FEA Methods (Blog)

The Nuts and Bolts of Stress Linearization

Linearization separates FEA stresses into membrane and bending. Examples are provided along with sample data and a spreadsheet based stress linearization tool. PRINT EXPAND SHRINK LINK

The Nuts and Bolts of Stress Linearization

File: 1844, Last Updated: March 2012, LB

Why classify stresses?

The ASME pressure vessel code is based on the observed safety of vessels. It is a real world working standard – its roots were born of failed vessels and dead operators in an era long before concepts like stress concentrations were even known. At its birth theory ran out when items got more complex than cylinders and spheres.

When rules were required for items like flanged and dished heads, models and full sized vessels were made and tested. The observations were turned into design rules. Vessels became safer through their efforts – but why did they work?

Later generations of vessel engineers developed magical tools like finite element analysis that allowed them to see stresses inside vessel components. They had to learn why we got away with weird rules like area replacement on nozzles. Different types of stresses were found to have different safety implications. Also, the location of the stress was very important.

They observed that a bending stress is less dangerous than a membrane stress – it is allowed to be 1.5x higher in VIII-1. Local stresses around nozzles or transitions could be higher than global stresses – sometimes 2x as high, depending on the location and cause. They wrote the VIII-2 rules and developed the stress linearization method.

More decades have passed. Finite element analysis is no longer a magical tool hiding in research labs. Many engineers and technologists now have access to it. But analyzing the stresses found in a pressure vessel is still a difficult task. Running a finite element model and looking for the highest stresses is not adequate.

This article is a guide to how the stress linearization tool works to separate stresses into membrane and bending. Examples are provided along with sample data and a spreadsheet based stress linearization tool. The programming code is explained in the appendixes and can be examined in the spreadsheet.

This article does not discuss whether the stresses are local or global and which allowable stresses should be used for where. This is a topic for a later article.

The Stress Classification Line

A Stress Classification Line or SCL is a straight line running from the inside to outside of a vessel. It is perpendicular to both the inside and outside surfaces. Finite Element Analysis provides the raw stress data at nodes along this line. The stress linearization tool takes the nodal data for the complex stress pattern found along this line and breaks it down into components:

Membrane – or average stress – always positive. You can not tell from stress classification whether the average stress is compressive or tension. This is the same problem as looking at Tresca or von-Mises plots. Magnitudes are provided but directions are missing. The membrane stress is usually equal to the code allowable stress for global areas and 1.5 as much for local areas.

Bending – is the difference in stress from inside to outside – always positive (a better definition follows).

Membrane + Bending – sum of the above two numbers – The ASME code allows the membrane + bending stress to be higher than the membrane only. In some local locations, the membrane + bending stress can be higher than the yield point for the material.

Peak – or highest stress found along the line. This is also always positive but not necessarily higher than the membrane + bending number. Peak stress is usually used to determine the fatigue life at the SCL.

ASME VIII-2 chart Figure 5.1 provides a guide to what the maximum allowed stresses are allowed for different locations. The combination of this chart and the output from the stress classification tool can be used to produce pass fail judgments on the component under study.

Warning – Figure 5.1 provides pass/fail criteria on vessel design, however thought is still required! Have the critical areas of the vessel been studied? Is the failure mechanism understood – some mechanisms such as snap through or external pressure buckling will not be detected by this analysis tool.

Example – Stress Classification at Work

This spherical head has a heavy nozzle full penetration welded into its crown. To know if the design is adequate, the membrane and membrane + bending stresses are required. A 5° slice of the model will represent the whole head. The slice has a split line near the weld to ensure that when meshed, the nodes at this location line up straight – the Stress Classification Line.

The utility determined the membrane, bending, membrane + bending and peak stresses along the SCL. The membrane and membrane + bending stresses have been compared with the code allowed limits. The complex stresses found in the finite model have been reduced to pass/fail criteria.

It can also be seen that the stress classification line did not pass through the area of highest stresses – the user repeated the analysis through a higher stress area – see the following page.

Some Stress Linearization utilities can interpolate data through areas where no nodes are found – no split lines are required. Where to put the split lines and how to interpret the results are not in the scope of this report – this report is concerned with how the stress linearization utility works.

FEA Report showing Stress Linearization

SCL through a location near the root of a weld fillet. Here the stresses are mostly uniform from inside to outside surface, which the SCL interprets as mostly membrane.

NutsBoltsStress_Image2

SCL through a weld and into the highest stress area of a nozzle. The SCL interprets the difference in stress from inside to outside as bending. Here the stresses are excesive.

How does Stress Linearization work?

What is happening under the hood when your stress linearization utility presents results? (Per ASME VIII-2 5.A.4 or “Stress Integration Method”) A spreadsheet stress linearization utility is attached that allows you to try this for your self.

Step 0 – Prepare the Model

The model might not provide nodes at the location where they are required. They might not exist, or the nodes might not line up in a straight line. In this case, the user splits the model to provide a line where a row of nodes stretching from the inside to the outside of the model.

The required location of the line might not be known until the model is run. Multiple lines might be required (Some programs provide tools to extract data where there are no nodes and without splitting models).

Caution – splitting a model to create stress classification locations can increase the number of surfaces with force loads. The forces that might be correct before the split can now be too large. Don’t forget to re-check your reaction force balances after spitting a model!

Step 1 – Import Data From a Finite Analysis Run

The FEA program exports results for each node in the model. When using high order elements, intermediated nodes are also generated. The required data is:

  • The location of the node – (x, y, z) in the models global coordinate system
  • The 6 stresses at each node – (Sx, Sy, Sz and shear Txy, Txz, Tyz).

The FEA program solves for the above stresses, but usually translates the results into vonMises or Tresca results which are more commonly viewed.

The utility included with this report is written to import data from Cosomos Designer. The code can be viewed by pressing Alt+F11 in Excel. It is up to the user to translate it to read other FEA outputs.

Step 2 – Order the Data

The data will probably be imported in nodal order. The program needs to arrange the nodes on the SCL from inside to outside. The stress linearization tool will determine the ends of the line, and sort the nodes between them.

The program finds the maximum and minimum x, y and z coordinates and decides which end will be the start (end i or inside) and which the finish (end j or outside). Usually the node closest to (0,0,0) is the start end (or end i). The distance from i to j is the length of the stress classification line or t. Half way between i and j is the center of the line.

Caution – the program might not order the data in the direction that you were expecting. If you are looking at graphical results, the stress classification line results might be the reverse of what was expected. Know which end of the line matches the inside of your vessel (coordinates for the lines can be found below the graph)…

The sample utility included with this report has a box that allows the direction of the line in the graph to be reversed (normal or reverse) – note: which end is chosen as end i or j has no impact on the calculated results.

Step 3 – Translate the Stresses to Local Coordinates

When the data is imported, 6 stress components are read for each node on the SCL. The stress components are aligned with the global coordinate system of the model. The data for each node needs to be translated along the line ij. Instead of directions x, y and z, we now have N, T and H.

Theoretically, N stands for Normal, T Tangential and H Hoop stress directions. However, when the program reads and translates the data, the only guaranty is that the tangential stress is aligned to the SCL running from ij and N and T are at 90 degrees to it and each other.

NutsBoltsStress_Image3

Step 3b – Interpolate the Data Points

This utility uses cubic splines to interpolate more data points along the SCL. 71 equally spaced nodes are used to reduce integration errors caused by too few data points. See Appendix 3.

Step 4 – Calculate the Membrane Stress: Pm

The distance between each node along the SCL is the dimension dx. dx usually varies between nodes depending on how the model is meshed. Sum (integrate) dx*Sn over the length of the SCL from i to j. Repeat for each of the other 5 local stress components. This produces 6 stress components (Snm, Stm, Shm, Tntm, Tnhm, Thtm). These 6 components are either fed into a Tresca routine (ASME VIII-2 2006 edition) or von Mises (ASME VIII-2 2007 edition). The output is a single value for the membrane stress.

NutsBoltsStress_Image4

Note – von Mises stresses can be 85% to 100% of the reported Tresca stress for the same input data. Von Mises stress criteria of VIII-2 2007 edition is less conservative than the 2006 Tresca criteria.

The membrane stress (and other intermediate stresses) can be found to the right of the output section of the sheet.

NutsBoltsStress_Image5

Step 5a – Calculate the Bending Stress: Pb

The bending component is perpendicular to the SCL. Only components Sn, Sh and Tnt are perpendicular to the line running from i to j. The program integrates the “linear varying portion” of these stresses along the line and produces Snb, Shb and Tnhb bending components. See the section “IntegrateMembraneAndBendingStress” in the code to see how the membrane and bending components are calculated.

The utility uses the three components to calculate the bending only stress.

NutsBoltsStress_Image6

The Pb stress has no real application in pressure vessels on its own. The code rules for determining the acceptability of stresses refer to membrane + bending stress…

Step 5b – Calculate the Bending + Membrane Stress: Pm + Pb

The membrane + Bending stress needs to be calculated for each end of the SCL.

NutsBoltsStress_Image7

The end with the larger stress is reported. The utility included with this report interpolates the membrane + bending stress from i to j.

Step 6 – Calculate the Peak Stress

The actual stress at each node is known from step 3. The SCL utility calculates and plots the von Mises or the Tresca stress for each node. The peak stress is simply the highest calculated stress along the line from i to j.

Note: The peak stress can be higher or lower than the membrane + bending stress. Two pages follow – in the first, the peak stress in a wide flange beam under bending load is slightly less than the membrane + bending stress. In the second, the peak stress in a heavy wall pipe is much higher than the membrane + bending stress.

Note – the Pm and Pm+Pb stress is used to determine if the stress is below the code allowed limits and for cycle life calculation. Peak stress is not normally used.

NutsBoltsStress_Image8

Peak stress is less than Membrane + Bending stress

NutsBoltsStress_Image9

Peak stress is much greater than Membrane + Bending stress

Step 7 – Show the Shear Stress at Each Node (A Step for the User, Not the Utility)

The shear stress can be used to judge the quality of the SCL. For many pressure vessel applications, the shear stress is expected to be zero at the inner and outer surface of a pressure vessel. The following 2 examples show an SCL firstly perpendicular to the surface and in the second example slanted. The components of shear in the second example are clearly not zero at each end.

For this very simple example, the shear stresses could be used to pick between a good SCL and a bad one. Some locations on a vessel have surface shear stresses so this rule will not always work.

