SolidWorks Simulation Validation

How do you know you are getting the correct FEA results? ASME Book PTB-3 Chapter 5 provides worked sample problems that we have compared with our FEA methods and got the same results. SolidWorks Simulation ships with a general engineering validation problem set, again we got the same results.

Getting good results is also dependent on checking the reaction forces, using the correct element types and choosing regular or large displacement settings. Contact locations like under bolt heads always report large errors – sometimes adjusting your expectations is also important.

Perfect results are useless unless others can understand what you have done. The Canadian B51 standard Annex J has some presentation requirements that must be met for Canadian use. We also have suggestions on how to take presentation screen shots.

Quick Links (to topics on this page)

SolidWorks Simulation and ABAQUS Compared to ASME PTB-3

PVE File File: PVE-9128, June 9, 2015, By: CBM/BTV/LRB

What is PTB-3

ASME problem sample manuals PTB-3 and PTB-4 are well kept secrets.  The samples that used to be in the back of ASME VIII-1 in Appendix L have been changed, expanded and published as PTB-4.  The ASME VIII-2 rewritten in 2007 got its own new PTB-3 problem sample manual in 2010.  PTB-3 contains worked examples with numerical results.  Although meant more as an educational guide than a verification set, here we compare our own results in both ABAQUS and SolidWorks against published PTB-3 results.


The sample vessel design used in PTB-3 sample E5.2.1. All dimensions are in the corroded state. We ran this sample through Abaqus and SolidWorks Simulation.

PTB-3 Example E5.2.1 and E5.3.2

PTB-3 example E5.2.1 “Elastic Stress Analysis” covers the correct use of stress linearization and provides numerical results.  The same model is used for sample E5.3.2 “Elastic Analysis”.  Here both are run.

[From E5.2.1] Evaluate the vessel top head and shell region for compliance with respect to the elastic stress analysis criteria for plastic collapse provided in [VIII-2] paragraph 5.2.2. Do not include the standard flanges or NPS 6 piping in the assessment for compliance to allowable stresses. Internal pressure is the only load that is to be considered. Relevant design data and geometry are provided below and in Figures E5.2.1-1 and E5.2.1-2.

In other words analyse the head and a nozzle in the top of a pressure vessel to determine its acceptability against ASME code rules for FEA. The instructions for E5.3.2 are:

Evaluate the vessel top head and shell region given in Example Problem E5.2.1 for compliance with respect to the elastic and elastic-plastic local failure criteria provided in [VIII-2] paragraphs 5.3.2 and 5.3.3. The same model and material conditions were used as in Example Problem E5.2.1.


The pressure vessel head with nozzle as shown in PTB-3 sample E5.2.1 and also used for E5.3.2. The scope of analysis is limited to some of the shell, the head and the nozzle. The flange on the nozzle is modeled to allow loads to be applied, but is not included in the analysis.


This example provides enough dimensional and material information to attempt to duplicate the results.  Exactly matching the published results is not possible because not all not all model geometry is given and some linearization locations are not exactly provided.  The 2D 8 node ABAQUS element type CAX8R was provided, however mesh sizes were missing.  Where information exists, we replicated the PTB-3 exactly.  Where information is missing, we tried to get a model that looked similar to the one in the publication.  Given these limitations, we hoped for results that match PTB-3 with less than 5% error.

The scope of study in Examples E5.2.1 and E5.3.2 is the shell, head and nozzle.  These are symmetric about the centerline allowing a 2D axisymmetric analysis to be chosen by the authors.  This reduced the complexity of the analysis and allows a refined mesh to be used.  Most model dimensions were provided in drawings E5.2.1-1 and -2.  We re-created the 2D model geometry in SolidWorks.  Where model dimensions were not available, we made our model visually match the published drawing.  A link to a drawing of our model is provided in the resources section below.

We used the same model in both ABAQUS – the software used by the authors and SolidWorks Simulation (SWS).  We inferred the mesh size used by counting the number of elements in areas of known dimensions.  We used this size of 0.015″ in both programs.  The materials were modeled using the two different material moduli as outlined in PTB-3.  The exact location of the change in modulus was not given, so we chose SCL #4 as the transition.


PTB-3 figure E5.2.1-10. Location of Stress Classification Lines (SCL) 1 thorough 4.


