ESRD Benchmarks

Verifying the accuracy of FEA solutions is straightforward when employing the following Key Quality Checks.

In a recent ESRD webinar, we asked a simple but powerful question: if you routinely perform Numerical Simulation via finite element analysis (FEA), how do you verify the accuracy of your engineering simulations? During this webinar, we reviewed ‘The Four Key Quality Checks’ that should be performed for any detailed stress analysis as part of the solution verification process:

• Global Error: how fast is the estimated relative error in the energy norm reduced as the degrees of freedom (DOF) are increased? And, is the associated convergence rate indicative of a smooth solution?
• Deformed Shape: based on the boundary conditions and material properties, does the overall model deformation at a reasonable scale make sense? Are there any unreasonable displacements and/or rotations?
• Stress Fringes Continuity: are the unaveraged, unblended stress fringes smooth or are there noticeable “jumps” across element boundaries? Note: stress averaging should ALWAYS be off when performing detailed stress analysis. Significant stress jumps across element boundaries is an indication that the error of approximation is still high.
• Peak Stress Convergence: is the peak (most tensile or compressive) stress in your region of interest converging to a limit as the DOF are increased? OR is the peak stress diverging?

When the stress gradients are also of interest, there is an additional Key Quality Check that should be performed:

• Stress Gradient Overlays: when stress distributions are extracted across or through a feature containing the peak stress, are these gradients relatively unchanged with increasing DOF? Or are the stress distribution overlays dissimilar in shape?

In this S.A.F.E.R. Simulation blog, we’ll explore each of the above Key Quality Checks as well as additional best practices for verifying the accuracy of FEA solutions. To help us drive the conversation in a practical manner, we selected a widely available and well understood benchmark problem to model, solve and perform each Key Quality Check using ESRD’s flagship FEA software, StressCheck Professional.

Note: the following Key Quality Checks for FEA Solution Verification focus on results processing for linear and nonlinear detailed stress analyses applications. Webinars containing solution verification best practices have been previously presented for fracture mechanics applications, global-local analysis (co-hosted by Altair), and fastened connection and bolted joint analysis.

Benchmark Problem: Tension Bar of Circular Cross Section with Semi-Circular Groove

Benchmark problem for Key Quality Checks for FEA Solution Verification.

The benchmark problem for the following discussion focuses on accurately computing a very common stress concentration factor, the classical solution(s) of which may be found in myriad engineering handbook publications and used often by many practicing structural engineers: tension bar of circular cross section with a semi-circular groove.

Since the available literature supports numerous classical solutions, we will limit our coverage to three (3) of the most popular classical stress concentration factor approximation sources: Peterson, Shigley and Roark.

Classical Source #1: ‘Peterson’s Stress Concentration Factors’ (Pilkey)

Our first classical source comes from Section 2.5.2 and Chart 2.19 (‘Stress concentration factors K_tn for a tension bar of circular cross section with a U-shaped groove’) in ‘Peterson’s Stress Concentration Factors’, 2^nd Edition, by Walter D. Pilkey:

Courtesy ‘Stress Concentration Factors’, 2nd Edition (Pilkey).

Courtesy ‘Stress Concentration Factors’, 2nd Edition (Pilkey).

The curve marked ‘Semicircular’ will be used for the classical stress concentration factor approximation.

Note: as is documented in Section 2.5.2 above, Chart 2.19 is computed from the Neuber 3D case K_tn curve (Chart 2.18, see below) for a nominal Poisson’s ratio of 0.3:

Courtesy ‘Stress Concentration Factors’, 2nd Edition (Pilkey).

Pilkey notes in Section 1.4 (‘Stress Concentration as a Three-Dimensional Problem’) that the Poisson’s ratio will have an effect on the K_tn for cases such as the above.

Classical Source #2: ‘Shigley’s Mechanical Engineering Design’ (Budnyas & Nisbett)

Our second classical source comes from Figure A-15-13, Table A-15, in ‘Shigley’s Mechanical Engineering Design’, 9^th edition, by Richard G. Budnyas & J. Keith Nisbett:

Courtesy ‘Shigley’s Mechanical Engineering Design’, 9th edition (Budnyas & Nisbett).

