Reduce your Mesh Time
File: PVE-4061
Last Updated: Jan 1 2010
LB
Sometimes mesh times can be much longer than solve times. Why?
Inside view of a storage sphere |
Front view of the storage sphere. |
This 25ft diameter storage sphere with unusual legs is solid meshed. At a 5" element size (the largest size that will mesh), it takes 172 seconds to mesh. The bad news is that a smaller mesh is require in a number of locations. When the overall element sizeis reduced to 3", it takes 1002 seconds to mesh.
Front view - Nodes = 123,000, Elements = 61,000, 172 seconds to mesh |
Detail meshed at 3" size - Nodes = 318,000, Elements = 158,000, 1002 seconds to mesh |
The solution? Splitting large objects into smaller items can reduce the mesh time. Here the sphere is split into 6 and 12 pieces.
The sphere split into 6 bodies |
The sphere split into 12 bodies |
The mesh times go down significantly as the sphere is split into smaller bodies.
 6 body sphere at 5 inch mesh - mesh time is 46 seconds (127,000 nodes, 63,000 elements) |
12 body sphere at 3 inch mesh - mesh time is 161 seconds (326,000 nodes, 163,000 elements) |
Summary of all mesh time data. The reduced body size makes a huge difference as the number of elements increases.
Reducing the body sizes can have a huge impact as the number of elements exceeds 1 million...
Mesh Tolerance Settings
File: PVE-4048
Last Updated: FEb 17 2010
Laurence Brundrett
What impact does the mesh tolerance option have on the mesh?
Caution: every time the mesh size is changed, the tolerance is adjusted to 5% of the mesh size. This is a very nasty feature! Keep your eye on the tolerance and set it back the to value you require after each mesh size change
 |
External Features
As the mesh tolerance increases, exterior model details disappear from the mesh. This block is 5 x 5 x 1 inch high. Each feature is 1 x 1 inch. Feature height changes as shown.
 |
Cosmos can mesh the object with very coarse mesh sizes, as long as the tolerance is fine enough:
 Run #1, the mesh size is at 1 inch and the tolerance at the cosmos default 0.05 inch (5% of mesh size). When the tolerance is increased to or above the size of a feature, it disappears from the mesh. |
 Run #2, the mesh size is still at 1 inch, but the tolerance is increased to 0.125 inch (the height of the first feature). The first feature disappears. |
|
 Run #4, the tolerance is at 0.26 inch, the second feature disappears (the center of it still exists, but the edges are gone). |
 Run #8, the mesh size is 1.125 inch and the tolerance 1 inch, all features and much of the base disappears. The mesh does not have to be smaller than the feature size modeled. |
|
 Run #9, The mesh size is 2.5 inch, but the small features are still modeled because the tolerance is set to 0.05 inch. |
Internal Features
 Slightly different results are achieved with internal cut features. |
Here the extruded bosses are replaced with cut slots: 1, 0.5, 0.25 and 0.125" wide all the way through the same 5 x 5 x 1" block. When the tolerance is too coarse, the mesh fails:
Watch for this reason for mesh failure. If the cut features are not desired in the mesh, they have to be removed from the model.
Mesh Refinement
File: NA
Last Updated: Nov. 26, 2008
LB
Using the Error Function Results for Areas At Discontinuities
Summary:
Error plots show how well the complexity of a mesh matches the complexity of the model. Once the mesh matches the complexity of the model, the reported error is low. We use 5% error as an acceptance criterion. This method checks the whole model at once, and is much less work than mesh refinement.
This study compares mesh refinement at a node with error plot methods to estimate the convergence of FEA results. CosmosDesigner 2708 SP5.0 FEA software is used for this report.
Example: Shell Element Error Plots
Test shape - a simple flat plate modeled at 1/4" thickness. 3 test points (1, 2, 3) are shown on this model. A split line has been added to guarantee a node will always be available at point 2 to sample. For this sample, the stress at the three points is of interest, so the error at those points has to be less than 5% per the acceptance criteria.
Applied loads - 2 x 500 psi at the left edge. The right edge is fixed. The shell model is meshed at 1/4" thick.
1" mesh size. The reported error in the area of interest is greater than 5%. The results can not be used.
Similarly, mesh sizes of 0.75", 0.5", 0.375", 0.25" and 0.1875" all report error greater than 5%. 1/8" mesh size is the first size to produce acceptable results (below). (All are scaled 0 to 5% error.)
1/8" mesh size - coarsest mesh to produce an acceptable error plot for the 3 areas of interest.
The overall stress pattern for the 1/8" mesh size - Tresca stress intensity (P1-P3).
Close up stress plot of the 3 nodes of interest. The Tresca stresses at the test locations: 1 - 22.2 psi, 2 - 674.7 psi, 3 - 941.0 psi. How accurate are these stress values?
Stress results and stress results graph. For this study, the results from 0.125 and 0.063" mesh size meet the 5% acceptance criteria.
An ultimate stress value is extrapolated using linear regression on the above stresses and extrapolating to a theoretical zero mesh size (the 1" mesh size data point for stress 1 is ignored).
