SolidWorks Simulation Validation

Validation of SolidWorks Flow Simulation CFD software

Validation is a vital method for knowing the strengths and weaknesses of Computational Fluid Dynamics (CFD) software.  Without it you will not know when the program is producing good results, or when it is producing results that need additional analysis before use.  Three CFD validation sets follow: First, a flat plate heat transfer simulation produced final and accurate results very fast. Second, a pressure drop through a straight pipe study produced results that converged to an approximate finish point very slowly and could not reach an ultimate calculated value.  Different methods are required for heat transfer and pressure drop.

Finally, the comparison of pressure drops in two 180° elbows shows a method to overcome the limitations of pressure drop convergence. The relative difference between two designs is studied instead of looking for absolute pressure drops which are never reached.  As with the heat transfer study, useful results are obtained, but this time more work is involved.

Validation Example – Flat Plate Heat Transfer

Our validation run of SolidWorks Flow Simulation sample #10 - "Flow Over a Heated Plate". How much computer resources are required to obtain a good result? PRINT EXPAND SHRINK

Validation Example – Flat Plate Heat Transfer

File PVE-11617 – LRB, CBM – May 11 2017

Heat transfer between fluids and the pressurized equipment that contains it is of interest to our customers. We use SolidWorks Flow Simulation which can solve many flow problems including heat transfer.  Flow Simulation ships with validation samples including #10 “Flow Over a Heated Plate”.   SolidWorks compares their results against published data.  Our interest is to learn how much computing resources are required to get a good result? Is it practical to use flow simulation to solve heat transfer problems?

SolidWorks Flow Simulation validation problem #10 “Flow Over a Heated Plate

Validation Example #10 is a simple 2D study of flow of air over a heated flat plate.  1 atmosphere air at 293.2 K (20 C) and inlet velocity of 1.5 m/s passes over a plate 0.31 m long. The plate is heated to maintain its temperature at 303.2 K, 10 K warmer than the inlet air temperature. The boundary layer starts at the leading edge of the heated plate. How does the heat transfer rate vary along the length of the plate?

The developed boundary layer for this problem. Fluid temperature is shown in solid colors, pressure drop by white isobars.

This is the results we got at mesh #5, the final mesh used in this study.  The development of the boundary layer from zero thickness at the left end of the plate can be seen from the temperature plot.  The pressure drop is also plotted with white isobars.  The temperature profile makes sense.

Results obtained by SolidWorks. Case 1- the flow simulation results (blue line) closely match the published results (red line)

SolidWorks found a close match between the published results and the heat transfer rate calculated by Flow Simulation.  

How much computer resources are required to get good results?  We started with a very coarse initial mesh (mesh #1 below) and programmed Flow Simulation in a four step process:

  1. Solve the flow problem with the mesh given and save the results.
  2. Determine which cells have converged and which need refinement (non-converged)
  3. Divide each non-converged cell into 4 smaller identical cells.  
  4. Do not change the cells that have converged.  Repeat step #1 ten times.

This was run on a medium power computer: i7 6600U CPU @ 2.6-2.81 GHz (2 physical cores, 4 hyper threaded cores),  16 GB ram.   Very little ram was used in the study.

Average heat transfer rate by iteration. “*” marks when the mesh was refined by dividing cells. At mesh 5 complete convergence is obtained and the mesh has finished refining.

Flow Simulation repeated the above four step process ten times.  By mesh #5 all cells were converged.  The remaining five iterations resulted in no new mesh, the process was complete.  Total time 111 seconds.

Auto-generated meshes produced by this study

  • Mesh #1 – All cells are identical in a 8×2 Gird (16 cells, iteration 45, 6 seconds).  All cells are non-converged, all are divided into 4 identical cells to create mesh #2.
  • Mesh #2 – All cells are identical, mesh size is  16×4 (64 cells, iteration 146, 16 seconds).  Some cells at the top have reached convergence and will not be divided again, others near or at the heated plate need to be divided.
  • Mesh #3 – First mesh with different cell sizes (576 cells, iteration 228, 26 seconds).  The light blue cells have reached convergence and will not be divided more.  Some green cells in the middle have also reached convergence. The cells next to the heated plate need to be further divided.
  • Mesh #4 – The mesh now has 3 different cell sizes (2340 cells, iteration 311, 39 seconds).  The blue, green and some yellow cells are fully converged and will not be further divided.  Again some of the cells next to the heated plate will be divided.
  • Mesh #5 – The final mesh (9396 cells, iteration 450, 90 seconds).  All the cells have reached convergence.  Although the program has five more iterations, no further cell division happens.