Classical Source #3: ‘Roark’s Formulas for Stress and Strain’ (Young & Budynas)

Our third source comes from the equation in Table 17.1, ’15. U-notch in a circular shaft’, ‘Roark’s Formulas for Stress and Strain’, 7^th Edition, by Warren C. Young and Richard D. Budynas:

Courtesy Roark’s ‘Formulas for Stress and Strain’, 7th Edition (Young & Budynas).

We will use the equation for the semi-circular notch (h/r = 1) for the classical stress concentration factor approximation.

Classical Stress Concentration Factor Comparison:

For this benchmark case study, the dimensions and axial tension force were defined as following (in US Customary units):

• D = 9″
• d = 6″
• h = 1.5″
• r = 1.5″
• P = 10,000 lbf
• σ_nom = 4*P/π/d² = 354 psi
• r/d = 0.25
• D/d = 1.5
• h/r = 1.0

These values result in the following classical solutions for the stress concentration factor:

The above classical solutions are noted by the authors as approximations of the stress concentration factor, given the configuration of geometric and axial loading parameter values; the exact solution can be obtained by solving the 3D elasticity problem. An approximation to the solution of the elasticity problem can be obtained using the finite element method (e.g. via StressCheck Professional or another FEA implementation).

A reasonable goal of our benchmark case study is to determine which (if any) of the classical solutions best approximates this particular configuration.

Modeling Process: CAD + Automesh + BC’s + Material Properties

The solid geometry for the benchmark case study was constructed in StressCheck Professional using 3D solid modeling techniques, an automesh of 3665 curved tetrahedral elements was generated, and boundary conditions (axial loads, rigid body constraints) were applied:

Curved Tetrahedral Automesh (courtesy StressCheck Professional)

The linear elastic material properties selected for the benchmark case study are representative of a 2014-T6 aluminum extrusion (i.e. E = 10.9 Msi, v = 0.397).

Solution Process: Linear P-extension + Fixed Mesh

The model was analyzed in StressCheck Professional’s Linear solver via an hierarchic p-extension process, in which the orders of all elements on the fixed mesh were uniformly increased from 2^nd order (p=2) to 8^th order (p=8) for a total of seven (7) runs.

Note: before executing the solution, the mesh was converted to geometric (blended) mapping, which ensured the optimal representation of the geometric boundaries. This conversion was required for the solution order to exceed p=5, as by default StressCheck Professional’s tetrahedral elements are curved using 2^nd order functions (Isopar).

Since StressCheck Professional automatically stores all completed runs of increasing DOF for results processing, we can determine the minimum DOF for which the benchmark case study was well approximated for each Key Quality Check.

Note: it is not necessary to always increase the order of all elements to 8^th order, unless the mesh is a) generated manually and is a minimum mesh of high-aspect ratio elements, or b) a solution of exceedingly low discretization error in the data of interest is the goal (our reason). Many times a sufficiently refined mesh at a lower order (p<6) will achieve an acceptable discretization error for most practical engineering applications.

Results Extraction: Do We Pass Each Key Quality Check?

After the solution process completed, the estimated relative error in the energy norm (EREEN) was automatically reported as 0.01%, indicating no significant discretization errors but telling us very little about our data of interest, the stress concentration factor.

Then, how do we determine if we have an accurate enough FEA solution to approximate the stress concentration factor for the benchmark case study? Let’s go through each Key Quality Check to determine if our discretization is sufficient.

Key Quality Check #1: Global Error

Key Quality Check #1: Global Error (courtesy StressCheck Professional)

Studying how the global error (% Error column), as represented by EREEN, decreases with increasing DOF is our first ‘Key Quality Check’. This value is a measure of how well we are approximating the exact solution of the 3D elasticity problem in energy norm.

Additionally, a Convergence Rate of >1.0 is also a good indicator of the overall smoothness of the solution. Note: in problems with mathematical singularities, such as the simulation of cracks in fracture mechanics applications, the convergence rate is typically <1.0.

VERDICT: Pass

Key Quality Check #2: Deformed Shape

Key Quality Check #2: Deformed Shape (courtesy StressCheck Professional)

Since the benchmark case study was loaded axially under self-equilibrating loads of P=10,000 lbf, rigid body constraints were applied to three nodes at the leftmost side to cancel the six rigid body modes in 3D elasticity.

