Results Environment


The Results environment serves two purposes:

Note

The date and time when the model was last "Checked" and last analyzed are stored. If a change is made to the model that would affect the results – such as changing the material properties or input in the Element Definition – then the "Checked" date is updated. When the "Checked" date is newer than the analyzed date, the following message is given whenever the model is displayed in the Results environment:

 

The existing results do not match the current model. If the changes have no affect on the results, then it is reasonable to proceed. (Changes include loads, mesh, materials, node numbering, and element numbering.) If the model has changed, the old results should not be used.

 

If the model has been changed, or if a different version of the software is being used (which could result in different node or element numbering), it is possible that the existing results will not match the "new" FEA model. If you proceed to use the existing results, check the validity of the results carefully. Alternatively, re-analyze the model to be certain that the results are for the current model. Note that changes to the model include any geometry changes which can either be deliberate (for example, deleting lines and re-drawing them) or transparent (for example, transferring to PV/Designer).

 

Note that this message will appear when doing a restart analysis for those analysis types that show the results while the analysis is running. This behavior is expected.

Understanding The Results:

Depending on the analysis type, there may be two distinct types of results that can be displayed. It is wise to understand the difference between these.

Smoothing Results. In a continuous material, the stresses change in a smooth pattern. But the FEA approach and the element results described above give discontinuous results; the degree of discontinuity depends on the mesh refinement. Thus, the default display method for element results is to show the "smoothed" or average value. The smoothed result is just the arithmetic mean of the results from all of the elements attached to the node, and this smoothing is likely to be closer to the real value than the individual results.

 

However, different parts may be made from different materials. Or, in the case of a model constructed from plate elements, different parts may be different thickness. In these situations, the results are theoretically different in each part at the common node; that is, the result is not continuous. So the default smoothing option is to not smooth the results across different parts.

 

Note

Some element results should not be smoothed, even within one part. For example, the "Heat Rate of Face" in a heat transfer analysis shows the amount of heat passing through each face. In an ideal model, the heat leaving one face equals the heat entering the adjacent face. So these results would be equal but opposite in sign, so displaying the smoothed result would show a heat rate of 0. For this type of situation, the smoothing should be deactivated.

 

The results of the analysis can be obtained either visually, by graphing, or by inquiring. There are some subtle differences between them.

When the model includes parts made from solid elements (solid element types include brick, 3-D, and tetrahedral elements), the values shown visually are by default based on all of the nodes that form the elements on the "surface" of the model. An element is considered to be on the surface if any of its nodes are on the surface. (Be aware that a surface may be on the inside of the model, such as the surface of an interior cavity.) So technically a maximum or minimum value shown in the legend etc. may be at a node one element underneath the surface. In this case, it can be hard if not impossible to see the color on the model that represents the maximum or minimum value. If some elements are selected and hidden, a new set of "surface elements" is created, and the results shown are based on the new set of nodes attached to the surface elements.

 

For stress models, viewing the results from the surface only is acceptable since the maximum stress is generally on the outside surface of the model. If the maximum expected stress is inside the model, such as a Hertz contact stress or thermal stress, then a slice plane or hiding elements would be used to show the inside, so the nodes on the new "surface" are used for all of the results. For other analysis types, the maximum result may be in the interior of the solid mesh. For these situations, use the "Display Options: Show Complete Mesh" menu. When this item is active, all of the solid elements are used when displaying the results. See Figure 1.

 

Default view of a solid cube modeled with brick elements. "Display Options: Show Complete Mesh" is off.

If the model were sliced, you would see that only the elements on the surface are shown (1). The results on the interior elements (2) are not shown by default. The results shown visually in the display area are based on the nodes attached to the surface elements (3).

Figure 1: Results with Solid Elements

 

Note that physically slicing the model in the Results environment exposes a new layer of surface elements, just like the example of hiding elements mentioned above. The "slice" in Figure 1 is a theoretical discussion.

 

See also the following sections of the documentation for additional information on these topics:

 

"Results Option Menu: Smooth Results"

to activate or deactivate the smoothing of the element results

"Results Options Menu: Smoothing Options"

to set the options used with the smoothing calculation, such as the smoothing function (mean by default, other options such as maximum, minimum, range) and smoothing across part boundaries.

"Display Options Menu: Plot Settings Dialog"

to change the display of the color contour and all things associated with the legend box.

"Inquire Menu: Probe"

to display the result at a node as the mouse hovers over it.

"Inquire Menu: Results"

to obtain the results of selected nodes in a text window, with options to sum the results and save them to a file.

"Display Options: Show Complete Mesh"

to activate or deactivate the display of the interior solid elements.

Graphing the Results of an Analysis

to graph the results of a single node or multiple nodes, and manipulate the results (derivative, integrate, etc).

 

Selection, Visible Items, and Hidden Elements:

Elements and nodes can be selected by these methods:

Results Environment Menus:

There are four pull-down menus in the Results environment that can be used to display and inquire on the results of the analysis. In addition there are additional commands in the FILE pull-down menu that can be used to export results.  For information on these menus, click on the link below.

 

Exporting Results

Results Menu

Results Options Menu

Inquire Menu

Display Options Menu

Utilities Menu

Fracture Analysis

Miscellaneous Tree and Toolbar Functions

Graphing the Results of an Analysis