Heat transfer along plate vs mesh

How fast does the heat transfer rate converge?  Although the program continued refining the mesh until mesh 5 (90 seconds), the results had practically converged by step 3 at 39 seconds.  However the additional runs producing the same results proved that convergence had been reached.  This is fast convergence.  Flow simulation provided good results even with a coarse mesh.  This makes it practical to use flow simulation on available computers to solve heat transfer problems.


Pressure Drop in a Straight Pipe

Flow induced pressure drop in a straight pipe is well studied making it a good subject for CFD validation. Here SolidWorks Flow Simulation results are compared with theory, with emphasis on the required computer resources. PRINT EXPAND SHRINK

Pressure Drop in a Straight Pipe

PVE-11633 and 7479 / LRB and CBM /May 18 2017

Flow induced pressure drop in a straight pipe is well studied making it a good subject for validating the results from SolidWorks Flow Simulation (called Flow Simulation in this article) a Computational Fluid Dynamics (CFD) program.  

The validation case is a straight pipe 0.01905 m (0.75″) inside diameter, 0.009525 m radius (0.375″) by 0.18796 m long (7.40″) has 293.2 K (20 C 68°F),  water flowing through it at  an average velocity of 1 m/s (3.281 ft/s). The pipe wall is assumed to be perfectly smooth.  Inlet flow condition is assumed to be fully developed.  The outlet static pressure is set to 101,325 Pa (1 atmosphere).  Calculate the average pressure drop from inlet to outlet.

Figure 1: The straight pipe used for this validation case.  The CFD is simplified to a quarter model using symmetry in two planes.


Straight pipe pressure drop calculators based on textbook methods are available . Here “Pressure Drop Online-Calculator” is used (

Figure 2: Using textbook methods, a pressure drop of 1.29 mbar or 129 Pa is predicted

The predicted pressure drop is 1.29 mbar or 129 Pa.

Flow Simulation

The validation case was modeled in SolidWorks and solved in Flow Simulation.  Symmetry in both the XZ and YZ planes was used to reduce the mesh complexity by four.  Initially a very coarse mesh was used.  Our standard four step iterative mesh refinement process was programmed into Flow Simulation:

  1. Solve the 3D flow problem with the given mesh and save the results.
  2. Determine which cells have converged and which need refinement (non-converged)
  3. Divide each non-converged solid cell into 8 smaller cells.  
  4. Do not divide the cells that have converged.  Repeat step #1 ten times.

This was run on our most powerful computer: i7 6850U CPU @ 3.6 GHz (6 physical cores, 12 hyper threaded cores),  128 GB ram. Processing was stopped by the operator after 16 hours when mesh 7 reached convergence.  The three remaining meshes were not run because all available computer resources had been used.  A final converged result had not been reached.

Flow Simulation Results:

Mesh Iteration Cells Time Drop (Pa) Error Comment
1 53 576 2 s 77.6 -39.8% One mesh size only – all cells need refining
2 83 4,224 5 s 118.5 -8.1% One mesh size only – all cells need refining
3 131 30,822 22 s 133.1 3.2% Two mesh sizes – central channel cells do not need further refining
4 220 176,759 3 min 144.8 12.2% Three mesh sizes – further separation of coarse and fine areas – 
5 347 662,364 20 min 141.6 9.8% Four mesh sizes – first boundary layer refinement
6 520 2,669,733 2 hrs 130.2 0.9% Five mesh sizes – two level boundary layer
7 763 14,275,278 16 hrs 126.2 -2.2% Six mesh sizes – three level boundary layer
             *program stopped
Theory       129   Calculated by “Pressure Drop Online-Calculator”

Chart 1:

The meshes saved at iteration steps in Chart 1 can be seen in Figure 4.  The average pressure drop is measured from the last iteration as indicated for each mesh size.  Percent error is calculated as (Drop/Theory-1)x100%.

Figure 3: Pressure drop vs iteration. Pressure drop at the final iteration for each mesh is shown in Chart 1.  Meshes highlighted are shown in Figure 4.  Theoretical pressure drop (blue line) is included for reference.  An ultimate answer has not been obtained.