The deformed shape for the highest DOF run indicates the model is behaving as expected at a 2,000:1 deformed scale (red outlines are the undeformed configuration).

VERDICT: Pass

Key Quality Check #3: Stress Fringes Continuity

Key Quality Check #3: Stress Fringes Continuity (courtesy StressCheck Professional)

When assessing the stress fringes for quality, it is important to ensure that there are no significant “jumps” across element boundaries (edges/faces) in regions where the stresses are expected to be smooth, continuous and unperturbed. This assessment requires that the stresses be plotted without any averaging or blending features enabled.

The 1^st principal stress (S1) fringe continuity for the highest DOF run is quite smooth across element boundaries, with no significant “jumps” detected in the region of interest (root of the notch). The maximum 1^st principal stress value (S1_max) is computed as 619.3 psi.

However, we will need to verify that this value has converged to a limit (e.g. independent of DOF) before it is compared with the benchmark case study’s theoretical K_tn and σ_max.

VERDICT: Pass

Key Quality Check #4: Peak Stress Convergence

Key Quality Check #4: Peak Stress Convergence (courtesy StressCheck Professional)

For this benchmark case study, our data of interest was the peak stress at the root of the circumferential groove. Since StressCheck Professional automatically keeps all solutions for ‘deep dive’ results processing, it is very simple and easy to ‘check the stress’.

Selecting the StressCheck model’s curve which encircles the root of the groove, an extraction of maximum 1^st principal stress (S1_max) vs. each run of increasing DOF was performed. Even though we have a fairly refined mesh in the groove, note the large differences between the first three runs (p=2 to 4) and the final four runs (p=5 to 8). For this reason, it is simply not enough to have a “good mesh” or smooth stress fringes that pass the “eyeball norm”; the peak stress values must be rigorously proven to be independent of mesh and DOF.

It can be observed from the table that convergence in S1_max was achieved by the 4th or 5th run, with a converged value of S1_max = 619.3 psi. Here is a summary of how the classical stress concentration factor approximations K_tn rate for this particular configuration:

% Relative Difference = 100*(σ_{max –} S1_max)/S1_max

It appears that Peterson’s classical stress concentration factor approximation is most appropriate, with a relative difference of 1.75% when compared to the estimated exact solution from the numerical simulation.

Note: the S1_max convergence table confirms that it was not necessary to continue increasing the DOF by p-extension past the 5th run (p=6 in this particular case); we could have stopped the p-extension process once the error in the S1_max was sufficiently small for our purposes.

VERDICT: Pass

A Note on the Poisson’s Ratio Effect

Recalling the derivation of the Peterson K_tn, the value use in the benchmark case study assumed a v=0.3 for its approximation, while a v=0.397 as was used in StressCheck Professional. This highlights the importance of understanding the derivation and limitations of classical solutions.

If we “eyeball” Chart 2.18 for r/d = 0.25 and a v~0.4, we get a K_tn of ~1.78 (vs. K_tn~1.81 for v=0.3). We then multiply the Peterson K_tn by 1.78/1.81 to get an ‘adjusted’ Peterson K_tn ~1.75 for v=0.397. This results in a σ_max = 619.67, a difference of 0.06%.

That being said, it is always up to the engineer and management to determine an acceptable classical solution error in practical engineering applications.

Key Quality Check #5: Stress Gradient Overlays

Key Quality Check #5: Stress Gradient Overlays (courtesy StressCheck Professional)

As an additional Key Quality Check, we should ensure that the stresses nearby the location of peak stress are also well-represented and do not change much with increasing DOF. In StressCheck Professional we can dynamically extract the stresses across or through any feature, for any resolution and available solution, and overlay these stress gradients on the same chart for an assessment of quality.

The stress gradient extraction was performed across the groove for the final three runs (p=6 to 8), and the automatic stress gradient overlay showed that there was practically no difference between the point-wise values. Again, this proves that the 5th run (p=6) was sufficient for representing both the peak stress and the groove stress gradient.

Note: as for the stress fringe continuity check (Key Quality Check #3), it is important to perform this extraction without averaging features enabled.