Step 8 (Also a Step for the User!) – Study the Results…

…and think about it. The SCL utility is just a tool – use your brain!

NutsBoltsStress_Image10

NutsBoltsStress_Image11

App. 1: Finding Endpoints of the Stress Classification Line (SCL)

The data is imported from the FEA program in nodal order. The nodal order has no relation to the order that the elements are needed for analysis. The nodes must be arranged from inside (i) of the model to outside (j). The endpoints have to be found, and the nodes ranked from i to j.

This utility sorts the imported nodes to find the two nodes with the largest distance from all the other imported nodes. These nodes are the endpoints i and j. The node closer to the origin is assigned as i.

Note: the use of i as the inside and j as the outside is an arbitrary but convenient notation. Identical results will be obtained if i and j are reversed.

See the routine ChooseNodeij for more details. This routine can handle distorted stress classification lines and individual nodes that are located off the true SCL. Curved SCLs could also be used.

App. 2: Routines for von Mises and Tresca Stress (VBA)

These routines are programmed into the sample excel spreadsheets. Von Mises is easy. Tresca is bear involving finding the principle stresses (Mohr’s circle). Look for the routines VonMisesStress and TrescaStress

App. 3: Integration Method

The quality of results obtained from stress classification are strongly dependent upon the number of nodes found on the SCL. When insufficient nodes are present, the linearization tool will typically over-report the membrane and the membrane+ bending stress.

NutsBoltsStress_Image12

The above membrane stress data is from the thick walled pipe sample. The stress linearization utility included with this report uses 71 node cubic spline interpolation along the imported SCL data. This original data set has 17 nodes from i to j. In the above graph, nodes are dropped from the data set to produce SCLs with 17, 9, 5, 3 and 2 nodes. Without interpolation 9 nodes are required to reduce the error level to below 5%. With cubic spline interpolation, this level of accuracy is reached with about 4-5 nodes. The more complex the stress pattern, the more pronounced the effect.

Typically the stresses in an object are highest at the surface. This effect causes the linearization tool to over-report stresses in the middle of the object when insufficient nodes are used. The end result is reported membrane and bending stresses that are higher than actual.

NutsBoltsStress_Image13

This is only one cause of bad results with few nodes. The other is the integration mathematics. Bending stresses calculations use both the distance from the center of the line and the magnitude at the point. These calculations are more accurate as the distance between points is decreased. Doubling the amount of data points on a SCL by simple linear interpolation between each given point increases the accuracy of the results. Using spline interpolation is better. For this utility 71 nodes are used to provide good quality graphs.

NutsBoltsStress_Image14

Here the results are shown for the same thick walled pipe sample. 17 nodes are read from the SCL. Cubic spline interpolation is used to setup new evenly spaced nodes along the line. The error from integration drops to less than 1% at 17 nodes. This error occurs for complex or simple stress patterns. Interpolation increases the accuracy of results.

71 nodes are used in the sample program. This corresponds to an expected integration error of 0.04% and provides plenty of nodes for a good graphing. An odd number of nodes are used to provide a middle node for the M+B graph. This same result using linear instead of cubic spline interpolation requires about 500 interpolated nodes.

Download:

Stress Classification Lines (SCL) – Passing Through Areas of Very High Error

Stresses at sharp corners rise towards infinity as the mesh size is reduced. However the forces have to balance in a Finite Element model regardless of the mesh size used. In these studies SCL (Stress Classification Line) results are compared a different mesh sizes . PRINT EXPAND SHRINK LINK

Stress Classification Lines (SCL) – Passing Through Areas of Very High Error

File: PVE-3277, Last Updated: Feb 2009, By:LB, Update Sept 14 2016 LB

Summary

Stresses at sharp corners rise towards infinity as the mesh size is reduced. However the forces have to balance in a Finite Element model regardless of the mesh size used. In these studies SCL (Stress Classification Line) results are compared a different mesh sizes. This report shows that it is possible to take stress classification lines through these areas of peak stress and get ultimate stresses – however the results will not be as expected.

Two studies are shown. In Study 1, the SCL passes between 2 sharp corners. The stress classification method produces results that do not vary as the mesh is refined. However, it misses the magnitude of the membrane and reports no bending stress. This is a limitation of the stress classification method.

In study 2, the SCL passes through only one sharp corner. This study shows results that converge to a finite value. Again, the reported membrane stress is less than expected.

Sharp corners exist in pressure vessels, and produce high stresses in those locations.  We rely on the pressure vessel being built from ductile materials reducing the corner stresses from infinity to the material yield point.  Where possible, removing the sharp corners removes peak stresses.  When this can not be done, the SCL is the tool used to report the stress in a manner consistent with code rules.

Study 1 – High Error on Both Ends

Drawing of simple flat plate model.

The test shape – a simple flat plate modeled at 1/4″ thickness.

Drawing of split lines used to provide fixed nodes.

The split lines to provide nodes in fixed locations regardless of the mesh size used. The first line passes through the corners with zero radius and a theoretical infinite stress.

Drawing of applied loads.

Applied loads – 500 psi at the left edge. The right edge is fixed. The shell model is meshed at 1/4″ thick. Line 1 and Line 2 are identified. They are referred to as Stress Line 1 and Stress Line 2 in the rest of the report.

Stress results at 1 inch mesh.

Stress results at 1″ mesh size. Stress Intensity (Tresca*2 or P1-P3).

Error plot for 1 inch mesh.

The error plot for the 1″ Mesh size – the error around the corners is greater than 5% and should not be used. However, the results will be included in line #1. Line 2 only passes through elements with less than 5% error and should be acceptable.

Graph of von Mises

SCL through Stress Line 1 at 1″ mesh size. Membrane Stress = 282.93 psi Membrane + Bending Stress = 289.28 psi

von Mises graph for 2 inch mesh

SCL through Stress Line 2 at 1″ mesh size.
Membrane Stress = 333.45 psi
Membrane + Bending Stress = 334.59 psi

von Mises graph for 0.5 inch mesh

SCL through Stress Line 1 at 0.5″ mesh size.
Membrane Stress = 289.963 psi
Membrane + Bending Stress = 290.71 psi

von Mises graph stress line 2

SCL through Stress Line 2 at 0.5″ mesh size.
Membrane Stress = 333.43 psi
Membrane + Bending Stress = 333.92 psi

von Mises graph

SCL through Stress Line 1 at 0.25″ mesh size.
Membrane Stress = 286.58 psi
Membrane + Bending Stress = 288.69 psi

StressClassLine_Image11

SCL through Stress Line 2 at 0.25″ mesh size.
Membrane Stress = 333.42 psi
Membrane + Bending Stress = 333.66 psi

StressClassLine_Image12

SCL through Stress Line 1 at 0.125″ mesh size.
Membrane Stress = 290.21 psi
Membrane + Bending Stress = 292.58 psi

StressClassLine_Image13

SCL through Stress Line 2 at 0.125″ mesh size.
Membrane Stress = 333.42 psi
Membrane + Bending Stress = 333.53 psi

FEA error plots for 4 mesh sizes

Error plots for the 4 mesh sizes studied. Same 0-5% scale.

Graph of stress vs mesh size

Conclusions for Study 1:

1) Although SCL 1 passes through 2 areas of theoretical infinite stress, and resulting high error, the SCL results are practically unchanged as the mesh is refined. Although the stresses are rising at the ends of the SCL at points that are approaching infinity, these high stresses are affecting increasingly smaller element areas and are having smaller impacts. The end result is constant reported Membrane and Membrane + Bending results.

2) The reported membrane stress for SCL 1 is less than for SCL 2. The expected answer is that the membrane stress is the same for both lines – 333 psi. For SCL 1, shear stress Tnt provides a large component of the stress. This stress is positive at one end of the SCL and negative at the other. The membrane stress is calculated by averaging these stresses over the length of the line, so Tnt makes no contribution.

The stresses at both ends of SCL 1 increase. They are not alternating (increasing on one end, decreasing on the other) as is found in a bending stress. The SCL tool does not see these stresses as being a bending stress because they are not alternating.

The results are not as expected for SCL 1 – this is a limitation of the stress classification method. Stress classification lines should not be run between 2 sharp corners.

Study 2 – High Error on One End Only

The shape from study 1 is cut in half for this next study. SCL 1 runs from a sharp corner to a smooth surface. Identical stress classification locations are used.

Drawing for study 2

The test shape #2 – One half of the test shape used in study #1 – again modeled at 1/4″ thickness. The split lines to provide nodes in fixed locations regardless of the mesh size used. The first line passes through one corner with zero radius (and a theoretical infinite stress). Line 1 and Line 2 are identified. They are referred to as Stress Line 1 and Stress Line 2 in the rest of the report.

FEA model - applied loads

Applied loads – 250 psi at the left edge. The right edge is fixed. The shell model is meshed at 1/4″ thick. Stress results are shown at 1″ mesh size. Stress Intensity is shown (Tresca*2 or P1-P3). Theoretical stress is 250 lbs/(3″ x 0.25″) = 333.33 psi.

Error plot of 1 inch mesh.

The error plot for the 1″ Mesh size – the error around the corners is greater than 5% and should not be used. However, the results will be included in line #1. Line 2 only passes through elements with less than 5% error and should be acceptable.

Graph of von Mises

SCL through Stress Line 1 at 1″ mesh size. Membrane Stress = 280.98 psi Membrane + Bending Stress = 337.22 psi

StressClassLine_Image20

SCL through Stress Line 2 at 1″ mesh size. Membrane Stress = 333.35 psi Membrane + Bending Stress = 334.85 psi
The remaining Stress Line 2 plots look identical and are not shown.

StressClassLine_Image21

SCL through Stress Line 1 at 0.5″ mesh size.
Membrane Stress = 289.43 psi
Membrane + Bending Stress = 365.89 psi

StressClassLine_Image22

SCL through Stress Line 1 at 0.25″ mesh size.
Membrane Stress = 293.38 psi
Membrane + Bending Stress = 381.87 psi

StressClassLine_Image23

SCL through Stress Line 1 at 0.125″ mesh size.
Membrane Stress = 296.27 psi
Membrane + Bending Stress = 392.75 psi

Chart of mesh sizes and stressesGraph of stress vs mesh size

Conclusions for Study 2:

1) SCL 1 which passes through an area of theoretical infinite stress reports increasing Membrane and Membrane + Bending results as the mesh is refined. However, these reported results converge to fixed, not infinite values. Ultimate stresses at zero mesh size can be extrapolated for the Membrane and the Membrane + Bending stresses. The ultimate membrane stress is less than the 333 psi expected because some of the stress is interpreted as bending.

