Specifying accuracy parameters for adaptive meshing

In the Adaptivity Meta Solution dialog box, you use the options in the Accuracy Parameters group to define the error criteria that the software uses to evaluate the mesh and determine areas where mesh refinement is needed to ensure solution accuracy.

Accuracy parameters and solution type

The applicable Accuracy Parameters depend upon your current solution type.

• For structural solutions, or for structural steps within Simcenter 3D Multiphysics solutions, you can define strain energy, steady stress, or minimum stress as criteria.

• For thermal solutions, or for thermal steps within Simcenter 3D Multiphysics solutions, you can define temperature as a criterion.

Depending upon the type of solution you are using, you can specify one or more accuracy parameters.

• If you do not specify a value for an accuracy parameter, the software does not use that parameter to evaluate the mesh.

• For structural analyses, if you specify values for both the Strain Energy (%) and the Steady Stress option, the software always envelopes the results to obtain the highest error value. It uses this worst case error value to identify locations for mesh refinement.For structural solutions, the software envelopes across all linear statics subcases to obtain the highest error value.For structural steps within Simcenter 3D Multiphysics solutions, the software envelopes across all time steps to obtain the highest error value.For normal modes solutions, the software envelopes across all modes to obtain the highest error value.

• For thermal analyses, the software envelopes the computed temperature error estimates for all time steps into a single error estimate. It uses the highest error value computed across all time steps to identify locations for mesh refinement.

Absolute or relative error values

You can define different accuracy parameters in terms of relative or absolute error values.

• A relative error value is relative to the entire model. The software computes a single error value for the entire model and compares it to the specified threshold value. If that single error value exceeds the threshold value, the software evaluates each location in the model to compute local error values. During the mesh refinement process, the software refines areas that have a high local error value and does not refine areas that have a low local error value.Using relative error values to define accuracy allows high local errors to exist in a model. However, the significance of that locally high error value decreases as the software increases the mesh density.Relative error calculations are influenced by the number of elements in the model. In a larger mesh, a model that has many elements with low error values and a few elements with high error values still converges.Meshes that contain singularities may converge if accuracy is measured relative to the entire model. As the software refines the mesh around the singularity, the overall element count in the mesh increases, and the influence of the singular region on the overall error values decreases.

• An absolute error value measures the error at a specific location. The software computes the error value at a location and compares it to the specified threshold value.Using absolute error values to define accuracy does not allow for high local error values within the model. Each location in the model must satisfy the specified threshold value.Absolute error calculations are not influenced by the number of elements in the model.For models that contain singularities, local absolute error values generally increase around the singularity and prevent the solution from converging.

Strain energy

The Adaptivity solution process uses the following equation to calculate the strain energy:

The Adaptivity solution process uses the following equation to calculate the strain energy error value:

where

Ω is the element volume

σunaveraged is the unaveraged stress vector

σaveraged is an averaged stress vector computed at a node using the stress vectors from elements connected to the node

D matrix is the constitutive relation

When the software computes σaveraged, it does not average the stress values across the following:

• Different element families.

• Material properties.

• Material coordinate systems.

• Orientation angles in 2D solid elements.

• Thicknesses in plane stress elements.

Steady stress

The Adaptivity solution process uses the following equation to calculate the stress norm:

The Adaptivity solution process uses the following equation to calculate the stress error norm:

where

Ω is the element volume

σunaveraged is the unaveraged stress vector

σaveraged is an averaged stress vector computed at a node using the stress vectors from elements connected to the node

D matrix is the constitutive relation

When the software computes σaveraged, it does not average the stress values across different element families, material properties, material coordinate systems, orientation angles in 2D solid elements, and thicknesses in plane stress elements.

If you specify an absolute error value for stress, you can also specify an optional, minimum allowable stress norm value. If the elements in a region of the mesh have an absolute stress norm value that is less than the specified minimum value, the software does not refine the mesh in that area. Use the Minimum Stress Norm option to prevent the software from refining the mesh in low stress regions.

Mesh refinement computations for strain energy and relative stress errors

The software uses the procedure recommended by Zienkiewicz and Zu in The Finite Element Method: Its Basics and Fundamentals, sixth edition to take the error estimates and calculate the mesh refinement level required at each element for strain energy and relative stress errors.

