Extracting Min/Max Values in StressCheck

An important feature of StressCheck is that the location and magnitude of minimal and maximal values of stress, strain and displacement data can be computed for a solution or a sequence of solutions. The data of interest may be a standard engineering function, a formula name or a calculator expression.

Generally, the solution can be considered to be of good quality if the error measured in energy norm is small and the location and magnitude of the minimal or maximal values of the data of interest clearly converge to a limiting value. Convergence is a requirement for solution verification in support of Simulation Governance, as well as benchmarking-by-FEA.

To perform minimum/maximum data extractions and/or convergence checks for a solved StressCheck model, select the Min/Max tab in the Results dialog and specify the desired Min/Max extraction options (Figure 1).

After specifying the Min/Max extraction options, click on Accept to perform the extraction. After the extraction is completed, a graph will appear displaying the min/max extraction results.

Specifying the Solution ID(s) and Run(s)

To extract min/max values for a solved StressCheck model, select the Min/Max tab in the Results dialog, set the Object and Method combo-boxes of the C/A/O/M to the desired configuration (discussed in the following), click on the Solution ID in the scrolling listbox and enter the range of Run numbers for which you wish to compute minimal and maximal values. For example, you may enter Run: 8 to 8 if only Run number 8 is of interest.

To compute an estimated convergence limit and relative error, at least three (3) Runs are required (e.g. Run: 1 to 3). For more information on convergence checks, refer to How Do I Check My Solution for Errors?

Multi-Solution Extractions

It is possible to compute the minimum/maximum values for different Solution ID’s. This is useful if you want to compare linear with nonlinear, or solutions having different boundary conditions. To activate multiple solution computation, select the multi-solution button near the upper left corner of the Results interface . The solution selection controls will change so that you may choose up to four different Solution ID’s and corresponding Run numbers (Figure 2).

Solution Run Wildcards

Entering a max Run number of “0” will automatically extract using the solution with the maximum DOF.

Specifying the Min/Max Object

Decide whether the extraction is for all elements (set the Object combo-box of the C/A/O/M to “All Elements”, the default), for one or more elements (set the Object combo-box of the C/A/O/M to “Any Element”), for one or more element faces (set the Object combo-box of the C/A/O/M to “Face” or “Face Surface”), for one or more element edges (set the Object combo-box of the C/A/O/M to “Edge” or “Edge Curve”), for one or more boundaries (set the Object combo-box of the C/A/O/M to to “Any Boundary”), or for an object set name (set the Object combo-box of the C/A/O/M to to “Sets”). Note: the option “Any Boundary” is applicable only if an element edge or an element face exists in the same space as the selected boundary. It is not required that the selected boundary be associated with the mesh, however.

Selecting Objects for Extracting Min/Max Values

If the Object combo-box is not set to “All Elements” or “Sets”, then in the Model View simply left-click on the objects on which the function will be extracted.

• If the extraction is on a group of elements, for example, then left-lick and drag the cursor to enclose the desired group of elements in a marquee selection. The selected elements will be highlighted and ready for extraction. Note: it is important to disable the Wetted Faces toggle if internal elements are to be included in the marquee selection.
• If you wish to add one or more elements to the selected group, hold the Shift key down and left-click on the elements to be added to the group.
• If you wish to remove one or more elements from the selected group, hold the Ctrl key down and left-click on the elements to be removed from the group.
• If you wish to cancel the current selection of objects, simply right-click on the Model View.

For example, to extract the maximum von Mises stress (Seq) for a group of element faces change the Object combo-box to “Face” and select the element face(s):

Specifying the Min/Max Method

Select the method of search from the Method combo-box of the C/A/O/M. The options are:

• Block: the search will be performed on a three-dimensional grid. This option is applicable only to solid elements.
• Grid: the search will be performed on a two-dimensional grid. This option can be used for 2D elements, or on surfaces or faces of 3D elements.
• Line (default): the search will be performed along element edges, along 2D boundaries, or along the outline of a surface.
• Wet Surface: the search will be performed on the free faces of the elements (excluding shared faces). This option is applicable only to solid elements.

Specifying the Display Format

You may input the precision with which you wish to display data values (“Format:” field, in C standard format). The default format is in scientific notation and any C language format specification can be used. For example, the number Pi (3.141592654…) will be displayed as: 3.141592654e+00 in format %16.9e or 3.14 in format %5.2f.

Specifying the Auxiliary/Independent Variable

Use the auxiliary variable input field (“Aux. Variable”) if you want to include a variable parameter in the
results. Switch the “Aux. Variable” toggle to “Indep. Var.” and enter a parameter name if you want the auxiliary variable to be the independent variable of the graph.

For example, if graphing the results of a Design Study analysis where one or more parameters is varied across a range of values.

Specifying the Function

Select a standard engineering function (e.g. Sx, Ey), or the formula (“Fmla”) or calculator (“Calc”) options by selecting the function name from the “Function:” combo-box. Note that only one function may be extracted at a time.

Specifying the Midsides

Specify the search grid (“Midsides:” field). The “Midsides:” field allows the user to increase/decrease the number of interior grid points used in the data extraction mesh. By default, this value is set to “3”. The “Midsides:” field is discussed further in the following note.

A Note on Midsides

Specify the data mesh, which is characterized by the number of “Midsides”. The specified function will be computed in the grid points of the data mesh. The data mesh determines the set on which the minimum and maximum will be sought. For a typical p-version mesh, between 8 and 12 midsides should be used.

