Working with Shear Walls

Dr. Frame2D includes basic real-time shear wall modeling. This page outlines how to create, modify, view, and remove shear walls. There is also a Notes and Caveats section providing implementation background and a discussion of limitations of the current release.

The image below shows an example of a typical shear wall analysis in progress.

This particular display shows stress intensity and orientation, as well as the deformed configuration. Note that the introduction of walls leads to discretization of the associated bounding beams and columns, with the wall mesh points acting as shared nodes connecting the components. This can be seen in the color gradient in the connecting columns and beams above (although it is partially obscured in this view).

Creating Walls

To create a shear wall, first select the shear wall tool ( ) and note that the Inspection Table will fill in with default values as indicated below:

Unlike most operations with Dr. Frame2D, for walls it is necessary to set the desired parameters before creating the object. In this respect, the creation of a wall is akin to automatically generating a frame or truss.

Once the desired parameters are set, use the tool to click at a starting joint, support, or member point, and this will cause a tracking rectangle to be drawn similar to the tracking line that appears with the other member tools:

Click a second time at the desired end location, and a wall will be created (and the connecting beams and columns will be discretized to match the wall mesh):

To create a free-standing wall (i.e., one without bounding beams or columns) begin with a surrounding frame with suitable dimensions, add the wall as described above, and then delete the bounding members.

Modifying Walls

To modify a shear wall, the important thing to note is that once created, the various nodes and elements making up the wall are automatically grouped. Thus, to select and modify individual wall components, one must hold down the alt/option key while selecting. Once selected, individual nodes and elements can be edited and manipulated as usual. For example, although not drawn unless selected, there are node objects located at each mesh point, and once selected, the usual node operations can be performed on these nodes (e.g., loading, relocating, etc.).

Depending on the wall mesh and the background grid settings, it may be necessary to turn off grid snapping when adjusting mesh node locations to avoid collapsing elements.

To remesh or resize a wall, it is generally necessary to delete the existing wall and re-install a new wall with desired mesh parameters.

To remove a shear wall, simply select it and use the delete key to erase it. To delete an individual element or set of elements, select them via alt/option-clicking (or dragging), and again use the Delete key. Among other things, this can be used to generate cutouts in walls. The figure below shows a set of wall elements (and the associated nodes) being selected with the select tool, which is being dragged while holding down the option/alt key:

Hitting the delete key with the above selection leads to the following model:

Using the SupportTool, we can add additional supports by alt/option-dragging a box around the set of nodes to which we wish to add supports:

After releasing the mouse button, the desired supports are installed as shown:

Note also in this case that the original fixed supports have been converted to pinned supports. A similar mechanism can be used to apply multiple loads, and this illustrated in the figures below.

In the figure above, the Point Load tool has been used to alt/option-drag a rectangle around a group of nodes. This results in the following set of loads being applied:

These loads are automatically grouped, so they can be manipulated and modified as a set.

Viewing Results

There are various options for viewing shear walls. The figures presented so far have had displacements and stress plotting turned off, but Dr. Frame2D handles shear walls in real time, just like everything else, so you can observe stress fields and displacements interactively. For example, the figure below shows the displaced shape and internal stress field:

In the figure above, the color intensity in the wall reflects the average magnitude of the in-plane maximum shear stress within the element. There are also glyphs indicating principal stress magnitudes and directions (see below for more details about this display option).

There are various ways to view stress fields. Maximum in-plane shear stress-based coloring for wall elements is controlled via the shared menu command Options:Member Display:Tension Compression Coloring. The remainder of the menu commands relevant to stress field display are indicated below:

The stress display options can be categorized broadly into how stresses are displayed, and which elements display stress values numerically. The following subsections consider each of these in turn.

Plotting Stresses

Color contours can display scalar quantities only, so Dr. Frame2D also supports simple glyph displays to help represent both magnitude and direction characteristics of a stress field. The figure below shows a close-up of a stress field in which the Show Stress Glyphs command has been activated:

In the figure above, the small crosses that are drawn at each point represent the average stress state within the corresponding element. The default glyph display depicts full principal stress information: the crosses are oriented according to the principal directions of the stress state, and each leg of the cross is drawn with a length proportional to the corresponding principal stress. Red indicates tension, and blue indicates compression. The size of the glyphs can be scaled using the standard stress scale buttons.

Choosing the Maximum Tension from the Plots menu leads to the figure below:

In the figure above, stresses are shown by plotting lines perpendicular to the maximum in-plane tensile stress direction, with the line lengths proportional to the maximum tensile stress magnitude. Such a depiction can help indicate where cracks might tend to form in materials sensitive to tension. Similarly, choosing the Maximum Shears option leads to the plot below in which the stress glyphs are aligned with the directions of maximum shear stress. This depiction can indicate yielding tendencies in ductile materials.

