Creating NPT Connections for Piping Fittings
File: NA
Last Updated: May 7, 2007
LB
Background:
The best way to analyze NPT threaded piping fittings using FEA methods is with the pipe included in the analysis. Pressurizing the pipe transmits realistic stresses to the fitting body. Anchoring a pipe instead of the fitting produces much more realistic stresses and deflections.
 Manifold block with 2 attached pipes. |
 Section view |
Construction of the Pipes:
 NPT Hole put into a block with the SolidWorks hole wizard. |
 Reference geometry plane created through the center of the hole. |
|
 Edges of the hole "Converted Entities" (highlighted in magenta) used as the basis of a sketch. Use a pipe chart for the wall thickness. The outside diameter of the hole matches the outside diameter of the pipe. |
 Part is revolved but not merged. |
|
 Repeated for the other connection, only the pipe is capped. |
 All inside surfaces are pressurized. The end of the green pipe is anchored. The pipes and body are bonded. |
|
 Two commonly missed areas (magenta circles) these two surfaces are hidden, but must be pressurized to balance the fully pressurized face on the end of the pipes (blue circles). When all the internal areas are properly selected, the reaction forces will be correct. |
 CosmosDesigner stress plot showing greatly magnified displacement of all components. The pipes are long enough because there is an area along each pipe that is straight (magenta ovals). |
|
 Hiding the pipes allows the stresses and deflections for the body to be seen. |
Any attempt to anchor faces or edges on this model would alter the deformed shape and the stresses measured. This method of including the pipes is simple and realistic.
This analysis method does not include the effects of thread shear stress on the connections. This can be calculated using Machinery Handbook formulas.
Simplification of FEA by Symmetry
File: NA
Last Updated:
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.
 In many cases, the geometry of the part is symmetrical about one or more base planes. |
 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. |
|
 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. |
 How is this symmetry accounted for in the analysis? When running the FEA one of the constraints is symmetry about the model cut planes. |
|
 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). |
 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.)
Simplification of Multi-Body FEA Models
File: NA
Last Updated:
LB
 |
An analysis can become more complicated than it needs to be when the model is composed of multiple bodies interacting with each other. Simplifications discussed: 1) Symmetry 2) Bonding Bolt Heads 3) Mesh Control 4) Gasket Space 5) Classical Calcs |
 1) Symmetry - As with many analyses, the following valve by Stainless Valve Co can be simplified by cuts along the two planes of symmetry as shown. |
 2) Bonding Bolt Heads - In many cases, the interaction between components can be considered "bonded" instead of using sliding contracts, which reduces calculation time. For this example, the bolt heads were considered bonded to their mating surface. Artificial stresses are generated by the method of preload approximation, and these stresses should be neglected. (See Preload Article.) |
|
 3) Mesh Control - A smaller mesh size was only used in the areas requiring greater calculation refinements (bolts). This improves calculation time while maintaining accuracy. The weldneck flange and its bolts have a coarser mesh because they are covered by classical calculations, as noted in section 5 below. |
 4) Gasket Space - This model contains a gasketted flange, which has been approximated in the FEA by a representative space between the flange and plate. To simulate the flange loads, the Appendix-2 forces were applied to both the flange and the plate. Since the bolts are bonded to the outer surface of the flange, one continuous mesh was created. |
|
 5) Classical Calcs - The weldneck flange and its attachment bolts are covered by Appendix 2 calculations and do no require a detailed FEA analysis. They are included to simulate the interactions with the valve, but are hidden in this view for clarity. |
A special thanks to Stainless Valve Co. Stainless Valve Co.for allowing us to use the geometry of their Stargate O Port Valve for this exercise.
When will FEA be Required in a Submission?
File: NA
Last Updated:
LB
Finite Element Analysis (FEA) is required in a submission when code equations cannot be directly applied to the configuration and/or when additional reinforcement needs to be accounted for to obtain acceptable stress values.
Classical B31.3 pipe or shell calculations assume a thin uniform cross section. These calculations do not accurately predict the resultant stresses in this scenario.
When code adaptation calculations are performed for the following 24" butterfly valve, a shell-equivalent area is used to calculate the hoop stress.