2) Avoiding the areas of high error on one end of an SCL is desired if possible.

Origins of the ASME Fatigue Life Curves Post

How do ASME permissible fatigue curves compare to actual fatigue life results? Can they be used to predict the expected life of equipment? PRINT EXPAND SHRINK LINK

Origins of the ASME Fatigue Life Curves Post

How do ASME permissible fatigue curves compare to actual fatigue life results? Can they be used to predict the expected life of equipment?

The graph below is the original data used to create the ASME permissible fatigue life curve for carbon steel alloys[1,2,3]. The black line is the best fit curve though the original data points. I traced the Table 3.F.1 permissible cycle life stress values, the red line, onto the original graph.

Graph

Best fit of test results (black line) versus permissible fatigue life.  Note that both axis are logarithmic.

The ASME permissible curve is obtained from the original data by adding the following factors of safety: Each point on the ASME line is either 1/2 the value of the original curve above it, or 1/20th the cycle life to the right [Ref 1, page 19]. See the green markups below:

CalculationDetail

Comparing one data point – the red line should be the most conservative of 20x to the left of, and 2x below the best fit data.  It is actually 26x to the left and 4x below.

The 20x safety factor on cycles equals (2x for data scatter) x (2.5x for size effects) x (4x for surface finish and environment) [Ref 1, page 37]. The actual data for the point chosen above – 110 permissible cycles at 200,000 psi has stress divided by 4 (800,000 psi on the graph) and cycles divided by 26 (2860 cycles) – much more conservative than the guideline. Further, when dealing with welds, an additional factor of up to 4x is removed from the permissible cycle life to account for increased stresses inside the weld [4].

These ASME curves are not useful for predicting the cycle life of equipment. They are used to specify a permissible design life which includes a large factor of safety.

[File: PVE-5522, Last Updated: Aug. 21, 2012, LRB]

References:

[1]Fatigue Design of Process Equipment, ASME Plant Engineering & Maintenance Technical Chapter, March 12, 2009, Chris Hinnant, Paulin Research Group, Houston, TX www.paulin.com . See pages 20 and 37

[2]STP770 – Low-Cycle Fatigue and Life Prediction, Amzallag C, Leis BN, Rabbe P, Published: 1982 www.astm.org

[3]”Code Design and Evaluation for Cyclic Loading – Sections III and VIII” ASME.org

[4]ASME VIII-2 2010 ed., 2011 add. Table 5.11 – Weld Surface Fatigue-Strength-Reduction Factors

Simplification of FEA by Symmetry

FEA model sizes and run times are reduced by finding symmetry. PRINT EXPAND SHRINK LINK

Simplification of FEA by Symmetry

File: NA, Last Updated: N/A, By:LB

For irregular geometry, classical B31.3 rules cannot be applied. As a result, a Finite Element Analysis (FEA) is required, meeting ASME VIII-2 guidelines as permitted by B31.3.

Ultraflo brochure

In many cases, the geometry of the part is symmetrical about one or more base planes.

Valve showing symmetry

In this case, one of Ultraflo’s wafer valves requires CRN registration. The valve is symmetrical about the centre of the valve from left to right, and front to back.

Solid model extracting 1/4 of model

Because of this symmetry the entire valve need not be analyzed. One quarter of the model can be extracted and used. This reduces the complexity of the mode and the time required to perform the analysis.

Applying constraint of symmetry to model cut planes.

How is this symmetry accounted for in the analysis? When running the FEA one of the constraints is symmetry about the model cut planes.

Applying contraints and loadings

The remaining constraints and loadings are applied as if the whole model is included. This is possible when the loadings are symmetrical about the same planes the geometry was sectioned. In this case internal pressure and surface contacts on the interface between the two halves (and bolt) are applied (for explanation of multi-body part analysis see below).

FEA results

The results are interpreted the same as if the entire model were analyzed. Ultraflo’s wafer valve analysis was accepted by the jurisdiction and Ultraflo obtained their CRN#.

A special thanks to Ultraflo Corporation, #8 Trautman Ind. Dr. Ste. Genevieve, MO for allowing use of their valve geometry for this exercise.

(Note: the stress results show do not represent actual stresses under operating conditions, arbitrary loadings were applied and arbitrary stresses are shown.)

Finite Element Analysis Reaction Forces

Reaction forces are the resulting loads seen at the restraints of a model being analyzed. They can be used to ensure an analysis is restrained from rigid body motion, and is static or in balance. The reaction forces are equal and opposite to the sum of the applied loads. Unless they are right, the results cannot be trusted. PRINT EXPAND SHRINK LINK

Finite Element Analysis Reaction Forces

File: PVE-3179, Last Updated: Jan. 22, 2009, By: BV

Reaction forces are the resulting loads seen at the restraints of a model being analyzed. They can be used to ensure an analysis is restrained from rigid body motion, and is static or in balance. The reaction forces are equal and opposite to the sum of the applied loads.

This report shows typical methods used for restraining models and compares the resulting displacement and stresses of identical models both in balance and out of balance for two different FEA models.

Example #1: F&D Head – 15 Degree Swept Model (Checking Static Condition)

FEA model of F&D Head

A 15 degree sweep of a F&D head is used in this example to demonstrate the method used for checking that a model is static or in balance.

alt="FEA model showing restraints"

The head is restrained using symmetry on all cut plane surfaces. These restraints allow the model to be held in model space while still being able to deform due to applied loads. The restraints must be applied in each of the three primary directions to avoid rigid body motion.

FEA model showing 80 psi pressure

An 80 psi pressure is applied normal to on all internal surfaces. The reaction resultant is calculated for each primary direction.

FEA model showing X component of reaction.

The X component of the reaction resultant can be found by looking at the model along the x-axis or normal to the YZ plane. The pressure boundary sketch outlines the area of applied pressure.

FEA model shows the X reaction area normal to the YZ plane

The above image shows the X reaction area normal to the YZ plane. The X reaction force is calculated by multiplying the reaction area in the x-direction by the applied pressure. X Reaction = (941.76 in^2) * (80 lb/in^2) = 75,340.8 lb

FEA model along Y axis

The Y component of the reaction resultant can be found by looking at the model along the y-axis or normal to the XZ plane.

FEA model shows the Y reaction area normal to the XZ plane

The above image shows the Y reaction area normal to the XZ plane. The Y reaction force is calculated by multiplying the reaction area in the y-direction by the applied pressure. Y Reaction = (975.99 in^2) * (80 lb/in^2) = 78,079.2 lb

Z component of the reaction resultant

The Z component of the reaction resultant can be found by looking at the model along the z-axis or normal to the XY plane.

ReactionForces_Image9

The above image shows the Z reaction area normal to the XY plane. The Z reaction force is calculated by multiplying the reaction area in the z-direction by the applied pressure. Z Reaction = (123.99 in^2) * (80 lb/in^2) = 9,919.2 lb

Theoretical Reaction Force Components:

X Reaction = -75,340.8 lb
Y Reaction = -78,079.2 lb
Z Reaction = -9,919.2 lb

Note: Component directions are generated by inspection of the pressure

ReactionForces_Image10

The reaction components can be reported from SolidWorks Simulation and measured against the theoretical values.

Theoretical Resultant = SQRT ((-75,340.8 lb)^2 + (-78,079.2 lb)^2 + (-9,919.2 lb)^2)
Theoretical Resultant = 108,954 lb

Actual Reaction Force Components:
X Reaction = -75,344 lb
Y Reaction = -78,075 lb
Z Reaction = -9,922 lb
Actual Resultant = SQRT ((-75,344 lb)^2 + (-78,075 lb)^2 + (-9,922 lb)^2)
Actual Resultant = 108,950 lb

Error Calculation:
Error = ((Resultant Theoretical - Resultant Actual) / Resultant Actual) * 100%
Error = ((108,954 lb - 108,950 lb) / 108,950 lb) * 100%
Error = 0.00%

From the error calculation we can see that the actual results fall within 2% of the theoretical results. This criteria determines if a model is acceptable for analysis of stresses and displacements.

FEA model showing displacement of F&D head.

The model is in balance and the stresses and displacements can be analyzed to prove the acceptability of the design. The above view shows the displacement of the F&D head. This displacement is typical for F&D heads.

FEA model showing stress in F&D head.

The above view shows the stress in the head. The head stresses are radial which indicates the model is reacting correctly to the applied pressure.

Example #2: Hydraulic Manifold Block

The hydraulic manifold block used in this example demonstrates how an out of balance model affects model displacement and stress results.

FEA model of a complete hydraulic manifold block.

Pipes and pipe caps have been added to this manifold block to simulate loads applied at the port locations.

FEA model - fixed restraint is placed on the end face of the in-line pipe

A fixed restraint is placed on the end face of the in-line pipe. Applying this restraint to the pipe end allows the hydraulic manifold block to deform without any undue restraints.

FEA model - internal cavity surfaces are pressurized to 300 psi

All internal cavity surfaces are pressurized to 300 psi. In this example the model is not sectioned using symmetry or other means. This requires the model to be closely examined for missing areas. Missing areas will unbalance the internal forces due to the pressure.

FEA model - reaction forces

Without observing the reaction forces it is evident that the deformation is not as expected. The entire block begins to rotate about its fixed restraint. The missing area on the left side of the model results in greater forces (due to pressure) in the positive y direction than the negative y.

FEA model displays large stresses.

Large stresses are generated in the line-in pipe due to the resulting moment shown in the previous figure. These results indicate that the model is out of balance.

FEA model rection forces 0.

The reported reactions forces from SolidWorks Simulation for this example are non-zero value in the Y directions. The model is not balanced and the displacement and stress results are not valid.

Three different methods of checking the model balance (unexpected displacement, unexpected stress and out of balance reactions) have all indicated the same thing: this model can not be used as is.

FEA model with unbalanced internal areas

The reaction forces unaccounted for are generated by unbalanced internal areas. The area on the right of the model is greater than that of the left. When forces are calculated by multiplying these areas by the internal pressure it is evident that the net reaction force will not be zero.

FEA model with reaction areas.

The reaction force in the y-direction is equal to the sum of all 3 areas multiplied by the internal pressure.