Displaying Values

In some of the figures above, numerical stress values are displayed as part of the various stress glyphs. When the Plot Stress Maxima option is selected, the maximum tension and compression stress values are identified and labeled automatically (be sure to see the caveats section below for a discussion of stress field accuracy). One can also choose to label all elements or no elements via the corresponding menu commands. For cases in which it is desirable to see numerical values within a certain region of a mesh, one can select the elements in question, and then use the Label Selected menu command to turn on labels for the selected elements:

It generally will be necessary to zoom in to such regions of interest to avoid label overlap.

As shown below, displacement values for internal wall nodes can be obtained either by attaching labels in the usual manner, or by selecting them using the Select Tool. This will cause the relevant results to appear in the Results Pane (for single selection, the results can also be viewed in the Inspector Pane):

Background Notes and Caveats

The elements used for wall modeling are plane stress quadrilaterals based on four overlapping triangular elements with 3 degrees of freedom per node: 2D vector translations plus a drilling rotation. These underlying elements are optimal for bending applications, and are described in detail in the following technical report: C. Felippa, "A study of optimal membrane triangles with drilling freedoms". University of Colorado Report CU-CAS-02-07, 2003.

Plane elements with rotational degrees of freedom can require somewhat more consideration of boundary/support conditions that pure displacement-based elements (e.g., constant strain triangles). See the examples below.

The following representative test cases illustrate the basic performance of the current wall elements:

• We will consider first the simplest of all cases: uniaxial loading with Poisson's ratio equal to zero. This example will highlight the boundary condition and loading differences between the current elements and elements that do not have rotational degrees of freedom. In particular, the image below shows the results obtained using a standard uniaxial laoding and boundary condition configuration (E=10,000 ksi, t = 0.5 in, w = 144 in, L = 288 in, P = 24 k):

  

  It can be seen that while the stresses and displacements are generally accurate, there is a deviation from uniaxial behavior near the corners. This is because the simple loading shown does not correctly model uniform applied stress consistent with these elements' shape functions. The simplest corrective measure is to constrain the corner rotations using stiff rotational springs as shown below:

  

  Similar results can be obtained by applying the load via a stiff end beam as indicated below:

  

• The image below shows the results of a common test of the bending/shear response of plane elements (12in x 48in beam; 1-in thickness; E = 30,000 ksi; Poisson's ratio = 0.2). The target ("exact") value for this case is 0.356 inches, and the Dr. Frame result can be seen to be 0.352 inches. This relatively accurate result for such a coarse mesh illustrates the way in which these particular elements are tuned for optimal bending modeling. (Strictly speaking, the end load actually should be applied in a manner consistent with the shear stress distribution, so more refined results are possible).

  

• The next result is the same configuration as above, but in this case a more refined set of boundary conditions have been applied at the wall so that the corresponding stresses can be considered. In particular, the vertical restraint of the top and bottom nodes has been released via roller supports (combined with stiff rotational springs to suppress rotation of the corner drilling degrees of freedom).

  

  Using elementary bending and shear relations, the bending stress at the labeled elements' midpoints can be calculated as My/I = 37.5 ksi, and the shear stress as VQ/Ib = 3.75 ksi. The corresponding principal stresses at this point become (37.87, 0.37) ksi. Neither these elementary relations nor the shown coarse mesh represent exact solutions, but the results are in reasonable agreement. Be sure to note that these results do not represent the true stress maxima, which would occur at the extreme beam fibers. In this particular case, linear extrapolation of the displayed results leads to a close match with the stresses predicted from beam theory.

The following are additional limitations and issues associated with using these elements:

Depending on your hardware, you should be able to maintain good performance with reasonably refined meshes. Realize, however, that memory and computational requirements grow nonlinearly with mesh size so it is not too difficult to create meshes that will bring Dr. Frame to its knees. Just how big is too big depends on your processor and RAM, so you will need to experiment.

Distributed area loads for transversely loading walls have not been implemented as of this release. Using multiple nodal loads applied via area dragging as described above can be used as a workaround.

Shift-dragging with the pan tool to relocate a structure with grid snapping on can cause wall nodes to coalesce at grid points leading to an unrealistic (and unexpected) model. Use undo to restore the prior state and disable grid snapping before dragging.

The connection between wall elements and the associated bounding beams and columns is discrete and does not account for beam on elastic foundation behavior (although the elements do share both displacement and rotational degrees of freedom). This typically leads to some discretization artifacts in moment and shear diagrams such as in the figures shown below:

Moment diagram along wall-member junctions.

Shear diagram along wall-member junctions.