In general, when the reported error is less than the 5% acceptance criteria, the actual error is much less. Even when the acceptance criteria is met, some elements will have higher error levels (Point 1 at 0.063" mesh).
Mesh Refinement vs Error Plots
Mesh refinement by measuring the stress at individual locations and extrapolating to a theoretical zero mesh size can be used to validate individual areas on a model. However, many FEA runs are required, and in this case, only 3 points on the model were proven. There is no guarantee that the most important points have been studied. The Error plots prove every element in the model. If the first mesh chosen is acceptable, no additional work is required to prove the model.
Mesh Refinements Near Discontinuities
File: NA
Last Updated:
LB
Summary
Error plots show how well the complexity of a mesh matches the complexity of the model. Once the mesh matches the complexity of the model, the reported error is low. As a guideline, Pressure Vessel Engineering uses 5% error as an acceptance criterion.
This report examines the accuracy of stress results near an area of discontinuity as the mesh is refined. The 5% error criteria estimates the errors in the mesh except in areas of very low stress located near high stress areas. These areas are not usually of interest in a pressure vessel study.
Download:
Why Use 2nd Order Integration Elements?
File: NA
Last Updated:
LB
 |
SummaryThis 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 CosmosWorks for Finite Element Analysis. It is expected that these results would also be applicable to other FEA programs. |
Download:
Surface Model Mesh Challenges
File: PVE-4048
Last Updated: Feb. 24, 2010
LB
Surface models can be challenging to mesh. Parts that touch might not share nodes preventing the correct transfer of loads. The resulting calculated stresses and displacements can be wrong.
 A segment of the bottom half of storage sphere - here 1/2 of 1 leg is being analyzed. |
 The sphere and legs are shell modeled. |
The stresses in this leg are wrong:
 Calculated stress values |
 Close up of the leg to skirt attachment |
The stress distribution in the leg to skirt attachment is uneven. Turning on the mesh shows the uneven mesh that is supposed to be connecting these two parts.
The mesh is not joining along the edge
The problem does not go away with mesh refinement or tolerance adjustments. The problem is intermittent - some parts will join, some not. A recent update to SolidWorks Simulation can fix this problem:
 Standard mesh fails |
 Curvature based meshing works |
That's better!
Curvature based meshing was not include in SolidWorks Simulation 2008. This example was run in SolidWorks Simulation 2010.
Update: An alternate fix is to knit the surface.
Here the standard mesher was used with the leg surface knit to the skirt. The standard mesher produces a better looking mesh.
Easier Surfaces
File: PVE-4048
Last Updated: Feb. 24, 2010
LB
Surfaces can be challenging to create, but solids are easy to convert into surfaces. Surfaces originally created as solids do not have the problem of nodes not joining at edges (previous topic)...
This complex duct shape was made with a few simple solid modeling commands and then turned into a shell model by removing a few faces at the end of the pipes.
The model before the faces have been removed converting the solid model into a surface.
The mode meshes without fuss even at very coarse settings using the standard mesher. All nodes connect across surface boundaries.
Beautiful stress results from thermal expansion.
Close up
Solid Model Mesh Challenges
File: PVE
Last Updated: May 2010
LB
Sometimes a multibody model refuses to mesh with the standard mesher. Regardless of the element size and tolerances used, some parts refuse to bond.
 A large propane storage sphere |
 Meshed with the standard mesher - 802,000 elements - 12" large and 4" small element sizes |
The standard mesher has run, but when the analysis is performed, some of the bodies are not joined.
 Stress results - a surface has not joined (Displacements magnified 100x) |
 A close up of the area that did not bond (Displacement magnified 20x) The 4" elements at the leg and the 12" general shell elements can be seen. |
The curvature based mesher produces a less uniform looking mesh, and in this case the produced mesh has more elements.
 Curvature based mesher settings used. A mesh refinement of 4" size is set for the legs. |
 A detail of the mesh created with the curvature based mesher, 925,000 elements are produced. |
|
 Correct results from the curvature based mesh run |
 Close up of the results |
In theory it should be possible to alter any model to make it meshable by the standard mesher. Here the panel that will not mesh into the leg is split in half.
 Alternate solution - a panel where the mesh does not work has been split in half. |
 The model has successfully meshed and run. The split panel is shown. |
Note: this model run is used to determine the frequency of vibration of a sphere with a 1g sideways load. The stresses and deflections do not represent real world seismic conditions.
Solution for Long Mesh Time of Shells
File: PVE-4048
Last Updated: June 2010
CM
When meshing shells, the mesh gets up to 99% and then hangs for a very long time sometimes for hours depending on the mesh size. The mesher is going through some type of crazy routine trying to orient all of the shell faces in the same direction. We can do this manually in a few seconds by picking the face and then right clicking mesh and "Flip Shell Elements".
Go to Simulation options and un-check the "Automatic re-alignment for non-composite shells":
In the example model, doing this reduced the mesh time from 8 min 21 seconds down to 20 seconds.
Adjusting the mesh size after setting the face orientation causes some of the faces to be re-oriented. Manually flipping the faces is still much quicker than waiting for the automatic re-alignment.