FEA model - section properties

The unbalanced force due to the missing area of each port can be calculated by multiplying the area by the internal pressure.

Reaction per Port = (0.864 in^2) * (300 lb/in^2) = 259.276 lb

Often the magnitude of the reaction force can be used to determine what is causing the imbalance.

alt="FEA model - force is added to each port to balance the model in the y-direction"

A force is added to each port to balance the model in the y-direction. These forces account for the missing areas of applied pressure and place the model in balance.

x-direction of the model

The x-direction of the model has a reaction force due to the uncapped line-in port of the manifold. The reaction areas in the x-direction are unbalanced due to the void at the line-in port.

FEA model - multiplying reaction area by pressure.

The reaction force at this port can be calculated by multiplying the reaction area by the pressure. Reaction X = (3.36 in^2) * (300 lb/in^2) = 1008 lb

FEA model showing x-direction out of balance.

The model is not in balance in the x-direction. The restraint needs to provide a force to prevent motion in the x-direction. The restraint provided an equal and opposite force to the pressure multiplied by the line-in area.

Theoretical Reaction Summary:

Reaction X = 1008 lb
Reaction Y = Force Applied – Force Due to Exit Pressure
Reaction Y = 3 Ports * (259 lb -259 lb)
Reaction Y = 0
Reaction Z = 0
Theoretical Resultant = SQRT ((1008 lb)^2 + (0 lb)^2 + (0 lb)^2)
Theoretical Resultant = 1008 lb

FEA model - final reaction components.

The final reaction components can be reported from SolidWorks Simulation and measured against the theoretical values.

Actual Reaction Force Components:
X Reaction = 1009.6 lb
Y Reaction = -4.03 lb
Z Reaction = -3.47 lb
Actual Resultant = SQRT ((1009.6 lb)^2 + (-4.03 lb)^2 + (-3.47 lb)^2)
Actual Resultant = 1009.6 lb

Error Calculation:
Error = ((Resultant Theoretical – Resultant Actual) / Resultant Actual) * 100%
Error = ((1008 lb – 1009.6 lb) / 1009.6 lb) * 100%
Error = -0.16 %

From the error calculation we can see that the actual results fall within 2% of the theoretical results. This model is in balance and can be used to calculate displacements and stresses.

FEA - diplacement as expected with balanced model

The displacement is as expected with the model in balance. The model displaces outward and elongates axially due to the internal pressure. This expected displacement is much less than the previously reported out of balance displacement.

FEA - line-in pipe view.

Stresses are no longer exaggerated at the line-in pipe. The balanced model provides realistic displacements and valid stress results that can be analyzed against material allowables.

Summary

Checking the model balance is an important step for verifying that all loads are acting upon restraints correctly. An out of balanced model provides invalid result that cannot be used.

Why Use 2nd Order Integration Elements?

Use of 2nd order integration elements is more than a requirement, it also produces the best results. PRINT EXPAND SHRINK LINK

Why Use 2nd Order Integration Elements?

This is part of a series of articles that examines the ABSA (Alberta Boilers Safety Association) requirements on writing FEA reports. These guidelines can be found at: ABSA Requirements. The use of 2nd or higher order elements is one of the requirements.

Pressure Vessel Engineering uses SolidWorks Simulation for Finite Element Analysis. It is expected that these results would also be applicable to other FEA programs.

Why use 2nd Order Integration Elements?

  • Because ABSA tells us to?
  • Because that is the default Cosmos Designer Setting?

1st Order integration is found in the Mesh Options box under quality. The Draft option produces first order elements. High option produces 2nd order or higher – the default option. Integration beyond 2nd degree has to be chosen through the analysis properties window. 2nd order is the highest order available for shell elements.

First and second order shell elements

First and second order shell elements – 2nd order adds mid-side nodes

Problem 1 – Shell Elements in Tension

Which elements will produce better results for a simple tension load? The sample problem below is worked out in both 1st and 2nd order elements.

FEA model of a bar.

The model – a bar 1″ wide x 4″ long – it is split at 1″ to make a sampling point.

FEA model showing fixed and sample points.

The bottom is fixed and a 1lb tension load is applied to the top. The model is meshed at 1″ thickness – a 1 psi stress is expected.

Model of typical error plot

Typical error plot: 1/4″ mesh 1st order elements shown

FEA - stress intensity plot

Stress Intensity plot for 1/8″ 2nd order elements.

Chart of Stress and Error results.

Stress and Error Results

Graph of Stress and Error

Graph of stress and error plot for the sample point. The stress values are practically identical; however, the 1st order elements have a much higher reported error level.

For this problem with a simple stress distribution, both the 1st and 2nd order elements produce excellent results as the mesh changed from 1/4 to 1/16″ size.

Problem 2 – Shell Elements in Bending

Using the same model from sample #1, the 1 lb tension load is changed to a 1 lb sideways or bending load. The moment of inertia is bh^3/12 = 1/12 in^4. The distance from neutral axis is 0.5″. The moment at the sample point is 3 in*lbs . The expected stress at the sample point is Mc/I = 3*0.5/(1/12) = 18 psi.

FEA model

Same model – load is now horizontal to create a bending load

Stress distribution

The expected stress distribution for a bending load

Error plot

Error plot for 1/4″ 1st order elements.

Stress plot

Stress plot for 1/4″ 1st order elements.

Graph of Stress and Error

Stress and Error Results

Graph of Stress and Error

Graph of stress and error plot for the sample point. The First order elements have much higher real and reported error levels.

The stress pattern in this bar is a simple linear distribution – but the 1st order elements do a lousy job of representing it. The second order elements did a good job, even at the coarsest mesh size.

The reported error in all cases is much higher than the real error. For example the reported stress for the 1st degree elements at 1/4″ mesh is 16.5131 psi, theoretical stress is 18 psi. The real error is 8.3%, but it is reported at 21.8%. This over estimation is true for all the reported errors.

Problem 3 – Complex Stress in Shell Elements

Simple uniform or linearly varying stresses do not often show up in real world FEA problems. How do the 1st and 2nd order elements handle more complex stress patterns?

Model of a bar

The model – a bar 1″ wide x 4″ long – it is split at 1″ to make a sampling point.

Model with fixed bottom.

The bottom is fixed and a 1lb tension load is applied to the top. The model is meshed at 1″ thickness – a complex stress pattern is expected.

Error plot

Error plot for 1/4″ 1st order elements.

Stress plot

Stress plot for 1/4″ 1st order elements.

Mesh close-up

Mesh close-up – 1st order 1/4″ elements

FEA model

Mesh close-up – 2nd order 1/4″ elements – note the better looking holes

Chart of Mesh vs. stress and error.

Stress and Error Results – Degrees of freedom of the models are added.

Graph of Mesh vs. stress and error.

Graph of stress and error plot for the sample point.

The 1st and 2nd order elements are both converging to the same stress value. The 2nd order models are getting to the end value much faster. The 2nd order result was obtained at 1/8″ mesh size when the error was reported at 2%. The 1st order elements have not got there at 1/32″ – and the reported error is above 2%. From the COSMOSWorks help files:

It is highly recommended to use the High quality option for final results and for models with curved geometry. Draft quality meshing can be used for quick evaluation.

The degree of freedom of the model is related to the computer resources required to solve the problem. In this case, the 1st order model did not reach the result with a DOF of 18,000, but the 2nd order study got there by DOF = 4,800, a much better use of computer resources and users time.

Solid Models

The same mesh quality issues apply to 3D as to the previous 2D studies. Here is a part with a round hole. With a coarse mesh size, the 1st order model only slightly looks round. The second order results look much better.

FEA model 1st order mesh

1st order mesh on a block with a hole

FEA model 2nd order mesh

Same mesh size – 2nd order elements

Why use 2nd Order Integration Elements?

  • Because ABSA tells us to?
  • Because that is the default Cosmos Designer Setting?
  • Because 2nd order elements do a better job of capturing the surface details.
  • Because 2nd order elements do a better job of calculating complex stresses.
  • Because 2nd order elements required fewer computer resources.

Large Displacement Solutions

This solar reflector uses a vacuum to pull the front and back surfaces together to focus the reflective surface. The deflected surface shape can be calculated using FEA, but the correct shape can only be computed with large deflection theory. PRINT EXPAND SHRINK LINK

Large Displacement Solutions

File: PVE-4048, Last Updated: March 2010, By: LB

This solar reflector uses a vacuum to pull the front and back surfaces together to focus the reflective surface. The deflected surface shape can be calculated using FEA, but the correct shape can only be computed with large deflection theory.

Stretched membrane heliostat

A stretched membrane heliostat

Surface model stretched membrane heliostat

A surface model of a stretched membrane heliostat reflector (not the same reflector as in the photo)

For this sample, a 0.064″ thick 16ft diameter stainless steel reflector is focused with a 0.1 psi vacuum. This reflector is studied first with linear theory:

0.1 psi vacuum applied to heliostat

A 0.1 psi vacuum is applied to create the focus by stretching the membrane

Linear theory results for heliostat

Initial linear theory results – the displacement is wrong (3235 inches!) – the two surfaces are shown passing through each other

What went wrong? The linear theory assumes that the stiffness of the reflector does not change as its shape changes. As a result the only stress computed is a flat panel bending stress. In reality, the application of the vacuum changes the shape from flat to spherical. After a very small deflection, the membrane stress in the deflected spherical shape is much higher than any bending stress.

Mesh for linear theory

Linear theory – no membrane stresses are reported for the mirror.

FEA Analysis for bending stresses

Linear theory – huge bending stresses are reported.

SolidWorks Simulation suggests using large displacement theory to solve the problem:

Solidworks Linear Static message

Large displacement theory is suggested for this study

From the SolidWorks Simulation help files:

The linear theory assumes small displacements… This approach may lead to inaccurate results or convergence difficulties in cases where these assumptions are not valid… The large displacement solution is needed when the acquired deformation alters the stiffness (ability of the structure to resist loads) significantly… The large displacement solution assumes that the stiffness changes during loading so it applies the load in steps and updates the stiffness for each solution step.

This perfectly describes this reflector. The application of a very small vacuum changes the shape from a flat plate to a curved shape. The correct analysis is membrane not bending.

SolidWorks Simulation applies the pressure in steps. The stiffness of the membrane is recalculated after each step. The large displacement solution takes a lot longer to run.

