminium with a brown paint over it. Young’s Modulus assumed for the Aluminium rod was \(E=69\) GPA.

Next I set out to compute the uniformly distributed load on the curtain rod with the hanging curtains. To accomplish this I weighed the curtains on a weighing machine and figured out its weight as \(wt_{curtains}=3\) kg.

Here’s a picture showing the curtain weight.

Next I estimated the weight of the Aluminium rod as its volume*density.

\(wt_{Al}=\frac{\pi}{4}*(24.45^2-22.39^2)*2884*(2700*10^{-9})=0.59\) kg.

Knowing the weights I calculated the udl intensity as

\(w=\frac{wt_{curtains}+wt_{Al}}{L}=\frac{3.59}{2884}=0.001245\) kg/mm \(=0.0122\) N/mm

Next I calculated the moment of inertia for the cross-section before moving to the last part of this analysis.

\(I=\frac{\pi(OD_{mean}^4-ID^4)}{64}=5206\) \(mm^4\)

Now the final part. For the sake of brevity, I wouldn’t do a derivation here, but the maximum central deformation for a simply supported beam with a uniformly distributed load is given by \(\delta=\frac{5wL^4}{384EI}=\frac{5*0.0122*2884^4}{384*69*1000*5206}=30.6\) mm. When I measured the central deformation of the rod it came out to be 31 mm (I used the shadow of rod on the wall before and after hanging the curtains to measure this). That the result got validated with such high accuracy in spite of the rough method used in the analysis actually amused me as might have amused you.

The post Curtain Rod – A Simply Supported Beam appeared first on Flexible Shell Elements FEA Software.

]]>The post Stress Linearization – ASME Sec VIII Div 2 appeared first on Flexible Shell Elements FEA Software.

]]>**Example Problem**: A carbon steel vessel (ID 500 mm x 20 thk x 1000 mm long) has a nozzle connection (ID 250 mm x 20 thk x 130 mm projection) of the same material. The ends of the vessel are fixed and a shear load of 1000 kN is applied at the nozzle to shell junction along the vessel axis. Using FEA the linearized Von-Mises Membrane and Membrane + Bending Stresses in the vessel needs to be evaluated near the location of maximum stress.

The problem analysis is conducted using ANSYS.

**ANSYS Analysis Plots**

The Finite Element Model

Boundary Conditions and Loads (Note: Both ends including the end not visible in the plot are fixed)

Von-Mises Stress in the vessel

Coordinate system to define the path for the Stress Classification Line (SCL). A local coordinate system is created (using create coordinate system aligned with hit point normal method in ANSYS) near the max Von-Mises Stress location, so that its X-Y-Z axes represent tangential (radial), hoop and normal (meridional) directions respectively.

SCL Path (Near the Location of Max Von-Mises Stress)

**Stress Linearization Procedure:**

The hoop, normal (meridional) and tangential (radial), direct along with corresponding shear stress components were recorded across 5 equidistant points along the SCL path.

Subscript Meanings: h – hoop, n – normal, t – tangential, hn – hoop normal, nt – normal tangential, th – tangential hoop

Thickness across SCL Path, t = 20 mm

Distance between points, Δx = t/4 = 5 mm

**Calculation of Membrane Stress Tensor**

The membrane stress tensor is the tensor comprised of the average of each stress component along the stress classification line.

Membrane Hoop Stress

Subscripts: hm – hoop membrane, hnm – hoop normal membrane etc

**Calculation of Bending Stress Tensor**

(a) Bending stresses are calculated only for the local hoop and meridional (normal) component stresses, and not for the local component stress parallel to the SCL or in-plane shear stress.

(b) The linear portion of shear stress needs to be considered only for shear stress distributions that result in torsion of the SCL (out-of-plane shear stress in the normal-hoop plane).

(c) The bending stress tensor is comprised of the linear varying portion of each stress component along the stress classification line

Bending Hoop Stress

Subscripts: hb – hoop bending, hnb – hoop normal bending etc

Note that bending for other components are not calculated (see points (a) and (b)) as required by ASME Sec VIII Div 2, Annex 5-A para 5-A.4.1.2. The default linearization routine of ANSYS or other FEA softwares will calculate bending for all components hence do not comply with Annex 5-A requirement. However some softwares eg. Abaqus allow users to select which stress components to include in the linearization routine, thus giving the user the flexibility to comply with the Annex 5-A requirements.

**Calculation of Membrane + Bending Stress Tensor**

x = 0 represents 1st point on the SCL

x = t represents the other end point on the SCL

Subscripts: hmb0 – hoop membrane + bending at x = 0, hnmbt – hoop normal membrane + bending at x = t etc

**Calculation of Linearized Von-Mises Membrane and Membrane + Bending Stress**

Subscripts: eqvm – Equivalent Membrane Stress or Von-Mises Membrane Stress, eqvmb0 – Equivalent Membrane + Bending Stress at x=0, eqvmbt – Equivalent Membrane + Bending Stress at x=t

Reference: Composite Simpson’s Rule

The post Stress Linearization – ASME Sec VIII Div 2 appeared first on Flexible Shell Elements FEA Software.

]]>