More FEA Samples

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 LINK

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.


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 LINK

Linear Multi-Body Analysis

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


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.


Reversed Dished Head

This 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. PRINT EXPAND SHRINK LINK

Reversed Dished Head

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

The Problem:

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.


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 LINK

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.


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 or 819-627-4387.

Thermal Analysis

FEA can calculate temperature profiles in single and multi-part models. From this displacements and stresses are obtained. Here FEA is used to determine heat time and required power for an injection mold. PRINT EXPAND SHRINK LINK

Thermal Analysis

File: File:PVE-4437, Last Updated: Aug 23 2010, By: BTV

Transient and Steady State Analyses

Transient and Steady State Analyses

Heat entering a part in a mold cavity

Thermal analyses are used to study thermal loadings and their resulting temperatures, heat transfer rates, displacements and stresses. These analyses are broken into two main types, steady state and transient. Steady state analysis will determine the energy balanced state at an infinite period in time without any detail on what happens while progressing to this point. Transient thermal analysis is able to analyze the heat flow through a body on a step by step basis allowing temperature effects to be observed over time.

Steady State Analysis

Steady state analysis is used to observe the effects of thermal loadings once the object in question has reached a constant, or steady state. This is useful to determine sustained temperatures, heat transfer rates, displacements and stresses. Steady state analysis is also useful to determine thermal loads and material properties to obtain a final desired result. As a steady state analysis only provides a final continuous result it only requires a single computation making it a very efficient solver.

Transient Analysis

Transient Temperature Graph

Temperature vs time for various locations in the cavity

A transient analysis is used to observe the effects of thermal loadings over time. It allows the user to view the changing temperature gradient through a component from initial though to a steady state condition. Transient thermal impacts are important to analyze as thermal loadings may result in peak stresses prior to reaching a steady state. It is also useful to answer questions such as how long will a component take to reach a desired temperature. As a transient analysis provides solutions for a defined number of time steps many computations are required resulting in a much more complex analysis.


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.