PTB-3 figure E5.2.1-11. Location of SCL 5 thorough 9. The exact location is not provided for 5 and 9.

We split the model at Stress Classification Line (SCL) locations 1-9 as shown in the PTB-3 figures E5.2.1-10 and E5.2.1-11.  The exact location was not provided for SCL 5 and SCL 9.  We attempted to visually match the publication.  We used exactly same location in both SWS and ABAQUS even if we could not exactly match PTB-3.

SCL Methods

Two issues stand in the way of getting good SCL data.  1) taking a SCL at a bad location, and 2) setting up the tool poorly.  Getting good SCL locations is not always possible.  Our article “ASME VIII-2 Permissible Cycle Life” discusses what to do when a good SCL is not possible.  PTB-3 does not discuss the reason for the 9 SCL locations chosen.  VIII-2 Annex 5-A.3 discusses the selection of SCLs  Because we often encounter results from improperly configured SCL tools some detail is provided here.

The SCL starts with stress data taken from the model.  The data set is taken on a straight line from the inside to the outside of the model. The data is rotated from global (or model) coordinates to local.  When the SCL is on the X axis (like SCL #1 above) no rotation is required.  The local direction 1-1 is the direction of the SCL.  Stress in this direction is S11.  Likewise S22 is perpendicular to the line on the plane of the SCL.  S33 is perpendicular to the line out of plane.  S12 is the shear stress in the plane of study.  For 2D axisymmetric studies S13 and S23 are zero.


Rotation of the global to local stress components along the 11 axis of the SCL

The correct SCL components must be included to get the correct membrane and membrane + bending results in the SCL.  The default settings in most SCL tools will not work for pressure vessel studies.  The ABAQUS tool must be configured to include S11, S22, S33 and S12 (all the available data) in the membrane stress calculation.  Here we have also included the same S11, S22, S33 and S12 components in the bending calculation – however the bending result has no defined meaning in pressure vessel studies and is ignored.

The “Bending Components for Computing Invariants” is the calculation of the averaged difference in stress from one end of the line to the other. Only bending components are included in the invariant calculation.  For this 2D study stresses S11 in the direction of the SCL and shear stress S12 are not perpendicular to the SCL and can not create a stress bending the SCL.  Stresses S11 and S12 are removed from the invariants.


2D Axisymmetric SCL setup for ABAQUS

Going beyond this PTB-3 example, a 3D FEA study will have data points with 6 stress components: S11, S22, S33 and S12 as discussed above, with the addition of S13 and S23 (shear components not shown in the above diagram).  Of these two new components, S23 produces a torsion of the SCL and is included.  S13 is not perpendicular and is removed.


PTB-3 does not discuss convergence of results or quality of the mesh.  We used the Error plot built into SWS to determine if the model is adequately converged at the mesh size used.  Acceptable mesh errors in non discontinuity zones is 5%.  Discontinuity areas often have higher errors.  For this model the error is less than 1% except at SCL 1 at the base of the flange to nozzle weld discontinuity where it is an acceptable 5%. ABAQUS does not have an error plot so it was only run in SWS.

We obtained displacement and stress plots from both SWS and ABAQUS that substantially matched the results published in PTB-3.


Table 1 – Results obtained by PVEng using SolidWorks Simulation and ABAQUS vs published results from PTB-3

A comparison of our SCL results from SWS and ABAQUS vs PTB-3 is presented in Table 1.  Our results matched PTB-3 within 4% of full scale stresses.  Given the assumptions we had to make in modelling this comparison, we consider this to be a bulls eye.  Our SWS results matched our ABAQUS results within 0.4%. We split the model at the SCL locations to remove sampling location errors between the two programs.  Even so, we did not expect results this close, as this ABAQUS analysis is based on 4 sided elements with 8 nodes while SWS is based on 3 sided elements with 6 nodes.  However, the model is highly converged as shown in the SWS error plot so the closeness of the results should not have been surprising.

SWS and ABAQUS in daily use

We use SolidWorks Simulation and ABAQUS for a variety of design tasks in our office.  The programs have different characteristics that lead them to be suitable for different applications.  SWS is a much easier to use program, usually resulting in finished results in half the time, however it does not have built in linearization results that are compatible with ASME methods.  We wrote our own tool to get around this shortcoming.