Solidworks Displacement at 3x

Large displacement theory deflection magnified 3x

Large displacement membrane stress plot

Large displacement membrane stress plot

Membrane stresses – the stresses are approximately those of a sphere (where the stress would be uniform across the whole surface).

Minimal stress results for large displacement theory

Minimal stress is shown in the large displacement theory bending stress results. Bending stresses are almost zero except at the fixed edges.

Graph of Deflection vs Location

A plot of the actual deflection vs the deflection for a true sphere shows that the shape is not truly spherical, which matches the membrane stress plot which shows a non uniform stress distribution. The linear theory plot is different in shape and magnitude.

The SolidWorks Simulation help file has useful information on using large displacement solutions.

Error Plots – Bolt Heads and Surface to Surface Contacts

Two common areas of high error in a FEA report are under bolt heads and at surface to surface contacts. This article explains in more depth why this happens. PRINT EXPAND SHRINK LINK

Error Plots – Bolt Heads and Surface to Surface Contacts

File: PVE-3179, Last Updated: Dec. 13, 2008, By: LRB

Summary

Error plots show how well the complexity of a mesh matches the complexity of the deflections in a model. Once the mesh complexity matches the model complexity the reported error is low. As a guideline, Pressure Vessel Engineering uses 5% error as an acceptance criterion.

It is possible to get stresses below 5% in general vessel areas by applying an appropriate mesh size. This report covers two areas where the error cannot be lowered to reach this acceptance criteria regardless of the mesh size used. These areas are: 1) stresses in and around the head of a bolt and 2) stresses at surface to surface contacts.

Other areas also exist in pressure vessels where mesh refinement can not be used to reduce errors to this 5% acceptance level. These areas: weld fillets, diameter transitions, nozzles, flanges and support legs and lug attachements are beyond the scope of this article.

Example:

Solid model of test shape

Example test shape – an assembly of 3 parts: 2 plates of 2″ x 2″ x 1/2″ thick with 1/2″ radius hole in one corner. The test plates are joined with a 7/8″ root diameter bolt. The bolt is made 0.002″ shorter than the two plates to create an interference fit preload.

Model with no penetration surface defined.

A no penetration surface is defined between the two plates. The plates can separate but not pass through each other.

Example of interference fit

An interference fit is defined between the bolt head and the top plate. The bolt will be stretched to reach the top surface. The top surface will be compressed by the bolt.

Model with symmetry boundary conditions applied.

Symmetry boundary conditions are applied to sides and bottom of assembled model.

Model with mesh at 1/8 size.

The model is meshed at 1/8″ size.

Close-up of model with interference mesh.

Close up of the interference mesh between the bolt and the top plate.

FEA Model of displacement plot.

Displacement plot – the plates are in contact under the bolt head, separated elsewhere. The bolt was stretched > 0.01″ to create a preload. The plate also compressed under the bolt head. This stretch is shown magnified x125 here so the bolt appears to be out of contact with the top plate – it is in contact.

Close-up of model showing contact area.

A close-up of the contact area between the two plates.

Intensity stress plot.

Intensity stress plot (Tresca P1-P3 criteria) – the highest stress is indicated under the bolt head.

Close-up of FEA model showing stress area.

Close-up of the highest reported stress area – under the bolt head.

Overall error plot.

Overall error plot. The error plot shows areas in and around the bolt head to be higher than the 5% acceptance criteria.

Error plot scaled to 100%.

The error plot scale re-scaled to 100% maximum. The maximum error is located under the bolt head at the edge of the bolt to top plate interference contact. The sharp edge of the contact area can not be eliminated regardless of the mesh size used. This area will always have a high indicated error.

ASME VIII-2 (2287 Ed.) sets the stress limits for bolts at locations away from the stress concentrations.

VIII-2 5.7.2(a): The maximum value of service stress, averaged across the bolt cross section and neglecting stress concentrations, shall not exceed two time the allowable stress values in paragraph 3.A.2.2. of annex 3.A

VIII-2 5.7.2(b): The maximum value of service stress, except as restricted by paragraph 5.7.3.1(b) [fatigue assessment of bolts] at the periphery of the bolt cross section resulting from direct tension plus bending and neglecting stress concentrations shall not exceed three times the allowable stress values in paragraph 3.A.2 of Annex 3.A

The bolts are studied at some location other than under the head. Large stresses concentrations are also created at the location where the bolt threads into its parent material (not shown in this model). This area will also show a high indicated error.

Model with area of high reported stress.

Another area of high reported error: the contact between the top and bottom plates.

Close-up of model with contact pressure.

Close-up of the previous shot – contact pressure at the surface to surface contact between the two steel plates. These contact areas show as high errors regardless of the mesh size used.

FEA Submission Requirements

Finite Element Analysis (FEA) can usually be used to support pressure equipment design submissions where the configuration is not covered by the available rules in the ASME code. Requirements vary by province. PRINT EXPAND SHRINK LINK

FEA Submission Requirements

Last Updated: Aug 19 2015, By: LRB

The requirements for FEA reports are outlined in CSA B51-14 annex J “Annex J (normative) Requirements regarding the use of finite element analysis (FEA) to support a pressure equipment design submission”. These requirements are mandatory to B51, but not universally accepted across Canada. At this date (Aug 2015) Alberta reviews are still done to ABSA AB-520, a similar but not identical document. Some extracts from the B51 standard are included in italics below.

J.1 General

This analysis method requires extensive knowledge of, and experience with, pressure equipment design, FEA fundamentals, and the FEA software involved. The FEA software selected by the designer shall be applicable for pressure equipment design.

FEA programs are physics engines. We have found that any of the main commercially available programs are suitable for pressure vessel analysis. In particular we use SolidWorks Simulation and ABACUS, but others also work.

J.2 Submission requirements

FEA may be used to support pressure equipment design where the configuration is not covered by the available rules in the ASME Code. The designer should check with the regulatory authority to confirm that use of FEA is acceptable. When this method is used to justify code compliance of the design, the requirements in Clauses J.3 to J.10 shall be met.

In general we find it acceptable to use FEA for design of non code items or portions of items. It is important to include code calculations for those portions of the vessel that are code calculable. On rare occasions a product is forced to be re-designed so that regular code sections can be used. This is discussed further here.

J.3 Special design requirement

The FEA analysis and reports shall be completed by individuals knowledgeable in and experienced with FEA methods. The FEA report shall be certified by a professional engineer.

We sometimes get asked to provide a report of our experience. See our Contacts page where we have posted qualification resumes for our review engineers. For example, the resumes of Ben, Cameron and Matt
have been written to present qualifications for performing FEA and reviewing FEA reports.
For the sections J.4 through J.10 we refer to sample reports found in our FEA samples section. These reports are written to meet this or various previous provincial guidelines. Beyond this CSA guideline, our sample reports are also modified to answer common questions from CRN review engineers and customers.

J.4 Report executive summary

The FEA report shall contain an executive summary briefly describing how the FEA is being used to support the design, the FEA model used, the results of the FEA, the accuracy of the FEA results, the validation of the results, and the conclusions relating to the FEA results supporting the design submitted for registration.

J.5 Report introduction

The report introduction shall describe the scope of the FEA analysis relating to the design, the justification for using FEA to support the design calculations, the FEA software used for the analysis, the type of FEA analysis (static, dynamic, elastic, plastic, small deformations, large deformations, etc.), a complete description of the material properties used in the analysis, and the assumptions used for the FEA modelling.

J.6 Model description

J.6.1

The report shall include a section describing the FEA model used for the analysis. The description shall include dimensional information and/or drawings relating the model geometry to the actual pressure equipment geometry. Simplification of geometry shall be explained and justified as appropriate. The mesh and type (h, p, 2D, 3D), shape, degrees of freedom, and order (2nd order or above) of the elements used shall be described. If different types of elements (mixed meshes) are used, a description of how the different elements were connected together shall be included. When shell elements are being used, a description of the top or bottom orientation with plots of the elements shall be included and shall indicate if they are thick or thin elements.

J.6.2

The model description shall include a list of all assumptions.

J.6.3

The turn angle of each element used on inside fillet radii shall be indicated.

The turn angle is simply the number of elements it takes to go around a circle. This Inventor support page explains the use of a turn angle. It is normal that a mesher needs around 8 elements to get around a circular hole which would produce a turn angle of 45 degrees per element. Decreasing the turn angle increases the number of elements and the accuracy of the FEA results, however not all areas of a model need to be highly accurate. The turn angle does not provide any predictive value, and the B51 standard provides no acceptance criteria. The use of an error plot as discussed in J.6.8 below is a much more useful measure of mesh and results quality.

J.6.4

The method used to select the size of mesh elements with reference to global or local mesh refinement shall be indicated.

We use the error plot to determine if the mesh is adequately refined. Beyond the scope of this standard, it is important to realize that pressure vessels have areas of discontinuity where in theory the stress approaches infinity as the mesh size is decreased. In practice the vessel experiences stresses above the yield point. Refer to our sample jobs for linearization analysis that can deal with stresses approaching infinity.

J.6.5

When items in contact (e.g., flange joints, threaded joints) are modeled, the model shall describe how two separate areas in contact are linked. Adequate mesh size shall be used to ensure that the elements are small enough to model contact stress distribution properly.

J.6.6

Boundary conditions, such as supports, restraints, loads, contact elements, and forces, shall be clearly described and shown in the report (present the figures). The method of restraining the model to prevent rigid body motion shall also be indicated and justified. When partial models are used (typically based on symmetry), the rationale for the partial model shall be described with an explanation of the boundary conditions used to compensate for the missing model sections.

J.6.7

The FEA report shall include validation and verification of FEA results. Validation should demonstrate that FEA results correctly describe the real-life behavior of the pressure equipment, and verification should demonstrate that a mathematical model, as submitted for solution with FEA, has been solved correctly.

Verification is as simple as comparing the reaction forces from the FEA run with the theoretical loads that can be calculated at the boundary conditions. What is acceptable for validation varies by reviewer. Rarely FEA runs must be provided that predict burst test results. Occasionally strain gauge testing or displacement testing must be provided that can be run against a standard non destructive hydrotest. Other methods used are comparing Roark’s predicted radial displacement of a shell with the results of a model run. Most commonly, it is recognized that a FEA run that meets the other requirements of this standard is far more accurate than other available methods of study so no further physical testing proof is required.

J.6.8

The accuracy of the FEA results shall be included in the FEA report, either by the use of convergence studies or by comparison to the accuracy of previous successful in-house models. An error of 5% or less from the convergence study shall be acceptable.

