VisualAnalysis Tutorials: Concrete Shear Wall
In this example a concrete shear wall will be analyzed for lateral loading due to diaphragm action. The wall will be modeled by a mesh of plate elements.
Setting Up the Project
When you start up VA, you are presented with the VisualAnalysis Startup Wizard by default. The wizard presents you with a number of options. We want to start fresh with a new project, so choose the "Start a New project" radio button. If you do not see the Startup Wizard, select File | New. Next, select "Plane Frame" as the structure type and click Start!. Change the unit style to Pounds & Feet (Drop down menu on the Command Bar), and name the project "Concrete Wall" (Modify Tab).
Modeling the Structure
Go the Create Tab and Double-Click or Drag-and-Drop the Quadrilateral mesh from the Plates & Tanks heading.
Specify the mesh type as Rectangular and click Next. Enter a length, L, of 50 ft and a height, W, of 20ft. The origin can remain at the default of (0,0). Click Next and you will be prompted for the number of elements in each direction. Enter 25 elements along the length and 10 elements along the width. This will create a 2'x2' plate mesh. Lastly, make the wall 8 in thick and specify the material as 3000 psi concrete.
Note: You can add additional materials to the database such as lightweight concrete. Materials are added by choosing the "<Add New>" option from the Source drop down under Material in the Modify tab of the Project Manager when a member or plate element is selected.
Editing the Generated Model
The mesh we generated must now be edited to model the windows and door. Simply delete the plate elements and nodes where the openings are to be placed. Support the wall by selecting all of the bottom nodes and making all them "pinned'. If this model was a space frame, additional constraints would be needed (fixing rotation about the X-axis).
Tip: To make node selection easier, simply go the Filter Tab and "Hide' the plate elements. Hold Shift + Drag and create box around the nodes you want to select.
Note: If you are modeling a shear wall with plate elements, and openings are of different geometries than what is easily adjusted for with square plate elements, you can adjust plate sizes by simply selecting and moving a node to grid points with your cursor. This will also change the shape of the plate. Be careful to ensure that all corners still coincide at a node.
Loading the Structure
This wall will be analyzed for self weight and wind loads applied through the diaphragm. The location of the diaphragm is at the bottom of the parapet wall. The total diaphragm load is 24,700 lbs, therefore, apply a 950 lb nodal load at each node that is on the level of the diaphragm in the Wind +X loads service case. If they were not created automatically, create a Wind +X loads service case as well as a Dead loads service case and include the structure self-weight in the Dead loads case. In the Load Case Manager, create an equation case combining the service cases as 1.2D + 1.6W (You can also use an existing load combination if the load factors are equivalent).
Analysis and Results
Now that we have our model created and loaded, we should check it for errors before setting the analysis options and actually analyzing. Select Analyze | Check Model for Errors to make sure there are no problems. Now select Analyze | Analyze Now, click the lightning bolt button on the toolbar, or simply click the Result View tab. Presented results can be changed using the drop boxes in the Filter Tab. Change the results to Tau xy stresses under your created dead and wind load combination. Notice that both overturning and shear can be checked using this model.
Try splitting each plate into four smaller plates. First select all the plates by Shift + Click. Right-click, select the "Split Plates" option, and break each plate into two parts in the x and two parts in the y. When the mesh is refined, you should edit the nodal loads applying 484.3 lb per node at the 16 ft level. You should also make sure all of the nodes at the base are pinned. This will give more accurate results. Analyze the model and observe the increased accuracy of the results.
We would like to determine the total shear force through the section A-A shown.
Select the plates that go through this section then use the Report Wizard to create a report of Plate Local Stresses. The report style may vary depending on the version of VA you are using.
Using the following equation you can determine the shear force in a plate element and then sum these forces. This will give the total shear through the section in question. For this example we will use the stresses at the plate's centroid location.
Shear stress (From VA output above)
Cross-sectional plate area
= (plate width)*(wall thickness) = 12 in * 8 in
= 96 in2
Vtotal = 11159.5 lbs