Computing Resultants in StressCheck

StressCheck provides information about the equilibrium and stress resultants of elements. The basic idea is that in the displacement formulation of the finite element method, the equilibrium conditions are satisfied approximately. As the number of degrees of freedom increases, the displacement field of each element will satisfy equilibrium with increasing accuracy.

To perform equilibrium and/or stress resultant extractions for a solved StressCheck model, select the Resultant tab in the Results dialog and specify the desired Resultant extraction options (Figure 1).

After specifying the Resultant extraction options, click on Accept to perform the extraction. After the extraction is completed, a graph will appear displaying the resultant extraction results.

In the equilibrium test, the tractions are computed along the boundaries of elements from the finite element solution and integrated along the perimeter:

• When no body forces are applied, the contour integral of the tractions should be nearly zero.
• When body forces are applied, the contour integral of the tractions should be nearly equal and opposite to the applied body forces.

The equilibrium test is a rough measure of the quality of the mesh and should be used for guidance in changing the mesh when the desired level of accuracy cannot be reached by p-extension. Additionally, the resultant is commonly computed in multi-body contact analyses to evaluate load transfer and reactions between contacting bodies.

For more information on equilibrium checks, refer to How Can I Check Load Transfer, Equilibrium and Nodal Reactions In Results?

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

To compute resultants for a solved StressCheck model, select the Resultant tab in the Results dialog, and set the Action and Object 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 resultant 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 the importance of checking solution quality, refer to What Are the Key Quality Checks for FEA Solution Verification?

Solution Run Wildcards

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

Specifying the Resultant Action

Decide whether the resultant will be computed automatically after left clicking a single element, element edge or element face (“Check”), or will be computed for one or more selected elements, element edges, element faces, or contact zones after clicking the Accept button (“Select”).

Specifying the Resultant Object

Decide whether the resultant computation is for one or more elements (set the Object combo-box of the C/A/O/M to to “Any Element”, the default), for one or more contact zones (set the Object combo-box of the C/A/O/M to “Contact Zone”), 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”), or for one or more nodes (set the Object combo-box of the C/A/O/M to “Node”). The following are the resultant computation expectations for each object:

• Node: Computes force resultants and moments for a beam element.
• Edge/Edge Curve: Computes the integral of the traction along an element edge for 2D problems.
• Face/Face Surface: Computes the integral of the traction over an element face for 3D problems.
• Any Element: Computes the contour integral of the traction over the element (equilibrium check).
• Fastener: Computes the load transferred by a fastener.
• Contact Zone: Computes the integral of the traction over the element edges (2D) or element faces (3D) associated with a contact zone.
  • Contact zone resultants are helpful when assessing load transfer quality between contacting regions.
  • Including additional element edges (2D) or element faces (3D) outside the contact zone may be required to recover the resultant if there are stress singularities in the contact zone region.

Checking Resultants for a Single Object

If the Action is set to “Check”, then in the Model View simply left-click on the element, element edge or element face on which the resultant is to be computed. The resultant computation will be automatically performed and a graph pane displayed. In addition, the Resultant tab Force and Moment summation fields will show the numerical values for the run with the highest number of DOF. Note: if you continue left clicking on new objects, the summation field values will show the cumulative result. If you click the “Reset” button, then the summation field values will be cleared.

The below animation shows checking a single element for equilibrium:

Selecting Multiple Objects for Resultant Computation

If the Action is set to “Select”, then in the Model View simply left-click on the object(s) on which the resultant will be computed.

• 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.

The below animation shows the resultant for a selected group of element faces. In this case, the applied load was 10 kip, and spring coefficient constraints were applied on a subset of the selected element faces:

For an example of computing a stress resultant for a group of selected element faces on an embedded plane surface, refer to StressCheck Tutorial: Embedding 3-Point Plane for Resultant Extractions.

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 Moment Center and Output Functions

Several inputs/buttons exist to set additional preferences during the resultant computation.

Moment Center

The moment center refers to the coordinates of the point about which the moment is to be computed. The default is the origin of the global system (0,0,0). Resultant extractions can also be computed with respect to the chosen local system (via the “System:” combo-box) and moment coordinates with respect to that local system.

Output Functions

The available output functions will depend on the reference and analysis types. For example, the appropriate functions for planar elasticity are Fx, Fy and Mz, that is the force resultants in the global X and Y-directions and the moment about the Z-axis. The results of the equilibrium or resultant computation will appear in the graph pane for the selected functions only, and also in the Force and Moment summation fields of the Resultant tab for all relevant functions.

To select an output function for display in the graph pane, simply enable the corresponding Force or Moment button in the summation fields area of the Resultant tab. The below animation demonstrates how the output function Fz was enabled for extraction on a group of selected element faces:

Specifying a Formula

A formula expression of one or more output functions (e.g. Fx, Fy, Mz) may be specified during the resultant computation. For example, if a formula expression of “Res = 2*Fx + 1/2*Fy” was specified, then the formula “Res” could be selected in the “Formula:” combo-box. The graph pane would provide the results of “Res” for the selected objects and system.

Specifying a Set Name

A set containing one or more objects for resultant computation may be selected by the user in the “Set:” combo-box. Once the Object combo-box of the C/A/O/M is set, the available sets will be listed. Note: selection of a set will automatically select the objects in the Model View.

Specifying a Local System

Optionally, select a local system as the reference for the computation (“System:” combo-box). By default, the “System:” combo-box is set to “Global”, but can be set to any local system (e.g. “SYS1”). The system combo box in the Results interface is used for deciding whether the output functions are interpreted in the global or local directions.

Performing the Resultant Computation

Once all selections have been made, and options specified, click on the Accept button. The Resultant computation will be performed for the selected Solution ID(s), Run(s) and output functions, and a graph pane will be produced containing exportable details on the Resultant computation. A new Resultant computation may be performed at any time, resulting in a new graph pane. In addition, the Resultant tab summation fields (e.g. Fx, Fy, Mz) will show the numerical values for the run with the highest number of DOF.

When computing output function 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 animation shows a typical graph pane where Fx, Fy and Fz were computed on a selection of contact zones (expected reaction was ~5 kip):

For an example of computing the resultant due to multi-body contact, refer to StressCheck Tutorial: Incorporating Contact Pressure Bleed in Resultant Extractions.