VERDICT: Pass

In Summary…

Example of the democratization of classical engineering handbook methods via FEA-based digital engineering applications.

Solutions of typical structural details in 2D and 3D elasticity obtained by classical methods are approximations obtained using various techniques developed in the pre-computer age. This benchmark case study shows that in order to rank results obtained by classical methods, they have to be compared with the corresponding values obtained from the exact solution of the problem of elasticity. Alternatively, when the exact solution is not available, classical methods can be compared with the results from an approximate solution of the same problem of elasticity obtained by FEA.

It was also shown that strict solution verification procedures are required to provide evidence that the approximation error in the quantities of interests are much smaller than the difference observed among the results obtained by classical solutions, an essential technical requirement of Simulation Governance and any benchmarking-by-FEA process.

Finally, this example also highlights another important point: Classical engineering handbooks and design manuals are examples of democratization practiced in the pre-computer age. With the maturing of numerical simulation technology it is now possible to remove the manifold limitations of classical engineering solutions and provide parametric solutions for the problems engineers actually need to solve. This is the main goal of democratization.

There is a fundamentally important prerequisite, however: The exceptionally rare talents of engineer-scientists who populated conventional handbooks have to be democratized, that is, digitally mapped into the world of modern-day analysis.

The time has come for democratization to be reinvented.

BAMF running as an AFGROW plug-in (courtesy Mr. Josh Hodges/Hill Engineering, LLC)

On July 17, 2019 a joint webinar on the latest developments in FEA-based 3D crack growth simulation, titled “3D Crack Growth Simulation: Advancements & Applications”, was provided by ESRD’s Brent Lancaster, LexTech’s James Harter and Hill Engineering’s Joshua Hodges.

In this webinar, we detailed the latest technological advancements for accurate simulation of three-dimensional crack growth in metallic structures, with and without residual stresses, via coupled finite element analysis (FEA) and fatigue life computations. Additionally, the webinar expanded further on the DaDT analysis best practices presented in ESRD’s June 2017 webinar, titled “Durability and Damage Tolerance (DaDT) Analysis Best Practices“, and highlighted the importance of mitigating the errors of approximation associated with stress intensity factors (SIF’s) and if applicable, engineered residual stresses (e.g. cold-working).

Webinar attendees from a wide range of industries were treated to a demo of Hill Engineering’s Broad Application for Modeling Failure (BAMF) Sim App, which provides a robust integration between StressCheck’s high-fidelity DaDT/fracture solutions and AFGROW’s crack growth life prediction capabilities. The BAMF demonstration showed how to set up a parametric model for DaDT analysis via StressCheck and then, with limited user intervention, integrate with AFGROW and StressCheck via their respective COM API’s to perform an on-demand 3D crack growth simulation. It was very impressive demo, indeed!

View Webinar Recording

Click the button below to view the 3 part, 65-minute webinar recording (scroll to the bottom of the webinar landing page to find the videos):

View Webinar Slides

Click the button below to view the webinar slides (PowerPoint Show):

Additional Resources

During the webinar, we identified several relevant DaDT and/or crack growth simulation resources that may be of interest:

• “Analytical Modelling of Fatigue Crack Behaviour Under Representative Spectrum Loading in the F/A-18 A/B Y508 Wing Root Shear Tie”, Dr. Kevin Walker (DST Group)
• “Crack Aspect Ratio Investigation, Analytical Methods Subcommittee: Round Robin for Cx Holes”, Mr. Robert Pilarczyk (Hill Engineering, LLC)
• “Benchmarking Problems in Fatigue Crack Growth Analyses”, Mr. Robert Pilarczyk (Hill Engineering, LLC)
• “Numerical Simulation Series: Fracture Mechanics Parameters”, Dr. Ricardo Actis (ESRD)
• “Improving Global-Local Simulation Workflows for High-Fidelity Stress and Damage Tolerance Analysis”, Mr. Eric Buettmann & Mr. Gordon Lehman (ESRD)
• “Computation of SIFs for Cracks in Cold-Worked Holes”, Dr. Ricardo Actis & Mr. Matt Watkins (ESRD), Dr. Scott Prost-Domasky (AP/ES) and Mr. Joshua Hodges (USAF)
• “Crack Propagation Analysis Tool for 3D Crack Simulation: A Simulation App Case Study”, Mr. Matt Watkins (ESRD)
• The Contour Method for Measuring Residual Stresses (Hill Engineering, LLC)

Acknowledgments

As always, many thanks to our attendees for their interest and feedback! And, of course, thanks to LexTech and Hill Engineering for their time and contributions. We hope to collaborate on another webinar in the future!

