Important Note: The internal shell element forces are forces per unit length acting along the mid-surface of the shell element (area object). The internal shell element stresses are stresses acting on the edges (not positive 3-axis face and negative 3-axis face) of the shell element (area object).
Note: Click the Apply button to update the active window using the parameters specified on the form. When the Apply button is used, the Shell Forces/Stresses form will remain open until the Close button is clicked. This allows another selection to be made on the form to review multiple displays without using the command to recall the form. The OK button can be used to both update the active window and close the form if only one view is needed.
The Shell Forces/Stresses form has the following options:
Load Case, Load Combination, Modal Case options. Choose the load case to be displayed. Note that shell element forces or stresses can be plotted for any static load case, response spectrum case, time history case, static nonlinear case, or load combination. For time history cases, also specify a time for display of the forces or stresses. For static nonlinear cases, also specify a step for display of the forces or stresses.
Component Type options. Choose to display shell element internal forces or internal stresses. When stresses are selected, also select the face of the shell object - visible, top, or bottom - for which stresses are to be displayed, or choose that the maximum, minimum or absolute maximum stress values are to be displayed.
Component options. Specify the component of force or stress to be displayed.
For shell element internal forces, the possible components are as follows:
F11: Direct force per unit length acting at the mid-surface of the element on the positive and negative 1 faces in the 1-axis direction.
F22: Direct force per unit length acting at the mid-surface of the element on the positive and negative 2 faces in the 2-axis direction.
F12: Shearing force per unit length acting at the mid-surface of the element on the positive and negative 1 faces in the 2-axis direction, and acting on the positive and negative 2 faces in the 1-axis direction.
FMax: Maximum principal force per unit length acting at the mid-surface of the element. Note that by definition principal forces are oriented such that the associated shearing force per unit length is zero.
FMin: Minimum principal force per unit length acting at the mid-surface of the element. Note that by definition principal forces are oriented such that the associated shearing force per unit length is zero.
FVM: Von Mises principal force per unit length acting at the mid-surface of the element.
V13: Out-of-plane shear per unit length acting at the mid-surface of the element on the positive and negative 1 faces in the 3-axis direction.
V23: Out-of-plane shear per unit length acting at the mid-surface of the element on the positive and negative 2 faces in the 3-axis direction.
VMax: Maximum principal shear per unit length acting at the mid-surface of the element. Note that by definition principal shears are oriented on faces of the element such that the associated shears per unit length on perpendicular faces are zero.
M11: Direct moment per unit length acting at the mid-surface of the element on the positive and negative 1 faces about the 2-axis.
M22: Direct moment per unit length acting at the mid-surface of the element on the positive and negative 2 faces about the 1-axis.
M12: Twisting moment per unit length acting at the mid-surface of the element on the positive and negative 1 faces about the 1-axis, and acting on the positive and negative 2 faces about the 2-axis.
MMax: Maximum principal moment per unit length acting at the mid-surface of the element. Note that by definition principal moments are oriented such that the associated twisting moment per unit length is zero.
MMin: Minimum principal moment per unit length acting at the mid-surface of the element. Note that by definition principal moments are oriented such that the associated twisting moment per unit length is zero.
For shell element internal stresses, the possible components are as follows:
S11: Direct stress (force per unit area) acting on the positive and negative 1 faces in the 1-axis direction.
S22: Direct stress (force per unit area) acting on the positive and negative 2 faces in the 2-axis direction.
S12: Shearing stress (force per unit area) acting on the positive and negative 1 faces in the 2-axis direction and acting on the positive and negative 2 faces in the 1-axis direction.
SMax: Maximum principal stress (force per unit area). Note that by definition principal stresses are oriented such that the associated shearing stress is zero.
SMin: Minimum principal stress (force per unit area). Note that by definition principal stresses are oriented such that the associated shearing stress is zero.
SVM: Von Mises principal stress (force per unit area).
S13: Out-of-plane shearing stress (force per unit area) acting on the positive and negative 1 faces in the 3-axis direction.
