If the current viewport contains a model plot (an undeformed, deformed, contour, symbol, or material orientation plot) or a model from the current model database,, Abaqus/CAE allows you to probe results from the selected model or output database. The Probe Values dialog box identifies the step, frame, and field output variable for which Abaqus/CAE will obtain values. To learn how to change the step, frame, or field output variable, see “Selecting the results step and frame,” Section 42.3, and “Selecting the primary field output variable,” Section 42.5.3.
When you probe a model plot of a three-dimensional shell or a composite solid, the results that Abaqus/CAE returns depend on your choice of active location in the Section Points dialog box. Abaqus/CAE returns results from the Top Location section point when Top is the active location and returns results from the Bottom Location section point when the active location is set to Bottom or Top and bottom. For more information about section points, see “Selecting section point data,” Section 42.5.9.
For model plots you can choose to obtain node-based or element-based data and results, as follows:
Probing nodes
When you choose to probe nodes and position the cursor over a nodal location in the current viewport, Abaqus/CAE highlights the node and displays the following information about the node in the data table:
the node's label,
the node's original coordinates,
the node's deformed coordinates (using the current deformed field output variable),
the elements sharing the node, and
the current field output variable (including component values, if the current field output variable is a tensor or vector quantity). If a model is selected in the current viewport, the current field output variable reflects the value of a model attribute such as a load at the selected node.
You can display field output at the node whether the current primary variable was originally saved to the output database at nodal, centroidal, or integration point locations. Abaqus/CAE calculates nodal values for centroidal and integration point data by extrapolating to the nodes and averaging according to options you select. If the node refers to unaveraged element data, all element data associated with the probed node will be displayed. For more information on averaging, see “Understanding result value averaging,” Section 42.6.2.
You can also display or hide annotations that appear in the viewport for each node you select. Probe annotations show the node's label and the results at that node for the current field output variable. You can customize the font and color of the probe annotation text.
Probing elements
When you choose to probe elements and position the cursor over an element in the current viewport, Abaqus/CAE highlights the element and displays the following information about the element in the data table:
the element's label,
the element's connectivity, and
the current field output variable (including component values, if the current field output variable is a tensor or vector quantity). If a model is selected in the current viewport, the current field output variable reflects the value of a model attribute such as a load at the selected element.
You can display field output at the element only if the current primary variable is an element-based variable, such as stress or strain. You can choose the output position at which field output results are calculated: integration point, centroid, element node, or element face. For each of these output positions, Abaqus/CAE calculates probe results on an element-by-element basis with no averaging.
You can also display or hide annotations that appear in the viewport for each element you select. Probe annotations show the element's label and the results at that element for the current field output variable. You can customize the font and color of the probe annotation text.
Regardless of the render style in which the model is displayed, only visible elements can be probed. If necessary, you can create a display group or use a view cut to reveal otherwise unavailable interior elements.
When an element is cut through by a crack, the cracked element splits into two parts, each part formed by a real domain and a phantom domain. When you probe cracked elements, only the contribution from one part of the elements is reported. For more information, see “Visualization” in “Modeling discontinuities as an enriched feature using the extended finite element method,” Section 10.7.1 of the Abaqus Analysis User's Guide.