ESRD has posed a new FEA challenge problem in the October 2018 issue of NAFEMS Benchmark Magazine. Can you show that you solved it with sufficient accuracy?

In the October 2018 issue of NAFEMS Benchmark magazine, ESRD Chairman Dr. Barna Szabó posed a new “FEA Puzzler”: Can you determine the progression in spring rate as a 3D coil spring is deformed and can you verify the accuracy of your solution?

Dr. Szabó has produced a converged solution for the spring rates in our high-fidelity FEA software StressCheck Professional, and is requesting solutions from the engineering community on how they tackled the problem.  He will publish his solution after the submission deadline of February 1st, 2019.

The problem posed in NAFEMS Benchmark magazine is as follows:

FEA Puzzler from NAFEMS Benchmark Magazine October 2018

You can download the geometry (in Parasolid or STEP format) from nafe.ms/puzzler. Do you think you have the “FEA Puzzler” solved? Submit your reply to challenge@nafems.org by February 1st, 2019.

Are you an ESRD customer? If you’d like some tips on how to solve the model in StressCheck Professional, feel free to contact us below:

Qualitative Deformation Contours for StressCheck’s Coil Spring Solution

In a recent S.A.F.E.R. Simulation post, we announced that ESRD Chairman Dr. Barna Szabó had posed a new “FEA Puzzler” in the October 2018 edition of NAFEMS Benchmark magazine. This challenge problem related to determining incremental spring rates for a coil spring under axial displacement AND demonstrating that the approximation errors are small via solution verification procedures.

As a refresher, the original NAFEMS FEA Puzzler description was as follows:

FEA Puzzler from NAFEMS Benchmark Magazine October 2018

As noted in a January 2019 LinkedIn post by Mr. David Quinn (Chief Marketing Officer at NAFEMS), the original deadline of February 1st, 2019 has been extended an additional four (4) months. From Mr. Quinn’s post:

Send your responses, in confidence, to Professor Szabó at challenge@nafems.org. Responses of sufficient merit will win an exclusive NAFEMS business card holder, and a summary of the responses will be published without attribution in a future issue of Benchmark.

The challenge will close on June 1st 2019 – best of luck!

So, there is still ample time to submit your solutions (along with proof of solution verification) to challenge@nafems.org. Feel free to use any FEA software tool, and make note of your modeling process and interpretation of results.

Need A Hint?

To help provide a nudge in the right direction, ESRD has recorded the following teaser video using its StressCheck Professional FEA software to show some of the model setup and results processing (no actual values, that would be cheating!):

Dr. Szabó and NAFEMS are very much looking forward to your submissions!

WATCH THIS WEBINAR

Part 1: Nuts & Bolts of StressCheck, Why Get StressCheck Training?

Part 2: Intro to StressCheck Training Course Preview, Self-Training Resources

Want to Set Up an Instructor-Led Training?

Click the below button to get a quote for an on-site, off-site or web-based training course:

WATCH THIS WEBINAR

Extraction of minimum principal stresses for the aircraft keel section case study. Digital Engineering case study results (bottom right) compared well with StressCheck’s live dynamic extractions (bottom left, images courtesy of Digital Engineering/ESRD).

Introductory Remarks

In recent years, Digital Engineering began publishing articles on practical engineering simulation case studies, walk-thrus and software overviews for a variety of FEA software tools. In each article, FETraining developer and NAFEMS FEA training instructor Tony Abbey selected a commercially-available FEA software tool to analyze a mechanical component under various loads and constraints, and provided commentary, tips, tricks and process workflow of how he arrived at the results. His goal for each article was to focus on general instruction and best practices for FEA rather than in the particular FEA tool used for solving the problem.