For more information on midsides, refer to What Is the Midsides Input, and What Does It Control?.

Specifying the Min/Max Extraction Options

Several buttons/toggles exist to set additional preferences during the the min/max extraction.

Et/Em

The Et/Em switch can be toggled when extracting min/max strains to indicate whether total (Et, default) or mechanical (Em) strains should be computed.

Locate Max.

If you wish to create a point object at the location of the maximum/minimum value, turn on the “Locate max.” button and then enable the “Maximum” button, “Minimum” button or both buttons.

In addition to the creation of a point object, a maximum/minimum marker and label will also be drawn on the Model View (as described below in the Minimum/Maximum section). Note: the point object generated at the location of the maximum/minimum value may be used for additional modeling or extraction steps.

For an example of using the max stress location for new extractions, refer to StressCheck Tutorial: Using Max Stress Location for New Extractions.

Display Points

The Display Points button can be turned on to display the sample points in the model.

Minimum/Maximum

Specify whether you wish to compute Minimum and/or Maximum values by turning on the appropriate buttons. Additionally, if the “Locate max.” button is also enabled, a marker and label will be created at the location of the minimum (if “Minimum” is enabled) and/or maximum (if “Maximum” is enabled) value of the selected function.

• If “Maximum” is enabled, the label will be drawn in a red outlined box and a red marker will be drawn to the maximum function location.
• If “Minimum” is enabled, the label will be drawn in a blue outlined box and a blue marker will be drawn to the minimum function location.

The label text will identify if it is a minimum or maximum, include the extraction function name and value (if a formula is selected, the formula name will be used), the Solution ID and the selected Run number.

Plane/Z-plane

If an element is selected and the analysis reference is Extrusion, then it is possible to perform the extraction on any plane parallel to the XY-plane. The location of the plane is controlled by the input in the Z-plane field. The value of the Z-plane can be any number between –1.0 and 1.0, with Z-plane=0 representing the mid-plane of the extrusion. If an element edge is selected and the analysis reference is Extrusion, then it is possible to interpret the extraction to indicate the position of the edge in any plane parallel to the XY-plane. This feature allows defining the extraction procedure in 2D, and then interpreting the extraction as if the edge is located in an arbitrary plane (defined by the Z-plane input field) when the model is extruded.

In the below animation, the “Display Points”, “Locate max.” and “Maximum” toggles were enabled:

Specifying a Local System

Optionally, select a local system as the reference for the extraction (“System:” combo-box). By default, the “System:” combo-box is set to “Global”, but can be set to any local system (e.g. “SYS1”) or the Material system. The system combo box in the Results interface is used for deciding whether the stress/strain/displacement selected must be interpreted in the global, local or material direction. The coordinates of the extraction points are reported in both local and global coordinates. Local coordinates are identified based on selected system number (#) and system type:

• “X(SYS#), Y(SYS#), Z(SYS#) for Cartesian.
• “R(SYS#), T(SYS#), Z(SYS#) for Cylindrical/Polar.
• “R(SYS#), T(SYS#), P(SYS#) for Spherical.

Global coordinates are given as Cartesian regardless of the system type selected and labeled as X(Global), Y(Global), Z(Global). Note: if a Cylindrical system is selected, the extraction values will be in terms of R, T, Z instead of X, Y, Z. For example, Sx will be transformed to radial stress and Sy will be transformed to tangential stress.

For an example of extracting results in Cylindrical coordinates, refer to StressCheck Tutorial: Results in Cylindrical Coordinates (R, T, Z) and How Do I View Radial and Hoop Stresses/Strains?

Performing the Min/Max Extraction

Once all selections have been made, and options specified, click on the Accept button. The Min/Max extraction will be performed for the selected Solution ID(s), Run(s) and function, and a graph pane will be produced containing exportable details on the Min/Max extraction. A new Min/Max extraction may be performed at any time, resulting in a new graph pane. If the “Display Pts.” button was enabled, a red “+” will appear in the Model View at each search location. Also, the points where the maximal (respectively minimal) values occur will be identified with a label containing the user selected extraction function, the maximum (respectively minimal) value, and the corresponding solution with the highest DOF chosen for extraction. To clear these labels, click the right mouse button while the Model View has focus.

When computing minimal and/or maximal values from a sequence of at least 3 solutions, StressCheck performs an estimation of the true value of the selected function by projecting the results from the finite element solutions to an infinite number of degrees of freedom. The result of this projection is reported as the “Estimated Limit” together with the percent deviation from the value corresponding to the solution chosen having the highest number of degrees of freedom. The below shows a typical graph output where the estimated limits computed by StressCheck are displayed for the maximum and minimum values of Sx using 10 midsides:

Note: The computation of the estimated limit is performed as follows: If the last three data points are non-monotonic with respect to the number of degrees of freedom (N) then a weighted average is computed, the weight being the number of degrees of freedom. When the last three data points are monotonic with respect to the number of degrees of freedom then it is assumed that the error decays in proportion to N^-β where β is a positive number. These should be understood as heuristic procedures which tend to work well when the errors in the data are small, but may give a false indication of the limit when the errors are large. The procedure may compute a limit even when the limit does not exist or fail to compute a limit even when one does exist. For more details or error estimation in numerical simulation, refer to Numerical Simulation Series: Numerical Simulation in Solid Mechanics.

For an example of assessing convergence of a maximum stress, refer to StressCheck Demo: 3D Shoulder Fillet Stress Concentration Factor Study and StressCheck Demo: 3D Tie Rod Stress Concentration Factor Study.