FEA Methods Blog

This collection of articles covers a variety of methods used in Finite Element Analysis (FEA). Topics include applying flange loads, creating connections, analyzing rivets and methods of simplification.

Pressure Analysis of a Flange

This basic sample illustrates how FEA is used to validate a flange design that cannot be calculated with standard VIII-1 Appendix 2 code rules due to the shape of its hub. Standard Appendix 2 loads are applied and assessed against the rules of ASME VIII-2 for full code compliance. PRINT EXPAND SHRINK

Pressure Analysis of a Flange

File: PVE-3396, Last Updated: March 18, 2009, By: BV

FEA Analysis of a Flange

This sample report illustrates how FEA is used to validate flange design. This report format may be used to justify ASME code compliance, provide stress and displacement analysis, provide cycle life estimates, complete thermal analysis, and perform design validation and optimization studies. This format is fully CRN compliant and may be applied to many applications. This level of analysis can typically be completed within a week.

Download:

Reversed Dished Head

The process in this vessel required a reverse dished head. The reverse dished head could not be fabricated thick enough to meet the ASME VIII-1 rules. The chosen solution was to reinforce the head with ribs to prevent snap through. Various alternate methods of analysis are shown here. Only the plate analysis was used for the actual job, however the comparison of the various methods is educational. PRINT EXPAND SHRINK

Reversed Dished Head

File: PVE-407, Last Updated: June 2, 2003, By: LB

The Problem:

Sample17_Reversed_Dish

The process in this vessel required a reverse dished head. The reverse dished head could not be fabricated thick enough to meet the ASME VIII-1 rules. The chosen solution was to reinforce the head with ribs to prevent snap through.

Various alternate methods of analysis are shown here. Only the plate analysis was used for the actual job. However, the comparison of the various methods is educational.

The head diameter and thickness and design pressure of 75 psi is the same for all of the examples bellow. The material has a yield strength of 30,000 psi and an allowed design stress of 20,000 psi. The maximum allowed membrane (tensile) stress is 20,000 psi, 30,000 at regions of discontinuities. The maximum allowed membrane + bending stress is 30,000 psi, 60,000 psi at discontinuities.

Analysis – 2D Axisymmetric with Linear Material Properties:

This is one of the simplest methods of analyzing this vessel. A cross section of the head without reinforcement is analyzed. Algor assumes that the 2D drawing is symmetrical about an axis (axisymmetric). The results show the stress distribution in the head if there is no material yielding (linear material properties).

Cross section of reverse dished head.

Cross section of the reverse dished head (from center to left side). Stresses are shown for an interior pressure in this and the following shots.

The peak stress is 54,000 psi in the knuckle region, well above the 30,000 psi yield point. This head fails the ASME VIII-1 code calculations for exterior pressure, but the stresses in the knuckle region are less than the discontinuity stress limit of 60,000 psi. Predicted deflection is 0.15 inches (not shown). Perhaps the head is safe? The ASME code calculations provide a safe pressure of 57 psi for a regular dished head. Also, the use of regular dished head exterior pressure calculations is not proven for a reverse dished head.

Analysis – 2D Axisymmetric with Non-Linear Material Properties:

This analysis allows for material yielding. The same cross section is analyzed, but for this analysis, the pressure is applied in steps, and the material will be allowed to yield (Non-Linear). The results can be seen in this movie.

Up to 64 psi, the head can be seen deflecting linearly under pressure. At 69 psi snap through is beginning (and the deflection is greater than the material thickness). At this point the head has started permanent deformation – it will not return to the original shape after the pressure is removed. Pressures beyond 72 psi show rapid snap through. The final frame shows the fully snapped through shape at 72 psi. This shape is kept permanently after the pressure is removed.

Defection of the center of the head.

Defection of the center of the head vs pressure. Snap through starts around 66 psi.

Original and final shape of head.

Original and final shape of head. Loaded to 75 psi and Pressure released.

Analysis – 3D Plate Analysis:

Reinforcing ribs were put on the head to prevent snap through. 3D analysis is required to calculate the stresses. A surface model was created in SolidWorks. The material thickness is specified at time of analysis in the Algor FEA program.

Plate model - top view.

Plate model – top view – created in SolidWorks.

Plate model - bottom view.

Plate model – bottom view.

The FEA analysis of the head in Algor showed that the stresses were acceptable. The maximum allowed membrane (tensile) stress is 20,000 psi, 30,000 at regions of discontinuities. The maximum allowed membrane + bending stress is 30,000 psi, 60,000 psi at discontinuities. Peak stresses around stress concentrations can be larger.

Membrane stress - model

Membrane Stress – limited to 20,000 psi except in areas of discontinuities. At areas of discontinuities, membrane stress can be 30,000 psi. This plot shows maximum membrane stresses at 42,000 psi at a concentration which is acceptable.