ABAQUS allows a lot of control over the generated mesh vs SWS.  This extra control also requires more effort.  The ABAQUS quadralateral mesh is expected to be more accurate than the SWS triangular mesh, but for this overrefined example, the difference is turned out to be negligible. Without a doubt ABAQUS has the better results plots where screen updates happen much much faster than SWS’s leisurely pace.  And for non-linear analysis, ABAQUS provides results more often and is more stable than SWS.

Downloads the two reports for this validation exercise:  ABAQUS and SolidWorks Simulation.

SolidWorks Static Verification Problem Set

File: PVE-9729 Last Updated: Oct 14 / 2016, Cameron Moore, Ben Vanderloo, Laurence Brundrett

SolidWorks Simulation ships with a series of validation sets. The “SOLIDWORKS Simulation Static Verification Problems” compare the results obtained by SolidWorks Simulation to theoretical textbook values or prior FEA studies. Here are our results using the 2016 release of SolidWorks Simulation:

Simply Supported Rectangular Plate
A simply supported plate is first center point loaded and then uniformly loaded.
The plate is 1″ thick and 40″ on a side. Modulus of elasticity = 3 X 10^7 psi, Poisson’s ratio = 0.3.
Using symmetry restraints, only 1/4 of the plate is required. The outside edges are simply supported.
A mesh size of 1/2″ with thin plate elements produces a close match between theory and our FEA results. The image shows displacement.
Center Deflection
Center point load = 400 lbs
Center Deflection
Uniform Pressure = 1 psi
Theory 0.0027023 0.00378327
PVEng 0.0027046 0.0037855
%Error -0.0851% -0.0589%
Timoshenko, S. P. and Woinowsky-Krieger, “Theory of Plates and Shells,” McGraw-Hill Book Co., 2nd edition. pp. 120, 143, 1962.
Center point load: UY = (0.0116 * F * b2) / D
D = (E * h3) / (12* (1 – v2))
Uniform Pressure: UY = ( 0.00406 * q * b4) / D


Deflection of a Cantilever Beam
A cantilever beam is subjected to a concentrated load (F = 1 lb) at the free end. Determine the deflections at the free end and the average shear stress. Dimensions of the cantilever are: L = 10″, h = 1″, t = 0.1″.
Deflection at free edge, inch Average Shear Stress, psi
Theory 0.001333 10
PVEng 0.001341 9.9407
%Error -0.6002% 0.5930%
UY = (F*L3 ) / (3 * E * I )
Average shear stress: τxy ave = V / ( t * h)
L = Beam length
E = Modulus of Elasticity
I = Area moment of inertia
V = Shear force
t = Beam thickness
h = Beam height


Tip Displacements of a Circular Beam
A circular beam fixed at one end and free at the other end is subjected to a 200 lb force. Determine the deflections in the X, Y direction. Radius of curvature of the beam = 10″. The beam width and thickness are 4″ and 1″ respectively. This problem is solved using thin shell elements.
X Deflection at free edge, inch Y Deflection at free edge, inch
Theory 0.00712 0.01
PVEng 0.007137 0.009992
%Error -0.2388% 0.0800%
Warren C. Young, “Roark’s Formulas for Stress and Strain,” Sixth Edition, McGraw Hill Book Company, New York, 1989.
DX = ( 3/4 * π-2)* H R3 / (E *I) , DY = (1/2*H*R3 ) / ( E* I ), Modulus of elasticity = 3 X 107 psi

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.


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


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.


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?

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

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.

Half Bolt Connectors in SolidWorks Simulation

File: PVE-6438, Last Updated: Aug. 20, 2012, By: BTV

Design and analysis of flanges in SolidWorks simulation often requires the use of a half bolt connector. This feature is available from the “Connections” group in the simulation tree.

1. Start by creating a standard bolt connector, selecting the inside edges where the bolt will terminate.


2. Specified the bolt head diameter, shank diameter and the material.

3. Select the axial preload and enter the total bolt pre-load for a full bolt ignoring the fact that this is a 1/2 bolt.


4. Open the advance option and check the 1/2 symmetry option. Select a plane that indicates where symmetry is taken about. Do not select a face or bolt connector loads will not report for this connector. Certain geometry may require a plane to be created.