 The equivalent area fulfills t<D/6 Req’t (304.1.2(a)). |
 Even though it satisfies the t<D/6 requirement, this equivalent area approach was rejected by the reviewer. FEA is the only alternative. |
|
 Due to symmetry, the entire valve can be analyzed by the quarter model shown in the figure. |
 A stress linearization was performed on two sections of the body resulting in membrane stresses of 1,129 and 789 PSI, and membrane + bending stresses of 1,449 and 1,034 PSI. |
|
 The maximum stress corresponds to a peak stress, as per Fig. 4-130.1 ASME VIII-2. A fatigue analysis yields infinite life cycles. (ASME VIII-2 Fig. 5-110.1.1) The stresses and corresponding cycle life were acceptable and Ultraflo obtained a CRN#. |
A special thanks to Ultraflo Corporation, #8 Trautman Ind. Dr. Ste. Genevieve, MO for allowing use of their valve geometry for this exercise.
FEA Submission Requirements
File: NA
Last Updated:
LB
Finite Element Analysis (FEA) can be used to support pressure equipment design where the configuration is not covered by the available rules in the ASME code.
ABSA Guidelines:
FEA Requirements Regarding the use of FEA to Support a Pressure Equipment Design Submission
We recommend that the designer check with ABSA whether the usage of FEA is acceptable, this must be clarified before the design is submitted.
ACI Central Inc Guidelines:
Finite Element Analysis Reaction Forces
File: NA
Last Updated:
BV
Summary
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.
Download:
Error Plots - Bolt Heads & Surface to Surface Contacts
File: PVE-3179
Last Updated: Dec. 13, 2008
LB
Summary:
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.
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.
Example:
 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. |
 A no penetration surface is defined between the two plates. The plates can separate but not pass through each other. |
|
 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. |
 Symmetry boundary conditions are applied to sides and bottom of assembled model. |
|
 The model is meshed at 1/8" size. |
 Close up of the interference mesh between the bolt and the top plate. |
|
 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. |
 A close-up of the contact area between the two plates. |
|
 Intensity stress plot (Tresca P1-P3 criteria) - the highest stress is indicated under the bolt head. |
 Close-up of the highest reported stress area - under the bolt head. |
|
 Overall error plot. The error plot shows areas in and around the bolt head to be higher than the 5% acceptance criteria. |
 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.
 Another area of high reported error: the contact between the top and bottom plates. |
 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. |
Setting Up Presentation Screen Shots for FEA Reports
File: NA
Last Updated: Oct. 20, 2008
LB
 |
This article supplements ABSA's (Alberta Boilers Safety Association) requirements on writing FEA reports: ABSA FEA Requirements. In particular refer to the section "Presentation of Results". |
Download:
COSMOS Validation Examples
File: NA
Last Updated:
LB
Summary
COSMOS has a number of validation problems built into the software. These problems are designed to prove the validity of its operation. Each problem provides an analytical and COSMOS generated solution for the problem.
Pressure Vessel Engineering validates each installation and update of the COSMOS software individually. The COSMOS validation problems are run in-house and results compared to the analytical solutions. All results are measured to be within 5% error or less of the COSMOS results.
Download:
COSMOS Validation Release
File: NA
Last Updated:
LB
 |
SummaryPressure Vessel Engineering Ltd. validates each release of Cosmos Designer with a simple validation set to confirm that the program produces results comparable to Roark's Formulas results. Roark's formulas provide the exact derivation of the stresses of components of different geometry under several loading conditions. These formulas can be compared with FEA results. The release form for the validation can be downloaded below. |
Download:
The Nuts and Bolts of Stress Linearization
File: NA
Last Updated:
LB
(With an Educational and Functional Stress Linearization Utility)
Summary
This article is a guide to how the stress linearization tool works to separate stresses into membrane and bending. Examples are provided along with sample data and a spreadsheet based stress linearization tool. The programming code is explained in the appendixes and can be examined in the spreadsheet.
This article does not discuss whether the stresses are local or global and which allowable stresses should be used for where. This is a topic for a later article.
Download:
Stress Classification Lines (SCL)
File: PVE-3277
Last Updated: Feb 2009
LB
SCL Passing Through Areas of Very High Error
Summary
Stresses at sharp corners rise towards infinity as the mesh size is reduced. However the forces have to balance in a Finite Element model regardless of the mesh size used. In these studies SCL (Stress Classification Line) results are compared a different mesh sizes. This report shows that it is possible to take stress classification lines through these areas of peak stress and get ultimate stresses - however the results will not be as expected.