Total stress - model

Total Stress (Membrane + Bending) – limited to 30,000 psi except in areas of discontinuities. At areas of discontinuities, membrane stress can be 60,000 psi. The total stresses are acceptable.

Analysis – 3D Solid Analysis:

A solid model was created in SolidWorks including the reinforcing ribs and all weld fillets. The actual material thickness was modeled. This was not done for the original analysis, but is included here for educational purposes.

Solid model - bottom

Solid model – bottom view

Solid model - detail

Solid model detail – meshed at 1/8″ mesh size

Top side stress

Top side stress

Bottom side stress detail

Bottom side stress detail

The solid model maximum calculated stresses are found in the same location as for the plate model, but are much lower. The solid model accounts better for the stresses at connections, and allows the effect of weld fillets to be included.

The maximum stress is 28,000 psi, found in small peak areas. This value could be used with a fatigue analysis if required. All of the general stresses are below the 20,000 tensile limit, so no stress linearization is required to separate membrane and membrane + bending loads.

Chart of Displacement

Snap through analysis results for the solid bottom head. pressure at 1 sec is 75 psi. At 3.5x operating press the head starts to yield.

Displaced head at 5x pressure

Displaced head at 5x operating pressure – displacement magnified 2x.

The Solution:

The design with the reinforcing ribs was successfully used. A report interpreting the results according to ASME VIII-2 rules allowed the vessel to be registered. A later modification to the process allowed a less expensive double wall head to be used instead.

Comparison of Methods Shown:

The Solid and Plate analysis methods here produced almost identical stress results except at attachments. The Solid model with the weld fillets gave more realistic and lower stress results. The solid model was also easier to make than the plate model which required each surface to be split at all intersections. If the stresses were higher in the solid model, stress linearization would have been required to separate the membrane and membrane + bending stresses. The solid model stress linearization is more difficult than reading the stresses off of the plate model.

Credits:

This tank was built by Price Schonstrom Inc., 35 Elm Street, Walkerton, Ontario, Canada, N0G 2V0

Riveted Vessels

This digester has been in use since 1926. Vessels built in that time period were typically constructed with riveted butt joints. PRINT EXPAND SHRINK

Riveted Vessels

File:PVE-4687, Last Updated: 5-Nov-10, By: CBM

Pressure Vessel Engineering was contacted to help re-certify a series of 17′ Diameter 56′ tall digesters for Tembec Inc. which are currently in use for the pulp and paper industry. These digesters are filled with wood chips and mixed with acid in order to convert the wood chips to paper pulp.

Digester with Riveted Butt Seams

This digester has been in use since 1926. Vessels built in that time period were typically constructed with riveted butt joints.

Shell Model

A shell model of the entire digester was created and analyzed to determine the stress distribution.

Resulting Stress Profile

The resulting stress profile from the design pressure and static head. The highest stresses were observed at the bottom shell segments.

The next step was to analyze a small segment encompassing the bottom shell and cone and modeling in the actual butt straps with rivets. Rivets are installed in a hot state, so as they cool, they contract and generate a preload force that compresses the butt straps and the shell together. As the rivets cool, they plastically deform with preload stresses relaxing back to the yield point. Bolt connectors with the corresponding preload equal to the yield stress have been used to simulate the rivets.

Solid Model of the Digester

A solid model was created, incorporating the butt straps and the legs. Weight is applied to the model to generate stresses at the leg attachments.

Bolt Connectors

Bolt connectors are applied at each of the rivet locations with the calculated axial preload. No penetration contact sets are applied between all butt straps and shells.

Symmetry Conditions

The plane of symmetry cuts through the cylindrical shell. Symmetry is applied here. A seam is present at the conical shell thus no symmetry is applied. This forces the rivets to restrain the model.

Cross Sectional View of the Rivet

The rivet head is bonded on the inside and the outside butt straps. The rivet is restrained from moving through the hole in the conical shell.

Displacement

The digesters experience radial expansion along with a bending load on the legs.

Von Mises Stress

Although the riveted areas are perforated, the butt straps provide additional restraint and actually reduce stresses at the seam. Peak stresses are generated immediately around the holes due to the high compressive preload stress.

Rivet Peak Stress

Higher stresses occur around the rivet holes. This is caused by the rivet preload being set to the yield strength. This causes a high compressive stress at the joint.

Outer Rivets

An outer row of rivets with a larger pitch was used in this design. Although this is still below the allowable stress, a concentration of stresses build up in this region.