Note: FEA inaccuracy usually consists of discretization errors, which result from matching geometry and displacement distribution due to the inherent limitation of elements, and computational errors, which are round-off errors from the computer floating-point calculation and the formulations of the numerical integration scheme.

A convergence study only proves that a single point of a model has converged, whereas an error plot proves a whole model, and does not required multiple FEA runs. As mentioned in J.6.4 we use error plots to prove convergence. Again as mentioned above, not all areas of a pressure vessel model converge, the areas that do not require special study that cannot be handled by convergence studies. These areas are usually handled by Linearization as outlined by ASME VIII-2 part 5.

J.7 Acceptance criteria

The criteria for acceptance of the FEA results shall be based on the code of construction and factor of safety established under that code. The FEA methodology may be based on another code. The acceptance criteria and code reference shall be presented in the report.

Note: For example, if the code of construction is Section VIII, Division 1, of the ASME Code, the allowable stress values are from Section VIII, Division 1, of the ASME Code. The FEA methodology could be based on Section VIII, Division 2, of the ASME Code (Figure 5.1).

J.8 Presentation of results

J.8.1

The following information and figures in colored prints shall be presented:
(a) resultant displacements (plot);
(b) deformed shape with undeformed shape superimposed;
(c) stress plot with mesh that
(c)(i) shows fringes using discrete color separation for stress ranges or plots; and
(c)(ii) allows comparison between the size of stress concentrations and the size of the mesh;
(d) plot with element stress and a comparison of nodal (average) stress vs. element (non-averaged) stress;
(e) reaction forces compared to applied loads (free-body diagrams);
(f) stress linearization methodology and the stress values in the area of interest; and
(g) accuracy of the FEA results.
The results shall be plotted to graphically verify convergence. The x axis of this plot shall show some indication of mesh density in the area of interest (number of elements on a curve, elements per unit length, etc.). This is necessary to show true convergence over apparent convergence that is due only to a relatively small change in the mesh.

J.8.2

When plots or figures are presented, an explanation relating to each figure shall be included to describe the purpose of the figure and its importance.

J.9 Analysis of results

Overall model results, including areas of high stress and deformation, shall be presented with acceptance criteria. The analysis shall include a comparison of the results with acceptance criteria.

Results that are to be disregarded shall be identified, and the determination to disregard them shall be justified.

J.10 Conclusion

As a minimum, the conclusion shall include
(a) a summary of the FEA results in support of the design;
(b) a comparison of the results and the acceptance criteria; and
(c) overall recommendations.

 

Mesh Refinement at Discontinuities

Error plots show how well the complexity of a mesh matches the complexity of the model. Once a match is made the reported error is low. PRINT EXPAND SHRINK LINK

Mesh Refinement at Discontinuities

Last Updated: Nov. 26, 2008, By: LB

Using the Error Function Results for Areas At Discontinuities

Error plots show how well the complexity of a mesh matches the complexity of the model and its loads. Once the mesh matches the complexity of the model, the reported error is low. We use 5% error as an acceptance criterion. This method checks the whole model at once, and is much less work than mesh refinement.

This study compares mesh refinement at a node with error plot methods to estimate the convergence of FEA results. CosmosDesigner (Now SolidWorks Simulation) 2708 SP5.0 FEA software is used for this report.

Example: Shell Element Error Plots

Mesh_Refinement_Image1

Test shape – a simple flat plate modeled at 1/4″ thickness. 3 test points (1, 2, 3) are shown on this model. A split line has been added to guarantee a node will always be available at point 2 to sample. For this sample, the stress at the three points is of interest, so the error at those points has to be less than 5% per the acceptance criteria.

Mesh_Refinement_Image2

Applied loads – 2 x 500 psi at the left edge. The right edge is fixed. The shell model is meshed at 1/4″ thick.

Mesh_Refinement_Image3

1″ mesh size. The reported error in the area of interest is greater than 5%. The results can not be used.

Mesh_Refinement_Image4

Similarly, mesh sizes of 0.75″, 0.5″, 0.375″, 0.25″ and 0.1875″ all report error greater than 5%. 1/8″ mesh size is the first size to produce acceptable results (below). (All are scaled 0 to 5% error.)

Mesh_Refinement_Image5

1/8″ mesh size – coarsest mesh to produce an acceptable error plot for the 3 areas of interest.

Mesh_Refinement_Image6

The overall stress pattern for the 1/8″ mesh size – Tresca stress intensity (P1-P3).

Mesh_Refinement_Image7

Close up stress plot of the 3 nodes of interest. The Tresca stresses at the test locations: 1 – 22.2 psi, 2 – 674.7 psi, 3 – 941.0 psi. How accurate are these stress values?

Mesh_Refinement_Image8

Stress results graph

Mesh_Refinement_Image9

Stress results

Stress results and stress results graph. For this study, the results from 0.125 and 0.063″ mesh size meet the 5% acceptance criteria.

Mesh_Refinement_Image10

Extrapolated stress value

An ultimate stress value is extrapolated using linear regression on the above stresses and extrapolating to a theoretical zero mesh size (the 1″ mesh size data point for stress 1 is ignored).

Mesh_Refinement_Image11

In general, when the reported error is less than the 5% acceptance criteria, the actual error is much less. Even when the acceptance criteria is met, some elements will have higher error levels (Point 1 at 0.063″ mesh).

Mesh Refinement vs Error Plots

Mesh refinement by measuring the stress at individual locations and extrapolating to a theoretical zero mesh size can be used to validate individual areas on a model. However, many FEA runs are required, and in this case, only 3 points on the model were proven. There is no guarantee that the most important points have been studied. The Error plots prove every element in the model. If the first mesh chosen is acceptable, no additional work is required to prove the model.

Mesh Refinements Near Discontinuities

his report examines the accuracy of stress results near an area of discontinuity as the mesh is refined. PRINT EXPAND SHRINK LINK

Mesh Refinements Near Discontinuities

Last Updated: May 10 2013, By:LB

Error plots show how well the complexity of a mesh matches the complexity of the model. Once the mesh matches the complexity of the model, the reported error is low. As a guideline, Pressure Vessel Engineering uses 5% error as an acceptance criterion.

This report examines the accuracy of stress results near an area of discontinuity as the mesh is refined. The 5% error criteria estimates the errors in the mesh except in areas of very low stress located near high stress areas. These areas are not usually of interest in a pressure vessel study.

In this study stresses are measured at 5 fixed locations in a simple shape as the mesh size is changed. The stress errors predicted by the error function are compared with ultimate stress predicted from mesh refinement. SolidWorks SimulationDesigner 2008 SP5.0 FEA software is used for this report using 2nd order shell elements.

Drawing of a simple flat plate model.

The test shape – a simple flat plate modeled at 1/4″ thickness. The model has a sharp radius and a sharp corner. Test data will be taken near the sharp radius and at the sharp corner.

Flat plate model with two test areas.

The surface is split to provide test areas 1 through 5 at fixed locations regardless of the mesh size used.

Flat plate model with applied load of 500 psi.

The applied load is a 500 psi force at the right edge. The left edge is fixed. The shell model is meshed at 1/4″ thick.

FEA model of flat plate with 1 inch mesh.

The stress results at 1″ mesh size. Stress Intensity (Tresca*2 or P1-P3) is used for all pictures.

FEA model of flat plate - error plot

The error plot for the 1″ Mesh size – results for areas 2, 3, 4 and 5 should not be used. Elements with errors greater than 5% are within 1 element of the test node locations. The result for test node 1 can be used.

Error plots for mesh sizes 1/2 - 1/8

Mesh sizes 1/2″ through 1/8″ all produce acceptable results for test nodes 1 to 4. Test node 5 is unacceptable for all mesh sizes.

FEA model of flat plate - stress pattern

The overall stress pattern for the 1/16″ mesh size – shown as Tresca stress intensity (P1-P3). How accurate are these stress values?

Charts comparing mesh with stress and error.

Stress and Error results for the 5 test points. All data for points 1-4 meet the 5% acceptance criteria, but points 2-5 were previously disqualified at the 1″ mesh size due to being within 1 element of areas of >5% error. Point 5 fails the criteria for all mesh sizes.

RefineNearDiscon_Image9

Point 1 – all stress results show an error of less than 5%. The ultimate stress is extrapolated to 113.52 psi.

RefineNearDiscon_Image10

Point 2 – all stress results show an error of less than 5%. Stress at 1″ mesh size has been disqualified as being within 1 element of a node with greater than 5% error.

RefineNearDiscon_Image11

Point 2 again – stress results extrapolated from mesh sizes 0.5″ or smaller. The ultimate stress is extrapolated to 31.47 psi

RefineNearDiscon_Image12

Point 3 – all stress results show an error of less than 5%. Stress at 1″ mesh size has been disqualified as being within 1 element of a node with greater than 5% error. The ultimate stress is extrapolated to 351.87 psi.

RefineNearDiscon_Image13

Point 4 – all stress results show an error of less than 5%. Stress at 1″ mesh size has been disqualified as being within 1 element of a node with greater than 5% error. The ultimate stress is extrapolated to 350.38psi.

RefineNearDiscon_Image14

Point 5 – all stress results show an error of more than 5%. Stresses at all sizes are disqualified as being over 5%. The ultimate stress is extrapolated to infinity at 0 mesh size.

Chart of Ultimate stress

The ultimate stress allows the SolidWorks Simulation error estimate to be compared to the true error. The true error is (actual stress – ultimate stress) / ultimate stress.

Graph of predicted error vs. true error.

The graph of the predicted error from the SolidWorks Simulation error functions vs. the true error. The predicted error is not very good for point 2. Point 2 is a very low stress area of the model. The results for point 2 change a lot as the mesh size changes and are not accurate.

Charts comparing error and reported error.

FEA model of points 2 and 4.

Point 2 is a low stress area adjacent to a high stress area (the sharp radius area) on the model. As the mesh is refined, small changes in the mesh in the radius area have large effects on point 2. The error function can not predict the error for this situation. Areas of low stress are not usually of interest in pressure vessel finite element studies.

Graph of predicted error vs. true error.

The same error results with point #2 removed.

Predicted error vs. true error.

The graph shows good correlation between the extrapolated true stress and the reported error from the SolidWorks Simulation error function. The true stress is approximately 1.49x the reported stress for points 1, 3 and 4 for this shape.