With the consent of Mr. Abbey, ESRD selected four (4) case studies from his list of Digital Engineering simulation articles and were provided the geometric description, material properties and boundary conditions to solve these problems in StressCheck Professional.

For comparative and instructional purposes, ESRD then recorded and published video demonstrations of the modeling, solution and live dynamic results extractions of each case study to our Resource Library.

Note: while these were not “blind” case studies (the Digital Engineering case study results were known in advance), the video demonstrations show the unaltered, associated StressCheck process workflow, with solution verification provided for each result to ensure that the approximation error is sufficiently small.

Case Studies in Detailed Stress Analysis

Case Study #1: “Stress in Finite Element Analysis”, Digital Engineering May 2016

Cross brace structure showing constraint and loading set up (image courtesy of Digital Engineering).

In this particular case study, Mr. Abbey’s focus was to examine detailed cross-sectional stresses for a 3D solid cross brace geometry under off-axis loading. This involved defining multiple “zones” for extracting stresses, for a multitude of stress components and local system directions:

Zones of interest A through E and the SX stress distribution (image courtesy of Digital Engineering).

The following video demonstrates how StressCheck was used to reproduce the 3D detailed cross brace analysis and how cross-sectional lines were added after the solution for mesh-independent, curve-based stress gradient extractions. It is shown that StressCheck’s live, dynamic extractions compared favorably with Digital Engineering’s zone-based detailed stress results:

Case Study #2: “Dealing with Stress Concentrations and Singularities”, May 2017

Geometry and mesh of filleted model (image courtesy of Digital Engineering).

For this case study, Mr. Abbey discussed the influence of stress singularities on the FEA solution, and why it is important to model radii and fillets in regions of interest for more accurate stresses if a subsequent fatigue analysis is the goal. He studied the convergence of the stresses in a shoulder fillet geometry by increasing the mesh refinement until the difference in his results was small:

Stress distributions for the filleted model (image courtesy of Digital Engineering).

The following video demonstrates how the 3D shoulder fillet detailed stress analysis was performed in StressCheck, including the steps required to show convergence in the peak stresses. The results were nearly identical with Digital Engineering’s computed peak stress of 65.6 ksi:

Case Study #3: “Siemens FEMAP with NX NASTRAN Overview”, March 2018

Initial imported geometry and cut-out region (image courtesy of Digital Engineering).

For this case study, Mr. Abbey utilized Siemens FEMAP with NX NASTRAN to model and solve a 3D solid tie rod under axial loading. He also recorded videos for how to perform the pre-processing, solution and post-processing and deployed them on his website, FETraining.net.

Below are the von Mises stress contours from the NX NASTRAN results, with an unaveraged peak von Mises stress of ~43.6 ksi:

von Mises stresses (image courtesy of Digital Engineering).

The following video demonstrates how the full 3D tie rod geometry is imported into StressCheck, modified to remove all solid material outside of the cut-out region, automeshed with curved tetra elements, assigned the appropriate boundary conditions and solved with a p-extension process to increase degrees of freedom (DOF) on the fixed mesh.

Then, the converged peak von Mises stress was computed from the hierarchic sequence of linear solutions via a live dynamic extraction request and was observed to compare closely to Digital Engineering’s refined mesh NX NASTRAN result:

Case Study #4: “SOLIDWORKS Simulation Overview”, July 2018

Applied loads and boundary conditions (image courtesy of Tony Abbey/Digital Engineering).

For this case study, Mr. Abbey utilized SOLIDWORKS from Dassault Systèmes to analyze a 3D solid aircraft keel section, in which several load cases (vertical and lateral loads) were applied to the structure’s attachment points via sinusoidal bearing distributions. From Mr. Abbey about the origin of this aircraft keel section structure:

The keel section is on the lower centerline of a combat aircraft fuselage. It transmits undercarriage loads into the fuselage. It also provides a load path through the lower fuselage section in overall bending and torsion loading due to maneuvers. The geometry has been created in SOLIDWORKS. Many of the smaller fillet radii have been defeatured in preparation.

Of interest were the peak von Mises stresses and minimum principal stresses in the left-hand end upper fillet radii (38.46 ksi and ~-37.5 ksi, respectively):

Von Mises stress distribution in the left-hand end upper fillet regions (image courtesy of Digital Engineering).