5. Export the bolt loads to a .csv file by right clicking the “Results” folder and selecting “List Pin/ Bolt/ Bearing Force”.

6. Open the .csv file and locate the 1/2 connectors (connector 1 for this example). The total applied preload is 100 lb. Note that the .csv export will show -50 lb axial force. Multiply all of these forces (Axial, Bending and Shear) by 2 before calculating bolt stresses. The von Mises bolt stress for this example should be equal for all bolts.


7. The deflections around the outside of the flange show that the bolt preloads applied create a uniform load. The full bolt connectors create the same deflection as the half bolt connectors.


The verification for 1/2 connector application can be seen in the deflection plot. The image below shows an incorrect method of applying a half connector. Note that the deflection is not radial around the outside of the flange. This indicates that the 1/2 connectors are not setup correctly.

HalfBolt_Image7When possible half connector should be avoided due to the affect they have on the global reaction forces. Half connectors often apply forces against the symmetry plane that cannot be accounted for. This prevents a user from checking that the applied loads equal the simulation resulting forces. These force do not have any adverse affects on the displacement or stress.

Error Plots – Bolt Heads and Surface to Surface Contacts

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


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.


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 [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

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 blue 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


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.


The model description shall include a list of all assumptions.


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.


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.


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.


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.


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.


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


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.


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.


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.

Setting Up Presentation Screen Shots for FEA Reports

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”. This report is based in part on these ABSA requirements and in part on our experience at Pressure Vessel Engineering Ltd.

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

Setting Up Presentation Screen Shots for FEA Reports

The ABSA FEA guideline has specific requirements for the Presentation of Results: The following figures must be presented (colored prints)

  • Displacements (plot);
  • Deformed shape with un-deformed shape superimposed;
  • Stress plot with mesh, that will :
    • Show discrete fringes – discrete color separation for stress ranges or plots
    • Allow comparison between the size of stress concentrations and the size of the mesh
  • Show plot with element stress and compare nodal (average) stress vs. element (non averaged) stress (if the [small] difference is less than 5%, the accuracy should be OK);
  • Compare reaction forces to applied loads;

When plots or figures have been presented, there must be [a]discussion relating to each and every figure to explain what is the purpose of the figure and why it is of importance.

Capture Size

FEA model screen shot

The starting point – a FEA screen shot with most Solidworks Simulation settings at default.

This image was captured using SnagIt at 952 x 540 pixels and shrunk by word to 60% of its original size to fit the page. The extra pixels provide good resolution for prints. Two images this size will fit on a page with space left over for captions. Have pity on the reader – do not try to fit more than 2 images on one page.

Background Color and Light Scheme

FEA model with straw yellow background.

The background color has been set.

Here the background color has been set to R-256, G-256, B-240. This is a light straw yellow that stands out slightly from a white page. The background color is set at Tools/Options/colors/Viewport background/Edit/custom colors .

Screen capture of colour menu.

Scene Selection pull down – Ambient Occlusion gives good readable lighting.



Deformation Scale

Example of deformation scale.

The deformation scale has been set to 150x – a rational number

A deformed model can make it easier to understand the stress results. However, it makes sense to choose a rational number. Here the scale has been set to 150x.

Edit Definitions - Before and After

Edit Definitions – Before and After

Stress / Deformation Display Scale

FEA model showing readable stress scale.

The stress scale is now more readable

The Show max option allows the legend to be rescaled to whole numbers (here 30,000 psi instead of 35,700 psi). Rescale the graph from 0 (or negative numbers when justified). Change to floating format, only show decimal points for small numbers like displacement graphs – scientific format numbers are harder to understand. Choose a logical number of colors so that the legend shows whole numbers – here 10 colors are used.

Screen shots of chart and display options.

Chart Options – Before and After

Displaced Model / Discrete Colors

Superimposed un-deformed model.

Here the superimposed un-deformed model has reduced the readability of the stress plot. The discrete color bands improve the readability – even on low quality printouts.

The superimposed plot makes more sense on a deformation plot then on a stress plot.

Screen capture of Settings

Settings – Before and After


Turn off unnecessary items like loads/restraints that have already been discussed.

Show at least one overall view and close-ups as required. Have pity on the reader who can not enlarge or spin your model on the printed page!

FEA Model overall view.

FEA Model close-up.