In an optimal mesh, the distribution of the element strain energy and the relative stress error norms should be equal for all elements. Therefore, the total permissible error is determined as:

The error in any element k should be:

m is the number of elements involved.

||e||k is the error estimate for any element k.

The software carries out the refinement by refining only a certain number of elements in which ξ is higher than a certain limit. Each time, it halves the size of elements when ξk>1. The software calculates the element refinement level as follows:

The goal of the mesh refinement process is to achieve ξk≤1.

Temperature

For thermal solutions or thermal steps in Simcenter 3D Multiphysics solutions, you can use the Temperature parameter to have the Simcenter 3D Thermal solver calculate a temperature error estimate that estimates the local spatial discretization errors due to the mesh used for the conduction scheme. This error estimate measures the change in temperature (Δ) across an element in units of temperature, for example, degrees C, degrees F, R or K).

• Because error estimates are local, they do not serve as a bound of the true error.

• Discretization errors related to other thermal physics models, such as radiation, convection, and thermal couplings, are not measured.

The Simcenter 3D Thermal solver uses either a finite volume method or a finite element method to calculate the temperature error estimates. When using the finite element method, the solver uses equations similar to the strain energy and relative stress error estimates for the temperature error estimates, as described in Mesh refinement computations for strain energy and relative stress errors.

The finite volume method adapts an idea from finite element methods developed by Zienkiewicz and Zhu in The Finite Element Method. Zienkiewicz and Zhu modified the computed finite element solution so that the solution does not contain jumps across element boundaries. They called this the improved solution. Zienkiewicz and Zhu then used the difference between the computed and the improved solution as the estimated error for the solution.

To understand how Simcenter 3D Thermal adapts this method, you must understand the software's finite volume method. The Simcenter 3D Thermal finite volume method has calculation points at:

• The center of gravity of each element.

• The center of gravity of each boundary element.For shell elements, the centers of gravity for boundary elements are at the mid-point of each element edge.For solid elements, the centers of gravity for boundary elements are at the center of gravity for each element face.

For example, the graphic below shows a triangular shell element. (1) shows the centers of gravity of the boundary element. (2) shows the location of the shell element’s nodes.

Temperatures are continuous from one element to another at the boundary element computation points. The heat flux through each element’s face, for solid elements, or each the heat flux through each element’s edge, for shell elements, is conserved. However, the solution that the finite volume scheme calculates does not result in a continuous temperature field. As you move from one element to the next across the nodes, the calculated temperature field is discontinuous.

Simcenter 3D Thermal uses a detailed nodal temperature reconstruction scheme to recover smoothed, continuous nodal temperatures at the nodes. Based on the ideas developed by Zienkiewicz and Zhu, Simcenter 3D Thermal does the following:

• Boundary element temperatures are the calculated solution.

• Nodal temperatures are the smoothed solutions.

Simcenter 3D Thermal computes the temperature error estimate for the finite volume method by using element shape functions to interpolate the nodal temperatures to the boundary element locations. It then calculates the differences between the smoothed, interpolated temperatures and the calculated boundary element temperatures. This elemental temperature error estimate is the maximum of these quantities over the element.

εT = max for all boundary elements abs(TBE-fBE(T1, T2, ..., TN))

Where:

TBE are the calculated temperatures for the boundary elements.

Ti are the N (number of nodes) smoothed nodal temperatures.

fBE uses element shape functions to interpolate the nodal temperatures to the boundary element.

Learn more

Adaptive meshing

Adaptive meshing workflow

Supported solution types for adaptive meshing

Pre-processing requirements for adaptive meshing

Specifying the mesh parameters for adaptive meshing

Singularities in adaptive meshing

Understanding the adaptive refinement process

Excluding parts of the model from adaptive meshing

Refining specific parts of an adaptive mesh

Viewing adaptive meshing results

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Specifying accuracy parameters for adaptive meshing, Simcenter 3D 2021.1 Series

© 2020 Siemens

window.mainLanguage="en_US"

window.delivId=""

window.projectId=""

MathJax.Hub.Config({ TeX: { extensions: ["autoload-all.js"] }, tex2jax: { displayMath: [ ] }, "SVG": { scale: 125 } });