Our FEA was successfully used to prove the integrity of the digesters in their current state to the local jurisdiction and insurance company. Although riveted boilers and pressure vessels have not been manufactured for many years, there are a number of them that are still in operation today. Although built to ASME code, many of these boilers were constructed at a time when no CRN requirement was in place. As inspectors come across these vessels, we expect to see more of this type of inspection and certification requirement.

We at Pressure Vessel Engineering Ltd are very grateful to Tembec for allowing us to post this analysis. Tembec can be contacted at www.tembec.com or 819-627-4387.

Linear Multi-Body Analysis

Connections such as flanges, tri-clamps and any other multi-body assemblies are analyzed using FEA. This example shows a Tri-Clamp connection under internal pressure and describes how FEA is used to provide insight into the interaction between components. PRINT EXPAND SHRINK

Linear Multi-Body Analysis

File: File:PVE-4472, Last Updated: Aug 23, 2010, By: DRV

image001

A highly displaced view of a coupler joining two pipes finished with sanitary ferrules

FEA may be used to analyze single as well as multiple body designs. For multiple body analysis the interactions and restraints between bodies must be defined. The solver can then provide the resulting displacement, stress and contact pressure plots. Utilizing multiple bodies is typical of connection or joint analysis and allows the user to ensure proper preload and observe that joint separation does not occur. A complete engineering report of a multi body analysis typical of what is provided by Pressure Vessel Engineering is available for download below.

Interaction between multiple bodies can be defined as bonded, no interaction, or no penetration. A bonded condition forces the bodies to act as a single component. For example a head bonded to a shell would simulate a welded condition and solve the analysis as if the head and shell were a single component. A no interaction condition does not account for the interaction between multiple bodies; it allows the bodies to displace individually without any imposed restraints by the adjacent components. This condition could result in bodies interfering or overlapping each other. A no penetration condition allows multiple bodies to contact each other, but not to penetrate. This condition is useful when analyzing connections such as flanges, tri-clamps or split rings. No penetration conditions also provide contact pressure plots. These plots are useful to ensure joint separation does not occur.

Contact Pressure Plot

A contact pressure plot showing resulting contact pressure between bodies. This plot is useful to ensure joint separation does not occur.  the length and color of the arrows shows the contact pressure.

Restraints between multiple bodies such as bolts may also be simulated. Bolt connectors are defined in place of solid model bolts, and their material properties and preload defined. The solver creates beams to simulate bolting where bolt connectors have been defined, and transfers the applied preload to the connection accordingly. The software can then output the resulting forces acting on each connector which can then be used to calculate stresses.

Defining appropriate restraints and interactions between bodies is critical to obtain accurate FEA results. Applying incorrect interaction conditions between components will result in incorrect results. FEA results with the wrong interactions may be interpreted as acceptable and allow for unsafe designs.

Downloads:

Simplification of FEA by Symmetry

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

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.)

NozzlePro FEA

This vessel has a large nozzle located on the straight shell with large loads and moments specified by the customer. NozzlePRO has been used to generate the model, apply loads, calculate the resulting stresses and provide a pass/fail assessment. The NozzlePRO results are much more accurate than using WRC-107 methods. PRINT EXPAND SHRINK

NozzlePro FEA

File: PVE-1388 , Last Updated: June 16, 2010, By: LRB

Download this drawing and the calculation files below

This sample vessel is drawn using SolidWorks. We also offer drafting services using AutoCAD.

This vessel has a large nozzle located on the straight shell. The diameter of the nozzle requires Appendix 1-7 calculations. The nozzle also has large loads and moments specified by the customer. Nozzle PRO has been used to calculate the resulting stresses. The Nozzle PRO results are much more accurate than using WRC-107 methods.

Since this sample was made, ASME introduced new App 1-8 and 1-10 methods which can also be used to calculate area replacement in large nozzles.

Downloads:

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

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

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

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

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

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.

Opinion

In the balance, these provincial requirements leading up to and including the CSA-B51 Annex J have been beneficial to the Canadian pressure vessel industry, even creating interest beyond the Canadian market. Many have experienced the frustration of being shown a couple of FEA screen shots and being told that a product is good. This standard is a significant improvement that outlines some valuable practices.

The other side must be considered as well. The people who wrote the standards leading up to this one are not FEA practitioners, and it shows. A real FEA report must follow the practices of ASME VIII-2 Part 5 and PTB-3. For example, the stress plots asked for in B51 are pretty, but that is not how pressure vessels are correctly analysed. Other problems also exist. Before other markets use this standard, or one derived from it, This annex J should be upgraded to match current ASME requirements.

This standard also gets used as a check list for reviewers without pressure vessel FEA experience to approved or reject FEA reports for CRN acceptance, a practice I do not support. FEA is too complex to review with a simple check list.

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

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

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

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

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

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

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

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

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…