Form: Member Force Diagram
Code-specified and other pre-defined material properties are defined in the installed files "CSiMaterialLibrary*.xml" located in the subfolder "Property Libraries" under the SAP2000 installation folder. Additional material property libraries that use the "CSiMaterialLibrary.xsd" schema may also be added by the user to this subfolder and/or to the subfolder "Property Libraries" under the user settings folder where the "SAP2000 v18.ini" file is located.
These files are first read in alphabetical order from the installation subfolder, then from the user settings subfolder. Any duplicated properties will use the values in the definition read last. Within each file, properties are grouped under user-defined Regions (e.g.: China, Europe, or USA). Within Regions, properties are grouped under user-defined Standards (e.g.: ASTM A572). Within Standards, individual materials are defined to be of a certain type (concrete, steel, aluminum, cold-formed steel, rebar, tendon, or other) and identified by a user-defined label called Grade. The set (Region, Standard, type, Grade) uniquely identifies a material and determines whether or not it is duplicated within a file or multiple files.
Use the Define menu > Materials command to add, copy, modify, or delete a material property definition. The material property definitions are then used in defining the structural objects (frame sections, cable sections, tendon sections, area sections, solid properties).
TIP: The forms described in this topic can also be accessed by clicking the + (plus) symbol that may appear next to a drop-down list of available materials, such as the Material drop-down list on the Shell Section Data form, or the {Type} Section forms, which can be accessed through the Add Frame Section Property form..
Click the Define menu > Materials command to access the Define Materials form.
Click the appropriate button to complete the required action:
Important note: The internal shell element forces are forces per unit length acting along the midsurface 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). See Sign Conventions for more information about the faces of shell objects.
Case/Combo Name edit box. Choose the load case or combination whose shell element forces or stresses are to be displayed.
Multivalued Options: For multi-mode cases, choose the mode number for which results are to be shown. For multi-step cases, choose the step number, time step, or frequency step; or choose Envelope to view the maximum or minimum results over all steps.
Component Type options. Choose the type of component to be displayed. The options available depend on the sections assigned in the model, and the option selected determines the other input required on the form.
Resultant Forces option. When this option is selected, also select the Component.
Shell Stresses option. When this option is selected, specify the Output Type (i.e., display the stresses for the Visible Face, Top Face or Bottom Face, or the Maximum stress, Minimum stress or Absolute Maximum stress) and the Component.
Note: When plotting Shell Stresses or Shell Layer Stresses, you can select the option to normalize the stresses with respect to the material strength. The strength used for this purpose is the yield strength (Fy) for steel, cold-formed steel, rebar, and tendon materials; the minimum of the two yield strengths (Fcy or Fty) for aluminum materials; and the compressive strength (f'c) for concrete materials. Zero normalized stresses will be plotted for other materials.
Shell Layer Stresses option. When this option is selected, specify to display the stresses By Area Section and Layer Name or By Layer Name Only. To display the stresses by area section, specify the area section by selecting it from the Area Section Property drop-down list. Then for both options, select the Layer Name and the Thickness Location within the layer from the drop-down lists. See note in Shell Stresses option above.
Concrete Design option. When this option is selected, specify the Output Type (i.e., display the member force for the Visible Face, Top Face or Bottom Face, or the Maximum, Minimum or Absolute Maximum member force) and the Component.
Component options. Specify which component of force or stress is to be displayed.
Click here for information about possible components of the shell element internal forces.
Click here for information about the possible components for shell element internal stresses.
Contour Range: The shell element internal forces and stresses are displayed as colored contours. Specify two values:
Min: Any element with a force or stress less than the value shown here is displayed in the color associated with Min in the Contours area of the Assign Output Colors form. Note that the color associated with Min is the top color in the form.
Max: Any element with a force or stress greater than or equal to the value shown here is displayed in the color associated with Max in the Contours area of the Assign Output Colors form. Note that the color associated with Max is the top color in the form.
The program spaces the intermediate range values equally between the specified Min and Max values. If the Min and Max values are set to zero, SAP2000 will automatically create a contour range that includes all values. This is the default. Click the Set To Default Contour Range button to apply the default values
Stress Averaging:
Specify if stress averaging is to be used when displaying the
forces or stresses. Consider the four elements labeled A, B, C
and D shown in the sketch at right. These four elements all have
a common point, labeled 1, in the sketch. Each of the elements
has an associated internal force or stress at joint 1. Typically
the forces or stresses at common points in different elements
are different. The finer the mesh
the closer the values become.
The options available for stress averaging are None for no stress averaging, At All Joints for stress averaging at all joints or over Objects & Groups for stress averaging at points selected just before plotting the shell forces or stresses, or for stress averaging of groups selected using the Set Groups button.
If the None option is used so that the force or stress contours are plotted with no stress averaging at the common points, the changes in force or stress from element to element typically will appear abrupt. Large stress variations between elements may indicate that the model is not properly meshed and may need to be refined to properly capture the variation in stress. Therefore, use this option to determine if the model is meshed properly.
Stress averaging using the At All Joints or over Objects & Groups option tends to eliminate abrupt changes in the plot and smoothes the contours. Thus, after the meshing of the model has been shown to be acceptable using the None option, the At All Joints option will give better results of the stress in the elements by averaging the stress between elements and reducing the error because of the stress on each individual element. The over Objects & Groups option should be used if a discontinuity, such as two planes meeting at an angle, is included in the model. In that case, each plane should be averaged independently using the over Objects & Groups option. This will avoid the problem of averaging across the two planes, which would give incorrect result. The results would be incorrect because the stress along the two planes is not continuous relative to the elements' local axes.
Show Deformed Shape check box. When this check box is checked, SAP2000 will display the model using color-coded contours with distortions to show where the model is subject to the effects of the forces and stresses.
Note: Shell element stresses (not forces) actually have different values at the top and bottom of the shell elements as a result of bending. Thus, depending on which side of the object is being displayed, different stresses will be shown. Two-dimensional views always look at area objects from the same side. To view stresses on the other side of the area object, switch to a 3D view or right click on the object while stresses are displayed to access the Shell Diagram form and click the Switch Face button.
Note: When forces or stresses are plotted for multi-valued combinations, SAP2000 displays whichever of the maximum and minimum values has the largest absolute value.
Example: Use of this command is demonstrated in Problem S.
See Also