Minimum principal stress, P3, plotted around the left-hand end upper fillet (image courtesy of Digital Engineering).

The following video demonstrates how the 3D solid aircraft keel section was imported in StressCheck as a Parasolid and analyzed for detailed stresses in the left-hand end upper fillet regions for the vertical/lateral load cases and end abuttment/bolt radial constraints. The end abuttments were represented by symmetry constraints, and the bolt radial by stiff normal springs. The vertical and lateral load cases would be represented by sinusoidal bearing load distributions applied to the lug holes.

Again, the solution was obtained by increasing the polynomial order of the approximation functions on the fixed mesh, and the solutions for each load case were available for live dynamic processing.

It can be observed that the peak von Mises stress in the left-hand end upper fillet radii converges tightly to a value similar to that produced in Digital Engineering’s results, and the live dynamic principal stress gradient extractions were also quite similar in nature to those produced by Mr. Abbey in SOLIDWORKS probes:

Case Study Summary and a Note on Benchmarking

Many thanks to Mr. Abbey, FETraining.net and Digital Engineering for providing the model files to ESRD. The outcome of these case studies reinforce that only with careful engineering analysis methodologies, appropriate modeling assumptions, and tight control of approximation errors is meaningful to perform comparisons of stress results produced by different analysts using different FEA software tools.

Also, as we highlighted in the above case studies, the practice of solution verification is especially important for any benchmarking, round-robin or other comparisons involving the computation of the results of interest by numerical means for a well-defined mathematical problem. Reporting results without objective measures of the size of the approximation errors does not meet the technical requirements of Simulation Governance.

Finally, if you are interested in results of published benchmark problems solved with StressCheck, check out our solutions to the Standard NAFEMS Benchmarks:

The Standard NAFEMS Benchmarks: Linear Elastic Tests

ESRD is pleased to announce a new webinar, scheduled for April 22, 2021 @ 11:00 am EST. This webinar, hosted by ESRD partner Revolution in Simulation and titled “Simulation Governance Is Critical for Reliable Condition-Based (Predictive) Maintenance“, will present a case study in which the goal was the development of a mathematical model for supporting condition-based maintenance (CBM) decisions.

The model was designed for estimating the remaining fatigue service life of high-value mechanical components, given their service history and that specific flaws (such as corrosion defects) have been discovered in them, thus enabling CBM to move damaged component removals from unscheduled to scheduled maintenance action.

The presenters will be ESRD Chairman Dr. Barna Szabó, and ESRD President & CEO Dr. Ricardo Actis.

We look forward to your attendance!

StressCheck Result for NAFEMS LE1: Plane Stress – Elliptic Membrane

To compliment and bolster our recent S.A.F.E.R. Simulation articles, and to provide the engineering analysis community quantifiable insight into the performance of our Numerical Simulation technology, verified StressCheck results for “The Standard NAFEMS Benchmarks” are now available for download in our Resource Library.

In the first volume of the StressCheck Benchmarks Guide, we focused on solving the Linear Elastic Test benchmarks referenced in “The Standard NAFEMS Benchmarks”, Rev. 3, October 1990.  In accordance with Simulation Governance rules, we ensured the benchmark’s target extraction converged before reporting our results or comparing with the NAFEMS benchmark reference.

You can download the first volume here:

About Our Results

• ESRD defines a “Minimum Mesh” as the least-refined mesh required to achieve numerical convergence within 1% of the target extraction, and “Dense Mesh” as an overly-refined mesh relative to the “Minimum Mesh” to demonstrate that adding more elements produced insignificant changes in the target extraction.
• The discretization error was reported to be < 1% for all StressCheck results in all benchmark models.  This means that the results no longer changed significantly as the degrees of freedom were increased, thus providing solution verification in our results.
• The StressCheck results and the NAFEMS reference benchmark solutions differed by < 3% for all benchmarks.  Differences in results were justified in the notes for each problem.

Benchmark Suggestions/References?

Do you have a benchmark challenge for ESRD?  If you can provide a reference, and it is within our current capabilities, we will be happy to consider it for future publication!