Two studies are shown. In Study 1, the SCL passes between 2 sharp corners. The stress classification method produces results that do not vary as the mesh is refined. However, it misses the magnitude of the membrane and reports no bending stress. This is a limitation of the stress classification method.
In study 2, the SCL passes through only one sharp corner. This study shows results that converge to a finite value. Again, the reported membrane stress is less than expected.
It is best not to run an SCL through sharp corners (areas of very high error).
Download:
Large displacement solutions
File: PVE-4048
Last Updated: March 2010
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.
 A 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:
 A 0.1 psi vacuum is applied to create the focus by stretching the membrane |
 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.
 Linear theory - no membrane stresses are reported for the mirror. |
 Linear theory - huge bending stresses are reported. |
SolidWorks Simulation suggests using large displacement theory to solve the problem:
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.
 Large displacement theory deflection magnified 3x |
 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 is shown in the large displacement theory bending stress results. Bending stresses are almost zero except at the fixed edges. |
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.
Evil SolidWorks Factory Default Material Properties
File: PVE-4261
Last Updated: May 18, 2010
LB
Problem:
When a new object is created, SolidWorks specifies that the material is <not specified>. However, if the item is evaluated, it has a factory default material density of 0.04 lb/cuin (1000 kb/m^3) or the density of water. The appropriate material density would be "!Error - material density is not set!".
Example:
 The model - 1" x 1" x 1" cubes |
 A missing material property |
An array of cubes is modelled in SolidWorks - each 1" x 1" x 1". The material has been set to 304 stainless steel for all but one which was missed. The bottom faces of the cubes are fixed. Gravity = 386.22 in/sec^2 (1g) is applied.
One material property was missed in SolidWorks. Simulation will wisely not run until it is set. It can be set in two places - in Simulation, or in SolidWorks. Here it is set in Simulation to match the other items.
 Material set in Simulation |
 Resultant Force = 4.6259 lbs. |
Time for a quick check - the model is run with gravity only to verify that the correct weight is recorded on the fixed cube faces as a reaction force. A Default gravity for 1g acceleration = 386.22 in/s^2 is applied to all bodies. They are meshed at 1/4" size and run.
The resultant force in Simulation - the vertical (z) direction = 4.6259 lbf. A quick check back with the SolidWorks Mass Properties tool indicates a problem - the mass is 4.37 lbs vs 4.63 lbs calculated with Simulation. Where does this unacceptable 5.6% error come from?
 SolidWorks Mass = 4.37 lbs |
 Simulation Material properties did not make it back to SolidWorks |
The material for the one cube that was specified in Simulation did not make it back into SolidWorks. Further, SolidWorks did not declare an Error "Hey bud - you're trying to weigh an object with the material properties not set - cut it out". Instead, SolidWorks tried to make the user happy by assuming that all <not specified> materials should have the density of water and produced the wrong answer.
Suggestions:
If I could change the Material <not specified> density to 4 * 10 ^ 17 kg/m^3 - the density of a Neutron star - then it would be impossible to be fooled by the default material properties. "Oh yeah my vessel has the same mass as the Earth, I set the material properties in Simulation again!" SolidWorks has lots of factory default values - each one is a hidden error waiting to happen!
Changes made in Simulation do not (usually) show up back in SolidWorks. This is just like a part that is modified in an assembly does not show the changes back in the part file.
It is a good idea to set material properties in SolidWorks instead of Simulation.
Bloating SolidWorks Files
File: File:PVE-4482
Last Updated: Aug 18 2010
By: LB
This SolidWorks part for a weld neck flange has a design table with 132 different configurations in it. The configurations cover changes in size and rated pressure. When the file was first created it was 2,422 KB in size (2.4 MB). With use it has grown in size without any changes to the file.
 A standard flange |
 The design table has 132 configurations |
 A standard flange |
The original file was 2.4 Mb in size. Each time a different configuration is viewed, the file size expands when it is saved. When all 132 configurations have been viewed, the file has bloated to 68.5 MB. The file has to be saved, closed, re-opened and saved as (without viewing additional configurations) to get it back to the original 2.4 MB size. |
I have been told and I have no way of knowing if it is true, that SolidWorks stores the surface display information for each configuration viewed. If this is true, then the files would be made larger to prevent the requirement to re-generate the surface information when viewed. The save - close - re-open - save-as restores the original file size.