Conclusion

The SolidWorks Simulation Error function will not work for all locations on a model. For this model, the error results for Point 2 – a low stress area adjacent to a high stress area – were found to be not useable (the reported stress was too low vs. the real stress). Areas of low stress like this would not normally be of interest in a pressure vessel study.

As a guideline, at Pressure Vessel Engineering we consider using caution when viewing results at a node when there are elements within 1 node that have errors over 5%.

Point 5 – the sharp corner – never achieved an acceptable error level of 5% or less. The theoretical stress at a sharp corner is infinite. As the mesh size was reduced, the stress followed a curve towards infinity. The error function correctly showed that the results for that node were never usable.

In spite of the presence of Point 5 on the model – that theoretically reaches infinity – the stress values at the other locations settled along a smooth trendline towards an ultimate finite value. For these remaining locations, the error function predicted error results of 2/3 the actual final error. (Other reports have shown true errors of less than the predicted error.)

With these limitations in mind, the error function is a useful predictor of the accuracy of the calculated results without the need to run multiple mesh size runs. The error function checks the results for entire models vs. mesh refinement which only validates the actual points under study.

Surface Model Mesh Challenges

>Surface models can be challenging to mesh. Parts that touch might not share nodes preventing the correct transfer of loads. The resulting calculated stresses and displacements can be wrong. PRINT EXPAND SHRINK LINK

Surface Model Mesh Challenges

File: PVE-4048, Last Updated: Feb. 24, 2010, LB

Surface models can be challenging to mesh. Parts that touch might not share nodes preventing the correct transfer of loads. The resulting calculated stresses and displacements can be wrong.

A segment of the bottom half of storage sphere - here 1/2 of 1 leg is being analyzed.

A segment of the bottom half of storage sphere – here 1/2 of 1 leg is being analyzed.

The sphere and legs are shell modeled.

The sphere and legs are shell modeled.

The stresses in this leg are wrong:

Calculated stress values

Calculated stress values

Close up of the leg to skirt attachment

Close up of the leg to skirt attachment

The stress distribution in the leg to skirt attachment is uneven. Turning on the mesh shows the uneven mesh that is supposed to be connecting these two parts.

The mesh is not joining along the edge

The mesh is not joining along the edge

The problem does not go away with mesh refinement or tolerance adjustments. The problem is intermittent – some parts will join, some not. A recent update to SolidWorks Simulation can fix this problem:

Standard mesh fails

Standard mesh fails

Curvature based meshing works

Curvature based meshing works

That's better!

That’s better!

Curvature based meshing was not include in SolidWorks Simulation 2008. This example was run in SolidWorks Simulation 2010.

Update: An alternate fix is to knit the surface.

Update: An alternate fix is to knit the surface.

Here the standard mesher was used with the leg surface knit to the skirt. The standard mesher produces a better looking mesh.

Easier Surfaces

Surfaces can be challenging to create, but solids are easy to convert into surfaces. Surfaces originally created as solids do not have the problem of nodes not joining at edges PRINT EXPAND SHRINK LINK

Easier Surfaces

File: PVE-4048, Last Updated: Feb. 24, 2010, By: LB

Surfaces can be challenging to create, but solids are easy to convert into surfaces. Surfaces originally created as solids do not have the problem of nodes not joining at edges.

This complex duct shape was made with a few simple solid modeling commands and then turned into a shell model by removing a few faces at the end of the pipes.

This complex duct shape was made with a few simple solid modeling commands and then turned into a shell model by removing a few faces at the end of the pipes.

The model before the faces have been removed converting the solid model into a surface.

The model before the faces have been removed converting the solid model into a surface.

he mode meshes without fuss even at very coarse settings using the standard mesher. All nodes connect across surface boundaries.

The mode meshes without fuss even at very coarse settings using the standard mesher. All nodes connect across surface boundaries.

Beautiful stress results from thermal expansion.

Beautiful stress results from thermal expansion.

Close up

Close up

Solid Model Mesh Challenges

Sometimes a multibody model refuses to mesh with the standard mesher. Regardless of the element size and tolerances used, some parts refuse to bond. PRINT EXPAND SHRINK LINK

Solid Model Mesh Challenges

File: PVE, Last Updated: May 2010, By:LB

Sometimes a SolidWorks Simulation multibody model refuses to mesh with the standard mesher. Regardless of the element size and tolerances used, some parts refuse to bond.

SolidWorks image - large propane storage sphere

A large propane storage sphere

SolidWorks image - meshed with 802,000 elements

Meshed with the standard mesher – 802,000 elements – 12″ large and 4″ small element sizes

The standard mesher has run, but when the analysis is performed, some of the bodies are not joined.

SolidWorks stress results

Stress results – a surface has not joined (Displacements magnified 100x)

SolidWorks close-up

A close up of the area that did not bond (Displacement magnified 20x) The 4″ elements at the leg and the 12″ general shell elements can be seen.

The curvature based mesher produces a less uniform looking mesh, and in this case the produced mesh has more elements.

SolidWorks - curvature based mesher settings used

Curvature based mesher settings used. A mesh refinement of 4″ size is set for the legs.

SolidWorks detail of mesh

A detail of the mesh created with the curvature based mesher, 925,000 elements are produced.

Correct results from the curvature

Correct results from the curvature based mesh run

Close up of the results

Close up of the results

In theory it should be possible to alter any model to make it meshable by the standard mesher. Here the panel that will not mesh into the leg is split in half.

Alternate solution

Alternate solution – a panel where the mesh does not work has been split in half.

The model has successfully meshed and run.

The model has successfully meshed and run. The split panel is shown.

Note: this model run is used to determine the frequency of vibration of a sphere with a 1g sideways load. The stresses and deflections do not represent real world seismic conditions.

Mesh Tolerance Settings

Getting the standard mesher tolerance incorrectly can make some external features disappear. Meshing can fail on internal features. PRINT EXPAND SHRINK LINK

Mesh Tolerance Settings

File: PVE-4048, Last Updated: FEb 17 2010, By: LRB

What impact does the mesh tolerance option have on the mesh produced by SolidWorks Simulation?

Caution: every time the mesh size is changed, the tolerance is adjusted to 5% of the mesh size. This is a very nasty feature! Keep your eye on the tolerance and set it back the to value you require after each mesh size change.

Mesh Size and Tolerance Setting

External Features

As the mesh tolerance increases, exterior model details disappear from the mesh. This block is 5 x 5 x 1 inch high. Each feature is 1 x 1 inch. Feature height changes as shown.

Mesh test shape

SolidWorks Simulation can mesh the object with very coarse mesh sizes, as long as the tolerance is fine enough:

Mesh Results

Run #1, the mesh size is at 1 inch and the tolerance at the cosmos default 0.05 inch (5% of mesh size). When the tolerance is increased to or above the size of a feature, it disappears from the mesh.

Run #1, the mesh size is at 1 inch and the tolerance at the cosmos default 0.05 inch (5% of mesh size). When the tolerance is increased to or above the size of a feature, it disappears from the mesh.

Run #2, the mesh size is still at 1 inch, but the tolerance is increased to 0.125 inch (the height of the first feature). The first feature disappears.

Run #2, the mesh size is still at 1 inch, but the tolerance is increased to 0.125 inch (the height of the first feature). The first feature disappears.

Run #4, the tolerance is at 0.26 inch, the second feature disappears (the center of it still exists, but the edges are gone).

Run #4, the tolerance is at 0.26 inch, the second feature disappears (the center of it still exists, but the edges are gone).

Run #8, the mesh size is 1.125 inch and the tolerance 1 inch, all features and much of the base disappears. The mesh does not have to be smaller than the feature size modeled.

Run #8, the mesh size is 1.125 inch and the tolerance 1 inch, all features and much of the base disappears. The mesh does not have to be smaller than the feature size modeled.

Run #9, The mesh size is 2.5 inch, but the small features are still modeled because the tolerance is set to 0.05 inch.

Run #9, The mesh size is 2.5 inch, but the small features are still modeled because the tolerance is set to 0.05 inch.

Internal Features

Block with cut features

Slightly different results are achieved with internal cut features.

Here the extruded bosses are replaced with cut slots: 1, 0.5, 0.25 and 0.125″ wide all the way through the same 5 x 5 x 1″ block. When the tolerance is too coarse, the mesh fails:

Mesh Results for internal cut holes

Watch for this reason for mesh failure. If the cut features are not desired in the mesh, they have to be removed from the model.

Solution for Long Mesh Time of Shells

When meshing shells using SolidWorks Simulation, the mesh gets up to 99% and then hangs for a very long time sometimes for hours depending on the mesh size... PRINT EXPAND SHRINK LINK

Solution for Long Mesh Time of Shells

File: PVE-4048, Last Updated: Feb. 24, 2010, By: LB

When meshing shells, the mesh gets up to 99% and then hangs for a very long time sometimes for hours depending on the mesh size. The mesher is going through some type of crazy routine trying to orient all of the shell faces in the same direction. We can do this manually in a few seconds by picking the face and then right clicking mesh and “Flip Shell Elements”.

Go to Simulation options and un-check the “Automatic re-alignment for non-composite shells”:

Image of Default Options for Mesh

In the example model, doing this reduced the mesh time from 8 min 21 seconds down to 20 seconds.

Adjusting the mesh size after setting the face orientation causes some of the faces to be re-oriented. Manually flipping the faces is still much quicker than waiting for the automatic re-alignment.

Reduce Your Mesh Time

Splitting a complex component into multiple smaller components can reduce the mesh time. PRINT EXPAND SHRINK LINK

Reduce Your Mesh Time

File: PVE-4061, Last Updated: Jan 1 2010, By:LB

Inside view of a storage sphere.

Inside view of a storage sphere.

Front view of a storage sphere meshed.

Front view of the storage sphere.

This 25ft diameter storage sphere with unusual legs is solid meshed. At a 5″ element size (the element size that will mesh), it takes 172 seconds to mesh. The bad news is that a smaller mesh is require in a number of locations. When the overall element size is reduced to 3″, it takes 1002 seconds to mesh.

Sphere meshed at 5in element size.

Front view – Nodes = 123,000, Elements = 61,000, 172 seconds to mesh

Detail of the sphere meshed at 3in element size.

Detail meshed at 3″ size – Nodes = 318,000, Elements = 158,000, 1002 seconds to mesh

Splitting large objects into smaller items can reduce the mesh time. Here the sphere is split into 6 and 12 pieces.