S23: Out-of-plane shearing stress (force per unit area) acting on the positive and negative 2 faces in the 3-axis direction.
SMaxV: Maximum principal shearing stress (force per unit area). Note that by definition principal shearing stresses are oriented on faces of the element such that the associated shears per unit length on perpendicular faces are zero.
Contour Appearance options. Use these options to choose if the forces and stresses will display on an Undeformed Shape, a Deformed Shape, or a display of an Extruded Contour by selecting an option from the drop-down list. Also use the Show Lines, Show Fill, Show Values, and Show Arrows check boxes to specify how the forces and stresses will be illustrated. The options are assumed to be self-explanatory.
Contour Values The shell element internal forces and stresses are displayed on screen as colored contours. Specify minimum and maximum values:
Min edit box: Any element with a force or stress less than the value specified in this edit box is displayed in the color associated with Min in the Contours area of the Assign Display Colors form. Note that the color associated with Min is the top color in the form.
Max edit box: Any element with a force or stress greater than or equal to the value specified in this edit box is displayed in the color associated with Max in the Contours area of the Assign Display Colors form. Note that the color associated with Max is the bottom color in the form.
With the Min and the Max values specified, ETABS spaces the intermediate range values equally between the specified Min and Max values. If the Min and the Max values are both set to zero, ETABS creates its own range. In that case, ETABS creates a stress range with rounded (even) values that the actual maximum and minimum stresses fit within. Note that setting Min and Max to zero is the default.
Contour Averaging at Nodes. Specify if stress averaging is to be used when displaying the shell element forces or stresses. ETABS offers the following options:
None - no stress averaging
By Objects - stress averaging at all objects
By Selected Groups - stress averaging at specific points selected just before plotting the shell forces or stresses; click the Groups button to access the Select Groups form and select objects by Group names.
Explanation of Contour Averaging. Consider the four shell elements labeled A, B, C and D shown in the sketch below. These four shell elements all have a common point, labeled 1, in the sketch.
Each of the shell elements has an associated internal force or stress at joint 1. Typically the forces or stresses at common points in the various shell elements are different. The finer the mesh, the closer the values become.
If the force or stress contours are plotted with no stress averaging at the common points, typically the changes in force or stress from element to element will be abrupt. Stress averaging tends to eliminate the abrupt changes in the plot and smooths the contours.
ETABS averages the stresses at a point by averaging the stresses from all shell elements that both connect to the point and are visible in the active window. Then when ETABS plots the stress for a particular shell element, it plots that average stress at the point considered instead of the actual stress calculated for that shell element at the point.
Do not overlook the implications of the underlined portion of the previous paragraph. For example, assume the active window is displaying stresses in a location where a wall intersects a floor. Further assume that the display shows averaged stresses in the floor. If the averaged stresses in the floor are displayed in a 2D plan view of the floor, only the shell elements that are in the floor, and thus visible in the window, are included in the stress averaging.
If the same averaged stresses are displayed in a 3D view, where both the wall and the floor are visible, the shell elements from both the floor and the wall are included in the stress averaging. Thus the averaged stresses in the floor at the intersection of the floor and the wall will appear differently in a 2D plan view versus a 3D view.
Scaling options. The scaling options will be available only if Display on Deformed Shape or Display Extruded Contours has been selected for the Contour Option. When available, the scale factor can be used to exaggerate the displacements/extrusions relative to the geometry of the structure. Choose Automatic scaling or specify a User Scale Factor to scale the deformed shape or the extruded results.
Miscellaneous Notes about Shell Element Forces and Stresses Note that shell element stresses (not forces) actually have different values at the top and bottom of the shell elements (area objects). Thus, depending on which side of the object is displayed, different stresses may be shown. Two-dimensional views always display area objects from the same side. To display stresses on the other side of the area object, view them in a 3D view.
Finally, when shell element forces and stresses are plotted for multi-valued load combinations, ETABS displays the maximum or minimum value that has the largest absolute value.
Access the Shell Forces/Stresses form as follows:
Run an analysis.
Click the Display menu > Force/Stress Diagrams > Shell Stresses/Forces command.