The theoretical pressure drop closely matched the Flow Simulation pressure drop for mesh 6 and 7 at 0.9 and -2.2% error respectively.  

Figure 4: 7 details of meshes produced during the 16 hour run. Refer to mesh 1 for location of each detail the scale is the same for all except 7-closeup.  See figure 3 for the iterations where each mesh is used.

Mesh 1 is the original user created mesh that started the refinement process. Initially all cells are too coarse and all get divided (meshes 1 and 2 figure 4).  Mesh 3 is the first to present cells at the flow centerline that have reached convergence and remained undivided in all the remaining meshes.  In each further mesh, cells near the boundary layer reach convergence, but the cells at the wall do not reach convergence and continues to divide.  It is expected that if further meshes could be computed, they would have further divided cells at the wall.

Boundary conditions.

Figure 5:  Flow velocity probe locations.  Inlet and A are 1 pipe diameter (0.01905 m or 0.75″) apart.  Same for A to B, B to C and C to D.  The red box is the location of the mesh details shown in figure 4.

The velocity of the flow is measured at the inlet, four locations each separated by 1 pipe diameter, and the outlet. At each location, the velocity is measured from the outer edge to the flow centerline.  

Figure 6: Velocity distributions, wall to the left, flow centerline to the right.  All results are from iteration 763 (the final iteration of mesh 7, the final mesh used).

Velocity profiles for the inlet, locations A to D and the outlet.  Results are from the final iteration of the final mesh.  The inlet condition is set as “fully developed”, but the flow still takes some distance to develop.  See figure 6:  

  • Inlet – partially developed velocity distribution – this is the Flow Simulation built in fully developed flow distribution.
  • Location A – usable but not great – this is one pipe diameter away from the inlet.  Differences between the outlet and this location are most apparent at the center line.
  • Location B, C, D and outlet – these are good, but changes can be seen compared to the outlet even for location D.

By one pipe diameter, a usable boundary layer has developed. By two diameters, it is close enough to the outlet profile to not matter. This distance to develop a boundary layer in the pipe makes it more unlikely that the Flow Simulation result can exactly match the theoretical value without redesigning the experiment to account for this.

It is up to the user to determine if models being studied need to be modified to allow extra length for boundary layers to develop before areas of interest. 

Computational Limits

This validation study is a very simple shape – a small portion of a straight pipe further simplified through symmetry.   Unlike the heat transfer validation case, this pressure drop study is very slow to converge with no final pressure drop obtained.  The final meshes did produce results impressively within 0.9 and 2.2% of the theoretical answer.  However the computational resources used are extreme.  A more complex real world problem would have much more detail and complexity, requiring a much coarser mesh.  Taking the results as far as mesh 4 and mesh 5 would be more likely.  At these meshes the error rate is in the 12 and 10% range for this problem.

For real problems where Flow Simulation would be used no theoretical comparisons are available.  Further, each problem has its own convergence pattern (compare with the convergence plots for the flat plate and the elbows on this page).  For these real pressure drop problems the operator will be faced with results that are not converged, and with no theoretical results to provide a bounds on the amount of error.  This seems grim, but very useful results can be obtained using relative instead of absolute pressure drop information.  Please refer to the elbow study on this page for our way to get robust results.


Product Design by Comparative Pressure Drop

While it is difficult to calculate ultimate pressure drops in CFD, relative pressure drops between two related designs can be calculated leading to useful design insights allowing the best design to be chosen. PRINT EXPAND SHRINK

Product Design by Comparative Pressure Drop

PVE-11652 LRB / CBM – May 17 2017

The validation study on flow in a straight pipe ran into difficulty determining the ultimate pressure drop.  Each time the mesh was further refined, a new pressure drop was calculated.  A final answer was not calculated even for extreme mesh sizes run over an entire weekend.  An approximate answer was possible, but without assurances that it was the final answer.  How can this CFD tool be useful?

When the ultimate pressure drop is not the goal, a way forward is available.  In this exercise, two similar designs for 180° pipe elbows are compared.  We do not need the absolute pressure drop.  The goal is to find which has the lower pressure drop.  How easy is it to get this result?  And finally, can this method be used on more complex objects?

Figure 1: Two 180° flow elbows to be compared. Section view.  Which has the lower pressure drop?  “U” configuration on left, “LR” for larger radius on right.