Sphere split into 6 bodies.

The sphere split into 6 bodies

Sphere split into 12 bodies.

The sphere split into 12 bodies

The mesh times go down significantly as the sphere is split into smaller bodies.

5 inch mesh size for split sphere

6 body sphere at 5 inch mesh – mesh time is 46 seconds (127,000 nodes, 63,000 elements)

Detail of the 12 body sphere at 3 inch mesh size.

12 body sphere at 3 inch mesh – mesh time is 161 seconds (326,000 nodes, 163,000 elements)

Mesh Time for all runs

Summary of all mesh time data. The reduced body size makes a huge difference as the number of elements increases.

Reducing the body sizes can have a huge impact as the number of elements exceeds 1 million…

Simulating Heat Exchanger Tubes with Springs Post

Heat exchangers are often very large models. In order to simplify them for FEA we usually remove all of the tubes and replace them with simulated springs. This significantly reduces the complexity of the mesh. PRINT EXPAND SHRINK LINK

Simulating Heat Exchanger Tubes with Springs Post

File: File:PVE-4473, Last Updated: Oct 4, 2010, By: CBM

Heat exchangers are often very large models. In order to simplify them for FEA we remove all of the tubes and simulate using springs. This will significantly reduce the number of elements and allow the model to mesh and solve in a more reasonable time frame.

The heat exchanger model with tubes

The heat exchanger model with tubes

The tubes have been removed and will be simulated with springs

The tubes have been removed and will be simulated with springs

In order to use the spring connectors we have to determine the applicable spring rate of the tubes. There is a direct relationship between Hooke’s law for springs and the material’s modulus of elasticity.

Hooke’s law for springs: F = k * d

Axial displacement: d = F * L / (A * E)

Where:

	F = Axial Force [lb]
	k = Spring Rate [lb/in]
	d = Displacement [in]
	L = Tube Length [in]
	A = Cross Sectional Area [sq. in]
	E = Modulus of Elasticity [psi]

Combining these equations we get: d = k * d * L / (A * E)

k = A * E / L

Solidworks Simulation has a distributed spring option which allows a distributed spring rate over a selected area. The equation now becomes:

k = A * E / (L * A)

Therefore: k = E / L

Preload:

In the case of fixed tubesheets, the differential thermal growth between the tubes and the shell generates a load acting on the tubesheets. The spring connectors must be preloaded to account for this force. We know that the equation for thermal expansion is:

d = ∝ * L * ΔT

where:
	d = Displacement [in]
	∝ = Material's thermal expansion coefficient [ in/in/°F]
	L = Original tube length [in]
	ΔT = Change in temperature [°F] from ambient to the operating temperature

The difference in expansion between the shell side and the tube side is:

d = ∝ tube side * L * (Ttube side – 70) – ∝shell side * L * (Tshell side – 70)

This value is substituted into the spring rate equation (F = k * d) to determine the corresponding preload.

Applied spring loads

The information required to define a spring connector is now available. A distributed option has been selected and is applied to all tube holes.

Frequency / Vibration Analysis

These stacked exchangers are analyzed using FEA and building code rules. FEA is used to determine the vibration frequency, which is put into building code rules to determine the base shear. PRINT EXPAND SHRINK LINK

Frequency / Vibration Analysis

File: File:PVE-4492, Last Updated: Sept 2, 2010, By: BV

Frequency and Vibration Analysis

Frequency and vibration analysis
FEA is used for frequency and vibration analysis to determine the natural frequency of objects which cannot be obtained from classical calculations. The natural frequency can then be compared to the system resonance to ensure large amplitude oscillations will not occur. The natural frequency may also be used with building codes to determine a base shear force which can then be input to a stress analysis to validate designs subject to seismic or other oscillating conditions. A complete engineering report is available below representing a typical seismic analysis and report completed by Pressure Vessel Engineering.

Seismic Analysis of Pressure Equipment

Seismic analysis of pressure equipment

To find the natural frequency two inputs are required, mass and stiffness. The object to be analyzed in modeled and its density (mass) and modulus of elasticity (stiffness) defined. The FEA solver then determines several displacement modes and their corresponding natural frequencies.

Pressure Vessel Engineering then uses the natural frequency provided by the FEA to determine a base shear force in accordance with building codes such as NBC, IBC, and UBC.

The base shear force is then converted to an acceleration (F = ma, both force and mass are known) and input into a stress analysis to investigate seismic loadings on the object. These stress results then either validate the design or provide insight as to how it should be revised.

Downloads

SolidWorks File Format

How to access the raw data contained in the SolidWorks output files. PRINT EXPAND SHRINK LINK

SolidWorks File Format

Background – Which Files!

SolidWorks Simulation (SWS) results are stored in a proprietary *.CWR format. SWS creates intermediate files during the analysis and combines them in the CWR file at end of run. SWS uses the standard Microsoft IStorage interface to create the CWR file, so it is possible to open the CWR file with the stg file examiner (formerly available from Microsoft Support).

SWS_FileFormat_Image1

The above files contain all the data required to show all of the results plots from a FEA run.

It is not necessary to extract the files from the CWR container file. Setting the save intermediate files in SWS prevents the above files and more from being erased after a run. The above list shows which files from the many available are important!

Set the above option flag under Simulation/Options.../Default Options/Results/Results Folder.

Set the above option flag under Simulation/Options…/Default Options/Results/Results Folder.

Most of the files are in proprietary binary format; a few are text providing SWS run time messages. The order of execution can provide useful information on the file contents. FEA programs solve for displacement before stresses, so file time stamps can hint at what will be in a file. A large FEA run provided the following approximate run sequence:

ELF -> LCD -> EFF -> OUT -> STE -> GEN -> MAS

All dimensions and stresses are stored in metric: m and N/m^2

ELF File Format – Element Flexibility? – File #1

The ELF format contains node ordered data. This file type has been examined for models with 3, 4, 6 and 10 nodes per element. The file contains data for 6 degrees of freedom for each node, whether the degrees of freedom are required or not. Plate models use 6 degrees of freedom per node, solid and axisymmetric 3 degrees per node. The data start point changes with the number of nodes per element. Data is in single precision.

See the macro “ExamineELF” in the attached spreadsheet ELF File Examiner to examine data in 3,4,6 and 10 node per element models. Other node counts have not been tested. These macros use an array write command that cannot process huge files – make sure all of your data is imported before using.

LCD File Format – Displacement – File #2

The LCD file contains node ordered data. This file type has been examined for models with 3, 4, 6 and 10 nodes per element. The data always starts at 370h. The nodes always have 6 degrees of freedom, required or not.

See the macro “ExamineLCD” in the attached spreadsheet LCD File Examiner to examine data in 3,4,6 and 10 node per element models. Other node counts have not been tested.

This data exactly matches the results from the Displacement listing.

EFF File Format – Unknown – File #3

The purpose of the EFF file has not been determined.

See the macro “ExamineEFF” in the attached spreadsheet EFF File Examiner to examine data in 3,4,6 and 10 node per element models. Other node counts have not been tested.

OUT File Format – Solver Messages – File #4

The OUT text file contains a plain English language report.

STE File Format – Stress and Strain – File # 5

The number of nodes per element, and if the model is a shell or solid is required prior to reading the STE file. The STE file contains stress and strain data per node per element. The stress for a node is the AVEARAGE of the stress for that node in all elements that it occurs in.

As an example, we use this data for our linearization program. For each node on the linearization line, we average the stress for that node as reported by all elements that connect to it. All other nodes are ignored.

See the macro “ExamineSTEFile” in the attached spreadsheet STE File Examiner The spreadsheet has been tested for 3 and 6 node per element plate models and 4 and 10 node solid models. Other node counts have not been tested. Enter the nodes per element and “plate” or “solid” options in the spreadsheet before importing the file. This macro does not contain array fast write methods, so large files will take a while to examine. The results will not match your stress plots until all nodal occurrences are averaged.

To examine Axis-Symmetric models, set the correct number of nodes per element (3 or 6), but set the plate/solid option to SOLID.

GEN File Format – Original Node Coordinates – File # 6

The GEN binary file contains nodal coordinates prior to displacement in meters. Number of Elements is stored at 18Ch and the number of nodes at 190h. Data starts at 408h. Each record of singles is X, Y, Z and followed by 10 unwanted singles.

See the macro “ExamineGENFile” in the attached spreadsheet GEN File Examiner. No difference in file format has been noticed for 3, 4 or 10 node per element files.

MAS File Format – Unknown – File # 7

Data blocks are long – contents are unknown.

General Comments

We developed this access method because we had difficulty getting raw data out of SWS. SWS provides a series of API function calls to access the data in open files. We tried that method and it took hours to get data out of a large file. SWS also has a series of export data commands in the drop down menus. They also are slow – it would take up to 10 hours to export the data from a large FEA run. We successfully used this file format information in VBA to extend our stress linearization spreadsheet to directly access the CWR file results. We can get at the data we need quickly and easily.

[File: PVE-4631 / PVE-9259, Last Updated: Aug. 24, 2015, By:LRB]

 

Finite Element Analysis at PVEng

We use FEA to design and validate fittings and vessels that can not be designed by rule-based codes like VIII-1 or B31.3. We are experts in the specialized field of pressure equipment design by FEA to validated ASME VIII-2 methods.

  • SolidWorks Simulation and Abacus software
  • Pressure and thermal stress analysis
  • Permissible service life (fatigue life)
  • Wind and seismic analysis
  • Leg, saddle and clip design
  • Frequency and vibration analysis
  • Computational Fluid Dynamics (CFD)

Pressure Vessel Engineering has used Finite Element Analysis (FEA) to design and verify thousands of pressurized components. We have the knowledge and experience to get the job done right.

Other Services

ASME Code DesignWe work to many ASME standards to design and validate pressure vessels, boiler, fittings and piping systems.

Pipe Stress AnalysisPipe stress analysis is mandatory for British Columbia registration and it is recommended practice for many other systems.

Canadian Registration Number (CRN)We are Canada’s largest independent registrar of fittings, vessels and piping under the CRN program registering for more than a thousand customers.

About Us

Pressure Vessel Engineering has twenty years of successful experience in the pressure vessel field working for more than a thousand customers.

  • Six Professional Engineers on staff licensed to stamp and sign off on designs for use in all Canadian jurisdictions.
  • Fast and professional assistance from our 20-person company.

Need help? Our contact information is to the right.