Like the previous validation sets, an initial very coarse mesh is used.  Flow Simulation is set to refine the mesh where required until all areas convergence and no further mesh refinement is required.  Inlet velocity to both elbows is 1 m/s water at 293.2 K and 1 atmosphere.  Half symmetry on the XZ plane isused to reduce the complexity of the model.  Flow Simulation was set to monitor the pressure drop across both elbows, and compute the ratio of the pressure drop in the “U” design to that of the “LR” design (LR/U – numbers greater than 1 indicate that the pressure drop is larger in the LR case).  

The inside flow passage diameter for both elbows is 0.019 m (0.75″).  Both have a leg to leg spacing of 0.0508 m (2″).  The bend radius of the U design is 0.0254 m (1″)  with a 0.0369 m (1.45″) inlet section and a 0.1511 m (5.95″) outlet straight pipe section to allow flow to develop before and after the elbow.  The LR design has a larger bend radius of 0.0285 m (1.125″) and the inlet and outlets are reduced in length to allow for a 0.019 m (0.75″) long flow offset section.  

The initial coarse mesh (fig 1) was solved by Flow Simulation over 240 steps over which time the pressure drop ratio reached a rough convergence.  As the convergence was too rough to allow automatic refinement, the iteration for refinement was chosen by the operator during the run.  Total run time was 3 hours on a medium power computer: i7 6600U CPU @ 2.6-2.81 GHz (2 physical cores, 4 hyper threaded cores),  16 GB ram (14 GB used).

Figure 2: Initial mesh used. Results are not expected to be useful, but the program uses the results from each mesh size to determine where more refinement is required in the next mesh.

Figure 3: Final mesh (#6) detail for “LR” elbow. many areas of the mesh have reached convergence and their final mesh size, areas of turbulence and the boundary layer are still being refined (darkest areas with the smallest cells).

Figure 4: Midplane velocity profiles for the final mesh size.  The flow pattern is not simple, and the “LR” elbow (right) has a more complex pattern than the “U” elbow (left).

Figure 5: Complex flow patterns around the elbows.  This is from the final mesh size (mesh 6).

Figure 6: Pressure drop for the “U” elbow (green) and “LR” (red). The pressure drop graphs did not reach convergence before the run was stopped.  However, the results are still useful.  Refinement points are shown as “*”.

Figure 7: The ratio of the two pressure drops from figure 6. Useful and consistent information emerges that can be used to compare the two elbows.  The highlighted areas are the areas used for the averages.

From Figure 7 – mesh densities for 1 and 2 are too coarse to accurately capture the complexity of the flow going through the elbows and should be ignored.  Meshes densities 3 and 4 are typical of what is attainable in a practical flow problem.   These results are obtained after 6 minutes (362 s). Mesh sizes 5 and 6 are probably not attainable in real world problems more complicated than this simple flow example.   Taking the results from meshes 3 and 4, the “LR” elbow is expected to have a pressure drop about 7.6 to 7.8% higher than the “U” shaped elbow.

Although the pressure drop has not converged, it can clearly be seen that the “U” shaped elbow has a lower pressure loss. This calculation was easily within the reach of the medium powered computer used.




Validation of FEA Stresses in Pressurized Equipment

How do you know you are getting good pressure vessel FEA stress results?  Chapter 5 of the little known ASME Book “PTB-3 VIII-2 Example Problem Manual” provides worked sample FEA problems showing both the correct use of FEA rules, and the expected results. We use both SolidWork Simulation and Abaqus in house.  The first validation set gets the same results as ASME PTB-3 using both programs.  The second set compares SolidWorks Simulation to Roark’s type problems and again gets comparable results.

SolidWorks and ABAQUS Compared to ASME PTB-3

ASME problem sample manuals PTB-3 and PTB-4 are well kept secrets. PTB-3 contains worked VIII-2 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. PRINT EXPAND SHRINK

SolidWorks and ABAQUS Compared to ASME PTB-3

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

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. PRINT EXPAND SHRINK

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” compares the results obtained by SolidWorks Simulation to theoretical textbook values or prior FEA studies. Here are some of 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

We documented our complete run of the 2010 SolidWorks Simulation static analysis validation set. Our results can be Downloaded.  In all cases, our results matched those obtained by SolidWorks, and also matched the theoretical results.